User Manual Fine Turbo V6.29

Rating

Date
June 2018 
Size
4.8MB 
Views
8,349 
Categories
Transcript
FINE ™ Flow Integrated Environment User Manual contains: FINETM GUI v6.2 Euranus v5.1 NUMERICAL MECHANICS APPLICATIONS ™ FINE User Manual Version 6.2d (May 2005) NUMECA International 5, Avenue Franklin Roosevelt 1050 Brussels Belgium Tel: +32 2 647.83.11 Fax: +32 2 647.93.98 Web: http://www.numeca.com NUMERICAL MECHANICS APPLICATIONS Contents CHAPTER 1: Getting Started 11 Overview 12 Introduction What is CFD? Components Multitasking Project Management 13 How To Use This Manual Outline Conventions 14 First Time Use Basic Installation Expert Graphics Options 15 How to start FINE™ Interface 16 Required Licenses Standard FINE™ License Additional Licenses CHAPTER 2: User Interface 21 Overview 22 Project Selection Creating a New Project Opening of an Existing Project Grid Units and Project Configuration 23 Main Menu Bar File Menu Mesh Menu Solver Menu Modules Menu 24 Icon Bar File Buttons Grid Selection Bar Solver Buttons Module Buttons User Mode 25 Computations Button 26 Parameters Button 27 View Area 28 Mesh Information 29 Parameters Area 210 Graphics Area Viewing Buttons 211 File Chooser 212 Profile Manager FINE™ 11 11 11 11 13 13 13 15 15 15 16 16 16 17 18 18 18 21 21 22 22 23 24 24 24 28 29 210 210 210 211 212 212 212 212 213 213 215 215 216 216 219 219 iii Contents CHAPTER 3: Fluid Model 31 Overview 32 The Fluid Model in the FINE™ Interface Properties of Fluid Used in the Project List of Fluids Add Fluid Delete Fluid from List Edit Fluid in List Showing Fluid Properties Filters Import Fluids Database Expert Parameters 33 Theory Transport Properties Fluid Models CHAPTER 4: Flow Model 41 Overview 42 Time Configuration The Interface for an Unsteady Computation Expert Parameters for Unsteady Computations Best Practice on Time Accurate Computations Theoretical Aspects for Unsteady Computations 43 Mathematical Model Euler Laminar NavierStokes Turbulent NavierStokes Expert Parameters for Turbulence Modelling Best Practice for Turbulence Modelling Theoretical Aspect of Turbulence Modelling Gravity Forces Low Speed Flow (Preconditioning) 44 Characteristic and Reference Values Reynolds Number Related Information Reference Values CHAPTER 5: Rotating Machinery 51 Overview 52 Rotating Blocks 53 Rotor/Stator Interaction in the FINE™ Interface 54 How to Setup a Simulation with Rotor/Stator Interfaces? Mixing Plane Approach Frozen Rotor Domain Scaling Method Phase Lagged Method 55 Theoretical Background on Rotor/Stator Interfaces iv 31 31 32 32 32 33 37 37 38 38 38 38 39 39 310 41 41 42 42 45 46 49 415 415 415 416 416 419 427 441 442 447 447 447 51 51 52 53 55 55 59 511 513 515 FINE™ Contents Introduction Default Mixing Plane Approach Full Nonmatching Technique for Mixing Planes Domain Scaling Method CHAPTER 6: Throughflow Model 61 Overview 62 Throughflow Blocks in the FINE™ Interface Global Parameters Block Dependent Parameters Mesh for Throughflow Blocks Boundary Conditions for Throughflow Blocks Initial Solution for Throughflow Blocks Output for Throughflow Blocks 63 File Formats for Throughflow Blocks Onedimensional Throughflow Input File Twodimensional Throughflow Input File Output File 64 Expert Parameters Related to Throughflow Blocks Underrelaxation Process Others. 65 Theoretical Background on Throughflow Method The Time Dependent Approach Basic Equations and Assumptions The Tangential Blockage Factor The Blade Force CHAPTER 7: Optional Models 71 Overview 72 FluidParticle Interaction Introduction FluidParticle Interaction in the FINE™ Interface Outputs Specific Output of the FluidParticle Interaction Model Expert Parameters for FluidParticle Interaction Theory References 73 Conjugate Heat Transfer Introduction Conjugate Heat Transfer in the FINE™ Interface Theory 74 Cooling/Bleed Introduction Cooling/Bleed Model in the FINE™ Interface Expert Parameters Theory Cooling/Bleed Data File: ’.coolingholes’ FINE™ 515 516 519 521 61 61 62 62 62 66 67 68 68 69 69 611 611 612 612 612 613 613 613 613 614 71 71 71 71 73 76 77 78 79 711 711 711 711 713 715 715 716 731 732 733 v Contents 75 Transition Model Introduction Transition Model in the FINE™ Interface Expert Parameters Theory CHAPTER 8: Boundary Conditions 81 Overview 82 Boundary Conditions in the FINE™ Interface Inlet Condition Outlet Condition Periodic Condition Solid Wall Boundary Condition External Condition (Farfield) 83 Expert Parameters for Boundary Conditions Imposing Velocity Angles of Relative Flow Extrapolation of Mass Flow at Inlet Outlet Mass Flow Boundary Condition Torque and Force Calculation Euler or NavierStokes Wall for Viscous Flow Pressure Condition at Solid Wall 84 Best Practice for Imposing Boundary Conditions Compressible Flows Incompressible or Low Speed Flow Special Parameters (for Turbomachinery) 85 Theory on Boundary Conditions Inlet Boundary Conditions Outlet Boundary Conditions Solid Wall Boundary Conditions Farfield Boundary Condition CHAPTER 9: Numerical Model 91 Overview 92 Numerical Model in FINE™ CFL Number Multigrid parameters Preconditioning Parameters 93 Expert Parameters for the Numerical Model Interfaced Expert Parameters Noninterfaced Expert Parameters 94 Theory Spatial Discretization Multigrid Strategy Full Multigrid Strategy Time Discretization: Multistage RungeKutta Implicit residual smoothing vi 737 737 738 739 740 81 81 81 84 86 89 810 813 813 813 814 814 814 815 815 815 815 816 816 816 817 822 826 829 91 91 92 92 92 93 93 93 95 97 97 913 916 917 920 FINE™ Contents CHAPTER 10:Initial Solution 101 Overview 102 Block Dependent Initial Solution How to Define a Block Dependent Initial Solution Examples for the use of Block Dependent Initial Solution 103 Initial Solution Defined by Constant Values 104 Initial Solution from File General Restart Procedure Restart in Unsteady Computations Expert Parameters for an Initial Solution from File 105 Initial Solution for Turbomachinery 106 Throughfloworiented Initial Solution CHAPTER 11:Output 111 Overview 112 Output in FINE™ Computed Variables Surface Averaged Variables Azimuthal Averaged Variables ANSYS Global Performance Output Plot3D Formatted Output 113 Expert Parameters for Output Selection Azimuthal Averaged Variables Global Performance Output 114 Theory Computed Variables Surface Averaged Variables Azimuthal Averaged Variables Global Performance Output CHAPTER 12:Blade to Blade Module 121 Overview 122 BladetoBlade in the FINE™ Interface Start New or Open existing BladetoBlade Computation BladetoBlade Data Boundary Conditions Numerical Model Initial Solution Menu Output Parameters Control Variables Page Launch BladetoBlade Flow Analysis 123 Expert Parameters 124 Theory Mesh Generator Flow Solver FINE™ 101 101 101 102 102 103 104 104 105 105 106 107 111 111 112 112 117 119 1110 1115 1117 1118 1118 1118 1120 1120 1121 1121 1124 121 121 122 122 123 128 1210 1210 1210 1210 1211 1211 1211 1211 1212 vii Contents 125 File Formats used by BladetoBlade Module Input Files Output Files CHAPTER 13:Design 2D Module 131 Overview 132 Inverse Design in the FINE™ Interface Start New or Open Existing Design 2D Project Creation of Inverse Design Input Files Initial Solution Menu Launch or Restart Inverse Design Calculation Expert Parameters 133 Theory 134 File Formats used for 2D Inverse Design Input Files Output Files CHAPTER 14:The Task Manager 141 Overview 142 Getting Started The PVM Daemons Multiple FINE™ Sessions Machine Connection from UNIX/LINUX Platforms Machine Connection from Windows Platforms Remote Copy Features on UNIX/LINUX Remote Copy Features on Windows 143 The Task Manager Interface Hosts Definition Tasks Definition 144 Parallel Computations Introduction Modules Implemented in the Parallel Version Management of Interblock Communication How to Run a Parallel Computation Troubleshooting Limitations 145 Task Management Using Scripts Launch IGG™ Using Scripts Launch AutoGrid using Scripts Launch EURANUS in Sequential using Scripts Launch EURANUS in Parallel using Scripts Launch CFView™ Using Scripts 146 Limitations CHAPTER 15:Computation Steering and Monitoring 151 Overview viii 1213 1213 1215 131 131 132 132 133 135 136 136 137 138 138 139 141 141 141 141 142 142 144 144 144 145 145 146 1411 1411 1412 1412 1413 1414 1414 1414 1415 1415 1416 1417 1421 1422 151 151 FINE™ Contents 152 Control Variables 153 Convergence History Steering Files Selection and Curves Export Available Quantities Selection New Quantity Parameters Definition Quantity Selection Area Definition of Global Residual The Graphics View 154 MonitorTurbo Introduction The Residual File Box Quantities to Display 155 Best Practice for Computation Monitoring Introduction Convergence History MonitorTurbo Analysis of Residuals APPENDIX A:Governing Equations A1 Overview A2 ReynoldsAveraged NavierStokes Equations General NavierStokes Equations Time Averaging of Quantities Treatment of Turbulence in the Equations Formulation in Rotating Frame for the Relative Velocity A3 Formulation in Rotating Frame for the Absolute Velocity APPENDIX B:File Formats B1 Overview B2 Files Produced by IGG™ The Identification File: project.igg The Binary File: project.cgns The Geometry File: project.geom The Boundary Condition File: project.bcs B3 Files Produced by FINE™ The Project File: project.iec The Computation File: project_computationName.run B4 Files Produced by the Flow Solver EURANUS The cgns file: project_computationName.cgns The mf file: project_computationName.mf The res file: project_computationName.res The log file: project_computationName.log The std file: project_computationName.std The wall file: project_computationName.wall The aqsi file: project_computationName.aqsi The Plot3D files The me.cfv file: project_computationName.me.cfv FINE™ 151 152 153 153 154 155 155 156 157 157 159 159 1510 1510 1511 1511 1512 A1 A1 A1 A1 A2 A2 A3 A3 B1 B1 B1 B2 B2 B2 B2 B2 B2 B3 B3 B3 B4 B4 B5 B5 B5 B6 B6 B7 ix Contents B5 Files Used as Data Profile Boundary Conditions Data Fluid Properties B6 Resource Files Boundary Conditions Resource File euranus_bc.def Fluids Database File euranus.flb Units Systems Resource File euranus.uni APPENDIX C:List of Expert Parameters C1 Overview C2 List of Integer Expert Parameters C3 List of Float Expert Parameters APPENDIX D: Characteristics of Water (steam) Tables D1 Overview D2 Main Characteristics x B7 B7 B9 B10 B10 B10 B10 C1 C1 C1 C2 D1 D1 D1 FINE™ CHAPTER 1: 11 Getting Started Overview Welcome to the FINE™ User’s Guide, a presentation of NUMECA’s Flow INtegrated Environment for computations on structured meshes. This chapter presents the basic concepts of FINE™ and shows how to get started with the program by describing: • what is CFD, • what FINE™ does and how it operates, • how to use this guide, • how to start the FINE™ interface. 12 Introduction 12.1 What is CFD? All the mathematical sciences are founded on relations between physical laws and laws of numbers, so that the aim of exact science is to reduce the problems of nature to the determination of quantities by operations with numbers. James Clerk Maxwell, 1856 In the late 1970’s, the use of supercomputers to solve aerodynamic problems began to pay off. One early success was the experimental NASA aircraft called HiMAT, designed to test concepts of high manoeuvrability for the next generation of fighter planes. Wind tunnel tests of a preliminary design for HiMAT showed that it would have unacceptable drag at speeds near the speed of sound; if built that way the plane would be unable to provide any useful data. The cost of redesigning it in further wind tunnel tests would have been around $150,000 and would have unacceptably delayed the project. Instead, the wing was redesigned by a computer at a cost of $60,000. Paul E. Ceruzzi, 1989 Computational Fluid Dynamics (CFD) is commonly accepted as referring to the broad topic encompassing the numerical solution, by computational methods, of the governing equations that describe FINE™ 11 Getting Started Introduction fluid flow related conservative equations (for instance involving energy or species concentration). It has grown from a mathematical curiosity few decades ago, to become an essential tool in almost every branch of fluid dynamics, from aerospace propulsion to weather prediction. Key elements of CFD are briefly described below. Please notice these informations have mostly been extracted from the web at http://www.crankfield.ac.uk/sme/cfd/whatiscfd.htm and http:// ltp.larc.nasa.gov/aero/login.htm. The reader is invited to consult the web at www.cfdonline.com for more insight in CFD theory. By 1900, theoretical and mathematical developments in fluid dynamics had not achieved significant progress as quickly as experimental efforts. Although the NavierStokes equations describing fluid behaviour had existed for over 75 years before the Wright brothers' first flight, they were simply too complex to solve in their complete form for anything but simplified problems under specific conditions. Even today, theoretical solutions to the NavierStokes equations are rare and only suited to specific classes of problems. As a developing science, CFD has received extensive attention throughout the international community since the advent of the digital computer. CFD interests are mainly driven by the desire to model complex physical fluid phenomena, that couldn't be easily or cost effectively simulated with a physical experiment. Computational techniques differ from analytical or theoretical solutions in the sense that they only solve equations at a finite number of points rather than for the entire flow field. Choosing these points may become quite difficult  especially for a complex geometry and may require hundreds of thousands or even million of points. In general, a dense grid with many points will give a solution of great detail, but require more computer memory and time to reach a solution. Since this tradeoff in computer resources and solution quality is required, the current trend is often to use a dense grid in areas where the solution may change rapidly such as in the boundary layer or near a shock wave, but use of a coarser grid with fewer computational points in areas where the solution is expected to change more gradually. The selection of grid nodes is the science of grid generation. It is a complex field on its own and has many applications outside CFD, such as in constructing solid models for stress, vibration and heat transfer analysis. There are several different techniques that are commonly used to develop computational grids for CFD. Grid nodes can be arranged either in a regular or irregular pattern. Depending on the pattern selected, the method of generation is referred to as structured or unstructured. Both techniques have their own advantages and disadvantages. Basically, structured methods enable the generation of regular grids, with high quality standards and good control in the distribution of grid nodes in shear and boundary layers. However, they may sometimes be hard to generate for very complex geometries. On the contrary, unstructured methods allow a limited control in the grid quality (and thus in the grid solution) but the grid generation process does usually require limited user resources, even for complex geometries. It is thus important that the user recognizes these so that the best grid can be created for a particular geometry. The quality of the grid is definitely important, since it strongly influences the solution including whether or not a solution can be found at all. FINE™/Turbo and FINE™/Design3D environments developed by NUMECA rely on structured grid methods, based on AutoGrid and IGG™ software tools. NUMECA offer also includes unstructured capabilities, through HEXPRESS™ hexahedral grid generator and FINE™/HEXA environment. More details can be provided upon request. 12 FINE™ Introduction Getting Started Usually, about 4 to 5 unknowns are computed at each grid node. This makes methods of presenting CFD results a difficult matter, mainly due to the large number of data to manage. Adequate postprocessing is then required to easily and quickly outline the major characteristics of the flow. This is usually done through surface color techniques and particle paths/ribbons. The latter method is mostly used to depict vortices and complex flowwall interactions. The user is invited to refer to CFView™ manual for a detailed information on NUMECA offer in that area. 12.2 Components The resolution of Computational Fluid Dynamics (CFD) problems involves three main steps: • spatial discretization of the flow domain, • flow computation, • visualization of the results. To perform these steps NUMECA has developed three software systems. The first one, IGG™, is an Interactive Geometry modeller and Grid generation system for multiblock structured grids. The second software system, the flow solver EURANUS, is a state of the art 3D multiblock flow solver able to simulate Euler or NavierStokes (laminar or turbulent) flows. The third one, CFView™, is a highly interactive Computational Field Visualization system. These three software systems have been integrated in a unique and user friendly Graphical User Interface (GUI), called FINE™, allowing the achievement of complete simulations of 3D internal and external flows from the grid generation to the visualization, without any file manipulation, through the concept of project. Moreover, multitasking capabilities are incorporated, allowing the simultaneous treatment of multiple projects. 12.3 Multitasking FINE™ has the particularity of integrating the concept of multitasking. This means that the user can manage a complete project in FINE™ interface; making the grid using IGG™, running the computation with EURANUS and visualizing the results with CFView™. Furthermore, the user has the possibility to start, stop and control multiple computations. Please note that the flow simulation can be time consuming, therefore the possibility of running computations in background has been implemented. See chapter 13 for more detail on how to manage multiple tasks through the interface or in background. 12.4 Project Management To manage complete flow analyses, FINE™ integrates the concept of project. A project involves grid generation, flow computation and visualization tasks. The results of each of these tasks are stored in different files that are automatically created, managed and modified within FINE™: • The grid files: The grid generation process, IGG™, creates files containing the representation of the geometry and the grid related to the project. The definition of the types of boundary conditions is also done during this process. The four files that contain the information about the mesh have the extensions .igg, .geom, .bcs and .cgns. • The project file: The project file is created by FINE™. It has the extension .iec and contains the input parameters needed for the flow computations. • The result files: FINE™ creates a new subdirectory for each computation where it stores the following files: — a file with extension .run containing all computation input parameters used by the solver and by CFView™, FINE™ 13 Getting Started Introduction — a .cgns file that contains the solution and is used for restarting the solver, — a .res file used by the Monitor to visualize the residual history (see Chapter 15), — two files used to visualize the convergence history in the Steering with extensions .steering and .steering.binary (see Chapter 15). — two files with extensions .mf and .wall that contain global solution parameters. — two files with extensions .std and .log that contain information on the flow computation process. — a .batch file used to launch the computation in batch (see Chapter 15). • The CFView™ visualization files: In addition to the .run file, the flow solver creates a series of files, which can be read by CFView™. These files have different extensions. For example in case of turbomachinery flow problem, the solver will create a file for the azimuthal averaged results with extension .me.cfv. Through the interface, the user can modify all the information stored in the files associated to the project. When creating a new project a new directory is made, e.g.; \project. In this directory the project file is stored: \project\project.iec and a directory is created called \project\_mesh. In this directory the grid files used for the computations can be stored. It is however also possible to select a grid that is located in another directory. Only one mesh file should be used for all computations in a project. If computations need to be done on another mesh file it is advised to duplicate the project (see section 23.1.4) or to create a new project (see section 23.1.1) for those computations. batch FIGURE 1.2.41 Example 14 of file management for a FINE™ project FINE™ How To Use This Manual 13 How To Use This Manual 13.1 Outline Getting Started This manual consists of five distinct parts: • • • • • • • Chapters 1and 2: introduction and description of the interface, Chapters 3 to 13: computation definition, Chapter 14: task management, Chapter 15: monitoring capabilities, Annex A: the NavierStokes equations, Annex B: used file formats, Annex C: list of supported noninterfaced expert parameters. At first time use of FINE™ it is recommended to read this first chapter carefully and certainly section 14 to section 16. Chapter 2 gives a general overview of the FINE™ interface and the way to manage a project. For every computation the input parameters can be defined as described in the chapters 3 to 13. Chapter 14 gives an overview of how to run computations using the Task Manager or using a script. Chapter 15 finally describes the available tools to monitor the progress on a computation. The expert user finds in chapter 3 to 13 a section describing advanced options that are available in expert user mode. Additionally Annex C provides a list with all supported expert parameters on the page Computation Steering/Control Variables in expert user mode. For each parameter a reference is given to the section in the manual where it is described. 13.2 The use of nonsupported parameters is at own risk and will not guarantee correct results. Conventions Some conventions are used to ease information access throughout this guide: • • • • • Commands to type in are in italics. Keys to press are in italics and surrounded by <> (e.g.: pressor the right mouse button to quit the option. This tool is also accessible with thekey. 210.1.8 Fit Button The fit button is used to fit the content of the view to the view limits without changing the current orientation of the camera (which can be interpreted as the user's eyes). 210.1.9 Original Button The original button is used to fit the content of the view and to give a default orientation to the camera. 210.1.10Cutting Plane This option displays a movable plane that cuts the geometry and the blocks of the mesh. The plane is symbolically represented by four boundaries and its normal, and is by default semitransparent. After having selected the button: • Press and drag the left mouse button to rotate the plane • Press and drag the middle mouse button to translate the plane • Press < x >, < y > or < z > to align the plane normal along the X, Y or Z axis • Press to revert the plane normal • Press < t > to toggle the transparency of the plane (to make it semitransparent or fully transparent). It is highly advised to deactivate the plane transparency when using X11 driver to increase the execution speed. 218 FINE™ File Chooser User Interface 211 File Chooser For file management (opening and saving of files) FINE™ uses the standard File Chooser window. The layout of the File Chooser depends on the used operating system but a typical layout is shown in Figure 2.11.03. The Directories list allows to browse through the available directory structure to the project directory. Then the Files list can be used to select the file name. In the case a file needs to be opened an existing file should be selected in the list of available files. In the case a new file needs to be created the user can type a new file name with the appropriate extension. In the List Files of Type bar the default file type is set by default to list only the files of the required type. For a description of all available file types in FINE™ see section 12.4. FIGURE 2.11.03 Typical layout of a File Chooser window 212 Profile Manager When a law is defined by a profile clicking on the button right next to the pull down menu will invoke a Profile Manager. FIGURE 2.12.04 Profile FINE™ Manager for fluid parameters 219 User Interface Profile Manager The Profile Manager is used to interactively define and edit profiles for both fluids and boundary conditions parameters. The user simply enters the corresponding coordinates in the two columns on the left. The graph is updated after each coordinate (after each pressing of key). The button Import may be used if the profile exists already as a file on the disk. The Export button is used to store the current data in the profile manager as a file (for example to share profiles between different projects and users). The formats of the profile files are explained in Appendix B where all file formats used by FINE™ and EURANUS are detailed. If the mouse cursor is placed over a point in the graph window, this point is highlighted and the corresponding coordinates on the left will be also highlighted, giving the user the possibility to verify the profile. The button OK will store the profile values and return back to the main FINE™ window. 220 FINE™ CHAPTER 3: 31 Fluid Model Overview Every FINE™ project contains a fluid with the corresponding properties. In FINE™ the fluid to use for a computation can be defined by: 1. Using the fluid defined in the project file of which the properties are shown on the fluid selection page (see section 32.1), or 2. selecting a fluid from the fluid database included in the release that contains a set of predefined fluids (see section 32.2), or 3. creating a new fluid (see section 32.3). In the next section the interface is described in detail including advice for use of the fluid definition. The theoretical background for the different fluid models is described in section 33. FINE™ 31 Fluid Model The Fluid Model in the FINE™ Interface 32 The Fluid Model in the FINE™ Interface list of predefined fluids filters list of properties FIGURE 3.2.01 Fluid 32.1 Selection page Properties of Fluid Used in the Project Every FINE™ project contains a fluid with the corresponding properties that are displayed in the interface (see Figure 3.2.01). When a new project is created the used fluid is a default fluid. When an existing project is opened the used fluid is defined by the properties as defined in the project file ’.iec’. The first listed fluid property is the fluid type. Four fluid types are available: • perfect gas, • real gas, • incompressible gas or liquid, • condensable fluid. For more detail on each of these types see section 33. For the first three fluid types the properties can be defined through the interface as described in section 32.3. For the use of the condensable fluid contact NUMECA to obtain the appropriate tables to add a condensable fluid to the list of fluids. To modify the properties of the used fluid a fluid may be selected from the list of predefined fluids (section 32.2) or a new fluid may be defined (where the new fluid is based on the current one, see section 32.3 for more detail). 32.2 List of Fluids The list of fluids (see Figure 3.2.01) contains predefined fluids in a database with for each fluid the fluid type and the permissions. 32 FINE™ The Fluid Model in the FINE™ Interface Fluid Model Every fluid is associated with the user who created it and can be modified or removed only by its owner (the owner has Read Write Delete permissions). All other users will have Read Only permissions only. The user may select a fluid from the list. The selection will be highlighted and the properties of the selected fluid are displayed in the information box below the fluid list. Those fluid properties will be saved in the project file ’.iec’ as soon as the project is saved. 32.3 Add Fluid To add a fluid to the database click on the Add New Fluid... button. A new fluid is then created with the current properties as shown in the list of properties. A wizard will appear allowing the user to modify those properties. On the first page of this wizard the user can enter the name and the type of the new fluid. The name should be entered by moving the mouse to the text box for the Fluid Name and to type the name on the keyboard. By default a name is proposed like new_fluid_1. The fluid type can be entered by selecting the appropriate check boxes. First make a choice for a compressible or incompressible fluid. For a compressible fluid select a perfect gas or a real gas. The fluid type corresponding to the selected checkboxes is shown in the text box for the Fluid Type. To cancel the modifications to the fluid definition and close the wizard click on the Cancel button. Once the fluid name and type are correctly set, click on Next>> to go to the next page of the wizard. On this page the following properties have to be defined: • Specific Heat Law, • Heat Conduction Law, • Viscosity Law, • Density Law (for an incompressible fluid only). The possible values to enter for these laws depend on the selected fluid type as described in the next paragraphs. In the case a law is defined by a constant value, type the value in the corresponding dialog box. In the case a law is defined by a profile, the Profile Manager can be opened by clicking on the button ( ) right next to the pull down menu (see section 32.3.6 for more detail). In the case a law is defined by a formula, the Formula Editor can be opened by clicking on the button ( next to the pull down menu (see section 32.3.5). ) right Information linked to fluid creation is stored in the fluid database only when closing the FINE™ interface. As a consequence, this information will not be available to other users as long as this operation is not completed. 32.3.1 Definition of a Perfect Gas For the definition of a perfect gas the user has to specify: • The specific heat at constant pressure. For a perfect gas only a constant Cp is allowed. • The specific heat ratio (Cp/Cv) characteristic of the fluid. • The heat conductivity which may be constant, defined by a polynome in temperature or specified through a constant Prandtl number. FINE™ 33 Fluid Model The Fluid Model in the FINE™ Interface • The viscosity law which may be constant, temperature dependent or specified by the Sutherland law. In case the viscosity depends on the temperature the user can specify the law through a polynome or as a profile through the Profile Manager. Furthermore, when the viscosity law is defined by the Sutherland law, the Sutherland parameters are accessible by clicking on the button ( ) right next to the pull down menu. The user can select a law for the dependence of the laminar viscosity in function of the static temperature. The default is the Sutherland’s law that imposes a temperature dependence of the dynamic viscosity. The viscosity may also be maintained constant. 32.3.2 Definition of a Real Gas A real gas is defined by laws for the dependence of Cp and/or γ with the temperature. The user can either define a profile, using the Profile Manager, or impose a polynomial approximation using the Formula Editor. In this last case, the polynomes take the following form: Cp ( T ) = A0 T γ ( T )= B0T –3 –3 + A1 T + B1 T –2 –2 + A2T + B2 T –1 –1 1 2 + A 3 + A 4 T + A5 T + A 6 T 1 2 + B 3 + B4 T + B 5 T + B6 T 3 3 , (31) , (32) where the coefficients A0, A1, A 2, A 3, A 4, A5, A6, B 0, B 1, B 2, B 3, B4, B5 and B 6 are chosen by the user and set in the dialog box for Cp and γ respectively. In the definition of real gas properties, lower and upper bounds of temperature variations [TminTmax] allowed in the domain must be provided. Depending on the local temperature during the iterative process, the physical properties will then be able to vary according to the laws defined in the fluid database. Note that it is necessary to cover the whole temperature range occurring in the system otherwise some inaccuracy in the results might be introduced. In addition, the local temperature may not fit at some occasion in the prescribed range; this is especially true during the transient. If so, as indicated by the formula editor (section 32.3.5), the physical properties are kept constant, at a value that corresponds to the lower/upper bound allowed by the range. For the default definition of a real gas, involving a compressibility factor, the user has to specify: • The specific heat at constant pressure characteristic and the specific heat ratio (γ=Cp/Cv) of the fluid, that can be dependent on the temperature through a polynome or a profile. In both cases, the user has to specify the temperature range over which the specific heat is defined. For alternative modelling methods for a real gas see section 32.9 and section 33.2.2. • The heat conductivity which is constant, defined by a polynome or profile in temperature or specified through a constant Prandtl number. • The viscosity law which may be constant, dependent on temperature or specified by the Sutherland law. In case the viscosity depends on the temperature the user can specify the law through a polynome or as profile. Furthermore, when the viscosity law is defined by the Sutherland law, the Sutherland parameters are accessible by clicking on the button ( down menu. ) right next to the pull Compared to a perfect gas computation (Cp and γ constant), the real gas option results in an increase of about 25% of the CPU time. Real gas calculations are usually robust enough to avoid any use of preliminary run with average physical properties. However, convergence difficulties may arise in the transient (say the first 100200 iterations) if either the temperature range allowed is too large or if the properties are expected to vary very significantly in the temperature range allowed. At these occasions, it is often useful to run an equivalent perfect gas, with average proper 34 FINE™ The Fluid Model in the FINE™ Interface Fluid Model ties, in order to remove any temperature dependency and ease the convergence process in the transient. 32.3.3 Definition of a Liquid For the definition of a liquid two models are available: • a ’pure’ liquid with constant density, • a barotropic liquid for which the density varies with pressure. Depending on the type of liquid the user has to specify: • The specific heat at constant pressure. For liquids only a constant Cp is allowed. • The heat conductivity which may be constant, defined by a polynome in temperature or specified through a constant Prandtl number. • The viscosity law which may be constant or depend on temperature. In case the viscosity depends on the temperature the user can specify the law through a polynome or as a profile through the Profile Manager. • The density law can be pressure dependent (using a polynomial law or as a profile through the Profile Manager) or follow Boussinesq law. In this latter case the density is constant and the Boussinesq coefficients are taken into account only if the button Gravity Forces (Flow Model page) is activated. These coefficients are used in source terms of the density equation in order to modelize the gravitational effect (i.e. natural convection) although the density is assumed to be strictly constant. For liquids, the reference temperature and pressure must lie in the expected range of the static temperature and pressure of the flow field. The reference pressure and temperature are defined on the Flow Model page (Eq. 485). 32.3.4 Definition of a Condensable Gas The aim of the Condensable Fluid module is the modelling of the real thermodynamic properties of the fluid by means of interpolation of the variables from dedicated tables. The module can be used for a singlephase fluid whose properties are too complex to be treated with a perfect or real gas model. It can also be used in order to treat thermodynamic conditions that are close to the saturation line. Note that the model can be used on the liquid or on the vapour side of the saturation curve. In case the thermodynamic state lies inside the twophase region a homogeneous equilibrium twophase mixture of vapour and liquid is considered. The hypothesis of an equilibrium mixture is however not valid if the dryness (wetness) fraction exceeds 20%. The module can not be used above these fractions, as it completely ignores evaporationcondensation phenomena. The approach that has been adopted in EURANUS consists of using a series of thermodynamic tables, one table being required each time a thermodynamic variable must be deduced from two other ones. This implies the creation of many tables as input, but presents the advantage that no iterative inversion of the tables is done in the solver, with as a consequence a very small additional CPU time. The thermodynamic tables are provided by NUMECA, upon request. The tables corresponding to water steam have been generated on basis of literature. NUMECA has also developed a tool for the generation of the thermodynamic tables on basis of equations presented in the literature. In order to use a condensable gas as fluid model, the user has to copy the provided tables in a userdefined subdirectory called /tables_username/ in /NUMECA_INSTALLATION_DIRECTORY/ COMMON/steam_tables on UNIX or in /NUMECA_INSTALLATION_DIRECTORY/bin/ FINE™ 35 Fluid Model The Fluid Model in the FINE™ Interface steam_tables/ on Windows before launching FINE™. When the subdirectory is created, the condensable gas is recognized by FINE™ and the fluid will appear in the list with respectively Fluid Name and Fluid Type as "_name" and Condensable Fluid. 32.3.5 Formula Editor When a law is defined by a formula clicking on the button right next to the pull down menu will invoke a formula editor. When a law is defined by a formula clicking on the button right next to the pull down menu will invoke the Formula Editor. FIGURE 3.2.32 The Formula Editor for polynomials in the fluid properties The Formula Editor is used to define polynomial values for the fluid properties. The user has to define the seven coefficients of the polynomial according to the displayed formula on the top, and also the lower and upper limits of the range, in which the polynomial function is defined. Press after each entry. The constant values equal to the minimal and maximal values will be considered outside of this range (as shown in the graph). If a fluid with "Read Only" permissions contains formulas they may be visualized by means of the Show Fluid Properties... button that opens the Formula Editor window, but they can not be modified  a message will warn the user that the selected fluid can not be modified. 32.3.6 Profile Manager When a law is defined by a profile clicking on the button right next to the pull down menu will invoke a Profile Manager. The Profile Manager is used to interactively define and edit profiles for both fluids and boundary conditions parameters. The user simply enters the corresponding coordinates in the two columns on the left. The graph is updated after each coordinate (after each pressing of key). The button Import may be used if the profile exists already as file on the disk. The Export button is used to store the current data in the profile manager as a file (for example to share profiles between different projects and users). The formats of the profile files are explained in detail in Appendix B. 36 FINE™ The Fluid Model in the FINE™ Interface FIGURE 3.2.33 Profile Fluid Model Manager for fluid parameters If the mouse cursor is placed over a point in the graph window, this point is highlighted and the corresponding coordinates on the left will be also highlighted, giving the user the possibility to verify the profile. The button OK will store the profile values into the fluid definition. 32.4 If a fluid with "Read Only" permissions contains profiles they may be visualized by means of the Show Fluid Properties... button that opens the Profile Manager window, but they can not be modified  a message will warn the user that the selected fluid can not be modified. Delete Fluid from List When the user has the permission to delete a fluid the button Delete Fluid... allows to remove the selected fluid from the list of fluids. 32.5 Information linked to fluid removal is stored in the fluid database only when closing the FINE™ interface. As a consequence, this information will not be available to other users as far as this operation is not completed. A message will however warn users that the fluid properties have been modified (up to removal in the present situation) by the owner. Edit Fluid in List When the user has the permission to write for a fluid, the properties of the selected fluid can be modified by clicking on Edit Fluid.... A wizard will appear allowing to modify the name, the type and the laws defining the selected fluid. The two pages of this wizard and the laws to define are described in detail in section 32.3. FINE™ Information linked to fluid edition is stored in the fluid database only when closing the FINE™ interface. As a consequence, this information will not be available to other users as far as this operation is not completed. A message will however warn users that the fluid properties have been modified by the owner. 37 Fluid Model 32.6 The Fluid Model in the FINE™ Interface Showing Fluid Properties When the user does not have the write permission (Read Only) for a fluid the Show Fluid Properties... button opens the wizard with the properties of the fluid. In this case it is not possible to modify any of the properties in the wizard but the user has access to visualize the fluid properties including the defined profiles and formulae. 32.7 Filters On the Fluid Model page two filters are available to display only a limited amount of fluids in the list of fluids. Select the owner(s) and fluid type(s) to display from the pull down menus to limit the list of fluids. 32.8 Please notice that under Windows™ the fluid database is not owneroriented. The database is stored locally and user defined fluids is accessible with full permissions to all Windows™ users. Import Fluids Database When the user has is own fluid database, the Import Fluids Database... enables to load a user defined database through a File Chooser window to select the ’.flb’ file containing the properties of all the fluids. 32.9 When loading an existing project and opening the Fluid Model page, please notice that FINE™ is automatically checking if the fluid is existing or not in the fluid database. If the fluid name is existing but the properties are different, a comparison window will invite the user to select the fluid to use (the default fluid in the database or the fluid defined in the project). Expert Parameters A list of the expert parameters which can be used in the definition of the fluid type follows hereafter. It is only a summary to know directly the expert parameters related to the definition of a fluid. More details about these expert parameters are given in section 33. All expert parameters related to fluid definition are available in Expert Mode on the Control Variables page. For these expert parameters the default values are appropriate ones that only have to be changed in case the user has specific wishes concerning the fluid modelling. PRT: Allows to define the turbulent Prandtl number. For the real gas (thermally perfect gas): IRGCON: defines how the real gas is modelled (default IRGCON = 0) = 0: a compressibility factor is used: two laws have to be entered to define the dependence of Cp and γ with the temperature. = 1: constant r model, γ is calculated from r and Cp. The dependence of Cp with temperature needs to be entered. RGCST: value of the gas constant r used with IRGCON equal to 1 (default RGCST = 287) 38 FINE™ Theory Fluid Model For condensable fluid: IHXINL = 0 (default), = 1: activation of special inlet boundary condition. 33 Theory 33.1 Transport Properties 33.1.1 The Laminar Viscosity In general the kinematic viscosity (in m2/s) is defined in FINE™. The laminar kinematic viscosity may be • constant, • given in terms of a polynomial function of the temperature, • given by a profile for a certain temperature range, • varying according to Sutherland’s law. The dynamic viscosity is then computed within the code by multiplying the kinematic viscosity by the reference density. The Sutherland law is given by: For T ∞ ≥ 120K T µ ( T ) = µ ( 120 ) 120 µ( T) = T µ ∞ ⎛ ⎞ ⎝T ⎠ ∞ 1.5 0 T ≤ 120 K (33) T + TSUTHE ∞ ⎛ ⎞ ⎝ T + TSUTHE ⎠ 0 T ≥ 120 K For T ∞ ≤ 120K T µ ( T ) = µ ∞ T∞ 0 T ≤ 120 K T 1.5 120 + TSUTHE µ ( T ) = µ ( 120 ) ⎛ ⎞ ⎛ ⎞ ⎝ 120⎠ ⎝ T + TSUTHE ⎠ (34) 0 T ≥ 120 K The viscosity µ ∞ in Eq. 33 and Eq. 34 is the dynamic viscosity specified in the Fluid Model page or is obtained from the kinematic viscosity and the density both specified in the Fluid Model page, while T ∞ and TSUTHE are respectively the reference temperature and the Sutherland temperature specified also in the Fluid Model page. FINE™ 39 Fluid Model Theory 33.1.2 The Heat Conductivity The laminar heat conductivity may be • constant, • given in terms of a polynomial function of the temperature, • given by a profile for a certain temperature range, • specified through the Prandtl number. In case the Prandtl number Pr is specified, the laminar thermal conductivity is obtained as: µC κ = pPr (35) The turbulent viscosity is calculated iteratively using one of the turbulence models discussed in section 43.3. The turbulent conductivity is obtained from the turbulent viscosity and a turbulent Prandtl number whose value can be controlled through the expert parameter PRT (default: 1.0): µt Cp . κ t = Pr t 33.2 (36) Fluid Models In this section, details are provided about the different fluid types available in FINE™: • perfect gas, • real gas, • liquid, • condensable fluid. 33.2.1 Calorically Perfect Gas The perfect gas law is used as constitutive equation: p = ρrT (37) with r the gas constant for the perfect gas under consideration: R r =  = c p – c v , M (38) with R the universal gas constant and M the molecular weight of the perfect gas. γ is the specific heat ratio, C p the specific heat at constant pressure, and C v the specific heat at constant volume with: Cp γ =  . Cv (39) When the gas temperature is so low that the vibrational and electronic modes are frozen, the internal energy of the gas will be proportional to the temperature and the specific heats as well as γ are constant. The gas is "calorically perfect". This is the usual assumption of moderate speed aerodynamics. 310 FINE™ Theory Fluid Model The relation between r and C p is given by γ–1 r =  C p . γ (310) The values of γ and C p are user input. The static pressure is obtained from the conservative variables through the following relation: 2 ( ρw ) . p = ( γ – 1 ) ρE – 2ρ (311) 33.2.2 Real Gas For real gases or more precisely thermally perfect gases, C p and γ depend on the temperature T. The corresponding values can be entered either through a polynomial approximation or through a profile. The thermally perfect gas model is based on two equations: • the perfect gas relation, still valid: R p = ρrT = ρ  T , M (312) • the enthalpy equation: h = ⎛ T ⎞ C p dT⎟ ⎜ ⎝ T0 ⎠ ∫ p = e +  = ρ T ⎧ ⎫ C v dT ⎬ + ⎨ ⎩ T0 ⎭ ∫ rT , (313) where T0 is a reference temperature. In practice T0 is set equal to the minimum temperature of the temperature range specified in the Fluid Model page. These two equations lead to: rT = ⎛ T ( Cp ⎜ ⎝ T0 ∫ ⎞ – C v ) dT⎟ . (314) ⎠ In the case of a real gas with varying specific heats one can notice that it is not possible to respect the 2 above equations with a constant value of r, unless the difference (CpCv) does not vary with temperature. Two solutions are proposed in EURANUS in order to model real gases: • Perfect gas with compressibility factor (expert parameter IRGCON=0) — the equation of state is modified to include a compressibility factor Z: R p = ZρrT = Zρ  T M ⎛ T ( Cp ⎜ ⎝ T0 ∫ (315) ⎞ – C v ) dT⎟ ⎠ Z = rT (316) • Constant r model FINE™ 311 Fluid Model Theory — the user specifies the gas constant r (expert parameter RGCST). Then Cp is provided and γ calculated as Cp γ = Cp – r (expert parameter IRGCON=1). 33.2.3 Incompressible Fluid a) Liquid The density is user input: ρ = Cst . (317) This implies a decoupling of the mass and momentum conservation equations from the energy conservation equation, since no term in the mass and momentum equations depends on the temperature. b) Barotropic Liquid The density is a user defined function of the pressure: ρ = f(p) . (318) The corresponding values can be entered either through a polynomial approximation or through a profile (see section 32.3.5 and section 32.3.6). The particularity of the barotropic liquid formulation is that although the density is not constant, a decoupling of the energy equation is still adopted, exactly as in the full incompressible formulation. Modification of the treatment of the energy equation A modification of the treatment of the energy is required in order to account for the density variations. The temperature equation for any type of fluid can be written as: dT ∂p ρc v  = – T ⎛ ⎞ ⎛ ∇V⎞ + ∇ ⎛ k∇T⎞ + ε v , ⎝ ∂T⎠ ⎝ ⎠ ⎝ ⎠ dt V (319) where εv is the viscous dissipation term and V is the specific volume (inverse of density). Since for a barotropic fluid there is a unique relation between the pressure and the density the first term on the right hand side of the above equation vanishes and the temperature for a barotropic fluid becomes: dT ρc v  = ∇ ⎛ k∇T⎞ + ε v . ⎝ ⎠ dt (320) In addition, since we have from classical thermodynamics that ⎛ ∂ 2 p⎞ ∂c v = T ⎜ 2⎟ , ∂V ⎝ ∂T ⎠ V (321) the specific heat at constant volume depends only on the temperature cv=cv(T). Note that we also have as for an incompressible fluid that the specific heats at constant pressure and at constant volume are equal (cv=cp). The modification of the formulation of the energy for a barotropic fluid can be derived from the above relations. Since we have for a barotropic fluid: 312 FINE™ Theory Fluid Model ∂p de = c v dT + ⎛ T ⎛ ⎞ – p⎞ dV = c v dT – pdV . ⎝ ⎝ ∂T⎠ ⎠ V (322) The barotropic relation can be integrated from a reference state to obtain finally T e ( p, T ) = e 0 + ⎛ ⎞ ⎜ c dT⎟ v ⎜ ⎟ ⎝ T0 ⎠ ∫ p + p ∂ρ  dp . ∫ ρ ∂p 2 (323) p0 Compared to an incompressible formulation the energy depends on both pressure and temperature. 33.2.4 Condensable Fluid a) Introduction The aim of the Condensable Fluid module is the modelling of the real thermodynamic properties of the fluid by means of interpolation of the variables from dedicated tables. The module can be used for a singlephase fluid whose properties are too complex to be treated with a perfect or real gas model. It can also be used in order to treat thermodynamic conditions that are close to the saturation line. Note that the model can be used on the liquid or on the vapour side of the saturation curve. In case the thermodynamic state lies inside the twophase region a homogeneous equilibrium twophase mixture of vapour and liquid is considered. The hypothesis of an equilibrium mixture is however not valid if the dryness (wetness) fraction exceeds 20%. The module can not be used above these fractions, as it completely ignores evaporationcondensation phenomena. For a real fluid the equation of state may be a complicated and usually implicit expression, generating unacceptable computational overhead if the corresponding equations are explicitly introduced in the solver. Similarly when an equilibrium mixture of vapour and droplets (wet steam for instance) is considered as a single fluid, the calculation from the saturation properties of thermodynamic variables must be done iteratively. The approach that has been adopted in EURANUS consists of using a series of thermodynamic tables, one table being required each time a thermodynamic variable must be deduced from two other ones. This implies the creation of many tables as input, but presents the advantage that no iterative inversion of the tables is done in the solver, with as a consequence a very small additional CPU time. This additional time corresponds to the one that is needed by the bilinear (or bicubic) interpolation procedures through the tables. In order to optimize the efficiency of these interpolations the input tables are always built on basis of a Cartesian mesh in the plane of the input variables (V1,V2) (N1 and N2 values for the variables V1 and V2 respectively). b) Thermodynamic Tables Tables are generated based on NUMECA internal tools, based on various sets of wellknown equations as described below: • BenedictWebbRubin equation (usually used with refrigerants), • Modified BenedictWebbRubin model (selected equation for hydrogen), • Vander Waals equation. Single tables are generally used, which means that the tables cover both singlephase and twophase regions, as for instance depicted in the figure 3.3.24, showing one of the tables used to model hydrogen. A bilinear interpolation approach is well adapted to these tables, providing an adequate smoothing of the saturation region. Bicubic interpolation techniques have also been implemented and tested. They provide a higher accuracy for a given number of data points but tend to create spu FINE™ 313 Fluid Model Theory rious oscillations in the saturation region. These oscillations can be avoided by adopting separated tables covering respectively the single and the twophase regions, these two tables intersecting along the saturation line. Five categories of tables are used by the solver 1. Basic tables: p(e,ρ) and T(e,ρ) The numerical scheme being based on a formulation of the equations on basis of the energy and the density, the basic tables are used in order to update the pressure and the temperature after each update of the formulation variables. 2. Entropy tables: p(h,s), ρ(h,s), s(h,p), h(s,p) The entropy tables are used at the inlet/outlet boundary conditions, and are required in order to calculate the total (static) thermodynamic conditions from the static (total) ones. 3. The (p,T) tables: e(p,T) and ρ(p,T) These tables are required in order to allow the use of the inlet boundary conditions based on total pressure and temperature. They are also required by the turbomachinery initial solution procedure. ρ [kg/m3] FIGURE 3.3.24 Thermodynamic Table: ρ(p,Τ) 4. The viscosity and conductivity tables: µ(e,ρ) and κ(e,ρ) 314 FINE™ Theory Fluid Model The viscosity and conductivity can also be interpolated from tables. If these tables are not present the other laws available within the user interface can be used. 5. The saturation table This table contains the liquid and vapour values of all thermodynamic variables along the saturation line. It is only required if the user activates the dryness fraction output and/or if the inlet boundary condition based on total enthalpy and dryness fraction is selected. c) Integration of Thermodynamic Tables in the Solver Provided that all the input tables are present, the full functionality of the basic solver is accessible. All boundary conditions are available, as well as the initial solution procedures. The numerical schemes are not different, making use of the same acceleration techniques (multigrid, local time stepping, residual smoothing) providing robust and fast convergence to steady state. The evaluation of the advective, viscous and artificial dissipation fluxes involves the pressure in the momentum and energy equations and the temperature in the energy equation. For a perfect gas both are easily deduced from the equation of state, the conversion being so rapid that only the pressure and the density are stored and the other variables recalculated from these whenever they are needed. In the condensable fluid module the density, the pressure, the temperature and the energy are stored in order to limit the number of interpolations. Only one interpolation is made in order to deduce the new values of pressure and temperature after the update of the density and the energy. The speed of sound which enters the numerical solution process through the spectral radius in the time step and in the residual smoothing and artificial dissipation coefficients is also required. It can either be interpolated from a table or computed from the partial derivatives of the p(e,ρ) table: ∂p p ∂p 2 c = ⎛ ⎞ + 2 ⎛ ⎞ ⎝ ∂ρ⎠ e ρ ⎝ ∂e⎠ ρ (324) The BaldwinLomax, SpalartAllmaras and (k,e) turbulence models can be used. The turbulent conductivity calculation is based on the usual relation: µt κ t =  c p Prt (325) The specific heat at constant pressure can either be constant (the value being provided in the user interface) or deduced from the specific table. Condensable fluid option is not compatible with the use of cooling/bleed module and/or upwind schemes for space discretization. By default, a set of thermodynamic tables for water (steam) is proposed starting FINE™/ Turbo v6.29. More details can be found in Appendix D. The installation of the thermodynamic tables must be performed as described in section 32.3.4 d) Specific Output Specific outputs can be created by the condensable fluid module: • enthalpy: static, total absolute and total relative • dryness fraction (0 3). The default value is 0. FINE™ 417 Flow Model Mathematical Model SIGRO: constant in the kε model when ICOPKE =1 in Eq. 470 and Eq. 472 (default value = 0.5). C3: constant for the kε model when ICOPKE = 1 in Eq. 472 (default value = 2.). ICODKE: parameter to active the compressible dissipation, = 0 (default): no compressible dissipation, = 1: Sarkar model for compressible dissipation (Eq. 475), = 2: Nichols model for compressible dissipation (Eq. 477). ALF: constant of Sarkar model for compressible dissipation when ICODKE=1 (default = 0.5). CP1: constant of Nichols model for compressible dissipation when ICODKE=2 (default value = 4.). MAVRES: allows to control the update of k and ε (default = 0.95), > 0: according to the restrictions defined by Eq. 478 and Eq. 479, = 0: according to the restriction defined by Eq. 478, < 0: according to the restriction defined by Eq. 480. MAVREM: allows to control the multigrid corrections for k and ε (default = 0.95), > 0: according to the restrictions defined by Eq. 478 and Eq. 479, = 0: according to the restriction defined by Eq. 478, < 0: according to the restriction defined by Eq. 480. MUCLIP: controls the maximum allowable value for the ratio MUT/MU (default value = 5000). LTMAX: maximum turbulent length scale (default = 1.E+6), = 1: control of turbulent length scale with automatic clipping. IYAP: (= 1) applies the Yap’s modification to control the turbulent length scale (default value = 0). The value of the expert parameter LTMAX must be the default value. TEDAMP: parameter to improve the robustness of the kε models (default value = 1), > 0: a minimum of TEDAMP multiplication factor of the clipping value (EKCLIP) is used for k in the factor 1 ⁄ T in Eq. 457, a minimum of TEDAMP multiplication factor of the clipping value (EPCLIP) is used for ε to compute the turbulent viscosity (Eq. 459), <= 0 : the minimum values used for k and ε correspond to the expert parameter EPS, GAMMAT: introduces the turbulence time scale in the computation of the local time step to control stability (default value = 10). PRCLIP: sets an upper bound for the ratio between production and dissipation (default value = 50). LIPROD: (= 1) corresponds to a linearization of the production term (default value = 0) when strain rate is large (i.e. impinging flow) and PRCLIP has no more effect on the flow field. EKCLIP: clipping value for the turbulent kinetic energy k (default value = 1.E5). EPCLIP: clipping value for the turbulent dissipation rate ε (default value = 1E5). KEGRID: Full multigrid parameter corresponding to the finest grid level on which the BaldwinLomax model is used (default = 2). On the lower grid levels, the kε model is used. IUPWTE: (= 1) uses an upwind scheme for the convection of kε instead of a centre scheme (default = 1). 418 FINE™ Mathematical Model Flow Model IKENC: (= 1) solves the kε equations with a nonconservative approach (default = 1). IKELED: (= 1) actives the LED scalar scheme for kε instead of the standard central scheme (default = 0). IOPTKE: (= 1) optimized implementation for kε (YangShi, Wall function, Lauder Sharma) (default = 1). 43.5 Best Practice for Turbulence Modelling 43.5.1 Introduction to Turbulence Turbulence can be defined as the appearance of nondeterministic fluctuations of all variables (velocity u", pressure p", etc ...) around mean values. Turbulence is generated above a critical Reynolds number that may range in values from 400 to 2000 depending on the specific case. In 95% of industrial applications the critical Reynolds number falls above that range. That is why it is in general necessary to predict adequately the turbulence effects on the flowfield behaviour. Τo model turbulent flow in a satisfactory way, four steps should be performed: • choosing a turbulence model, • generating an appropriate grid, • defining initial and boundary conditions, • setting expert parameters to procure convergence. 43.5.2 First Step: Choosing a Turbulence Model. A turbulence model is chosen based on the specific application. Table 41 states the most appropriate turbulence models to use for different types of flows. Although these are the "most appropriate" this does not mean that certain turbulence models cannot be used for the flow types listed, but just that they are "less appropriate". TABLE 41 Recommended turbulence models for different flow types Three main kinds of turbulence models exist: • algebraic models (e.g. BaldwinLomax), • oneequation models (e.g. SpalartAllmaras), • twoequation(s) models (kε). When quick turbulence calculations are required, for example, in designcycle analysis, it is recommended that the BaldwinLomax model is used due to its high numerical stability and low computational expense. To simulate more precisely the turbulent quantities with also a good rate of convergence the SpalartAllmaras model should be preferred. FINE™ 419 Flow Model Mathematical Model Another model often used in design is "standard" kε. This model employs an empirically based logarithmic function to represent the nearwall physics and requires a lower grid resolution in this region as a result. One drawback of this treatment is that the logarithmic function does not apply for separated flows, although the NUMECA extended wall function will still work. If it is expected that a significant amount of separation will have to be predicted, one of the lowReynolds number turbulence models would be more appropriate. All of the listed turbulence models employ constant turbulent Prandtl numbers which is somewhat of a restriction when performing heat transfer calculations. However, experience has shown quite successful prediction of heat transfer coefficients when using BaldwinLomax and LaunderSharma kε. 43.5.3 Second Step: Generating an Appropriate Grid. a) Cell Size viscous sublayer buffer layer log layer Separating flow logarithmic law Data of Lindgren (1965) Note that the sublayer extends up to y+=5 but 10 is an acceptable approximation for design calculations. Note: The variable v* displayed in the figure is uτ. Picture from White, F.M., Viscous Fluid Flow, McGraw Hill, 1991. FIGURE 4.3.53Boundary layer profiles When calculating turbulence quantities it is important to place the first grid node off the wall within a certain range (ywall). This can be done for the blade and the endwalls (hub and shroud) independently. When doing computations including viscosity (NavierStokes equations) the boundary layer near a solid wall presents high gradients. To properly capture those high gradients in a numerical simulation it is important to have a sufficient amount of grid points inside the boundary layer. When Euler computations are performed no boundary layer exists and therefore the cell size near solid walls is of less importance. 420 FINE™ Mathematical Model Flow Model To estimate an appropriate cell size ywall for NavierStokes simulations including turbulence, the local Reynolds number based on the wall variable y+is computed. The value of y+ associated with the first node off the wall will be referred to here as y1+: ρu τ y wall = µ y1+ (422) where uτ is the friction velocity: uτ = τ wall = ρ 1( V ) 2 Cf 2 ref (423) Note that the value of ywall depends on the value of y1+. In Figure 4.3.53 is represented the evolution of u+ against y+ from the measurements of Lindgren(1965) with: u+= u / u τ LowRe models resolve the viscous sublayer and are well suited for y1+ values between 1 and 10 whereas highRe models apply analytical functions to the loglayer and are appropriate to y1+ values ranging from 20 to 50 (it depends on the extension of the buffer layer for the considered flow). Moreover one can notice that the logarithmic function does not apply for separated flow. So whether it is expected that a significant amount of separation will have to be predicted, one of the lowReynolds number turbulence models would be more appropriate. Recommendations are given in the table below for ranges of y1+ specific to the different types of models. Turbulence Models + Y1 HighRe: Standard kε, Extended wallfunction kε (will accept lower values) 2050 LowRe: BaldwinLomax, SpalartAllmaras, LaunderSharma kε, YangShih kε, Chien kε, Extended wallfunction kε. 110 TABLE 42 Appropriate y1 + Nonlinear ke (Suited for research, not designcycle analysis) HighRe LowRe 2050 110 values for available turbulence models One way to estimate ywall as a function of a desired y+ value is to use a truncated series solution of the Blasius equation: Vref – 7 / 8 ⎛ L ref⎞ 1 / 8 + y ... y wall = 6 ⎛ ⎞ ⎝ ν ⎠ ⎝ 2 ⎠ (424) Note that the reference velocity, Vref, can be taken from an average at the inlet. For instance, if the mass flow is known the value can be calculated using density and the crosssectional area of the inlet. If the mass flow is not known the reference velocity may be calculated from the inlet total pressure and an estimated static pressure using isentropic relations. The reference length, Lref, should be based on streamwise distance since an estimation of boundary layer thickness is implied FINE™ 421 Flow Model Mathematical Model in this calculation. For instance, in the case of a turbomachinery simulation one could use the distance of hub and shroud curves that exist upstream of the first row of blades. This is approximate, of course, as the thickness of boundary layers will vary widely within the computational domain. Fortunately it is only necessary to place y+ within a range and not at a specific value. Another method of estimating ywall is to apply the 1/7th velocity profile. In this case the skin friction coefficient Cf is related to the Reynolds number: 0.027Cf = Re x1 / 7 (425) where Rex should be based on average streamwise values of Vref and Lref as discussed above. Since uτ is based on Cf it may be calculated based on Eq. 423, and ywall may then be calculated from Eq. 422. Note that either method is not exact but they will yield results that are quite close to each other. In fact, it can be instructive to calculate ywall using both methods as a check. Since only one wall distance is being calculated, the particular flow being studied should be kept in mind. For instance if it is a diffusing flow Cf, and hence y+, can be expected to drop. Since a certain range is desired (e.g., 20< y+<50 for highRe Standard k ε) the user may choose to base the calculation of wall distance on an average of that range (e.g., 40). b) Things to Look Out For These instructions should provide reasonable estimates but it is always wise to plot y+ once a solution has finished. Spot checks should be made to ensure that most y+ values fall within the desired range. For instance it is useful to plot y+ contours over the first layer of nodes from a given wall. There are some special cases where such checks do not strictly apply. For instance, skin friction approaches zero at points of separation so it is expected that y+ will be low in such regions. It is generally recommended that turbomachinery blade tip clearances are meshed with uniform spanwise node distributions. In such cases, the y+ values will tend to be higher within the gap than elsewhere in the computational domain nearwall regions. This should not raise concern as the tip clearance flow consists of thoroughly sheared vortical fluid that undergoes significant acceleration and is therefore quite different than a standard boundary layer. It is expected that the skin friction will be high in this region due to the acceleration. c) General Advice • What grid resolution is adequate? The resolution method employed in the EURANUS flow solver requires approximately 9 nodes across a free shearlayer and approximately 15 across a boundary layer to provide gridindependent results for turbulent flows. If wall functions are used the boundary layer only requires approximately 9 nodes. Of course the flow field under study will realistically consist of shear layers of which the width varies substantially throughout the flow field. The user must therefore decide what is important to capture and what is not. For instance, in the designcycle analysis of a compressor with a volute it would probably be acceptable to choose a fullydeveloped boundary layer. The number of nodes across the diameter would therefore be approximately 29. However, it would be wise to select a number like 33 to maintain a a large number of multigrid levels. The selection of nodes in the streamwise direction should be governed by what resolution adequately represents the studied geometry. Regions of concentrated high gradients, such as airfoil leading or trailing edges or any geometrical corners should contain a relatively high clustering of nodes. 422 FINE™ Mathematical Model Flow Model • What determines the grid quality? After the various grid resolution concerns are addressed, the level of skewness must be analysed. Providing clustering in a curved geometry can often lead to internal angles of grids cells of 10o. It is important to minimize the number of cells containing such low angles as the calculation of fluxes can become significantly erroneous under such conditions. More information concerning how to check the quality of a grid can be found in the IGG™ or AutoGrid manual. If the adjustment of node numbers and clustering does not reduce the level of skewness, local smoothing should be applied. The expansion ratio, or the ratio of adjacent cell sizes, should also be checked. It is particularly important to keep this value within an absolute range of about 01.6 in regions of high gradients, such as boundary layers, free shearlayers and shocks. If it is evident that adjacent cells are different in size by factors significantly greater than two, the clustering in this region should be reduced or the number of nodes should be increased. d) Verification of y1+ By following this instructions it should be possible to generate a grid of reasonable quality for turbulent flows. It is recommended however, that the user checks values of y1+ after approximately one hundred iterations on the fine grid to ensure the proper range has been specified. At the same time, it can be useful to plot contours of residuals (continuity, momentum, energy and turbulence) over selective planes. If the level of skewness is too high, this will be indicated by local peaks in residuals that are orders of magnitude greater than the rest of the flow field. If a multiblock grid is used, the residual levels in each block can be compared in the monitor. 43.5.4 Defining Initial and Boundary Conditions Turbulence is commonly modelled by emulating molecular diffusion with a socalled "eddyviscosity" (µT). A standard method for determining µT is based on turbulenteddy length and time scales that are modelled through turbulence kinetic energy (k) and dissipation (e.g. ε) equations. It is important to note that the level of turbulence quantities (i.e. turbulence intensity, µT, k, ε) specified at the inlet boundary can have a strong effect on the flowfield prediction for quantities like the total pressure, velocity profiles, flow angles, total temperature etc. Since the measurement of turbulence is rarely conducted in a design and test environment, the designer faces the problem of setting these quantities without knowing the correct values. a) SpalartAllmaras Model When the SpalartAllmaras model is selected the user should specify in the inlet boundary condition the kinematic turbulent viscosity νΤ (m2/s). If no information is available on the turbulence properties of the flow, estimates can be made based on the following assumptions that: ν ν • For internal flows (e.g. turbomachinery): T = 1 to 5. ν ν • For external flows (e.g. vehicle aerodynamics): T = 1 . b) Kε Models • Estimation of k The value of the turbulent kinetic energy can be derived from the turbulence intensity Tu or from the wall shear stress. FINE™ 423 Flow Model Mathematical Model — From the turbulence intensity. The turbulence intensity Tu can be expressed against the streamwise fluctuating velocity u" and the streamwise velocity Uref: ″2 u T u =  . U ref (426) For internal flows the value of Tu is about 5% and for external flows it is reduced to 1%. With these considerations k can be calculated in considering an isotropic turbulence: 3 ″2 2 k =  ( u ) 2 (427) — From the wall shear stress. If the wall shear stress is known, the user can use the wall functions defined for the fully turbulent flow: τ wall k = ρ Cµ (428) This value of k could be used as an initial value and also for the inlet boundary condition. • Estimation of ε The value of the turbulent dissipation can be specified through one of the following rules: — Specify the ratio of the turbulent viscosity to the laminar viscosity 2 µ ρref k ε = C µ  µ it µ (429) For internal flows (such as turbomachinery flow), typical values are µ it ⁄ µ = 50 . For external flows (in aerodynamics computations), typical values are µ it ⁄ µ = 1 . — Specify the turbulent length scale (only for internal flows). A typical values is l = 0.1D H . where DH is the hydraulic diameter of the inlet section 3 3  4 2 cµ k ε =  . l (430) — Derive ε from the asymptotic turbulent kinetic equation: In a free uniform flow the turbulent kinetic energy equation reduces to ∂k u  = – ε . ∂x (431) This relation can be used to specify the value of the turbulent dissipation in the following way: ∆k ε = – u  , L (432) where u is the inlet velocity, ∆k the decay of the turbulent kinetic energy over a length L. For example, in a turbomachine, L is the maximum geometric length and ∆k could be set to 10% of the inlet value of k. 424 FINE™ Mathematical Model Flow Model Using this method, the user must make sure that the value of the turbulent viscosity obtained µ µ from these values of k and ε is not too big or too small. i.e. 1 < t < 1000 . If this condition is not satisfied, it is advised to scale down or up the value of k inlet or the ∆k and compute again the turbulent dissipation — Specify the wall shear stress. If the wall shear stress is known, the user can use the wall functions defined for the fully turbulent flow. 3 2 ( τ wall ⁄ ρ ) ε = l (433) If there is an initial solution file containing k and ε , the k and ε values of this file are used to initialize the fields. The initial values mentioned above can also be used to set the inlet boundary conditions for the k and ε fields. However, to reduce the possibility of oscillations in skin friction due to nonphysical relaminarisation during convergence, it is recommended to insure ε ≈ 0.1 ε inlet . 1. Either of the above methods can be applied for setting the boundary conditions in turbomachine applications. However, if the given values of k and ε lead to the killing of the turbulence shortly after the inlet section, we suggest to apply Eq. 432 and select an inlet values of k such that the ratio of the turbulent viscosity to the laminar viscosity equals 50. In some cases a crosscheck between Eq. 429 and Eq. 431 may result in very different values for ε. In such a case it is recommended to reevaluate k and ε in the following manner: Use relation Eq. 432: 0.1k ∆k ε = – u  = u  . ∆L ∆L (434) This relation expresses that k0 (k at the inlet) is expected to be decreased by about 10% over a length ∆L that is characteristic to the size of the domain. 2. Use relation Eq. 429. In this relation Cµ=0.09 and ν represents the laminar viscosity of the fluid. 3. Combine the relations of the two previous steps to remove ε0, leading to: 0.1U µ T ν k 0 =  ⎛⎝  ⎞⎠ . ∆L µ C µ 4. (435) Using either relation Eq. 429 or Eq. 432 then easily leads to an estimation of ε0. 43.5.5 Setting Expert Parameters to Procure Convergence Several expert parameters may be set to procure convergence. FINE™ 425 Flow Model Mathematical Model a) Cutoff (Clipping) of Minimum k Value The float parameter EKCLIP controls the minimum allowable value of k. This is done to prevent nonphysical laminarisation and remove the possibility of negative values being calculated during numerical transients. Setting this value to a reasonable level has been shown to significantly increase convergence rate. EKCLIP: clipping k to about 1% of inlet value maintains minimum residual turbulence in the domain. b) Minimizing Artificial Dissipation in the Boundary Layer An alternative treatment of the dissipation terms in the k and ε equations has been introduced to overcome difficulties related to turbulence decay in boundary layers observed in some specific test cases. Currently, the dissipation terms are scaled with the spectral radius of the equations and are further damped in an exponential manner across the boundary layer. The major drawback of this formulation is that it introduces an excessive amount of artificial dissipation into the boundary layer, leading to nonphysical relaminarisation problems. A different implementation, based on the L.E.D. (Local Extrema Diminishing) version of the JamesonSchmidtTurkel treatment introduces better monotonicity properties of the k and ε equations. IKELED = 0 (default): Dissipation scaled with spectral radius. = 1: Less diffusive L.E.D. scheme activated. c) Wall Function for the kε Turbulence Model INEWKE = 0: Wall function applies for first node off the wall at Y+ =2050, Launder & Spalding. = 10 (default): Meshindependent formulation of the wall function. d) Full Multigrid kε / BaldwinLomax Model Switch KEGRID = 2(default) Grid 222  Baldwin Lomax, Grid 111  Baldwin Lomax, Grid 000  ke Model. KEGRID = 3: Grid 222  Baldwin Lomax, Grid 111  ke Model, Grid 000  ke Model. Example: kε run on the finest grid level (000) with 3 levels of grid (222, 111 & 000) in the multigrid procedure. The BaldwinLomax model remains active on levels 222 and 111 before ke is automatically switched on when the finest grid is reached. This is controlled through the expert parameter KEGRID whose value is set to 2 by default, meaning that the Baldwin Lomax model is used up to the second level of grid. The µt / µ field computed using the BaldwinLomax model is then transferred to the finest mesh and used to calculate initial k and ε values. The use of a KEGRID value higher than the number of grid levels available enables the k and ε equations to be solved on all grid levels. A similar procedure can be followed when a calculation on 111 mesh is first desired. Providing KEGRID is set to 2 (default value), the BaldwinLomax is then active on level 222 before the kε model is automatically switched on when the finest grid level (111 in this case) is reached. However, the question then arises when a restart procedure on the 000 level is required. How to restart on 000 while transferring strictly the k and ε fields already computed on 111? By default, since KEGRID=2, the solution computed on 111 is seen as a BaldwinLomax solution. The k and ε fields 426 FINE™ Mathematical Model Flow Model are then reset using the classical procedure while the other variable fields (density, velocity and energy) are transferred adequately. To overcome this difficulty, KEGRID must again be set to a value higher than the number of grids. This procedure results in a much better initialization of k and ε, thus preventing some relaminarisation while enhancing convergence. e) Cutoff (clipping) of Maximum Turbulence Production/Destruction Value The float parameter PRCLIP controls the maximum allowable value of turbulence production/ destruction (=production/density*dissipation in ke model). Limiting this to a finite value enhances convergence rate by removing the possibility of unbounded turbulence spikes occurring during the numerical transient. However, care must be taken to apply a reasonable limit. Recommended values are: PRCLIP (Float): For most flows: 50 (default), In turbulent diffusion dominated flows (e.g., seals): 200. f) Linearization of Turbulence Production/Destruction Value The integer parameter LIPROD activates the linear production (PRCLIP is no more used if LIPROD set at 1). This linearization of the turbulence production is relevant for impingement flows for which the standard model is well known to overestimate the production of kinetic energy at stagnation point. LIPROD = 1: activate the linear production (PRCLIP no more used in that case). 43.6 Theoretical Aspect of Turbulence Modelling An algebraic (BaldwinLomax), an oneequation (SpalartAllmaras) and several twoequation turbulence models ( k – ε ) are available. Wall distance All turbulence models need to compute the wall distances everywhere in the computed domain. It is a rather time consuming process so that they are saved in the *.cgns mesh file at the beginning of the first computation. These values will be read and used for the next computations. If the mesh file is modified or saved again, they are erased and will be computed again. Different important expert parameter are used in the calculation of the wall distance. The default values are generally sufficient and they have to be changed only if a problem arises. The expert parameter NREPET allows to take into account the periodicity of the computed domain. Indeed, at each point of the domain, the closest wall is not always in the computed domain if periodic boundary conditions are used. Consequently the domain is repeated beyond the periodic boundaries to compute correctly the wall distance. The default value is 1 and can be increased to 2 in very particular cases. The expert parameter NSUBM is the maximum number of subdomains a domain is split into. Its value is sufficiently high and it must be changed only if an error message tells you to increase it. The expert parameter NTUPTC is the number of patches whose subpatches will be searched. In a very complex geometry, the value of this parameter can be increased if the calculation of the wall distances fails. Another expert parameter can be decreased in parallel with the increase of NTUPTC. This parameter is the real RTOL. It is the maximum angle allowed between two normals of a patch. If a larger value is found, the patch is subdivided. FINE™ 427 Flow Model Mathematical Model 43.6.1 BaldwinLomax The BaldwinLomax algebraic turbulence model, Baldwin & Lomax (1978) is a two layer model where the turbulent viscosity in the inner layer is determined using Prandtl’s mixing length model, and the turbulent viscosity in the outer layer is determined from the mean flow and a length scale. The strainrate parameter in Prandtl’s mixing length model is taken to be the magnitude of the vorticity. The influence on the mean flow equations through the turbulent kinetic energy is neglected. The turbulent viscosity is given by µt = ⎧ ( µ t ) i, n ≤ n c ⎨ ⎩ ( µ t ) 0, n > n c (436) where n is the normal distance to the wall, and n c is the smallest value of n at which the inner and outer viscosity is equal. The inner viscosity is 2 ( µ t ) i = ρl ω (437) where l = kn ( 1 – e + –y ⁄ A + ) (438) ⎛ ρ w τ w⎞ + ⎟ n y = ⎜ ⎝ µw ⎠ (439) and ω i = ε ijk ∂u j ∂ xk (440) with ε ijk the Kronecker symbol. The outer viscosity is ( µ t ) 0 = KC cp ρF wake F Kleb ( n ) (441) where F wake is the smaller of n max F max 2 and C wk n max 2 2 2 2 2 2 ( u + v + w )max – ( u + v + w ) min /F max (442) The term n max is the value of n corresponding to the maximum value of F , F max , where F(n) = n ω (1 – e + – n /A + ) (443) and 428 FINE™ Mathematical Model Flow Model 6 F Kleb = 1 + 5.5 ( nC Kleb /n max ) –1 (444) + The constants used are hard coded and equal: A = 26 , C wk = 1. , C cp = 1.6 , k = 0.41 , C kleb = 0.3 , K = 0.0168 .The turbulent Prandtl number, needed to calculate the turbulent conductivity, is accessible through the expert parameter PRT (see section 33.1.2). The expert parameter IATFRZ allows to control the interaction of the model with the multigrid system. When IATFRZ is set to 0, the model is applied separately on all grid levels. When it is set to 1, the model is only applied on the finest grid and the turbulent viscosity is restricted (through the restriction operator) to the coarser grids where the turbulent viscosity is frozen. It is possible to freeze the turbulent viscosity field on all grid level by setting IATFRZ to 2. The value can be automatically changed by using a criteria based on a maximum iteration number or on a minimum convergence. The maximum iteration number is specified by the expert parameter ITFRZ. The minimum reduction of order of magnitude is set in the expert parameter RESFRZ. 43.6.2 SpalartAllmaras The SpalartAllmaras turbulence model is a one equation turbulence model which can be considered as a bridge between the algebraic model of BaldwinLomax and the two equation models. The SpalartAllmaras model has become quite popular in the last years because of its robustness and its ability to treat complex flows. The main advantage of the SpalartAllmaras model when compared to the one of BaldwinLomax is that the turbulent eddy viscosity field is always continuous. Its advantage over the kε model is mainly its robustness and the lower additional CPU and Memory usage. The principle of this turbulence model is based on the resolution of an additional transport equation for the eddy viscosity. The equation contains an advective, a diffusive and a source term and is implemented in a non conservative manner. The implementation is based on the papers of Spalart and Allmaras (1992) with the improvements described in Ashford and Powell (1996) in order to avoid negative values for the production term ( S˜ in Eq. 450). The turbulent viscosity is given by ν t = ν˜ f v1 where ν˜ is the turbulent working variable and f v1 (445) a function defined by 3 χ f v1 = 3 χ + c v1 (446) with χ is the ratio between the working variable ν˜ and the molecular viscosity ν , ν˜ χ = ν (447) The turbulent working variable obeys the transport equation ∂ν˜ 1  + V ⋅ ∇ν˜ =  { ∇ ⋅ [ ( ν + ( 1 + c b2 )ν˜ ) ∇ν˜ ] – c b2 ν˜ ∆ν˜ } + Q ∂t σ (448) where V is the velocity vector, Q the source term and σ , c b2 constants. FINE™ 429 Flow Model Mathematical Model The source term includes a production term and a destruction term: Q = ν˜ P ( ν˜ ) – ν˜ D ( ν˜ ) (449) ˜ ν˜ P ( ν˜ ) = c b1 Sν˜ (450) 2 ν˜ ν˜ D ( ν˜ ) = c w1 f w ⎛ ⎞ ⎝ d⎠ (451) where The production term P is constructed with the following functions: ν˜ f ; S˜ = Sf v3 + 2 2 v2 κ d 1 f v2 = 3 ; ( 1 + χ ⁄ c v2 ) ( 1 + χf v1 ) ( 1 – f v2 ) f v3 = χ (452) (453) where d is the distance to the closest wall and S the magnitude of vorticity. In the destruction term (Eq. 451), the function f w is 6 fw = 1 ⎛ 1 + c w3 ⎞ 6 ⎟ g ⎜ 6 6 ⎝ g + c w3⎠ (454) with 6 g = r + c w2 ( r – r ) ; ν˜ r = 2 2 S˜ κ d (455) The constants arising in the model are 2 c w1 = c b1 ⁄ κ + ( 1 + c b2 ) ⁄ σ , c w2 = 0.3 , c w3 = 2. , c v1 = 7.1 , c v2 = 5. c b1 = 0.1355 , c b2 = 0.622 , κ = 0.41 , σ = 2 ⁄ 3 The equation Eq. 448 is solved with the appropriate boundary conditions: on solid wall ν˜ = 0 , along the inflow boundaries the value of ν t is specified ( ν˜ is obtained by using a NewtonRaphson procedure to solve Eq. 445) and along the outflow boundaries it is extrapolated from the interior values. 430 FINE™ Mathematical Model Flow Model 43.6.3 kε Turbulence Models a) General Formulation In the k – ε turbulence model two additional transport equations for the turbulent kinetic energy, k , and the turbulent dissipation rate, ε , are solved. In EURANUS, 4 linear and 2 nonlinear models are currently used. In the following, the trace of the tensor X will be written {X} In the k – ε turbulence model two additional differential equations need to be solved respectively for k and ε . These additional equations can be put in the following general form: µ ⎧ ⎫ ∂ρk  + ∇•⎛ ρwk – µ + t ∇k⎞ = – ⎨ ρw″ ⊗ w″ S ⎬ – ρε ⎝ ⎠ ∂t σk ⎩ ⎭ (456) ⎞ µ ⎧ ⎫ 1⎛ ∂ρε˜+ ∇•⎛ ρwε˜ – µ + t ∇ε˜⎞ = –  ⎜ C ε1 f 1 ⎨ ρw″ ⊗ w″ S ⎬ + C ε2 f 2 ρε˜⎟ + E ⎝ ⎠ T⎝ ∂t σε ⎠ ⎩ ⎭ (457) where S is the mean strain tensor and – ρw″ ⊗ w″ the turbulent Reynolds stress tensor. The variable ε˜ is the modified dissipation rate ε˜ = ε – D (458) and the turbulent viscosity µ t is given by the following relation µ t = ρC µ f µ kT (459) b) Linear Models In the linear models, the turbulent Reynolds stress tensor is related to the mean strain tensor in a linear way. 2 ( – ρ w″ ⊗ w″ )ij = 2µ t S ij – 2  ( ∇w )δ ij –  ρkδ ij 3 3 (460) ˜ ∂w˜ ⎞ 1 ⎛ ∂w S ij =  ⎜ i + j⎟ 2 ⎝ ∂ xj ∂ x i ⎠ The implemented linear models are:  Chien, low Reynolds number kε model (Chien, 1982).  Extended wall functions (Hakimi, 1997) = Standard high Reynolds (Launder & Spalding, 1974) if the expert parameter INEWKE is set to 0.  LaunderSharma, low Reynolds number kε model (Launder & Sharma, 1974).  YangShih, low Reynolds number kε model (Yang & Shih, 1993). FINE™ 431 Flow Model Mathematical Model The constants or functions Cµ, Cε1, Cε2, σk, σε, fµ,f1, f2, D, E and T are model dependent and they 2 0.5 k k y are defined in the Table 43 where Re t =  and Re y = νε ν TABLE 43 Coefficients kε Model of the kε models Chien Standard highRe Launder & Sharma Yang & Shih Cµ 0.09 0.09 0.09 0.09 Cε1 1.35 1.44 1.44 1.44 Cε2 1.80 1.92 1.92 1.92 σk 1.0 1.0 1.0 1.0 σε 1.3 1.3 1.3 1.3 1.0 – 3.4 2( 1 + ( Re t ) ⁄ 50 ) fµ 1–e – 0.0115y + e [1 – e a b c – ( Ax + Bx + Cx ) d ] x Rey A 1.5 104 a 1 B 5 107 b 3 C 1010 c 5 d 0.5 f1 1.0 f2 1 – 0.22e T k ⁄ ε˜ D 2νk ⁄ y E kw 1.0 1.0 1.0 1 – 0.3e k⁄ε k ⁄ ε˜ 0. 2ν ( ∇ k ) –2µε˜ e 2 y 0. 2νµ t ( ∇•S ) 0. uτ ⁄ Cµ / 2 – Re t ⁄ 36 2 – 0.5y 1.0 – Re t 2 1.0 k ⁄ ε + (ν ⁄ ε) 2 0.5 0. + 2 2 νµ t ( ∇•S ) 2 0.5 0. 0. 0. 2ν ( ∇ k ) DNS εw 3 0. u τ ⁄ ( κy ) / DNS 2 The constants Cµ, Cε1, Cε2, σk, σε can however be changed by the user (respectively the expert parameters CMU, CE1, CE2, SIGK, SIGE in the Computation Steering/Control variables page. The turbulent Prandtl number, needed to calculate the turbulent conductivity, is also an expert parameter (PRT). 432 FINE™ Mathematical Model Flow Model Two variants of the high Reynolds kε with wall functions (section d) Solid Boundary and Wall Functions) exist: • If the expert parameter INEWKE=10 (Default), the wall functions are derived from DNS (Direct Numerical Simulation) curve fitting. The kε model is in that case derived from the YangShih model. This new model, named extended wall functions, allows to obtain accurate results on fine mesh contrary to the standard high Reynolds kε model. • if the expert parameter INEWKE=0, standard wall function are applied and the y+ value of the near wall cell should be greater than 20. The Chien and the LaunderSharma models belong to the same family (zero value of ε at the wall) while the standard model and YangShih model belong to a second family (non zero value of ε at the wall). Launching the restart is allowed as long as the user sticks to the same family. c) Non Linear Models The nonlinear models are based on two linear models: the Yang and Shih model for low Reynolds variant and the Standard kε model for high Reynolds variant. c.1) The low Reynolds model The production term is modified through: i ⎛ fµ γRi t ⎞ 4 2 ⎟ kTS –  ρkI  ⎜ 1 – – ρw″ ⊗ w″ =  i 3A + f s⎝ 3 1 + γRi ⎠ µ 1 t C τ2 2 2 2 2 – kT' ⎛⎝ 2S – SΩ + ΩS –  { S }⎞⎠ 3 3 3 A2 + s + ω (461) C τ3 2 2 2 2 kT' ⎛ 2S + SΩ – Ω S –  { S }⎞ – 3 3 ⎝ ⎠ 3 A2 + s + ω where T is defined in Table 43 and: 1⁄3 T' = 1 ⁄ ( f t1 ⁄ T w + f t2 ⁄ T ) A2 T w = 2 2{S } ; 1 f t1 = 1 – 22 ( 1 + 2 { S }ν ⁄ ε ) ˜ j⎞ 1 ⎛ ∂w˜ i ∂w S ij =  ⎜ + ⎟ 2 ⎝ ∂ xj ∂ xi ⎠ ; f t1 f t2 = 1 – 1 + Re t ⁄ 70 ; 2 1 ⎛ ∂w˜ i ∂w˜ j⎞ Ω ij =  ⎜ – ⎟ 2 ⎝ ∂ xj ∂ xi ⎠ 2 2 s = T' 2 { S } ; ω = T' – 2 { Ω } ; Ri t = – ωs – ω and Cτ2 = 46; Cτ3 = 7; A1 = 4; A2 = 1000 and γ = 0.2 c.2) The high Reynolds model The model is modified in the following way: • f µ is set to unity FINE™ 433 Flow Model Mathematical Model • T’ is replaced by T The production term becomes: i γRi t ⎞ 4 1 ⎛ 2 ⎟ kTS –  ρkI – ρw″ ⊗ w″ =   ⎜ 1 – i 3 A1 + s ⎝ 3 1 + γRi ⎠ t C τ2 2 2 2 2 kT ⎛ 2S – SΩ + ΩS –  { S }⎞ – 3 3 ⎝ ⎠ 3 A2 + s + ω (462) C τ3 2 2 2 2 kT ⎛ 2S + SΩ – Ω S –  { S }⎞ – 3 3 ⎝ ⎠ 3 A2 + s + ω where s and ω are modified according to: 2 s = T 2{ S } (463) 2 ω = T –2 { Ω } The coefficients Cτ2, Cτ3, A1, A2 and γ remain unchanged. Note that the High Reynolds nonlinear model uses the wall functions as it is based on the standard kε model. Before launching the nonlinear model, it is recommended to apply first the linear model and restart from this solution. This procedure will provide a good initial solution for the nonlinear model and prevent the nonlinear terms to cause divergence of the code at the early stage. Since the nonlinear model is from YangShih, the restart can be done only from the YangShih model (linear or not) and the Standard model with wall functions. d) Solid Boundary and Wall Functions The values of kw and εw are imposed at the boundary for the Chien, Launder & Sharma and Low Reynolds nonlinear models, while for the Standard and nonlinear High Reynolds number models, it is imposed in the first inner cell. The wall friction velocity uτ is calculated through a wall function (Eq. 464 or Eq. 465) from the velocity at the cell center and the normal distance to the wall. For the models that do not use wall functions (Chien, Launder Sharma, Yang & Shih and Low Reynolds non linear model), the profile of the boundary layer is directly inferred from the input values at the wall. Consequently, particular attention must be paid to the grid refinement in this region in order to capture the viscous sublayer. A typical + value is given by 1 < y < 10 at the first node from the wall. The wall functions are used to mimic the presence of the walls by reflecting the effect of the steep, nonlinear variations of the flow properties through the turbulent boundary layer. They define the shear stress and the heat flux on the cell faces lying on solid boundaries as well as the values of k and ε in the vicinity of the wall. The wall functions are applied in the Standard (see kw and εw in Table 43 ) and in the High Reynolds non linear kε models. For the extended wall functions model, the wall functions for k and ε are fitted with polynomials to the DNS data. 434 FINE™ Mathematical Model Flow Model d.1) Velocity For smooth walls: The wall function in the viscous sublayer is given by: u +  = y uτ (464) yu ν + with y = τ , the dimensionless normal distance from the walls and u τ = τ wall ⁄ ρ , the wall friction velocity directly related to the wall shear stress. While in the turbulent layer, the wall function becomes: u 1 +  =  ln y + B κ uτ (465) where κ is the von Karman constant (default value 0.41) and B another constant (default value 5.36). They can be modified by the user in the Boundary Condition page. For rough walls: The wall function is given by (no viscous sublayer considered): u 1 y–d  =  ln 0 + B uτ κ k0 (466) where κ and B are defined just above and k0 and d0 are constants asked for each rough wall. The constant k0 is the equivalent roughness height while d0 is known as the height of the zero displacement plane, defined by u ( k 0 + d 0 ) = 0. (if B=0). For small roughness elements, d 0 = 0 . For high roughness elements, the flow behaves as if the wall was located at a distance d0 from the real wall position. ks k 0 = 30 where ks is the average roughness height + For rough walls, the constant B is usually zero (when ks+ > 70 with + ks y k s = y ). Otherwise the value of B is evolving as presented in below graph. + s FINE™ 435 Flow Model Mathematical Model When a rough wall is specified, the distance from the wall to the cellcentre of the first inner cell should be bigger than k0 + d0. In general, the first inner cell should be located within the fully turbulent layer. d.2) Temperature Similarly, for isothermal walls, the following laws are considered in the code: + T = Pr y + in the viscous sublayer (467) where Pr is the laminar Prandtl number and: + + Pr t y T =  ln ⎛ ⎞ + 13.2Pr ⎝ 13.2⎠ κ where in the turbulent layer (468) + Tw – T T =  . Tτ The heat flux at the wall is defined as: q w = ρCpuτ T τ (469) A complete description of the available thermal boundary conditions at walls is provided in section 85.3. The "law of the wall" distributions of velocity, temperature and other variables are assumed to prevail across the boundary layer. They are imposed at the node of a single + grid cell for which the user is advised to check that 20 < y < 100 . As a result, if the first cell node from the wall is placed too close, calculation is conducted in the viscous sublayer and the law is no longer valid. Similarly, if the first node is placed too far away, then a discrepancy may exist between the profiles and their assumed shape. e) Numerical Concerns This paragraph provides a description of the numerical method used to deal with the k and ε equations. e.1) Choice of the initial and boundary conditions Initial values for k and ε must be specified by the user, as well as the inlet boundary condition. The specified values at the inlet boundary can have a strong effect on the flowfield prediction. Several methods are proposed in section 43.5.4 to help the user in the choice of suitable values. e.2) Compressibility correction The compressibility correction is present only in the kε model of Chien and is useful only for high Mach number flows (M>3). Two kinds of compressibility effects are implemented: 1) the contributions from the modelled pressure gradientvelocity term and 2) the compressible dissipation. They can be activated by using respectively the expert parameters ICOPKE or ICODKE. The first compressibility correction is associated with the modelling of pressure gradientvelocity term in the equation of the turbulent kinetic energy, and, according to Zhang et al. (1991), leads to the source term Rk: 436 FINE™ Mathematical Model Flow Model µ t ∂ρ ∂p R k = – , 2 ρ σp ∂ xi ∂ xi (470) which modifies the term D of Eq. 458: µ t ∂ρ ∂p D' = D + . 3 ρ σp ∂ xi ∂ xi (471) Similarly a term R ε can be added to the ε equation. After Vandromme (1991) one has: µ t ε ∂ρ ∂p R ε = – C 3 , 2 ρ σ k ∂ xi ∂ xi (472) p which modifies the term E of Eq. 457: µ t ε ∂ρ ∂p E' = E – C 3 . 2 ρ σ k ∂ xi ∂ x i (473) p The above terms are included in the k – ε equations if the expert parameter ICOPKE is set to 1; if ICOPKE=0 (Default) they are set to zero. The empirical constants in these equations are two expert parameters (SIGRO and C3), with default values: σ p = 0.5 C 3 = 2.0 . (474) The second correction concerns the modelling of compressible dissipation. The physical foundation for this correction is the observation of decreased turbulent viscosity with increased Mach number (Nichols, 1990). The type of compressible dissipation is controlled by the expert parameter ICODKE. For ICODKE=0 no correction for compressible dissipation is done. In the correction of Sarkar (1989) (ICODKE=1), the dissipation of k is expressed as the sum of solenoidal ( ε ) and dilatational ( ε d ) components. The dissipation in the source term of the k equation (Eq. 456) is then corrected according to: 2 ε corr = ε ( 1 + αM t ) (475) with M t a turbulent Mach number defined as M 2 t k = 2a (476) where a is the speed of sound.The constant α is an expert parameter (ALF), with default value =0.5. Nichols (1990) developed a model that corrects the production term in the turbulent kinetic energy equation (ICODKE=2): ⎛ – ρw″ ⎝ FINE™ ⊗ w″ S⎞ ⎠ ( corr ) k = – ρw″ ⊗ w″ S ⎛ 1 – C p1 ( γ – 1 )M 2⎞ ⎝ a⎠ (477) 437 Flow Model Mathematical Model where a is the local speed of sound, γ is the specific heat ratio and C p1 an empirical constant (CP1 in the list of expert parameters available on the Control Variables page, with default value =4.). This correction improves the prediction of the turbulent production level by directly taking the effect of the Mach number (M) into account. e.3) Limiters for the turbulence variables Successive limitations are set for the turbulence variables to ensure physical values and the stability of the calculation. Indeed, the term sources in the kε equations can vary strongly especially at the beginning of the computation and lead to unphysical values and divergence. 1. To control the stability of the calculation, the expert parameter MAVRES, denoted here ζ , is used This parameter limits the variation of the turbulence variables for each RungeKutta stage. Denoting the new value of k or ε as q > 0: q n+1 q n+1 n+1 , the following restrictions are imposed when MAVRES = max ( q n+1 = min ( q n , EPS,ζq ) n+1 (478) n , ( 2 – ζ )q ) (479) where EPS is an expert parameter with a small value, default 1E28, also used to avoid possible divisions by zero. The restriction defined in Eq. 479 is not applied to the turbulent dissipation rate (ε) when this tends to increase, in order to avoid excessive values of the turbulent viscosity. If MAVRES = 0, only the restriction defined in Eq. 478 is applied (avoiding negative values) If MAVRES < 0, the restriction is: q n+1 n+1 n (1 + ζ)(q –q ) n – q = n + 1 n ⎛ q –q ⎞ ⎟ ⎜ 1 + n ⎝ ⎠ q (480) 2. A similar system is applied to the multigrid corrections with the expert parameter MAVREM, denoted below as ζ : If MAVREM > 0: q n+1 n – q < ( 1 – ζ )q n If MAVREM = 0: restriction to positive values If MAVREM < 0: q n+1 n+1 n –q ) (1 + ζ )( q n – q = n + 1 n ⎛ q –q ⎞ ⎟ ⎜ 1 + n ⎝ ⎠ q 3⁄2 k 3. The expert parameter LTMAX is used to limit the turbulence length scale L turb =  to a ε value compatible with the domain scale. If Lturb>LTMAX and MAVRES > 0, the value of ε is set to respect the maximum length scale. If Lturb>LTMAX and MAVRES <= 0, the values of k and ε are set to a small value EPS. The default value for LTMAX is 1E+6. 438 FINE™ Mathematical Model Flow Model 4. An automatic control of the turbulent length scale is possible by setting the expert parameter LTMAX to a negative value (LTMAX = 1). In this case, the following length scale control is proposed: L = min ( kT, 5le max ) (481) with le max the maximum equilibrium length scale in the computation, defined by –3 ⁄ 4 le max = κd max C µ (482) where d max is the maximum distance to the wall among all grid points of all blocks. The factor 5 in Eq. 481 is set to avoid to clip the length scale too early. The turbulent viscosity is then written as ν t = C µ f µ kL For the update of turbulent variables (previous paragraph), LTMAX is replaced by 5le max 5. Another way to control the turbulent length scale is the Yap’s modification. It is applied by setting the expert parameter IYAP to 1. In this case, the expert parameter LTMAX should be set to its default value (1.E+6) to avoid conflicts. Yap’s modification consists of adding to the epsilon equation a source term that control the turbulent length scale. It can be applied to all kε models. The source term to be added writes: l l 2ε S YAP = 0.83max ⎛  – 1, 0⎞ ⎛ ⎞ ⎝l ⎠ ⎝l ⎠ T e e where l and l e are respectively the turbulent length scale ( l = –3 ⁄ 4 length scale ( l e = κdC µ (483) kT ) and the equilibrium ). A weakness of Yap’s correction is that it might conflict with Inlet boundary conditions if these are set without respecting a turbulent length scale criteria. 6. The expert parameter TEDAMP is another parameter to control stability. This parameter prevents the factor 1 ⁄ T in the ε equation from being singular as k tends to zero (see Eq. 457 and the relationship between k and T in Table 43 ). A minimum of TEDAMP multiplication factor of the clipping value (expert parameter EKCLIP) is used for k . The same parameter is used to damp 1/ε coming from T in the calculation of the turbulent viscosity, Eq. 459: a minimum of TEDAMP multiplication factor of the clipping value (expert parameter EPCLIP) is used for ε . If TEDAMP<=0, the minimum values used for k and ε correspond to the expert parameter EPS. The default value of TEDAMP is 1. Irrespective of the value of TEDAMP, this strategy always avoids the use of possible negative values of k in the source term and of ε in the turbulent viscosity. FINE™ 439 Flow Model Mathematical Model 7. Another control on the stability is available through the parameter GAMMAT which introduces the turbulence time scale Tturb in the computation of the local time step: 1 1 GAMMAT  =  + ∆t kε ∆t T turb (484) The default value of GAMMAT is set to 10. 8. Another important consideration is the amount of turbulence production compared to its dissipa· tion, Prod ⁄ ( ρε ) . This quantity should stay within physically admissible ranges so that the turbulence production remains limited. The parameter PRCLIP allows the control of this ratio. As an example, Prod ⁄ ( ρε ) ≈ 1 for homogeneous core flows and thin shear layers, whereas Prod ⁄ ( ρε ) < 1 for separated shear layers and wakes. Flows of high shear, such as jets in cross · flow, can exhibit much higher values of Prod ⁄ ( ρε ) . An upper bound of PRCLIP=50 is recommended to the user. However, this control is removed by the use of a linearised turbulent production model introduced in all linear kε models. This simple modification is relevant for impinging flows, for which the turbulence models are well known to overestimate the turbulent production of kinetic energy. It corresponds to a linearisation of the production term when the strain rate is large when the expert parameter LIPROD is set at 1. 9. The expert parameters EKCLIP and EPCLIP are respectively the minimum allowable values of the turbulent kinetic energy (k) and the turbulent dissipation rate (ε). They avoid nonphysical negative values. Moreover the minimum value of k (EKCLIP) allows to maintain a minimum residual turbulence in the domain. The default value is 1.E5. The minimum value of ε is chosen so that the computed value of the turbulent viscosity is reasonable. With a default value set to 1.E5, the turbulent viscosity has a value of the order 1.E6. 10. The input parameter KEGRID allows the use of a particular full multigrid strategy for kε computations. The BaldwinLomax model is used on the coarse grids during the full multigrid stage and the k and ε initial solution is obtained from the BaldwinLomax model solution. KEGRID corresponds to the last grid level on which the algebraic model is used. For example, if the computation is done with 4 levels of multigrid and KEGRID is equal to 2, the BaldwinLomax model is used on the 333 (or level 4), 222 (or level 3) and 111 (or level 2) and the kε computation is initiated when transferring to the finest grid. If KEGRID is set to 3, the kε computation will be initiated when transferring to 222. If KEGRID is greater than the number of multigrid levels, the computation will be started on the coarsest level with kε. 11. The expert parameter IKENC allows solving kε equations with a nonconservative approach. This settings avoids the appearance of an artificial source term in the kε equations during the convergence process. This artificial term comes from the residuals of the equation of the mass conservation that can be nonnegligible at the beginning of the convergence process. This approach is new and not sufficiently tested to ensure that the loss of conservation is not excessive in all cases. 12. The expert parameter IKELED allows to avoid an excessive artificial dissipation of the standard central scheme into the boundary layer. Indeed this scheme can lead to a nonphysical relaminarisation in some specific test cases. An alternative computation of the artificial dissipation, based on the Local Extrema Diminishing (LED) version of the JamesonSchmidtTurkel treatment has been implemented. It is active when the expert parameter IKELED is set to 1. 440 All the above mentioned limiters are very important for the robustness of kε computations. With the exception of the length scale LTMAX all limiters are given appropriate defaults and we do not recommend to modify them. For LTMAX we recommend to set it to ten times the geometrical length scale. FINE™ Mathematical Model Flow Model 43.6.4 References Ashford G.A. , and Powell K.G. 1996, "An unstructured grid generation and adaptative solution technique for highReynolds number compressible flow", VKI (Von Karman Institute) Lecture Series 199606. Baldwin B., Lomax H. (1978) 'Thin Layer Approximation and Algebraic Model for Separated Turbulent Flows', AIAA78257. Chien K.Y. (1982) 'Predictions of Channel and BoundaryLayer Flows with a LowReynoldsNumber Turbulence Model', AIAA J., Vol. 20, No. 1. Hakimi N. (1997) ’Preconditioning methods for time dependent NavierStokes equations’, PhD Thesis, Dept of Fluid Mechanics, Vrije Universiteit Brussel. Jameson A., Schmidt W., Turkel E. (1981) 'Numerical Solutions of the Euler Equations by Finite Volume Methods using RungeKutta TimeStepping Schemes', AIAA811259. Jameson A., 1995, "Positive schemes and shocks modelling for compressible flows", International Journal for Numerical Methods in Fluids, Vol 20, pp 773776. Launder B.E. and Sharma B.I., 1974,"Application of the EnergyDissipation Model of turbulence to the Calculation of Flow Near a Spinning Disc", Letters in Heat and Mass Transfer, Vol. 1, pp. 131138. Launder B.E. and Spalding D.B., 1974, "The numerical computation of turbulent flow", Comput. Methods App. Mech. Eng., vol. 3, pp. 269289. Nichols R.H. (1990) 'A TwoEquation Model for Compressible Flows', AIAA paper 900494. Sarkar S., Erlebacher G., Hussaini M.Y., Kreiss H.O. (1991) 'The analysis and modelling of dilatational terms in compressible turbulence', J Fluid Mech, Vol.227, pp.473493. Spalart P.R. and Allmaras S.R. (1992),"A one equation turbulence model for aerodynamic flows",, AIAA 920439 Vandromme D. (1991) 'Turbulence Modelling for Compressible Flows and Implementation in NavierStokes Solvers', VKI Lecture Series 199102. Yang Z. and Shih T.H., 1993, "A ke model for turbulence and transitional boundary layer", NearWall Turbulent Flows, R.M.C. So., C.G. Speziale and B.E. Launder(Editors), ElsevierScience Publishers B. V., pp. 165175. Zhang H.S., So R.M.C., Speziale C.G., Lai Y.G. (1991) 'A NearWall Model for Compressible Turbulent Flow', ICASE Report 9182. 43.7 Gravity Forces When gravity should be taken into account the box marked Gravity Forces should be checked. If gravity is activated by checking this box three input dialog boxes appear to define the Gravity Vector. The default gravity vector is defined as: (gx,gy,gz)=(0,9.81,0) [m/s2], representing the gravity on Earth where the yaxis is oriented normal to the ground. When the gravity is taken into account in the NavierStokes equations, the source terms ρg and ρ ( g ⋅ V ) are respectively introduced in the momentum and energy conservation equations where ρ is the density, g the gravity vector and V the velocity vector. FINE™ 441 Flow Model Mathematical Model If the fluid is a liquid, the density is constant and you do not have any influence of the pressure or temperature on the flow by interaction with the gravity. To simulate these interactions, one can use the Boussinesq approximation in the gravity source terms. With this approximation, the density is developed in the first order of the MacLaurin series. It becomes: ρ = ρ ref + α ( p – p ref ) – β ( T – T ref ) (485) with α the compressibility and β the dilatation coefficients specified in the fluid properties. This variation of the density is only applied to the gravity source term (Boussinesq approximation). Otherwise, the density is kept constant in the conservation equations. The value of ρ ref is the characteristic density specified in the Flow Model page. p ref and T ref are the reference values in the Flow Model page. 43.8 When the gravity is taken into account, a reference pressure must be specified at a reference altitude to add the hydrostatic pressure in the initial pressure field. The reference pressure is the reference value in the Flow Model page. The reference altitude is specified in the expert parameter IREFPT. Low Speed Flow (Preconditioning) This option appears in the Flow Model page only if the fluid type is compressible. Indeed, the preconditioning is automatically used for an incompressible fluid. This option is only implemented for central schemes. Consequently, the upwind spatial scheme (Numerical Model page) is not available if the preconditioning option is chosen. 43.8.1 General Description In the low subsonic Mach number regime, timemarching algorithms designed for compressible flows show a pronounced lack of efficiency. When the magnitude of the flow velocity becomes small in comparison with the acoustic speeds, time marching compressible codes converge very slowly. The problems faced by compressible codes at low Mach number are: • High disparity between the convective eigenvalues u and the acoustic eigenvalues u+c, uc leading to a much too restrictive time step for the convective waves causing thus poor convergence characteristics. • Round off errors mostly due to the use of absolute pressure in the momentum equations. • Impossibility to treat strictly incompressible flows. Therefore the development of a low speed preconditioner was motivated in order to provide fast convergence characteristics and accurate solutions as the Mach number approaches zero. Over the past years and up to now, many attempts have been made to solve nearly incompressible flow problems within available compressible codes and with minor programming efforts. The corrective action brought to the discretization of the conservation equations is called preconditioning and is derived from the artificial compressibility method introduced for incompressible flows by Chorin, (1967). 442 FINE™ Mathematical Model Flow Model For steady state applications solved by time marching algorithms the time derivatives of the unknowns arising in the flow equations are of no physical meaning and can thus be modified without altering the final steady state solution. The idea of preconditioning precisely uses this property and consists of multiplying the time derivatives of the dependent variables with a matrix called preconditioning matrix. The main property of this matrix is to remove the stiffness of the eigenvalues. In addition, reduced flow variables such as the dynamic pressure and the dynamic enthalpy are introduced, reducing drastically the round off errors at low Mach numbers. The acoustic wave speed c is replaced by a pseudowave speed c’ of the same order of magnitude as the fluid speed. To be efficient the selected preconditioning matrix should be valid for inviscid computations as well as for viscous computations with heat transfer. The preconditioning methodology developed (Hakimi, 1997) is of sufficient generality and can treat any type of fluids including perfect gases and incompressible Newtonian and non Newtonian fluids. On the numerical level, the solution procedure including space discretization, time integration and boundary conditions have been adapted to the new transient behaviour of the conservation equations. The low speed preconditioner has been validated for inviscid flows, viscous flows, turbulent flows and unsteady flows. Efficient convergence rates and accurate solution have been obtained for Mach numbers from M=0.1 to M=106, Reynolds numbers from Re=106 to 106 and aspect ratios from 1 to 2000. 43.8.2 Basic Equations The preconditioned equations considered for a compressible fluid are: 1 ∂p ∂ρu ∂ρv ∂ρw + +  +  = 0 2 ∂t ∂x ∂y ∂z β ∂τ xx ∂τ yx ∂τ zx αu ∂p  + ρ du  + ∂p  =  +  + 2 ∂t dt ∂x ∂x ∂y ∂z β dv ∂p ∂τ xy ∂τ yy ∂τ zy αv ∂p  +  +  – ρg   + ρ  +  = 2 ∂t ∂x ∂y ∂z dt ∂y β (486) αw ∂p dw ∂p ∂τ xz ∂τ yz ∂τ zz  +  +   + ρ  +  = 2 ∂t ∂x ∂y ∂z dt ∂z β de ρ  + p ⎛ ∇ ⋅ V⎞ = ∇ ⋅ ⎛ k∇T⎞ + ε v ⎝ ⎠ ⎝ ⎠ dt Compared to the unpreconditioned NavierStokes equations a pressure time derivative is added to the continuity equation and also to the momentum equations. The internal energy equation is con∂v i sidered to build the system and εv is a dissipation term defined as: ε v = ⎛ τ ⋅ ∇⎞ ⋅ V = τ ij  ; ⎝ ⎠ ∂x j V = ( u, v, w ) is the velocity vector. At this stage the eigenvalues as well as the eigenvectors associated with the preconditioned method defined by Eq. 486 are already completely defined. 43.8.3 General Form of the Preconditioning Matrix The Preconditioned ReynoldsAveraged NavierStokes equations including turbulence and species transport equations written in a Cartesian frame of reference and integrated over a control volume Ω are expressed as: FINE™ 443 Flow Model Mathematical Model ∫∫∫Γ Ω – 1 ∂Q  dΩ + ∂t ∫ ∫ F ⋅ dS = ∫ ∫ ∫ ST dΩ (487) Ω S with T Q = ( p g, u, v, w, E g, ρk, ρε˜ ) . (488) The variable p g = p – p ref is the gauge pressure and the variables E g is the total gauge energy. For a perfect gas with constant Cv , E g is given by: 2 V E g = C v ( T – T ref ) + 2 (489) For an incompressible fluid with constant C p , Eg is given by: 2 V E g = C p ( T – T ref ) +  . 2 (490) The extension of the preconditioning matrix to the turbulence transport equations is then given in its general form both for compressible and incompressible fluids by: Γ * –1 = ⎛ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎜ ⎝ 1 2 β ( 1 + α )u 2 β ( 1 + α )v 2 β ( 1 + α )w 2 β 0 0 0 0 0 0 0 . . 0 ρ 0 0 0 0 0 0 . . 0 0 ρ 0 0 0 0 0 . . 0 0 0 ρ 0 0 0 0 . . 0 2 αv + Eg  ( – 1 )∗ 0 0 0 ρ 0 0 0 . . 0 2 β 0 0 0 0 0 1 0 0 . . 0 0 0 0 0 0 0 1 0 . . 0 ⎞ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎟ ⎠ (491) the term 1 should be added in compressible cases only. We notice from Eq. 491 that the preconditioning matrix does not apply to the transport equations of k and ε. This choice is the simplest and did not cause any particular instability for turbulent test cases run so far. 43.8.4 Eigenvalues of the System The eigenvalues of the preconditioned system defined by Eq. 486 are determined from the Euler part and can be obtained easily if the equations are written in terms of the primitive variables (p,u,v,w,p or e ). 444 FINE™ Mathematical Model Flow Model Their expression is given in 3D for compressible fluids by: λ 1 ,2, 3 = V ⋅ n 2 ⎛ 1 β⎞ λ 4 ,5 =  V ⋅ n ⎜ 1 – α + 2⎟ ± 2 ⎝ c ⎠ ⎛ ⎜V ⎝ 2 2 2 ⎛ ⎛ 2 ( V ⋅ n) ⎞ 2 β ⎞⎞ ⎟ β ⋅ n ⎜ 1 – α + 2⎟ ⎟ + 4 ⎜ n – 2 ⎝ ⎝ c ⎠⎠ c ⎠ (492) The two parameters α and β are chosen so that the stiffness of the eigenvalues is minimised at low speed. The corresponding eigenvalues for incompressible fluids are: λ 1 ,2, 3 = V ⋅ n 2 2 2 1 λ 4 ,5 =  V ⋅ n ( 1 – α ) ± ( V ⋅ n ( 1 – α ) ) + 4n β 2 (493) Compared to preconditioned system of compressible fluids, the first three eigenvalues are unchanged and the eigenvalues of the acoustic waves can be obtained by setting in Eq. 492 the speed of sound to infinity. We note in particular that the acoustic eigenvalues are always of opposite sign showing that the flow remains subsonic with respect to the pseudosonic speed. As for the compressible preconditioner the two parameters α and β are chosen so that the stiffness of the eigenvalues is minimised at low speed. Note that if a kε model is considered, the corresponding eigenvalues will be: λi kε = V⋅n (494) 43.8.5 Choice of the Parameters α, β and the Reference Velocity The user control variables are P ref, T ref ,α ,β . Pref ,T ref are accessible through the Flow Model page and are referred to as reference pressure and reference temperature. A value of Tref of the order of magnitude of the expected temperature field will reduce the machine roundoff errors influence on the temperature field. The value of Pref fixes the absolute level of the pressure in the field. This value is used in the equation of state for a compressible fluid and in the second order artificial dissipation term. A value of Pref close to the real pressure level is therefore recommended. The parameter α is accessible in the ‘Expert parameters’ list of the Control variables page as ALPHAP. According to several computations accomplished with the central scheme, good convergence rates were obtained for values of α lying in the range [1,1]. So far the best value is found to be α=1. This optimal value is not surprising since it increases the spectral radius and therefore adds an additional amount of artificial dissipation. Τhe preconditioning parameter β is imposed by the user in the Numerical Model page through a coefficient β∗ and a characteristic velocity U ref such that FINE™ 445 Flow Model Mathematical Model 2 2 β = β∗ U ref (495) U ref is representative of the maximum velocity in the flow field. For example, in external flows, Uref could be taken as the free stream velocity whereas in internal flows it could be taken as the maximum inlet velocity. For the user’s convenience, the constant Uref is however always set equal to the reference velocity specified in the Flow Model page and used in the calculation of the Reynolds Number. The choice of Uref has an influence on the convergence. The default value of β∗ is 3. Based on our experience with the presented low speed preconditioner the parameter β∗ can be taken of order unity for inviscid flow computations. For viscous computations associated with Reynolds numbers greater than about Re=1000, a constant value β∗ of order unity is also adequate. If convergence difficulties are encountered at the very beginning of a computation, it is recommended to increase the value of the parameter β∗. Remember however that a too large value of β∗ will introduce excessive artificial dissipation into the solution. For lower Reynolds number the parameter β∗ has to vary in order to preserve numerical stability and a good convergence rate. The parameter β∗ should increase as the Reynolds number decreases and may vary over several orders of magnitude (see Figure 4.3.84). If the local velocity scaling option is activated in the Numerical Model page, another definition of β is used: 2 2 2 β = β∗ max ( Uref, Uloc ) (496) where U loc is the local velocity. β * 10000 1000 100 10 1 1 10 FIGURE 4.3.84 Typical 100 1000 10000 Re variation of the preconditioning parameter β* with Reynolds number For high Reynolds flows it is suggested to choose β among the following values: • β=3 • β=30 • β=300 Too small or too big values of β may lead to divergence and to a too dissipative solution (if β is too high) 446 FINE™ Characteristic and Reference Values Flow Model 43.8.6 References Chorin, A. J. (1967) ’A numerical method for solving incompressible viscous flow problems’, J. of Comput. Phys., Vol 2, pp. 1226. Hakimi N. (1997) ’Preconditioning methods for time dependent NavierStokes equations’, PhD Thesis, Dept of Fluid Mechanics, Vrije Universiteit Brussel. 44 Characteristic and Reference Values 44.1 Reynolds Number Related Information The user has to specify some characteristic values (length, velocity and density). These values are used to calculate the Reynolds Number (only plotted when the kinematic viscosity is constant) that provides an useful information to choose the suitable model (section 43.5). These characteristic values can be used for other purposes as well. The characteristic length is used: — in the outlet boundary condition for which the mass flow is imposed with pressure adaptation, — in the computation of CP1 and CP3 for cylindrical cases. The characteristic velocity is used: — in the preconditioning method to compute the parameter β (see section 43.8.5), 2 — in the computation of the solid data Cf (normalized by ( ρ ref U ref ⁄ 2 ) ). The characteristic density is used: — in the Boussinesq approximation for incompressible fluid (Eq. 485), 2 — in the computation of the solid data Cf (normalized by ( ρ ref U ref ⁄ 2 ) ), — in the evaluation of the Reynolds number only when the dynamic viscosity of the fluid is specified in the Sutherland law on the Fluid Model page. 44.2 Reference Values The reference values have been introduced for the precoditioning to define a gauge pressure and a gauge total energy. Now these reference values have some additional uses which are described hereafter: — in the Boussinesq approximation for incompressible fluid (Eq. 485), — in the outlet boundary condition for which the mass flow is imposed with pressure adaptation. FINE™ 447 Flow Model 448 Characteristic and Reference Values FINE™ CHAPTER 5: 51 Rotating Machinery Overview The Rotating Machinery page contains the following thumbnails: • Rotating Blocks defining for each block typical information concerning cylindrical cases. This thumbnail is only available when the mesh is cylindrical (see Mesh/Properties... to see whether the mesh is cylindrical or Cartesian). See section 52 for more detail on this thumbnail. • Rotor/Stator defining the properties of each rotor/stator interface. This thumbnail is only available when the mesh contains Rotor/Stator interfaces. Rotor/Stator interfaces are defined in IGG™ as ROT boundary condition. For more detail on this thumbnail see section 53. • Throughflow Blocks giving access to twodimensional throughflow Euler simulation and this is only accessible for nonviscous flow (Euler selected as mathematical model on the Flow Model page). See Chapter 6 for more detail on the options available under this thumbnail. FINE™ 51 Rotating Machinery 52 Rotating Blocks Rotating Blocks FIGURE 5.2.01 Rotating Blocks on Rotating Machinery Page When selecting the Rotating Blocks thumbnail the page appears as shown in Figure 5.2.01. On the left a list of all blocks is displayed. It is possible to group the blocks that have the same properties on this page: 1. Select several blocks in the list of blocks by simply clicking on them. Clicking on a block deselects the currently selected block(s). It is possible to select several blocks situated one after another in the list by clicking on the first one and holding the left mouse button while selecting the next. To select a group of blocks which are not situated one after another in the list, click on each of them while keeping the key pressed. 2. Click on the Group button. A text box will appear just below the Group button. Place the cursor in the text box and type the name of the group and press . The name of the group will appear on the list of blocks in red with a plus sign on the left of the name. To see the blocks that are included in a certain group double click on the name of the group or click on the + symbol in front of the name. 3. To remove a group of blocks select the group and click on the Ungroup button. The group will be removed and the blocks that were in this group will be listed again in the list as separate blocks. On the right of the list with blocks the information is given for the selected block or group of blocks. If multiple blocks are selected the information is only displayed for the first selected block. For each block the current and maximum number of nodes in the three grid directions is given. Four items need to be defined by the user: the streamwise direction, the spanwise direction, the azimuthal direction and the rotational speed: — The streamwise, spanwise and azimuthal directions allow to determine the block orientation. Remark that if the AutoGrid module is used for the grid generation, the streamwise direction is automatically taken as being the kdirection, the spanwise direction as the jdirection and the azimuthal direction as the idirection. — EURANUS flow solver solves the equations in a relative frame of reference. This implies that the mesh blocks surrounding rotating blades rotate with the blades and should therefore been set as "rotating" in this page. The rotational speed of the block has to be given in RPM (Revolutions Per Minute). A positive value for the rotation speed indicates a rotation in pos 52 FINE™ Rotor/Stator Interaction in the FINE™ Interface Rotating Machinery itive θdirection with θ positive according to a right handed coordinate system. In Figure 5.2.02 this is illustrated for the case where the zaxis is the axis of rotation which is automatically the case in a mesh created with AutoGrid. FIGURE 5.2.02 Positive rotation speed The different computations in a project can not have different configuration settings. If any of the settings in this area is changed, the modifications will be taken for all (active and not active) computations. The rotation axis should be the zaxis in order to be compatible with the EURANUS flow solver. 53 Rotor/Stator Interaction in the FINE™ Interface The RotorStator thumbnail gives access to the definition of the rotor/stator interfaces as shown in Figure 5.3.03. This thumbnail is only accessible when the mesh contains rotor/stator interfaces. Rotor/stator interfaces are defined in IGG™ as ROT boundary condition. Consult the IGG™ manual for more detailed information on how to define this boundary condition. For more theoretical information on rotor/stator interfaces see section 55. The rotor/stator patches should not include R=0 regions. On the left the list of patches is displayed which are defined as part of a rotor/stator interface in IGG™ (boundary condition type: "ROT"). It is possible to display only a limited amount of patches by using the Filter. Type in the text box the part of the name that is common to all patches to display and press . All patches containing in the name the entered text will be displayed. Note that the filter is case insensitive. It is possible to group patches that have the same definition by selecting them in the list and clicking on the Group button. A text box will appear below this button which allows to enter a name for the group. The group will be displayed in red in the list of patches. Double click on the group name to see which patches are in the group. To select multiple patches select them while keeping the key pressed. To remove the group simply select the group from the list and click on Ungroup. The patches in the selected group will be put back into the list of patches and the group name will be removed from the list. FINE™ 53 Rotating Machinery Rotor/Stator Interaction in the FINE™ Interface Multiple rotor/stator interfaces can be treated in one single project. Each rotor/stator interface is indicated by an ID number and each of them may contain an arbitrary number of upstream and downstream patches. For each patch in the list the ID number of the corresponding rotor/stator interface has to be provided by the user. Also it should be specified whether the patch is located in the upstream or downstream side of the interface. It should be mentioned that no hypothesis is made on the direction of the flow through the interface. The purpose of the upstream and downstream denominations is only to establish the two groups of patches belonging to respectively the rotor and the stator side. .The ID number of the rotor/stator interface cannot be higher than the total number of rotor/stator interfaces. FIGURE 5.3.03 Rotor/stator Interface Definition In addition to the ID number and the upstream/downstream side specifications the user has to select also: • the order of extrapolation (zero or first order). Zero order extrapolation (default) is used in most cases and usually provides satisfactory results. First order extrapolation may be useful in case of important flow gradients in the direction normal to the interface together with a relatively coarse mesh. • one of the four available steady state techniques (for steady state applications only), i.e. the Local Conservative Coupling, Conservative Coupling by Pitchwise Rows, Full Non Matching Mixing plane and Full Non Matching Frozen Rotor approaches. 1. The first approach is only recommended for the rotor/stator interface between an impeller and a volute. Experience has shown that in cases where significant flow variations are observed in the circumferential direction (as for instance in the case of rotorvolute interactions) it is more stable to base the flux decomposition on the local flow direction as it is done in the Local Conservative Coupling. Small conservation errors can be observed with this technique, which is therefore only used for special configurations. 54 FINE™ How to Setup a Simulation with Rotor/Stator Interfaces? Rotating Machinery 2. The second approach is recommended due to its capability to provide an exact conservation of mass flow, momentum and energy through the interface. This approach adopts the same coupling procedure for all the nodes along the circumferential direction, even if the local flow direction is different from the averaged one. This technique offers the advantage of being able to guarantee a strict conservation of mass, momentum and energy through the interface. Moreover it shows to be very robust and is therefore used by default. 3. The third approach is respecting an exact conservation of mass flow, momentum and energy through the interface as the second approach but has less constraint on the interface geometry. 4. The fourth approach is considering the rotor/stator interface as a perfect connection and is neglecting the rotor movement in the connecting algorithm. In this approach, the periodicities must be equal between the rotor and the stator. 54 How to Setup a Simulation with Rotor/Stator Interfaces? Three different approaches are available in FINE™ to simulate the interaction between rotating and nonrotating blocks: Steady state: • Mixing plane approach: a pitchwise averaging of the flow solution is performed at the rotor/ stator interface and the exchange of information at the interface depends on the local direction of the flow. See section 54.1 for more detail on how to use this approach and section 55.3 and section 55.3 for the theoretical background. • Frozen rotor: a steady simulation of one specific position of the rotor with respect to the stator. For more information on how to set up a project according to this method see section 54.2. For its theoretical background see section 55.4.4. Unsteady: • Domain scaling method: unsteady simulation in which the mesh periodicities are constrained to be identical on both sides of the interface. See section 54.3 for more detail on how to use this approach and section 55.4 for the theoretical background. • Phase lagged method: unsteady simulation in which the mesh periodicities are not constrained to be identical on both sides of the interface. See section 54.4 for more detail on how to use this approach and section 55.3 for the theoretical background. 54.1 Mixing Plane Approach In the mixing plane approach the flow solution at the rotor/stator interface is azimuthally averaged and the exchange of information at the interface depends on the local direction of the flow. In this section it is described how to use this approach in FINE™. For more theoretical detail on the mixing plane approach itself consult section section 55.2 and section 55.3. 54.1.1 Geometrical Constraints The default mixing plane method (Local Conservative Coupling and Conservative Coupling by Pitchwise Rows) used in FINE™ imposes the following geometrical constraints: FINE™ 55 Rotating Machinery How to Setup a Simulation with Rotor/Stator Interfaces? • The patches on both sides of the rotor/stator interface must cover the same range in spanwise direction, • The meshes need not to match in the spanwise direction, but the azimuthal mesh lines on the boundary must be circular arcs. An illustration of these constraints is given in Figure 5.4.14. Consisting of two stripes, the depicted configuration provides a complete description of the capabilities. The upstream side of the quasisteady interface consists of three blocks, represented by the bold frames and the surface meshes, while a single block is assumed for the downstream side. A gap may exist between two blocks, e.g., if the mixing plane coincides with the exit plane of a blade row having a blunt trailing edge. The grid points distribution are different for each of the boundary patches involved, but the pitchwise grid lines have constant radius and the pitchwise line along which two patches of the same side join (e.g., BC 1 and BC 3) exists as an inner grid line on all other boundaries. In the example, the interface is thus decomposed into two stripes, stripe 1, consisting of BC 1 and BC 2 on the upstream side and BC 5 on the downstream side, and stripe 2, consisting of BC 3 and BC 4 on the upstream side and BC 6 on the downstream side. . FIGURE 5.4.14 Example of stripe configuration A new interpolation technique (Full Non Matching Mixing plane) has been implemented to avoid those geometrical constraints. This new technique is based on the full nonmatching algorithm and has clear advantages: • The geometrical constraints have been removed, the only remaining constraint being that the rotor/stator patches belonging to a given interface should lie on the same common axisymmetric surface. 56 FINE™ How to Setup a Simulation with Rotor/Stator Interfaces? Rotating Machinery • An exact conservation of the mass flow, momentum and energy is guaranteed. In special configurations such as rotorvolute interaction it is preferable to use Local Conservative Coupling and thus it may be required to use the previous approach (IRSNEW=0). When setting the expert parameter IRSNEW=1 only Full Non Matching Mixing plane approach will be applied on all rotor/stator interfaces even if another mixing plane approach has been selected in the Rotating Machinery page under RotorStator thumbnail. 54.1.2 Constraints on the Mesh Only one blade passage needs to be meshed for both the rotor and the stator, regardless of their respective periodicity. The boundary condition type must be set to "ROT" in IGG™ for all grid patches belonging to a rotor/stator interface. 54.1.3 Settings in FINE™ 1. The mixing plane approach is a steady simulation technique which requires to set on the Flow Model page the Time Configuration to Steady. 2. The patches that have boundary condition type "ROT" in the mesh are listed in FINE™ on the Rotating Machinery page under the RotorStator thumbnail. The user has to specify for each of these patches: • an ID number that will identify the rotor/stator interface (useful when multistage), • a switch to indicate if the patch is belonging to the "upstream" or "downstream" part of the rotor/stator interface. ID = 2 Upstream Upstream Downstream Downstream ID = 1 Flow Direction FIGURE 5.4.15 Aachen Turbine: Upstream/Downstream and ID number identification • the boundary condition: Local Conservative Coupling, Conservative Coupling by Pitchwise Rows or Full Non Matching Mixing plane as described in section 53. FINE™ When setting IRSNEW=1 only conservative coupling by pitchwise rows is available. Selecting local conservative coupling in the FINE™ interface will have no effect when IRSNEW=1. 57 Rotating Machinery How to Setup a Simulation with Rotor/Stator Interfaces? 54.1.4 Illustrative Example To illustrate the mixing plane approach the flow around a cube is considered as shown in Figure 5.4.16. The flow is entering the domain at the bottom of the figure. The upstream portion of the domain is the 'rotor' with a cube fixed on it. The second part is a 'stator'. Due to the pitch wise averaging process one can see that the vortex occurring slightly downstream the 'trailing edge' of the cube is spread when entering in the 'stator' component. If the rotational speed of the cube is high, this approximation is acceptable since one can consider that the stator "sees" a more statistically average flow. If the rotational speed is low, this approximation is essentially invalid and thus another method should be considered. FIGURE 5.4.16 Flow around a cube: Mixing Plane approach 54.1.5 Expert Parameters This section provides a summary of the expert parameters related to mixing plane approach. a) Selection of Technique IRSNEW = 0: default mixing plane interpolation technique imposing geometrical constraints as listed in section 54.1.1. = 1: new full nonmatching algorithm for rotor/stator interfaces removing the geometrical constraints of the default mixing plane technique. More detail on this interpolation technique can be found in section 55.3. 58 When setting IRSNEW=1 only conservative coupling by pitchwise rows is available. Selecting local conservative coupling in the FINE™ interface will have no effect when IRSNEW=1. FINE™ How to Setup a Simulation with Rotor/Stator Interfaces? Rotating Machinery b) Underrelaxation with Default Mixing Plane Approach NQSTDY gives the possibility to the user to update the rotorstator boundary conditions every NQSTDY iterations. If the parameter NQSTDY is set to zero (default), the update is done at every RungeKutta step. This is an underrelaxation technique that is rarely used. Before the mixing process, the averaged variables can be underrelaxed to stabilize the calculation: RQSTDY= 1 (default): no relaxation = 0 to 1: underrelaxation This is another underrelaxation technique that allows to limit the changes in the variables from one iteration to the next. This technique is used in special cases where stability problems are encountered. 54.2 Frozen Rotor The basic idea at the origin of the frozen rotor technique consists of neglecting the rotor movement in the connecting algorithm. The governing equations are solved for the rotor in a rotating frame of reference, including Coriolis and centrifugal forces; whereas, the equations for the stator are solved in a absolute reference frame. The two components are literally connected, and hence a rotorstator approximation is not required, rather the continuity of velocity components and pressure is imposed. As a result, the final steady solution will be depending on the relative position of the rotor and the stator. Unsteady 'history effect' (such as shedding separated zones) are neglected. It is usually well accepted that the frozen rotor approach is an appropriate solution for the treatment of rotorvolute interactions, where pitchwise variations of the flow are too important to be neglected. However, it requires the meshing of the complete impeller (all passages). Another drawback is that the flow solution depends on the rotor position. 54.2.1 Constraints on the Mesh Exactly as for the domain scaling approach a constraint must be satisfied on the mesh periodicity. The pitchwise distance must be the same for both side of the rotor/stator and coincident (no gap allowed between rotor and stator components in the pitchwise direction). For each different position of the rotor with respect to the stator a new mesh will have to be created in IGG™ and a new steady calculation has to be performed. 54.2.2 Settings in FINE™ There are three ways to run a frozen rotor calculation: 1. To mesh all blade rows completely and to use matching connections (CON) in IGG™ for the patches at the interface of the rotor and the stator. The blocks of the rotor should be made rotating, as well as the boundary conditions. A steady calculation can be run for this configuration. A non matching (NMB) connection or periodic non matching (PERNM) connection can not be used in this case: even though the computation might run the result would not be correct. This was previously the only way to perform frozen rotor calculations in FINE™. This approach is no longer used as the constraint on matching connections is too restrictive. 2. FINE™ Only CON matching connections are allowed in this first method. To create a mesh covering the same pitchwise distance on both sides of the interface and to impose Full Non Matching Frozen Rotor in the Rotating Machinery page under the RotorStator thumbnail. Furthermore the user has to specify for each of these patches the ID and the 59 Rotating Machinery How to Setup a Simulation with Rotor/Stator Interfaces? upstream/downstream location as described in section 5.4.1.3 at step 2. Therefore, the boundary condition type must be set to "ROT" in IGG™ for all grid patches belonging to a rotor/stator interface. 3. To start an unsteady computation by imposing iterations as a steady initialization in the Control Variables page. Note that for example for an impellervolute computation the complete impeller would need to be meshed in all three cases since the periodicity of the volute is 1. 54.2.3 Illustrative Example Results obtained from frozen rotor calculations usually look similar to unsteady ones. More detailed analysis shows that the approximation introduced in the connection algorithm induces a deviation of the wake when passing through the interface. FIGURE 5.4.27 Aachen Turbine: Frozen Rotor approach As an illustration the frozen rotor method is compared to the sliding mesh approach for the Aachen Turbine in Figure 5.4.27 and Figure 5.4.28. FIGURE 5.4.28 Aachen 510 Turbine: Domain Scaling (Sliding Mesh) approach FINE™ How to Setup a Simulation with Rotor/Stator Interfaces? Rotating Machinery 54.2.4 Expert Parameters The only expert parameter in case of a frozen rotor simulation is IRSNEW. This parameter should always be set to 2 when performing a frozen rotor simulation. 54.3 Domain Scaling Method The Domain Scaling Method is an unsteady simulation technique for rotor/stator interfaces. The effect of displacement due to rotation is taken into account. At each time step, the rotor is set at its correct position and equations are solved for that particular time step for the whole computation domain. The final solution is therefore a succession of instantaneous solutions for each increment of the rotor position. 54.3.1 Constraints on the Mesh The boundary condition type must be set to "ROT" in IGG™ for all grid patches belonging to a rotor/stator interface. The blade passages of each blade row to include in the mesh should cover the same pitch distance (have the same periodicity). If the periodicity of the rotor and the stator is not the same this can be solved in three different ways: • modelling a higher number of blade passages on each side to find a common periodicity, • scaling the geometry (with the scaling being as close to 1 as possible). The common way to scale the geometry is to modify the number of blades during the mesh generation process. The time frequencies are resolved with an error that is proportional to the scaling coefficient. • using the phase lagged approach explained in section 54.4. Apart from this constraint on the periodicity, there is no constraint on the patches and mesh nodes configurations. 54.3.2 Settings in FINE™ 1. Domain Scaling Method is an unsteady simulation technique so the Time Configuration in the Flow Model page should be set to Unsteady. 2. By default, in the Rotating Machinery page under RotorStator thumbnail, the Domain Scaling approach is selected. However the user has to specify for each of these patches the ID and the upstream/downstream location as described in section 5.4.1.3 at step 2. Therefore, the boundary condition type must be set to "ROT" in IGG™ for all grid patches belonging to a rotor/stator interface. 3. The initialization process can be performed in two ways: • A steady state initialization is performed in a separate computation with steady Time Configuration. It is suggested to model all rotor/stator interfaces in this case using frozen rotor approach. The unsteady domain scaling computation is using the result of this steady computation as initial solution. See Chapter 10 for more information on how to start a computation from an initial solution file. • The steady state initialization is automatically performed before starting the time accurate computation (that means within the same computation), switching to unsteady Time Configuration in the Flow Model page and selecting in the interface an appropriate Number of Steady Iterations in the Steady Initialization parameters on the Control Variables page. FINE™ 4. The Number Of Angular Positions is defined in the Control Variables page. 5. The Number Of Time Steps is defined in the Control Variables page. 6. The Outputs Files available in the Control Variables page are: 511 Rotating Machinery How to Setup a Simulation with Rotor/Stator Interfaces? • Output For Visualization/At end only and Multiple Files: multiple set of output files saved for restart of the unsteady computation and visualization in CFView™ only available at the end of the computation. • Output For Visualization/At end only and One Output File: one set of output files saved for restart of the unsteady computation and visualization in CFView™ only available at the end of the computation. • Output For Visualization/Intermediate and Multiple Files: multiple set of output files saved for restart of the unsteady computation and visualization in CFView™ during the computation. • Output For Visualization/Intermediate and One Output File: one set of output files saved for restart of the unsteady computation and visualization in CFView™ during the computation. IRSNEW =1 to activate the full nonmatching interpolation algorithm at the rotor/stator interface. This is in general recommended since it requires less memory and significantly reduces the preprocessing time. It also offers the advantage that conservation of mass, momentum and energy is guaranteed. Note: When a sliding mesh simulation with IRSNEW=1 is started from a mixing plane simulation with IRSNEW=0 it is not possible to use the *.fnmb file of the mixing plane simulation to read in the initialization of the sliding mesh simulation. It is necessary to compute the full nonmatching connections again. 54.3.3 Illustrative Example For the example case of the flow around a cube where the flow is entering the domain at the bottom of Figure 5.4.39. The upstream portion of the domain is the 'rotor' with a cube fixed on it. The second part is a 'stator'. With domain scaling approach, one can observe a strong vortex shed into the stator passage, leading to a correct physical simulation of the unsteady phenomenon (at the expense of much higher CPU time compared to mixing plane approach). FIGURE 5.4.39 Flow 512 around a cube: Domain Scaling method FINE™ How to Setup a Simulation with Rotor/Stator Interfaces? Rotating Machinery 54.3.4 Expert Parameters The following expert parameters can be used with an unsteady computation using domain scaling method: IRSNEW = 0 (default): old interpolation method at the rotor/stator interface IRSNEW = 1: full nonmatching interpolation at the rotor/stator interface. This is in general recommended since less memory is required. Parameters for Saving/Reading of PreProcessing Data: When IRSNEW = 0 (default approach): ISIDAT = 1 (default): preprocessing performed and results saved in the file with extension ".burs". ISIDAT = 2: preprocessing not performed, results read in the file with extension ".burs". When IRSNEW = 1 (new approach): IFNMFI =1 (default): preprocessing performed and results saved in .fnmb file. IFNMFI =2: preprocessing not performed and results read from .fnmb file. In both cases the preprocessing needs to be restarted if either the Number Of Angular Positions or the number of grid levels is changed. ICYOUT =1 is used in combination with Multiple Files option to avoid overwritting of the output files at each blade passage. 54.4 Phase Lagged Method The Phase Lagged Method is an unsteady simulation technique for rotor/stator interfaces. The effect of displacement due to rotation is taken into account. At each time step, the rotor is set at its correct position and equations are solved for that particular time step for the whole computation domain. The final solution is therefore a succession of instantanious solutions for each increment of the rotor position. This method is allowing the user to reduce the CPU time needed for computing an unsteady simulation of a turbomachinery stage (rotorstator interaction). This capability has been implemented as an additional functionality into the release FINE™/Turbo. 54.4.1 Constraints on the Mesh The only constraints is that the boundary condition type must be set to "ROT" in IGG™ for all grid patches belonging to a rotor/stator interface. It is recommended to have an overlapping in the circumferential direction between the channel(s) of the rotor and the channel(s) of the stator. 54.4.2 Settings in FINE™ 1. Phase Lagged Method is an unsteady simulation technique so the Time Configuration in the Flow Model page should be set to Unsteady. 2. At the top of the Rotating Machinery page, the Phase Lagged option has to be activated and under RotorStator thumbnail, the Phase Lagged approach is selected automatically. However the user has to specify for each of these patches the ID and the upstream/downstream location as described in section 5.4.1.3 at step 2. Therefore, the boundary condition type must be set to "ROT" in IGG™ for all grid patches belonging to a rotor/stator interface. 3. The initialization process can be performed in two ways: FINE™ 513 Rotating Machinery How to Setup a Simulation with Rotor/Stator Interfaces? • A steady state initialization is performed in a separate computation with steady Time Configuration. It is suggested to model all rotor/stator interfaces in this case using frozen rotor approach. The unsteady domain scaling computation is using the result of this steady computation as initial solution. See Chapter 10 for more information on how to start a computation from an initial solution file. • The steady state initialization is automatically performed before starting the time accurate computation (that means within the same computation), switching to unsteady Time Configuration in the Flow Model page and selecting in the interface an appropriate Number of Steady Iterations in the Steady Initialization parameters on the Control Variables page. 4. The Number Of Angular Positions defined in the Control Variables page is the number of time step per full revolution (2π) of the rotor. In theory, the number of time step per full rotation has to be a multiple of the number of blades in the rotor (Nbrotor) and number of blades in the stator (Nbstator). Number Of Angular Positions = i x Nbrotor x Nbstator 5. The two periods of blade passing frequencies are respectively (ixNbrotorx∆t) and (ixNbstatorx∆t). Since the number of time step per passage is usually imposed around 40, the value of i should be adjusted so that (ixNbrotor) and (ixNbstator) are both close to this number. By experience, if the number of time step per passage is lower than 30 the solution starts to be deteriorated. The Number Of Time Steps in the Control Variable page is defined as: Number Of Time Steps = j x (Number Of Angular Positions)/min(Nbrotor,Nbstator) 6. During the calculation, it is recommended to repeat the longer period at least 15 to 20 times (j evolves from 15 to 20). By experience, usually after 20 times (j=20), the flow becomes periodic. There are thus no need to make many full rotation and sometimes even one full rotation. The Outputs Files available in the Control Variables page are: • Output For Visualization/At end only and Multiple Files: multiple set of output files saved for restart of the unsteady computation and visualization in CFView™ only available at the end of the computation. • Output For Visualization/At end only and One Output File: one set of output files saved for restart of the unsteady computation and visualization in CFView™ only available at the end of the computation. • Output For Visualization/Intermediate and Multiple Files: multiple set of output files saved for restart of the unsteady computation and visualization in CFView™ during the computation. • Output For Visualization/Intermediate and One Output File: one set of output files saved for restart of the unsteady computation and visualization in CFView™ during the computation. 514 By default, the Phase Lagged method used to compute the viscous fluxes at the rotor/ stator interface from dummy cells values set from other side inner cells instead from same side inner cells by extrapolation (more detail in section 55.4.3). FINE™ Theoretical Background on Rotor/Stator Interfaces Rotating Machinery 54.4.3 Illustrative Example Results obtained from Phase Lagged calculations usually look similar to unsteady ones when the expert parameter IRSVFL=1. Old Viscous Fluxes Detection at R/S interface New Viscous Fluxes Detection at R/S interface IRSVFL = 0 IRSVFL = 1 FIGURE 5.4.410 Aachen Turbine: Domain Scaling method: IRSVFL=0 vs IRSVFL=1 54.4.4 Expert Parameters The following expert parameters can be used with an unsteady computation using phase lagged method: ICYOUT =1 is used in combination with Multiple Files option to avoid overwritting of the output files at each blade passage. RELPHL =0.5 0.5 if necessary, underrelaxation factor can be applied on Periodic and R/S boundary conditions by reducing the two values of the expert parameter for respectively the periodic and the R/S boundary conditions. NPLOUT =0 (by default) enables to visualize multiple non periodic passage output in CFView™ by loading the corresponding ’.cfv’ file. 55 Theoretical Background on Rotor/Stator Interfaces 55.1 Introduction The relative motion between successive blade rows together with boundary layers, wakes, shocks and tip leakage jets are the major sources of unsteadiness that may affect a turbomachinery flow locally or as it travels through the next rows. All these interactions are strongly coupled, increasing in magnitude as the gap between successive blade rows is decreased, and affecting consequently the performance of the machine. FINE™ 515 Rotating Machinery Theoretical Background on Rotor/Stator Interfaces Solving for such flows requires an unsteady and viscous flow solver with the capability to manage enormous data storage. One way to optimize the computer memory requirement is to resolve the steady flowfield on a truncated computational domain. This requires a pitchwise averaging process to be performed at the socalled rotor/stator interfaces. This particular boundary condition is available under the FINE™/Turbo environment as the mixing plane approach. The rotorstator interaction is done by exchanging circumferentially averaged flow quantities. Physically, this means that the blade wake or separation occurring in the blade passage are mixed circumferentially before entering the downstream component. As a result, the velocity components and pressure is uniform in the circumferential direction at the rotor/stator interface. This physical approximation tends to become more acceptable as rotational speed is increased. This mixing plane technique is by far the most used rotor/stator modeling in industry approach. See section 55.2 and section 55.3 for more detail on the mixing plane approach. The second step allowing for a higher level of accuracy consists of considering an unsteady rotor/ stator interaction. Various techniques allowing to treat configurations with an arbitrary number of blades in the rotor and the stator have been proposed by many authors (Giles, 1990, Lemeur, 1992, Erdos et al, 1977, He, 1997), each of them having their own advantages and disadvantages, each of them affecting differently the memory requirement, solution time and the most important parameter, the accuracy of the computed flow solution. But none of these techniques allows to resolve on a truncated computational domain all time frequencies present in the turbomachinery configuration, except if the pitch distance is the same in the successive rotors and stators. In fact, each of them are affecting the computed time frequencies and Fourier modes that are propagating the flow information inside the gap region. The Domain Scaling Method is another type of unsteady rotor/stator interface treatment (Rai, 1989), that has been selected and implemented in the EURANUS flow solver. This technique is based on the constraint that the pitch distance must be identical on both sides of the interface. If the numbers of blades in the rotor and the stator are different, this implies either to increase the number of passages modelled or to scale the geometry. The Domain Scaling Method presents the advantage that it allows to resolve all time frequencies with an error that is proportional to the scaling coefficient. The accuracy of the computed unsteady flow solution may then be improved at the expense of more data storage and larger solution time if more blade passages are considered. Finally, the Phase Lagged Method is the last type of unsteady rotor/stator interface treatment that has been selected and implemented in the EURANUS flow solver. This technique is removing the Domain Scaling constraint that the pitch distance must be identical on both sides of the interface. The Phase Lagged Method presents the advantage that it allows to resolve all time frequencies with an error that is proportional to the scaling coefficient. The accuracy of the computed unsteady flow solution may then be improved at the expense of more data storage and larger solution time if more blade passages are considered. 55.2 Default Mixing Plane Approach 55.2.1 Geometrical and Topological Constraints The rotorstator interfaces are defined by stripes. A stripe is the element along which the required averaging in tangential direction is carried out. It is composed of a number of boundary patches which must cover the same range in the spanwise direction. The upstream and the downstream sides are distinguished. Each boundary condition must belong either to the upstream or to the downstream side. These two sides communicate through the exchange of pitchaveraged variables. The meshes do not need to match in the spanwise direction, but the azimuthal mesh lines on the boundaries must be circular arcs. 516 FINE™ Theoretical Background on Rotor/Stator Interfaces Rotating Machinery 55.2.2 Communication Process On both sides, the flow state is extrapolated from the inner cells onto the interface. It is then interpolated onto meshes that share the same spanwise grid point distribution on both sides. The pitchwise averaging is carried out on those meshes and the mixing process, depending on the boundary condition type, is applied. This mixing process combines the variable on one side of the interface with the pitchwise averaged variables of the other side. Once the mixing process is completed, the flow state is interpolated back onto the initial mesh interface and the dummy cells are set to impose the calculated variables on the interface. The extrapolation of the flow state from the inner cells onto the interface can be done using different techniques. These are the same as those used by the outlet boundary conditions exposed in section 85. Before the mixing process, the averaged variables can be underrelaxed to stabilize the calculation. The relaxation factor is user input (RQSTDY), the default value being 1, which means that no underrelaxation is performed in the default configuration of the solver. The possibility is given to the user to update the rotorstator boundary conditions every NQSTDY iterations. If the parameter NQSTDY is set to zero (default), the update is done at every RungeKutta step. 55.2.3 Different Available Boundary Conditions The rotor/stator interface included in the EURANUS flow solver exchange the mass, momentum, and energy fluxes instead of the classical primitive variables. The advantage of a fluxbased approach is that a more strict global conservation through the interface is ensured. Two kinds of boundary conditions are currently available and are described in this paragraph: • The local conservative coupling (with flux decoding), • The conservative coupling by pitchwise rows (no flux decoding). a) Local Conservative Coupling (With Flux Decoding): On each mesh point of both sides of the interface, a test is done to detect whether the interface can be considered as a sub or supersonic in or outlet. Then a transfer of the fluxes and pressure from the other side is performed depending on the result of the test. • If the side is considered as a supersonic inlet, all the averaged fluxes from the other side are taken with the averaged pressure. • If the side is considered as a subsonic inlet, the averaged fluxes are taken from the other side. The local pressure is kept. • If the side is considered as a subsonic outlet, only the pressure is transferred from the other side. The local fluxes are kept. • If the side is considered as a supersonic outlet, nothing is taken from the other side. Once the transfer is completed, a decoding of the fluxes with pressure is carried out on each side with the formulas which depend on the type of fluid. Compressible flows For compressible flows, the density, velocity vector and pressure are derived from Q ρ, Q v, Q E , respectively the flux of mass, the flux of momentum plus the pressure force and the flux of energy. The other variables such as k or ε are also derived from their fluxes. They are referred to, in the following as X an QX. The fluxes are constructed from the primitive variables using: FINE™ 517 Rotating Machinery Theoretical Background on Rotor/Stator Interfaces Qρ = ρ ( V ⋅ S ) Q v = ρV ( V ⋅ S ) . (51) 2 Q E = ρ ( CpT + V ⁄ 2 ) ( V ⋅ S ) Q X = ρX ( V ⋅ S ) where ρ is the density, V the absolute velocity vector, T the temperature, Cp the heat capacity and S the surface vector of the cell face. After application of the mixing process the primitive variables are calculated from the fluxes using: Qv ⋅ S ± p s = 2 S (γ + 1) ⎛ Qv ⋅ S ⎞ ⎟ ⎜ 2 ⎝ S ( γ + 1 )⎠ 2 · 2 ( γ – 1 ) ( Q v – ( 2Q ρ Q E ) ) + 2 S (γ + 1) Qv – ps S v = Qρ (52) Qρ ρ = v⋅S Q X = XQρ where γ is the specific heat ratio. Incompressible flows For incompressible flows, the velocity vector and pressure are derived from Q ρ, Q v , respectively the flux of mass and the flux of momentum plus the pressure force (See Eq. 51). The other variables like k or ε are also derived from their fluxes. They are referred to, in the following, as X and QX. As far as the energy equation is concerned, the temperature is also derived from its flux like the other X variables. 2 ( Qv ⋅ S – Qρ ⁄ ρ ) p s = 2 S ( Qv – ps S ) V = Qρ (53) QX X = Qρ b) Conservative Coupling by Pitchwise Rows (No Flux Decoding): The local conservative coupling approach presents two weaknesses: • The decoding of the fluxes might in some case lead to a blow up of the process, especially at transonic flow conditions, because of the presence of a square root in Eq. 52, whose positivity is not always guaranteed. • The local approach may lead to opposite decisions on the flow direction for the corresponding mesh points of both sides of the interface, which as a consequence decreases the accuracy on the global conservation. 518 FINE™ Theoretical Background on Rotor/Stator Interfaces Rotating Machinery Therefore a new boundary conditions has been developed, in which the decision on the direction of the flow is taken only once per pitchwise row, and which avoids the fluxes decoding. This new boundary condition has shown to be more robust in most cases and guarantees a strict global conservation. As mentioned in section 53 the only type of application for which a local approach would better suit is the impellervolute interaction. 55.3 Full Nonmatching Technique for Mixing Planes 55.3.1 Concept The major purpose of the development of the new mixing plane module was the elimination of the geometrical constraints imposed by the previous module. The new module uses the concept of image. An image of the real mesh patches is built on both sides of the interface, the left and right images respecting the above constraints and being in addition matching in the spanwise direction. The only remaining constraints are the followings: • the hub and the shroud lines are assumed to be located on a circular arc, and each extremity of the hub and shroud lines should coincide with one corner of one of the patches. • all patches constituting a rotor/stator interface should form a filled closed surface with no gap • the rotor/stator patches should be fully included in the rotor/stator interface: contrary to the full non matching algorithm, which includes an automatic detection of the connection zone, and in which the patches can then be partially connected, the rotor/stator module assumes that the patches are fully connected. FIGURE 5.5.311 Creation of the image mesh One image mesh is constructed on both sides of the interface. It respects the following constraints: FINE™ 519 Rotating Machinery Theoretical Background on Rotor/Stator Interfaces • The image is a "concatenation" of all the patches constituting the left or right side of the interface. • The pitchwise mesh lines lie on circular arcs. • The left and right images have the same spanwise distribution of the nodes. • The mesh density of the image is similar to the one of the initial patch. The creation of the image mesh is illustrated by Figure 5.5.311, showing the creation of the image of a butterfly configuration. With the previous version of the mixing plane module such a configuration would have required the creation of an intermediate block with one face connected to the butterfly and the opposite face respecting the constraints of rotor/stator patches. 55.3.2 Implementation of Mixing Plane Approach with Full Nonmatching Technique The communication algorithm between rotors and stators is organised in several steps: 1. Extrapolation of the flow solution from the inner cells to the boundary: the cylindrical velocity components are extrapolated. 2. Sending of the flow solution from the initial mesh to the image (on both sides): an interpolation tree is built between the image and the initial mesh, by applying the full non matching connecting algorithm. 3. Application of the mixing plane algorithm between the left and right images, with construction of flux variables to be imposed on the left and right side. 4. Sending of the fluxes from the image to the initial meshes: this is again performed with the aid of the full non matching algorithm, which allows for an exactly conservative distribution of the calculated fluxes throughout the cells. The transformation of the flux variables to the primitive ones is not required, as the fluxes are directly added to the residuals of the finite volume scheme, without the use of the dummy cells. The mixing plane algorithm implementation is similar to the one of the previous module. Only the conservative coupling by pitchwise rows has been implemented. The algorithm is organised under the following steps: 1. Calculation of the flux variables on both sides F 1 = ρV n ∆S F 2 = ρV r V n ∆S F 3 = ρV θ V n ∆S F 4 = ρV z V n ∆S F 5 = ρHV n ∆S 520 2. For all spanwise positions perform a pitchwise averaging of the flux and of the primitive variables. 3. For all spanwise positions determine the upstream and downstream side according to the flow direction, and build the mixing plane fluxes. FINE™ Theoretical Background on Rotor/Stator Interfaces Rotating Machinery The local fluxes on the upstream side are taken from the upstream, with a contribution of the averaged downstream static pressure.: ups ups F1 ups = F1 ups F2 = F2 + p ups down n r ∆S ups F3 = F3 ups ups F4 = F4 + p ups F5 down n z ∆S ups = F5 On the downstream side the local fluxes are taken as the averaged fluxes on the upstream side with a contribution of the local static pressure: ups down = F1 F1 down F2 ups = F4 + p down 55.4 n r ∆S = F3 down F5 down ups down F3 F4 ups = F2 + p down n z ∆S ups = F5 Domain Scaling Method The Domain Scaling Method considers in the computational domain respectively K1 and K2 blade passages with the following condition to be satisfied: K1 P1 = K2 P 2 . (54) where the indices 1 & 2 refer to the upstream and downstream sides of the interface, and P1 & P2 are the pitches of the two connected blade rows. If the numbers of blades in respectively the rotor and the stator are not equal, the user should make the choice between: • modelling a higher number of blade passages (or even the entire machine if a common multiple can not be found). If for instance the numbers of blades are 16 & 24, the numbers of passages to model are respectively 3 & 2. This permits to avoid the introduction of an error due to the geometry scaling, at the cost of an increased memory requirement. • scaling the geometry. The easiest way to proceed in order to obtain the required scaling is to generate a mesh with a blade number different from the real one. The ratio between the modified and the real blade numbers should be as close as possible to 1.0. In some cases the most appropriate treatment may be a combination of the 2 above approaches. If for instance the numbers of blades are 18 & 24, one could scale the stator by changing the number of blades from 18 to 16, and then choose to model 2 & 3 passages. The scaling factor is then 1.125, instead of 1.33 in case only one blade passage is modelled. The major advantage of having the same pitch distance on both sides of the interface is that it permits to avoid considering any time periodicity in the boundary condition treatment. The boundary conditions to be imposed along the periodic boundaries inside the gap region are given by FINE™ 521 Rotating Machinery Theoretical Background on Rotor/Stator Interfaces R R R R U i ( r, θ i , z, t ) = U i ( r, θ i ± p, z, t ) i = 1, 2 , (55) where p = K 1 P 1 is the pitch distance on both sides of the interface. The “+” sign is to be used when imposing boundary conditions on the lower periodic segment (minimum azimuthal coordinates) and the “” sign is to be used for the higher periodic segment (maximum azimuthal coordinates). Along the rotor/stator interface, the boundary condition is defined as R(i) Ui R(i) ( r, θ i R(i) R(i) , z, t ) = U 3 – i ( r, θ i – mp, z, t ) R(i ) where the parameter m is selected such that the point θ i m∈Z i = 1, 2 , (56) – mp is part of the computational domain of row 3i to allow for the interpolation across the interface. Since only the spatial periodicity is accounted for in the connecting boundary condition, the periodic surfaces become simple nonmatching rotating boundaries, while the interface is a nonmatching connecting boundary. The solution procedure is then as follows, for each physical time t: • Rotate the grid in function of the physical time step and of the rotation speed of each row. • Resolve the flowfield at the given physical time t. The boundary conditions to be imposed along the periodic segments are defined by equation Eq. 55. The boundary condition to be imposed along the interface boundary is defined by equation Eq. 56. • Save the flow solution for future postprocessing. This method does not impose any time periodicity in the boundary condition treatment and thus, allows to capture all time frequencies of the various unsteady interactions, but occurring on a modified geometry due to the grid scaling. The effect of the grid scaling on the accuracy of the computed flow solution is of great importance when comparing computational results with the experimental data, as another onestage configuration has been truly resolved. These effects may be summarized as: • a shift in the spectrum of time frequencies for the blade row that has not been scaled. • the modification in both blade rows of the Fourier modes that are propagating the flow information. The unsteady governing flow equations are resolved in the relative system of each row. Thus, no grid rotation needs to be performed at each physical time step and only the interpolation data structure needs to be modified in function of the relative position of each component. For example, a downstream rotor will see an upstream stator moving in the opposite direction of its own rotation velocity, while the upstream stator will see the rotor moving in the direction of the rotor rotation velocity. Finally, the previous implementation lets the rotor do the full rotation. The problem in this method is that the rotor and the stator are in front of each other for a little fraction of time. During this time, no time shift is necessary at the R/S interface which acts then as a pure connection. The modification proposed aims at increasing the time during which the R/S interface acts as a connection. To perform this, only the periods during which the rotor and the stator are in front of each other, are repeated. But, since the length of the periods are different in the 2 blades rows, the solution has to be stored and reset in the row with the smallest period. Example: if row 1 has the highest number of blades and therefore is submitted to the larger period, this last period T1 is repeated over and over, while a fractional number of periods will be simulated in row 2. The solution is thus stored at the end of the last completed period in row 2, to be reused at the beginning of each T1. This method increases a lot the speed of exchange between the two blade rows. It increases also the robustness of the computation. 522 FINE™ Theoretical Background on Rotor/Stator Interfaces Rotating Machinery 55.4.1 Full Nonmatching Approach (IRSNEW=1) It is highly recommended to activate the FNMB approach when using the domain scaling method as it presents several advantages: • smaller preprocessing CPU time, • smaller memory requirement, • strict conservation of mass, momentum and energy. The implementation is practically identical to the one that is adopted in the steady state frozen rotor approach. The FNMB connecting algorithm is used in order to exchange the flow variables and fluxes between the left and right image. The difference in the case of unsteady calculations is that the boundary condition patches linked to the rotor side need to be positioned according to the current time step. This implementation is organised in nearly the same way as the mixing plane approach, except from the fact that the mixing plane technique applied between the two image must be replaced by an additional full nonmatching connection. The global organisation is the following: 1. Extrapolate the inner flow solution to boundary condition patches (on both sides), 2. Interpolate the flow solution from initial patches to the image (on both sides), 3. Full nonmatching connection between the two images (with appropriate rotation of the rotorlinked image), 4. Transfer of the calculated fluxes to the initial boundary condition patches. 55.4.2 Sliding Grid Interpolation Approach (IRSNEW=0) The sliding grid interpolation approach is still available (IRSNEW=0), mainly for backward compatibility reasons. This connection algorithm is based on a high order interpolation of the flow variables. Although well validated the approach does not strictly guarantee conservation. Another drawback is that different interpolation data structures are built for all relative stator/rotor positions, with as a consequence a very long preprocessing time. 55.4.3 Improved Rotor/Stator Viscous Fluxes (IRSVFL=1) The previous implementation of the R/S interface only ensured the continuity of the inviscid fluxes. The viscous fluxes were computed at the interface from the value in the dummy cells which were extrapolated from the inner cells. This new implementation simply interpolates the value from the other side inner cells to the dummy cells, reproducing the correct behaviour of a connection (Figure 5.5.412). FIGURE 5.5.412 Rotor/stator FINE™ interface improvement: viscous fluxes continuity 523 Rotating Machinery Theoretical Background on Rotor/Stator Interfaces X’ and X” are respectively extrapolated on R/S interface from X3 and X4. Then X2’ is interpolated from X’ and X”. Finally, X2” is defined in the dummy cell by extrapolating X2 (result coming from the stator) and X2’ (result coming from the rotor). This last method, automatically activated when dealing with phaselagged simulation, can be activated for non phaselagged simulation through the expert parameter IRSVFL (by default set at 0) that has to be set at 1. 55.4.4 Frozen Rotor The frozen rotor technique consists of a simple connecting boundary condition, ignoring the rotation of the rotor. The implementation is identical to the one adopted in the full nonmatching domain scaling approach (section 55.4.1), except from the fact that no rotation of the rotorlinked image is performed, allowing the creation of a steadystate solution. 55.4.5 References Erdos J.I., Alzner E. & McNally W. (1977), Numerical Solution of Periodic Transonic Flow Through a Fan Stage, AIAA Journal, Vol. 15, No. 11, pp. 15591568 Giles M.B. (1990), Stator/Rotor Interaction in a Transonic Turbine, Journal of Propulsion, pp. 621627 He L. (1997), Computational Study of RotatingStall Inception in Axial Compressors, Journal of Propulsion & Power, Vol. 13, No. 1, pp. 3138 Lemeur A. (1992), Calculs 3D stationnaire et instationnaire dans un étage de turbine transonique, AGARD Report CP510 Rai M.M. (1989), ThreeDimensional NavierStokes Simulations of Turbine RotorStator Interaction; Part I  Methodology and Part II  Results, Journal of Propulsion, Vol. 5, No. 3, pp. 305319 Van Leer B. (1985), UpwindDifference Methods for Aerodynamic Flows Governed by the Euler Equation, Lectures in Applied Mathematics, Vol. 23, Part 2, AMS, Providence, pp. 327336 524 FINE™ CHAPTER 6: 61 Throughflow Model Overview The Throughflow module is intended for the design and the analysis of turbomachinery flows. This kind of simulation is based on the twodimensional steady state axisymmetric Euler equations with a specific model for blade rows. It is fully integrated in EURANUS, the threedimensional EulerNavierStokes flow solver. As a consequence: • Options that apply to comparable 3D calculations also apply to throughflow calculations: the physical fluid model, the boundary conditions, the spatial and time discretization, the convergence acceleration techniques and the output, including data for visualization. • The code accepts any number of blade rows. • Throughflow blocks can be combined with 3D blocks in a single computation. • Any improvement introduced in the 3D solver also applies to the througflow blocks. The throughflow simulation should be used only with the perfect gas model currently available through the FINE™ interface. The throughflow simulation can be activated directly from the FINE™ interface by clicking on the Throughflow Blocks thumbnail in the Configuration/Rotating Machinery page. This thumbnail is only accessible when the Mathematical Model is set to Euler on the Flow Model page. In the next section the Throughflow Blocks option in the FINE™ interface is described including all related parameters. Finally, section 65 provides its theoretical background. FINE™ 61 Throughflow Model 62 Throughflow Blocks in the FINE™ Interface Throughflow Blocks in the FINE™ Interface When selecting this thumbnail the page as displayed in Figure 6.2.01 is appearing. Two sections are displayed: Global parameters and Block dependent parameters. The global parameters affect all throughflow blocks, while the block dependent parameters can be tuned independently for each throughflow block. FIGURE 6.2.01Throughflow 62.1 Blocks in Rotating Machinery page Global Parameters The Global parameter for the throughflow method only concern the time discretization of the blade force equation (see section 65.1). The relaxation factor determines the amplitude of the blade force updates and can be interpreted as a CFL number whose value can be different from the one that is adopted for the other equations. The default value is 1. The optimal value usually varies between 0.5 and 5. Higher values result in faster convergence, but can lead to divergence if the stability limit is exceeded. 62.2 Block Dependent Parameters The Block dependent parameters section is subdivided into two areas. The left area is dedicated to the block selection. The right area allows to specify the throughflow parameters for the selected block(s). The Apply to Selection button assigns to the selected block(s) the values of the parameters specified in the right area. One or several blocks may be selected in the left area by simply clicking on them. Clicking on a block unselects the currently selected block(s). Clicking on several blocks while simultaneously pressing the key allows to select a group of blocks. 62.2.1 Block Type: Throughflow or 3D Two toggle buttons are provided to specify the block type: 3D or Throughflow. The 3D choice disables the throughflow method for the selected block(s). This is the default. It is also the required setting for 3D blocks coupled with throughflow blocks in a single computation. Each throughflow block contains exactly one blade row, with a mesh configuration that corresponds to the one prescribed in section 62.3. 62 FINE™ Throughflow Blocks in the FINE™ Interface Throughflow Model Two different types of throughflow blocks are available. The throughflow module is fully active by selecting either the Compressor or Turbine options. The difference between the two lies in the definition of the loss coefficient: for a turbine the pressure used as reference is taken at the trailing edge and for a compressor at the leading edge. 62.2.2 Analysis or Design Mode Two main working modes are available: • Classical Analysis: the blade geometry is known, and the user specifies the relative flow angle distribution along the trailing edge. The leading edge flow angle distribution results from the calculation and the user specifies the type of streamwise distribution to be used between the leading and trailing edges. • Design: the user specifies the relative tangential velocity distribution along the trailing edge, and the throughflow module is used to compute the flow angles and hence to define the blade geometry. The leading edge tangential velocity distribution results from the calculation and the user specifies the type of streamwise distribution to be used between the leading and trailing edges. Two additional analysis modes are provided to the user, more appropriate than the classical one in some cases: • Hybrid Analysis mode: similar to the classical analysis mode, but the user specifies the streamwise distribution of the tangential velocity instead of the flow angle, which has shown to provide more accurate results especially at transonic conditions. • analysis mode with Throat Control: this mode permits to impose the throat section instead of the tangential thickness, which is more appropriate in case of high relative flow angles with respect to the axial direction (high turning turbine blades for instance). In this working mode the user has to specify the flow angle distributions along both leading and trailing edges. In all working modes the user has to specify: • the blockage distribution (tangential thickness of the blades) or the throat section. • the relative flow angle (analysis) or relative tangential velocity (design) at the trailing edge • the value of the loss coefficient along the trailing edge. Depending on the chosen analysis or design mode the appropriate parameters are available under the three thumbnails described in the next paragraphs. 62.2.3 Number of Blades When the block type throughflow is selected, the number of blades needs to be specified for each throughflow block presenting a grid recommended periodicity of 360 (α = 1o), with a mesh configuration that corresponds to the one prescribed in section 62.3. 62.2.4 Blade Geometry When clicking on the Blade geometry thumbnail the parameters as shown in Figure 6.2.22 appear. In the case the analysis mode with Throat Control is selected different parameters will appear as shown in Figure 6.2.23 and described at the end of this paragraph. FINE™ 63 Throughflow Model FIGURE 6.2.22Blade Throughflow Blocks in the FINE™ Interface Geometry Parameters in Design, Classical or Hybrid Analysis mode In all modes except the analysis mode with Throat Control the geometry can be defined by: • 2D input file: the file defining the blade geometry should contain the (Z,R,θcl,θss,θps) coordinates of the blade camber line, suction and pressure sides throughout the meridional domain covered by the blade. For each (Z,R) meridional position the circumferential coordinate θ is given at the camber line, the suction and pressure sides. For the format of a 2D input file see section 63. • 1D input parameters where the user specifies: — the streamwise location of the maximum thickness at hub and shroud (a linear evolution is assumed from hub to shroud), — a file containing the spanwise distribution of maximum tangential thickness, — the normalised streamwise distribution of blade thickness: This distribution can be computed using a power function whose exponent has also to be specified or loaded from a 1D input file with the format as specified in section 63. For most configurations a power function with an exponent of 2 leads to a correct modelling of the blade generating a quadratic thickness evolution. The thickness function is set to zero at the leading and trailing edges and presents a maximum at the prescribed position of maximum thickness. An additional blockage can be introduced to take the endwall boundary layers (Endwall boundary layer and wake blockage factors) into account. The two real parameters refer to the inlet and outlet values of the endwalls blockage. A linear variation is assumed between the inlet and the outlet. 64 FINE™ Throughflow Blocks in the FINE™ Interface FIGURE 6.2.23Blade Throughflow Model geometry parameters in Throat control Analysis mode In case the analysis mode with Throat Control is selected the user specifies the streamwise evolution of the effective blockage, which results from the tangential blockage and the flow angle beff= b cosβ, with b the tangential blockage and β the relative flow angle at the trailing edge. The user specifies: — the streamwise location of the throat at hub and shroud. If a negative value is entered, it is assumed that there is no throat and a linear evolution of the effective blockage from the leading to the trailing edge will be adopted. — a file containing the spanwise distribution of the throat section. The throat is by definition the section in which the effective blockage is minimum. In transonic turbines it determines the mass flow. — the normalised streamwised distribution of effective blockage: This distribution can be computed using a power function whose exponent has also to be specified, or loaded from an input file. The streamwise distribution of effective blockage results from the values specified by the user at the leading and trailing edges and at the throat (if a throat is given). 62.2.5 Flow Angle/Tangential Velocity When clicking on the Flow angle/Tangential velocity thumbnail the parameters related to the direction of the velocity at the trailing edge become available: In Analysis mode the user should always provide the spanwise distribution of the flow angle β at the trailing edge. In Design mode the tangential velocity Wθ (design) at the trailing edge is required instead of the flow angle. A normalized streamwise distribution is also required. It is either read from a file or specified through a power function whose exponent is given by the user. A zero value at the shroud implies that the shroud value is equal to the hub one. The leading edge value being a result of the calcula FINE™ 65 Throughflow Model Throughflow Blocks in the FINE™ Interface tion, the streamwise distribution of the flow angle or of the tangential velocity is iteratively computed according to the calculated value at the leading edge and the value defined at the trailing edge. The default value of the exponent is 1, which generates linear evolutions from leading to trailing edge. Two definitions of the flow angle are available, respectively based on the axial and meridional directions. The choice between these definitions is made through the expert parameter ITHVZM: Wθ=Wz.tan β(ITHVZM=0, default) Wθ=Vm.tan β(ITHVZM=1). In case of radial configurations the parameter ITHVZM should be set to 1. In the case of the analysis mode with throat control one additional input is required: the spanwise distribution of the leading edge flow angle has to be provided in a file. This is required in order to define the value of the effective blockage at the leading edge. 62.2.6 Loss Coefficient When clicking on the Loss coefficient thumbnail the distribution of the loss coefficient can be defined through: • The spanwise distribution along the trailing edge as specified in a file. • The normalized streamwise distribution as imposed through an external file or by using a power function. The value 1 (recommended value) for the exponent of the power function means that a linear function with a shift towards front is used. The leading edge value of the loss coefficient is assumed to be 0. 62.3 Mesh for Throughflow Blocks Figure 6.2.34 shows a configuration with two blade rows. Each throughflow block contains a single blade row. The mesh has only one cell in the pitchwise direction. The cell opening angle, α in Figure 6.2.34, has no influence theoretically but excessive values should be avoided (α > 10o or α < 0.01o). A value of 1o is recommended. All blocks, must have the same cell opening angle. The mesh indices I, J, and K are oriented as shown in Figure 6.2.34. The hub and shroud surfaces correspond to the I=1 and I=Imax grid surfaces respectively, whereas the I=Cst grid surfaces correspond to the successive streamwise positions. Rotors are computed in the relative frame of reference. The leading trailing edges positions are described by spanwise mesh lines (I=Cst). The blade region is identified through the patchdecomposition of the periodic faces (See section 62.4.1). If multigrid is to be used, the inlet region, blade row, and outlet region must each have a suitable number of cells in the IJdirections. Please note that according to Figure 6.2.34 the K=1 surface must be defined along the (Y=0) plane. 66 FINE™ Throughflow Blocks in the FINE™ Interface Throughflow Model FIGURE 6.2.34 The 62.4 throughflow mesh Boundary Conditions for Throughflow Blocks Compared with 3D turbomachine cases, throughflow calculations require the same boundary conditions. All the necessary boundary conditions can be set through the general dialog box Patch Selector through the menu Grid/Boundary Conditions... in IGG™. Table 61 lists the four types of boundaries and the pertaining boundary conditions. TABLE 61 Boundary Conditions Type of Boundary Boundary condition number Periodic Boundaries (Kfaces) BC 2 Hub and Shroud Walls (Ifaces) BC 16, BC 17 Inlets and Exits (Jfaces) BC 124, BC 125, BC 27, BC 23, BC 22 Connecting Boundaries (Jfaces) BC 1, BC 44 62.4.1 Periodic Boundaries The axisymmetric periodic boundaries require a rotational periodicity condition. Except for the patch decomposition, they are set exactly as periodic boundaries of a 3D or axisymmetric nonthroughflow block. As described in section 62.3 the block is composed of an inlet region, a blade passage, and an outlet region. Instead of specifying one boundary condition for the entire Kface, the latter must be artificially divided in three boundary patches, labelled P1, P2, and P3 in Figure 6.2.34 and designating respectively the inlet, the blade, and the outlet region. Both patches P1 and P3 must have at least one cell in the Jdirection. The decomposition needs to be performed in IGG™. • The block is composed by the blade passage only. One boundary patch covers the entire Kface, leading and trailing edge coincide with respectively inlet and exit of the domain. FINE™ 67 Throughflow Model Throughflow Blocks in the FINE™ Interface 62.4.2 Hub and Shroud Walls The present throughflow model assumes an inviscid fluid. Euler wall boundary conditions have to be applied to the hub and to the shroud walls (Ifaces). 62.4.3 Inlet and Exit All rotor inlet and outlet boundary conditions as described in Chapter 8 can be applied at inlet and outlet (Jfaces). 62.4.4 Connecting Boundaries Under the framework of throughflow calculations, rotor/stator interfaces are replaced by simple connections between the throughflow blocks. Connection between throughflow blocks must be matching. Throughflow blocks can also be connected to 3D blocks. This implies the use of a quasisteady interface (rotorstator interface). 62.5 Initial Solution for Throughflow Blocks Especially for the throughflow module the initial flow solution has an important influence on the speed and robustness of the resolution algorithm. Exactly as in FINE™/Turbo for 3D applications, a turbomachineryoriented initial solution algorithm has been implemented, generating automatically an initial solution based on the inlet/outlet boundary conditions and on a userspecified value for the inlet static pressure. The initial solution constructed with this algorithm respects the basic laws of rothalpy and mass conservations. In order to activate this algorithm, the user should select on the Initial Solution page the for turbomachinery option. The user then has to enter a value for the inlet static pressure and a radius if radial equilibrium is selected. The rotor/stator interfaces do not appear in the Initial Solution page because they are identified as simple connections. The static pressure level at the successive rotor/stator interfaces can however be specified through the expert parameter PRSCON. The values to be entered are p1, R1, p2, R2,...,pi,Ri, where i is the index of the rotor/stator interface, p the static pressure in Pascal [Pa] and R the radius in meters [m]. If the expert parameter is not modified by the user, a linear pressure evolution is assumed from inlet to outlet. 62.6 In order to impose a constant pressure at the rotor/stator interface, the corresponding radius has to be set at zero. Output for Throughflow Blocks The output for throughflow simulations can be selected on the Output/Computed Variables page under the Throughflow thumbnail. The following quantities can be stored: • Blockage: tangential blockage factor b = ⎛⎝ 1 – d⎞⎠ , s ∇b  vector, • Grad(B)/B1st component: radial component of the b 68 FINE™ File Formats for Throughflow Blocks Throughflow Model ∇b  vector, • Grad(B)/B3rd component: axial component of the b • Lean vector (tangential vector along the blade in the spanwise direction), • Shape function for β = atan ( W θ ⁄ Wm ) or Wθ , • Loss coefficient ψ , • Blade force vector fB , • Friction force vector f F , • Unit stream vector (USV), · • Flow angle atan ( W θ ⁄ ( Wm ⋅ USV ) ) , • Effective streamtube thickness, • Blade force magnitude: magnitude of blade force f B , • Friction force magnitude: magnitude of friction force f F , • W_theta target: target relative tangential velocity Wtθarg et , • Beta target: target relative flow angle β t arg et = atan ( Wtθarg et ⁄ W m ) . 63 File Formats for Throughflow Blocks The names of all throughflow input files are specified by the user in the above described interactive windows (Figure 6.2.22). The aim of this section is to present the structure of these files. A short description of a specific throughflow output file generated by the interface is also provided. One can distinguish two types of files: the twodimensional and the onedimensional files. The file format for each is described in the next paragraphs. 63.1 Onedimensional Throughflow Input File The onedimensional files consist of two parts: 1. A header line containing four integer (the number of data points and 3 integer switches). 2. The data, organised in 2 columns. The 4 integers contained in the header line define: — the number of data points. — the type of coordinate along which the data is given. The available coordinates are the Xcoordinate (1), the Zcoordinate (3), the radius (4) and the meridional coordinate (6). — if the coordinate should be normalized (1) or not (0). The normalized data describes a distribution between the leading and the trailing edge, or between the hub and the shroud. FINE™ 69 Throughflow Model File Formats for Throughflow Blocks — if for a streamwise distribution, the leading and/or trailing edge values should be extended to the upstream/downstream ends of the block. Values of 1 and 3 extend the upstream region, whereas values of 2 and 4 extend the downstream regions. This switch is used to achieve a blockage factor below 1. upstream and/or downstream of the blade passages. The angles are in degrees, the length in meters, except for the blade thickness, which is in millimetres. Some examples of the geometrical files are given hereafter: • Spanwise distribution of the maximum blade thickness: 14 4 1 0 .1181262 .1282913 .138422 .1484767 .1583352 .1680261 .1778827 .1877939 .197697 .2076666 .217709 .2277728 .2378241 .2477884 8.20958 8.22191 8.16546 8.03777 7.85892 7.58743 7.26814 6.86779 6.45259 6.11613 5.78311 5.65696 5.84635 6.27821 • Spanwise distribution of the trailing edge flow angle: 11 4 1 0 .0 .1060092 .2095564 .3126917 .4146 .5148696 .6134925 .7112999 .8084939 .9048644 1.0 10.10562 5.70642 16.2939 27.0153 35.7384 41.7166 46.4628 50.3735 54.3548 57.9392 59.542 • Spanwise distribution of trailing edge loss coefficient: 11 4 1 0 1.0 .9048644 .8084939 .7112999 .6134925 .5148696 .4146 .3126917 .2095564 .1060092 .0 610 3.78416E02 3.78416E02 3.28353E02 3.74248E02 1.96157E02 3.18909E02 3.61507E02 3.23982E02 5.45700E02 9.97951E02 9.97951E02 FINE™ File Formats for Throughflow Blocks 63.2 Throughflow Model Twodimensional Throughflow Input File The twodimensional input file, only available for the blade geometry definition, consists of two parts: 1. A header line containing the number of points in the two dimensions of the structured data surface and three switches. 2. The data organised in 5 columns (the coordinates should be R,Z,θcl,θss,θps where θcl,θss,θps are respectively the angle at the camber line, suction side and pressure side of the blade) and evolves from hub to shroud and from the leading to the trailing edge. The three additional switches define: — the type of coordinates: should be 4. — the type of structure: should be 3. — the number of variables: should be 5. All lengths in the data files should be in meters, and the angles in radians. Following is an example of the twodimensional input file: 57435 9.37745E02 .1934945 ... 63.3 **(5*7 points: 5 points in spanwise and 7 points in streamwise)** 8.87817E03 6.47041E02 7.40556E02 5.53526E02 8.93166E03 5.71797E02 5.99261E02 5.44332E02 Output File Absolute (V) and Relative (W) velocities components along R,T,M ALPHA = arctg(VT/VZ) BETA = arctg(WT/VZ) GAMMA = arctg(VR/VZ) Mach Number Meridional Mach Number Static Pressure, Static Temperature, Density Absolute Total Pressure Rothalpy Total Pressure Relative Total Pressure Absolute Total Temperature Rothalpy Total Temperature Relative Total Temperature Isentropic Efficiency Polytropic Efficiency Mass Flow Total Area FIGURE 6.3.35 FINE™ Throughflow Output File ".gtf" 611 Throughflow Model Expert Parameters Related to Throughflow Blocks In addition of files which can be read by CFView™, a summary file is created when the throughflow module is activated. It has the extension ".gtf" and gives the average inlet and outlet results for each block in SI units. 64 Expert Parameters Related to Throughflow Blocks 64.1 Underrelaxation Process Two types of underrelaxations have been introduced, allowing for an increased robustness of the algorithm during the initiation of the resolution procedure. This underrelaxation process is controlled through 2 sets of expert parameters (accessed on the Computation steering/Control variables page in expert mode), THNINI (2 integer parameters) and THFREL (2 real  float parameters). • the first THNINI and THFREL parameters permit to impose that during the first THNINI(1) iterations, the blade force update factor is not the one specified in the "Throughflow blocks" menu (section 62.1), but a (lower) value given by THFREL(1). This underrelaxation process can be important for transonic cases especially. The default values for THNINI and THFREL are respectively 10 and 0.1 • the second THNINI and THFREL parameters permit to underrelax the imposed value of trailing edge velocity or flow angle during the first THNINI(2) iterations. The underrelaxation factor multiplying by the imposed value varies linearly between THFREL(1) and 1.0 during the first THNINI(2) iterations. The default values for THNINI and THFREL are respectively 10 and 0.85. 64.2 Others. • ITHVZM = 0 (default): Wθ=Wz.tan β = 1: Wθ=Vm.tan β Definition of the flow angle. The selection of ITHVZM to 1 is crucial for a correct treatment of radial machines. • PRCON to define the pressure for the initial solution at rotor/stator interfaces. If this parameter is not modified a linear pressure distribution from inlet to outlet is assumed. 612 FINE™ Theoretical Background on Throughflow Method Throughflow Model 65 Theoretical Background on Throughflow Method 65.1 The Time Dependent Approach The dominant aspect of an Euler throughflow method is the modelling of the turning and the associated distributed blade force. Most authors so far have adopted a spatial discretization approach, in which the blade force is determined from the tangential projection of the momentum equation in conjunction with the imposed flow direction (analysis) or swirl (design), leaving four differential equations to be solved. In the present approach the blade force is treated as an additional time dependent unknown. The full 5equations Euler system is then solved, with an additional equation for the blade force. This is the socalled time dependent approach, which has proven to be more robust than the space discretization, especially at transonic and supersonic flow conditions. The other advantage is that the fact that the throughflow solver is based on the same time marching algorithm as the 3D one makes hybrid 3Dthroughflow calculations possible. 65.2 Basic Equations and Assumptions The basic equations describing axisymmetric throughflow are obtained through averaging in the θdirection of the threedimensional Euler conservation laws for mass, momentum, and energy, yielding, in concise notation and after introduction of the distributed loss model, ρ 0 bρW ∂ 1 +  ∇ ⋅ b ( ρW ⊗ W + pI ) ∂t ρW b ρE bρWH = ∇b ρQ + p  + ρ ( f B + f F ) b ρQ (61) This is a system of 5 PDE for 5 unknowns (the dependent variables, e.g., the primitive variables in cylindrical coordinates, ρ, Wr, Wθ, Wz, p) in two spatial dimensions (r and z). Apart from the absence in the differential operators of derivatives with respect to the tangential direction, the system differs from the threedimensional Euler equations in three ways: • The presence of the blockage factor b in the fluxes. ∇b  and fB representing the inviscid action of the blades. • Source terms p b • A source term f F grouping all the effects of viscosity and heat conduction. The system is solved in Cartesian coordinates using explicit RungeKutta integration in time and either central or upwind spatial discretization. 65.3 The Tangential Blockage Factor The tangential blockage factor, b, also called the stream tube thickness parameter, represents the contraction of the flow path that arises from the tangential thickness of the blades, d. With the pitch, s, depending on the radius, r, and the number of blades, z, the tangential blockage factor is defined as: FINE™ 613 Throughflow Model Theoretical Background on Throughflow Method d b = 1 – s where 2πr s = z (62) Thus, b = 1 outside blade rows and 0 < b ≤ 1 inside blade rows (including the hypothetical case of blades with zero thickness). The blockage factor is an external input to the computation. 65.4 The Blade Force By definition, the inviscid action of the blades consists in a distributed force normal to the blade surfaces, i.e., suction and pressure surface. In our implementation the blade force is split into two components: • the first main component is proportional to the suctiontopressure side difference, and is oriented in the direction normal to the mean camber surface. The tangential component of this force is the additional unknown considered in the time dependent approach, for which an additional equation will be solved together with the 5 Euler equations. • the second component is due to the deviation of the suction and pressure side normals from the ∇b b normal to the mean camber surface. It is computed according to p  , and is therefore determined entirely by the tangential blockage factor, b, which is external input as seen in the preceding section, and by the static pressure, which is a result of the computation. As mentioned in section 65.2, the blade force is treated as an additional unknown with the present approach. Starting from some initial value in each cell, the blade force is modified locally, until the current converged solution exactly matches the externally imposed target, for instance the flow angle β (analysis) or the tangential velocity Wθ (design). The correction is proportional to the difference between the actual and a required tangential velocity: ( ρF Bθ ) k+1 k t = ( ρF Bθ ) + κ ( W θ – W θ ) (63) where the constant κ is user input. The target tangential velocity Wθt is either direct external input (design mode) or locally calculated from the prescribed relative flow angle β and the current meridional velocity (analysis mode: Wθ=Vmtanβ). The vector of the blade force, fB , is perpendicular to the mean camber surface, which is internally defined by the flow angle and the lean angle. Currently, a zero lean angle is assumed. Robust analysis mode In the case of the analysis mode another formulation of the above equation is adopted, based on the magnitude of the blade force instead of its tangential component: ( ρFB ) k+1 ·· k F˜ = ( ρF B ) – κ ⎛⎝ W n⎞⎠ ˜ W (64) where FB is the magnitude of the blade force and n is the normal vector whose direction results from the imposed relative flow angle distribution. In case the angle is measured with respect to the axial direction (ITHVZM=0): n r = 0.0 614 n θ = – sin β n z = cos β (65) FINE™ Theoretical Background on Throughflow Method Throughflow Model 65.4.1 The Friction Force The distributed loss model retains, from all the effects of heat conduction and viscous stresses, the contribution to the entropy production. The dissipative action of the viscous stresses is expressed through a distributed friction force, f F . It acts in the direction opposite to the velocity vector and for a perfect gas its amplitude is proportional to the loss coefficient derivative in the streamwise direction: p W ρf F = –  p ref ∂ m ψ pt rot W (66) This formulation ensures that a loss coefficient of zero will give exactly a zero friction force. The imposed loss coefficient is defined as: LE ptrot – ptrot ψ = p ref (67) where ptrot is the total pressure associated with rothalpy defined as: γ Tt rot γ – 1 ptrot = p ⎛ ⎞ ⎝ T ⎠ where 2 2 W – ( ωr ) Tt rot = T + 2c p (68) where W is the relative velocity magnitude and pref is a reference dynamic pressure taken at the leading edge (for compressors) or trailing edge (for turbines) on each streamwise mesh line. FINE™ 615 Throughflow Model 616 Theoretical Background on Throughflow Method FINE™ CHAPTER 7: 71 Optional Models Overview FINE™ contains the following three optional models: • FluidParticle Interaction to model solid particles in the flow. • Conjugate Heat Transfer to model the heat transfer between the fluid and solid walls. • Cooling/Bleed to model cooling holes or bleed. • Transition Model to model the flow transition. Each of these models requires a special license feature. If the model is not accessible due to a missing license it is displayed in gray under Optional Models. Contact NUMECA sales or support team for more information about the possibility to obtain a license. 72 FluidParticle Interaction 72.1 Introduction Particleladen flows cover a large class of twophase flows, such as droplets or solid particles in a gas or liquid flow, or bubbles in liquids. One phase is assumed to be continuous and occupies the majority of the flow. It is called the "carrier" phase. Another phase, whose volume fraction is relatively small (usually less than 102), exists as a number of separate elements or particles. It is called the "dispersed" phase. 72.1.1 Lagrangian Approach A Lagrangian approach is used here, whereby the trajectories of individual groups of particles are calculated as transported by the velocity field of the carrier phase, including the effect of drag and other forces. The calculations of the carrier flow and of the particles can be fully coupled, the fully coupling approach implying that the calculation of the particles trajectories is followed by a second flow calculation, taking into account the presence of the particles in the flow (the interphase forces are introduced as source terms in the flow calculation). The sequence consisting of a flow calcula FINE™ 71 Optional Models FluidParticle Interaction tion and of the particle traces tracking can be repeated several times until no changes are observed in the results (usually 3 to 10 times). In the present Lagrangian model, the motion of the particles is only influenced by their own inertia and by the flow, i.e. the local aerodynamic or hydrodynamic forces. Interactions between the particles are currently not considered. This implies the hypothesis of a dilute flow. On the contrary in a dense flow, particle motion is governed by their direct interaction, which implies more complex models, such as the Eulerian ones, in which both phases are modelled as continuous phases. Particleladen flows are found in many industrial applications such as cyclone separators, pneumatic transport of powder, droplet and coal combustion system, spray drying and cooling or sandblasting. In all cases, the flow consists of a continuous phase  also named carrier flow  and a dispersed phase in the form of solid particles, liquid droplets or gas bubbles. In general, the motions of the carrier flow and of the dispersed phase are interdependent. In the lagrangian approach, the physical particle cloud is represented by a finite number of computational particles. The continuous phase (fluid) is treated as a continuum using a boundarycontrolled method whereas the dispersed phase (particles) is treated as a number of separate particles. The particles are successively tracked as a single probe particle through the flow field using a Lagrangian formulation. In the case of laminar flows, each particle will follow a unique deterministic trajectory. In the case of turbulent flows however, particles will have their own random path due to interactions with the fluctuating turbulent velocity field. This feature is taken into account in EURANUS through a stochastic treatment. This approach consists of employing a sampling technique based on a Gaussian probability density function to introduce the random nature of the turbulent velocity field. The particle diffusion due to turbulence can therefore be modelled without introducing artificial diffusion properties of the cloud. According to the distribution and contents of the particles, an averaging procedure provides phase coupling source terms to be added into the Eulerian carrier phase conservation equations. The twoway coupling can be achieved through global iterations. 72.1.2 The Algorithm The hypothesis of a dilute mixture permits to have a very simple sequential calculation of the trajectories of the different particles injected through the inlet sections. The algorithm considers successively the different inlet patches. The user specifies the number of trajectories per cell. The origins can be located at a given point chosen by the user, or equally distributed throughout the cell. The algorithm proceeds cell by cell, the time step being calculated so that several time steps are performed in each mesh cell. The procedure starts at a cell of an inlet boundary and stops when a boundary is reached. Each time step consists of: • the calculation of the force on the particle. • the integration to find the new velocity and position. • the determination of the cell in which the particle is located. 72.1.3 Overview In this chapter an overview is given of the fluid particle interaction module incorporated in NUMECA’s FINE™ environment: 72 FINE™ FluidParticle Interaction Optional Models • section 72.2 describes the main functionalities of the module and the way to proceed in the FINE™ interface. • section 72.3 gives the format of the files associated with the module. • section 72.6 summarizes the main theoretical features of the Lagrangian model. 72.2 FluidParticle Interaction in the FINE™ Interface To access the parameters related to FluidParticle Interaction select the corresponding page under the Optional Models. In the parameters section click on Fluidparticle calculation to activate this model (see Figure 7.2.21). The user enters not only the main features of the numerical simulations but also the characteristics (i.e. processes to be taken into account) of the interphase force between the fluid and the particles. The top window allows to choose the degree of influence of the particles on the flow. The calculation of the carrier flow and of the particles can be fully (2way) or weakly (1way) coupled: • in the 1way coupling approach the flow calculation (ignoring the influence of the particles on the flow field) is followed by a calculation of the trajectories of particles. In this case, there is no influence of the particles on the flow. • in the 2way coupling approach the calculation of the trajectories of particles is followed by a second flow calculation, taking into account the presence of the particles in the flow (the interphase forces are introduced as source terms in the flow calculation). The sequence can be repeated several times (by entering the Number of global iterations) until no changes are observed in the results (usually 3 to 10 times). Concerning the simulation itself, the user can choose the Global Strategy: • Start from scratch: to start the flow calculations and then pursue with the particle tracking simulation. In this particular case, the criterion for the carrier flow calculations convergence is the one set on the Control variables page (6 by default). • Start from converged flow solution: to proceed directly with the Lagrangian coupling from a previous converged flow calculation. FIGURE 7.2.21 Parameters page of the lagrangian fluidparticle interaction model. The usual way to proceed is: FINE™ 1. perform a pure flow study without activating the FluidParticle Interaction model in a computation. 2. while this computation is active in the list of Computations on the top left of the interface create a new project by clicking on the New button. 73 Optional Models 3. FluidParticle Interaction in this new computation activate the Lagrangian Fluidparticle calculation and perform a computation with Lagrangian coupling.The particles encounter several forces: the friction force, i.e. the resultant of the pressure and viscous stress in the carrier phase over the particle surface, as well as potential inertia and gravity forces. The user is free to introduce the gravity force through the vectorial components of the acceleration of gravity on the Flow Model page. An inertial force due to the rotation of the system of reference can also be included. If some of the blocks are rotating this button should systematically be activated. In this case the reference rotation velocity is the one specified on the Rotating Machinery page. 72.2.1 The Boundary Conditions All boundary conditions available for the carrier flow solver are also accepted by the particle tracking algorithm. The only boundary conditions requiring user’s input are: • inlet boundary • solid boundary The boundary conditions are imposed by selecting a patch on which to fix the condition. The user has to confirm the entered values by clicking on the Apply to selection button (Figure 7.2.22). In the list of patches it is not possible to group patches but multiple patches can be selected at the same time to apply the same boundary conditions to all of them. To select multiple patches hold the key while selecting them. a) Inlet Boundary The user can enter a number of classes of particles, each class representing a different type of particles. For each class the inlet boundary conditions have to be specified. The displayed boundary conditions are the one for the class specified in the bar as indicated (a) in Figure 7.2.22. To select another class use the scroll buttons on both sides of this bar. The purpose of this is to be able to simulate the presence of different types of particles in the same patch. (a) FIGURE 7.2.22 Inlet 74 boundary conditions for the fluidparticle interaction model FINE™ FluidParticle Interaction Optional Models Note however that multiple classes are of interest for fully couples calculations only, by allowing the flow calculation to account for the presence of different particle types. In the case of a weak coupling strategy it is recommended to create one computation per particle class, because only one particle class can be visualized in CFView™. The Expert parameter (in Expert Mode on the Control Variables page) CLASID permits to specify which particle class must be included in the CFView™ output. The inlet boundary conditions are the following: • spatial distribution of the injection points: uniform over the chosen patch or located at a chosen point of coordinates (x,y,z). • inlet velocity of the particles (absolute or relative frame of reference). The velocity is always considered in the same relative frame of reference as the one of the block in which the inlet particle is located. The relative velocities here defined as the difference between the particle and the flow velocity (a zero relative velocity is therefore very commonly used) whereas the absolute velocity boundary conditions is used when the velocity of the particle is well known and different from the velocity of the flow. Note that only the Cartesian coordinate system is available. • density and mean diameter of the particles. • particle concentration (number of particles/m3). • number of particles per cell should be seen as the number of trajectories per cell. The use of multiple trajectories per cell permits to ensure a more uniform covering of the inlet (and hence of the computational domain) by the particles. This is only of interest in the case of fully coupled calculations where it is important to ensure that the source terms are correctly evaluated in all mesh cells. The use of multiple trajectories does not modify the number of particles entering the domain. Each trajectory must be seen as an ensemble of particles. It is also very often referred to as a computational particle. In the case of full coupling, the number of particles per cell should be statistically large enough to provide accurate averaging of the dispersed phase parameters. Therefore it is recommended in this case to have a high number of particles per cell. This increases the computational time required for the particle tracking process, but gives rise to a smoother distribution of the particles in the domain. In the case of a weak (1way) coupling, only one particle per cell is usually enough to provide a sufficiently detailed description of the particles distribution in the field. b) Solid Wall Boundary Condition The solid wall boundary condition requires an additional input data, which is the reflection ratio. If the ratio is zero, all the particles remain stuck on the wall, whereas if it is 1.0, all particles are reflected, without any loss of mass or energy. The user can choose the reflection ratio by clicking on the corresponding button while moving the mouse (Figure 7.2.23). Two reflection modes are available and can be selected by the expert parameter IBOUND: • In the default mode (IBOUND = 1) the particle loses a fraction of its mass and hence of its kinetic energy at each wall hit. After several wall hits, the size of the particles becomes very small, and the tracking stops (once the diameter has reached a given ratio of the initial one, specified by the expert parameter DIAMR). • In the other mode (IBOUND = 2) the velocity of the particle is reduced, with an unchanged mass. The particle is stopped as soon as the velocity becomes too small (also specified by the parameter DIAMR). FINE™ 75 Optional Models FluidParticle Interaction FIGURE 7.2.23 Solid 72.3 boundary conditions for the fluidparticle interaction model Outputs The following quantities are calculated by the solver (see Figure 7.2.34): • the number concentration of volume Ω, ⎛ ⎜ ⎝ • the mass concentration ρ ipart ⎛ ⎜ ⎝ ⎞ ∑ Ni⎟⎠ ⁄ Ω where Ni is the number of particles of class i in the cell i ⎞ ∑ ρipart Ni Ωipart⎟⎠ ⁄ Ω (mass of particles per cell volume) where i is the density of the particle of class i and volume Ω ipart , ⎛ ⎞ • the volumetric concentration ⎜ ∑ Ni Ωipart⎟ ⁄ Ω (volume of particles per cell volume), ⎝ • the Vx = components ⎛ ⎜ ⎝ ∑ i of ⎞ V xi ρ ipart Ω ipart N i⎟ ⎠ i the ⎠ mass weighted absolute velocity vector ⁄ ∑ ρ ipart Ω ipart N i , i • the weighted mass and weighted absolute or relative velocity vectors number, • the components of the interphase force F = ⎛ ⎜ ⎝ ⎞ ∑ Fi Ni⎟⎠ ⁄ Ω . i The solver automatically writes an output file containing the particle traces that is read by the CFView™ post processing software. 76 FINE™ FluidParticle Interaction Optional Models FIGURE 7.2.34 Outputs 72.4 of the fluidparticle interaction model Specific Output of the FluidParticle Interaction Model This section describes the specific outputs generated by the Lagrangian module. 72.4.1 Field Quantities The solver automatically includes in the CFView™ output (’.cgns’) of the project the field quantities that have been specified by the user under the Outputs thumbnail in the FluidParticle Interaction page. These quantities can be scalars or vectors, and are the following: • Vectors Massweighted relative velocity (1) Numberweighted relative velocity (2) Massweighted absolute velocity (3) Numberweighted absolute velocity (4) Interphase force vector (5) • Scalars Number concentration (51) Mass of particles per cell volume (52) Volume of particles per cell volume (53) Presence (1) or absence (0) of particles in cells (54) Vx: xcomponent of massweighted velocity vector (55) Vy: ycomponent of massweighted velocity vector (56) Vz: zcomponent of massweighted velocity vector (57) Fx: xcomponent of interphase force (58) Fy: ycomponent of interphase force (59) Fz: zcomponent of interphase force (60) 72.4.2 Particles Traces (’.tr’) The solver also creates an specific lagrangian output file (’.tr’), containing the trajectories of the all the particles. This file is automatically transmitted to CFView™, which allows for the visualization of the trajectories. FINE™ 77 Optional Models FluidParticle Interaction 72.4.3 Summary File (’.tr.sum’) In addition to the previous outputs, a summary file ’.tr.sum’ is automatically written by the solver (in the same directory as the CFView™ project), giving for each injection patch the particles numbers and mass flows through the inlet/outlet boundaries, and the number of particles that remain stuck on the walls. 72.5 Expert Parameters for FluidParticle Interaction Other parameters appear in the Expert Mode of the FluidParticle Interaction page under the Parameters thumbnail: • The maximum residence time (TMAX in corresponding ’.run’ file), which is the time limitation for particle residence in the flow. It may be used either to prevent particle stopping or to avoid an infinite loop, having for instance a particle captured in a separation bubble. After the time has expired, the particle disappears. • The governing equations for particles in a carrier flow consist of a set of nonlinear ordinary equations. Two methods are provided to integrate this equations with respect to time (that can be selected in expert mode): — The RungeKutta scheme, in which the transfer to the next time level is fulfilled through a finite number of intermediate steps. A twostage and a fourstage option (NRKS in corresponding ’.run’ file) are available. This scheme is limited to big particles. — The exponential scheme that lies on a semianalytical method. This scheme is particularly suitable for small particles. • The Drag force is in general the only considered part of the interphase force. It corresponds to the force on a particle moving in a still fluid at constant velocity (or using the particle reference system, a fixed particle in a uniform laminar flow). At extremely low Reynolds numbers (Rep << 1 i.e. at low relative velocities), it is expressed through the Stokes formula. For higher Reynolds numbers, an optional standard curve fit may be chosen (section 72.6.1). The choice between the two types of forces can be made in expert mode. Other parameters have a standard value, which may be modified only on rare occasions. They are accessible in the Expert Mode of the Computation Steering/Control Variables page: CLASID: selection of class for CFView™ output LMAX: the maximum number of segments along a trajectory may be used to avoid an infinite loop in the case of an oscillatory movement for instance. DDIMAX: tolerance factor to establish that a particle has left a cell (default=1.E4). I2DLAG: simplification for 2D problems (0 if 3D, 1 if 2D). DIAMR: diameter ratio under which the particle tracking process stops (default value: 0.1). CELT: coefficient for eddy life time (for turbulent flows only): 0.28. KOUTPT: enables to write the ASCII ’.tr.out’ file containing the output of the trajectories (default value: 0). Contact support at support@numeca.be to have more details on this file. 78 FINE™ FluidParticle Interaction 72.6 Optional Models Theory In a Lagrangian approach the particle cloud is modelled by a finite number of computational particles, representing a group of real physical particles with similar properties. The particles are tracked separately, each as a single probe particle, through the flow field. 72.6.1 Calculation of the Trajectories  Integration Method The calculation of the trajectories is based on the Newton law: ∆V F = ma = m ∆t (71) where a is the acceleration vector of the particle of velocity V and F is the sum of the friction force between the fluid and the particle and the eventual inertia and gravity forces: F = Fd + F inertia + Fgravity (72) The gravity force is defined by the user on the Flow Model page: Fgravity = mg It is assumed that the mesh blocks for which a rotation of the reference system is introduced in the carrier flow equations (when rotation of the reference system is selected under the Parameters thumbnail of the FluidParticle interaction page) are also considered as rotating ones for the particles calculation. The inertia force due to the rotation of the reference system contains the two terms related to the inertia and Coriolis effects: F inertia = – m [ ω × ( ω × r ) + 2ω × V ] (73) Fd is the drag force between the flow and the particles, calculated according to the Stokes law: D Fd = –  ( V – U ) Fs (74) where D is the diameter of the particles, U is the velocity of the fluid and Fs depends on the viscosity of the fluid and on the Reynolds number Re p based on D: F s = 1 ⁄ ( 3πµC ) (75) where: ρ ( V – U )D C = 1 (simple Stokes law for Re p ≡  « 1 ) µ or 0.5 C = 1 + 0.179Re p + 0.013Re p (standard curve approximation). Up to now, no model is incorporated in which the mass and the volume of the particle would change (for instance by combustion or evaporation). FINE™ 79 Optional Models FluidParticle Interaction 72.6.2 Integration Time Step  Relaxation Time The calculation of the trajectories is obtained by integrating the Newton law in time, using either a 2 or 4steps RungeKutta or an exponential scheme. At each time step the force vector is recalculated to obtain a new value for the velocity vector, whereas the velocity vector is used to calculate the new position of the particle. This sequence is repeated until a boundary is reached. In order to have an appropriate integration method to calculate the trajectories, the integration time step must be properly chosen. The time step used by the algorithm is the minimum between the time required to traverse the mesh cell (which depends on the particle velocity and on the cell size) and the relaxation time, which is the time required by the particle to lose its initial slip velocity: 2 τ drag = ( ρD ) ⁄ ( 18µC ) (76) For a stationary reference system (no inertia force) and in the case of no gravity, the relaxation time is the time required by the particle to reach the flow velocity U, whereas in the presence of an inertia and/or a gravity force, the velocity reached by the particle after the relaxation time is not U, but U + g . τdrag. In some cases (for instance with very small particles) the relaxation time is very small, which leads to a large number of time steps per mesh cell, and hence to a larger CPU time for the particle tracking algorithm. A faster convergence may then be reached by using the socalled exponential scheme for the time integration step. 72.6.3 Full Coupling Between the Carrier and Particle Flows In case of a full coupling between the carrier and particles flows, the particles traces calculation is followed by a coupled carrier flow calculation including the effect of the presence of the particles. This is achieved by the introduction of source terms in the momentum equations, these source terms being calculated according to the interphase force vector: ∆V F interphase = m  – Finertia – F gravity ∆t (77) 72.6.4 Interaction with Turbulence While moving through a turbulent flow, each particle faces a sequence of random turbulent eddies that result in a lack of accuracy in particle velocity and position. This process is taken into account using a stochastic treatment. The kε turbulence model is assumed for the carrier flow simulation. The instantaneous fluid velocity is represented as the sum of the local mean velocity (available from the computed carrier flow field) and a random fluctuation: U = U + U' (78) The fluctuation U' is randomly sampled from the normal Gaussian distribution with the probabilitydensityfunction f: u' 2 ⎛ u' ⎞ 1 f ( u' ) =  exp ⎜ – ⎟ and ⎝ 2u' 2⎠ 2 2πu' U' = ∫ f ( u' ) du' (79) –∞ The individual components of the velocity fluctuation are assumed to be noncorrelated. The mean square deviation is evaluated from the turbulent kinetic energy: 710 FINE™ Conjugate Heat Transfer Optional Models 2 2 u' =  k 3 (710) It is accepted that this sample velocity fluctuation remains unchanged within the turbulent eddy during its life time. The eddy life time Te and size Le are calculated according to: k Te = C lt ε and Le = Te ⎛⎝ 2 k⎞⎠ 1⁄2 3 (711) Where C lt is an empirical coefficient with a default value of 0.28. The calculated fluctuation gives the instantaneous flow velocity, which is used while tracking the particle. As soon as the life time has expired or the particle has left the eddy, a new fluctuation is chosen as described before, assuming no correlation with the previous sample. 72.7 Note that turbulence is therefore taken into account only for the different linear and non linear kε models. In the particular case of the BaldwinLomax model, turbulence does not have a direct influence on the particles trajectories. References Chang, K. C., Wang, M. R., Wu, W. J., Liu, Y. C., Theoretical and Experimental Study on TwoPhase Structure of Planar Mixing Layer, AIAA Journal, Vol. 31, No 1, pp 6874, 1993. 73 Conjugate Heat Transfer 73.1 Introduction The conjugate heat transfer model allows the simulation of the thermal coupling between a fluid flow and the surrounding solid bodies, i.e. the simultaneous calculation of the flow and of the temperature distribution within the solid bodies. The current version of the model has been validated for steady state applications. It assumes that some of the blocks of the multiblock mesh are "solid", whereas the other ones are "fluid". The connections between the solid and fluid blocks become "thermal connections" along which the fluidsolid coupling is performed. First section 73.2 explains how to set up a project involving the Conjugate Heat Transfer model under the FINE™ user environment. In section 73.3 a theoretical description is provided, presenting the approach used to solve the conduction problem and describing the adopted solidfluid coupling strategy. 73.2 Conjugate Heat Transfer in the FINE™ Interface The Conjugate Heat Transfer model can be directly activated from the FINE™ interface under Optional Models. When opening the Conjugate Heat Transfer page it looks like Figure 7.3.25. All blocks in the mesh are listed on the left of the page and all of them are by default set as "fluid". FINE™ 711 Optional Models Conjugate Heat Transfer FIGURE 7.3.25 Conjugate Heat Transfer page The only action required from the user to set up a computation involving the Conjugate Heat Transfer model can be decomposed in three steps: 1. Determine the Solid and Fluid Blocks. 2. Set the Global Parameters. 3. Define the thermal connections. Those steps are described in the following paragraphs in more detail. 73.2.1 Step 1: Determine the Solid and Fluid Blocks The use of the Conjugate Heat Transfer model requires the generation of a multiblock mesh, the "solid" and "fluid" parts of the domain being discretised with separate blocks. Once the mesh is generated, the first step consists in pointing the "fluid" and the "solid" blocks via the FINE™ user interface. In the default configuration of the solver all blocks are of "fluid" type, so that the Conjugate Heat Transfer page does not need to be entered for a classical flow calculation. The transfer of some of the blocks from "fluid" to "solid" is performed by selecting those blocks on the left part of the window and by pressing the button Solid. For each solid block the thermal conductivity has to be specified (in W/m/K). 73.2.2 Step 2: Setting the Global Parameters The only global parameter is the CFL number used for the time integration of the conduction equation. It can be different from the one used for the fluid. The default value is 1.0. 73.2.3 Step 3: Setting the Thermal Connections Once some blocks of the multiblock mesh are pointed as "solid" blocks, the connections between solid and fluid blocks become "thermal connections". These connections are solid wall boundary conditions with a particular thermal condition, along which the imposed temperature profile is iteratively recalculated in order to ensure a correct coupling. These patches appear in the list of patches under the thumbnail Solid on the Boundary Conditions page. Although the thermal aspect is fully controlled by the coupling procedure, the kinematic boundary condition must be specified by the user (rotation speed). 73.2.4 Type of Connections Between Solid and Fluid Blocks Two types of thermal connections are allowed: • matching connections (one patch on each side), 712 FINE™ Conjugate Heat Transfer Optional Models • full nonmatching connections (one patch or one group of patches on each side). The connection algorithm is implemented in a general way, allowing on both sides a grouping of solid and fluid patches. This is useful for instance in order to facilitate the coupling of a turbine block with holes with the external flow. One single connection can be built, with on the inner side a group of patches including the blade surface and the outer face of the holes. 73.3 Theory This section describes the Conjugated Heat Transfer model implemented within EURANUS: • the technique used to solve the conduction in the solid bodies, • the thermal coupling strategy. 73.3.1 Simulation of Conduction in EURANUS It has been shown in the previous chapters that the EURANUS flow solver is based on a cell centred finite volume approach, associated with a entered or upwind space discretization scheme together with an explicit RungeKutta time integration method. The same type of approach can be used to simulate the conduction in solid bodies. The only term remaining in the finite volume equilibrium results from the heat conduction. The discretised form of the remaining part of the energy equation applied to the control volumes can be written as: ∆T ρC p  Vol = Σ ⎛ k∇T⎞ n∆S ⎝ ⎠ ∆τ (712) where Vol is the volume of the control volume, n∆S is the normal vector to the faces of the control volume and k,ρ and Cp are respectively the conductivity, density and specific heat of the solid body. This equation is applied to calculate the change of temperature T at a given time step resulting from the equilibrium of the conduction fluxes through the faces of the control volume. One can notice that the absence of any advective contribution in the equilibrium permits to avoid the use of artificial dissipation (case of a centred scheme). It also imposes to adopt a pure diffusive approach for the calculation of the time step. For a 2D problem the time step is calculated according to: ρC ∆τ Vol  = p Vol k 2 2 Si + Sj + 2Si·Sj (713) One can notice that once the 2 above equations are put together the heat capacity Cp is eliminated from the equation, and is hence not required as input data. Exactly as for the flow solver the adopted time integration approach is a 4 or 5step RungeKutta scheme whose efficiency is largely enhanced by the use of an implicit residual technique and of a multigrid strategy. This finite volume approach can be used for both steady and unsteady conduction problems. Its efficiency has been compared for steady state applications to the classical GaussSeidel and PSOR schemes often employed for the resolution of pure elliptic equations. The results have shown that the use of a time marching approach together with multigrid is much more efficient. 73.3.2 Thermal Coupling Between the Solid and Fluid Blocks The fluidsolid interfaces constitute a new type of boundary condition, referred to as "thermal FINE™ 713 Optional Models Conjugate Heat Transfer connections", along which the heatflux and temperature are imposed to be equal. The calculation is performed simultaneously on the fluid and solid blocks. The thermal coupling is applied each time the boundary conditions are applied. Note that no particular procedure is required in order to initiate the calculation. The full multigrid strategy is very efficient in order to rapidly establish an overall temperature distribution in the domain. On both solid and fluid sides, the thermal boundary condition imposes a temperature profile. This profile is iteratively recalculated in order to ensure equality of the heatfluxes calculated on both sides: hf(TwTf)=hs(TwTs), (714) where hf and hs are the heat transfer coefficients and Tf and Ts are the inner temperatures. The heat transfer coefficients are calculated in a simple way, assuming a sufficient orthogonality of the mesh: k h =  , ∆y (715) where k is the local conductivity and ∆y is the distance between the inner cell centre (where the temperature of Tf and Ts is taken) and the wall. 73.3.3 Full Nonmatching Thermal Connections The Full Nonmatching algorithm already used for the fluidfluid connections can be used in the Conjugate Heat Transfer (CHT) module. It is based on the same coupling procedure, including the calculation of the interface temperature and heatflux. In case the patches are not fully connected, as for instance in Figure 7.3.36, the remaining patch is assumed to be adiabatic. The thermal coupling equation is applied successively to all elements resulting from the FNMB decomposition algorithm. This procedure gives as a result a separate value of the interface temperature and of the heatflux for all elements. The interface temperature on the left and right patch cells is then calculated as a weighted averaging of the temperatures of the elements concerned by the cell. If the cell is not fully connected an additional contribution is added, the non connected part of the cell being assumed to be adiabatic: i Tw = ∑ i T n w n + T inner W i with elmts ∑ i wn + Wi = 1 . (716) elmts In the generic case of Figure 7.3.25: • the cell 1 is not connected and the above equation is applied with Wi=1, • the cell 2 is partially connected and 0 > to go to the next page of the wizard. On this page, depending of the role, type and mode of injector, the flow parameters and geometry/positioning parameters have to be defined in the second page of the wizard. When defining a cooling or bleed using the Cartesian or cylindrical coordinates no procedure are implemented to check if the specified direction is correct. e) Injection Sector Geometry/Positioning Parameters As presented in Table 71, 11 combinations are available. As the transformation from cylindrical to Cartesian coordinates is obvious, only 8 combinations will be described in more details. e.1) Relative positioning for a single hole The user specifies the diameter of the hole in case of a single hole. 718 Each hole is circular. The diameter of the hole is specified by the user but a hole is included in one cell only even when the diameter exceeds the cell width. FINE™ Cooling/Bleed Optional Models As for the old algorithm, the holes are located by means of a spanwise and a streamwise relative position. The algorithm can be applied to H, I or Omeshes generated by AutoGrid. For Omesh the blade surface is divided in two different subpatches (one for the pressure side and one for the suction side). Therefore, the user has to select on which side of the blade (Side1/Side2) the injection will be located. A button has been added in the interface in order to select the side. This button is active only for Omeshes. FIGURE 7.4.29 Geometry Parameters for relative positioning of a hole Only the version of AutoGrid provided with FINE™ 6.11 (and latter versions) can be used to generate the mesh and this relative positioning is only available for blade surfaces. The location is defined as a fraction of the arc length from hub to shroud and from the leading edge to the trailing edge. Spanwise and streamwise coordinates are computed for each cell vertex. The closest point found in this relative coordinate frame is the one that is concerned by the injection. An option has been setup in order to use the axial chord (Axial Coordinates button) instead of the arc length (only available for axial machines). The relative positioning does not accept meshes with a blunt at the leading edge FIGURE 7.4.210 . Relative positioning of a hole at 70% spanwise and 50% streamwise. Finally, when a cooling injection sector has been selected, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. FINE™ 719 Optional Models Cooling/Bleed When Grid Indices is selected, the injection direction is provided by the user through 2 angles expressed in degrees (depending of the units selected in the menu File/Preferences). Each angle is measured with respect to the local normal and one of the 2 grid line directions tangent to the wall. In case of an I J K = ct surface, the angles are measured with respect to the ( J, K ) ( K, I ) ( I, J ) grid lines respectively. Figure 7.4.211 illustrates the definition of angle βk for an I = cst surface. I=constant surface V J K βk n βk is the angle of the velocity projection in the (K,n) plane with respect to the normal n to the surface. FIGURE 7.4.211 Angle definition in the cooling flow page of the FINE™ interface Each angle is defined as: Vi, j, k β i, j, k = atan ⎛ ⎞ ⎝ V ⎠ n (718) For example, in order to make the velocity direction oriented along the normal, the two angles should be set equal to 0. A 90 degrees angle is not allowed as it will induce a velocity vector tangent to the corresponding grid line direction, with null mass flow. For holes located on the blade walls and when the mesh is generated with Numeca’s AutoGrid software, the K and J lines are the two tangent directions along the blade wall, respectively oriented in the streamwise and spanwise directions. e.2) Relative positioning for a line of holes The user specifies the diameter of the hole in case of a line of holes. Furthermore, the number of holes has to be specified and will be uniformly distributed on the line. Each hole is circular. The diameter of the hole is specified by the user but a hole is included in one cell only even when the diameter exceeds the cell width. As for the old algorithm, the line of holes is defined by two points (holes) that are located by means of a spanwise and a streamwise relative position. The algorithm can be applied to H, I or Omeshes generated by AutoGrid. For Omesh the blade surface is divided in two different subpatches (one for the pressure side and one for the suction side). Therefore, the user has to select on which side of the blade (Side1/Side2) the injection will be located. A button has been added in the interface in order to select the side. This button is active only for Omeshes. 720 FINE™ Cooling/Bleed Optional Models For each point of the line the algorithm works as for the single hole positioning. FIGURE 7.4.212 Geometry Parameters for relative positioning of a line of holes Only the version of AutoGrid provided with FINE™ 6.11 (and latter versions) can be used to generate the mesh and this relative positioning is only available for blade surfaces. The location is defined as a fraction of the arc length from hub to shroud and from the leading edge to the trailing edge. Spanwise and streamwise coordinates are computed for each cell vertex. The closest point found in this relative coordinate frame is the one that is concerned by the injection. An option has been setup in order to use the axial chord (Axial Coordinates button) instead of the arc length (only available for axial machines). The relative positioning does not accept meshes with a blunt at the leading edge Finally, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When Grid Indices is selected, refer to the end of section e.1) for more details. e.3) Cartesian positioning for a single hole The user specifies the diameter of the hole in case of a single hole. Each hole is circular. The diameter of the hole is specified by the user but a hole is included in one cell only even when the diameter exceeds the cell width. As for the old algorithm, the holes are located by means of the (X,Y,Z) Cartesian coordinates. FINE™ For a single hole, the cell that is concerned by the injection is the closest cell face centre to the defined point. In case of repetition, the point is automatically transferred to the meshed patch 721 Optional Models Cooling/Bleed Furthermore, in order to ease the capture of the right coordinates, the button Get Coordinates enables the user to interactively select the point in the mesh view after opening the mesh through the menu Mesh/View On/Off or Mesh/Tearoff graphics (only available on UNIX). FIGURE 7.4.213 Geometry Parameters for space Cartesian positioning of a hole Finally, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When Grid Indices is selected, refer to the end of section e.1) for more details. e.4) Cartesian positioning for a line of holes The user specifies the diameter of the hole in case of a line of holes. Furthermore, the number of holes has to be specified. Each hole is circular. The diameter of the hole is specified by the user but a hole is included in one cell only even when the diameter exceeds the cell width. As for the old algorithm, the line of holes is defined by two points (holes) that are located by means of the (X,Y,Z) Cartesian coordinates. For the two points defining the line, the cells that are concerned by the injection are the closest cell face centre to the defined point. In case of repetition, the point is automatically transferred to the meshed patch FIGURE 7.4.214 Geometry 722 Parameters for space Cartesian positioning of a line of holes FINE™ Cooling/Bleed Optional Models Furthermore, in order to ease the capture of the right coordinates, the button Get Coordinates enables the user to interactively select the point in the mesh view after opening the mesh through the menu Mesh/View On/Off or Mesh/Tearoff graphics (only available on UNIX). A line is drawn from those two points (this line do not necessarily follow the surface of the patch, see Figure 7.4.215). The segment is then uniformly divided into N1 subsegments (where N is the number of holes on this line). Each N2 limits of the subsegment is then projected on the patch (the closest cell face centre is found). Those are the cells where the injection will be applied. They are not necessarily uniformly distributed on the patch. points defined by user points at cell face centre where injection will be applied View from the top FIGURE 7.4.215 Construction View at Constant Radius of a line of holes on a turbine hub For a mesh with an important clustering, or for an important number of points in the line, several projected points could end on the same cell. This is taken into account in the algorithm. The mass flow injected is then multiplied by the relevant factor. Therefore, one should be aware that the number of cells that are highlighted in the interface should not strictly match the number of hole in the line. within Parametric Space without Parametric Space FIGURE 7.4.216 Definition FINE™ of a line of holes without or within the parametric space 723 Optional Models Cooling/Bleed On the contrary for a mesh with a relatively poor spatial discretisation, the location of the cell face centres where the injection will be applied will not be strictly on a line. A limitation of this algorithm is that the line does not necessarily follow the patch surface. Therefore, defining a line of holes at the hub of a gap (upper surface of a rotor blade) could produce the problem presented on the left side of Figure 7.4.216. The same problem can arise generally on a convex surface. In order to solve this problem, it has been decided to allow the user to define a line of holes following a parametric surface defined by the grid lines by activating Parametric Space. Therefore, a line of hole on a convex surface could be more easily defined (right side of Figure 7.4.216). One limitation of this option is that a line of hole cannot cross a connection. For instance defining a line of holes (in the parametric space) close to the trailing edge of a O mesh will produce the result sketched bellow. POSSIBLE FIGURE 7.4.217 Definition of a line of holes in the parametric space. For turbomachinery configuration with periodic conditions, points could be located either on the meshed passage or on one of its repetitions. Therefore, the injections should automatically be transferred to the meshed patch. Two methods are available. FINE™ 6.2 FINE™ 6.1 Meshed Patches Repetition FIGURE 7.4.218 Two 724 Meshed Patches Repetition methods to respect repetition for a line of 3 holes. FINE™ Cooling/Bleed Optional Models • In FINE™ 6.1, the method was transferring only the extremities of the line of holes to the meshed patch. • In FINE™ 6.2, the method is rotating only the final position of the injections in order to be located on the meshed patch. As illustrated in Figure 7.4.218, those two options could lead to rather different results. In case of multipatch selection the algorithm described above is applied independently for each patch. Therefore, a direct definition of a line of hole crossing several patches is not possible. In this case it is recommended to define as many line as necessary (see figure bellow). In order to overcome this problem the multipatch selection has been restricted to the slots defined by Cartesian or cylindrical coordinates. FINE™ 6.2 FINE™ 6.1 FIGURE 7.4.219 Example of definition of a line of 5 holes with multipatch selection. Finally, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When Grid Indices is selected, refer to the end of section e.1) for more details. e.5) Cartesian positioning for a slot The user specifies the width of the slot. has to be specified. The multipatch selection has been restricted to the slots defined by Cartesian or cylindrical coordinates. FIGURE 7.4.220 Geometry FINE™ Parameters for space Cartesian positioning of a slot 725 Optional Models Cooling/Bleed For the positioning of the slot, the radius and z values are asked to the user. The closest cell face of the patch to this point is found. The radius and axial position of this cell face centre become the slot position in the (r,z) plane. It should be noted that this slot position is not identical to the initial user input. For most axial machines the radius can be easily identify by calculating the closest point on the patch. In this case only the axial position of the slot is required in the interface. For radial machines, or for axial machines with complex vein geometry, the two components of the original point are required (Figure 7.4.221). Axial Machine Radial Machine FIGURE 7.4.221 Examples of slot positioning The algorithm that defines the cell faces that are concerned by this slot is the following one. For each cell face of the patch, the two extremities in the (r,z) plane of this polygon (A,B and A’,B’) are identified (i.e., the two vertices with the maximum distance in this plane). They define the limits of the cell face in the (r,z) plane. If those two points are called A,B for cell 1 and A’,B’ for cell 2, and S is the slot location specified by the user in the (r,z) plane through FINE™, as presented on Figure 7.4.222, S is only included in the domain of cell 1 limited by A,B in the (r,z) plane, therefore, the cell 1 is the only cell concerned by the slot S. FIGURE 7.4.222 Identification 726 of the cells concerned by the slot S in the (r,z) plane. δ is the distance between A and B. FINE™ Cooling/Bleed Optional Models On the contrary, S is not inside the domain defined by A',B'. Thus, the cell 2 will not be concerned by the slot. For Omeshes with small cells close to leading or trailing edges, this algorithm could leads to missing cells. This problem is due to a (r,z) position specified by the user in FINE™ for the slot that is not precise enough. not precise enough value exact value points are missing FIGURE 7.4.223 Definition points are represented of a slot for a Omesh Furthermore, in order to ease the capture of the right coordinates, the button Get Coordinates enables the user to interactively select the point in the mesh view after opening the mesh through the menu Mesh/View On/Off or Mesh/Tearoff graphics (only available on UNIX). Finally, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When Grid Indices is selected, refer to the end of section e.1) for more details. e.6) Grid positioning for a single hole The user specifies the diameter of the hole in case of a single hole. Each hole is circular. The diameter of the hole is specified by the user but a hole is included in one cell only even when the diameter exceeds the cell width. The grid positioning used in EURANUS depends on the grid indices of the centre of the cell faces. It is different from the grid indices used in IGG™ and in CFView™. The grid indices are directly used by the flow solver in order to introduce the flow of mass, momentum and energy at this cell face. FINE™ 727 Optional Models Cooling/Bleed FIGURE 7.4.224 Geometry Parameters for Grid positioning of a hole Finally, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When Grid Indices is selected, refer to the end of section e.1) for more details. e.7) Grid positioning for a line of holes The user specifies the diameter of the hole in case of a line of holes. Furthermore, the number of holes has to be specified. Each hole is circular. The diameter of the hole is specified by the user but a hole is included in one cell only even when the diameter exceeds the cell width. From the two cell face centres defined in the interface, two geometrical points are defined by their (x,y,z) coordinates. Then, a line is constructed in the same way as for the Cartesian positioning (section e.4). In this case there is no problem of repetition because the two extremities of the line are located on the meshed patch. Furthermore, concerning the Parametric Space option, refer to section e.4) on page 724 for more details. FIGURE 7.4.225 Geometry Parameters for Grid positioning of a line of holes Finally, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When Grid Indices is selected, refer to the end of section e.1) for more details. 728 FINE™ Cooling/Bleed Optional Models e.8) Grid positioning for a slot The user specifies the width of the slot. has to be specified. From the grid indices a geometrical point is defined. Then the slot is defined in the same way as for the Cartesian positioning (section e.5). FIGURE 7.4.226 Geometry Parameters for Grid positioning of a slot Finally, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When Grid Indices is selected, refer to the end of section e.1) for more details. f) Flow Parameters The user has to specify the Mass flow: the specified mass flow is actually the total mass flow through all the blades and through all the holes in the case of a line of holes. Thus the mass flow through one hole is the specified mass flow divided by the number of blades and the number of holes. The mass flow is often responsible for initialization troubles as it might be too high. The FINE™ interface allows a tuning of the specified mass flow through an expert parameter. This is described in section 74.3. For cooling flow the mass flow specified in FINE™ will be considered as positive and as negative for bleed flow. FIGURE 7.4.227 Flow FIGURE 7.4.228 Flow FINE™ Parameters for Bleed Parameters for Cooling 729 Optional Models Cooling/Bleed Furthermore, the Arrows scaling factor parameter enables the user to control the shape of the arrows representing the injection direction after opening the mesh through the menu Mesh/View On/Off or Mesh/Tearoff graphics (only available on UNIX). For cooling additional parameters have to be defined: • static or total temperature. • turbulent kinetic energy and dissipation or turbulent intensity when the kε model is used. • kinematic turbulent viscosity when the SpalartAllmaras model is used. 74.2.2 Injector Sector Visualization When adding an injection sector into FINE™, the location (cell face are highlighted) and the direction of the injection can be visualized. In order to be able to visualize, the user has to load the mesh through the menu Mesh/View On/Off. FIGURE 7.4.229 Injection Sector Visualization within FINE™ The parameters area will then be overlapped by the graphic window, and the small control button on the upper  left corner of the graphic window can be used to resize the graphics area in order to visualize simultaneously the parameters and the mesh (see section 210). 730 Mesh/Tearoff graphics is only available on UNIX and enables to open the mesh in a new window. FINE™ Cooling/Bleed Optional Models Furthermore, new outputs have been added into FINE™ on the Outputs/Computed Variables page under the thumbnail Solid data in order to enable the visualisation in CFView™ of the injected flow and the injection direction. FIGURE 7.4.230 Injector 74.3 Sector Outputs for CFView™ Expert Parameters a) COOLRT In the old algorithm (COOLFL=0), in case some difficulties appear at the beginning of the simulation, the mass flow can be reduced with the expert parameter COOLRT. The value of COOLRT (less than 1) corresponds to a constant factor applied to the imposed mass flow. This parameter has an influence on the initialization as the specified mass flow is sometimes too large. The user should definitely tune this parameter in case of problems. b) ZMNMX In the old algorithm (COOLFL=0) for the relative mode, the injector position in streamwise direction can be provided with 0 and 1 defined in two different ways: ZMNMX = 0 (default): the leading and trailing edges are the grid edges, i.e the points where the periodic lines of the mesh meet the blade walls = 1: the points located at respectively the minimum and maximum axial positions. c) COOLFL There is a possibility to specify the cooling/bleed flow data through an external input file with the extension ’.coolingholes’. This file can be useful in case the flow calculation is integrated into an automatic procedure. For more details on the format of the file, refer to section 74.5. COOLFL = 0: the old algorithm of the cooling/bleed model will be used (model used in FINE™ 6.1 and previous releases). The backward is ensured through this parameter set at 0. = 1: the old algorithm of the cooling/bleed model will be used (model used in FINE™ 6.1 and previous releases) based on an external file with the extension ’.coolingholes’ located in the corresponding computation subfolder will be read and the data specified through the FINE™ interface will be ignored. = 2 (default): the new algorithm of the cooling/bleed model will be used. FINE™ 731 Optional Models Cooling/Bleed d) MAXNBS The maximum allowed number of injection sectors is controlled through the expert parameter MAXNBS (the default value is 50). If the input file contains a higher number of sectors the parameter should be modified. 74.4 Theory If COOLFL=0, the model consists in the addition of local source terms to all the flow equations (mass, momentum, energy and ke equations when a 2equations turbulence model is used). These terms are added as fluxes through the solid boundary cells where a cooling hole has been placed by the user. Fluxes are computed as: • Mass: • Momentum • Energy • k,εequations: F F mass = ρV n S momentum F energy F x, y, z = ρVx, y, z V n S + p∗ n x, y, z S = V n ( ρE + p∗ )S k, ε = ρV n ( k, ε )S where ρ is the density, Vn is the velocity component normal to the solid wall and S is the cooling hole surface.The increased static pressure is computed as: 2 p∗ = p +  ρk 3 (719) V2 E∗ = e +  + k 2 (720) and the total energy E* is: The density required to calculate the velocity components is obtained from the computed pressure field along the walls and from the imposed static or total temperature. Note that for the momentum equations only the velocity term is added as a source term. The pressure term already exists even in the absence of holes. If COOLFL=2, the cooling injection/bleed are treated as additionnal inlet or outlet boundary condition. Finally, the turbulent kinetic energy and dissipation can either be directly imposed by the user or be calculated from the turbulent intensity. In that case, the turbulent kinetic energy is obtained as: k = 1.5 ( Tu ⋅ V ) 2 (721) where V is the velocity magnitude and Tu is the turbulent intensity. The turbulent dissipation is obtained from the relation: 0.75 1.5 Cµ k ε = 0.1D (722) where D is the diameter of the hole and Cµ = 0.09. 732 It should be noted that the velocity remains equal to zero at the walls even in the cooling flow region. Thus the boundary condition on the velocity is left unchanged and the FINE™ Cooling/Bleed Optional Models effect of the cooling flow will be observed in the surrounding cells. However, the temperature field will be affected on the wall itself. 74.5 Cooling/Bleed Data File: ’.coolingholes’ A parser is used to find the data in this file, using keywords to locate the position of the data in the file. The advantage of this technique is that the data do not have to be positioned at a given line in the file, but only have to be followed by the appropriate keyword (the keywords can be written with capitals or not). The user specifies in the file a series of 'injection sectors'. An injection sector is either — a single cooling hole — a series of distributed cooling holes along a line (all holes having the same geometrical and flow properties) — a hub or shroud slot (continuous line of holes along a constant radius and axial position line) Each injection sector should respectively start and end with the keywords INJECTION SECTOR END DATA Each injection sector should contain all the appropriate data. If one data is missing, the flow solver will stop and a message will appear on the screen. 74.5.1 Specification of an injection sector a) Type of injection sector The user should start by defining if the sector is a single injection hole (1), a line of holes (2) or a slot (3): b) Boundary patch The user should specify the block and face number, as well as the boundary patch on which the holes are located. The face number can be 1 (I=1), 2 (J=1), 3 (K=1), 4 (K=KM), 5 (J=JM), 6 (I=IM) The patch number is only required if several solid patches are present on the face (for instance on a hub or shroud wall). c) Position of the holes and slot Three modes are available to locate the holes: c.1) Relative Positioning  for blade walls (can not be used for slots) • spanwise position(s) of the hole or of the 2 extremities of the line of holes (between 0 at the hub and 1 at the shroud) • streamwise position(s) of the hole or of the 2 extremities of the line of holes (between 0 at the leading edge and 1 at the trailing edge). The leading and trailing edges can either be the grid edges, i.e. the points where the periodic lines of the mesh meet the blade walls (parameter ZMNMX=0), or the points located at respectively the minimum and maximum axial positions (parameter ZMNMX=1, valid for axial flow machines). The choice between the two possibilities is made through the expert parameter ZMNMX, whose default value is 0. FINE™ Note that this "blade wall" positioning option is only valid for H or Itype meshes, the 733 Optional Models Cooling/Bleed pressure and suction surfaces being assumed to be located on two opposite faces of the mesh. c.2) space Cartesian (X,Y,Z) positioning data • in case of a hole or of a line of holes the user specifies the Cartesian coordinates of the hole or of the 2 extremities. • in case of slot the user specifies the radius and the Zcoordinate of one point of the slot. A searching procedure is applied to find the closest solid wall cell to the specified point(s). The point is periodically repeated around the machine axis so that the specified point does not need to be located in the blade passage used for the computation. c.3) Grid positioning data The user specifies the grid indices of the hole, of one point of the slot or of the 2 extremities of the line of holes. Depending on the face number, only 2 indices have to be provided (for instance, along the I=1 face, only the J and K indices are required). d) Size of the holes or Width of the slot The user specifies in addition either the diameter of the holes in case of a single hole or a line of holes, or the width of the slot (in meters). e) Flow properties • the mass flow through the hole(s): the specified mass flow is the total mass flow through all the blades. In case of a line of holes, the specified mass flow is the overall mass flow through all the holes. Therefore the mass flow through one hole is the specified mass flow divided by the number of blades and by the number of holes. Mass flow has to be negative for Bleed flow. • the static or total temperature (if both are present only the static temperature will be read). • he turbulent kinetic energy and dissipation, or the turbulent intensity (if the kε model is used). The kinematic turbulent viscosity (if SpalartAllmaras model is used) cannot be specified through an external file ’coolingholes’. f) Velocity direction Finally, when a cooling injection sector has been selected, three ways to impose the injection direction are proposed through the interface: Cartesian, cylindrical or grid indices. When the injection direction is provided by the user through grid indices, 2 angles have to be expressed in degrees. Each angle is measured with respect to the local normal and one of the 2 grid line directions tangent to the wall. The user specifies 2 of the following 3 angles (in degrees), depending on the face on which the hole is located: • Angle with respect to Igrid line • Angle with respect to Jgrid line • Angle with respect to Kgrid line β i , j , k = arctg ( Vi , j , k Vn ) Note that the two angles should be equal to 0 degree to make the velocity direction oriented in the normal direction to the blade wall, whereas a 90 degrees angle induces the velocity vector to be tangent to the corresponding grid line direction. In the case of holes located on the blade walls, and if the mesh has been generated with the AutoGrid software, the K and Jlines are the two tangent directions along the blade wall, respectively oriented in the streamwise and spanwise directions. The Kangle is the streamwise angle, whereas the Jangle is the spanwise angle. 734 FINE™ Cooling/Bleed Optional Models 74.5.2 Summary of all required input data a) Global Data Single hole (1), line(2) or slot(3) Number of holes (if line) Diameter (single hole or line) Width (slot) Block Number Face Number Patch Number (only if several patches) Input Mode (1relative, 2Cartesian(X,Y,Z), 3Grid(I,J,K)) Keyword type number of holes diameter width block face patch mode b) Positioning Positioning  Single Injection Hole if mode 1 Streamwise position of the hole Spanwise position of the hole Positioning  Single Injection Hole if mode 2 Xcoordinate of the hole Ycoordinate of the hole Zcoordinate of the hole Positioning  Single Injection Hole if mode 3 Iindex of the hole Jindex of the hole Kindex of the hole Positioning  Line of Injection Holes if mode 1 Streamwise position of first point Spanwise position of first point Streamwise position of second point Spanwise position of second point Positioning  Line of Injection Holes if mode 2 Xcoordinate of first point Ycoordinate of first point Zcoordinate of first point Xcoordinate of second point Ycoordinate of second point Zcoordinate of second point Positioning  Line of Injection Holes if mode 3 Iindex of first point Jindex of first point Kindex of first point Iindex of second point Jindex of second point Kindex of second point FINE™ Keyword Streamwise position Spanwise position Xcoordinate Ycoordinate Zcoordinate Iindex Jindex Kindex streamwise position of first point spanwise position of first point streamwise position of second point spanwise position of second point Xcoordinate of first point Ycoordinate of first point Zcoordinate of first point Xcoordinate of second point Ycoordinate of second point Zcoordinate of second point Iindex of first point Jindex of first point Kindex of first point Iindex of second point Jindex of second point Kindex of second point 735 Optional Models Positioning  Slot  mode 2 Radius of one point of slot Zcoordinate of one point of slot Positioning  Slot  mode 3 Iindex of one point of slot Jindex of one point of slot Kindex of one point of slot Cooling/Bleed radius Zcoordinate Iindex Jindex Kindex c) Flow Properties Mass Flow (negative if bleed flow) Static Temperature (only for cooling flow) Total Temperature (only for cooling flow) Turbulent Kinetic Energy (only for cooling flow and kε model) Turbulent Dissipation (only for cooling flow and kε model) Turbulent Intensity (only for cooling flow and kε model) Keyword mass flow static temperature total temperature width turbulent dissipation turbulent intensity d) Flow Direction (only for cooling flow) Flow Direction  Cartesian mode Angle with respect to xdirection(degrees) Angle with respect to ydirection(degrees) Angle with respect to zdirection(degrees) Flow Direction  Cylindrical mode Angle with respect to rdirection(degrees) Angle with respect to thetadirection(degrees) Angle with respect to zdirection(degrees) Flow Direction  Grid mode Angle with respect to Kgrid line(degrees) Angle with respect to Jgrid line(degrees) Angle with respect to Igrid line(degrees) Keyword xangle yangle zangle rangle thetaangle zangle Kangle Jangle Iangle 74.5.3 Examples Example 1  Bleed Flow through a Slot define in Grid (I,J,K) mode 736 FINE™ Transition Model Optional Models Example 2  Bleed Flow through a Slot define in Cartesian (X,Y,Z) mode Example 3  Cooling Flow through a Hole define in Cartesian (X,Y,Z) mode Transition Model 75 Transition Model 75.1 Introduction The boundary layer which develops on the surface of a solid body starts as a laminar layer but becomes turbulent over a relatively short distance known as the transition region. This LaminarTurbulent transition is a complex and not yet fully understood phenomenon. Among the numerous parameters that affect the transition one can list: the free stream turbulence intensity, the pressure gradient, the Reynolds number, and the surface curvature. Furthermore, predicting the onset of turbulence is a critical component of many engineering flows. It can have a tremendous impact on the overall drag, heat transfer, and performances especially for lowReynolds number applications. However, most of the turbulent models fail to predict the transition location. Therefore, it is proposed to include a transition model in the original SpalartAllmaras turbulence model in order to take into account the transition onset at a certain chord distance on a blade pressure and suction sides. The transition location (transition line in 3D) should be imposed either through a FINE™ 737 Optional Models Transition Model user input or via a separate guess. It should be pointed out that these transition terms should only be active when the transition module is used. When it is not used, the fully turbulent version of the SpalartAllmaras turbulence model remains unchanged. In the next sections the following information is given on the Transition Model: • section 74.4 provides a theoretical description of the approach used to solve the transition region. • section 74.3 gives a summary of the available expert parameters related to the Transition model. • section 74.2 describes how to set up a project involving the Transition Model under the FINE™ user environment. 75.2 Transition Model in the FINE™ Interface The transition model can be directly activated from the FINE™ interface by opening the Transition Model page under Optional Models. The layout of the page is shown in Figure 7.4.27. FIGURE 7.5.231 Transition Model page in FINE™ A list of all the blades appears in the left box and the remaining area is divided into two boxes for suction and pressure side, respectively. Four choices are possible: — — — — Fully Turbulent Fully Laminar Forced Transition AbuGhannam and Shaw (AGS) Model Furthermore, for Forced Transition, the user has to specify the position of the transition lines on each side of each blade. It is based on the relative streamwise position and it is defined as a line on the blade pressure and/or suction sides from hub to shroud. The user specifies two anchor points through which a straight line will be built by the solver. It should be noted that only blades are transitional while end walls are fully turbulent. 738 The transition model is only available for the oneequation SpalartAllmaras model using AutoGrid mesh and is applied to blade boundaries and work in both steady and FINE™ Transition Model Optional Models unsteady modes. The transition model is not adapted to external cases. R/S interfaces should be correctly oriented (from upstream to downstream) and solid wall of the blades should be adiabatic. For the AbuGhannam and Shaw model: only one "downstream" R/S upstream of each blade is allowed. Furthermore, there are no restrictions on the number of inlets. Finally, a new output has been added into FINE™ on the Outputs/Computed Variables page under the thumbnail Solid data in order to enable the visualisation in CFView™ of Intermittency (more details on this quantity in section 75.4). 75.3 Expert Parameters INITRA (integer): control the number of multigrid iterations (default = 100) performed in fully turbulent after the coarse grid initialization process. Thereafter, the blade pressure side and suction side are identified and the transition line is defined. The computation pursue for the remaining iterations in transitional mode. The transition line derived from the AbuGhannam and Shaw model is computed at each iteration. . Fully Turbulent MultiGrid Initialization Full MultiGrid Coarse Grid Initialization INITRA Transition Model MultiGrid For starting or restarting a computation in transitional mode from a previous solution (fully turbulent or in transitional mode) the expert parameter INITRA should be set to 0 (otherwise iterations will be performed in fully turbulent mode). INTERI (integer): control the type of intermittency distribution (0:binary or 1: from Dhawan and Narasimah) (default = 0). INTERL (integer): control the type of location used for forced transition (0: base on arc length or 1: based on axial chord) (default = 0). FTURBT (real): control the proportion close to the trailing edge that is fully turbulent (default = 0.95). FINE™ 739 Optional Models Transition Model FTRAST (real): prevents the transition to start in an area defined from the leading edge of the mesh. The value set is a percentage of the chord upstream of which the transition is not allowed (by default 0.05: 5%). ITRWKI (integer): switches on the wake induced transition model. When activated (ITRWKI set to 1), the free stream turbulence intensity (defined at the inlet or at the rotor/stator interface) and the turbulence intensity from the boundary layer edge are used to define the transition region. When this parameter is not checked, only the free stream turbulence intensity is used. 75.4 Theory The Transition Model consists of introducing a socalled intermittency, Γ, defined as the fraction of time during which the flow over any point on a surface is turbulent. It should be zero in the laminar boundary layer and one in fully developed turbulent boundary layer. The intermittency function is defined on each point of the blade surface and at each iteration. It is extended to the computational domain by a simple orthogonal extension (i.e., each point of the computational domain has the same intermittency than the closest point on the blade surface). The intermittency is used to multiply the turbulence production term. For the SpalartAllmaras turbulence model this gives: ~ ~ S = ΓS (723) where S˜ is the production term in the SpalartAllmaras in Eq. 452. Freestream wakes (with only a weak production term) will not be affected by the intermittency. A laminar boundary layer will be preserved upstream of the transition location and turbulence could freely develop thereafter. The transition location imposed by the user through the Forced Transition option and by the AGS Model is only appearing if it has been defined in a turbulent boundary layer. 75.4.1 Fully Turbulent When the Fully Turbulent model is selected, the intermittency, Γ is set at 1 on the whole blade suction and/or pressure sides (fully developed turbulent boundary layer). 75.4.2 Fully Laminar When the Fully Laminar model is selected, the intermittency, Γ is set at 0 on the whole blade suction and/or pressure sides (laminar boundary layer). 75.4.3 Forced Transition The first step is to have a description of the blades in EURANUS to be able to position the transition line. Therefore AutoGrid has been adapted to output the position of the leading and trailing edges and the topological patches composing the blade surfaces. This last information is read by FINE™ and transmitted to the solver EURANUS. A dialog box has been created to allow the positioning the transition line on the blade surfaces (Figure 7.5.432). 740 FINE™ Transition Model Optional Models In Forced Transition mode, each transition line is positioned through a point on the hub and a point on the shroud. By default, these points are defined by a percentage of the arc length (Appendix 7.5.432). However, a special treatment is also available where the transition points are defined by a percentage of the axial chord (only available for axial machines). This option can be activated via the expert parameter INTERL that should be set to 1 (default value = 0). The intermittency, Γ, is then computed on each point of the blade surface (it is set to 0 upstream of the transition line and tends towards 1 downstream). Each point of the computational domain has the same intermittency as the one of the closest point on the blade surface. However a special treatment is required close to the trailing edge and in tip gaps. FIGURE 7.5.432 Example of the calculation of a transition point on a blade suction side as a percentage of the chord length. A last aspect of the implementation is the postprocessing. Spalart & Allmaras propose in their article a turbulent index to be able to distinguish turbulent zone from laminar zone. This index is implemented in EURANUS as a solid data. It is defined as: it = ∂ν~ κ ν ω ∂n 1 (724) where n is the direction normal to the solid wall. It is near 0 in the laminar zone and near 1 in the turbulent zone. 75.4.4 AbuGhannam & Shaw Model (AGS) The location of transition could be computed from the flow solution by using empirical relations related to external parameters. It is here proposed to use the correlations obtained by AbuGhannam FINE™ 741 Transition Model Optional Models and Shaw [1980] and derived from experimental data from transition on a flat plate with pressure gradients. According to these authors transition starts at a momentum thickness Reynolds number: F (λθ ) ⎞ ⎛ τ⎟ Rθs = 163 + exp⎜ F (λθ ) − 6.91 ⎠ . ⎝ (725) λθ is a dimensionless pressure gradient defined as: λθ = θ 2 dU e ν ds (726) where Ue is the velocity at the edge of the boundary layer, s is the streamwise distance from the leading edge, and θ denotes the momentum thickness in the laminar region. τ is the free stream turbulence level (in %). The function F(λθ ) depends on the sign of the pressure gradient: F (λθ ) = 6.91 + 12.75λθ + 63.64(λθ ) 2 for adverse pressure gradient (λθ < 0), (727) F (λθ ) = 6.91 + 2.48λθ − 12.27(λθ ) 2 for a favourable pressure gradient (λθ > 0). (728) Therefore, according to these relations, transition is promoted in adverse pressure gradient whereas it is retarded in favourable pressure gradient. The range of application of the AGS correlation is 0.1 > λθ > 0.1, and for a free stream turbulent level ranging from 0.3 to 10%. 75.4.5 Expert Parameters Either using the Forced Transition option or the AbuGhannam and Shaw (AGS) Model, the streamwise evolution of intermittency should be defined. It could be either a binary field or a smoother field. In the current implementation those two options are available. It is controlled by the expert parameter INTERI. With its default value (INTERI = 0) the intermittency is 0 before transition and 1 after the transition onset. If INTERI = 1, intermittency is defined following the relation of Dhawan and Narasimha [1958]: Γ = 1 − exp(−0.412ξ 2 ) ξ= 1 λ Max( s − st ,0) (729) (730) where st is the position of the transition onset and s is the current position on the arc from leading edge to trailing edge. λ is the characteristic extent of the transition region and is determined from the correlation: Re λ = 9 Re st 0.75 (731) Close to the trailing edge the intermittency is set to 1. This is necessary in order to allow a turbulent wake to be generated downstream of the blade. This special treatment is controlled by the expert parameter FTURBT that is set to 0.95 by default (i.e., only the last 5% of a blade side will have an 742 FINE™ Transition Model Optional Models intermittency of 1). In order to get a tridimensional distribution of the intermittency, the intermittency of a cell is the one of the closest cell on a solid surface (hub, shroud, and tip gap are fully turbulent and have an intermittency equal to unity). FINE™ 743 Optional Models 744 Transition Model FINE™ CHAPTER 8: 81 Boundary Conditions Overview During the IGG™ grid generation process, the user has to define the type of boundary condition to be imposed along all boundaries. The parameters associated with these boundary condition types can be fully defined using the Boundary Conditions page. This chapter gives a description of the boundary conditions available on the Boundary Conditions page. In section 82 the Boundary Conditions page is described. For expert use section 83 gives an overview of the available expert parameters. In section 84 some advice is provided on the combinations of boundary conditions to use. For more detailed information section 85 provides a theoretical description of each available boundary condition 82 Boundary Conditions in the FINE™ Interface When selecting the Boundary Conditions page the Parameters area appears as shown in Figure 8.2.01. Five thumbnails are available, depending on the boundary condition types defined in the mesh. There are currently five types of boundary conditions available in the NUMECA flow solver: • • • • • inlet, outlet, periodic (connection with or without rotational or translational periodicity), solid walls, external (farfield). Each of those is described in the next sections. FINE™ Note that the connecting (matching (CON) and nonmatching (NMB)) boundary conditions (without periodicity) do not appear in this menu, because they do not require any input from the user. Only the "periodic" conditions appear under the Periodic menu. 81 Boundary Conditions Boundary Conditions in the FINE™ Interface A common particularity of the five Boundary Conditions pages is their subdivision into two areas. The left area contains always a list of the different patches that are of the boundary condition type of the selected thumbnail. A patch can be identified either by the name of the block face to which it belongs and by its number, or by the numbers of the block and face and by its local index on the face (if no name is provided in IGG™). The right area is the area where the boundary condition parameters are specified for the selected patch(es). FIGURE 8.2.01 Boundary Conditions page One or several patches may be selected in the left area by simply clicking on them. Clicking on a patch unselects the currently selected patch(es). It is possible to select several patches situated one after another in the list by clicking on the first one and holding the left mouse button while selecting the next. To select a group of patches that are not situated one after another in the list, the user should click on each of them while simultaneously holding the key pressed. Several patches can be grouped by selecting them and clicking on the Group button. A dialog box will appear asking for a group name. The name of the group will appear in red color in the list of patches to indicate that this is a group of patches. Every change in the parameters when a group is selected applies to all patches in the group. The Ungroup button removes the group and its patches are displayed individually in the list. The Ungroup button is active only when at least one group is selected. Clicking with the left mouse button on the plus sign + left of a group name in the list will display the patches included in this group. 82 If some of the patches have been given names in IGG™, these names will appear in FINE™ Boundary Conditions in the FINE™ Interface Boundary Conditions FINE™. If the patches have been grouped in IGG™, by giving the same name to many patches, they will appear ungrouped in FINE™ (with block, face and patch number shown after the name) to avoid contradiction between grouping in IGG™ and FINE™. Ungroup button will toggle the IGG™ name of the selected patch(es) with the default FINE™ name (block, face and patch number). If the Graphics Area window with the mesh topology of the project is opened (Mesh/View On/Off menu), all the selected patches and/or groups will be highlighted. A click with the right mouse button over a selected patch will select all the patches and groups in the list that have the same parameters. If the user selects several patches that have different parameters, a warning dialog box will appear. When clicking on OK all parameters will be set equal to the ones of the first patch. Selecting Cancel instead will cancel the selection. (1) (2) (3) FIGURE 8.2.02 Two patches have been grouped into a group called HUB. The right area of all the notebook boundary condition pages is created in a generic way by means of a resource file, where all the boundary condition parameters are described altogether with their default values. Some boundary conditions are only available for an incompressible, compressible or condensable gas flow. FINE™ will automatically disable the boundary conditions that are not available, depending on the type of fluid selected on the Fluid Model page. Also the type of boundary conditions are adjusted according to the selection for Cartesian or cylindrical boundary conditions. The five pages associated to each of the five types of boundary conditions are described in detail in the following sections. FINE™ 83 Boundary Conditions in the FINE™ Interface Boundary Conditions 82.1 Inlet Condition 82.1.1 Available Inlet Boundary Condition Types The inlet boundary condition page is customized according to the configuration of the project (Cartesian or cylindrical) as shown in the following two figures. The user has the freedom to access both types of configurations in the boundary conditions page independently of the mesh properties. 84 FIGURE 8.2.13 Subsonic inlet boundary conditions page for cylindrical problems. FIGURE 8.2.14 Subsonic inlet boundary conditions page for Cartesian problems. FINE™ Boundary Conditions in the FINE™ Interface Boundary Conditions The upper part of the inlet boundary condition page allows the user to select the type of inlet condition to apply to the selected patches through a series of toggle buttons. There are two categories of inlet conditions: conditions applicable to subsonic inlets and conditions applicable to supersonic inlets. Note that to determine whether an inlet (or an outlet) boundary is subsonic or supersonic, the velocity component normal to the boundary should be considered. For each inlet condition type, the lower part of the page is adapted in order to provide input boxes only for the physical variables that are required to fully determine the boundary condition. These variables are for instance: the pressure and temperature (static or total), the velocity components, the velocity magnitude, the velocity angles (specified in radians), or the mass flow. In case of a simulation involving the kε turbulence model, the inlet values of the parameters k and ε are also required. A turbulent viscosity entry appears in case the SpalartAllmaras turbulence model is used. For the inlet boundary conditions: • The velocity components are defined in the Cartesian or cylindrical coordinate system, depending on the selected type. • The pressure and the temperature values to specify can be the static or the total values. • For rotating configurations, the specified values are always the absolute quantities. Three major types of inlet boundary conditions can be identified: • velocity components and the static temperature, • total pressure, total temperature and the flow angles, • total enthalpy, dryness fraction and the flow angles (only for condensable fluid), • mass flow and the static temperature (see the next paragraph for detail on coupling with the outlet). See section 85.1 for more theoretical detail on those boundary conditions. 82.1.2 Coupling Temperature with Outlet Taverage Outlet Taverage + ∆T Inlet FIGURE 8.2.15 Meridional view of the "Coupling with Outlet ID" functionality When mass flow is imposed at an inlet patch, the temperature may be chosen to be coupled to an outlet patch. The coupling is performed through the static temperature. Only in that case, the average temperature Taverage is computed at the specified outlet and imposed at the inlet as Tinlet = Taverage + ∆T (see Figure 8.2.15). The quantity ∆T is a constant temperature difference (>=0 or <0) FINE™ 85 Boundary Conditions in the FINE™ Interface Boundary Conditions specified by the user. This is done in FINE™ by choosing Mass Flow Imposed as boundary condition type for the inlet and clicking on the Coupling Temperature With Outlet button. A pulldown menu allows to select which patch of the outlet must be involved in the coupling. The value to be entered in the static temperature box is ∆T. 82.1.3 Imposing Variables as an Interpolation Profile Each variable can be defined as constant or as an interpolation profile of the variable. The imposed boundary condition may be variable in space (one or two dimensions) and/or in time (in case of an unsteady calculation). To visualize and/or edit the profile data press the small button ( ) on the right side of the label "profile data". This button opens the Profile Manager with the existing profile. See section 212 for a detailed description of the Profile Manager. It offers the possibility to modify or to create a data profile interactively. Click on the OK button to set the new profile to the selected patch(es). FIGURE 8.2.16 The Profile Manager The button Surface data toggles 1D and 2D editing modes. It can be used to change the dimension of an existing profile. 2D profiles are displayed as a "cloud of points". Selecting a point will display the f(x,y) value in blue in the corresponding column of the Profile Manager. 82.2 If a quantity is defined as a function without the definition of a valid profile a warning message will appear when saving the project or opening a new page or thumbnail. In such a case a default constant value is used in the computation. Outlet Condition For a supersonic outlet all variables are extrapolated. An outlet is considered as supersonic on the basis of the normal velocity direction to the boundary. 86 FINE™ Boundary Conditions in the FINE™ Interface Boundary Conditions Three types of subsonic outlet boundary condition are available, as shown in Figure 8.2.27. These three different boundary conditions are described in the following paragraphs. An option for treatment of Backflow Control can be activated in the case of radial diffusers outlet. The purpose of this option is to control the total temperature distribution along the exit section. In case the flow partially reenters the domain through the boundary, the total temperature of the entering flow is controlled so that the entering and outgoing flows globally have the same total temperature. . FIGURE 8.2.27 Outlet boundary conditions page. 82.2.1 Pressure Imposed There are three different methods to impose the pressure at the outlet: • Static Pressure Imposed: the static pressure is imposed on the boundary, the static temperature and the absolute velocity components are extrapolated. As described for the inlet conditions, the static pressure can be constant or defined as a data profile. • Averaged Static Pressure: if imposing an uniform static pressure at the outlet is not an appropriate approximation of the physical pressure distribution at the outlet this boundary condition may be used. In this case only an averaged value for the static pressure is imposed while the pressure profile (around this average) is extrapolated from the interior field (see section 85.2.1). • Radial Equilibrium: This boundary condition is applicable only to cylindrical problems. It is adapted for a patch in which the mesh lines in the circumferential direction have a constant radius. The outlet static pressure is then imposed on the given radius and the integration of the radial equilibrium law along the spanwise direction permits to calculate the hubtoshroud profile of the static pressure. A constant static pressure is imposed along the circumferential direction. See section 85.2.1 for further details. FINE™ 87 Boundary Conditions in the FINE™ Interface Boundary Conditions The pressure imposed at the outlet can be constant or as a function of space and/or time. To define a profile as a function of space and/or time click on the profile button ( box. The Profile Manager will appear as described in section 82.1.3. ) right next to the input text 82.2.2 Mass Flow Imposed When imposing the mass flow at the outlet the related patches must be grouped. This permits to have several groups of patches, each of the groups constituting an outlet through which the mass flow can be controlled. Two different techniques are available to impose the mass flow: • Velocity Scaling: the pressure is extrapolated and the velocity vector is scaled to respect the mass flow. This technique is only valid for subsonic flows, and is not recommended in case of significant back flows along the exit boundary. • Pressure Adaptation: this boundary condition is identical to the ’Uniform outlet pressure’ or ’Radial equilibrium’ boundary conditions, except from the fact that the exit pressure is automatically modified during the resolution process so that after convergence, the prescribed mass flow is obtained. The pressure asked in addition to the imposed mass flow with both options is only used to create the initial solution and for the fullmultigrid process, during which a uniform static pressure outlet condition is used. 82.2.3 Characteristic Imposed This boundary condition has been implemented to increase the robustness in the frame of a design process and is only available when using a perfect and real gas in the Fluid Model page. Figure 8.2.28 shows as an illustration performance curves for a centrifugal compressor. Near choking conditions the mass flow stays almost constant with a variation of the pressure. Therefore it is recommended in this region to impose the static pressure at the outlet. Near stall however, the pressure varies only slightly with varying mass flow. Therefore it is recommended in this region of the performance curve to impose the mass flow at the outlet instead of the static pressure. (static pressure) (mass flow) FIGURE 8.2.28 Example 88 of performance curves for centrifugal compressor FINE™ Boundary Conditions in the FINE™ Interface Boundary Conditions In a design process, with a variation of the geometry, it is not always known in advance where in the performance curve the computations are performed. Therefore it is not always possible to choose the appropriate boundary condition at the outlet for the complete design process. To overcome this problem this boundary condition allows to impose a relation between the mass flow and the pressure at the outlet. It is no longer needed to choose between imposing pressure when working around the chocking part and imposing mass flow when working close to the stall limit. The user has to impose a very simple characteristic line defined through 3 parameters: a target outlet mass flow and a target outlet pressure (at point 2 in Figure 8.2.28) and the pressure at zero mass flow (point 1 in Figure 8.2.28). For more detail on this boundary condition see section 85.2. 82.3 Periodic Condition One important feature of the IGG™ mesh generator concerns the automatic establishment of all connecting and periodic boundary conditions. The corresponding information is transmitted to the FINE™ interface, with the advantage that the user does not need to specify any input concerning these boundary conditions. In the present version, periodic connection is not allowed for blocks with different rotation speed on each side of an interface. Thus no frozen rotor calculation should be performed with periodic connections. Normally no user input is required on this page. The only periodic boundary condition cases for which a user input is required are those in which some of the boundary conditions have to be applied with a periodicity angle that differs from the global periodicity angle of the block. FIGURE 8.2.39 Periodic boundary condition page. In case some input is required this section explains how to define the periodic conditions using the PERIODIC thumbnail. The type of periodicity connection between the patches (Matching or Non Matching) can be entered. A connection is Matching if the numbers of mesh points along the connected patches are FINE™ 89 Boundary Conditions in the FINE™ Interface Boundary Conditions identical, and if all the corresponding points along these patches coincide. The Non Matching connection requires the use of an interpolation process to establish the connection, whereas a matching one consists of a single communication of the flow variables. Some additional characteristics need to be given to fully determine the periodic boundary condition: • For rectangular (Cartesian) problems, the user has to specify the translation vector defining the periodicity. The positive translation vector goes from the current patch to the periodicity patches. • For cylindrical problems, the user has to specify the rotation angle in degrees. The rotation angle is calculated from the connected patch to the current patch, according to the rule of the right handed system. 82.4 Solid Wall Boundary Condition The solid wall boundary condition page is customized essentially according to the type of calculation (inviscid or viscous). For Euler cases (i.e. inviscid), no parameter is requested for the wall boundary conditions. For NavierStokes cases, the box at the top of the page allows to set both velocity and thermal conditions. The type of boundary conditions determines the way the velocity and thermal conditions are defined for the solid boundary. 82.4.1 Cylindrical Boundary Condition a) Area Defined Rotation Speed The wall rotation velocity can be constant or area defined (see Figure 8.2.410). The area defined option allows to attribute a specific rotation velocity to a rectangular zone in the meridional plane independently of the grid structure. FIGURE 8.2.410 Solid 810 boundary conditions page in case of a cylindrical boundary condition FINE™ Boundary Conditions in the FINE™ Interface Boundary Conditions When the area defined option is selected, a small picture defining the parameters is displayed (the z axis is the rotation axis, the r axis is the radial axis). The rotation velocity is set to ω 1 outside the domain and to ω 2 inside the domain. The specified range must be a valid range for the used geometry. For example, for an axial machine the limits for rotation of the hub can be defined by setting the lower and higher axial limit to appropriate values. In such a case it is important to set the radial limits such that they include the full solid (hub) patch. b) Thermal Condition Three options are available for the thermal condition: constant heat flux (in W/m2), adiabatic or isothermal. The imposed heat flux or temperature can be constant on the patch or defined as a profile. Use the pull down menu to change Constant Value to for example Fct(space). Click on the profile button to launch the Profile Manager as described insection 82.1.3. 82.4.2 Cartesian Boundary Conditions The user can define a translation or a rotation velocity vector. In the latter case, the coordinates of the rotation centre are requested. The thermal conditions are similar to those for cylindrical flows. 82.4.3 Force and Torque Below the box, a "Compute force and torque" button is provided that permits to include the selected patches in the calculation of the global solid boundary characteristics. For a cylindrical project (as defined in Mesh/Properties) in an internal flow (the expert parameter IINT set to 1 as by default): — the axial thrust, i.e. the projection of the global force on the rotation axis, — the torque, i.e. the couple exerted by the global force, calculated at (0,0,0). These quantities are often calculated on the rotating walls. They are calculated from the pressure and the velocity fields on the walls. The axial thrust is computed as: ∑ F ⋅ nz . (81) S The projection of the torque along a given direction z , i.e. the couple exerted by the global force along the rotation axis: ⎛ ⎜ ⎝ ⎞ ∑ r × F⎟⎠ ⋅ z (82) S In all other cases the force and torque are computed as: — the lift, — the drag, — the moment calculated at (0,0,0) by default. The direction of the forces and torque as well as the location of the point for the moment can be determined with the expert parameters IDCLP, IDCDP, IDCMP and IXMP (see section 83). Within EURANUS v5.16 it is possible to calculate and to store the partial torque in the corresponding ".wall" file of the computation through the use of the expert parameter IFRCTO within FINE™ GUI. FINE™ 811 Boundary Conditions Boundary Conditions in the FINE™ Interface The partial torque is the torque computed for each layer on the whole blade. When IFRCTO is set to 2 (1 or 3), the torque is defined on each Jdirection (Idirection or Kdirection) layer (i.e. when using AutoGrid meshes, Jdirection corresponds to the spanwise direction). IFRCTO = 2 Total Torque and Force on Suction Side Partial Torque and Force on Suction Side • 56 = 56 sublayers in Jdirection (spanwise) • column 1: %span corresponding to the layer • column 2: Fx on the sublayer • column 3: Fy on the sublayer • column 4: Fz on the sublayer IFRCTO = 0 Total Torque and Force on Suction Side FIGURE 8.2.411 File ".wall" when computing partial torque along the blade Finally, the resulting ".wall" will contain, in addition of the global torque and force on the selected blade, the partial torque for each layer along the Jdirection of the blade as presented in Figure 8.2.411. 82.4.4 Properties of Solid for Turbulence In addition, if the standard kε model or the nonlinear highReynolds kε model is used, the user has to specify the type of wall ("Smooth" or "Rough") and the following constants: the von Karman constant κ and the B constant. If the wall type is rough, the equivalent roughness height k0 and the height of the zero displacement plane d0 are also required. A description of these constants is provided in section 43.6.3. The application field of the ’law of the wall’ imposes restrictions on the grid. The user is strongly advised to check the conformity of this grid with these conditions (section 43). 812 FINE™ Expert Parameters for Boundary Conditions 82.5 Boundary Conditions External Condition (Farfield) The external boundary condition is provided to treat the farfield boundaries when dealing with external flow computations (the expert parameter IINT=0). An example is given in Figure 8.2.512. This type of boundary condition determines whether the flow is locally entering or leaving the flow domain and uses the theory of the Riemann invariants to act consequently on the appropriate variables (see section 85.4). Depending on the chosen turbulence model, five or seven input boxes are provided to specify the freestream values of the variables to be used in the boundary condition formulation. FIGURE 8.2.512 External (farfield) boundary conditions page. Use an external condition rather than an inlet condition for cases for which it is not known if the flow enters or leaves the domain. Condensable gas is not compatible with external boundary condition. 83 Expert Parameters for Boundary Conditions 83.1 Imposing Velocity Angles of Relative Flow In case of a stator calculation it may be convenient to impose the velocity angles of the relative flow at the exit of the upstream rotor. In case of rotors the user may also prefer to impose relative boundary conditions. This procedure is only available in case total conditions and flow angles are FINE™ 813 Expert Parameters for Boundary Conditions Boundary Conditions imposed. In addition to that the extrapolation of Vz must be selected. Note also that both flow angles and total conditions are then treated in the relative mode. The following parameters have to be defined: INLREL: allows to specify relative angles for the cylindrical inlet boundary conditions with total quantities imposed (default value = 0) = 1: inlet for a stator (extrapolation of the axial velocity only). The expert parameter OMGINL has also to be specified, = 2: inlet for a rotor. ANGREL (for stator only): data use with the expert parameter INLREL (default = 1 0.05 0.05): 1st real: relaxation angle (in degrees), 2nd real: distance (%) from hub where the absolute flow angle is extrapolated, 3rd real: distance (%) from shroud where the absolute flow angle is extrapolated. 83.2 IMASFL: Extrapolation of Mass Flow at Inlet expert parameter specially dedicated to radial inlets. The mass flow is extrapolated instead of the velocity for the cylindrical inlet boundary conditions with imposed total quantities: = 0 (default): treatment inactive, the velocity is extrapolated, = 1: option activated, extrapolation of the massflow. 83.3 RELAXP: Outlet Mass Flow Boundary Condition is the underrelaxation for the outlet boundary condition where the mass flow is imposed with the exit pressure adaptation (default value = 1.). VELSCA: is the maximum value allowed for the velocity scaling (outlet boundary condition with mass flow imposed by scaling velocity) (default value = 2.) 83.4 IDCDP: Torque and Force Calculation if cylindrical project (as defined in Mesh/Properties) and IINT=1: direction (x,y,z) of axial thrust, in all other cases: direction (x,y,z) of drag. IDCLP: direction (x,y,z) for lift (not used if cylindrical project and IINT=1), IDCMP: direction (x,y,z) for moment, IFRCTO: calculate and to store the partial torque in the corresponding ".wall" file. More details in section 82.4.3, on page 11, IXMP: 814 coordinate (x,y,z) of the point around which the moment has to be calculated. FINE™ Best Practice for Imposing Boundary Conditions 83.5 Boundary Conditions Euler or NavierStokes Wall for Viscous Flow If the flow type selected is laminar or turbulent NavierStokes, it is possible in Expert Mode to choose between an Euler wall (zero normal velocity) and a NavierStokes wall (noslip condition). Further details on the numerical treatment of the walls are provided in section 85.3. Note that the default (’normal mode’) is a NavierStokes wall. 83.6 Pressure Condition at Solid Wall When the interface is in Expert Mode, two toggle buttons are provided to select the type of pressure condition at the wall: extrapolated or computed from the normal momentum equation. The default (active in Standard Mode) is the extrapolation of the pressure. 84 Best Practice for Imposing Boundary Conditions The quality of the flow simulation rests primarily on the quality of the grid and the imposed boundary conditions. In this section the most adapted boundary conditions are proposed according to the type of studied flow. 84.1 In case of divergence in calculations it is strongly recommended to check by post processing of the solution (in CFView™) that appropriate boundary conditions have been imposed. Compressible Flows For compressible flows it is recommended that the inlet boundary condition fixes the absolute total quantities (pressure, temperature) and the flow angles and that the outlet boundary condition fixes the static pressure (exit pressure). This exit pressure can be imposed as: • a constant value along the exit, • an average value at the exit, • the pressure at midspan for radial equilibrium (only for an axial outlet). The static pressure at the exit of the domain is rarely constant. It is thus advised to impose the pressure as an average value or as a initialization data for radial equilibrium. Even if this value of pressure is known, for numerical reasons it is possible that the computed massflow differs from the expected one. It is thus necessary to modify the exit pressure repeatedly until obtaining the accurate massflow. This procedure can be numerically expensive especially if the calculations are carried out on fine grid. A solution to overcome this drawback is to impose the massflow at the outlet. This can be made by the way of two options: • Velocity Scaling: for low subsonic outlet (Mach number lower than 0.4) this condition fixes the massflow at a given control surface by scaling the vectors on this surface. This is not as robust as to impose the exit pressure and is not recommended in case significant backflow are detected along the exit. In this condition the next option is better suited. FINE™ 815 Theory on Boundary Conditions Boundary Conditions • Pressure Adaptation: in this case, an automatic procedure introduces a variation of the imposed exit pressure at each iteration of the calculation. The pressure is then iteratively updated in order to reach at convergence the imposed massflow. This is not as robust as to impose the exit pressure but is more robust than the velocity scaling option. 84.2 Incompressible or Low Speed Flow For compressible or low speed flows it is recommended to impose the massflow and the static temperature at the inlet and a static pressure at the exit. This couple of conditions inletoutlet has a stabilizing effect on calculations and is also well adapted to provide initial solutions for multistage calculations. 84.3 Special Parameters (for Turbomachinery) In case of flow separation at the outlet of radial diffusers it is recommended to use the backflow treatment option. This option can be activated by pressing the corresponding button (Backflow Control) in the FINE™ interface on the Boundary Conditions page under the OUTLET thumbnail. When endwalls in the inlet regions are strongly varying in radius (e.g. centripetal turbines as in Figure 8.4.313) or in case of highly tangential inlet flow angles it is advised to use the IMASFL expert parameter (in the list of expert parameters on the Computation Steering/Control Variables page in Expert Mode). This option is adapted when the inlet boundary conditions fixes the absolute total quantities (pressure, temperature) and is only valid for nonpreconditioned computations. When it is activated, the massflow is extrapolated instead of the velocity. Radial turbine FIGURE 8.4.313 Example 85 of case with strongly varying radius in the inlet1 Theory on Boundary Conditions The boundary conditions are identified in EURANUS by a number (ITYPE) indicating the type of boundary condition and an index (OPSEL) indicating the variant of the type of boundary condition. In this section the type number and variant index of each described boundary condition is given. 1. Picture from D. Japikse, N.C. Balines, Introduction to Turbomachinery, Concept ETI Inc. and Oxford University Press, 1994. 816 FINE™ Theory on Boundary Conditions 85.1 Boundary Conditions Inlet Boundary Conditions 85.1.1 Cylindrical Inlet Boundary Conditions This boundary condition is activated for the values of the parameter ITYPE = 124 (subsonic) and ITYPE=23 (supersonic). a) Static Quantities Imposed (Subsonic) The complete absolute velocity vector followed by the static temperature on the boundary are specified. Several possibilities exist: • the magnitude of the velocity and the flow angles α and γ are specified (OPSEL = 1): V α = atan θVz (83) V γ = atan r Vz • the magnitude of the velocity and other flow angles δ and ε are specified (OPSEL = 5): V δ = acos r Vm (84) V ε = atan t Vm with V m the meridional velocity ( V m = 2 2 V r + V z ). This option has been designed to allow radial inlet with zero axial velocities, • the cylindrical velocity components are specified (OPSEL = 7). The static pressure is extrapolated from the interior by Eq. 813, which allows to calculate all the primitive variables on the boundary. For a turbulent calculation with the SpalartAllmaras model, the turbulent viscosity has also to be specified on the inlet boundary. When the twoequation turbulent model is selected, the boundary values of k and ε have to be specified. These conditions can also be used for incompressible flows. b) Total Quantities Imposed (Subsonic) Several variants are available based on the specification of flow angles or velocity components. b.1) Absolute flow angles from axial direction: The user specifies two flow angles (of the absolute flow) at the boundary, α and γ, which are defined by Eq. 83 and given in radians. The absolute total pressure and the absolute total temperature on the inlet boundary are also specified and imposed. For turbulent models with additional equations, the corresponding quantities are also specified and imposed. Three variants are available depending on the value that is extrapolated. FINE™ 817 Theory on Boundary Conditions Boundary Conditions • the module of the absolute velocity vector is obtained by extrapolation from the interior field, cf. Eq. 815. (OPSEL=2) • the axial velocity component is extrapolated (OPSEL = 3): ( Vz )0 = ( Vz )1 (85) Note that it is assumed that the angular velocity vector is in the zdirection, ω = ω ⋅ 1z , (86) which makes this direction the axial one. Also note that, as a result of Eq. 86 the absolute and relative axial velocity component are equal. • the mass flow is extrapolated, assuming that the meridional component of the velocity is the one contributing to the mass flow. ( Qm )0 = ( Qm )1 , (87) with Q m = ρV m S . (88) This boundary condition is specially dedicated to radial turbomachinery for which problem of mass flow conservation can arise. It is not interfaced but it can be used by selecting the previous boundary condition (absolute flow angles with extrapolation of velocity) and setting the expert parameter IMASFL to 1. the inlet patches have to be grouped in one group to use this last boundary condition (extrapolation of mass flow). b.2) Relative flow angles from axial direction For a stator calculation it may be convenient to impose the velocity angles of the relative flow at the exit of the upstream rotor. In case of rotors the user may also prefer to impose relative boundary conditions. This procedure is only available in case total conditions and flow angles are imposed. In addition to that the extrapolation of Vz must be selected. Note also that both flow angles and total conditions are then treated in the relative mode. This boundary condition is not directly available in the Boundary Conditions page of the interface. It can be used by selecting the previous boundary condition (absolute flow angles with extrapolation of the axial velocity component) and using the expert parameter INLREL. In this case, relative flow angles, relative total pressure and relative total temperature are specified in the interface instead of the absolute values. Set INLREL to 1 in the case of stators. In the case of rotors (INLREL=2) the approach is exactly the same as the one used when absolute conditions are imposed. The adopted approach consists of imposing boundary conditions, which are still defined in the absolute frame of reference, but which vary from one iteration to the other in order to respect the imposed relative value. This technique provides a robust algorithm with an underrelaxation of the evolution of absolute conditions and a special treatment of the hub and shroud boundary layers. Indeed as the hub and shroud walls are usually not rotating, the relative flow angle tends to 90 degrees in the boundary layer, which complicates the boundary condition treatment if the relative conditions are imposed. The above approach (switch to the absolute frame of reference) allows computing the absolute flow angles distribution through an extrapolation in the boundary layers. The underrelaxation factor as well as the percentage of the distance from the hub and the shroud where the angle is extrapolated are specified in the expert parameter ANGREL. The relation between the relative (β) and absolute (α) angles is the following: 818 FINE™ Theory on Boundary Conditions Boundary Conditions ωr tan α = tan β + Vz (89) where ω is the speed of rotation of the upstream rotor specified in the expert parameter OMGINL and r the radial position. The update of the flow angle is followed by the update of the absolute total conditions according to: ( ωr ) ωrV a r T 0 = T 0 –  + θ2c p cp 2 a p0 = a γ ⁄ (γ – 1) r ⎛T ⎞ p 0 ⎜ 0r⎟ ⎝ T 0⎠ . (810) The initial values of the absolute flow angle and total conditions are set to the value of the relative ones except with the initial solution for turbomachinery. In the initial solution for turbomachinery, Eq. 89 and Eq. 810 are used to compute the initial absolute flow angle and total conditions from the specified relative values. b.3) Velocity direction The user first specifies a direction (given under the form of a vector) that corresponds to the direction of the absolute velocity vector. Note that this vector does not have to be a unitary vector. The r,θ,z components of the direction vector are given. E.g. if the user enters the direction (0,1,1) the user imposes that the θ and zcomponents of the absolute velocity vector at inlet are equal and that the radial velocity is zero. The absolute total pressure and the absolute total temperature on the inlet boundary are also specified. These values will be imposed. The module of the absolute velocity vector is extrapolated from the interior field. Using subscript 0 for the boundary, and subscript 1 for the first internal cell: V0 = V 1 (811) where V represents the absolute velocity. (OPSEL = 4). The velocity vector on the boundary is found by scaling the velocity vector specified in the boundary condition file such that the correct module is obtained. For a turbulent calculation with the SpalartAllmaras model, the turbulent viscosity has also to be specified on the inlet boundary. When the twoequations turbulent model is chosen, the boundary values of k and ε have to be specified. c) Mass Flow Imposed (Subsonic) This boundary condition permits to impose the value of the mass flow through a specified control surface. The control surface is defined by grouping several patches into the same group. In addition to the mass flow the direction of the velocity vector and the static temperature are imposed (ITYPE=28). Two variants are available: • the swirl can be imposed, as well as the direction of the velocity vector in the meridional plane (Vr/Vm,Vθ,Vz/Vm) (OPSEL 1). • the direction of the absolute velocity vector can be imposed (Vr /V, Vθ/V, Vz/V) (OPSEL 2). FINE™ 819 Theory on Boundary Conditions Boundary Conditions Two possibilities exist for the treatment of the static temperature: • it can be imposed at a given fixed value, • a relation can be imposed between the inlet static temperature and the averaged temperature along a specified outlet. In this case the user specifies the patch name (or group name) of the connected outlet and the difference of temperature between the inlet and outlet temperatures. The difference of temperature is specified instead of the static temperature. If the specified value is zero, the temperature at the inlet will be equal to the average outlet temperature, whereas if the specified values is for instance 20, the temperature will be equal to the outlet temperature + 20. For turbulent models with additional equations, the corresponding quantities are also specified and imposed on the inlet boundary. d) Imposing the Complete Flow Conditions (Compressible, Supersonic) d.1) Total quantities Instead of specifying static pressure, static temperature and the three absolute velocity components, one can also specify absolute total pressure, absolute total temperature, absolute Mach number and two flow angles α, β defined as (ITYPE = 23, OPSEL = 1): V α = atan θVr V β = acos zV , (812) with the angles given in radians. For a turbulent calculation with twoequation model the boundary values of k and ε also have to be specified. With the SpalartAllmaras model, the turbulent viscosity has to be specified along the boundary. d.2) Static quantities The flow at inlet is completely specified, by giving the static pressure, static temperature and the three absolute cylindrical velocity components (ITYPE = 23, OPSEL = 2). For turbulent models with additional equations, the corresponding quantities are also specified and imposed on the inlet boundary. e) Total Enthalpy & Dryness Fraction Imposed (Subsonic  Condensable Gas) In cases where the inlet thermodynamic state is located on the saturation curve or inside the biphasic zone, traditional boundary conditions based on total temperature and total pressure are not sufficient, as pressure and temperature become interdependent. An additional information is required, which is the dryness fraction. The boundary condition proposed under FINE™ GUI is based on the absolute total enthalpy and the dryness fraction. The velocity direction is also specified, either by means of two flow angles (from axial direction) or of velocity direction vectors. 820 It should be mentioned that the use of this boundary condition requires the presence of the saturation table (’PSA.atab’) of the fluid in the corresponding subfolder. The boundary condition is based on the dryness fraction (X), whose value is bounded between 0 and 1. The inlet thermodynamic must be either saturated or be located inside FINE™ Theory on Boundary Conditions Boundary Conditions the biphasic zone. The validity of the condensable fluid model is limited to gases with small fraction of liquid (X > 0.9) or reversely to liquids with small fraction of gas (X < 0.1). The implementation of the boundary condition is based on extrapolation of the static pressure, which permits to evaluate the saturated liquid and gas values of the density and enthalpy. The dryness fraction permits to deduce the values of the local static enthalpy and density. The other boundary conditions are then used to calculate the velocity vector. 85.1.2 Cartesian Inlet Boundary Conditions This boundary condition is activated for the values of the parameter ITYPE = 24 (subsonic) or ITYPE=23 (supersonic). a) Static Quantities Imposed with Extrapolation of the Static Pressure (Subsonic) The complete absolute velocity vector followed by the static temperature on the boundary are specified (OPSEL = 1). For turbulent models with additional equations, the corresponding quantities are specified also. The static pressure is extrapolated from the interior. Using subscript 0 for the boundary, and subscript 1 for the first internal cell one has: p0 = p 1 , (813) which allows to calculate all the primitive variables on the boundary. These conditions can also be used for incompressible flows. b) Total Quantities Imposed (Subsonic) The user first specifies a direction (given under the form of a vector) that corresponds to the direction of the absolute velocity vector. Note that this vector does not have to be a unitary vector. The x,y,z components of the direction vector are given. E.g., entering the direction (0,1,1) imposes that the y and zcomponent of the absolute velocity vector at inlet should be equal. In other words, the flow comes in at an angle of 45 degrees between z and ydirection, whereas the angle between zand xdirection is 0 degrees. The absolute total pressure and the absolute total temperature on the inlet boundary are also specified. These values will be imposed.Two variants are available depending on the value that is extrapolated: • the absolute Mach number is extrapolated from the interior field (OPSEL = 2, only available for compressible fluid): M0 = M1 , (814) • the module of the absolute velocity vector is extrapolated from the interior field. V0 = V1 (815) where V represents the absolute velocity. (OPSEL = 3). For both variants, the velocity vector on the boundary is found by scaling the velocity vector specified in the boundary condition file such that the correct module is obtained. FINE™ 821 Boundary Conditions Theory on Boundary Conditions For a turbulent calculation with the SpalartAllmaras model, the turbulent viscosity has also to be specified on the inlet boundary. For a turbulent calculation with a twoequation model, the boundary values of k and ε have to be specified. c) Mass flow, Direction of Absolute Velocity Vector and Static Temperature Imposed (Subsonic) This boundary condition permits to impose the value of the mass flow through a specified control surface. The control surface is defined by grouping several patches into the same group. In addition to the mass flow, the direction of the velocity vector and the static temperature are imposed (ITYPE=28). • the direction of the absolute velocity vector is imposed in the Cartesian coordinate system (Vx/ V,Vy/V,Vz/V) (OPSEL 3). Two possibilities exist for the treatment of the static temperature: • it can be imposed at a given fixed value, • a relation can be imposed between the inlet static temperature and the averaged temperature along a specified outlet. In this case the user specifies the patch name (or group name) of the connected outlet and the difference of temperature between the inlet and outlet temperatures. The difference of temperature is specified instead of the static temperature. If the specified value is zero, the temperature at the inlet will be equal to the average outlet temperature, whereas if the specified values is for instance 20, the temperature will be equal to the outlet temperature + 20. For turbulent models with additional equations, the corresponding quantities are also specified and imposed on the inlet boundary. d) Imposing the Complete Flow Conditions (Supersonic) The flow at inlet is completely specified, by giving the static pressure, static temperature and the three absolute Cartesian velocity components (ITYPE = 23, OPSEL = 0). This boundary condition is only available for a compressible fluid. For a turbulent calculation with the SpalartAllmaras model, the turbulent viscosity has also to be specified on the inlet boundary. When the twoequation turbulent model is selected, the boundary values of k and ε have to be specified. 85.2 Outlet Boundary Conditions 85.2.1 Outlet Boundary Conditions for Subsonic Flow a) Static Pressure Imposed ITYPE = 25; OPSEL = 10. The static pressure at the outlet boundary is specified. The remaining dependent variables on the outlet boundary are obtained from the interior field through extrapolation. The default extrapolation is a zero order extrapolation of the static temperature and the absolute velocity. Several options are available: • order of extrapolation: zero or first order (in expert user mode), • backflow treatment (see section 85.2.3): active or not. 822 FINE™ Theory on Boundary Conditions Boundary Conditions The purpose of the treatment of backflow is to control the total temperature distribution along the exit boundary. In case the flow partially reenters the domain through the exit boundary, the total temperature of the entering flow is controlled so that the entering and outgoing flow globally have the same total temperature. b) Averaged Static Pressure Imposed ITYPE = 27; OPSEL = 40 In some cases, an uniform pressure can not be imposed on the whole outlet area. This boundary condition allows imposing an averaged static pressure. The remaining dependent variables on the outlet boundary are obtained from the interior field through extrapolation. The pressure profile is obtained by extrapolation from the interior field and it is translated to ensure that the computed averaged pressure on the outlet area is the target averaged pressure specified by the user. This translated profile is then the imposed pressure profile. The options described in the previous paragraph (section a) are still available. The outlet patches have to be grouped in one group to use this boundary condition. c) Static Pressure Imposed with Radial Equilibrium ITYPE = 125 This boundary condition is only valid on surfaces with mesh lines at constant radius. The static pressure in the outlet section is assumed to be uniform in the tangential direction and to vary in radial direction according to: 2 v θ ∂p = ρ ⋅  . ∂r r (816) The user specifies the static pressure at a specific radius, followed by that radius and the radial direction. The radial direction is specified by using the block orientation (Idirection, Jdirection or Kdirection). The pressure distribution in the outlet section is then found by integrating Eq. 816 with pitchwise averaged values of Vθ and r. The other variables are extrapolated following the system of options exposed above. See “Static Pressure Imposed” on page 22. The treatment of backflow is not implemented for this boundary condition. d) Mass Flow Imposed ITYPE = 27 The outlet patches have to be grouped in one group to use this boundary condition. d.1) Velocity Scaling OPSEL = 20 This condition can be used for low speed subsonic outlet (Mach Number < 0.3). It fixes the mass flow at a given control surface by scaling the velocity vectors on this surface. The other variables are extrapolated following the system of options exposed above. FINE™ 823 Theory on Boundary Conditions Boundary Conditions The scaling of the velocity vector is not totally free. The value of the scaling factor is constrained between VELSCA and 1/VELSCA, where VELSCA is an expert parameter available in the Control variables page in the expert mode. Given that the pressure is also extrapolated with this condition, it is imperative that the inlet boundary condition fixes the pressure through the total pressure. Fixing the mass flow is not as robust as to impose the pressure and this is particularly sensitive with fullmultigrid. A pressure is thus requested as input and is imposed during the fullmultigrid process. Consequently, the mass flow computed at outlet is not exactly the target mass flow during the computation on the coarse grids. This option is not recommended in case significant backflow is detected along the exit. The next option (exit pressure adaptation) is then better recommended. d.2) Pressure Adaptation OPSEL = 30 This boundary conditions is an adaptation of the "uniform static pressure imposed" and "static pressure imposed with radial equilibrium" boundary conditions. The only difference is that an automatic procedure is included that introduces a variation of the imposed exit pressure at each iteration of the calculation. The pressure is iteratively updatet in order to reach at convergence the imposed mass flow. The successive pressure modifications are calculated according to: p new = p old · r gas T ref actual imposed (Q + RELAXP –Q ) , 2 L ref (817) where Lref and Tref are the characteristic length and reference temperature specified in the Flow Model page. rgas (RGAS) and RELAXP are expert parameters defined in the Control Variables page. The expert parameter RELAXP introduces an underrelaxation of the successive modifications of the exit pressure. The default value is 1. The value of the exit pressure provided by the user is the initial one. In case the radial equilibrium is used, the initial value of the exit pressure is imposed at midspan. Contrary to the previous option fixing the mass flow through velocity scaling, it is only after convergence of the procedure that the mass flow reaches the imposed value. e) Characteristic Imposed ITYPE = 29 This boundary condition has been implemented to increase the robustness in the frame of a design process. Indeed it is not always suitable to impose the pressure at the exit because it can drive the machine to stall when the geometry change affects its characteristic line. The proposed solution is to impose a relation between the mass flow and the pressure at the outlet. It is no longer needed to choose between imposing pressure when working around the chocking part and imposing mass flow when working close to the stall limit. The user has to impose a line defined through 3 parameters: a target outlet mass flow ( Qt ), a target outlet pressure ( p Qt ) and the pressure at zero mass flow ( p Q0 ). See section 82.2 for a schematic representation of this boundary condition. The implementation follows three principles: 824 FINE™ Theory on Boundary Conditions Boundary Conditions • The relation between mass flow and pressure is imposed from a function of the type: F ( Q, p ) = 0 , (818) ( p Qt – p Q0 ) 2 Q . F = p – p Q0 – 2 Qt (819) with (820) A linearisation of the relation is applied to obtain: ∂F ∂F F +  δQ +  δp = 0 , ∂p ∂Q (821) where the δ are the variations of the mass flow and averaged exit pressure and where F and its derivatives are computed from the old values of p and Q. • The local outgoing characteristic variables are extrapolated. • the relation between p 1 and p 0 is imposed as follows: p 0 = p 1 + ∆p , (822) with ∆p is constant over the whole outlet and with the subscripts 0 and 1 corresponding respectively to the value in the first outer cell and in the first inner cell. Combining these three principles and expressing Q and p in function of ∆p at the outlet, Eq. 821 can be written as a polynome of second order in ∆p. The suitable root is chosen so that the imposed pressure always respects the relation defined between the mass flow and the pressure during the computation. 85.2.2 Outlet Boundary Conditions for Supersonic Flow ITYPE = 22 This condition is to be used in case of supersonic outflow and is only valid for compressible fluids. The dependent variables at the outlet are extrapolated from the interior through firstorder extrapolation. If no preconditioning is used, there is some checking on negative or small pressures: if the static pressure is less than 1E15 after extrapolation, it is put to 1E15. 85.2.3 Treatment of Backflow at Outlet (Radial Diffuser) The option for the treatment of backflow can be activated by pressing the corresponding button in the FINE™ interface. This option has been initially implemented in order to ensure a proper treatment of radial diffusers outlets in case of flow separations. The treatment is based on the hypothesis that the absolute total temperature should be constant throughout the outlet section. If the flow is reentering the numerical domain through a part of the outlet section, a hybrid boundary condition is applied in that region: • the static pressure is imposed, • the velocity vector is extrapolated, FINE™ 825 Theory on Boundary Conditions Boundary Conditions • the absolute total temperature is imposed at a value equal to the averaged total temperature along the outlet (the averaging is performed throughout the region where the flow leaves the domain. This treatment permits to avoid the introduction of an uncontrolled total temperature level in the regions where the flow reenters the domain, and in this way to better respect the physics of the flow. Limitations: • only for compressible fluid, • it is applied separately on each outlet patch when an uniform static pressure is imposed (it is applied to a group of patches if ITYPE=27, i.e. averaged static pressure and mass flow imposed). • not available for the outlet boundary conditions where static pressure is imposed with radial equilibrium. 85.3 Solid Wall Boundary Conditions 85.3.1 Euler Walls ITYPE = 15, ITYPE = 16 (default). For Euler walls the velocity has to be tangential to the wall. To obtain the velocity vector on the wall, the velocity vector is first extrapolated from the interior with zero or first order extrapolation according to the selected option in the FINE™ interface: w∗ w = w 1 3 1 w∗ w =  w 1 –  w 2 2 2 (823) with subscripts w,1,2 denoting respectively the wall, the first and the second inner cell. The tangential part of the extrapolated velocity vector is: w ** w = w∗ w – ( w∗ w ⋅ n )n , (824) with n the normal to the wall. The velocity vector on the wall is finally found by a scaling process such that its module equals: ww = w1 . 3 1 w w =  ⋅ w 1 –  ⋅ w 2 2 2 (825) The wall density and pressure are obtained through extrapolation from the interior with zero order: ρw = ρ1 pw = p1 826 FINE™ Theory on Boundary Conditions Boundary Conditions or first order: 3 1 ρ w =  ρ 1 –  ρ 2 2 2 pw 3 1 =  p 1 –  p 2 2 2 . (826) Alternatively the pressure can be solved from the normal momentum equation (ITYPE=15): n ⋅ ∇p = ρv ⋅ ⎛ v ⋅ ∇⎞ n , ⎝ (827) ⎠ which is written in a local curvilinear system as: ∂n ∂n ∂p ∂p ∂p ρv wall ( v wall ⋅ S i )  + ( v wall ⋅ S k )  = S i ⋅ n  + S j ⋅ n  + S k ⋅ n ∂ξ ∂ζ ∂ξ ∂η ∂ζ , (828) where ξ, η, ζ represent the coordinate directions, and where it is assumed that the jdirection and η is the direction away from the wall (which is not necessarily perpendicular to the wall). ∂p Eq. 828 is then solved for  , whereas zeroorder extrapolation is used for the density. ∂η 85.3.2 NavierStokes Walls a) Adiabatic Walls The velocity vector on the wall vanishes. ITYPE = 11 or 13 are used for Cartesian boundary condition, 111 or 113 for cylindrical. If condition 111 or 113 is used, the angular velocity of the wall (in the absolute frame of reference) has to be specified. The velocity relative to the wall should be zero, leading to: w = – ( u s – uw ) , (829) with subscripts s, w referring to respectively the system and the wall. A relation for the pressure is obtained by projection of the momentum equation onto the wall normal direction n . Written in the absolute frame of reference: n ⋅ ∇p = – ρ n ⎛ V ⋅ ∇⎞ V + n ⋅ ⎛ ∇ ⋅ τ⎞ . ⎝ ⎠ ⎝ (830) ⎠ The normal pressure gradient can be written as a function of pressure derivatives along the coordinate lines: 1 ∂p ∂p ∂p n ⋅ ∇p =  S j ⋅ S i + S j ⋅ S j + S j ⋅ S k ∂ ζ ∂ η ∂ζ Sj Ω , (831) where ξ, η, ζ represent the coordinate in the i, j and k directions, and where it is assumed that the jdirection is directed away from the wall (not necessarily perpendicular to the wall). S i, j, k are the surface vectors of the corresponding cell faces. Combining Eq. 830 and Eq. 831 and considering that the velocity vanishes on the wall, yields: FINE™ 827 Theory on Boundary Conditions Boundary Conditions ∂p 1 Ω ∂p ∂p Ωρ ⎛ = – 2 S j ⋅ S i + S j ⋅ S k –  ⋅ n V ⋅ ∇⎞ V +  n ⎛ ∇ ⋅ τ⎞ ⎝ ⎠ ⎝ ⎠ ∂η ∂ξ ∂ξ S Sj Sj j = COR 1 COR2 (832) COR3 Two implementations of the adiabatic NavierStokes wall are available. In the simplest one (ITYPE=13 or 113), only the terms COR1 and COR2 of the equation above are taken into account in the evaluation of the pressure derivative. This corresponds to assume that the normal pressure gradient equals zero. Taking into account that the velocity, appearing in the term COR2, is the velocity on the wall, this term can be simplified to: Ωρ 2 COR2 = 2 ⋅ S j r ⋅ ω w Sj (833) Note that COR2 vanishes for a stator wall. In the more complicated implementation (ITYPE=11 or 111) the complete normal momentum equation is considered in the evaluation of the pressure derivative, i.e. the term COR3 is also accounted for. Applying Gauss' theorem this term can be rewritten as: n n COR3 =  Ω ⎛ ∇ ⋅ τ⎞ = ⎠ S S ⎝ Sj n ∫ ⎛⎝ ∇ ⋅ τ⎞⎠ dΩ = S °∫ τdS ≈ ∑τ ⋅S S i 2 i . (834) faces Once ∂p/∂η is determined, the pressure on the wall is obtained as (assuming the direction points inside the interior field, and with indices w,1 representing the wall and the first inner cell): 1 ∂p p w = p 1 –   . 2 ∂η (835) The temperature on the wall is obtained by expressing that the normal temperature gradient vanishes, or in terms of the derivatives along the coordinate lines, cf. Eq. 831: ∂T 1 ∂T ∂T = – 2 S j ⋅ S i + S j ⋅ S k ∂η ∂ξ ∂ξ Sj . (836) The wall temperature is then found using a similar equation as Eq. 835. The density follows from pressure and temperature through the appropriate relation, depending on the type of gas. b) Isothermal Walls The implementation of this boundary condition is very similar to the adiabatic NavierStokes wall. The only difference is in the determination of the wall temperature, which is fixed to the specified temperature in the current boundary condition. Again two versions are available, depending on whether all the terms in the normal momentum equation are taken into account when determining the wall pressure (ITYPE 12 ≡ 11; 14 ≡ 13; 112 ≡ 111; 114 ≡ 113). For the cylindrical isothermal walls, #112 and #114, the angular velocity of the wall has to be specified. For all versions (#12,#112,#14,#114) the wall temperature is specified. The pressure is determined as in the adiabatic condition and the density follows from pressure and temperature through the appropriate relation, depending on the type of gas. 828 FINE™ Theory on Boundary Conditions Boundary Conditions c) Wall with Imposed Heat Flux The implementation of this boundary condition is very similar to the previous ones. For this condition (ITYPE = 10 or 110) the temperature is determined from the imposed heat flux (W/m2). The pressure is determined as in the adiabatic condition and the density follows from pressure and temperature through the appropriate relation, depending on the type of gas. 85.4 Farfield Boundary Condition ITYPE = 21 uses Riemann invariants that are defined as: 2c ± R n = Vn ±  , γ–1 (837) + where R n are the Riemann variables associated with the direction n and c is the local speed of sound. + + For subsonic inflow, R n corresponds to a positive, incoming characteristic. R n is then obtained from the free stream values: 2c ∞ +  , R n = V ∞ ⋅ n + γ–1 (838) where V ∞ is the free stream velocity, c ∞ the free stream speed of sound.  R n , on the other hand, corresponds to an outgoing characteristic and has to be estimated from inside the computational domain by an appropriate extrapolation: 2c R n = V i ⋅ n – i , γ–1 (839) where subscript i refers to values from the interior. Linear extrapolation of the variables to the external boundary will be used to obtain a sufficiently accurate solution: 3 1 q i =  q 1 –  q 2 , 2 2 (840) where subscript 1 and 2 refer to the first two inner points. The normal velocity and the local speed of sound can now be obtained on the boundary by adding +  and subtracting both Riemann variables R n and R n : +  Rn + Rn γ–1 , c wall = ( R +n – R n )  . V w ⋅ n = 2 4 (841) The entropy on the wall is set to the free stream entropy. All the flow variables can then be obtained. Corresponding formulas hold for a subsonic outflow with the difference that R n + and the wall entropy are obtained from interior values. FINE™ 829 Theory on Boundary Conditions Boundary Conditions For supersonic flows, both Riemann variables and the entropy are obtained from free stream values for inflow, interior values for outflow. For preconditioning computation, the same principle is used with modified invariants defined as: 2 2 2 2 ⎛ ⎞ ⎞ ⎛ pg vn ⎞ 2 β β ± 2⎛  – α⎟ + 4 ⎜ 1 –  β , R n = v n – 2 v n ⎜ 1 – 2 – α⎟ − v 1 – ⎜ + n 2 2⎟ ⎝ ⎠ ⎝ ⎠ ⎝ 2ρβ c c c ⎠ (842) where p g = p – p ref β = β∗ U ref 2 2 . (843) The free stream variables of static pressure, static temperature and the three velocity components are specified by the user in the boundary condition file. For a turbulent calculation with a twoequation model, the k and ε values on the boundary are set to their free stream values (inflow) or extrapolated from the interior (outflow). 830 FINE™ CHAPTER 9: 91 Numerical Model Overview To define numerical parameters of the computation, the Numerical Model page allows to define several aspects of the computation: • the CFL number, • the multigrid parameters, • preconditioning parameters (if applicable). These parameters are described in the next section. FIGURE 9.1.01 Numerical model interface In expert user mode (Expert Mode) additional parameters are available as shown in Figure 9.1.02: additional multigrid parameters and unsteady parameters. These interfaced expert parameters are described in section 93. Also the noninterfaced expert parameters are described in this section. More theoretical information on the available parameters related to the numerical model (spatial and temporal discretizations) is provided in section 94. FINE™ 91 Numerical Model in FINE™ Numerical Model FIGURE 9.1.02 Numerical Model page in expert mode 92 Numerical Model in FINE™ 92.1 CFL Number This box allows to tune the CFL (CourantFriedrichLevy) number to be employed in the computation. This number globally scales the timestep sizes used for the timemarching scheme of the flow solver. A higher value of the CFL number results in a faster convergence, but will lead to divergence if the stability limit is exceeded. 92.2 Multigrid parameters In the left part of the Numerical Model page, three boxes are visible. The first one is an information box, named ’Grid levels: current/coarsest’. It indicates for each of the i, j and k directions the currently selected grid level and the number of the coarsest grid level available in the corresponding direction. The second box of the Numerical Model page is an input box that allows to define for each of the i, j and k directions the ’Current grid level’. • The coarsest grid level depends on the number of times the grid can be coarsened, along each of the (i,j,k) directions. For example, if the grid has 17*33*33 points in the i, j, k directions, it has respectively 16*32*32 cells. The i direction (16 cells) can thus be divided 4 times by 2, while the others can be divided 5 times by 2. The following grid levels are then available: 000 17*33*33 (18,513 points) 111 9*17*17 (2,601 points) 222 5*9*9 (405 points) 333 3*5*5 (75 points) 444 2*3*3 (18 points) 455 2*2*2 (8 points) 92 FINE™ Expert Parameters for the Numerical Model Numerical Model The coarsest grid level available is then 4 along i and 5 along j and k. • The current grid level is the finest grid level (for each of the i, j and k directions) on which the computation will take place. The selected levels should be in the range between 0 and the coarsest grid level available for each of the i, j and k directions. Referring to the example given just above, the user can do a first run on level 3 3 3 to validate the computational parameters and then switch to level 1 1 1 or 0 0 0 for a finer solution. It gives a high flexibility to the system since with one grid, the user can run simulations on several submeshes. All combinations between the i, j and k grid levels, in the specified range, are possible such as 2 3 1 or 0 3 2...etc. Press after each modification to validate the new specified levels. The use of multigrid is highly recommended in order to ensure fast convergence of the flow solver. The mesh used to discretise the space can have multiple grid levels in each direction of the computational domain i, j and k. These levels are numbered from 0 (finest grid) to N (coarsest grid). The grid level (N) available in one direction (I, J, or K) is the smallest grid among all patches on that particular direction (I, J, or K). The third box, named ’Number of Grid(s)’, permits to significantly accelerate the convergence to steady state if several grid levels are available: the flow calculation is performed simultaneously on all the grid levels. This technique is referred to as the multigrid strategy. This number should be chosen as high as possible, and deduced from the information displayed on the available grid level and the grid level on which the computation will be performed (’Current Grid Level’). Finally, the toggle button ’Coarse Grid Initialization’ enables, before calculating the flow on the mesh contained in the IGG™ files, to perform a preliminary flow calculations on a coarser mesh automatically created by the flow solver by coarsening the initial one. This provides a rapid estimation of the flow. This technique is referred to Full Multigrid. 92.3 Preconditioning Parameters This box allows to define the preconditioning numerical parameters. These parameters are only available when an incompressible fluid is selected on the Fluid Model page or when the Low Speed Flow (M<0.3) option is selected on the Flow Model page. Preconditioning is described in detail in section 43.8. Especially section 43.8.5 provides more information on the value to choose for β*, the reference velocity and the option to use Local velocity scaling. 93 Expert Parameters for the Numerical Model 93.1 Interfaced Expert Parameters 93.1.1 Multigrid Strategy If the button ’Coarse Grid Initialization’ is activated, the computation starts on the coarsest grid level and includes a finer grid level each time one of the two following criteria is satisfied: FINE™ 93 Expert Parameters for the Numerical Model Numerical Model • The maximum number of cycles to be performed on each grid level is reached. This parameter is specified through the input box in the Full MultiGrid Parameters area as the Maximum number of cycles per grid level. • The residual on the current grid level has dropped a certain order of magnitude as indicated by the Convergence criteria on each grid level in the Full MultiGrid Parameters area. • An additional input box permits to select the number of sweeps to be performed on the coarse grid levels through the input box ’Number of sweeps on successive grid levels’. The amount of sweeps is the amount of times the RungeKutta operator respectively the chosen relaxation operator is applied (see section 94.4 for more detail). In the default configuration of the solver called ’Linear progression’, the number of sweeps on each level equals the level number (2 sweeps on second level,...). It has been observed in many cases that the convergence rate may be significantly improved by performing a higher number of sweeps on the coarsest levels. Recommended sets of values are proposed in the Sweeps area through the parameter Scheme definition: for instance (1,2,16) in case of 3 grid levels. However, it is should be noted that more sweeps have as a consequence more time required for an iteration. 93.1.2 Spatial Discretization Two types of spatial discretization are available: • central scheme (default) and • upwind scheme. Furthermore, if an upwind discretization is chosen, an input box appears in a ‘Spatial discretization parameters’ area to specify the order of accuracy of the desired upwind scheme: first or second order. See section 94 for more detail on those different schemes. Condensable fluid option is not compatible with the use of upwind schemes for space discretization. 93.1.3 Temporal Discretization The temporal discretization scheme used for the computation is an explicit multistage RungeKutta scheme. In the interface, the time stepping technique should be selected between Local time stepping (default) and Global time stepping. See section 94 for more detailed information on the temporal discretization. In general the default scheme is recommended. If the computation is an unsteady computation, unsteady parameters box appears. Please refer to chapter section 42.1 for a description of those unsteady parameters. 94 FINE™ Expert Parameters for the Numerical Model 93.2 Numerical Model Noninterfaced Expert Parameters Additional parameters related to the numerical model are available in the list on the Control Variables page in Expert Mode. 93.2.1 Multigrid IPROLO: Indicates the order of the prolongation within the multigrid approach: = 0: is piecewise constant prolongation, = 1 (default): is linear prolongation (no damping if 1), = 2 linear prolongation except at boundaries(2). When used with a preconditioned formulation, this damping option is somewhat useless and can be damaging. FINETM sets it therefore to off when the preconditioning is involved. IRESTR: Gives the order of the restriction operator of the multigrid. = 0 (default): corresponds to linear restriction, = 1: to quadratic restriction. MGRSTR: Applies only for multigrid and fixes the type of multigrid cycle. MGRSTR=1: Vcycle; MGRSTR=2: Wcycle; MGRSTR=3: Fcycle; MGRSTR=4: Vcycle in sawtooth; MGRSTR=5: Wcycle in sawtooth; MGRSTR=6: Fcycle in sawtooth. Default MGRSTR=1. MGSIMP: Applies only for multigrid. If MGSIMP>1 a simplification will be used on coarser levels. If MGSIMP=1 a more dissipative scheme is used on coarser meshes, i.e. firstorder upwind (if IUPWIN=1) or central scheme with increased 4th order dissipation on solid walls (if IUPWIN=0). If MGSIMP=2, in addition to the simplification for MGSIMP=1, viscous and source terms (of turbulence) are neglected on coarser levels. No simplification for MGSIMP=0. Default MGSIMP=1 RSMPAR: Residual smoothing parameter σ*/σ. A value less or equal to zero means no residual smoothing. SMCOR: Only used in case of multigrid. SMCOR has the same meaning as RSMPAR but applies to the interpolated multigrid corrections instead of the residuals. SMCOR indicates whether interpolated corrections should be smoothed or not. The default value for SMCOR is 0. 93.2.2 Spatial Discretization IFACE: = 1(default): Cell face gradients are used for the viscous fluxes, = 0: cell corner gradients. IWAVVI: Only used if IFACE=0. If IWAVVI=0 the cell face gradients are obtained by arithmetic averaging of the cell corner gradients. If IWAVVI=1 a weighted averaging is used instead, taking the cell volumes into account. a) Central Discretization CDIDTE: FINE™ Constant used in the exponential damping factor that is used in the numerical dissipation for k and ε, both if central or upwind schemes are used. The default value for CDIDTE is 100 95 Expert Parameters for the Numerical Model Numerical Model EXPMAR: Exponent in the multidimensional scaling model of Martinelli of the dissipation used in central schemes (see section 94.1.3). Default EXPMAR=0.5 i.e. multidimensional scaling not used. IARTV2: Define whether the second order artificial dissipation switch should be based on both pressure and temperature gradients (parameter IARTV2=1) or on pressure gradients only (IARTV2=0). In the default configuration, only pressure gradients are taken into account. Both pressure and temperature gradients (IARTV2=1) can only be taken into account for compressible cases. VIS2: Coefficient κ(2) for 2nd order dissipation in the central scheme (default VIS2=1.0). VIS2KE: Used only for kε turbulence model. Coefficient κ(2) for 2nd order dissipation in the central scheme, as applied to the k and ε equations. Default VIS2KE=1.0 VIS2SW: This parameter switches off all second order dissipation for incompressible fluids (when set to the default: VIS2SW=1). Second order dissipation is intended for stabilization of the shocks but there are no shocks in incompressible flows. Therefore the default is to switch off all second order dissipation for incompressible fluids. Sometimes it may be stabilizing to use some second order dissipation. In that case set this parameter to zero. VIS4: Coefficient κ(4) for 4th order dissipation in the central scheme. Default VIS4=0.1 VIS4KE: Used only for kε turbulence model. Coefficient κ(4) for 4th order dissipation in the central scheme, as applied to the k and ε equations. Default VIS4KE=0.1 VISNUL: Eliminates 2nd order dissipation fluxes along the physical boundaries (central scheme). Default VISNUL=1. If VISNUL=0, the procedure is not applied. b) Upwind Discretization ENTRFX: Entropy coefficients, see Eq. 92, on page 98 and Eq. 93, on page 98. The first value is the entropy coefficient applied to the linear field, the second value is applied to the nonlinear field. ENTRFX<1. means a constant value, ENTRFX>1. means scaled with the spectral radius through a factor ENTRFX1. IRATIO: Vector of two values, that indicate which effective ratio is to be used, see Eq. 927, on page 913. The first value applies to the linear field, the second to the nonlinear field. IRATIO is only active for secondorder upwind schemes. IROEAV:1 indicates that Roe averages are to be used to calculate cell face data. See Eq. 914, on page 910. If IROEAV=0, arithmetic averaging will be used. 93.2.3 Time Discretization IBOTH: used in combination with ISWV. The latter parameter indicates whether the dissipation terms are recalculated or not in the different RungeKutta stages. IBOTH=0 means that the dissipation term only contains the physical, viscous dissipation; IBOTH=1 means that it also contains the artificial/upwind dissipation. The default value = 2 means that the dissipation term contains only the artificial dissipation. The physical dissipation is computed once per time step. IRKCO: RungeKutta coefficients. One for each stage, the first one for the first stage, the second one for the 2nd stage and so on. The default values that are used when nothing is set in IRKCO are: 96 FINE™ Theory Numerical Model 1st order upwind  Van Leer: 4stage .0833 .2069 5stage .0533 .1263 2nd order upwind  Van Leer: 4stage .1084 .2602 5stage .0695 .1602 central scheme  Jameson: 4stage .25 .3333 5 stage .25 .1666 both central and upwind  Eliasson: 4stage .125 .306 5stage .0814 .191 .4265 .2375 1. .4414 1. .5052 .2898 1. .5060 1. .5 .375 1. .5 1. .587 .342 1. .574 1. NSTAGE: number of stages for the explicit RungeKutta scheme. In practice, 4 or 5 stage schemes are mostly used. IRSMCH: specifies the type of residual/correction smoothing. ISWV: = 1: standard version, Eq. 958, = 2 (default in incompressible cases): Radespiel & Rossow, Eq. 959, = 3 (default in compressible cases): Zhu, time step dependent coefficients, see Eq. 961, = 4: Swanson & Turkel viscous, = 5: Vatsa, Eq. 963. On meshes without high aspect ratio. governs the recalculation of the dissipative residual in the different RungeKutta stages. A value α between 0 and 1 is allowed. Zero means no recalculation of dissipative residual (latest available value will be used); 1 means recalculation. For intermediate values, a weighted averaging of the latest dissipation residual and of the preceding one is applied with the weight α and (1α) respectively. E.g. for a 5stage scheme: ISWV = 1 0 1 0 1, means that the dissipative residual is calculated in 1st,3rd and 5th stage only. ISWV is used in combination with IBOTH. RSMPAR: residual smoothing parameter σ*/σ. A value less or equal to zero means no residual smoothing. Default value 2. 94 Theory 94.1 Spatial Discretization The discretization in space is based on a cell entered control volume approach. The general Navier Stokes equation Eq. 91 is discretised as: ∫ ∂U Ω∂ t dΩ + ∑ F ∆S + ∑ F ∆S = ∫ Q dΩ , I faces V faces (91) Ω where F I ∆S , F V ∆S are respectively the inviscid and viscous fluxes. FINE™ 97 Theory Numerical Model 94.1.1 Viscous Fluxes The viscous fluxes are determined in a purely central way. As they contain gradients, gradients must be evaluated on the cell faces. This is done by applying Gauss' theorem: 1 1 ∇Φ =  ∇Φ dΩ =  ΦdS . Ω Ω ∫ °∫ (92) Two options exist: If the expert parameter IFACE=0, the gradients are first calculated in cell corners. This is done by applying Eq. 92 using as control volume, the volume that has the cell centres that surround the cell corner of interest as corner points, as depicted in Figure 9.4.13 (a) below for two dimensions. The cell face gradient is then obtained by averaging the gradients in the 4 corners of the cell face. Arithmetic averaging (input variable IWAVVI=0) or a more accurate weighted averaging may be chosen (IWAVVI=1). cell centre cell corner (a) FIGURE 9.4.13 : cell face i+1/2 cell face j+1/2 (b) (c) Different control volumes used to calculate gradients in cell corners or cell faces. If IFACE=1 (Default), gradients are calculated directly on cell faces. Figure 9.4.13 (b) and (c) illustrate the control volumes used to find the gradient on respectively the cell face i+1/2 and j+1/2. The option IFACE=1 is more robust and therefore preferred (default), although it is more expensive as the total number of cell faces is approximately 3 times the number of cell corners. 94.1.2 Inviscid Fluxes The inviscid fluxes appearing in Eq. 91 are upwind based numerical fluxes, and therefore noted with a * superscript. The inviscid numerical flux is expressed as, Hirsch (1990): ( Fn ) * i+1⁄2 1 =  { ( Fn ) i + ( Fn ) i + 1 } – d i + 1 ⁄ 2 . 2 (93) The first term in the righthandside of Eq. 93 corresponds to a purely central evaluation of the flux. The term d i + 1 ⁄ 2 represents a numerical dissipation term, that may be an artificial dissipation, used in combination with central schemes, or the dissipation associated with upwind schemes. In Eq. 93 an arithmetic averaging technique is used. Alternatively, instead of averaging the fluxes in Eq. 93, a flux can be used, based on the averaged unknowns, i.e. 98 FINE™ Theory Numerical Model ( Fn ) Ui + Ui + 1 = Fn ⎛⎝ ⎞⎠ – d i + 1 ⁄ 2 . 2 * i+1/2 (94) Theoretically, the formulation Eq. 93 is to be preferred, but, in combination with the central scheme, the formulation of Eq. 94 (default) is sometimes more robust, especially for high speed flows. Both central schemes and upwind schemes are available within EURANUS. Currently, the arithmetic averaging given by Eq. 94 is the only available option. 94.1.3 Central Scheme In the former case, a Jameson type dissipation is used with 2nd and 4th order derivatives of the conservative variables, Jameson (1981): di + 1 ⁄ 2 = ε (2 ) i + 1 ⁄ 2 δU i + 1 ⁄ 2 ( 4) 3 + εi δ Ui + 1 . (95) The scalar coefficients ε are given by: ε (2 ) i+1⁄2 ε (2) The coefficients κ , κ ters. (4) (4 ) The cell entered values of ε 1 (2) * =  κ λ max ( ν i – 1, ν i, ν i + 1, ν i + 2 ) 2 i+1⁄2 1 (4 ) * (2 ) = max ⎛ 0,  κ λ ε i + 1 ⁄ 2⎞ ⎝ 2 ⎠ . (96) are user input, respectively VIS2,VIS4 in the noninterfaced parame(4) in Eq. 95 are obtained by arithmetic averaging of the cell face val ues of Eq. 96. The variables v i are sensors to activate the seconddifference dissipation in regions of strong gradients, such as shocks, and to deactivate it elsewhere. They are based on pressure and temperature variations (depending on the value for the expert parameter IARTVZ) and are defined as: ⎧ p i + 1 – 2p i + p i – 1 , T i + 1 – 2T i + T i – 1 v i = max ⎨  p ⎩ i + 1 + 2p i + p i – 1 T i + 1 + 2T i + T i – 1 ⎫ ⎬ ⎭ (97) for all equations except the k and ε equations. For liquids, only a pressure switch is used. For the k and ε equations, v i is based on the pressure, on the turbulent kinetic energy and on the dissipation rate: ⎧ p i + 1 – 2p i + p i – 1 , k i + 1 – 2k i + k i – 1 , ε i + 1 – 2ε i + ε i – 1 v i = max ⎨   ⎩ p i + 1 + 2p i + p i – 1 k i + 1 + 2k i + k i – 1 ε i + 1 + 2ε i + ε i – 1 ⎫ ⎬ ⎭ . (98) * λ in Eq. 96 is a measure of the inviscid fluxes and is commonly chosen as the spectral radius multiplied with the cell face area: * λ = λ * i+1⁄2 = ( v∆S + c∆S ) i + 1 ⁄ 2 . (99) On high aspect ratio meshes, the resulting dissipation in the streamwise direction may become very low. Increasing it may improve the robustness and the convergence rate. According to Martinelli (1987), the spectral radii in the other directions are also accounted for. Instead of Eq. 99 one uses: FINE™ 99 Theory Numerical Model * λ = max { λ * i + 1 ⁄ 2, (λ * i + 1 ⁄ 2) 1–σ (λ * j + 1 ⁄ 2) σ ,(λ * i + 1 ⁄ 2) 1–σ (λ * k + 1 ⁄ 2) σ } (910) The spectral radii in the other directions are defined similar as in Eq. 99, e.g. for the jdirection: λ * j+1⁄2 = ( v i + 1 ⁄ 2 ∆S j + 1 ⁄ 2 + c i + 1 ⁄ 2 ∆S j + 1 ⁄ 2 ) (911) The cell face normal ∆S j + 1 ⁄ 2 is obtained by averaging the normals on the 4 cell faces in the jdirection, belonging to the 2 cells that share the i+1/2 cell face. The parameter σ is user input (EXPMAR). The default value is 0.5, i.e. Eq. 99 is used. In the current version of EURANUS, the Martinelli approach is not yet implemented for the turbulence equations. Note that if the k – ε turbulence model is chosen, the resulting equations for k and ε are solved (2) (4 ) with the central scheme. Separate coefficients κ , κ for the artificial dissipation can be chosen, respectively VIS2KE and VIS4KE in the noninterfaced expert parameters. Both the 2nd and 4th order dissipation are damped by multiplying them with the following exponential function: + 2 y 1 – exp ⎛ – ⎛ ⎞ ⎝ ⎝ C⎠ ⎛ V 2⎞ ⎞ exp – ⎜ 3⎟ ⎠ ⎝ S ⎠ . (912) The constant C corresponds to the input variable CDIDTE. The above expression means that the damping is applied in the region where y+ δ (917) Eq. 917 limits the minimum value of λ i + 1 ⁄ 2 to δ . In subsonic and transonic cases a small constant value (<1.) for the entropy fix δ suffices (choose the input variable ENTRFX < 1.). For flow simulations in high speed regime, it is advised to scale the entropy fix with the spectral radius, by choosing the input variable ENTRFX > 1, e.g. ENTRFX=1.05 or 1.1. The scaling factor is then ENTRFX1., i.e.: δ = ( ENTRFX – 1. ) λ * i+1⁄2 . (918) The latter choice also increases the robustness, at the expense of a slightly increased dissipation. Two values for ENTRFX are to be specified. The first one applies to the linear field (the characteristic variables that propagate with speed un ), the second value to the nonlinear field (the characteristic variables that propagate with speed un ± c ). For firstorder upwind schemes, the limiter vanishes and both FDS TVD and STVD reduce to the same firstorder accurate upwind scheme. FINE™ 911 Theory Numerical Model For secondorder upwind schemes, the limiter is activated. The limiter Q i + 1 ⁄ 2 acts on ratios r i + 1 ⁄ 2 of variations of the characteristic variables, defined as: δi – 1 ⁄ 2W + δi + 3 ⁄ 2W , r i + 1 ⁄ 2 = r i + 1 ⁄ 2 = δi + 1 ⁄ 2W δi + 1 ⁄ 2W (919) For the FDS TVD scheme, Q is function of only one of the ratios, according to the sign of the eigenvalue:  Q = Q ( ri + 1 ⁄ 2 ) λi + 1 ⁄ 2 > 0 + Q ( ri + 1 ⁄ 2 ) λi + 1 ⁄ 2 < 0 Q = (920) The following limiters are available: Q ( r ) = minmod ( 1, r ) , (921) 2 r+r Q ( r ) = 21+r r>0 (922) r<0 = 0 r+ r Q ( r ) =  , 1+r (923) Q ( r ) = max [ 0, min (1,2r), min (2,r) ] , (924) which represent respectively the Min Mod limiter (LIMITE=1), the Van Albada limiter (LIMITE=2), the Van Leer limiter (LIMITE=3) and the Super Bee limiter (LIMITE=4). The function minmod chooses the value with the minimum module. In the STVD scheme, the check on the eigenvalue sign is avoided by choosing Q as a function of  the two ratios r and r +  + Q = Q ( r i + 1 ⁄ 2, r i + 1 ⁄ 2 ) . (925) Since the 'classical' limiters such as Van Leer, Van Albada, Min Mod, Super Bee are defined as a function of one ratio, Eq. 925 would exclude these limiters in a STVD context. A new family of nonseparable limiters, containing also smooth limiters, is proposed within EURANUS, Lacor et al. (1993). * The classical limiter functions are applied to a socalled effective ratio r , which is an average of  + r and r :  + Q ( r , r ) = Q ( r* ) . (926) The same functions Q as given in Eq. 921 to Eq. 924 can be chosen, where the ratio r is replaced by the effective ratio r* (the same limiters as for the FDS scheme are used). The following possible choices for the effective ratio are proposed: 912 FINE™ Theory Numerical Model +  2  + 2 +  r (r ) + r (r ) 2r r +  ≤  ≤ r + r ≤ .5 ( r + + r  ) ≤ max (r +,r ) . min (r ,r ) ≤ 2 2 + + r +r (r ) + (r ) (927) It can be shown that these new limiters guarantee monotonicity provided that: r* ≥ 0 , (928) which is easily achieved by switching the limiter off for negative r* . The effective ratios in Eq. 927 are given in order of increasing magnitude. It can be shown that the lower r* , the more diffusive the resulting limiter is. The choice of effective ratio is governed by the input parameter IRATIO. IRATIO=1 corresponds to the smallest value in the list of Eq. 927, IRATIO=2 to the 2nd smallest value, and so forth, with IRATIO=6 corresponding to the maximum value. For both the FDS and the STVD scheme, different limiters can be applied to the linear field (the characteristic variables that propagate with speed un ) and to the nonlinear field (the characteristic variables that propagate with speed un ± c ). In addition, for the STVD scheme, a different specific ratio can be chosen for both fields. To this end, the input variables LIMITE (corresponding to the type of limiter selected in the Numerical Model page) and IRATIO are vectors of length two. The first component determines the choice of limiter, respectively the effective ratio for the linear field, the second component for the nonlinear field. In general, robustness is increased by applying a more diffusive limiter. By applying this limiter only to the nonlinear field, and a compressive one to the linear field, a good compromise between robustness and accuracy can be obtained. The upwind dissipation can also be reformulated to let the limiter act on ratios of variations of the primitive variables. Combining Eq. 99 to Eq. 911 the limiter function can be moved outside the diagonal matrix and put in front of the primitive variable variation: 1 1 –1 d i + 1 ⁄ 2 =  R i + 1 ⁄ 2 diag ( λ i + 1 ⁄ 2 )L i + 1 ⁄ 2 [ 1 – Q i + 1 ⁄ 2 ]δ i + 1 ⁄ 2 V . 2 (929) The limiter function is the same as before and acts on ratios as in Eq. 919 or Eq. 927 where the characteristic variable variations are replaced by primitive variable variations. Eq. 929 can be simplified to 1 d i + 1 ⁄ 2 =  An i + 1 ⁄ 2 ( 1 – Q i + 1 ⁄ 2 )δ i + 1 ⁄ 2 V . 2 (930) ∂ ( Fn ) The Jacobian matrix in Eq. 930 is the Jacobian with respect to the primitive variables  : ∂V An = RΛL 94.2 –1 . (931) Multigrid Strategy EURANUS uses multigrid for efficiency and fast convergence. The input variable given by the user (Numerical Model page: Number of Grid(s)) denotes the number of grid levels to be used. The coarser grids are automatically created within EURANUS by dropping nodes in each direction. If in FINE™ 913 Theory Numerical Model a certain direction, the grid can not be coarsened any more (because of an odd number of cells) before reaching the desired number of grid levels, EURANUS will create the missing grids by coarsening only in the remaining directions. Finest level : 000 Coarse level : 111 Coarse level : 2 2 2 Coarsest level : 3 3 3 MG Cycle FIGURE 9.4.24 Scheme of the multigrid strategy The multigrid method is based on the Full Approximation Storage (FAS) approach. V (input parameter MGRSTR=1), W (MGRSTR=2) and Fcycle (MGRSTR=3) can be chosen by the user, or if preferred their sawtooth variant (MGRSTR =4,5,6 for respectively V,W,F sawtooth). In the sawtooth variant no smoothing (i.e. RungeKutta solver or implicit solver) will be applied in the coarsetofine part of the cycle. As a result, the solution is only prolonged when passing from coarse to fine. FIGURE 9.4.25 Scheme of the multigrid method Consider a set of meshes denoted with an index l = 1,...,L with L being the finest level. The NavierStokes problem on the finest level can be written as: L ∂U  + N L ( U L ) = 0 , ∂t (932) L where N L ( U ) is the spatial discretization of the NavierStokes operator on the finest mesh L . The problem is then approximated on coarser levels l as: l ∂U  + N l ( U l ) = F l , ∂t (933) with F l the forcing function, defined recursively as: l F l = N l ( Il + 1 U 914 l+1 l l+1 ) + ˆI l + 1 [ F l + 1 – N l + 1 ( U ) ] , (934) FINE™ Theory Numerical Model l l where I l + 1 and ˆI l + 1 represent restriction operators of respectively the unknowns and the residu als. If the input variable IRESTR=0, they are defined as: ∑R , ∑Ω U =  , ∑Ω ˆI l R l + 1 = l+1 l+1 l+1 l+1 l Il + 1 U where R l+1 (935) l+1 (936) l+1 is defined as: R l+1 = Fl + 1 – Nl + 1 ( U l+1 ) (937) and Ω represents the cell volume. The summation in Eq. 935 and Eq. 936 is over the 8 fine cells contained within a coarse cell. If IRESTR=1 a more complicated quadratic restriction is used both for the residuals and the unknowns. After temporal discretization, Eq. 933 becomes: l S∆U + N l ( U l(0) ) = Fl . (938) l (0 ) U is the current solution on mesh l, around which the equations have been linearized (in an implicit method) and which has to be smoothed. One has: U l ∆U is an update of U l (0 ) l (0 ) l = Il + 1 U l+1 (939) and is to be calculated. S is the smoother. It is the operator that corresponds to the chosen time integration method. In EURANUS, an explicit multistage RungeKutta timemarching scheme has been implemented, see below. l l The linear problem Eq. 938 can be solved for ∆U . The updated solution U will be smoothed (provided S is a good smoother) and can be restricted to the next coarser level, according to Eq. 939 with l replaced by l1. Note that the number of smoothing sweeps (i.e. the number of times the RungeKutta operator respectively the chosen relaxation operator is applied) can be chosen by the user for each grid level (Numerical Model page in Expert Mode: Scheme definition and Number of sweep on successive grid levels) as described in section 93.1.1. Once the solution on the coarsest mesh is smoothed, the coarsetofine sweep of the multigrid cycle is initiated. The current solutions on finer grids are updated with the solution on the next coarser level: l Ul= Ul + Ill1 (Ul1  Il1 l U) (940) l The operator Il1 is a prolongation operator, which may be of zero (i.e. piecewise constant, input parameter IPROLO=0) or firstorder (IPROLO=1). FINE™ 915 Theory Numerical Model In the basic V,W,F cycle (MGRSTR = 1,2,3 respectively) the new solution on the finer mesh is l ( 0) l smoothed before proceeding to the next finer level, by solving Eq. 935, with U = U . The number of sweeps of the smoothing operator is user input (Numerical Model page in Expert Mode: Scheme definition and Number of sweep on successive grid levels). In the sawtooth type cycles (MGRSTR=4,5,6) the system of equations is not solved in the coarsetofine part of the multigrid cycle. The user also has the possibility to smooth the corrections after prolongation (2nd term in the righthandside of Eq. 940) before adding them to the current finer grid solution, by applying the residual smoothing operator to the corrections. This is governed by the input parameter SMCOR which has the same definition as RSMPAR, see below, and allows to calculate the smoothing parameter, according to the chosen type of residual smoothing (parameter IRSMCH), see below. In EURANUS, the computing cost of a multigrid cycle is significantly reduced by using simplifying assumptions on coarser (i. e. all levels but the finest) grids (input parameter MGSIMP). If MGSIMP=1, a firstorder accurate upwind scheme is used on coarser levels (if Upwind spatial discretization scheme is selected in the Numerical Model page in Expert Mode), else a more diffusive central scheme is used on coarser levels (if Central spatial discretization scheme is selected in the Numerical Model page in Expert Mode). If MGSIMP=2 in addition to the changes for MGSIMP=1 also viscous terms as well as source terms (of turbulence and chemistry) are omitted on coarser levels. 94.3 Full Multigrid Strategy In order to create a good initial solution, Full Multigrid is also available. The structure of Full Multigrid can be well explained through Figure 9.4.36. One starts an iteration method, such as a multistage RungeKutta explicit scheme, on the coarsest grid. The solution on that level will not be interpolated to the next finer grid until it converges to a certain accuracy level. Then the solution on the finer grid is taken as the initial solution for further iterations run on that grid level. The process is recursively used until the finest grid is reached. The initial solution on the finest grid is called the solution obtained by a Full Multigrid method. Finest level : 000 Coarse level : 111 Coarse level : 2 2 2 Coarsest level : 3 3 3 FMG Cycle FIGURE 9.4.36 Scheme Prolongation of solution Prolongation of correction of the full multigrid strategy It should be mentioned that there are two different kinds of prolongation in Full Multigrid. One is the same as that used in the standard multigrid cycle, the other is the prolongation of solutions, which replaces corrections in a standard multigrid prolongation. The latter could be different from the former. Normally a zeroorder prolongation is often used for the solution interpolation in a full multigrid cycle. Based upon numerical experiments, it has been found out that it is very important to check the convergence level of solutions on the coarser grid before switching to the next finer grid. The reason 916 FINE™ Theory Numerical Model for this is that if solutions do not converge on the coarser grid, it may cause divergence on the next finer grid. In addition, an initial solution on coarse grids is less sensitive to multigrid convergence than on the finest grid. A large cell size makes solutions converge easily and fast. Hence it takes much less computational time and risk of blowing up to get reasonable solutions on the finest grid, when compared to the start directly on the finest grid. A full multigrid method can therefore improve the robustness and efficiency of numerical iterations methods. 94.4 Time Discretization: Multistage RungeKutta An explicit qstage RungeKutta scheme for the equation dU = F(U) dT (941) can be written: 1 n n 2 n 1 n q–1 u = u + α 1 ∆tF ( u ) u = u + α 2 ∆tF ( u ) … q (942) u = u + ∆tF ( u u n+1 = u ) q The coefficients α i determine the stability area and the order of accuracy of the RungeKutta scheme. They can be chosen in such a way that they suit the problem to be solved. For inviscid calculations the local (i.e. for each cell) inviscid time step is calculated as: t ⎛∆ ⎞ ⎝ Ω⎠ I CFL =  . wS i + wS j + wS k + c [ S i + S j + S k ] (943) CFL is the user specified CFL number (variable CFL on the Numerical Model page). The vectors S are cell normals at the cell centre (obtained by averaging the normals on the cell faces) in respectively i,j and kdirection. The module corresponds to the cell face area. For viscous calculations one also calculates a local viscous time step in each cell. If a viscous CFL number (expert parameter CFLVIS by default set at 1) is specified by the user in the Control Variables page, i.e. the input variable CFLVIS > 0, the following formula is used for the viscous time step: t ⎛∆ ⎞ ⎝ Ω⎠ ν CFLVISΩρ  , = 2 2 2 8µ { S i + S j + S k + 2 [ S i S j + S i S k + S k S j ] } (944) with µ the local laminar viscosity (laminar simulation) or the sum of local laminar and turbulent viscosity (turbulent simulation). The actual local time step is then the minimum of both time steps: FINE™ 917 Theory Numerical Model t ⎛∆ ⎞ ⎝ Ω⎠ ⎧ ∆t ∆t ⎫ = min ⎨ ⎛ ⎞ ,⎛ ⎞ ⎬ . ⎝ Ω⎠ ⎝ Ω⎠ I ν⎭ ⎩ (945) If the input variable CFLVIS < 0 (Default) the viscous CFL number, CFLVIS, is replaced by the inviscid CFL number, CFL in Eq. 944. The actual local time step is then obtained by weighting the inviscid and viscous time step according to a harmonic mean formula: t ∆t ⎛∆ ⎞ ⎛ ⎞ ⎝ Ω⎠ ⎝ Ω⎠ ∆ t I ν ⎛ ⎞ = ⎝ Ω⎠ t⎞ ⎛ ∆t⎞ ⎛∆  + ⎝ Ω⎠ ⎝ Ω⎠ I ν (946) If local time stepping is used i.e. each cell in the computation domain has its own time step given by Eq. 943, for inviscid calculations and Eq. 945 or Eq. 946 (depending on CFLVIS) for viscous calculations. If global time stepping is used, i.e. in all cells the same time step is used, which is, for stability reasons, the minimum of the local time steps. This option is only to be used for unsteady simulations when the dual time stepping approach (default) is not selected. For steady simulations, it is recommended always to choose local stepping, as it will increase the convergence rate. In practice, 4 or 5 stage RungeKutta schemes are mostly used. In EURANUS the following coefficients are default for 4 and 5 stage schemes: For central schemes α 1 = .125; α 2 = .306 ; α 3 = .587 ; α4 = 1. α 1 = .0814 ; α 2 = .191 ; α3 = .342 ; α4 = .574 ; α5 = 1. (947) For firstorder upwind schemes: α 1 = .0833 ; α 2 = .2069 ; α 3 = .4265 ; α4 = 1. α 1 = .0533 ; α 2 = .1263 ; α 3 = .2375 ; α4 = .4414 ; α 5 = 1. (948) For secondorder upwind schemes: α 1 = .1084 ; α 2 = .2602 ; α 3 = .5052 ; α 4 = 1. α 1 = .0695 ; α 2 = .1602 ; α 3 = .2898 ; α4 = .5060 ; α5 = 1. (949) The user has the possibility to provide the RungeKutta coefficients through the expert parameter IRKCO. The first element of IRKCO corresponds to the first coefficient, the 2nd element to the second, and so forth. A maximum of 10 coefficients (i.e. a 10stage scheme) is foreseen. If all elements of IRKCO are zero the default values are used as listed in section 93.2.3. In Jameson (1985) the dissipative terms are calculated only once or a few times in a qstage RungeKutta scheme. This approach reduces the computational cost substantially. The disadvantage is that the dissipative terms need to be stored separately. For the laminar NavierStokes equations with 5 equations, 5 extra arrays are required to store the dissipative residuals from the artificial dissipation. The residual F ( U ) is split into a convective and a dissipative part: F(U)=Q(U)D(U) (950) The artificial (central or upwind) dissipation terms, cf. Eq. 92, are accounted for either in the convective part (parameter IBOTH = 0) or in the dissipative part (parameter IBOTH = 1). 918 FINE™ Theory Numerical Model The expression for F in Eq. 942 at any stage m is then F m= F(Um ) = Q(Um ) – D(U r) (951) where m is the current stage and r is the latest stage at which the dissipative residuals have been evaluated. The recalculation of the dissipative residuals is governed by the (vector) variable ISWV. For a mstage RungeKutta scheme the m first elements of this vector are used, the first element corresponding to the 1st stage, the 2nd element to the 2nd stage and so on. If the element of ISWV is 0 it means that the dissipative residual should not be calculated at the corresponding stage, and the latest available dissipative residuals will be used; if it is 1, D will be calculated. Note that for consistency reasons, the first value of ISWV should always be one. For upwind schemes, in order to run at high CFL numbers, it is advised to recalculate the upwind dissipation at every stage. The best strategy is to chose IBOTH=0 (upwind dissipation put in convective residuals, and hence calculated at each stage). ISWV monitors then only the recalculation of the physical dissipation (i.e. NavierStokes terms) and a calculation on the first stage only is usually enough (ISWV=1 0...0). Central schemes are usually less sensitive to the recalculation of the artificial dissipation, so that IBOTH=1 can be used. The recalculation of artificial dissipation is then also governed by ISWV. However only one calculation (ISWV=1 0...0) may not be enough; a better choice is for instance recalculation once every 2 stages, e.g. ISWV= 1 0 1 0 1 for 5stage RungeKutta. For IBOTH=2 (Default), the same strategy as for IBOTH=1 is used but in addition the physical viscous terms are evaluated only once per iteration. For nonequilibrium real gas calculations (ITYGAS=4 in corresponding ’.run’ file) the input variable ISWS governs the recalculation of the source terms of the species equations. Apart from the source terms, ISWS also governs the recalculation of the diagonal terms of the Jacobians of the source terms (which are used in the point implicit procedure). From Eq. 942 it can be seen that, after the update in the last stage, the residual is normally not recalculated any more. Strictly spoken however, within a multigrid approach, one should use in the calculation of the forcing function for the coarser level, Eq. 934, the residual corresponding to the latest solution. For single grid computations, recalculation is never done. Within multigrid, the RungeKutta operator can be applied more than once on each grid level, to ensure a better smoothing. The parameter "Number of sweeps on successive grid levels" give the number of times the RungeKutta operator has to be applied to each grid level during the finetocoarse  respectively the coarsetofine  part of the multigrid cycle. They can take different values on each grid level. Within the explicit RungeKutta approach, the source terms of the twoequation turbulence models and of the chemistry equations (nonequilibrium real gas) are treated in a point implicit way. For the kε equations the Jacobian of the negative part of the source term is diagonalized by assuming that the turbulent viscosity is approximately constant. This leads to the following relations between ρk and ρε : ρk = µ t ρε Cµfµ 2 . (952) ( ρk ) ρε = C µ f µ µt FINE™ 919 Theory Numerical Model For instance, for the Chien model, this results in the following diagonal terms of the Jacobian, including the compressibility corrections of Sarkar and of Nichols, cf. Eq. 475, on page 437, Eq. 477, on page 437:  ∂S k Cµ C p1 ( γ – 1 )Mk µ 1 2  Pk , = – 2  ρk ⎛ 1 +  αM t ⎞ – 2 2 – 2 2 ⎠ ∂ ( ρk ) 2 µt ⎝ ρka ρy (953)  ∂S ε C µ ρε 3 µ – 0.5y+ = –  C ε 2 f 2  – 2 2 e . 2 ∂ ( ρε ) µt y (954) Note that in the equations above the damping function f µ is not taken into account. 94.5 Implicit residual smoothing Implicit residual smoothing can be used in combination with RungeKutta to speed up the convergence to steady state. One stage in the explicit RungeKutta scheme Eq. 941 might be written: u m+1 n m n m = u + α m ∆tF ( u ) = u + α m R ( u ) (955) The residual R may then be smoothed first, before applying the update of Eq. 955. The smoothing may be obtained by applying a central type operator leading to a smoothed residual R˜ : with the operator ∆ i 2 2 2 ( I – ε i ∆ i ) ( I – ε j ∆ j ) ( I – ε k ∆ k )R˜ = R (956) 2 ∆ i R˜ = R˜ i – 1 – 2R˜ i + R˜ i + 1 (957) 2 and similar for the operators in the directions j and k. ε is a smoothing parameter on which the stability criterion is: 1 ε > 4 * 2 σ σ –1 , (958) * where σ , σ are the CFL numbers of the smoothed and unsmoothed RungeKutta scheme respectively. The result of the residual smoothing is thus that one can run at higher CFL numbers: choose * σ /σ > 1 and by an adapted choice of ε, according to Eq. 958, the scheme remains stable. Though * theoretically Eq. 958 guarantees stability for any value of σ /σ , in practice this is not the case. A * * good practical value is σ /σ =2. The parameter σ /σ is user input (RSMPAR). Different types of residual smoothing, corresponding to different definitions of ε are available. Each one corresponds to a different value of the input parameter IRSMCH. For IRSMCH = 1 the definition of Eq. 958 is used, with the restriction that ε should be positive. For higher values of IRSMCH, the definition of ε also takes the mesh aspect ratio into account. For IRSMCH = 2 one uses, after Radespiel & Rossow: 920 FINE™ Theory Numerical Model 1 ε i = 4 σ* 1 + max ( ( λ j * ⁄ λ i * ), ( λ k * ⁄ λ i * ) )  σ 1 + max ( λj * ⁄ λ i *, λ k * ⁄ λ i * ) 2 –1 , (959) with the spectral radius (scaled with the cell face area), e.g.: λ i * = [ ( un + c ) ⋅ S ] i . (960) A similar definition as Eq. 959 holds for ε in the directions j and k. For IRSMCH = 3, after Swanson & Turkel, one has: 1 ε i = 4 σ* 1  σ 1 + 0.0625 ⋅ ( ( λ j * ⁄ λ i * ) + ( λ k * ⁄ λi * ) ) 2 –1 (961) IRSMCH=4 is also after Swanson & Turkel but for viscous flows. First Eq. 961 is applied. Denoting the obtained value as ε*, the final value is: 10 ⋅ λ d 1 ] ε i = max [ε*, 4 λ i * + λj * + λ k * . (962) Finally, for IRSMCH = 5, one has, after Martinelli & Vatsa: 1 ε i = 4 FINE™ σ* 1 + ( λ j * ⁄ λ i * ) + ( λ k * ⁄ λ i * )  1 + λ j * ⁄ λi * + λ k * ⁄ λ i * σ 2 –1 . (963) 921 Numerical Model 922 Theory FINE™ CHAPTER 10:Initial Solution 101 Overview FINE™ provides the possibility to start a computation from an initial solution. The following initial solution types are available: • constant values, • from file, • for turbomachinery, • from throughflow. Each of these types is described in the next sections. FINE™ allows to define a different initial solution type for each block or group of blocks. Such a block dependent initial solution provides more flexibility in the restart of previously computed solutions. The next section describes how to set up a block dependent solution. 102 Block Dependent Initial Solution This procedure permits to initiate the calculation of some of the blocks with the results of a previous calculation, whereas the other blocks are started from a uniform flow. Another possibility is to initiate one new calculation with the results of several previous calculations. This is for instance the case if a multistage turbomachinery calculation is preceded by the calculation of the separate stages. The flow solver can start from files resulting from calculations performed on different grid levels. Only the grid levels that are used in the multigrid cycle are considered here. For instance, a computation of a threestage turbine can start from three solutions for each stage, each one on a different grid level. Furthermore, the full multigrid cycle is automatically removed when at least one file is provided on the finest grid level. FINE™ 101 Block Dependent Initial Solution Initial Solution 102.1 How to Define a Block Dependent Initial Solution The Initial Solution page is divided in two parts. On the left, a tree displays the structure of the groups of blocks. On the right, four buttons allow the user to choose the type of initial solution: constant values, turbomachinery oriented, restart from a solution file or restart from a throughflow file. At the bottom two buttons allow to modify the group(s). It is possible to create new groups of blocks in the same way as for the groups of patches on the boundary conditions page (see section 81). Different initial solutions can be assigned to these groups of blocks. By default, all the blocks are grouped in one group named "MESH" and constant values are selected. In the constant values page, the toggle button Cylindrical is set on. FIGURE 10.2.11Default settings of the initial solution page 102.2 Examples for the use of Block Dependent Initial Solution The block dependent initial solution is helpful in many industrial cases. The following are two scenarios in which this capability is very useful: 1. 102 A solution has been calculated for a turbine including 10 stages. A new stage is added. Now the turbine has 11 stages. The designer does not want to begin a computation from scratch for the turbine with 11 stages. He can take advantage of the solution that has been found for the 10 first stages. The new computation will contain one group with the 10 stages and one group with the last stage. The first group will be assigned to a from file initial solution and the second group can be assigned to another type of initial solution. FINE™ Initial Solution Defined by Constant Values 2. Initial Solution A turbine includes 10 stages. Even with the turbomachineryoriented initial solution, the code does not succeed to converge properly. The designer could split the turbine in several parts and calculate the solution for each of these parts. Then a global project is created. In the Initial Solution page, a from file initial solution is assigned to each part of the project. The computation will have a far better chance to succeed. 103 Initial Solution Defined by Constant Values When selecting on the Initial Solutions page constant values the user can modify the physical values used as initial solution on the page as shown in Figure 10.2.11. The physical values are uniformly used as initial solution all over the selected group of blocks, except on the boundaries. The variables for which initial values need to be specified are the static pressure, the static temperature, the velocity components and the turbulencebased variables k and ε, if a twoequation turbulence model is used. Note that the velocity components specified by the user are the Cartesian (cylindrical) ones for a Cartesian (cylindrical) case. The lower part of the page allows for a further control of the initial field. First, for both Cartesian and cylindrical projects, the velocity direction can be fitted along the I, J or K mesh lines. The reverse option determines whether the velocity vectors will point in the I (J or K) increasing or decreasing direction. By default, no specific velocity direction is set and the input box is set to “None”. For the cylindrical projects only, an option for the fitting method can be chosen. The first option fits Vm, the meridional velocity (defined as Vm = 2 2 V r + V z ), and uses Vθ to set the azimuthal absolute velocity. The second option fits W, the relative velocity, to the mesh lines. Furthermore, for the cylindrical projects only, it is also possible to act on the initial pressure field. To this end, two options are available: constant pressure field (default) and a radial equilibrium pressure gradient. In a rotational machinery for instance, a radial equilibrium pressure gradient is often closer to the physics than a constant field. The radial equilibrium factor allows to adjust the influence of the pressure gradient (its default value is 1.0). FINE™ 103 Initial Solution from File Initial Solution 104 Initial Solution from File 104.1 General Restart Procedure FIGURE 10.4.11Restarting from a file To continue on the result of a previous computation the user must simply select the solution. Clicking on the Open browser button will open a File Chooser window to select the ’.run’ (or ’.cgns’) file of a computation. To restart from a solution the computation definition file with extension ’.run’ is not sufficient. It is required that the solution file with extension ’.cgns’ is present, which contains all the saved and requested quantities. The toggle button Reset convergence history can be selected. When selecting this button the ’.res’ file, which contains all the residuals from the previous computation, will be erased. The new residuals will be calculated with respect to the first iteration of the new computation. If the from file solution is already very close to the exact solution, the normalized residuals will decrease slowly. It is just because the starting state is already a good approximation of the solution. When all the blocks are grouped in only one group, the user is able to unselect the button Reset convergence history. In this case, the new residuals are appended to the ’.res’ file and are calculated with respect to the first iteration of the old computation. If only one group of blocks exists the button to Reset convergence history can be set on or off. If several groups of blocks exist, the button is disabled and automatically the convergence history is reset. There is a limitation in the current version of the FINE™ interface: if the user wants to keep the convergence history, the ’.run’ file MUST belong to the active computation. The following steps 1. 104 Compute a solution. FINE™ Initial Solution from File 2. Create a new computation. 3. In this new computation, select a from file initial solution. Initial Solution are not compatible with the Reset convergence history option. Whatever the user selects, the toggle button Reset convergence history will be set ON automatically. If, for some reason, the user still wants to keep the convergence history in a new computation, the only workaround is to copy all the files from the old computation directory to the new computation directory and to rename them with the name of the new computation. Then the File Chooser will point to a ’.run’ file belonging to the active computation and the convergence history will not be reset. The initialization of the flow computation from a solution file is currently limited to CGNS files. As the initial pressure and temperature fields are block dependent, discontinuities in these quantities can be present at block connections and the flow solver could have difficulties to converge in that case. Therefore boundary conditions should be carefully checked in order to avoid any important discontinuity at block connections. The flow solver can start from files resulting from calculations performed on different grid levels. Only the grid levels that are used in the multigrid cycle are considered here. For instance, a computation of a threestage turbine on 0/0/0 with 3 grid levels can start from three solutions for each stage, each one on a different grid level (0/0/0, 1/1/1, and 2/2/2). Furthermore, the full multigrid cycle is automatically removed by the flow solver when at least one file is provided on the finest grid level. 104.2 Restart in Unsteady Computations To allow a second order restart for unsteady computations it is necessary to set in the Computation Steering/Control Variables page Multiple Files in the Output Files. This parameter allows to have multiple output files: for each saved time step also the solution of the previous time step is saved. To perform a second order restart for an unsteady computation select in the Initial Solution page from file. Using the File Chooser select the solution file with extension ’.cgns’ at a certain step (’_ti.cgns’). EURANUS will automatically find the solution of the previous time step if present (’_ti1.cgns’). If EURANUS can not find the solution of the previous time step a message will appear in the Task Manager to indicate that a first order restart will be performed. 104.3 Expert Parameters for an Initial Solution from File There is no current limitation to start a kε computation from a BaldwinLomax solution. In this case, the turbulent quantities are estimated from the friction velocity if the expert parameter INIKE is set to 2 (default value) or from the turbulent viscosity field µt if INIKE = 1. In the latter case, the turbulent viscosity is initialized or read from file depending on the value of the expert parameter IMTFIL (default value IMTFIL = 0 to initialized µt or IMTFIL = 2 to read µt from file). FINE™ 105 Initial Solution for Turbomachinery Initial Solution 105 Initial Solution for Turbomachinery This type of initial solution respects the inlet and outlet boundary conditions and assumes a constant rothalpy along the axisymmetric grid surfaces typical of the turbomachinery oriented meshes (e.g., created by AutoGrid). In addition, the velocity field is automatically aligned with the blade passages. When using the turbomachineryoriented initial solution, make sure that the INLET boundary condition is set in cylindrical mode and not in Cartesian mode. This last mode is not compatible with the turbomachinery initial solution in the present version. FIGURE 10.5.01Example of Turbomachineryoriented initial solution The turbomachineryoriented page displays two major panels: one for the inlet patches and one for the Rotor/Stator interfaces (see Figure 10.5.01). On the left of each panel, a tree shows the names of the patches. If no patch name has been given in IGG™, the default name will be a concatenation of the name of the block, the index of the face and the index of the patch. The Inlet Patches grouping displayed in this initial solution page is identical to the Inlet Patches grouping created under the INLET thumbnail of the Boundary Conditions page. Similarly, the Rotor/stator interface grouping displayed in the initial solution page is based on the ID given in the RotorStator thumbnail of the Configuration/Rotating Machinery page. There is no way to modify the groups of patches in the Initial Solution page. If the user wants to edit the groups of patches, the user must go back to the Boundary Conditions and the Rotating Machinery pages. An input dialog box is provided per group of patches in order to select the type of static pressure specification: constant distribution or radial equilibrium. One or two input boxes are provided per group of patches in order to define the static pressure value to be used and, if radial equilibrium is chosen, the radius on which this radial equilibrium will be based. Provided that a kε turbulence model is selected, a third panel is displayed that requires the initial values for the turbulent kinetic energy (k) and the turbulent dissipation rate (epsilon). For advice on the initial values to choose for k and epsilon see section 43.5.4. 106 Make sure that there is an inlet patch among the blocks for which a Turbomachinery initial solution has been chosen. If there is no inlet patch for the selected group of blocks, a warning message is displayed in the FINE™ interface asking the user either to edit the FINE™ Throughfloworiented Initial Solution Initial Solution group or to change the type of initial solution. 106 Throughfloworiented Initial Solution This type of initial solution, of interest in turbomachinery calculations, allows to get an initial field on the basis of an axisymmetric throughflow solution. The initial solution is defined through an external file created by the user. The file contains 2D data in the format described hereafter. The solver will use data to generate an initial throughfloworiented solution. Note that there is no direct link between the throughflow module integrated in the FINE™ interface and the format currently available. Work is in progress to make the bridge between both tools. The solver will create a virtual mesh based on the hub and shroud definitions, forcing points on the data points. Two additional stations will be created, at the inlet and outlet, respectively. The inlet data are extrapolated from the first spanwise station while the outlet data come from the last station. It is therefore recommended that the inlet and outlet boundaries of the mesh lie outside the meridional domain covered by the throughflow data. 106.1 The meridional velocity is based on the mesh direction. File Format The file will include three parts, that must be separated by a blank line: • solution definition, • hub definition, • shroud definition, Once it is created, the file is selected in the FINETM interface through a File Chooser click on the Open browser button in the Initial Solution/from throughflow page. 106.1.1 Solution Definition The first part of the file contains the values of the flow variables throughout a meridional structured mesh covering the entire machine. For each node of the meridional mesh, the (R,Z) coordinates are specified together with the pressure, temperature and velocity components. Here an axial case is taken as an example: Throughflow Axial Stator RZ 43 #Comment line #Type of data (ZR or RZ are accessible) #Number of spanwise and streamwise stations 0.246 0.025 150000 0 0 0 0.275 0.025 150000 0 0 0 1st spanwise section close to inlet at Z=0.025 0.29 0.025 150000 0 0 0 0.246 0.0 130000 0 0 0 0.275 0.0 130000 0 0 0 FINE™ 2nd spanwise section at Z=0.0 107 Throughfloworiented Initial Solution Initial Solution 0.29 0.0 130000 0 0 0 0.246 0.025 100000 0 0 0 3rd spanwise section at Z=0.025 0.275 0.025 100000 0 0 0 0.29 0.025 100000 0 0 0 0.246 0.05 90000 0 0 0 0.275 0.05 90000 0 0 0 4th spanwise section close to outlet at Z=0.05 0.29 0.05 90000 0 0 0 There are 4 spanwise stations in this example (Z=0.025, Z=0.0, Z=0.025 and Z=0.05), each with 3 points in spanwise direction (R direction). The point order in a streamwise and spanwise station goes respectively from hub to shroud and from inlet to outlet. Each data line is made of the two (R,Z) coordinates (in m), the static pressure (in Pa), the static temperature (in K), the meridional velocity and the tangential velocity (in m/s). 106.1.2 Hub Definition The hub definition uses the same format as for AutoGrid. The first line must be HUB. The second line specifies the type of coordinate (ZR or RZ) and the third line the number of hub points. The next lines correspond to the hub coordinates. Taking again the example of the case above: HUB RZ 2 0.245 0.02 0.245 0.051 #Type of data (ZR or RZ are accessible) #Number of points on hub #Point coordinates (in m) The hub is described in increasing Z coordinate from 0.02 to 0.051. The first column contains the R coordinate for each of the two points on the hub. 106.1.3 Shroud Definition The shroud definition is similar to the hub definition, except for the first line that will be replaced by SHROUD and the points coordinates. SHROUD RZ 2 0.3 0.02 0.3 0.051 108 #Type of data (ZR or RZ are accessible) #Number of points on hub #Point coordinates (in m) FINE™ Throughfloworiented Initial Solution Initial Solution Meridional Average View SHROUD BLADE 3D View 1st spanwise section 2nd spanwise section 3rd spanwise section INLET 4th spanwise section OUTLET HUB FIGURE 10.6.14 Throughfloworiented FINE™ Initial Solution 109 Initial Solution 1010 Throughfloworiented Initial Solution FINE™ CHAPTER 11:Output 111 Overview With the EURANUS flow solver in the FINE™ environment the user has the possibility to specify the content of the output generated by the solver. The output does not only contain the flow variables for which the equations are solved (density, pressure, velocity components), but also other variables such as the temperature, the total conditions, the Mach number, customized velocity projections, etc... Furthermore CFView™ allows to calculate derived quantities, which permits to limit the memory size of the output and to avoid relaunching the flow solver in case one quantity of interest is not available. With this functionality the user can find the compromise between an acceptable memory size for the output and the ease of having all flow quantities of interest immediately available for visualization. In the next sections the way to control the output from the EURANUS flow solver is described in more detail: • field quantities: calculated at all the mesh nodes (see section 112.1), • solid data: calculated along the solid wall boundaries (see section 112.1.5), • customized averaged data: — the evolution of some averaged quantities can be provided along the streamwise direction as described in section 112.2, — for turbomachinery applications, a pitchwise averaged output can be created for visualization as described in section 112.3, • global performance output (see section 112.5), • additional output for the ANSYS code, a widely used finite element code for structural analysis (see section 112.4). The global performance output is written in a ASCII file with the extension ’.mf’. All other output generated by the solver is written in one single ’.cgns’ file, compatible with the CFView™ visualisation software. It is also possible to request for the output to be written in Plot3D format as described in section 112.6. FINE™ 111 Output in FINE™ Output 112 Output in FINE™ 112.1 Computed Variables Using the Outputs/Computed Variables page, the user can choose which physical variables have to be included in the output generated by the flow solver EURANUS, see Figure 11.2.11 to Figure 11.2.16. All the selected variables will then be automatically available when launching CFView™ in order to visualize the results. 112.1.1 Thermodynamics n FIGURE 11.2.11 Thermodynamics computed variables page (for cylindrical projects) Table 111 and Table 112 give the formulae used to calculate the thermodynamic quantities. Quantity Static pressure Total pressure Cartesian and cylindrical cases Incompressible Compressible Pstat Pstat Static temperature Density Entropy Dynamic viscosity 2 2 V +k T tot = T stat + 2C p V +k T tot = T stat + 2C p ρ ρ T stat s = C p ln T statinlet µ TABLE 111 Thermodynamics 112 T tot γ – 1 Ptot = Pstat ⎛⎝ ⎞⎠ T stat P stat T stat = ρr gas T stat Total temperature γ  2 V +k Ptot = P stat + ρ 2 ( P stat ⁄ P statinlet ) s = C v ln γ ( ρ ⁄ ρ inlet ) µ quantities generated by EURANUS FINE™ Output in FINE™ Output Cylindrical cases only Compressible Incompressible Relative total pressure 2 r W +k P tot = Pstat + ρ 2 Relative total temperature r Ptot = 2 W +k r T tot = T stat + 2C p Rothalpy Pstat W 2 + k – ω 2 r 2 I = C p T stat +  + ρ 2 γ r γ–1 ⎛ T tot ⎞ P stat ⎜ ⎟ ⎝ T stat⎠ 2 r W +k T tot = T stat + 2Cp 2 2 2 W +k–ω r I = C p T stat + 2 ω is the angular rotation speed and r, the distance from the rotation axis TABLE 112 Thermodynamic quantities generated by EURANUS in cylindrical cases Furthermore five definitions of the pressure coefficient are available: CP1, CP*1, CP2, CP*2, CP3: 2 ( P – Pt ) inlet , — CP1 = 2 ρinlet U ref — Pt inlet – Pt , CP∗ 1 = Pt inlet 2( P – P ) inlet — CP2 = 2 , ρ inlet W inlet 2 ( Pt – Pt ) inlet , — CP∗ 2 = 2 ρ inlet W inlet 2( P – P ) inlet . — CP3 = 2 ρU where Xinlet corresponds to the mean value of the variable X on the inlet, and where Uref is defined as: • ω RLEN in cylindrical cases, with RLEN, the reference length given in the Flow Model page, and ω, the rotational speed (defined block per block), • UENTR (Cartesian case) to be specified in the expert parameters list of the Computational Steering/Control Variables page. When applying FINE™ to external flow situations (expert parameter IINT set to 0), only the quantity CP2 is welldefined. In external flows this pressure coefficient is defined in terms of the Reference values and Reynolds Number Related Info specified in FINE™ on the Flow Model page: 2 ( P – P ref ) CP2 = 2 ρ ref U ref . The user must then ensure that the far field or free stream quantities set on the Boundary Conditions page as well as the initial solution values (set on the Initial Solution page) are fully consistent with the reference values specified on the Flow Model page. FINE™ 113 Output in FINE™ Output Finally, when a condensable fluid is selected in the Fluid Model page, new quantities at the bottom of the page will appear. Those variables are defined using the thermodynamic tables defining the condensable gas (see section 32.3.4 for more details). When the condensable fluid option is used, 6 flow variables are stored at all mesh cell centers instead of 5 for a perfect gas or liquid. These variables are the following: density, velocity compo2 V 2 nents, static pressure and total energy ( ρE = ρ ⎛⎝ e + ⎞⎠ ). The static and total enthalpy can easily be derived using: • static enthalpy h = ⎛⎝ e + p⎞⎠ . ρ 2 V ⎞  . • absolute total enthalpy H a = ⎛⎝ h + ⎠ 2 2 ⎞ . • relative total enthalpy H r = ⎛⎝ h + W ⎠ 2 The dryness fraction permits to evaluate the location of the local thermodynamic state with respect to the saturation curve. For each value of the pressure an interpolation from the saturation table (’PSA.atab’) permits to determine the saturated liquid (ρl) and gas (ρv) values of the density. The dryness fraction is then computed by: ( ρ – ρl )ρv . • dryness fraction X = ( ρv – ρl )ρ The generalised dryness fraction directly results from the above expression whereas the standard dryness fraction is bounded in the [0,1] interval. It should be mentioned that the presence of the saturation table (’PSA.atab’) is required in order to allow the calculation of the dryness fraction, although this table is not required by the solver itself (unless an inlet boundary condition based on dryness fraction is used). 112.1.2 Velocities FIGURE 11.2.12 114 Velocities computed variables page (for cylindrical projects) FINE™ Output in FINE™ Output The velocity quantities that can be selected are described below. Both for Cartesian and cylindrical cases: • Absolute velocities: Vx, Vy, Vz, Vxyz, V. • Velocity projections: Vi, Vj, Vk, Vi, Vj, Vk,Vis,Vjs,Vks. · Vi = ⎛ V ⋅ Si⎞ ⋅ Si with Si , surface vector of the i surface, ⎝ ⎠ · Vis = V – ⎛⎝ V ⋅ Si⎞⎠ ⋅ Si . • Absolute Mach Number, only for compressible fluids: γP stat⎞ M abs = V ⁄ ⎛  . ⎝ ρ ⎠ For cylindrical projects only: • Absolute velocities in the rotating frame:V, Vr, Vθ, Vm: Vr = Vx cos θ + Vy sin θ , Vθ = Vy cos θ – V x sin θ , Vm = 2 2 Vr + Vz . • Relative velocities: Wx, WY, Wxyz, W, Wθ: W= V – ω × r , Wθ = Wy cos θ – W x sin θ . • Relative velocity projections: Wi, Wj, Wk, Wi, Wj, Wk, Wis, Wjs, Wks · Wi = ⎛⎝ W ⋅ Si⎞⎠ ⋅ Si with Si , surface vector and · Wis = W – ⎛ W ⋅ Si⎞ ⋅ Si . ⎝ ⎠ • Relative Mach Number: γPstat⎞  . M rel = W ⁄ ⎛⎝ ρ ⎠ 112.1.3 Vorticities FIGURE 11.2.13 Vorticities computed variables page The vorticity is calculated according to the following expression: FINE™ 115 Output in FINE™ Output ζ= ∇ × V , where ∇ is the gradient operator. From the above expression, ζx, ζy, ζz, ζxyz, and ζ are available. 112.1.4 Residuals FIGURE 11.2.14 Residuals computed variables page The residuals are computed in FINE™/Turbo by a flux balance (the sum of the fluxes on all the faces of each cell). The absolute value RES resulting from the flux balance is written as output for each cell. The residuals for the following quantities can be selected: • density ρ, • energy E, • velocity component Wx, • velocity component Wy, • velocity component Wz, • turbulent kinetic energy k for two equations turbulence models, • turbulent energy dissipation rate ε for two equations turbulence models. 112.1.5 Solid Data FIGURE 11.2.15 Solid data computed variables page The solid wall data refer to quantities that are estimated at the solid boundaries: • static pressure at walls (see section 112.1.1). • static temperature at walls (see section 112.1.1). τ • normalized tangential component C f = of the viscous stress at walls, where τ is the vis2 ρV ⁄ 2 cous stress, V is the reference velocity and ρ is the reference density defined in Flow Model page. • heat transfer at walls in general DT q w = K ⋅ Dn and for kε extended wall function q w = ρCpu τ T τ where u τ and T τ are coming from page 434. 116 FINE™ Output in FINE™ Output • relative velocity at walls (see section 112.1.2). • viscous stress τ xyz at walls. • y+ (in first inner cell). 112.1.6 Turbulence FIGURE 11.2.16 Turbulence computed variables page. The following quantities can be stored: • y+ (3D field) ρy wall u w y + =  , µ • wall distance (i.e. closest distance to the wall: ywall), • turbulent Viscosity (µt/µ), • production of kinetic energy (Production), • k and ε for two equation turbulence models. 112.1.7 Throughflow For the output specific for Throughflow computations see Chapter 6. 112.2 Surface Averaged Variables This option is customised for turbomachinery applications and displays in a Cartesian plot the evolution of surfaceaveraged variables along the streamwise direction. The user should select blocks along the streamwise direction. A surface averaging is performed on the grid surfaces perpendicular to the streamwise direction. Computation on each block will be performed to create the plot. The Surface Averaged Variables page is modified according to the type of project as defined in the Mesh/Properties... menu. For a Cylindrical project the page looks like shown in Figure 11.2.27. In this case the streamwise direction (by default K) is defined on the Rotating Machinery page of the FINE™ interface. The blocks to include in the averaging can be selected from the list of blocks by leftclicking on them. Selected blocks appear highlighted. This selection acts as a toggle where clicking ones on a block name selects the block and clicking a second time deselects the block. To select multiple blocks it is sufficient to leftclick on each of them. The variables available for averaging are listed on this page and a averaging method can be selected for each variable independently. The turbulent quantities k and ε only appear for selection if a twoequations turbulence model is used. FINE™ 117 Output in FINE™ Output FIGURE 11.2.27 Surface averaged variables page for a Cylindrical project Since the integration is performed on mesh surfaces, some differences could appear. For example, in a case with splitter, two curves will be generated and a sum on this curve should be performed to see the evolution of the quantity in streamwise direction of one channel. Since the surface averaging is performed on grid surfaces this option is mainly suitable for Htopology meshes. Especially computing the evolution of the mass flow in streamwise direction with HOH mesh topology is not correct. For Cartesian projects as defined in the Mesh/Properties... menu the Surface Averaged Variables page is displayed as shown in Figure 11.2.28. In this case the streamwise direction needs to be selected directly in this page by selecting to average on surfaces of constant index (in the example of Figure 11.2.28 surfaces of constant k). The blocks to include in the averaging need to be selected in the same way as for a cylindrical case as described before. Contrary to a cylindrical project, in this case no relative quantities are available. 118 Like for a cylindrical project the surface averaged evolution of the quantities is shown for each block separately. FINE™ Output in FINE™ Output FIGURE 11.2.28 Surface averaged variables page for a Cartesian projects 112.3 Azimuthal Averaged Variables The FINE™/Turbo environment provides the user with a specific turbomachinery output, i.e. the twodimensional meridional view of the circumferentiallyaveraged results. Note that this functionality is also available in CFView™. Using the Azimuthal Averaged Variables page, the user can choose which physical variables have to be included in the pitchwiseaveraged output generated by the flow solver. This page is therefore only accessible if the project is of the cylindrical type. The azimuthal averaging of the variables is calculated at the end of the computation. The results will be displayed as a 2D case in CFView™. The name of the file from which CFView™ can read which variables have been averaged in the azimuthal direction has the extension .me.cfv. The choice is left to the user to apply mass or area averaging, and to merge into one patch the averaging patches. This last option (Merging of meridional patches) simplifies the meridional view but the patches are merged in increasing order one after another, which is not suitable for all topologies. If Surface of revolution mesh (Autogrid) option is activated, a specific algorithm will be applied to enhance azimuthal averaging of the solution performed on revolution surfaces. The Parameters area is divided into five ’notebook pages’ which can be selected by clicking on one of the five corresponding thumbnails: Thermodynamics, Velocities, Vorticities, Residuals and Turbulence in the same way as for the control variables. Figure 11.2.39 shows an example of the corresponding information page for thermodynamics variables. Other pages are similar to those described in section 112.1. At the bottom of Figure 11.2.39 in expert mode the user can define the meridional patches for azimuthal averaging. See section 113.1 for more detail on this possibility. By default meridional averaging patches are set. FINE™ Automatic setting of the meridional averaging patches only works if no manual action is involved (like renaming of some patches). 119 Output in FINE™ Output FIGURE 11.2.39The thermodynamics azimuthal averaged variables page 112.4 ANSYS The FINE™/Turbo environment provides the user with a specific ANSYS output. The objective is to export results of the CFD computation on solid surfaces (nodes and elements) into ANSYS as a boundary condition for the finite element model. This approach is called FEM loading method for loading the CFD results on a Finite Element Model. The transferred results on the interface fluidstructure can be the pressure field for a structural analysis and the temperature field or the heat fluxes for a thermal analysis in the structure. 1110 The FEM approach needs to have the finite element mesh of ANSYS. If this mesh does not exist before the CFD computation, it is impossible to create directly a file that can be imported in ANSYS to apply the suitable boundary condition. Consequently the best way to manage the interface between FINE/TURBO and ANSYS can be a new postprocessing tool. The postprocessing tool is needed with the specification of the ANSYS mesh, the common surfaces where the data must be interpolated and the type of boundary condition on each surface. The transfer will be carried out through the ANSYS file saved with the command CDWRITE ("project_ANSYS.cdb") in ANSYS. This file will be modified and read again in ANSYS to impose the CFD results as boundary conditions (see Figure 11.2.410). FINE™ Output in FINE™ Output FIGURE 11.2.410Data transfer of CFD results into the ANSYS project 112.4.1 ANSYS PreProcessing Before completing the Outputs/ANSYS pages, the user must create the file ’project_ANSYS.cdb’ with the command CDWRITE in ANSYS. Furthermore before the save in ANSYS, some operations needs to allow the identification of the common surface between the fluid model and the structural model. The ANSYS project must be completely defined with a special treatment for the surface loads that will be replaced by the interpolated CFD results. On each common surface, a coded constant value is specified. The default coded values are given in the table 113 for the different types of boundary condition. The value is incremented by one for each different surface so that for example the pressure imposed on the first surface is set to 1000001 and it is set to 1000002 on the second, ... Boundary Condition Code Pressure field 1000001 Temperature field 2000001 Temperature field for heat 3000001 flux by convection Heat flux 4000001 TABLE 113 Default code for different type of boundary condition imposed from CFD results FINE™ The coded value can be modified in order to avoid confusion with physical values. Note that the surface must be relatively flat or smooth (without sharp angle) so that the six surfaces define a cube. Moreover the surface closed on itself as a cylinder or a blade must be divided into two parts. Validation tests are performed with ANSYS release v8.0. Please refer to ANSYS user manual for more details on the ’.cdb’ file format 1111 Output in FINE™ Output 112.4.2 Global Parameters The user can complete the Outputs/ANSYS pages when the file ’project_ANSYS.cdb’ has been created (refer to section 112.4.1 for more details). (1) (2) (3) (4) (5) FIGURE 11.2.411General Parameters of ANSYS outputs Firstly, the user needs to specify under the thumbnail Global Parameters in Boundary Conditions (Figure 11.2.411  (1)) the coded constant value used in the file ’project_ANSYS.cdb’. The default coded values are given in the table 113 for the different types of boundary condition. Furthermore, the user has to specify the required units of the data for each type of boundary condition. The units will be specified next to the coded value. Then, the user needs to load the file ’project_ANSYS.cdb’ (Figure 11.2.411  (2)) created in ANSYS (refer to section 112.4.1 for more details) in Input File. The data transfer between the CFD mesh and the structural mesh is possible if the common geometries are matching. It is possible that this condition is not fulfilled and the causes can be diverse. • the units: a first difference can come from the units of the meshes. Consequently the units used in the ANSYS mesh must be specified in ANSYS Mesh Units. The conversion Factor will be deduced automatically (Figure 11.2.411  (3)). • the coordinate system: the second cause of mismatching is the use of different coordinate systems (Figure 11.2.411  (3)). For example, the original geometry can be only rotated for the CFD model so that the axial direction corresponds to the Z axis. The necessary change of coordinate will be done through the specification of the position of the coordinate center of the ANSYS mesh in the coordinate system of the CFD mesh and the specification of the location of three common points in both meshes in Reference System. 1112 Note that these points cannot be located on a line or a plane including the zero point (not linearly dependent). The coordinates are specified in their respective units. FINE™ Output in FINE™ Output The origin of the ANSYS mesh should be at (0,0,0). Finally in Output File, the user specifies the new output file ’project_CFD.cdb’ (Figure 11.2.411 (4)) containing the transferred CFD results on the solid boundaries coded in ANSYS (refer to section 112.4.1 for more details). In order to create the new output file, the user has to complete the page under the Surface Selection thumbnail before clicking on the Create Output File button (Figure 11.2.411  (5)). 112.4.3 Surface Selection After completion of the page under Global Parameters thumbnail, the user can complete the page under Surface Selection page (refer to section 112.4.2 for more details) before creating the ANSYS output file. When the ANSYS input file is read in Input File, the common surfaces where data must be transferred are identified in the ANSYS mesh. The interface FINE™ lists each surface with the corresponding coded value (Figure 11.2.412  (1)). For each detected surface of the structural ANSYS mesh, by clicking on Selected Surface Properties button (Figure 11.2.412  (2)), a new window (Figure 11.2.413) allows the user to specify the solid patches from which the data will be interpolated and some interpolation parameters: interpolation type (Interp Type) and the allowed maximal distance (Max Dist). (1) (3) (4) (2) FIGURE 11.2.412Surface FINE™ Selection of ANSYS outputs 1113 Output in FINE™ Output Two different interpolation types (Interp Type) are proposed: a conservative and a nonconservative. The suitable interpolation scheme is dependent on the type of boundary conditions. The spatial field of pressure or temperature can be interpolated from cell faces to nodes whereas a conservative transfer of the heat fluxes can be preferred. An allowed maximal distance (Max Dist) can be used to control the interpolation process by ensuring that it is performed in the nearest element of the selected solid CFD patches. FIGURE 11.2.413Add Solid Patches to ANSYS surface Then, the user specifies the solid CFD patches in the list of Solid Patches by or and leftclick. To add or remove solid patches linked to the highlighted ANSYS surface, the buttons Add Selection and Remove Selected are respectively used. When the solid patches are well selected, the window has to be closed (Close) and the patches will appear in the list Selected Solid Patches and Groups (Figure 11.2.412  (3)). Note that the ANSYS surface must be completely overlapped by the selected IGG solid patches in order to ensure a complete data transfer. The area of the selected IGG solid patches can be larger than the area of the ANSYS surface. Since the IGG™ solid patches defining a periodic structure can be divided (Figure 11.2.414), a periodic shift can be required to match the common ANSYS surface. This shift must be specified for each solid patch, highlighted in Selected Solid Patches and Groups list, in Periodicity by activating Rotation and Translation (Figure 11.2.412(4)). The rotation and translation shifts are respectively specified degrees and IGG™ units mesh. FIGURE 11.2.414Mesh 1114 differences IGG™ vs. ANSYS FINE™ Output in FINE™ Output Moreover one ANSYS surface can be covered by a group of solid patches and by the same group rotated (or translated). Consequently, a duplication of the periodic solid patches is possible by activating Duplicate patch(es) after applying a Rotation and Translation to the highlighted solid patch (Figure 11.2.412(4)). FIGURE 11.2.415Duplicate Option Utility Finally, the new output file can be created by clicking on the Create Output File button (Figure 11.2.411  (5)). 112.5 Global Performance Output The main results for global performance are summed up in a file with extension ’.mf’. Inlet and outlet averaged quantities, pressure ratios and efficiency are computed and stored in this file. The user can select which and what kind of information is stored using expert parameters as described in section 113.2. In this section the default contents of the global performance output is described. 112.5.1 Solid Boundary Characteristics This part of the file gives the characteristics of the quantities that are estimated at the solid boundaries. Those quantities are inferred from the global force F = Fpressure + Fviscous exerted by the flow at a given point. This force can be estimated from the pressure and velocity fields at each point. The calculated quantities for an internal configuration are: • Axial thrust, i.e. the projection of the global force on the rotation axis: ∑ F ⋅ nz . S • The projection of the torque along a given direction z , i.e. the couple exerted by the global force ⎛ ⎜ ⎝ ⎞ ∑ r × F⎟⎠ ⋅ z along direction z . This direction is given through the expert parameter S IDCMP, the default value of which is (0,0,1). For external flow configurations the expert parameter IINT must be set to 0 and the output file will contain the quantities as described in section 113.2 instead of the axial thrust and the torque FINE™ 1115 Output in FINE™ Output 112.5.2 Global Performance EFFDEF Compressors 1 p η is t2⎞ ⎛ ⎝p ⎠ γ–1 γ –1 t1 = T t2 –1 T t1 2 p 2⎞ ⎛ ⎝p ⎠ p t2 >p t1 η pol η is p γ ⎛ 2⎞ –1 ⎝p ⎠ 1 = T 2 – 1 T1 ln ⎛ 2⎞ ⎝p ⎠ R t1  η is η pol =  ⋅ cp T 2 ln ⎛ ⎞ ⎝T ⎠ t1 γ–1  TABLE 114 Isentropic T t2 p 1 – ln ⎛ t2⎞ T t1 ⎝p ⎠ R t1 η = γ– 1=  ⋅  is cp T t2⎞ p t2⎞ γ ⎛ ln ⎛ 1 – ⎝T ⎠ ⎝p ⎠ t1 p η is p t2 p t1 is p t2
p t1 Turbines p t2
0 α<0 V RPM (<0) z FIGURE 12.5.112 Coordinate system and reference for flow angles and speed of rotation In a 2D case, if the ZTR coordinate system is used, the radius does not have to be specified in the blade geometry input file. The number of columns can be 2 or 3, the third column being not read by the solver (the radius is automatically set to the value given in the streamsurface data input file). The suction side is by convention located above the pressure side in the θdirection Figure 12.5.112. It does not necessarily have to be the physical suction side. 125.2 Output Files Several output files are generated by the bladetoblade module: 125.2.1 Geometry Files a) ’project_computationname.geoini’ and ’project_computationname.geo’ These files contain the blade shape in the (m,θ) plane. The ’.geoini’ file contains the initial blade shape as given in the input files (or resulting from the 3D interpolation process in a 3D case), whereas the ’.geo’ file contains the blade discretization points used in the computation. These files can be read and plotted by the NUMECA MonitorTurbo (Blade profile menu). b) ’project_computationname.merdat’, ’project_computationname.mer.ori’ and ’project_computationname.mer’ These files contain respectively the hub and shroud walls and the streamtube projection onto the meridional plane. The ’.merdat’ file contains the hub and shroud walls (3D case only), whereas the ’.mer’ and ’.mer.ori’ files contain the streamtube. These files can be read and plotted by the NUMECA MonitorTurbo (Blade profile menu). c) ’project_computationname.ps.ori’ & ’project_computationname.ss.ori’ These files contain respectively the pressure side and the suction side of the blade. FINE™ 1215 File Formats used by BladetoBlade Module Blade to Blade Module d) ’project_computationname.split.ps.ori’ & ’project_computationname.split.ss.ori’ (if splitter blades) These files contain respectively the pressure side and the suction side of the splitter blade. 125.2.2 Quantity Files a) ’project_computationname.cgns’ This file contains the results of the calculation, i.e. the five flow variables (density, xyz components of the relative velocity and the static pressure) at all the mesh cell centers (including the dummy cells generated by the boundary conditions). It also contains all output variables to be displayed by CFView™. b) ’project_computationname.mf’ This file is a summary file containing the averaged flow quantities at the inlet and the outlet boundaries. c) ’project_computationname.mfedge’ This file is a summary file containing the averaged flow quantities at the leading and trailing edge planes. d) ’project_computationname.2d.cfv’ & ’project_computationname.3d.cfv’ The bladetoblade module automatically creates all the files required by the NUMECA CFView™ postprocessing tool. Two projects are created, the first one being named ’***.3d.cfv’, allowing a 3D visualization of the case, the second one being named ’***.2d.cfv’, allowing a 2D visualization in the (m,θ) plane. e) ’project_computationname.velini’ & ’project_computationname.vel’ These files contain the isentropic Mach number and the pressure coefficient distributions along the blade surfaces. The two quantities are plotted along the curvilinear abscissae measured along the blade surface (nondimensionalized by the blade chord). The isentropic Mach number is calculated (for compressible flows only) using the inlet relative total temperature and pressure, which are not necessarily imposed (depending on the choice of the inlet boundary condition). In case the total conditions are not imposed, the values are the ones resulting from the calculation (average along the inlet boundary). Mis = ⎛ p 2  ⎜ ⎛ 0⎞ ⎜ ⎝ γ – 1 p⎠ γ–1 γ ⎝ ⎞ – 1⎟ , ⎟ ⎠ (122) where p is the local static pressure, and p0 is the local relative total pressure calculated assuming a constant rothalpy and a constant entropy in the field. The pressure coefficient is defined by: p – p exit Cp =  , p exit (123) where pexit is the exit static pressure, and p is the local static pressure. 1216 FINE™ File Formats used by BladetoBlade Module Blade to Blade Module These files can be read and plotted by the NUMECA MonitorTurbo (Loading diagram menu). The ’.velini’ file contains the initial distributions, whereas the ’.vel’ contains the actual ones, and is iteratively updated during the resolution process. f) ’project_computationname.split.velini’ & ’project_computationname.split.vel’ (if splitter blades) These files contain the isentropic Mach number and the pressure coefficient distributions along the splitter blades. These files can be read and plotted by the NUMECA MonitorTurbo (Loading diagram menu). g) The ’project_computationname.loadini’ & ’project_computationname.load’ Provided that the parameter ISQUEL specified in the ’.run’ file is different from 0, these files are automatically generated, and contain the distributions of the suctiontopressure side Mach number and pressure coefficient difference and average. These distributions can be superimposed to the suction and pressure side distributions. These files can be read and plotted by the NUMECA MonitorTurbo provided with the FINE™ user interface (Loading diagram menu). The ’.loadini’ file contains the initial distributions, whereas the ’.load’ contains the actual ones, and is iteratively updated during the resolution process. h) ’project_computationname.split.loadini’ & ’project_computationname.split.load’ (if splitter blades) These files contain the same results as the ’.load’ and ’.loadini’ files along the splitter blades. These files can be read and plotted by the NUMECA MonitorTurbo provided with the FINE™ user interface (Loading diagram menu). 125.2.3 Numerical Control Files a) ’project_computationname.log’ & project_computationname.std’ These files contain all the informations written by the solver during its execution. When the solver fails for any accidental reason, the explanation can usually be found in these files. b) ’project_computationname.res’ This file contains the evolution of the mean and maximum residuals and of the inlet and outlet mass flows. This file can be read and plotted by the NUMECA MonitorTurbo (Convergence history menu). FINE™ 1217 Blade to Blade Module 1218 File Formats used by BladetoBlade Module FINE™ CHAPTER 13:Design 2D Module 131 Overview This chapter describes the new quasithreedimensional FINE™/Design 2D Module for turbomachinery cascade inverse design. This module is associated with the FINE™/Design 2D BladetoBlade module presented in Chapter 12. In addition to the mesh generator and the flow solver, the FINE™/Design 2D module includes one of the latest inverse methods for the redesign of the blades with improved performance. Such a method permits to redesign the blade shape for a target pressure distribution along the blade surfaces. The use of the design method requires a license for bladetoblade simulation. The FINE™/Design 2D module can be used (and acquired) independently from the other NUMECA tools. In the near future NUMECA intends to extend the FINE™/Design 2D environment to other types of applications and to other design techniques. This first version is limited to the inverse design of turbomachinery cascades, and has therefore been integrated with the BladetoBlade method in the FINE™/Design 2D user environment. Both analysis and design modules are based on the assumption that the flow in the turbomachinery cascade remains on an axisymmetric streamsurface. The geometrical inputs required from the user to perform an inverse design are not different from the ones required to perform an analysis (as described in Chapter 12). For more information about the BladetoBlade method, see the description provided in the Chapter 12. In the next section the interface is described in detail including advice for use of the inverse design method. The theoretical background for the inverse method is described in section 133. Finally, the Design 2D Module requires geometrical data files and generates output as detailed in section 134. FINE™ 131 Inverse Design in the FINE™ Interface Design 2D Module 132 Inverse Design in the FINE™ Interface The Blade Design module is proposed under the new NUMECA FINE™/Design 2D environment presented in Chapter 12, which permits a very rapid, easy and interactive use of the solvers. All the parameters can be selected interactively by means of this user interface, which automatically creates the input files and permits to launch the analysis and inverse solvers. A graphical control software, called MonitorTurbo, is provided. It permits to observe the evolution of the convergence history, of the pressure distribution along the blade surface, and of the blade geometry (case of an inverse design). It also permits to create the target pressure distribution interactively. The results can be analysed with the NUMECA CFView™ postprocessing software, whose connection with the bladetoblade module is automatically provided. The geometrical data are specified in ASCII input files, whereas the definition of the flow solver parameters and of the boundary conditions are specified via the interface. This section describes the creation of the inverse design input files using the interactive menus provided in FINE™/Design 2D. Further details concerning the input and output files are provided in section 134. The next sections provide information concerning: • The starting of a new or an existing bladetoblade project. • The creation of the solver input files required for a flow analysis. • The launching of a bladetoblade flow analysis. 132.1 Start New or Open Existing Design 2D Project To start the FINE™/Design 2D module from the FINE™ interface select the menu item Modules/ Design 2D. When launching the FINE™ interface a Project Selection window allows to Create a New Project or to Open an Existing Project. To create a new BladetoBlade project: 1. Click on the button Create a New Project. 2. Browse to the directory in which the new project directory needs to be created and enter a name for the project. 3. Close the Grid File Selection window since no grid file is associated to a Design 2D project. 4. Switch to the Design 2D module through the menu Modules/Design 2D. When an existing Design 2D project should be opened click on the button Open an Existing Project in the Project Selection window and select the project in the File Chooser window. The most recently used projects can also be selected from the list of recent projects. If the selected project was saved in the Design 2D module, the FINE™ interface is automatically switched to this module showing the interface as in Figure 12.2.11. It is not possible to have Design 2D and threedimensional computations in one project. A project is either a FINE™/Design 2D project or a FINE™/Turbo project. The type of the project is determined by the module in which it is saved. The interface in the Design 2D module is described in Chapter 12. The only difference with a bladetoblade analysis computation is the use of the Inverse Design page. This page is described in more detail in the next sections. 132 FINE™ Inverse Design in the FINE™ Interface Design 2D Module 132.2 Creation of Inverse Design Input Files An inverse design calculation should always start from the converged flow analysis of the initial geometry. Once a converged flow solution for the bladetoblade analysis has been obtained, the user can proceed with a modification of the blade using the inverse method. For this purpose the two input files "project_computationname.req" and "project_computationname.run" have to be prepared, in addition to the files required for the analysis ("project_computationname.run" and the geometrical input files). 132.2.1 Recommendations It is often useful to save the results obtained after the analysis computation. Therefore it is recommended to perform the inverse design in a new computation. With the analysis computation selected in the Computations area on the top left of the FINE™ interface click on the New button. A new computation is created with the same parameters as the initial computation. The Rename button may be used to rename the new computation. analysis inverse design FIGURE 13.2.22 Computations area The expert integer parameter IATFRZ is usually set to 2 during the inverse design procedure in order to freeze the computation of the turbulent viscosity. The consequence of this is to drastically reduce the computational time per inverse design iteration. 132.2.3 The Input File "project_computationname.req" The ’project_computationname.req’ file has exactly the same format as the ".vel" or ".load" output files automatically generated by the bladetoblade analysis module. The most appropriate way to generate this file is to modify the ’projectname.b2b.vel’ or ’projectname.b2b.load’ file resulting from the flow analysis of the initial geometry, using the MonitorTurbo. In order to create a target with the MonitorTurbo, the following operations should be made: FINE™ 1. Start the ’MonitorTurbo’. 2. Select the "Loading diagram" menu. 3. Open the ’project_computationname.vel’ or ’project_computationname.load’ file. 4. Choose between the ’Mis’ or ’Cp’ distributions (in case the inlet total conditions are not imposed as boundary conditions, the inverse problem has to be formulated in terms of Cp). The definition of Mis and Cp are provided in Eq. 131 and Eq. 132 presented in section 134. 5. Activate the ’Markers’ to distinguish the discretization points. 6. Activate the Edit a curve button. 7. Choose the suction or the pressure side curve, by placing the cursor on the corresponding legend, and typing
to select. The activated curve changes color. 133 Inverse Design in the FINE™ Interface Design 2D Module 8. Modify the curve using the middle button of the mouse: a. Choose the left point where the modification will start (click on the middle button). b. Choose the right point where the modification will end (click on the middle button). c. Choose control points between the left and the right points (click on the middle button). d. Displace the control points. — Select the control point by placing the cursor on the point. — Presson the keyboard, and displace the point vertically. The exact position of the point can be specified by pressing the right button of the mouse. e. Save the new curve by clicking on the Save button, and giving the name of the new curve, or cancel the modifications by clicking on the Cancel button. At any moment, a zoom of the curves can be obtained by defining a new rectangular window, using the left button of the mouse. The previous unzoomed view can be retrieved by pressing the right button of the mouse. 132.2.4 Input File "project_computationname.run" The "project_computationname.run" input file is created via the Inverse design page included in the FINE™/Design 2D interface (Figure 13.2.21). One of the three possible inverse formulations should be chosen: • Pressure and suction side distributions or classical formulation: both suction and pressure sides of the blade are modified for an imposed pressure distribution along the whole blade contour. If this formulation is used the profile closure constraint has to be activated. • Suction side distribution or mixed formulation: only the suction side is modified for a prescribed suction side pressure distribution. The profile closure conditions should also be activated, so that the pressure side follows the suction side modifications. • Blade loading or loading formulation: the camber line of the blade is modified for a prescribed loading (suctiontopressure side pressure difference) distribution from the leading to the trailing edge. The blade thickness distribution is maintained constant and therefore the profile closure condition does not need to be used. The target of the inverse design computation may either be constructed in terms of isentropic Mach number (Mis) or pressure coefficient (Cp) (see Eq. 131 and Eq. 132 in section 134). The isentropic Mach number formulation is limited to compressible flows. Control of the leading and trailing edges is provided. The inverse method permits to maintain some parts of the blade unchanged, such as the leading and trailing edge regions. The number of frozen points along the suction and the pressure sides should be specified for each edge by the user. The default value is 1. However in many cases it is recommended to freeze the leading edge region where no modification is imposed. At the trailing edge it is highly recommended to freeze the regions where a flow separation appears in the analysis of the initial blade. Two relaxation factors are available: • The first relaxation factor (default value = 1.0) permits to consider an intermediate target between the one present in the ".req" file and the initial distribution present in the ".vel" file. This factor is not often used. • The second relaxation factor (default value = 0.05) permits to underrelax the geometry modifications. The range of variation of this factor is from 0.01 to 0.1. Higher values than 0.1 are not recommended for reasons of stability, whereas lower values than 0.01 usually mean that the inverse problem can not be treated. 134 FINE™ Inverse Design in the FINE™ Interface Design 2D Module The following geometry constraints are available: • the profile closure constraint should always be used, unless: — the blade thickness is automatically controlled ("loading" formulation). — the trailing edge of the blade is blunt, and the trailing edge thickness does not need to be maintained. • Constant stagger angle is not often used. • Constant blade chord: this constraint permits to maintain the blade chord (measured on the transformed mθ plane). This constraint should not be used together with the constant radius option, as the two constraints are contradictory. • Constant radius: this option is recommended for radial machines, as it permits to guarantee an unchanged meridional position of the leading and trailing edges. The points are displaced along the circumferential direction. This option is not recommended for large rounded leading edges. • Reference point: the fixed reference point can be either the leading edge (by default) or the trailing edge (if the corresponding button is selected). FIGURE 13.2.21 Inverse design page Finally, the number of iterations performed for the inverse design calculation. 132.3 Initial Solution Menu An inverse design calculation should always start from the converged flow analysis of the initial geometry. Once a converged flow solution for the bladetoblade analysis has been obtained, the user can proceed with a modification of the blade using the inverse method. (Figure 13.2.32) FINE™ 135 Inverse Design in the FINE™ Interface Design 2D Module FIGURE 13.2.32 Initial solution page 132.4 Launch or Restart Inverse Design Calculation Once the ’.req’ and ’.run’ input files have been correctly created, an inverse design can be started, by selecting the Inverse design option in the "run type" parameter included in the Control Variables page, and by pressing the Start button in the Solver menu. FIGURE 13.2.43 Run type page of the information area Exactly as in the case of the restart of a flow analysis the user has to specify the name of the initial solution file. It is recommended to save the results of the flow analysis under a different name, so that several inverse design calculations can be performed successively, starting from the same initial solution. An interrupted inverse design calculation can be "restarted". For this purpose the user should set the expert parameter INVMOD to 1 instead of 0. This implies that in addition to the correct flow solution file, the actual blade geometry will be read by the solver and considered as the initial one. 132.5 Expert Parameters 132.5.1 Using a Parametrised Target Distribution Using a parametrised target distribution is possible through the two expert parameters IADAPT and RADAPT, that can be accessed via the Control variables page. The expert mode must be activated in the top right corner of the interface. The integer variable IADAPT contains 6 values: • Type of parametrisation — 0: parametrised distribution is not used — 1: suction side (or loading) distribution is parametrised — 2: pressure side distribution is parametrised. 136 FINE™ Theory Design 2D Module • Number of iterations after which the adaptation process will start. • Index of starting (left) point of the parametrised target. The user specifies the position with respect to the leading edge (typically about 10 points). • Index of the ending (right) point of the parametrised target. The user specifies its position with respect to the trailing edge (typically about 10 points). • Turning angle is imposed value (0) or the change of swirl RVθ between inlet and outlet (1). • Imposed turning or swirl is taken from the analysis solution (0) or set by the user (1). The real variable RADAPT contains 4 values: • Reduced curvilinear position of the free parameter between 0. (left point) and 1.0 (right point (default: 0.5). • Relaxation factor governing the amplitude of successive updates of the parameter (default: 0.25) • Range of variation of the free parameter (in isentropic Mach number or pressure coefficient, depending on previous choice of the user) (default: 0.2). • User imposed value of the turning angle (in deg.) or swirl RVθ (m2/s) (used if the last integer of IADAPT is set to 1). INVMOD: set this parameter from 0 to 1 to allow the restart of an inverse design computation. 132.5.2 Splitter Blades Design Centrifugal compressors with splitters can be redesigned with FINE™/Design 2D. It is possible to modify either the main blades or the splitter blades. The choice is made through the expert variable INVSPL (accessed in the "Computation Steering" menu of the FINE™ interface): • INVSPL= 1: main blades are modified • INVSPL= 2: splitter blades are modified The target should be constructed from the ’project_computationname.vel’ or ’project_computationname.load’ files if the main blades are modified, or from the ’project_computationname.split.vel’ or ’project_computationname.split.load’ files if the splitter blades are modified. 133 Theory The purpose of an inverse method is to redesign the blade shape in order to obtain a prescribed pressure distribution along the blade surfaces. This provides a detailed control of the boundary layer behaviour, by limiting the amount of diffusion and by eliminating the eventual spurious acceleration and deceleration detected along the initial blade profile. Such a method also offers an indirect control of the secondary losses, as a control of the blade loading distribution can be obtained. The inverse design method adopted in FINE™/Design 2D consists of modifying iteratively the blade geometry, until a target pressure distribution is reached on the blade surfaces. The geometry modification algorithm is based on the permeable wall concept. Each iteration of the process is composed of 2 separate steps, respectively related to the geometry and to the flow field updates. Both viscous and inviscid problems can be treated with this approach. Three formulations of the inverse problem are possible: FINE™ 137 Design 2D Module File Formats used for 2D Inverse Design • the classical formulation, in which both suction and pressure sides are redesigned in order to obtain a pressure distribution prescribed along the whole blade surface. • the mixed formulation, in which the suction side is redesigned in order to obtain a pressure distribution specified along the suction side only. This formulation is for instance interesting for rotor blades on which strict mechanical constraints are imposed. In those cases the classical inverse formulation may be less efficient because the blade thickness is a result of the calculation, and it is often difficult and time consuming to find an appropriate target leading to a blade with an acceptable thickness distribution. • the loading formulation, in which the distribution of blade loading (pressuretosuction side pressure difference) from the leading to the trailing edge is prescribed, and in which the camber line of the blade is redesigned (the blade thickness distribution being kept unchanged). This approach is interesting especially for radial machines. This is due to the fact that in radial machines, the average velocity level in the blade channel is mainly controlled by the shape of the hub and shroud endwalls, and therefore a modification of the blade shape mainly influences the loading distribution. The "loading" formulation is therefore more appropriate and efficient for radial machines. However no general rule can be set, and improvements can be reached in many cases using the second formulation. Several geometrical constraints and options have been implemented, to increase the flexibility of the method: • Control of the leading and trailing edges: several points can be kept unchanged in the leading/ trailing edge regions. • Constant blade chord. • Specification of the fixed reference point (leading or trailing edge). • Inverse problem formulated in terms of isentropic Mach number or of pressure coefficient. • Constant meridional position of leading and trailing edges (recommended for radial machines): with this option, the points are displaced along the circumferential direction, which guarantees that their meridional position is unchanged. An important advantage of the present method is the possibility to control the outlet flow angle or swirl. A major drawback of most inverse methods is the lack of control of the turning angle or work exchange in the cascade. The user does not have the guarantee that the specified target pressure distribution will lead to an unchanged turning angle. This implies that several iterations are sometimes required before finding the target leading to an acceptable design. FINE™/Design 2D offers a unique solution to that problem, allowing the control of the turning angle or of the change of swirl from inlet to outlet. A degree of freedom is introduced in the target pressure distribution, that is automatically modified in order to respect the outlet flow angle constraint. A part of the target pressure distribution is defined using a fourth order polynomial curve. The parameter defines the vertical position of a point of this polynomial curve. A smooth transition is ensured between the fixed part of the target and variable one. The parameter is iteratively and automatically adjusted in order to respect the outlet flow angle or the outlet swirl RVθ. 134 File Formats used for 2D Inverse Design 134.1 Input Files The input files required to run a bladetoblade study can be split into 3 categories: 138 FINE™ File Formats used for 2D Inverse Design Design 2D Module • The geometrical input files, defining the blade geometry. • The solver input files, which define the solver parameters and the fluid and flow conditions. • The inverse design input files, which permit to define an inverse problem. The geometrical and solver input files have been described in Chapter 12. The inverse design input files can be interactively created with the FINE™ environment, and are described in this section. 134.1.1 Inverse Design Input Files In order to perform an inverse design problem, 2 additional input files are required: — The ’project_computationname.req’ file, which defines the target pressure distribution. This file can be interactively created using the MonitorTurbo. — The ’project_computationname.run’ file, which specifies the parameters for the inverse design (automatically written by the user interface when saving the ’.run’ file). It should be mentioned that an inverse design always starts from a converged analysis of the initial geometry. The target pressure distribution can be generated by modifying the pressure distribution resulting from the analysis of the initial geometry. 134.2 Output Files Several output files are generated by the bladetoblade module, which have been described in Chapter 12. The inverse design method produces additional output files which are presented in this section. 134.2.1 Geometry Files a) ’project_computationname.geoini’ & ’project_computationname.geo’ These files contain the blade shape in the (m,θ) plane. The ’.geoini’ file contains the initial blade shape, whereas the ’.geo’ file contains the actual one. These files can be read and plotted with the NUMECA MonitorTurbo (Blade profile menu). In the case of an inverse design the visualization of the two files permits to compare the initial and the new geometry. b) ’project_computationname.split.geoini’ & ’projectname_computationname.split.geo’ (if splitter blades) These files contain the splitter blade shape in the (m,θ) plane. The ’.geoini’ file contains the initial blade shape, whereas the ’.geo’ file contains the actual one. These files can be read and plotted with the NUMECA MonitorTurbo (Blade profile menu). In the case of an inverse design the visualization of the two files permits to compare the initial and the new geometry. c) ’projectname_computationname.ss.ori’ ,’projectname_computationname.ps.ori’ & ’projectname_computationname.mer.ori’ These three files are automatically generated at the beginning of the solver execution, and contain respectively the suction side, the pressure side and the axisymmetric streamsurface on which the calculation is performed. These files are especially interesting in a 3D input type, with which this blade section results from the 3D interpolation procedure between the 3D blade and the streamsurface. These files have the same format as the blade geometry and streamsurface data input files. The coordinate system for the blade data is always XYZ, which makes these files compatible with IGG™ or AutoGrid. The coordinate system for the streamsurface is always ZRB (B is the streamtube thickness). FINE™ 139 File Formats used for 2D Inverse Design Design 2D Module The coordinates are given in the same unit length chosen by the user for the input data. d) ’project_computationname.ss.new’ & ’project_computationname.ps.new’ After an inverse design stage, these two files are automatically generated, and contain the new suction and pressure sides. These files have the same format as the blade geometry data input files. The coordinate system is always XYZ, which makes them compatible with IGG™ or AutoGrid. The coordinates are given in the same length unit chosen by the user in the input. In the default configuration of the solver the points included in these files are the mesh points along the blade walls. The number of points can be different and controlled by the user through the expert parameter NPTB2B. If this parameter is set to a value N different from 0, the number of points describing both suction and pressure sides will be N. 134.2.2 Quantities Files a) ’project_computationname.velini’ & ’project_computationname.vel’ These files contain the isentropic Mach number and the pressure coefficient distributions along the blade surfaces. The two quantities are plotted along the curvilinear coordinate measured along the blade surface (nondimensionalized by the blade chord). The ’.velini’ file contains the initial distribution, whereas the ’.vel’ file contains the actual one. The isentropic Mach number is calculated using the inlet relative total temperature and pressure, which are not necessarily imposed (depending on the choice of the inlet boundary condition). In case the total conditions are not imposed, the values are the ones resulting from the calculation (average along the inlet boundary). The isentropic Mach number is defined by: Mis = ⎛ p 2  ⎜ ⎛ 0⎞ γ – 1⎜⎝ p ⎠ γ– 1γ ⎝ ⎞ – 1⎟ ⎟ ⎠ (131) where p is the local static pressure, and p0 is the local relative total pressure calculated assuming a constant rothalpy and a constant entropy in the field. The pressure coefficient is defined by: p – p exit Cp = p exit (132) where pexit is the exit static pressure and p is the local static pressure. These files can be read and plotted by the NUMECA MonitorTurbo (Loading diagram menu). In the case of an inverse design the visualization of the two files permits to compare the initial and the new pressure distributions. b) ’project_computationname.loadini’ & ’projectname_computationname.load’ Provided that the parameter ISQUEL specified in the ’.run’ file is different from 0, these files are automatically generated and contain the distributions of the suctiontopressure side Mach number and pressure coefficient difference and average. These distributions are useful when the ’loading’ 1310 FINE™ File Formats used for 2D Inverse Design Design 2D Module formulation of the inverse design method is selected. The ’.loadini’ file contains the initial distribution, whereas the ’.load’ file contains the actual one. These files can be read and plotted by the NUMECA MonitorTurbo (Loading diagram menu). In the case of an inverse design the visualization of the two files permits to compare the initial and the new distributions. c) ’project_computationname.split.loadini’ & ’project_computationname.split.load’ (if splitter blades) Provided that the parameter ISQUEL specified in the ’.run’ file is different from 0, these files are automatically generated and contain the same quantities as the ’.load’ and ’.loadini’ files calculated along the splitter blades (Loading diagram menu). d) ’project_computationname.tarini’ & ’project_computationname.tar’ The inverse solver automatically generates these two output files, which contain respectively the initial and actual target pressure (or loading) distributions. FINE™ These files can be read and plotted by the NUMECA MonitorTurbo (Loading diagram menu). The comparison of the .tarini and ’.velini’ (or ’.loadini’) permits to observe the inverse problem to be solved, whereas the comparison of the ’.tar’ and ’.vel’ (or ’.load’) files permits to verify the correct convergence of the inverse design. 1311 Design 2D Module 1312 File Formats used for 2D Inverse Design FINE™ CHAPTER 14:The Task Manager 141 Overview Using the Solver menu in FINE™/Turbo computations can be started, suspended or killed. For basic task management these menu items are sufficient. The Task Manager provides more advanced features for the management of (multiple) tasks. It allows to manage tasks on different machines on a network, to define parallel computations or to delay tasks to a given date and time. Before using the Task Manager for the first time it is important to read the next section first. This section provides important information for getting started with the Task Manager. Read this section carefully to fully benefit of the capabilities of the Task Manager. From FINE™/Turbo the Task Manager can be accessed by the Modules/Task Manager menu item. The interface as shown in Figure 14.3.11 will appear. In section 143 the Task Manager interface is described in detail including a description of all capabilities. The current limitations of the Task Manager are listed in section section 146. To manage tasks through the use of scripts is also possible and has the benefit that it is not necessary to stay logged in on the machine on which the tasks are launched. See section 145 for more detail on the scripts to use to launch NUMECA software. 142 Getting Started 142.1 The PVM Daemons The Task Manager is based on the PVM library. It allows FINE™ to control processes and communication between processes on all the machines available by the user. PVM works with a virtual machine managed through a pvm daemon. In this section the way PVM daemons are working and its limitations under Windows are described. FINE 141 The Task Manager Getting Started 142.1.1 What PVM Daemons Do. If a user starts the FINE™ interface on a given computer where no PVM daemon is running, FINE™ will start the process pvmd on this machine that becomes the virtual machine server for the user. When adding a host in the Task Manager (on the Hosts definition page) a pvmd is started on the remote computer that is added to the virtual machine. If after that the user logs on the second computer and starts the FINE™ interface this second computer belongs also to the virtual machine whose server is the first pvmd started. If after that the user logs on a third computer on which no pvmd is running and starts the FINE™ interface, FINE™ will start a pvmd that becomes the server of a new virtual machine. When trying to add a host belonging the first virtual machine (containing the two first computers), he will see the a warning message that he cannot connect to the virtual machine because a pvmd is already running. If the user wants to have the three computers in the same virtual machine, one of the virtual machines must be shut down (on the Hosts definition page) and add the corresponding computers from the second one. 142.1.2 Limitation under Windows On windows only one pvmd can run and hence, only one single user can connect to the virtual machine. If an other user wants to use the NUMECA software on the PC as server (FINE™) or as client (EuranusTurbo), the first one needs to shut down the pvm daemons on this machine. To shut down go to the Hosts definition page and click on Shutdown. This will close the interface and removes all the pvm daemons on the machine. Remove the files pvml. and pvmd. from the directory defined by the PVM_TMP (by default C:\tmp). 142.2 Multiple FINE™ Sessions During a FINE™ session all the tasks defined by the user are stored in the tasks file in the NUMECA tmp directory. This directory is in the .numeca/tmp directory below the home directory. On UNIX the home directory corresponds to the HOME environment variable. This is also true on Windows if this variable is defined and, if it is not the case, it is set to the concatenation of HOMEDRIVE and HOMEPATH environment variables. When FINE™ is started more than once at the same time, a warning indicates to the user that FINE™ is already running and can enter in conflicts with the other FINE™ sessions. Indeed, the user can define tasks in both interfaces but the task definitions saved when exiting FINE™ will be overwritten by the other sessions. Therefore, it is not advised to open multiple FINE™ sessions when the Task Manager must be used. 142.3 Machine Connection from UNIX/LINUX Platforms The Task Manager allows the user to control processes on all the machines connected to the network. The rsh command is used by the PVM library to access the machines. Before using the Task Manager, the following actions must be done: 1. 142 Modify the .rhosts file in the home directory by introducing all the machines which can be used by the Task Manager. i.e.: if the machines machine1 and machine2 will be used by the user’s tasks, the .rhosts file must be modified as follows: line1: machine1 line2: machine2 where machine1 and machine2 are the host names. FINE Getting Started The Task Manager login1 and login2 are optional. They must be set if the login on remote host is different from the login on the local host. The .rhosts file needs to be ended by a blank line. The .rhosts file permission must be set to ’rw’ (chmod 600 ~/.rhosts). 2. Test the rsh command on the desired machine: an external check that the .rhosts file is set correctly is to enter the following command line: % rsh remote_host ls where remote_host is the name of the machine to connect to. If the login on the remote host is not the same, ensure that the .rhosts file contains the line: remote_host local_login and in this case the command line is: % rsh remote_host l local_login ls If the .rhosts is set up correctly, a listing of the files is shown on the remote host. 1. Log on the machine where the connection must be established. 2. Start FINE™ and open the Task Manager through Modules/Task Manager and use the button Shutdown of the page Hosts definition. The button Shutdown can be used to switch off all the PVM daemons of all the machines connected to FINE™. This action will stop all the daemons on all the machines connected, kill all the tasks and finally exit FINE™. 3. On UNIX: remove all the /tmp/pvmd. and /tmp/pvml. files. Under Windows these files should be removed from the directory defined by PVM_TMP (by default this directory is C:\tmp). 4. Repeat this operation for all the machines on which the problems appear. 5. The operations 2 and 3 can be done automatically using the script NUMECA_INSTALLATION_DIRECTORY/COMMON/cleanpvmd provided with the NUMECA software. If PVM still has a problem to get the connection, it will print an error message either to the screen, or in the log file /tmp/pvml. (on UNIX) or in the directory defined by the environment variable PVM_TMP (by default C:\tmp) in the log file called: pvml. . Please send this log file to NUMECA support team (support@numeca.be). FINE Due to a limitation of the PVM library, FINE™ can not be connected to a machine where FINE™ has already been started. When PVM tries to establish the connection, it detects that a server FINE™ is already running and/or pvm daemons are still running and finally refuses the connection with a warning. To solve this problem, the PVM daemons must be stopped on the machine on which FINE™ must be connected: All these operations apply only to the user’s daemons and user’s files. Multiple users can use the Task Manager simultaneously. No interaction appears between PVM daemons and PVM log files of different users. The Task Manager does not allow to launch processes from a UNIX platform to a Windows platform. 143 Getting Started The Task Manager 142.4 Machine Connection from Windows Platforms When a user stops the pvmd on a remote host (using Remove Host button on the Hosts definition page) and immediately try to restart it (using the Add Host... button), a message will appear stating that it is not possible to connect. This problem does not occur in general since there is no need to remove a host and add it immediately after. When it occurs the only solution is to wait until the host is available again (after 5 to 10 minutes). From time to time, when a user tries to connect on a remote host, an error message can appear very briefly: "Can not connect to RSH Port!!!" This may happen on Windows connecting to a host, disconnecting, and trying to reconnect again to the same host. It has the inconvenience to stop the interface FINE™. There is a socket release time parameter which keeps the connection for some time. 142.5 Remote Copy Features on UNIX/LINUX All the tasks defined by the user are associated with files used or created by the NUMECA’s software. When the files are not visible from the machine on which the task must be launched (i.e. the files are on the local disk of the host where FINE™ is running), the user can use the remote copy feature proposed in the Task Manager. All the files needed by the tasks will be transferred into a directory (specified by the user) of the remote machine and at the end all the created or modified files are transferred back to the host machine from which the task has been launched. By default, the available remote directories are "/tmp". The user can also specify any other directory, as long as it is visible from the remote host and has writing permission. This feature uses the rcp UNIX command. Before using the remote copy feature, it is advised to first check if the rcp command works correctly between the machines: — First try the rsh.exe command (see section 142.3). — Type the command: touch test;rcp p r test destination_machine:/tmp/test. If no error is returned by the system, the remote copy works between the local host and the destination_machine. Errors may appear if the .cshrc file contains an stty command. In order to be able to use the remote copy feature, remove all the stty commands from the .cshrc file. — If the login on the local host is different from the login on the remote host, type the command: touch test;rcp p r test remote_login@destination_machine:/tmp/test. 142.6 Remote Copy Features on Windows As files located on the local disk are not visible from a UNIX machine, this feature is proposed to be able to launch tasks on remote UNIX platforms. The principle is the same as the one described in the previous section: local files are copied in the remote directory specified by the user, then the task starts. When it terminates, all results files are transferred in the original directory. This feature uses rcp.exe windows command. Before using the remote copy feature, it is advised to first check if this command works properly: — First try the rsh.exe command (see section 142.3). — Create a file test, then type the command: rcp b test destination_machine:/tmp/test. If no error is returned by the system, the remote copy works between the local host and the destination_machine. Errors may appear if the .cshrc file contains an stty command. In order to be able to use the remote copy feature, remove all the stty commands from the .cshrc file. — If the login on Windows is different from the login on the remote host, type the command: 144 FINE The Task Manager Interface The Task Manager rcp b test destination_machine.remote_login:/tmp/test rcp.exe is provided with FINE™ and is located in the same directory as rsh.exe. 143 The Task Manager Interface 143.1 Hosts Definition On the Hosts definition page hosts in the virtual machine, the operating system of the machine and their connection status are visualized. For an explanation of the virtual machine see section 142.1.1. If the connection is not OK, it means that the corresponding computer is no more in the virtual machine. This may occur for example if the computer has been rebooted. FIGURE 14.3.11Hosts definition page 143.1.1 Add Host When the user clicks on the Add Host... button, the interface asks for a host name and a login name. The login name is optional. It is needed only if the user login on the local host and the one on the remote host are different. When the user accepts (Accept), the host name appears in the host list, with type of operating system and its connection status. At this point, the host is in the virtual machine, and is ready to receive a task. FINE if the connection can not be established, check for more detail in section 142.1, sec 145 The Task Manager Interface The Task Manager tion 142.3 and section 142.4. 143.1.2 Remove Host When the user clicks on Remove Host button, the selected host is removed from the list, and is not in the virtual machine any more. This operation is not allowed when a task is running on the host to be removed, or when the selected host is the local one. 143.1.3 Shutdown When the user clicks on Shutdown button, all hosts in the virtual machine are removed. FINE™ exits and the virtual machine halts. All running tasks are killed. This option is useful when the user wants to change the machine on which FINE™ is running. See section 142.1.1 for more detail on virtual machines and when to change this. 143.2 Tasks Definition A task is a collection of subtask where a subtask is one of the program with its arguments (’.run’ file for EURANUS and Design3D, template ’.trb’, geometry ’geomTurbo’ and mesh ’.igg’ files for AutoGrid and macro file .py and ’.run’ file for CFView™). The different subtasks of a given task can be run simultaneously if the output of one subtask is not needed by other ones (for example: several CFView™ subtasks with different macro ’.py’ files or several EURANUS subtasks with different ’.run’ files started on different computer). If the output of one subtask is needed by other ones, it must be run sequentially. For example: AutoGrid generates the mesh that is used for starting an EURANUS computation whose output is used for starting CFView™. 143.2.1 Task List In this section, the user can visualize the defined tasks and their status. To create a task, just click on New Task button. The defaults task name can be modified by clicking on Rename Task button. The selected task can be removed by clicking on Remove Task button. Once a task is created and defined (see following section), it can be started or stopped just by clicking respectively on the Start, or Stop button. A task can be delayed: click on Delay button and enter the date and time for the moment the task needs to be launched in the dialog box. The delayed task can be disabled using the button Cancel. When the user validates the data, a little watch in the task list indicates that the task is scheduled: FIGURE 14.3.22Task 146 List with Delay window to start a task at a later moment When exiting FINE™, all the delayed tasks are automatically started and stay in sleep mode until their starting dates are reached. When starting FINE™ again, all the task FINE The Task Manager Interface The Task Manager manager related to the delayed tasks still in sleep mode are killed and FINE™ Task Manger gets back the control of these tasks. 143.2.2 Task Definition In this section the subtasks of the selected task of the Task List are listed. A subtask is defined by its type (euranusTurbo, AutoGrid, CFView™ or Design3D), their status and the host on which they are launched. To add a subtask click on the New Subtask. Select the executable name (EURANUS, AutoGrid, CFView™ or Design3D) and the host on which the process should be started in the two lists. The host name list contains the hosts that are in the virtual machine. They are set in the Host definition page. 143.2.3 Subtask Arguments a) Definition of Input and Output Once a subtask is created, input and/or output files must be defined in the Subtask arguments section: — The flow solver EURANUS and Design3D requires one argument file: the name of the runfile. This files is created using the menu File/Save Run Files in the FINE™/Turbo module. — The mesh generation system AutoGrid requires three files as arguments: the trb file, the geomTurbo file and as output the grid file name (see the AutoGrid manual for more details) FINE 147 The Task Manager Interface The Task Manager — The flow visualization system CFView™ requires two files: the run file and a macro file (see CFView™ manual for more details) The run file is automatically opened by CFView™ before starting the macro. The macro file may open other ’.run’ files to perform flow comparisons (see CFView™ manual for more information about the macro ’.py’ file). b) Simultaneous or Sequential Mode Moreover, a process can be executed simultaneously with the other subtasks (by selecting Run Simultaneously with Previous Subtask) or sequential (by selecting Run After Previous Subtask). In this last case, the process waits the previous subtask to be finished before starting. This is only available for AutoGrid, Design3D and EURANUS subtasks. Only a certain amount of tasks can be performed at the same time depending on the available licenses. The subtasks related to postprocessing with CFView™ are always executed in sequential mode. c) Remote Copy The Remote copy to button allows the user to specify that the files are not visible from the remote machine and must be transferred. This is only available for AutoGrid, Design3D and EURANUS. d) Parallel Computations. d.1) MPI system The flow solver euranusTurbo has integrated multiprocessor machine concept. The button Parallel Computation can be activated to specify that the parallel version of the flow solver can be used for this computation. The button Flow solver parallel settings gives access to the dialog box used to set up a parallel computation. When the dialog box is opened, the block list displayed all the block of the mesh. The user can defined new processes on all the available machines and defined manually or automatically the load balancing (using the Automatic Load Balancing button). The parallel processing can only be used on multiprocessor machine (shared memory mode) or on machines with the same operating systems (homogenous distributed memory mode) See section 144 for more detailed information on parallel computations. 148 FINE The Task Manager Interface The Task Manager Processes list with the load balancing of the cells Buttons used to remove or add new processes on the specified machine List of the block in the associated mesh Default block distribution Button used to link the selected block with a process d.2) SGE system Within the Task Manager provided in FINE™/Turbo v6.27, the parallel process can be set using the SGE (Sun Grid Engine) batch system. This last sytem includes the possibility to add a SGE type host and to define arguments needed to launch the computation within the Task Manager. Host Definition In the page Hosts definition the user needs to add host. When adding the host, automatic checks are performed: 1. it will detect if the "sge_qmaster" is running on the platform. If not, it means that the platform does not have SGE capabilities or the platform is not the SGE master processor. 2. it will detect all parallel environment defined in SGE. 3. it will detect all parallel environment that the user is allowed to use. If no parallel environment could be accessed by the user, his login should be added to the user list by the SGE administrator. When all checks are successfull, the SGE capability of the added host is activated and the user can see if the host added is a SGE paltform within the Task Manager GUI (Figure 14.3.11). Task Definition In the page Tasks definition, if the user select a SGE platform when launching an EURANUS task in parallel, he has the access to the MPI system or the SGE system (Figure 14.3.23). When the SGE system is used, the number of processor and the SGE environment have to be specified. Depending on the number of processor, an automatic load balancing is performed to update the block distribution and the process needs only to be started by the user. FINE 149 The Task Manager Interface The Task Manager FIGURE 14.3.23Tasks Definition  SGE inputs Process Management Once the process is starting, the ".run" file is modified automatically depending of the number of processor. Then a script file ".sge" is created at the same time as the ".p4pg" file when using MPI system. The name of the SGE job is limited to 8 characters and the following format is thus chosen "comp#000" where 000 stands for a any number depending of the number of SGE jobs already running under the same environment. To test if a computation is running, because there are no communication with the task manager since EURANUS has not been launched using PVM daemon, the "qstat" command with the jobID number of the SGE job is used. To suspend the SGE job, the user could use the Suspend function of the Task Manager. It will create automatically a ".stop" file in the running computation directory that will enable EURANUS to suspend after saving the solution at the next iteration or after the full multigrid initialization. To kill the SGE job, the user could use the Stop function. The Task Manager will then use the SGE’s function "qdel" to kill the computation without saving the solution. To kill EURANUS properly, the SGE’s "execd parameters" variable should be set to "NOTIFY_KILL=TERM" and the "notify time" variable of nodes should be set to a sufficient value to allow EURANUS to exit properly. We invite the user to ask the SGE administrator to check these variables. e) Message Window When a task is started, a Task Manager process is launched to take care about the task management: process communication, automatic launching of the sequential and parallel subtasks. A message window linked to the Task Manager is opened. In this window the user can follow the evolution of the status of all the subtasks of the current task. In case of flow solver computations the iterations are also displayed in this window as shown in Figure 14.3.24. At the bottom of the Task Manager window a Refresh Rate can be chosen. This rate determines how frequently the Task Manager window is updated. A higher refresh rate will update the information in the window more frequently but will use more of the available CPU. 1410 FINE Parallel Computations The Task Manager FIGURE 14.3.24Task Manager information window If the user quits FINE™, all the message windows will stay open and the tasks will continue. Closing a message window will immediately kill all the subtasks of the corresponding task. 144 Parallel Computations 144.1 Introduction Parallel computations can be defined through the FINE™ interface as described in section 143.2.3. Parallel processing relies on the distribution of independent tasks among several processors using communication protocols to transfer data from one processor to another whenever this is necessary. This induces of course an acceleration of the computation itself but it also makes possible very large computations that would not fit on a single processor. The present parallel processing relies on the block structure of the flow solver EURANUS. Each process is assigned a given number of blocks. As a consequence, the number of processors cannot exceed the number of blocks. Boundary data are exchanged between processors each time an update of the flow solution is required. The parallel version makes use of MPI (Message Passing Interface) libraries. MPI was chosen among other tools such as PVM or Open MP for its high communication performances (high bandwidth, low latencies). Although Open MP has better performance on shared memory configurations, i.e. on a given computer with single global memory and several processors, it is not designed for distributed memory configurations (several computers with their own memory). The parallel version is implemented for UNIX, LINUX and Windows platforms. FINE 1411 Parallel Computations The Task Manager The present MPI implementation is based on a host/node approach. One host process is dedicated to input/output management. The host reads the mesh and input files, sends the data to the computation processes (the nodes), receives the computation results from the nodes and writes the output files. Figure 14.4.15 shows the task distribution on a 4 processors configuration. Note that the host/ node implementation will be replaced progressively as parallel MPI input/output functionalities are now available. Input data base reading Node 1 Host Node 2 boundary conditions FIGURE 14.4.15Tasks writing Output data base Node 3 boundary conditions in a parallel computation 144.2 Modules Implemented in the Parallel Version The following flow solver functionalities are already available in the parallel version: • All turbomachine boundary conditions (including Phaselagged). These include rotor/stator interfaces, non matching boundaries and the fully conservative non matching boundary treatment (FNMB), • Turbomachinery initial solution, • BaldwinLomax, SpalartAllmaras and kε turbulence models, • Real gases, • Preconditioning (low Mach number and incompressible fluids), • Cooling holes, • Outputs including pitchwise averaged output. No solid data nor surface averaged outputs are available yet. The lagrangian module is not available for parallel computations. 144.3 Management of Interblock Communication The block structure of the solver allows to distribute blocks across processors or computers (in case of a cluster). Each processor will handle an integer number of blocks. The treatment of the boundary condition will be replaced by message passing between the processors or remote computers. Communication optimization The parallel version of the flow solver is optimized in order to minimize duplicated data as well as the number and the volume of exchanged messages. A significant improvement of the code performance was obtained by grouping small messages into larger buffers: the information contained in small messages is usually shared by a large number of blocks, leading to frequent messages of 1412 FINE Parallel Computations The Task Manager that type. This is the case for block edges data that are exchanged several times during each iteration. Significant latency times are induced by these communication processes and message grouping highly reduces the number of such messages. Large message limitation Very large messages are usually exchanged during initialization and at the end of the computation between the nodes and the host. These also need to be avoided as they can cause important memory needs and eventually lead to system failure. Messages are split into buffers of maximum size MXBFSZ (see section 144.4) in order to avoid excessive MPI memory requests. 144.4 How to Run a Parallel Computation The setting of a parallel run using the FINE™ interface is described in section 143.2.3. The user selects the number of nodes, making sure it is smaller than the number of blocks. A balanced distribution of the blocks among the various processes is automatically performed by the FINE™ interface but the user can also define its own load balancing, i.e. process distribution. Memory allocation Memory allocation is performed as follows: • The integer data structure is duplicated for all processes. Since the integer data structure size is about a tenth of the real data structure, this does not lead to high memory overload when the number of processes is less than 10. • The real memory allocation is performed for each process. It should be set to the minimal amount of memory necessary to hold the data structure on the process that has most grid points. When the load is well balanced, the real memory overload is due to face and edge data structures. These data need indeed to be duplicated when two processors are involved in the same block connection. The total memory need Mtotal for a parallel computation involving n ( n ≥ 2 ) processors can be estimated as: n M total = M real ⋅ 1, 2 ⋅  + M integer ⋅ n n–1 where Mreal and Minteger are the real and integer memory needed for the same computation in sequential mode. From a practical point of view, the user does not specify the total memory needed but the integer M real and real memory required per processor. This can be estimated as  ⋅ 1, 2 for the real mem n ory and Minteger for the integer memory. FINE In case of parallel calculation the estimated number of real memory displayed by FINE™ on the page Control Variables shall not be followed but the formula shown above shall be respected. 1413 Task Management Using Scripts The Task Manager The following table states the total memory need for a parallel computation using respectively 4 and 6 and 8 processors. The values of Mreal and Minteger are set to 10 Mb and 1 Mb respectively. The equivalent memory request on a single processor is thus 11Mb. n Mtotal (Mb) Parallel overhead (Mb) 4 20 9 6 20.4 9.4 8 21.7 10.7 TABLE 141 Parallel memory request In the present implementation, the presence of the host processor increases the global memory request. It also reduces the overall speedup of the computation as it is mainly dedicated to I/O management and no computation is affected to it. Future versions of EURANUS will optimize this aspect by removing gradually the need of a host processor. Message size limitation During initialization and final steps, large messages are usually exchanged between the nodes and the host process. In order to avoid any system failure, messages are split into buffers of maximum size. This size is set to 100000 by default but the user can eventually tune this value through the expert parameter MXBFSZ. 144.5 Troubleshooting If the computation is interrupted for an unknown reason, more detailed information is provided in the ’.std’ and ’.log’ computation files. The file contains all relevant informations including MPI error messages and should be sent to the NUMECA support team. 144.6 Limitations • The distributed memory mode is restricted to homogeneous (i.e. with the same operating system) clusters. • The number of processors should not exceed the number of blocks. 145 Task Management Using Scripts This section provides all available information to launch installed NUMECA Software from a shell, without using IGG™, AutoGrid, FINE™ or CFView™ interfaces. Every time a task is started a script file is automatically created. On UNIX the name of this file has the extension .batch and under Windows the extension is .bat. Such files contain text lines with the commands to launch the software with the appropriate command arguments. To launch a task from a shell simply execute the automatically generated file by typing its name in a shell. In the next sections the available commands to launch NUMECA software are described in more detail. 1414 Please notice that the capability to launch in batch is currently not supported for EURANUS in Parallel Mode on PC. FINE Task Management Using Scripts The Task Manager 145.1 Launch IGG™ Using Scripts 145.1.1 How to Launch IGG™ on UNIX To launch IGG™ without use of the interface the commands to perform must be written in a macro script file. To create such a file: 1. Create a script file *.py. For more details on the commands that can be included in such a script file see the IGG™ manual. 2. Set permission for execution for the script by using the command: "chmod 755 *.py". 3. Launch the macro script in a shell by typing: igg script /user/script.py batch niversion 62_7 The command line to start the grid generator IGG™ contains its name, the full path name of the script "*.py" file to launch and the IGG™ release that will be used. The "batch" option avoids the display of the IGG™ graphical user interface. "igg SCRIPT_PATH/script.py batch niversion " 145.1.2 How to Launch IGG™ under Windows 1. Create script file "*.py". For more detailed information on the commands to include in a macro script see the IGG™ manual. 2. Set permission for execution of the file *.py Launch the macro script *.py by typing in a shell: d:\NUMECA_SOFTWARE\fine62_7\bin\igg.exe script d:\user\test.py batch 3. The command line to start the grid generator IGG™ contains its full path name and the full path name of the script "*.py" file to launch. The "script" & "batch" options respectively permits to launch the script and avoids to display the IGG™ graphical user interface. "IGG_PATH\igg.exe script SCRIPT_PATH\script.py batch" REMARKS: • The full path name of the executable (igg.exe) has to be specified. • The full path name of the script has to be specified. • If there is a segmentation fault at exit (due to an incontrollable "opengl" problem), it is possible to avoid it by adding driver msw option: d:\NUMECA_SOFTWARE\fine62_7\bin\igg.exe script d:\test.py batch driver msw 145.2 Launch AutoGrid using Scripts 145.2.1 How to Launch AutoGrid on UNIX 1. Create a template and geometry files (*.trb and *.geomTurbo) using the AutoGrid interface. Start AutoGrid to create a mesh from these files by typing: igg batch autoGrid /user/test.trb /user/test.geomTurbo /user/test.igg niversion 62_7 2. The command line to start the grid generator AutoGrid contains its name, the full path name of the template, of the geometry files, the full path name of the mesh that will be saved and the IGG™ release that will be used. The "batch" option avoids the display of the IGG™ graphical user interface. FINE 1415 The Task Manager Task Management Using Scripts 145.2.2 How to Launch AutoGrid under Windows 1. Create a template and geometry files (*.trb and *.geomTurbo) using the AutoGrid interface. Start AutoGrid to create a mesh from these files by typing on one line: d:\NUMECA_SOFTWARE\fine62_7\bin\igg.exe batch autoGrid c:\users\template.trb c:\users\template.geomTurbo c:\users\mesh.igg 2. The command line to start the grid generator AutoGrid contains its full path name, the full path name of the template, of the geometry files and the full path name of the mesh that will be saved. The "batch" option avoids the display of the IGG™ graphical user interface. 145.3 Launch EURANUS in Sequential using Scripts 145.3.1 How to Launch EURANUS in Sequential on UNIX 1. Create a script file (for example, with the name ’batch.sh’). Such a script file (e.g. ’batch.sh’) must be created with permission for execution to launch a series of computations. An example of a ’batch.sh’ file for a series of computations on UNIX: #! /bin/csh euranusTurbo /users/project/project_computation_1/project_computation_1.run niversion 62_7 euranusTurbo /users/project/project_computation_2/project_computation_2.run niversion 62_7 The script is started in a Cshell that is obtained by having as its first line: " #! /bin/csh". The command line, to start the flow solver EURANUS, contains its name, the full path name of the ’.run’ file to launch and the FINE™ release that will be used: "euranusTurbo COMPUTATION_PATH/computation.run niversion " 2. Set Permission for execution for the script file ’batch.sh’ by typing the command: "chmod 755 batch.sh". 3. Create an input file (’.run’) for each computation. To create those files through the FINE™ interface, click on the File/Save Run Files menu in order to save the ’.run’ file of the activated computation, after opening the corresponding project. 4. Launch the script ’batch.sh’ by typing the script file name: ’./batch.sh’. When saving the ’.run’ file of the computation (File/Save Run Files) and launching the computation (Solver/Start...) killed just afterwards (Solver/Kill...), a new script ’.bat’ on WINDOWS (’.batch’ on UNIX) is created in the corresponding computation subfolder that enables the user to launch the same computation in batch. 145.3.2 How to Launch EURANUS in Sequential under Windows 1. Create Script File ’.bat’. An example of ’.bat’ file for a series of computations on Windows: C:\NUMECA_SOFTWARE\fine62_7\bin\euranus.exe C:\users\project\project_computation_1\project_computation_1.run seq \\ C:\NUMECA_SOFTWARE\fine62_7\bin\euranus.exe \\ C:\users\project\project_computation_3\project_computation_3.run seq 1416 FINE Task Management Using Scripts The Task Manager C:\NUMECA_SOFTWARE\fine62_7\bin\euranus.exe \\ C:\users\project\project_computation_2\project_computation_2.run seq The command line, to start the flow solver EURANUS, contains its full path name, the full path name of the ’.run’ file to launch and the sequential mode selection: INSTALLATION_DIRECTORY\fine62_7\bin\euranus.exe COMPUTATION_PATH\project_computation_1.run seq \\ 2. Set Permission for Execution ’.bat’ 3. Create an input file (’.run’) for each computation. To create those files through the FINE™ interface, click on the File/Save Run Files menu in order to save the ’.run’ file of the activated computation, after opening the corresponding project. 4. Launch the script ’.bat’ by typing the script file name: ’.bat’ in a shell or double click on the ’*.bat’ file from the Windows Explorer. When saving the ’.run’ file of the computation (File/Save Run Files) and launching the computation (Solver/Start...) killed just afterwards (Solver/Kill...), a new script ’.bat’ on WINDOWS (’.batch’ on UNIX) is created in the corresponding computation subfolder that enables the user to launch the same computation in batch. 145.4 Launch EURANUS in Parallel using Scripts 145.4.1 How to Launch EURANUS in Parallel using MPI on UNIX 1. Create a script file ’batch.sh’ with permission for execution. An example of a ’batch.sh’ file for a parallel computation on UNIX: #! /bin/csh euranusTurbo_parallel /users/project/computation/computation.run niversion 62_7 p4pg / users/project/hosts.p4pg The script is started in a Cshell that is obtained by having as its first line: " #! /bin/csh". The command line, to start the flow solver EURANUS in parallel, contains the script name that enables parallel computation, the full path name of the ’.run’ file to launch, the FINE™ release and the full path name of the file ’hosts.p4pg’ containing the definition of the machines that will be used to launch the computation in parallel: "euranusTurbo_parallel COMPUTATION_PATH/computation.run niversion p4pg HOST_PATH/hosts.p4pg" 2. The name of the executable is different from the one for sequential computations. Create Hosts Definition File ’hosts.p4pg’. A file needs to be created to define the hosts (e.g. ’hosts.p4pg’). This file specifies the machine information regarding the various processes. An example of a ’hosts.p4pg’ file: Example 1: Hostname1 4 euranusTurbo62_7(master host on Hostname1 and 4 processes on Hostname1) Hostname2 2 euranusTurbo62_7(2 processes on Hostname2) FINE 1417 Task Management Using Scripts The Task Manager Example 2: Hostname1 0 euranusTurbo62_7 (master host on Hostname1 and no other process on Hostname1) Hostname2 2 euranusTurbo62_7 (2 processes on Hostname2) For each machine, a line must be added consisting of the machine name (the machine hostname), the number of processes to run on the machine, the name of the executable and the FINE™ release: "hostname 4 euranusTurbo " If additional machines are to be used, subsequent lines are required for each one. If the number of processors is set to 0 for the first machine (first line of the ’hosts.p4pg’ file), only the master host process will run on that machine while the nodes will run on the next machines declared in the following lines. 3. The first machine (hostname) specified in the file ’hosts.p4pg’ should be the one from which the script will be launched. The total number of processes defined in the file ’hosts.p4pg’ should be equal to the number of nodes running. Set permission for execution ’batch.sh’ by using the command: "chmod 755 batch.sh" Create input files ’.run’ to launch the computation. The parallel settings of the computational file (’.run’) are managed by the Task Manager. Therefore before launching the parallel computation script, the following steps must be performed through the FINE™ interface: 4. Create computational file (’.run’) by activating the corresponding computation and clicking on the File/ Save Run Files menu in the interface. 5. To set the final parallel settings: — — — — 6. create a task in the Task Manager, define the parallel settings of EURANUS subtask (parallel computation), launch the task through the Task Manager by clicking on Start, kill the task when EURANUS flow solver starts by clicking on Stop. This operation is mandatory in order to have all the parallel settings correctly imposed in the computation file (’.run’). Launch the script ’batch.sh’ by typing the script file name: "./batch.sh". When saving the ’.run’ file of the computation (File/Save Run Files) and launching the computation in parallel as explained in step 5 through the Task Manager (Modules/Task Manager) and killed it just afterwards, a new script ’.batch’ and a file ’.p4pg’ are created in the corresponding computation subfolder that enable the user to launch the same computation in batch and in parallel. 145.4.2 How to Launch EURANUS in Parallel using MPI on Windows 1. Create a script file ’batch.bat’ with permission for execution. An example of a ’batch.bat’ file for a parallel computation on Windows: D:\NUMECA_SOFTWARE\Fine62_7\bin\mpirun.exe "D:\test\test_computation_1\test_computation_1.p4pg" "D:\test\test_computation_1\test_computation_1.run" / / The command line, to start the flow solver EURANUS in parallel, contains the script name that enables parallel computation, the full path name of the ’.run’ file to launch and the full path name of the file ’.p4pg’ containing the definition of the machines that will be used to launch the computation in parallel: 1418 FINE Task Management Using Scripts The Task Manager "NUMECA_RELEASE_PATH/mpirun.exe HOST_PATH/hosts.p4pg COMPUTATION_PATH/computation.run " 2. Create Hosts Definition File ’.p4pg’. A file needs to be created to define the hosts (e.g. ’hosts.p4pg’). This file specifies the machine information regarding the various processes. An example of a ’hosts.p4pg’ file: Example 1: Hostname1 5 D:\NUMECA_SOFTWARE\Fine62_7\bin\euranus.exe (master host on Hostname1 and 4 processes on Hostname1) Hostname2 2 D:\NUMECA_SOFTWARE\Fine62_7\bin\euranus.exe(2 processes on Hostname2) Example 2: Hostname1 1 D:\NUMECA_SOFTWARE\Fine62_7\bin\euranus.exe (master host on Hostname1 and no other process on Hostname1) Hostname2 2 D:\NUMECA_SOFTWARE\Fine62_7\bin\euranus.exe (2 processes on Hostname2) For each machine, a line must be added consisting of the machine name (the machine hostname), the number of processes to run on the machine, the name of the executable and the FINE™ release: "hostname 4 NUMECA_RELEASE_PATH\bin\euranus.exe" If additional machines are to be used, subsequent lines are required for each one. If the number of processors is set to 1 for the first machine (first line of the ’.p4pg’ file), only the master host process will run on that machine while the nodes will run on the next machines declared in the following lines. 3. The first machine (hostname) specified in the file ’.p4pg’ should be the one from which the script will be launched. The total number of processes defined in the file ’.p4pg’ should be equal to the number of nodes running. Set permission for execution ’batch.bat’ Create input files ’.run’ to launch the computation. The parallel settings of the computational file (’.run’) are managed by the Task Manager. Therefore before launching the parallel computation script, the following steps must be performed through the FINE™ interface: 4. Create computational file (’.run’) by activating the corresponding computation and clicking on the File/ Save Run Files menu in the interface. 5. To set the final parallel settings: — — — — 6. create a task in the Task Manager, define the parallel settings of EURANUS subtask (parallel computation), launch the task through the Task Manager by clicking on Start, kill the task when EURANUS flow solver starts by clicking on Stop. This operation is mandatory in order to have all the parallel settings correctly imposed in the computation file (’.run’). Launch the script ’batch.bat’ by typing the script file name: "./batch.bat" in a DOSshell. FINE When saving the ’.run’ file of the computation (File/Save Run Files) and launching the computation in parallel as explained in step 5 through the Task Manager (Modules/Task Manager) and killed it just afterwards, a new script ’.bat’ and a file ’.p4pg’ are created in the corresponding computation subfolder that enable the user to launch the same computation in batch and in parallel. 1419 The Task Manager Task Management Using Scripts 145.4.3 How to Launch EURANUS in Parallel using SGE on UNIX 1. Create a script file ’batch.sge’ with permission for execution. An example of a ’batch.sge’ file for a parallel computation on UNIX: #! /bin/csh #$ S /bin/sh #$ o /home/sgeuser/parallel_sge/parallel_sge_computation_1/ parallel_sge_computation_1.std j y #$ N comput1 #$ pe numecampi 3 #$ notify P4_GLOBMEMSIZE=15000000 Export P4_GLOBMEMSIZE NI_VERSIONS_DIR=/usr/numeca MPIR_HOME=$NI_VERSIONS_DIR/_mpi cd /home/sgeuser/parallel_sge/parallel_sge_computation_1 $MPIR_HOME/bin/mpirun np $NSLOTS machinefile $TMPDIR/machines \ $NI_VERSIONS_DIR/bin/euranusTurbo62_7 \ /home/sgeuser/parallel_sge/parallel_sge_computation_1/parallel_sge_computation_1.run where: #$ S /bin/sh requires Bourne shell to be used by SGE for job submission and hence, only the .profile file of the user is executed if exists on each computation host. There is nothing specific to Numeca software that must be written . the .profile file. #$ o /home/sgeuser/parallel_sge/parallel_sge_computation_1/ parallel_sge_computation_1.std j y tells SGE system that the standard output has to be redirected in the ".std" in the computation directory, the option "j y" indicates that the standard error is redirected into the same file. #$ N comput1 is the name of the job given to SGE and that will be seen when monitoring the job with the graphical monitoring utility qmon (Job Control button ) or with the qstat SGE command. SGE has a limitation of 8 characters for the job name. #$ pe numecampi 3 requests 3 slots (processors) to the SGE system for executing the job using the numecampi parallel environment described in chapter 2.1. This must correspond to NTASK +1 where NTASK is the number of computation processes in the ".run" file, the "+1" being the host process that manages inputs/outputs. #$ notify gives a delay between the send of the SIGKILL signal and SIGUSR2 signal. The delay is defined in the SGE interface. P4_GLOBMEMSIZE=15000000 Export P4_GLOBMEMSIZE NI_VERSIONS_DIR=NUMECA_RELEASE_PATH MPIR_HOME=$NI_VERSIONS_DIR/_mpi are the environment variables indicating respectively the Numeca software installation directory and the mpi directory that are used in the following command: 1420 FINE Task Management Using Scripts The Task Manager $NSLOTS is the number of slots (processors) that have been allocated by SGE for the job, $TMPDIR is generated by SGE for providing the machines file used by the mpirun script. $NI_VERSIONS_DIR/bin/euranusTurbo is a symbolic link to the numeca_start startup script for all Numeca softwares and 62_7 is the version of the code that will be used and requires that it is installed under /NUMECA_RELEASE_PATH/fine62_7. /home/sgeuser/parallel_sge/parallel_sge_computation_1/parallel_sge_computation_1.run is the argument to the euranusTurbo executable. 2. For sequential runs, the line "#$ pe numecampi 3" must be removed and the final command must be: $NI_VERSIONS_DIR/bin/euranusTurbo62_7 \ /home/sgeuser/ parallel_sge/parallel_sge_computation_1/parallel_sge_computation_1.run seq Set permission for execution ’batch.sge’ by using the command: "chmod 755 batch.sge" Create input files ’.run’ to launch the computation. The parallel settings of the computational file (’.run’) are managed by the Task Manager. Therefore before launching the parallel computation script, the following steps must be performed through the FINE™ interface: 3. Create computational file (’.run’) by activating the corresponding computation and clicking on the File/Save Run Files menu in the interface. 4. To set the final parallel settings: — — — — 5. create a task in the Task Manager, define the parallel settings of EURANUS subtask (parallel computation), launch the task through the Task Manager by clicking on Start, kill the task when EURANUS flow solver starts by clicking on Stop. This operation is mandatory in order to have all the parallel settings correctly imposed in the computation file (’.run’). Launch the script ’batch.sge’ by typing the script file name: "./batch.sge". When saving the ’.run’ file of the computation (File/Save Run Files) and launching the computation in parallel as explained in step 4 through the Task Manager (Modules/ Task Manager) and killed it just afterwards, a new script ’.sge’ is created in the corresponding computation subfolder that enables the user to launch the same computation in batch and in parallel. 145.5 Launch CFView™ Using Scripts 145.5.1 How to Launch CFView™ on UNIX 1. Create a macro file ’.py’. For more details see the CFView™ for more detailed information on the format of a macro file and the commands that can be included in a macro file. 2. Launch the macro ’.py’ by typing: cfview macro /user/test.py batch niversion 62_7 The command line to start CFView™ contains its name, the full path name of the macro ’.py’ file to launch and the CFView™ release that will be used. The ’batch’ option avoids the display of the CFView™ graphical user interface. "cfview macro MACRO_PATH/macro.py batch niversion " 145.5.2 How to Launch CFView™ on PC under Windows 1. FINE Create a macro file ’.py’. For more details see the CFView™ for more detailed information on the format of a macro file and the commands that can be included in a macro file. 1421 The Task Manager Limitations Launch the macro ’.py’ by typing: d:\NUMECA_SOFTWARE\fine62_7\bin\cfview.exe macro \user\test.py batch 2. The command line to start CFView™ contains its full path name and the full path name of the macro ’.py’ file to launch. The ’batch’ option avoids the display of the CFView™ graphical user interface. 145.5.3 Command Line Arguments The command cfview may be followed by a set of command line arguments. Those command line arguments allow to override some system defaults (used driver, display, doublebuffering and update abort options) or to specify files to be loaded immediately (project, macro, defaults settings, macro module). The supported command line arguments are: help prints a summary of the command line arguments, version prints the CFView™ version number, date prints the CFView™ version date, defaults starts CFView™ with the default settings from the specified file, project starts CFView™ and opens immediately the specified project, macro starts CFView™ and execute the specified macro script, macromodule starts CFView™ and load the specified macro module, display starts CFView™ on the specified display device, doublebuffering on (off) activates (disables) double buffering, updateabort on (off) activates (disable) update aborting (see the CFView™ manual for more detail on this option), driver starts CFView™ with the specified graphics accelerator, reversevideo on (off) starts CFView™ with black (white) background color (see the CFView™ manual for more detail on this option), facedisplacement starts CFView™ with the specified face displacement (see the CFView™ manual for more detail on this option), loaddata all (none, ask) when opening a project the quantities fields are loaded in the computed memory (are not loaded, a specific dialog box is raised where the user choose the field variables to be loaded). The defaults is to load all field quantities. (see the CFView™ manual for a description of the data management facility and of the associated dialog box), batch on (off) starts CFView™ without graphical user interface. This mode can be used in combination with the macro command line option in order to perform the execution of a macro script without user interaction, hoops_relinquish_memory off this option disables the hoops garbage collection feature that is activated when CFView™ is idle during a long period of time. 146 Limitations The task manager have some limitations due to the current PVM and MPI libraries: 1422 FINE Limitations The Task Manager • UNIX to PC connections are not allowed. • The remote copy works only if there is enough disk space on the remote machine. Currently, no check is performed to identify the available disk space and the flow solver crashes with "undifined reason". • Parallel computation with distributed memory are only available on homogenous UNIX/Windows platforms. • When a user launches FINE™ on different machines, the connection between these machines is not allowed as described in section 142.1.1. FINE 1423 The Task Manager 1424 Limitations FINE CHAPTER 15:Computation Steering and Monitoring 151 Overview This chapter describes the Computation Steering pages and the additional tool MonitorTurbo. First section 152 describes the Computation Steering/Control Variables page. Furthermore this chapter is completely dedicated to the monitoring tools available in FINE™ to monitor the global solution during and after a computation: • Computation Steering/Convergence History and Task Manager/Convergence History, see section 153 and • MonitorTurbo, see section 154. In section 155 advice is provided on how to use the monitoring tools in analysing the progress of a computation. 152 Control Variables The Computation Steering/Control Variables page allows to define some global parameters for the selected computation: • the Maximum Number Of Iterations on the finest grid level (i.e. not including the iterations performed during coarse grid initialization). • the Convergence Criteria corresponding to the (negative) number of orders of magnitude the norm of the residuals must decrease before stopping the calculation. If this criterium is not reached the calculation proceeds until the maximum number of iterations is performed. • The frequency for saving output (Save Solution Every): every x iterations the solver saves the flow solution and creates the output files to be read in CFView™(where x is the number of iterations defined in the FINE™ interface). • When the option Mimimum output is selected the solution is only saved at the last iteration. • the Memory Requirements for the computation. By default an estimation is given for the required memory. Depending on the parameters defining the computation additional memory may be needed. For example, more memory is required when full nonmatching connections FINE™ 151 Convergence History Computation Steering and Monitoring or a kε turbulence model is used. Also the amount of selected output may require more memory. To allocate more memory for the computation select the button Set the requested memory. This will allow to define the amount of memory in Mb used for reals and integers. For unsteady computations the Control Variables page is updated to give access to additional parameters as described in section 42.1 and section 42.3. Furthermore this page contains in expert mode two lists of expert parameters. Only the expert parameters that are described in the manual are supported. Use of the other parameters is not recommended. For a summary of all supported expert parameters see Appendix C. 153 Convergence History The Computation Steering/Convergence History or Task Manager/Convergence History page allows the user to define quantities to be followed during the convergence process of the flow solver EURANUS. This pages is divided in 5 areas as shown in Figure 15.3.01: 1. The steering files selection (Select Computations) and the curves export (Export Curves To File...) only available in Task Manager/Convergence History page. 2. The available variables (Available Variables). 3. The parameters (Parameters type). 4. The selected variables (Selected Variables). 5. The graphics view (Convergence History). (3) (2) (4) (1) (5) FIGURE 15.3.01The 152 five areas of the Convergence History page FINE™ Convergence History Computation Steering and Monitoring When the flow solver EURANUS is invoked, a communication is automatically established with FINE™ allowing the user to follow the selected quantities. Two representations of the quantities are currently available: the convergence curves displayed in the area 5 and the quantity value at the last iteration in the area 4. All these data are stored in files with extension .steering and .steering.binary. These files are created and managed automatically by FINE™ If the communication between the flow solver and FINE™ is interrupted (i.e.: network problem), parts of the convergence curves can be lost. 153.1 Steering Files Selection and Curves Export Different mode exists for the selection of the current steering results stored in the steering files: 1. When a project is opened, the active computation steering files is automatically selected and appears in the Add or select computations window (a) appearing when clicking on Select Computations button. Each time a new computation is selected, the associated steering file is automatically loaded and becomes the active one. (a) (b) (c) FIGURE 15.3.12Steering (d) files selection area 2. All the steering files already loaded can be selected by leftclick and leftclick in the list of available computations. 3. The file can also be loaded manually using the button Add Computation (c). A file chooser prompts the user to select the file. 4. The button Remove Computation allows the user to remove from the memory the selected computation (the file is not removed and remains available for selection). 5. Additionally, when a task is started, the steering files of the flow solver computation called in the task are automatically loaded and become available through the list (b). The Export Curves To File... button enables the user to save in an ASCII file ’.cvh’ all the curves plotted in the Graphics View. 153.2 Available Quantities Selection The available quantities selected by default are linked to the type of computation. For example, when launching a turbomachinery computation, the global residual, the inlet and outlet mass flow, the efficiency, the pressure ratio, the axial thrust and the Torque are computed during the convergence process. The Available Quantities list (b) allows the user to select and add (c) new quantities to the computed list FINE™ 153 Convergence History Computation Steering and Monitoring . (a) (b) (c) FIGURE 15.3.23Available quantities selection area All the quantities can be added before or during the computation. When a quantities has been added, it appears in the selection list and becomes the selected quantity. If the flow solver is running, the value and the convergence curve of the new quantities is displayed after a few seconds. The convergence curve begins at the iteration corresponding to the moment when the new quantity has been added in the Selected Variables list. When a quantity is added for selection it appears in the selection list with a number behind the name. This number is only added to avoid to have two times the same variable name in the list. This is especially necessary when, for example, the static pressure is monitored at two different points in the domain. 153.3 New Quantity Parameters Definition When a new quantity has been added, it becomes available for selection in the Selected Variables list (area 4 in Figure 15.3.01). The user can select the way the flow solver computes the quantity through the parameter type area (area 2 in Figure 15.3.01). Several types of parameters can be chosen through the parameter type list box (a in Figure 15.3.34). The available types of parameters that can be defined to computed the selected quantities: 1. global: the computed variable is averaged over all the domain. 2. local 3d grid point: the user specify the grid point indices (I,J,K) and the block index (block id) where the quantity must be computed. (a) FIGURE 15.3.34Parameter type definition Care should be taken when using the steering of a parameter on a local 3d grid point. It should be carried out in the following way:  select the parameter (relative velocity u, static pressure...).  add for selection. It becomes available for the selected variables. 154 FINE™ Convergence History Computation Steering and Monitoring  set the block id and the I,J,K indices of the grid point on which the evolution of the selected parameter will be visualized. All the user modifications (I,J,K indices...) can also be done (and modified) during the computation run. 153.4 Quantity Selection Area When a quantity has been added, it becomes available for selection in the Selected Variables list. The list is divided in 3 columns as shown in Figure 15.3.45: the variable name (a) which can be changed using the button rename (d) , the quantity value (b) which displays the last computed value and the units (c) of the variable. The button remove (e) is used to remove the first selected variable. . (b) (a) (c) (d) (e) FIGURE 15.3.45Selected variables area When a quantity is not yet computed, the value indicated is undefined. Selecting a quantity will show its history in the graphics view as described in the next paragraph. To select multiple quantities click on them (with the left mouse button) in the list while holding the or key. To select quantities that are next to each other in the list simply click on the first one and keep the mouse button pressed while moving to the last variable. 153.5 Definition of Global Residual The residuals are computed by EURANUS as a flux balance (the sum of the fluxes on all the faces of each cell): RES = ∑ fluxes . (151) The root mean square of the residuals is computed with the following formula: RES RMS RES = log ⎛ RMS ⎛ ⎞ ⎞ , ⎝ ⎝ cellvolume⎠ ⎠ (152) and the maximum of the residuals in the same way: RES MAXRES = log MAX ⎛ ⎞ , ⎝ cellvolume⎠ FINE™ (153) 155 Convergence History Computation Steering and Monitoring with log the logarithm to the base ten. On the Computation Steering/Convergence History or Task Manager/Convergence History page, the global root mean square of the residuals normalized by its value at the first iteration is shown. These values are stored in the file with extension .steering.binary. Additionally the global residuals are shown in numerical values in the Task Manager window (3rd column). The RMS value listed in the Task Manager window is the global root mean square normalized by its value at the first iteration: RMSRES(RMSRES)it=1. The maximum value (4th column) is the maximum residual at a certain iteration normalized by the RMS residual at the first iteration: MAXRES(RMSRES)it=1. FIGURE 15.3.56Task Manager window 153.6 The Graphics View (a) (b) FIGURE 15.3.67Graphics 156 view area in Computation Steering/Convergence History page FINE™ MonitorTurbo Computation Steering and Monitoring The convergence history of the selected curves are displayed inside the graphics view. In the Computation Steering/Convergence History page, the color of the curves is different (up to 8 selected quantities). The automatic chosen curves colors are also used for the displayed value (a). Additionally, the error between the two first selected quantities is also indicated (b). This is especially important for checking the difference between the mass flow at inlet and outlet (Figure 15.3.67). In the Task Manager/Convergence History page, the color of the curves is the same (but with different markers) if related to the same computation and is different for each curves if related to different computations (up to 10 selected quantities). FIGURE 15.3.68Graphics view area in Task Manager/Convergence History page 154 MonitorTurbo 154.1 Introduction The MonitorTurbo can be launched independently from FINE™ in order to facilitate the batch mode control. It is a separate graphic control window in which the user can visually monitor: • the convergence history of one or several computations (Convergence history), • the blade loading distribution (Loading diagram available with FINE™/Design 2D only), • the blade profile (Blade profile available with FINE™/Design 2D only). The two last displays are only available under the FINE™/Design 2D environments, as described in Chapter 12 and Chapter 13. This section only describes the functionalities of the convergence history display. FINE™ 157 MonitorTurbo Computation Steering and Monitoring On UNIX and LINUX platforms type: monitorTurbo print When multiple versions of FINE™ are installed the installation note should be consulted for advice on how to start FINE™ in a multiversion environment. On Windows click on the Monitor icon in Start/Programs/NUMECA software/fine#. Alternatively FINE™ can be launched from a dos shell by typing: \fine#\bin\monitor FINE™ allows multiprocess analyses. Therefore, the convergence histories of multiple (running) projects can be visualized at the same time. It is also possible to compare the convergence history associated with different computational parameters for the same project. The monitored variables are displayed as a xy graph in the upper part of the window (a). The xaxis represents the number of multigrid cycles or work units (see section 154.3.3 and Section B4.3) achieved by the flow solver. The yaxis is a logarithmic axis representing the power of ten of the residual values. The user can choose the residual of any of the equations solved and some global parameters using the buttons visible in the lower right part of the graphic control window (b) as shown in Figure 15.4.19. The lower part of the graphic control window contains four boxes. The small box (c) located on the left side contains a Print button (which allows to save the current graph as a postscript file) and a Quit button (which allows to close the MonitorTurbo window). The three other boxes are described in the next sections. . (a) (c) (b) FIGURE 15.4.19The 158 monitorTurbo window FINE™ MonitorTurbo Computation Steering and Monitoring 154.2 The Residual File Box Three buttons are provided in this box to Add, Remove or Activate residual files through a file chooser. The residual files describe the iteration process of previous or current computations. They contain the history for internal flow of the axial thrust, mass flow, torque, efficiency, pressure ratio (lift, drag and momentum coefficients if external flow) and the residuals of five (seven or six if respectively the kε or the SpalartAllmaras turbulence model is used) physical variables. The activation of a part of the residual files ’.res’ has the effect of deactivating the other loaded residual files. When a residual file is deactivated, its associated convergence history is not displayed. The selective activation of residual files allows thus to display only the convergence histories of some of the loaded residual files ’.res’. The input boxes File and Block, visible just below the three buttons Add, Remove and Activate, allow to select for which file and block the choice of the monitored variables performed in the Quantities to display menu should be applied. 154.3 Quantities to Display 154.3.1 Residuals Buttons are provided to select the type of residuals: rms or maximum as shown in Figure 15.4.19 on the right. The residuals relative to all transport equations of the problem are available: these are the continuity, the momentum, the energy, and eventually the turbulent kinetic energy k and the turbulent dissipation ε (if the turbulent computation is using a kepsilon model, e.g. not for Baldwin Lomax), and the turbulent kinematic viscosity nu (if the SpalartAllmaras model is used) or the blade force for a throughflow application. While the Computation Steering/Convergence history or Task Manager/Convergence History page displays only the global residual, the MonitorTurbo gives the RMS and maximum values per block. Computation of the RMSRES and MAXRES values is done according to Eq. 151 to Eq. 153. The values shown in the MonitorTurbo for the RMS are normalized by the value of RMSRES at the first iteration: RMSRES(RMSRES)it=1. The values shown for the maximum residuals are normalized by the maximum residual at the first iteration: MAXRES(MAXRES)it=1. Since the RMS and maximum residuals are normalized differently it may occur that the RMS value shown in the MonitorTurbo is higher than the maximum residual. 154.3.2 Global Quantities Several buttons are provided to visualize the additional global quantities available under the environment FINE™/Turbo: • Internal flow problems (expert parameter IINT=1): The axial thrust, the (inlet and outlet) mass flows, torque, pressure ratio, and efficiency. • External flow problems (expert parameter IINT=0): The drag, the lift and the momentum coefficients. The user has to specify the axis that has to be taken into account for these global quantities as described in section 113. If several computations are performed at the same time, the curves associated with the different projects are drawn in different colors. The buttons of the present box act only on the curves of the file and block selected through the File and Block menu. FINE™ 159 Computation Steering and Monitoring Best Practice for Computation Monitoring 154.3.3 Display Options The Legend button is used to display which files are currently activated. In addition, if the mass flow button is activated, the relative errors between the inlet and the outlet are indicated. The Work Unit button is provided to set the type of unit used on the horizontal axis in the MonitorTurbo window: multigrid cycles or work units. If Cycles option is chosen (Work Unit button deactivate), the abscissa will show the number of iterations, Work Unit option will adapt the values on the horizontal axis with respect to the grid levels (if 3 grid levels are used, one iteration on 222 and 111 is taking respectively 1/64s and 1/8s considering that one iteration on 000 is taking 1s. The Update now button updates the graph for the active residual file and the selected block. The Auto update button can be switched on to follow the iteration processes automatically. It is however a rather timeconsuming option and this button is not active by default. 154.3.4 Zooming Option This option allows to interactively zoom in and out: 1. In the drawing window, press the left mouse button to initiate a zooming operation, 2. Then drag the mouse to the left or to the right to zoom in, the zooming window number is displayed on the screen, 3. Click again on the left button when finished, 4. To zoom out, click on the right button of the mouse. 155 Best Practice for Computation Monitoring 155.1 Introduction Several tools are available in the FINE™/Turbo package to follow the evolution of a calculation: • the Convergence History page available in FINE™/Turbo and in the Task Manager module, which allows to follow the evolution of a calculation easily and to compare globally the evolution of multiple computations. • Another useful tool is the MonitorTurbo to compare per equation the evolution of multiple computations and per block in the domain. • CFView™ to enter even into more detail. Each of them has its own specific features, but they are very complementary. This section describes how to use those tools to monitor a computation. For a detailed description of the use of CFView™ see the separate CFView™ user’s guide. When a computation has just been launched for the first time, and initialization steps have been properly passed, the solver writes a first solution file. In fact it is not yet a solution but only the result of the initialization. Still this first output is interesting to check if all boundaries conditions have been set correctly. Especially think to have a look at the rotating elements of the machine, the profiles of velocities at inlet and at outlet. This operation aims to detect a user mistake, which could cause a loss of time, like for example, a forgotten patch. To check this first output use CFView™. To check the rotating part of the machine, select the rotating walls (hub or shroud for rotating walls) using the menu item Geometry/Select Surfaces and select for the quantity the velocity. Using the 1510 FINE™ Best Practice for Computation Monitoring Computation Steering and Monitoring Representation menu the velocity will be displayed on the selected patches and this will be the rotation speed everywhere. 155.2 Convergence History The global residual on the Convergence History page allows to see quickly whether the computation is iterating properly. The residuals should go down first on the coarser grid levels of the Full Multigrid strategy as shown in Figure 15.5.210. See Chapter 9 for more detail on Full Multigrid. When going to a finer grid level the global residual increases suddenly to decrease immediately after. When the computation reaches the finest grid, the curve of the global residual should normally decrease gradually. In general a fall of 3 orders with a stabilization of this curve is considered as a good convergence. But it is important to check if other global quantities like mass flow, efficiency, pressure ratio are also stabilized and to compare the differences between massflow at inlet and outlet (in general a difference of less than 5% is acceptable). FIGURE 15.5.210Example of convergence history for global residuals 155.3 MonitorTurbo The MonitorTurbo follows the same quantities as the Convergence History, but its main interest is to offer the possibility to follow the convergence block by block. Thus, one can localize problems and, if necessary, modify the mesh in the region associated to the block, or change a boundary condition. Finally, coming back to the Task Manager, it is possible to get a deeper control, locally, by adding control points (local 3d grid point). These points allow to track in important parts of the domain, the speed, the pressure and turbulent quantities, which could be a requested information sometimes. In the case of steady computations, the values associated to these points should converge to a constant value. One additional advice is to use CFView™ during the computation with intermediate and nonconverged solutions. When having convergence problems for example CFView™ may be used to look for the zones were the residuals have too high values compared to other regions or an incorrect turbulence field. To know in which block(s) the residuals start to increase first in case of divergence problem, the MonitorTurbo may already give an indication. Combining the information from the FINE™ 1511 Computation Steering and Monitoring Best Practice for Computation Monitoring MonitorTurbo and CFView™ allows to find the cause of convergence problems in the computations. 155.4 Analysis of Residuals In some cases it may occur that the MonitorTurbo shows high RMS and maximum values of the residuals in a certain block while CFView™ shows high residuals in a different block. This difference between the two tools is caused by the different ways of representing the residuals. In CFView™ the absolute values of the residuals resulting from the flux balance are directly plotted for each cell. In CFView™ the residuals are not scaled with the cell volumes and no normalization with values at the first iteration is applied. This explains why some high maximum residuals in scaled mode can be invisible in CFView™ because they occur in small cells. Also the fact that the residuals are computed on the cell centers in the solver and shown in CFView™ on the cell corners may lead to some, minor, interpolation differences. 1512 FINE™ APPENDIX A:Governing Equations A1 Overview The flow solver integrated into the FINE™ user environment is named EURANUS ("EURopean Aerodynamic NUmerical Simulator"). EURANUS is a multipurpose code for 2D and 3D flows in complex geometries, using the latest numerical developments in CFD. A structured mesh is required and complex geometries can be easily handled through a flexible multiblock meshing procedure. This appendix describes the basic governing equations solved in EURANUS. For more detailed information on the different aspects like turbulence, fluid modeling, multi grid strategy etc., see the related chapters in this manual. A2 ReynoldsAveraged NavierStokes Equations A2.1 General NavierStokes Equations The general NavierStokes equations written in a Cartesian frame can be expressed as: ∂ U + ∇F I + ∇F V = Q , ∂t (A1) where U is the vector of the conservative variables: ρ U = ρv , ρE (A2) F I and F V are respectively the inviscid and viscous flux vectors: FINE™ A1 ReynoldsAveraged NavierStokes Equations Governing Equations ρv i ρv 1 v i + pδ 1i F li = ρv 2 v i + pδ 2i and – F vi = 0 τ i1 τ i2 ρv 3 v i + pδ 3i τ i2 ( ρE + p )v i q i + v j τ ij , (A3) where the stress and the heat flux components are given by: ∂w˜ ∂w˜ τ ij = ( µ + µ t ) i + j – 2  ( ∇w )δ ij ∂x j ∂x i 3 and q i = ( κ + κ t ) (A4) ∂ ˜ T. ∂xi (A5) Q contains the source terms: 0 Q = ρf e , Wf (A6) with f e expressing the effects of external forces and W f the work performed by those external forces: W f = ρf e ⋅ v . Other source terms are possible, like gravity, depending on the chosen functionalities. A2.2 Time Averaging of Quantities The NavierStokes equations are averaged in time. The density and the pressure are time averaged related to the instantenous value through: q = q + q' (A7) where where q is the time averaged value and q' the fluctuating part and q' = 0 (A8) The energy, velocity components and temperature are density weighted averages defined as: ρq q˜ = ρ (A9) A2.3 Treatment of Turbulence in the Equations Except for the nonlinear kε turbulence model, a firstorder closure model based on Boussinesq's assumption, is used: – ρw i ″w j ″ = µ t A2 ∂w˜ i ∂w˜ j 2 2 + –  ( ∇w˜ )δ ij –  ρkδ ij ∂ xj ∂ x i 3 3 (A10) FINE™ Formulation in Rotating Frame for the Absolute Velocity Governing Equations with w i the xi component of the relative velocity. In this equation k is the turbulent kinetic energy and is defined as: 1 k =  ρw i ″w i ″ ⁄ ρ . 2 (A11) In contrast to the laminar case, both the static pressure and the total energy contain contributions from the turbulent kinetic energy k and are defined as: 2 p* = p +  ρk , 3 (A12) 1 ˜ E˜ = e˜ +  w˜ i w i+k 2 (A13) Note that Eq. A13 does not contain a term in the angular velocity. This term is accounted for in the source term, and assuming stationary flow, corresponds to the last term of Eq. A15. A2.4 Formulation in Rotating Frame for the Relative Velocity The resulting time averaged NavierStokes equations for the relative velocities in the rotating frame of reference become: ρw˜ i ρ ρw˜ 1 p*δ 1i + ρw˜ i w˜ 1 U = ρw˜ 2 F Ii = p*δ 2i + ρw˜ i w˜ 2 ρw˜ 3 p*δ 3i + ρw˜ i w˜ 3 ρE˜ ( ρE˜ + p* )w˜ i 0 τ i1 – F vi = τ i2 (A14) τ i3 q i + w˜ j τ ij where the shorthand notation , i, in the Fvi expression, is used to denote derivatives with respect to x i . The source term vector Q contains contributions of Coriolis and centrifugal forces and is given by: 0 Q = ( – ρ ) [ 2ω × w + ( ω × ( ω × r ) ) ] (A15) 2 2 ρw∇ ( 0.5ω r ) with ω the angular velocity of the relative frame of reference. A3 Formulation in Rotating Frame for the Absolute Velocity Although the governing equations for rotating systems are usually formulated in the relative system and solved for the relative velocity components, the formulation retained for ship propeller applications or ventilators are often expressed in the relative frame of reference for the absolute velocity FINE™ A3 Formulation in Rotating Frame for the Absolute Velocity Governing Equations components. This formulation is different from the one generally used to solve internal turbomachinery problems, where the equations are solved for the relative velocity. The two formulations should lead to the same flow solution. However, experience shows that the solution can be different, especially in the far field region. For propeller problems, the formulation based on relative velocities has the disadvantage that the far field relative velocity can reach high values. This induces an excess of artificial dissipation leading to a non physical rotational flow in the far field region, this dissipation being based on the computed variables. This formulation is controlled by the expert parameter IVELSY=0. This formulation is valid only if all boundary conditions are uniform in the azimuthal direction. If the flow field boundary conditions are not uniform in the azimuthal direction, the boundary conditions expressed in this formulation must be unsteady. In this case, the formulation for the relative velocity is suggested. Except for the nonlinear kε turbulence model, firstorder closure, based on Boussinesq's assumption, is used for the Reynolds stress: – ρv i ″v j ″ = µ t ∂v˜ i ∂v˜ j 2 2 + –  ( ∇v˜ )δ ij –  ρkδ ij 3 ∂ xi ∂ xi 3 (A16) with v i the xi component of the absolute velocity. The flux vectors are decomposed into Cartesian components: F I = f I1 1 x + f I2 1 y + f I3 1 z (A17) F v = f v1 1 x + f v2 1 y + f v3 1 z and ρw˜ i ρ ρv˜ 1 p*δ 1i + ρw˜ i v˜ 1 U = ρv˜ 2 F Ii = p*δ 2i + ρw˜ i v˜ 2 ρv˜ 3 p*δ 3i + ρw˜ i v˜ 3 ρE˜ ρE˜ w˜ i + p*v˜ i 0 τ i1 – F vi = τ i2 (A18) τ i3 q i + v˜ j τ ij where the shorthand notation , i, in the Fvi expression, is used to denote derivatives with respect to x i . The velocity w i is the xi component of the relative velocity. This formulation envolves thus both the absolute and the relative velocity components. The source term vector Q is given by: 0 Q = –ρ( ω × v ) , (A19) 0 with ω the angular velocity of the relative frame of reference. Other source terms are possible, like gravity, depending on the chosen functionalities. A4 FINE™ Formulation in Rotating Frame for the Absolute Velocity Governing Equations The averaged NavierStokes equations are obtained by the Favre averaging as described in section A2.2. In contrast to the laminar case, both the static pressure and the total energy contain contributions from the turbulent kinetic energy k and are defined as: 2 p* = p +  ρk , 3 (A20) 1 E˜ = e˜ +  w˜ i w˜ i + k . 2 (A21) The stress and the heat flux components are given by: ∂v˜ ∂v˜ τ ij = ( µ + µ t ) i + j – 2  ( ∇v )δ ij ∂x j ∂x i 3 and q i = ( κ + κ t ) FINE™ ∂ ˜ T, ∂ xi (A22) (A23) A5 Governing Equations A6 Formulation in Rotating Frame for the Absolute Velocity FINE™ APPENDIX B:File Formats B1 Overview This Appendix describes the files used by FINE™ and the flow solver EURANUS. It is divided in two parts. The first one gives the file format information needed to use FINE™, while the second one describes the format of the files used and produced by EURANUS. As FINE™ is intended to handle the file treatment for the user, knowing the exact format of all the files used in a simulation process is not required. This Appendix is therefore written for advanced users. In the following description, it is assumed that all the files are related to a generic project called 'project'. The chapter is divided in five sections: • files produced by IGG™, • files produced and used by FINE™, • files produced and used by the flow solver EURANUS, • files used as data profile, • resource files used to control the layout and which contain default values and reference information. To simplify the notations, it is assumed that the related mesh has a topology of one block. B2 Files Produced by IGG™ This section describes the files produced by the grid generator IGG™ and used by FINE™: • the identification file project.igg, • the binary file project.cgns, • the boundary conditions file project.bcs, • the geometry file project.geom. FINE™ B1 Files Produced by FINE™ File Formats B2.1 The Identification File: project.igg This file contains all the mesh geometric and topologic information. It is used by FINE™ to identify the mesh topology. A complete description of this file is given in the IGG™ User’s Guide. B2.2 The Binary File: project.cgns When the mesh is created and saved in IGG™, the binary file project.cgns containing the grid point coordinates is created. Later on, the solver will store the wall distances used for the different turbulence models in the same file. B2.3 The Geometry File: project.geom When the mesh is created and saved in IGG™, the geometry file project.geom containing the whole geometry (curves, surfaces and cartesian points) is created. B2.4 The Boundary Condition File: project.bcs As described in Chapter 8, the settings of the boundary condition type have to be set inside IGG™ while the physical boundary condition parameters are set in FINE™. The settings of IGG™ are stored in the file project.bcs. This files is used by FINE™ to initialize the boundary condition types for each patch. They are updated each time the boundary condition type is changed inside IGG™. B3 Files Produced by FINE™ This section describes the files produced and used by FINE™ (or used by the flow solver EURANUS launched from FINE™). Please note that FINE™ acts as a file manager between different software systems. Therefore, it is important that the read, write and execute permissions are set properly for all the files and directories used by FINE™. B3.1 Manual modification of these files is not supported since it may corrupt the file or provide incorrect results. Such a modification should only be done on explicit advice of NUMECA support team (support@numeca.be). The Project File: project.iec This file contains all the information related to the project. It is used by FINE™ to save and recover all the user settings. This file is subdivided into several blocks. Each block contains data and/or other blocks. The beginning of the blocks is identified by the key word NI_BEGIN and by a name and the end of the block is identified by the key word NI_END and by the name of the block. a) File Header The file always has the following header containing the version number and the project type: NUMECA_PROJECT_FILE VERSION 5.0 PROJECT_TYPE STRUCTURED After the header, 3 new lines are used to store the name of the files linked to the project: B2 FINE™ Files Produced by the Flow Solver EURANUS File Formats GRID_FILE /usr/_turnkey_tutorials/_rotor37/rotor37/_mesh/rotor37.igg TRB_FILE /usr/_turnkey_tutorials/_rotor37/rotor37/rotor37.trb GEOMETRY_FILE /usr/_turnkey_tutorials/_rotor37/rotor37.geomTurbo These are respectively the mesh, the template and the geometry files. The template and the geometry files are not used by FINE™/Turbo and are only there for backward compatibility reasons. b) The Computation Block The project file contains the settings of all the computations defined by the user. Each computation block is identified by the following keywords: NI_BEGIN computation ... NI_END computation The computation block contains the following subblocks: • The Solver Parameters Section block containing all the parameters of the solver EURANUS. • The Initial Solution & Boundary Condition Section block containing the initial solution and the boundary conditions. • The BladetoBlade Parameters Section block containing all the parameters of the bladetoblade module. • The Grid Parameters Section block containing the topology of the mesh. • The Fluid Properties Section block containing the fluid properties. B3.2 The Computation File: project_computationName.run When the solver is started, FINE™ creates a new directory using the name of the active computation. A subproject file (’.run’ extension) containing the settings of the active computation is saved into this new directory. This file is used as input by the flow solver EURANUS and by the flow visualization system CFView™. B4 The menu File/Save Run Files enables to save the ’.run’ file without starting the solver EURANUS. Files Produced by the Flow Solver EURANUS This section describes the files produced and used by the flow solver EURANUS. The flow solver uses most of the files described above and produces the following files: B4.1 The cgns file: project_computationName.cgns This binary file contains the flow solution. It is used to restart the solver and also by CFView™ to visualize the flow field. The data structure is the following: 1. For block i= 1 to n: The primitive flow variables: density, velocity components, pressure. These are computed at cell centers and are used for restart. Depending on the type of computation, temperature or turbulent quantities such as k, ε or µt are also stored. FINE™ B3 Files Produced by the Flow Solver EURANUS File Formats 2. For block i= 1 to n: The grid point coordinates and the 3D output flow variables as selected by the user through FINE™ (see Chapter 11). This data will be read by CFView™. Flow quantities are interpolated at mesh nodes by the flow solver as required by CFView™ (see section 114 for mathematical details). If the user selected solid data output, azimuthal averaged output or surface averaged output (see Chapter 11), the corresponding mesh coordinates and computed quantities are added to the corresponding ’.cgns’ file. B4.2 The mf file: project_computationName.mf This ASCII file contains averaged quantities over the inlet, outlet and rotorstator sections. It is generated only if both inlet and outlet boundary conditions are present. B4.3 The res file: project_computationName.res This file contains the residual values for all blocks for each iteration of a computation as described in section 154.3.1. It is continuously updated during the computation. It is used by the MonitorTurbo to visualize the convergence history. The format of this file is the following: • line 1: Version line. • line 2: Number of blocks. • line 3: 3D or 2D. • line 4: NOKEPS or KEPS or SPLALM. • line 5: Number of chemistry species (not used, for backward compatibility only). • line 6: STEADY or UNSTEADY. • line 7: TURBO (not used, for backward compatibility reasons only). • For iteration i=1 to itmax Iteration number, Total iteration number (for unsteady computations only), Work unit, CPU time, Physical time (for unsteady computations only), Lift, Drag, Torque, Qmax, Tmax, Mass flow in and out. For block j = 1 to n: RMS residual for the density ρ, the 3 momentum components (ρvx, ρvy, ρvz), the energy e, the turbulent variables k, ε and υ, and the same data for the maximum residual. Where: Iteration number = the number of iterations. For unsteady computations it includes the number of iterations performed in stationary mode to initialize the unsteady computation. Total iteration number = the total number of iterations including the dualtime step subiterations and the initial stationary iterations. Work unit: for single grid computations, one work unit is equal to one iteration, while in multigrid, the work unit corresponds to the computing effort of the multigrid run to the single grid run. For 3D cases it is computed as follow: WU = 1 + n2(1/2)3 + n3(1/2)6 +... While for 2D: WU = 1 + n2(1/2)2 + n3(1/2)4 +... where nx is the number of iteration done on the xth multigrid level B4 FINE™ Files Produced by the Flow Solver EURANUS File Formats Σ R es  (see section 154.3). 2 RMS is the root mean square of the residual, defined by n Physical time = the physical time step. Lift, Drag and Torque are scalar values corresponding respectively to the projection of the force vector along a lift direction (IDCLP), a drag direction (IDCDP) and a torque direction (IDCMP). These directions are controlled by the real expert parameters "IDCLP", "IDCDP", "IDCMP" in FINE™ (on the Computation Steering/Control Variables page in expert mode) as described in section 112.5.1 and section 113.2. For internal flows (expert parameter IINT=1): • Qmax = efficiency between inlet and outlet, • Tmax = total pressure ratio between inlet and outlet. For external flows (expert parameter IINT=0): • Qmax = maximum heat flux on surface = k*Grad T*n, • Tmax = maximum static temperature. Mass flow in/out = total mass flow for both inlet and outlet boundaries. When no inlet or outlet is present in the computation, the corresponding mass flow is set to zero. Finally, the ".res" file is given with the CPU time included. In case of parallel computations the wall clock time will be given instead of the CPU time. B4.4 The log file: project_computationName.log This ASCII file contains all the information related to the current computation. It contains a summary of the computation variable as well as warnings and error messages. If the flow solver encounters a problem, the latter is described in the ’.log’ file. This file is for support purposes only. When a problem appears please send this file together with a detailed problem description to NUMECA support team at support@numeca.be. B4.5 The std file: project_computationName.std This ASCII file contains all the information related to the current computation. It contains the whole content of the Task Manager window as well as warnings and error messages. If the flow solver encounters a problem, the latter is described in the ’.std’ file. This file is for support purposes only. When a problem appears please send this file together with a detailed problem description to NUMECA support team at support@numeca.be. B4.6 The wall file: project_computationName.wall This selfexplained ASCII file gives information about forces and torques on the patches for which the Compute force and torque button is activated on the Boundary Conditions page in the Solid thumbnail (see section 82.4). FINE™ B5 Files Produced by the Flow Solver EURANUS File Formats B4.7 The aqsi file: project_computationName.aqsi This ASCII temporary file is created and read by the code to ensure a smooth restart in the presence of quasisteady rotorstator interfaces. B4.8 The Plot3D files The Plot3D output module of EURANUS creates 4 files. • The project_computationName.g file contains the grid data. • The project_computationName.q file contains the conservative variables. • The project_computationName.f file contains additional variables. • The project_computationName.name file contains the names of the additional variables. The first 3 files can be written in ASCII or binary format, the binary format being the Fortran unformatted format. The .name file is always written in ASCII. When the "Unformatted file (binary)" FORTRAN format is selected in FINE™: the user has to make sure that the file format is also correctly defined in CFView™. When opening the Plot3D project in CFView™ through the menu File/Open Plot3D Project... , click on the File Format... button and select Unformatted. Do not select Binary as it corresponds to binary files generated by C programs. Once this is done, the user also needs to check the "binary low endian" or "binary big endian" format on the same page. On PC platforms (Windows or LINUX) make sure to use "binary low endian" format whereas "binary big endian" is mandatory on all other platforms. 1. The project_computationName.g file format: • Line1: number of blocks, • Line2: the 3 dimensions of each block, • for each block, the coordinates of the mesh points. 2. The project_computationName.q file format: • Line1: number of blocks, • Line2: the 3 dimensions of each block, • for each block: the free stream mach number, the flow angle, the Reynolds number and the time, the 5 conservative unknowns: density, the 3 momentum components and energy. 3. The project_computationName.f file format: • Line1: number of blocks, • Line2: for each block, the 3 dimensions and the number of additional variables selected by the user, • for each block: the additional flow variables. 4. The project_computationName.name file format: This file contains the names of the additional variables stored in the ’.f’ file, one name per line. If the quantity is a vector, it will be written on 3 different lines like in the following example: B6 FINE™ Files Used as Data Profile File Formats VelocityX VelocityY VelocityZ B4.9 The me.cfv file: project_computationName.me.cfv This ASCII file contains data required for the visualization of the meridional averaged output under CFView™. It is created whenever the user specifies variables in the Outputs/Azimuthal Averaged Variables page of the FINE™ interface. B5 Files Used as Data Profile This section describes the files created by the user and used as input data for the boundary conditions and for the fluid model. Once these files are read by the interface, they are imported in the ’.iec’ file described in section B3. The flow solver does not read these files, it retrieves the profiles from the computation definition file with extension ’.run’. Profiles may also be specified by entering the coordinates directly into the profile viewer, as described in section 212. The imported values will be interpreted in the current project units. These values would change (in the database) if the user changes the corresponding units. Therefore all values will be converted for the flow solver EURANUS in SI system units (in radians for the angles). The values for 1D profiles should be given in increasing order of the xcoordinate. For example, when entering a profile of temperature as a function of R, FINE™ checks whether the two first points are in increasing order. If this is not the case, the profile will be inverted automatically in order to ensure compatibility with the flow solver. The next time the Profile Manager ( opened, the profile will be shown in increasing order, contrary to what was initially entered. ) is For 2D profiles there is no such constraint except for profiles as a function of rθ (see section 42.3.2). B5.1 Boundary Conditions Data When defining the inlet (or outlet) boundary condition parameters, the user has the option of specifying one or several input files containing each a data profile. These profiles are used to compute by interpolation the corresponding physical variables at the inlet (or outlet). The file containing the profile must be created by the user and its name must possess the ’.p’ extension. The values of the physical variable stored in this file can come from any source: experiments, previous computations, etc. The format used to create this file contains: • Line 1: • Line 2: Two strings defining the name of the coordinate axes. Type of interpolation and number of points of the profile curve. The types are: 0 for data given at each cell centre 1,2,3,4 and 5 for 1D interpolation respectively along x, y, z, r and θ. 51 for 2D interpolation along x and y. 52 for 2D interpolation along x and z. FINE™ B7 Files Used as Data Profile File Formats 53 for 2D interpolation along y and z. 54 for 2D interpolation along r and θ. 55 for 2D interpolation along r and z. 56 for 2D interpolation along θ and z. The theta angle is defined as θ = arctg (y/x). The θ profile should cover the patch geometry, so it may take negative values. For unsteady calculations with profile rotation the θ profile must be given form 0 to 2π (see section 42.3.2). For time dependant profiles the interpolation type is 100. • The next lines contain the coordinate(s) of each point with the associated physical value. Example 1: r pressure 45 0.5 101000 0.6 102000 0.6 103000 0.7 102000 0.8 101000 This example is related to the interpolation of the pressure along the radius. There are 5 point coordinates in the file. This is a space profile. FINE™ uses the same file formats to import space, time, and space and time profiles. Thus if there is only one profile in the file, it will be interpreted as a space profile, if a second profile exists, FINE™ will recognize it as a time profile. Following is an example of a space and time profile: Example 2: R Pt 46 .3 95600.13 .251765 98913.46 .248412 100909.6 .24445 101527.6 .240182 101740.4 .23622 101811.4 100 10 .216713 101811.4 .210922 101872.1 .205435 101872.1 .199644 101872.1 .195682 101872.1 .191414 101872.1 .187452 101872.1 .18349 101740.4 .179222 99946.98 .1 99946.98 B8 FINE™ Files Used as Data Profile File Formats The two profiles are separated by an empty line. The interpolation type in time is specified as 100. If this file is imported with the profile viewer invoked as "fct(space)" only the first part will be taken into account. If "fct(time)" is specified  only the second part will be read by the flow solver. Both profiles will be imported if "fct(spacetime)" is specified for the variable type. If there are less coordinates supplied than the number of points specified, FINE™ will put zero for the missing coordinates. B5.2 Fluid Properties Fluid properties like Cp or Gamma or the viscosity can be input in the solver as constant but can also be input as variables in function of the temperature. The format used is the following: • Line 1: Two strings: "T" and the name of quantity considered ("P" and "Density" for barotropic law). • Line 2: Contains two integers: — the first number is the type of interpolation: 11 for Temperature and 12 for Pressure (barotropic profiles only), — the second one defines the number of points on the profile curve. • The next lines list the data of each point: temperature and the fluid property. Example 1: T Mu 11 5 270 6e5 275 3e5 280 2e5 290 1.5e5 300 0.9e5 It is recommended to cover the whole temperature range of the problem. The format for the Cp and Gamma profiles is slightly different because the two profiles are specified in the same file (with extension .heat_capacity). It is as shown in the example below: Example 2: T Cp 11 4 295 1004.9 298 1005.3 301 1010.8 318 1011.0 11 3 296 1.31 298 1.34 303 1.36 FINE™ B9 Resource Files File Formats The first set of points is for the Cp profile, the second is for the Gamma profile as functions of the temperature. B6 Resource Files All the resource files are located in the same directory, which is ~/COMMON under UNIX and ~\bin under Windows. It is not possible to start FINE™ if any of these files is missing. B6.1 Boundary Conditions Resource File euranus_bc.def This file contains the default values for all parameters of the available boundary conditions. The same file is also used to create the graphical layout of the page Boundary Conditions in FINE™. FINE™ only reads from this file so this file is not modified while using FINE™. B6.2 Fluids Database File euranus.flb This file contains all the data relative to the fluids created by the users in the page Configuration/ Fluid Model. This file is overwritten each time a user quits FINE™ after modifying the fluids database (add, remove, or modify a fluid). All the users should have read and write permissions for this file. It is not recommended to modify this file manually. B6.3 Units Systems Resource File euranus.uni This file contains the conversion factors for all physical quantities used in FINE™ for all possible combinations between existing systems of units. To add a new units system the user should add the corresponding conversion factors following the existing format shown in the extract below: ... # new units can be added by respecting the format # for UNITS NAMES AND CONVERSION FACTORS # NOTE: VALUE_UNITS_NAME value should NOT begin with capital letter ! # # # these are the names of the systems # used to change all the quantities at the same time DEFAULT_SYSTEM SI DEFAULT_SYSTEM Default DEFAULT_SYSTEM American 1 DEFAULT_SYSTEM American 2 # #  B10 FINE™ Resource Files File Formats # this is the system that will be taken as default # when creating a new project NEW_PROJECT_DEFAULT_SYSTEM Default #  #  UNITS NAMES AND CONVERSION FACTORS NI_BEGIN UNITS_RECORD NUMBER_OF_SYSTEMS 4 VALUE_UNITS_NAME length UNITS_NAME 1 [m] CONV_FACTOR 1 2 1. CONV_FACTOR 1 3 3.280839895 CONV_FACTOR 1 4 39.37007874 UNITS_NAME 2 [m] CONV_FACTOR 2 1 1. CONV_FACTOR 2 3 3.280839895 CONV_FACTOR 2 4 39.37007874 UNITS_NAME 3 [ft] CONV_FACTOR 3 1 0.3048 CONV_FACTOR 3 2 0.3048 CONV_FACTOR 3 4 12. UNITS_NAME 4 [in] CONV_FACTOR 4 1 0.0254 CONV_FACTOR 4 2 0.0254 CONV_FACTOR 4 3 0.08333333333 NI_END UNITS_RECORD NI_BEGIN UNITS_RECORD NUMBER_OF_SYSTEMS 4 VALUE_UNITS_NAME mass UNITS_NAME 1 [kg] CONV_FACTOR 1 2 1. CONV_FACTOR 1 3 0.06852176586 CONV_FACTOR 1 4 0.005710147155 UNITS_NAME 2 [kg] CONV_FACTOR 2 1 1. CONV_FACTOR 2 3 0.06852176586 CONV_FACTOR 2 4 0.005710147155 UNITS_NAME 3 [lbf s2/ft] FINE™ B11 File Formats Resource Files CONV_FACTOR 3 1 14.59390294 CONV_FACTOR 3 2 14.59390294 CONV_FACTOR 3 4 0.08333333333 UNITS_NAME 4 [lbf s2/in] CONV_FACTOR 4 1 175.1268352 CONV_FACTOR 4 2 175.1268352 CONV_FACTOR 4 3 12. NI_END UNITS_RECORD ...... If, for example, a new system is added on the fifth position, the user should supply the factors to convert the physical quantities from all the existing systems (1, 2, 3, and 4) to the fifth, and back from the fifth to all the others as shown below: NI_BEGIN UNITS_RECORD NUMBER_OF_SYSTEMS 5 VALUE_UNITS_NAME length UNITS_NAME 1 [m] CONV_FACTOR 1 2 1. CONV_FACTOR 1 3 3.280839895 CONV_FACTOR 1 4 39.37007874 CONV_FACTOR 1 5 new_factor_value_from_1_to_5 UNITS_NAME 2 [m] CONV_FACTOR 2 1 1. CONV_FACTOR 2 3 3.280839895 CONV_FACTOR 2 4 39.37007874 CONV_FACTOR 2 5 new_factor_value_from_2_to_5 UNITS_NAME 3 [ft] CONV_FACTOR 3 1 0.3048 CONV_FACTOR 3 2 0.3048 CONV_FACTOR 3 4 12. CONV_FACTOR 3 5 new_factor_value_from_3_to_5 UNITS_NAME 4 [in] CONV_FACTOR 4 1 0.0254 CONV_FACTOR 4 2 0.0254 CONV_FACTOR 4 3 0.08333333333 CONV_FACTOR 4 5 new_factor_value_from_4_to_5 UNITS_NAME 5 [new_units_name] CONV_FACTOR 5 1 new_factor_value_from_5_to_1 CONV_FACTOR 5 2 new_factor_value_from_5_to_2 CONV_FACTOR 5 3 new_factor_value_from_5_to_3 CONV_FACTOR 5 4 new_factor_value_from_5_to_4 NI_END UNITS_RECORD B12 FINE™ Resource Files File Formats The default units sytem can be changed by modifying the line NEW_PROJECT_DEFAULT_SYSTEM Default with the name of the desired system. FINE™ The first (SI) and the second (default) systems are identical except for the rotational speed units (RPM vs. radian). B13 File Formats B14 Resource Files FINE™ APPENDIX C:List of Expert Parameters C1 Overview On the Control Variables page under Expert Mode a list of noninterfaced expert parameters is available. As stated in the interface these parameters should not be used unless explicitly stated in this manual. This chapter contains a list of all noninterfaced expert parameters that are described in this manual. For each parameter a reference is given to the corresponding section. If more information is desired on another parameters please contact NUMECA support at support@numeca.be. C2 List of Integer Expert Parameters CLASID: COOLFL: EFFDEF: I2DLAG: IADAPT: IATFRZ: IBOTH: IBOUND: ICODKE: ICOPKE: ICYOUT: IFACE: IFNMB: IFNMFI: IFRCTO: IHXINL: IINT: IKELED: IKENC: IMASFL: IMTFIL: INEWKE: FINE™ class of particles for CFView™ output select cooling/bleed through external file and version efficiency definition simplification of Lagrangian module parametrised target distribution mutligrid parameter for Baldwin Lomax time discretization reflection treatment of particles on solid wall activation of compressible dissipation pressure gradient velocity model solution overwritten every NOFROT timesteps spatial discretization transform PERNM boundaries in FNMB reading full nonmatching data from file activate partial torque output inlet boundary condition for condensable fluid internal or external flow activation of LED scalar scheme for kε nonconservative approach for kε mass flow extrapolation at inlet instead of velocity initial solution for kε definition of high Reynolds kε model section 72.5 section 74.3 section 113.2 section 72.5 section 132.5 section 43.4 section 93.2 section 7.22 section 43.4 section 43.4 section 42.2 section 93.2 section 42.2 section 54.3.4 section 82.4.3 section 32.9 section 113.2 section 43.4 section 43.4 section 83.2 section 104.3 section 43.4 C1 List of Expert Parameters INIKE: INVMOD: INVSPL: IOPTKE: IPROLO: IRESTR: IRGCON: IROEAV: IRSMCH: IRSNEW: IRSVFL: ISIDAT: ITFRZ: ITHVZM: ITRWKI: ITYSTO: IUPWTE: IVELSY: IWAVVI: IWRIT: IYAP: KEGRID: KOUTPT: LIPROD: LMAX: MAXNBS: MGRSTR: MGSIMP: MXBFSZ: NIBOUND: NCLASS: NPERBC: NQSTDY: NREPET: NSUBM: NTUPTC: OUTTYP: THINI: VISNUL: ZMNMX: List of Float Expert Parameters initial solution for kε restart of inverse design inverse design of splitter blades optimized implementation for kε multigrid prolongation order multigrid restriction order real gas modelling upwind discretization residual smoothing rotorstator interaction viscous fluxes treatment at R/S interface rotorstator connectivity structure freezing of turbulent viscosity definition of flow angle in throughflow wake induced transition through AGS model storage of the energy upwind discretization for turbulence equations relative frame of reference spatial discretization writing of global performance data Yap’s modification for turbulent length scale switch from BaldwinLomax to kepsilon model particles trajectories output linear production term maximum number of segments in Lagrangian module maximum number of injection sectors multigrid strategy multigrid strategy maximum buffer size reflection treatment of particles on solid wall maximum nuber of classes inlet/outlet signal periodicity update rotorstator boundary condition calculation of the wall distance number of subdomains in calculation of wall distance number of patches in calculation of wall distance select type of output throughflow underrelaxation central discretization indication of injector positions in cooling/bleed section 104.3 section 132.5 section 132.5 section 43.4 section 93.2 section 93.2 section 32.9 section 93.2 section 93.2 section 54 section 55.4 section 54 section 43.4 section 64 section 75.3 section 32.9 section 4.3.4 section A3 section 93.2 section 113.2 section 43.4 section 4.3.4 section 72.5 section 43.5 section 72.5 section 7.43 section 93.2 section 93.2 section 144.4 section 72.5 section 72.5 section 4.22 section 54 section 43.4 section 43.4 section 43.4 section 113.2 section 64 section 93.2 section 74.3 C3 List of Float Expert Parameters ALF: ALPHAP: ANGREL: C3: CDIDTE: CE1: CE2: C2 constant for compressible dissipation preconditioning parameter relative angles for the inlet boundary conditions constant for kε model central discretization constant for kε model constant for kε model section 43.4 section 43.8 section 83 section 43.4 section 93.2 section 43.4 section 43.4 FINE™ List of Float Expert Parameters CMU: COOLRT: CP1: CREF: DDIMAX: DIAMR: EKCLIP: ENTRFX: EPCLIP: EXPMAR: FTRAST: GAMMAT: IDCDP: IDCLP: IDCMP: IRKCO: ISWV: IXMP: LTMAX: MAVREM: MAVRES: MUCLIP: NUTFRE: PRCLIP: PRT: RADAPT: RELAXP: RELPHL: RESFRZ: RGCST: RSMPAR: RTOL: SIGE: SIGK: SIGRO: SMCOR: SREF: TEDAMP: THFREL: VELSCA: VIS2: VIS2KE: VIS4: VIS4KE: FINE™ List of Expert Parameters constant for kε model section 43.4 reduction of mass flow in cooling holes section 74.3 constant for compressible dissipation section 43.4 reference chord for nondimensionalizing section 113 tolerance factor for Lagrangian module section 72.5 diameter ratio for Lagrangian module section 72.5 clipping value for turbulent kinetic energy section 43.4 upwind discretization section 93.2 clipping value for turbulent kinetic dissipation section 43.4 central discretization section 93.2 forbid transition before FTRAST*chord with AGS model section 75.3 turbulence time scale section 43.4 direction of drag or axial thrust section 113.2 direction of lift section 113.2 direction of moment or torque section 113.2 RungeKutta coefficients section 93.2 RungeKutta dissipative residuals section 93.2 definition of point for moment or torque section 113.2 maximum turbulent length scale section 43.4 control of multigrid correction for k and ε section 43.4 update control of k and ε section 43.4 clipping value for Mut/Mu for k and ε and SpalartAllmaras section 43.4 initial value of turbulent viscosity for Spalart Allmaras section 43.3 turbulence parameter section 43.4 turbulent Prandtl number section 43.4 parametrised target distribution section 132.5 underrelaxation for mass flow imposed at outlet section 83 relaxation factor for PhaseLagged section 4.2.2 freeze turbulent viscosity field section 43.4 value of the gas constant section 32.9 residual smoothing parameter section 93.2 maximum angle for normals in calculation wall distance section 43.4 constant for kε model section 43.4 constant for kε model section 43.4 constant for kε model section 43.4 residual smoothing section 93.2 reference surface to nondimensionalize coefficients section 113 damping for ke model section 43.4 throughflow underrelaxation section 64 maximum value allowed for velocity scaling section 83 central discretization section 93.2 central discretization section 93.2 central discretization section 93.2 central discretization section 93.2 C3 List of Expert Parameters C4 List of Float Expert Parameters FINE™ Characteristics of Water (steam) Tables APPENDIX D: D1 Overview As described in section section 32.3.4, the Condensable Fluid module aims at the modelling of the real thermodynamic properties of a given fluid by means of interpolation of the variables from dedicated tables. The approach that has been adopted in EURANUS consists of using a series of thermodynamic tables, one table being required each time a thermodynamic variable must be deduced from two other ones. This implies the creation of many tables as input, but presents the advantage that no iterative inversion of the tables is done in the solver, with as a consequence a very small additional CPU time. Information related to • the range of variation of admissible values for thermodynamic variables • the discretization of the grid • the nature of the interpolation algorithm selected • the relative mean error (mean and maximum) on thermodynamic variables • the size of the table is discussed here below for water (steam) tables. D2 Main Characteristics Water (steam) tables come in the form of 11 tables, described as follows: TER: PER: RPT: EPT: SHP: PHS: FINE™ interpolates static temperature as a function of internal energy and density interpolates static pressure as a function of internal energy and density interpolates density as a function of static pressure and temperature interpolates internal energy as a function of pressure and static temperature interpolates entropy as a function of total enthalpy and static pressure interpolates static pressure as a function of entropy and total enthalpy D1 Main Characteristics Characteristics of Water (steam) Tables RHS: HSP: MER: KER: PSA: interpolates static pressure over density as a function of entropy and total enthalpy interpolates total enthalpy as a function of entropy and static pressure interpolates dynamic viscosity as a function of internal energy and density interpolates thermal conductivity as a function of internal energy and density defines the saturation line Tables Variables Minimum Maximum TER / PER Energy [J/kg] 500,000 4,000,000 Density [kg/m3] 0.001 1,020 Pressure [bars] 0.0003 26,600 Temperature [K] 237 1,630 Pressure [bars] 0.002 24,000 Temperature [K] 250 1,350 Density [kg/m3] 0.00032 1,432 Energy [J/Kg] 187,568 4,212,000 Enthalpy [J/kg] 99,726 5,500,000 Enthalpy [J/kg] 1,500,000 4,500,000 Pressure [bars] 0.002 24,000 Entropy [J/kg/K] 1,582 12,733 Enthalpy [J/kg] 1,850,000 4,500,000 Entropy [J/kg/K] 2,000 10,500 Pressure [bars] 0.00021 46,700 Enthalpy [J/kg] 1,655 50,000,000 Entropy [J/kg/K] 0 13,000 Pressure [bars] 0.002 24,000 Energy [J/Kg] 500,000 4,000,000 0.001 500 Viscosity [Pa.s] 0.0000085 0.00013 Conductivity [W/m/K] 0.015 0.58 RPT / EPT SHP PHS / RHS HSP MER / KER Density [kg/m TABLE 1. Admissible 3] range of variations for thermodynamic variables Table 1 on page 2 lists the range of admissible variations for the thermodynamic variables, in the different tables proposed. Ranges have been extended from the default tables proposed up to FINE™ /Turbo v6.27, especially at low pressures (< 1000 Pa). Significant improvements, both in terms of robustness and accuracy, are expected in that area. D2 FINE™ Main Characteristics Characteristics of Water (steam) Tables Tables Grid Interpolation Error RMS [%] Error Maximum [%] Size [Mb] PER 71 x 71 bicubic (double precision) 0.02 80.7 3.2 TER 71 x 71 bicubic (double precision) 0.014 1.7 3.2 RPT 101 x 101 bicubic (single precision)  < 0.1 3.3 EPT 101 x 101 bicubic (single precision)  < 0.1 3.3 SHP 41 x 41 bicubic (single precision) 0.0015 0.008 0.5 PHS 81 x 81 bicubic (single precision) 0.005 5.8 2.1 RHS 81 x 81 bicubic (double precision) 0.026 9.7 4.2 HSP 81 x 81 bicubic (single precision) 0.0003 0.01 2.1 MER 41 x 61 bicubic (double precision) 0.126 8.7 1.6 KER 41 x 61 bicubic (double precision) 2.02 27.2 1.6 PSA 120 cubic   0.1 TABLE 2. Main characteristics of water (steam) thermodynamic tables Both RMS (root mean square) and maximum errors should be interpreted as relative errors. RMS error does not exceed 2%, while in most tables it is ranging from 0.0001% to 0.1%. Maximum relative errors are located nearby the saturation line, where the interpolation naturally degrades despite the use of bicubic double precision algorithms. Tables RPT and EPT have been tuned so as to guarantee maximum accuracy in the vapor phase (< 0.1% at maximum). However, run performed in the liquid phase are consequently prohibited since they would lead to large relative errors (> 100%) in that area. A dedicated set covering RPT and EPT tables balancing maximum relative errors both on vapor and liquid phases can however be obtained upon request. Please take direct contact at support@numeca.be for any question on this purpose. FINE™ D3 Characteristics of Water (steam) Tables D4 Main Characteristics FINE™ Index INDEX A AbuGrannamShaw Model 741 Add Fluid 33 ANSYS Outputs 1110 AutoBlade 23, 210 AutoGrid 12, 23, 25, 210 Axial Thrust 811, 1115 Azimuthal Averaged Output 119 B Background Color 17 Barotropic Liquid, see Fluid, Barotropic Liquid BenedictWebbRubin 313 Blade To Blade 121–?? Boundary Conditions 128 File Formats 1213–1217 Flow Solver 1212 Geometrical Data 123 Initial Solution 1210, 135 Input Files 1213–1215 Inverse Design 128 Mesh Generator 126, 1211 New Project 122 Numerical Model 1210 Open Project 122 Output Files 1215–1217 Stream Surface Data 124 Theory 1211 Bleed flow Data file 733 Flow Parameters 729 Outputs 731 Positioning 718 Visualization 730 Wizard 716 Block Conjugate Heat Transfer 712 Throughflow 62–63 Boundary Conditions 81 Blade To Blade 128 Lagrangian Module 74, 74–76 Rotor/Stator 517–519 Throughflow 67–68 Turbulence 416 Unsteady 42 Boussinesq 447 FINE™ C CFD Governing equations A1 Introduction 11 CFL Number 712, 92, 917 CFView™ 13–14, 210 CGNS B3 Characteristic Values, see Reference Values Computation Definition Area 212 Condensable fluid Boundary conditions 820 Outputs 114 Condensable Fluid, see Fluid, Condensable Conductivity 33–35 Laminar 310 Turbulent 310 Turbulent, Condensable Fluid 315 Conjugate Heat Transfer 711–715 Blocks Types 712 Theory 713–715 Control Variables 151 Unsteady 44 Convention 15 Convergence History 104 Cooling Theory 732, 733 Cooling flow Bleed flow 715 Data file 733 Flow Parameters 729 Outputs 731 Positioning 718 Visualization 730 Wizard 716 Create Grid File 23 Project 22, 24, 122, 132 Run Files 26 D Delete Fluid 37 Design 2D 210, 131–?? Formulation 134, 137 Input Files 133, 138 Interface 132 Output Files 139 Start 136 Theory 137–138 Design 3D 12, 23, 210 i Index INDEX Discretization Central Scheme 99–910 Limiters 912 Spatial 94, 97–913 Temporal 94 Time 917–921 Upwind Scheme 910–913 Drag 811 Drag Coefficient 1119 Driver 16 Dryness Fraction 315 Duplicate Active Project 26 E Edit Fluid 37 Efficiency 1116 Enthalpy 311, 315 Entropy 314 Euler 415 2D 61 Equations 613 EURANUS 13 EuranusTurbo Parallel Computation 148, 1417 Expert Mode 212 Expert Parameters C1, D1 External Boundary Condition 813 F File Chooser 219 File Format 69, B1 File Management 13 File Menu 24 File Names, Limitations 27 Fluid Add 33 Condensable 313–316 Delete 37 Edit 37 Incompressible 518 Interface 32 Liquid 312 List 32 Models 31–316 Perfect Gas 310 Real Gas 311 FluidParticle Interaction. See Lagrangian Module. Force 811 ii Blade 614 Friction 615 Forced Transition 738, 740 Formula Editor 36 Full Nonmatching 520 Fully Laminar 740 Fully Turbulent 740 G Gauss Theorem 98 Global Layout 27 Global Performance 1115, B4 Graphics 16 Graphics Area 216 Gravity 35, 441 Grid Create Grid File 23 Grid Generation 12–14 Units 24, 28 Group Block Rotation 52 Boundary Conditions 82 Rotor/Stator 53 H Hand Symbol 15 Host Definition 145 Hybrid Analysis 63 I Icon Bar 210 IGG™ 13, 23, 25, 210 Incompressible Fluid Model, see Fluid Model, Incompressible Local Conservative Coupling 518 Initial Solution 101–108 Blade To Blade 1210, 135 Block Dependent 101–103 Coarse Grid 93 Constant Values 103 File 104–105 Full Multigrid Strategy 916 Throughflow 68–69, 107–108 Turbomachinery 106–107 Turbulence 416 Unsteady 105 Initialization Full Multigrid Strategy 101 Unsteady 44 FINE™ Index INDEX Installation 16 Interface 17 General Description of FINE™ Interface 21–219 L Lagrangian Module Boundary Conditions 74, 74–76 Global Strategy 73 Interaction With Turbulence 710 Outputs 76 Particles Traces 77 Theory 79–711 Laminar 415 Layout 27 License 18 Lift 811 Lift Coefficient 1119 Light Bulb 15 Limitations 27, 28 Limiter Lacor 912 Minmod 912 Superbee 912 Van Albada 912 Van Leer 912 Linearization 427 LIPROD 427 Liquid, see Fluid, Liquid Local Conservative Coupling 517–?? Loss Coefficient 66 Low Speed Flow 442 M Mach Number Absolute 115 Condensable Fluid 315 Isentropic 134, 1310 Relative 115 Mathematical Model 415 Menu File 24 Menu Bar 24 Mesh 28 Modules 210 Solver 29 Merge Merge Mesh Topology 211 Patch For Azimuthal View 119 Mesh 12–14 FINE™ Information 215 Properties 28 Selection 211 Toggles 214 View 28, 216–218 View Area 213 Modules 210 Moment 811 Momentum 1119 Monitor Convergence History 1511 Display 1510 Quantities 153 Residual File Box 159 Solution 151–1512 Steering File 153 Zoom 1510 MonitorTurbo 157 MSW Driver 16 Multigrid 92 Full 916 Prolongation 916 Strategy 93, 913–917 N New Project 24, 122, 132 Numerical Model 91 Blade To Blade 1210 O Open Project 23, 25 OPENGL Driver 16 Outputs 315, 111–1124 3D Quantity 112–117, 1120 Azimuthal Averaged 119, 1118, 1121–1123 Lagrangian Module 76 mf File 1115, 1118 Particle Traces 77 Surface Averaged 118, 1121 Theory 1120–1124 P Pair of Scissors 15 Parallel Computation 1413 Parameter Button 213 Parameters Area 22 Particles 71 Perfect Gas, see Fluid, Perfect Gas iii Index INDEX Performance 1115, B4 Periodic Boundaries 67, 89 Phase Lagged 43, 413 Plot3D 1117, B6 Post Processing 13–14 Prandtl Number 310 Preconditioning 442 Parameters 445, 93 Preferences 26 Profile Manager 219, 33–36 File Formats B7 Project Configuration 24 Creation 22 Duplicate 26 Management 13 New 24 Open 23, 25 Save 26 Units 26 Properties Fluid 31 Mesh 28 PVM Daemons 141–145 Q Quit 27 R Real Gas, see Fluid, Real Gas Reference Density 39, 447 Length 447 Pressure 35, 445 Reference Values 447 Temperature 35, 39, 445 Velocity 445, 447 Residual 116, 155, B4 Implicit Smoothing 920 Radespiel & Rossow 920 Swanson & Turkel 921 Vasta 921 Restart 210 Design 2D 136 Unsteady 45 Reynolds Number 447 Rotation Blocks 52–53 iv Rotor/Stator Domain Scaling 511–512, 521–524 FNMB Mixing Plane Coupling 519–521 Frozen Rotor 59–510, 524 Initial Solution 106 Interface 53–55 Local Conservative Coupling 517–518 Mixing Plane Coupling 55–58, 516–521 Phase Lagged 513 Pitchwise Rows Coupling 518–519 Steady 55–58, 59–510, 516–521, 524 Theory 515–524 Unsteady 511–512, 513, 521–524 Rough Wall 435 Run File 13, 26 RungeKutta Scheme 917 S Save Intermediate Solution 29 Project 26 Scripts 1414 Second Order Restart 45 SI System 26 Smooth Wall 435 Solid Data 116 Solver Menu 29 Specific Heat 310–312, 315 Standard Mode 212 Start Flow Solver 29 Stator Rotor/Stator Interface. See Rotor/Stator. Steady Rotor/Stator 55–58, 59–510, 516–521, 524 Stop Flow Solver 29 Surface Averaged Output 117 Suspend Flow Solver 29 Sutherland 39 Sutherland Law 39 T Task Definition 146 Taskmanager 141–1423 Add Host 145 Delay 146 Limitations 1422 Parallel Computation 148 PVM 141–145 FINE™ Index INDEX Remove Host 146 Scripts 1414–1422 Shutdown 146 Subtask 147–1411 Task Definition 146–1411 Tearoff Graphics 28 Temperature Reference 39 Sutherland 39 Thermal Connections 712 Thermodynamic Tables 313 Throat Control 63 Throughflow Analysis Mode 63 Blade Geometry 63–65 Block Type 62 Boundary Conditions 67–68 Expert Parameters 612 File Format 69–611 Flow Angle/Tangential Velocity 65–66 Global Parameters 62 Initial Solution 68–69, 107–108 Loss Coefficient 66 Mesh 66 Model 61–615 Theory 613–615 Time Configuration 42 Time Step Global Time 94 Local Time 94 Physical 414 Torque 811, 1115 Transition Model 737 AbuGrannamShaw Model 741 Forced Transition 738, 740 Fully Laminar 740 Fully Turbulent 740 Turbulence Boundary Condition 416 Initial Solution 416 Linearization 427 Output 117 Turbulence Models BaldwinLomax 428 kepsilon 431 Non Linear kepsilon 433 SpalartAllmaras 429 TVD 911 FINE™ U Units Grid 24, 28 Project 26 Unload Mesh 28 Unsteady 42 Boundary Conditions 42, 46, 412 Control Variables 44 Create 46 Initial Solution 105 Initialization of 47 Phase Lagged 43 Rotor/Stator 511–512, 521–524 Rotor/Stator Phase Lagged 513 Second Order in Time 45 Turbomachinery 412 User Mode 212 V Vander Waals 313 Velocity Absolute 115 Friction 421 Local Scaling 446 Projections 115 Reference 447 Relative 115 Relative Projections 115 View Area 213 View Manipulation 216 View On/Off 28, 213 Viscosity Inviscid Flux 98 Laminar 39 Turbulent 310, 439 Viscous Flux 98 Vorticity 115 W Wall Rough 435 Smooth 435 Work Unit B4 X X11 Driver 16 Z Zoom In/Out/Region 218 v