CFX Reference Guide

CFX Reference Guide
ANSYS CFX Reference Guide
ANSYS, Inc.
Southpointe
2600 ANSYS Drive
Canonsburg, PA 15317
[email protected]
http://www.ansys.com
(T) 724-746-3304
(F) 724-514-9494
Release 16.2
July 2015
ANSYS, Inc. is
certified to ISO
9001:2008.
Copyright and Trademark Information
© 2015 SAS IP, Inc. All rights reserved. Unauthorized use, distribution or duplication is prohibited.
ANSYS, ANSYS Workbench, Ansoft, AUTODYN, EKM, Engineering Knowledge Manager, CFX, FLUENT, HFSS, AIM
and any and all ANSYS, Inc. brand, product, service and feature names, logos and slogans are registered trademarks
or trademarks of ANSYS, Inc. or its subsidiaries in the United States or other countries. ICEM CFD is a trademark
used by ANSYS, Inc. under license. CFX is a trademark of Sony Corporation in Japan. All other brand, product,
service and feature names or trademarks are the property of their respective owners.
Disclaimer Notice
THIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION INCLUDE TRADE SECRETS AND ARE CONFIDENTIAL AND PROPRIETARY PRODUCTS OF ANSYS, INC., ITS SUBSIDIARIES, OR LICENSORS. The software products
and documentation are furnished by ANSYS, Inc., its subsidiaries, or affiliates under a software license agreement
that contains provisions concerning non-disclosure, copying, length and nature of use, compliance with exporting
laws, warranties, disclaimers, limitations of liability, and remedies, and other provisions. The software products
and documentation may be used, disclosed, transferred, or copied only in accordance with the terms and conditions
of that software license agreement.
ANSYS, Inc. is certified to ISO 9001:2008.
U.S. Government Rights
For U.S. Government users, except as specifically granted by the ANSYS, Inc. software license agreement, the use,
duplication, or disclosure by the United States Government is subject to restrictions stated in the ANSYS, Inc.
software license agreement and FAR 12.212 (for non-DOD licenses).
Third-Party Software
See the legal information in the product help files for the complete Legal Notice for ANSYS proprietary software
and third-party software. If you are unable to access the Legal Notice, please contact ANSYS, Inc.
Published in the U.S.A.
Table of Contents
1. ANSYS CFX Launcher .............................................................................................................................. 1
1.1. The ANSYS CFX Launcher Interface .................................................................................................... 1
1.1.1. Menu Bar ................................................................................................................................. 1
1.1.1.1. File Menu ........................................................................................................................ 1
1.1.1.1.1. Save As ................................................................................................................... 1
1.1.1.1.2. Quit ........................................................................................................................ 1
1.1.1.2. Edit Menu ....................................................................................................................... 2
1.1.1.2.1. Clear ....................................................................................................................... 2
1.1.1.2.2. Find ........................................................................................................................ 2
1.1.1.2.3. Options .................................................................................................................. 2
1.1.1.2.3.1. User Interface Style ........................................................................................ 2
1.1.1.2.3.2. Application Font and Text Window Font .......................................................... 2
1.1.1.3. CFX Menu ....................................................................................................................... 2
1.1.1.3.1. CFX-Pre .................................................................................................................. 2
1.1.1.3.2. CFX-Solver Manager ............................................................................................... 2
1.1.1.3.3. CFD-Post ................................................................................................................ 2
1.1.1.3.4. Other CFX Applications ........................................................................................... 2
1.1.1.4. Show Menu ..................................................................................................................... 3
1.1.1.4.1. Show Installation .................................................................................................... 3
1.1.1.4.2. Show All ................................................................................................................. 3
1.1.1.4.3. Show System .......................................................................................................... 3
1.1.1.4.4. Show Variables ....................................................................................................... 3
1.1.1.5. Tools Menu ...................................................................................................................... 3
1.1.1.5.1. ANSYS Client Licensing Utility ................................................................................. 3
1.1.1.5.2. Command Line ....................................................................................................... 3
1.1.1.5.3. Configure User Startup Files (Linux only) ................................................................. 4
1.1.1.5.4. Edit File .................................................................................................................. 4
1.1.1.5.5. Edit Site-wide Configuration File ............................................................................. 4
1.1.1.6. User Menu ....................................................................................................................... 4
1.1.1.7. Help Menu ...................................................................................................................... 4
1.1.2. Toolbar .................................................................................................................................... 4
1.1.3. Working Directory Selector ....................................................................................................... 4
1.1.4. Output Window ....................................................................................................................... 5
1.2. Customizing the ANSYS CFX Launcher .............................................................................................. 5
1.2.1. CCL Structure ........................................................................................................................... 5
1.2.1.1. GROUP ............................................................................................................................ 5
1.2.1.2. APPLICATION ................................................................................................................... 6
1.2.1.2.1. Including Environment Variables ............................................................................. 8
1.2.1.3. DIVIDER ........................................................................................................................... 8
1.2.2. Example: Adding the Windows Calculator ................................................................................. 8
2. Volume Mesh Import API ........................................................................................................................ 9
2.1. Valid Mesh Elements in CFX ............................................................................................................... 9
2.2. Creating a Custom Mesh Import Executable for CFX-Pre ................................................................... 10
2.2.1. Compiling Code with the Mesh Import API ............................................................................. 11
2.2.2. Linking Code with the Mesh Import API .................................................................................. 11
2.2.2.1. Linking a Customized C Mesh Import Executable on a Linux Platform ............................. 11
2.2.2.2. Linking a Customized Fortran Mesh Import Executable on a UNIX Platform ..................... 12
2.2.2.3. Linking a Customized Mesh Import Executable on a Windows Platform .......................... 12
2.3. Details of the Mesh Import API ........................................................................................................ 12
2.3.1. Defined Constants .................................................................................................................. 13
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
iii
Reference Guide
2.3.1.1. Element Types ............................................................................................................... 13
2.3.1.2. Region Types ................................................................................................................. 13
2.3.2. Initialization Routines ............................................................................................................. 14
2.3.2.1. cfxImportStatus ............................................................................................................. 14
2.3.2.2. cfxImportInit ................................................................................................................. 14
2.3.2.3. cfxImportTest ................................................................................................................ 14
2.3.3. Termination Routines ............................................................................................................. 15
2.3.3.1. cfxImportDone .............................................................................................................. 15
2.3.3.2. cfxImportTotals ............................................................................................................. 15
2.3.4. Error Handling Routines ......................................................................................................... 15
2.3.4.1. cfxImportError ............................................................................................................... 15
2.3.4.2. cfxImportFatal ............................................................................................................... 16
2.3.5. Node Routines ....................................................................................................................... 16
2.3.5.1. cfxImportNode .............................................................................................................. 16
2.3.5.2. cfxImportGetNode ........................................................................................................ 16
2.3.5.3. cfxImportNodeList ......................................................................................................... 16
2.3.6. Element Routines ................................................................................................................... 16
2.3.6.1. cfxImportElement .......................................................................................................... 16
2.3.6.2. cfxImportGetElement .................................................................................................... 18
2.3.6.3. cfxImportElementList .................................................................................................... 18
2.3.6.4. cfxImportGetFace .......................................................................................................... 18
2.3.6.5. cfxImportFindFace ......................................................................................................... 19
2.3.7. Primitive Region Routines ....................................................................................................... 19
2.3.7.1. cfxImportBegReg .......................................................................................................... 19
2.3.7.2. cfxImportAddReg .......................................................................................................... 20
2.3.7.3. cfxImportEndReg .......................................................................................................... 20
2.3.7.4. cfxImportRegion ........................................................................................................... 20
2.3.7.5. cfxImportRegionList ...................................................................................................... 20
2.3.7.6. cfxImportGetRegion ...................................................................................................... 20
2.3.8. Composite Regions Routines .................................................................................................. 21
2.3.8.1. cfxImportBegCompRegion ............................................................................................ 21
2.3.8.2. cfxImportAddCompRegComponents ............................................................................. 21
2.3.8.3. cfxImportEndCompReg ................................................................................................. 21
2.3.8.4. cfxImportCompositeRegion ........................................................................................... 21
2.3.9. Explicit Node Pairing .............................................................................................................. 21
2.3.9.1. cfxImportMap ............................................................................................................... 22
2.3.10. Fortran Interface .................................................................................................................. 22
2.3.10.1. cfxinit .......................................................................................................................... 22
2.3.10.2. cfxtest ......................................................................................................................... 22
2.3.10.3. cfxunit ......................................................................................................................... 22
2.3.10.4. cfxwarn ....................................................................................................................... 22
2.3.10.5. cfxfatl .......................................................................................................................... 22
2.3.10.6. cfxdone ....................................................................................................................... 22
2.3.10.7. cfxnode ....................................................................................................................... 23
2.3.10.8. cfxnodg ....................................................................................................................... 23
2.3.10.9. cfxnods ....................................................................................................................... 23
2.3.10.10. cfxelem ..................................................................................................................... 23
2.3.10.11. cfxeleg ...................................................................................................................... 23
2.3.10.12. cfxeles ....................................................................................................................... 23
2.3.10.13. cfxfacd ...................................................................................................................... 23
2.3.10.14. cfxface ....................................................................................................................... 24
2.3.10.15. cfxffac ....................................................................................................................... 24
iv
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Reference Guide
2.3.10.16. cfxregn ...................................................................................................................... 24
2.3.10.17. cfxregb ...................................................................................................................... 24
2.3.10.18. cfxrega ...................................................................................................................... 24
2.3.10.19. cfxrege ...................................................................................................................... 24
2.3.10.20. cfxregs ...................................................................................................................... 25
2.3.10.21. cfxregg ...................................................................................................................... 25
2.3.10.22. cfxcmpb .................................................................................................................... 25
2.3.10.23. cfxcmpa .................................................................................................................... 25
2.3.10.24. cfxcmpe .................................................................................................................... 25
2.3.11. Unsupported Routines Previously Available in the API ........................................................... 25
2.4. An Example of a Customized C Program for Importing Meshes into CFX-Pre ..................................... 26
2.5. Import Programs ............................................................................................................................ 26
2.5.1. ANSYS .................................................................................................................................... 26
2.5.2. CFX Def/Res ........................................................................................................................... 27
2.5.3. CFX-4 ..................................................................................................................................... 27
2.5.4. CFX-5.1 .................................................................................................................................. 27
2.5.5. CFX-TfC .................................................................................................................................. 29
2.5.6. CGNS ..................................................................................................................................... 29
2.5.6.1. SplitCGNS.exe ................................................................................................................ 30
2.5.7. Fluent .................................................................................................................................... 30
2.5.8. GridPro/az3000 ...................................................................................................................... 30
2.5.9. I-DEAS ................................................................................................................................... 31
2.5.10. ICEM CFX ............................................................................................................................. 31
2.5.11. PATRAN ................................................................................................................................ 31
2.5.12. NASTRAN ............................................................................................................................. 32
2.5.13. CFX-TASCflow ...................................................................................................................... 32
3. Mesh and Results Export API ................................................................................................................ 33
3.1. Creating a Customized Export Program ........................................................................................... 33
3.1.1. An Example of an Export Program .......................................................................................... 34
3.1.1.1. File Header .................................................................................................................... 34
3.1.1.2. Allowed Arguments ....................................................................................................... 34
3.1.1.3. Main Program Initialization ............................................................................................ 34
3.1.1.4. Checking File Names ..................................................................................................... 36
3.1.1.5. Opening the CFX Results File ......................................................................................... 36
3.1.1.6. Timestep Setup ............................................................................................................. 37
3.1.1.7. Geometry File Output .................................................................................................... 38
3.1.1.8. Template Results File ..................................................................................................... 40
3.1.1.9. Creating Files with Results for Each Variable ................................................................... 41
3.1.2. Example of Output Produced ................................................................................................. 43
3.1.2.1. example.geom .............................................................................................................. 43
3.1.2.2. example.res ................................................................................................................... 44
3.1.2.3. example.s01 .................................................................................................................. 44
3.1.3. Source Code for getargs.c ....................................................................................................... 44
3.2. Compiling Code with the Mesh and Results Export API .................................................................... 45
3.3. Linking Code with the Mesh and Results Export API ......................................................................... 45
3.3.1. Linux ..................................................................................................................................... 46
3.3.2. Windows ................................................................................................................................ 46
3.4. Details of the Mesh Export API ........................................................................................................ 46
3.4.1. Defined Constants and Structures ........................................................................................... 47
3.4.1.1. Element Types ............................................................................................................... 47
3.4.1.2. Volume List Types .......................................................................................................... 47
3.4.1.3. Region List Types ........................................................................................................... 47
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
v
Reference Guide
3.4.1.4. Count Entries ................................................................................................................. 47
3.4.1.5. Node Data Structure ...................................................................................................... 48
3.4.1.6. Element Data Structure .................................................................................................. 48
3.4.2. Initialization and Error Routines .............................................................................................. 48
3.4.2.1. cfxExportInit .................................................................................................................. 48
3.4.2.2. cfxExportDone .............................................................................................................. 48
3.4.2.3. cfxExportError ............................................................................................................... 49
3.4.2.4. cfxExportFatal ............................................................................................................... 49
3.4.3. Zone Routines ........................................................................................................................ 49
3.4.3.1. cfxExportZoneCount ..................................................................................................... 49
3.4.3.2. cfxExportZoneSet .......................................................................................................... 49
3.4.3.3. cfxExportZoneGet ......................................................................................................... 50
3.4.3.4. cfxExportZoneFree ........................................................................................................ 50
3.4.3.5. cfxExportZoneIsRotating ............................................................................................... 50
3.4.3.6. cfxExportZoneMotionAction .......................................................................................... 50
3.4.4. Node Routines ....................................................................................................................... 50
3.4.4.1. cfxExportNodeCount ..................................................................................................... 51
3.4.4.2. cfxExportNodeList ......................................................................................................... 51
3.4.4.3. cfxExportNodeGet ......................................................................................................... 51
3.4.4.4. cfxExportNodeFree ........................................................................................................ 51
3.4.5. Element Routines ................................................................................................................... 51
3.4.5.1. cfxExportElementCount ................................................................................................. 51
3.4.5.2. cfxExportElementList ..................................................................................................... 52
3.4.5.3. cfxExportElementGet ..................................................................................................... 52
3.4.5.4. cfxExportElementFree ................................................................................................... 53
3.4.6. Region Routines ..................................................................................................................... 53
3.4.6.1. cfxExportRegionCount .................................................................................................. 53
3.4.6.2. cfxExportRegionSize ...................................................................................................... 53
3.4.6.3. cfxExportRegionName ................................................................................................... 53
3.4.6.4. cfxExportRegionList ....................................................................................................... 53
3.4.6.5. cfxExportRegionGet ...................................................................................................... 54
3.4.6.6. cfxExportRegionFree ..................................................................................................... 54
3.4.7. Face Routines ......................................................................................................................... 54
3.4.7.1. cfxExportFaceNodes ...................................................................................................... 54
3.4.8. Volume Routines .................................................................................................................... 55
3.4.8.1. cfxExportVolumeCount .................................................................................................. 55
3.4.8.2. cfxExportVolumeSize ..................................................................................................... 56
3.4.8.3. cfxExportVolumeName .................................................................................................. 56
3.4.8.4. cfxExportVolumeList ...................................................................................................... 56
3.4.8.5. cfxExportVolumeGet ..................................................................................................... 56
3.4.8.6. cfxExportVolumeFree .................................................................................................... 56
3.4.9. Boundary Condition Routines ................................................................................................. 56
3.4.9.1. cfxExportBoundaryCount .............................................................................................. 57
3.4.9.2. cfxExportBoundaryName ............................................................................................... 57
3.4.9.3. cfxExportBoundaryType ................................................................................................ 57
3.4.9.4. cfxExportBoundarySize .................................................................................................. 57
3.4.9.5. cfxExportBoundaryList .................................................................................................. 57
3.4.9.6. cfxExportBoundaryGet .................................................................................................. 58
3.4.9.7. cfxExportBoundaryFree ................................................................................................. 58
3.4.10. Variable Routines .................................................................................................................. 58
3.4.10.1. cfxExportVariableCount ............................................................................................... 58
3.4.10.2. cfxExportVariableSize .................................................................................................. 58
vi
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Reference Guide
3.4.10.3. cfxExportVariableName ............................................................................................... 59
3.4.10.4. cfxExportVariableList ................................................................................................... 59
3.4.10.5. cfxExportVariableGet ................................................................................................... 59
3.4.10.6. cfxExportVariableFree .................................................................................................. 60
4. Remeshing Guide .................................................................................................................................. 61
4.1. User Defined Remeshing ................................................................................................................. 62
4.1.1. Remeshing with Key-Frame Meshes ........................................................................................ 63
4.1.2. Remeshing with Automatic Geometry Extraction .................................................................... 63
4.2. ICEM CFD Replay Remeshing ........................................................................................................... 64
4.2.1. Steps to Set Up a Simulation Using ICEM CFD Replay Remeshing ............................................. 66
4.3. Directory Structure and Files Used During Remeshing ..................................................................... 67
4.4. Additional Considerations ............................................................................................................... 68
4.4.1. Mesh Re-Initialization During Remeshing ................................................................................ 68
4.4.2. Software License Handling ..................................................................................................... 68
4.4.3. Results File Option ................................................................................................................. 69
5. Reference Guide for Mesh Deformation and Fluid-Structure Interaction ............................................ 71
5.1. Mesh Deformation .......................................................................................................................... 71
5.1.1. Mesh Folding: Negative Sector and Element Volumes .............................................................. 71
5.1.2. Applying Large Displacements Gradually ................................................................................ 71
5.1.3. Consistency of Mesh Motion Specifications ............................................................................. 72
5.1.4. Solving the Mesh Displacement Equations and Updating Mesh Coordinates ........................... 72
5.1.5. Mesh Displacement Diffusion Scheme .................................................................................... 72
5.1.6. Mesh Displacement vs. Total Mesh Displacement .................................................................... 75
5.1.7. Simulation Restart Behavior .................................................................................................... 75
5.2. Fluid Structure Interaction .............................................................................................................. 76
5.2.1. Unidirectional (One-Way) FSI .................................................................................................. 76
5.2.1.1. Using CFX Only .............................................................................................................. 76
5.2.1.2. Using CFX and the Mechanical Application .................................................................... 76
5.2.1.2.1. Importing Data from the Mechanical Application Solver ........................................ 76
5.2.1.2.2. Export Data to Other ANSYS Software Products ..................................................... 77
5.2.1.2.3. Mechanical Import/Export Example: One-Way FSI Data Transfer ............................. 77
5.2.1.3. Using CFX and Other CAE Software ................................................................................ 77
5.2.2. Bidirectional (Two-Way) FSI .................................................................................................... 78
5.2.2.1. Using CFX Only .............................................................................................................. 78
5.2.2.2. Using CFX and the Mechanical Application .................................................................... 78
5.2.2.3. Using CFX and Other CAE Software ................................................................................ 80
6. CFX Best Practices Guide for Numerical Accuracy ................................................................................ 81
6.1. An Approach to Error Identification, Estimation and Validation ......................................................... 81
6.2. Definition of Errors in CFD Simulations ............................................................................................ 82
6.2.1. Numerical Errors .................................................................................................................... 83
6.2.1.1. Solution Errors ............................................................................................................... 83
6.2.1.2. Spatial Discretization Errors ........................................................................................... 84
6.2.1.3. Time Discretization Errors .............................................................................................. 84
6.2.1.4. Iteration Errors .............................................................................................................. 85
6.2.1.5. Round-off Error .............................................................................................................. 86
6.2.1.6. Solution Error Estimation ............................................................................................... 86
6.2.2. Modeling Errors ..................................................................................................................... 88
6.2.3. User Errors ............................................................................................................................. 89
6.2.4. Application Uncertainties ....................................................................................................... 90
6.2.5. Software Errors ...................................................................................................................... 90
6.3. General Best Practice Guidelines ..................................................................................................... 91
6.3.1. Avoiding User Errors ............................................................................................................... 91
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
vii
Reference Guide
6.3.2. Geometry Generation ............................................................................................................ 91
6.3.3. Grid Generation ..................................................................................................................... 91
6.3.4. Model Selection and Application ............................................................................................ 93
6.3.4.1. Turbulence Models ........................................................................................................ 93
6.3.4.1.1. One-equation Models ........................................................................................... 94
6.3.4.1.2. Two-equation Models ........................................................................................... 94
6.3.4.1.3. Second Moment Closure (SMC) Models ................................................................. 95
6.3.4.1.4. Large Eddy Simulation Models .............................................................................. 95
6.3.4.1.5. Wall Boundary Conditions ..................................................................................... 96
6.3.4.1.5.1. Wall Function Boundary Conditions .............................................................. 96
6.3.4.1.5.2. Integration to the wall (low-Reynolds number formulation) ........................... 96
6.3.4.1.5.3. Mixed formulation (automatic near-wall treatment) ...................................... 97
6.3.4.1.5.4. Recommendations for Model Selection ......................................................... 97
6.3.4.2. Heat Transfer Models ..................................................................................................... 97
6.3.4.3. Multi-Phase Models ....................................................................................................... 97
6.3.5. Reduction of Application Uncertainties ................................................................................... 98
6.3.6. CFD Simulation ...................................................................................................................... 98
6.3.6.1. Target Variables ............................................................................................................. 98
6.3.6.2. Minimizing Iteration Errors ............................................................................................. 99
6.3.6.3. Minimizing Spatial Discretization Errors ......................................................................... 99
6.3.6.4. Minimizing Time Discretization Errors ........................................................................... 100
6.3.6.5. Avoiding Round-Off Errors ........................................................................................... 101
6.3.7. Handling Software Errors ...................................................................................................... 101
6.4. Selection and Evaluation of Experimental Data .............................................................................. 101
6.4.1. Verification Experiments ....................................................................................................... 102
6.4.1.1. Description .................................................................................................................. 102
6.4.1.2. Requirements .............................................................................................................. 102
6.4.2. Validation Experiments ......................................................................................................... 102
6.4.2.1. Description .................................................................................................................. 103
6.4.2.2. Requirements .............................................................................................................. 103
6.4.3. Demonstration Experiments ................................................................................................. 104
6.4.3.1. Description .................................................................................................................. 104
6.4.3.2. Requirements .............................................................................................................. 105
7. CFX Best Practices Guide for Cavitation .............................................................................................. 107
7.1. Liquid Pumps ................................................................................................................................ 107
7.1.1. Pump Performance without Cavitation ................................................................................. 107
7.1.2. Pump Performance with Cavitation ....................................................................................... 108
7.1.3. Procedure for Plotting Performance Curve ............................................................................ 109
7.1.4. Setup ................................................................................................................................... 109
7.1.5. Convergence Tips ................................................................................................................. 110
7.1.6. Postprocessing ..................................................................................................................... 110
8. CFX Best Practices Guide for Combustion ........................................................................................... 111
8.1. Gas Turbine Combustors ............................................................................................................... 111
8.1.1. Setup ................................................................................................................................... 111
8.1.1.1. Steady-state vs. Transient ............................................................................................. 111
8.1.1.2. Turbulence Model ........................................................................................................ 111
8.1.1.3. Reference Pressure ...................................................................................................... 111
8.1.1.4. Combustion Model ...................................................................................................... 111
8.1.2. Reactions ............................................................................................................................. 112
8.1.3. Convergence Tips ................................................................................................................. 112
8.1.4. Postprocessing ..................................................................................................................... 113
8.2. Combustion Modeling in HVAC Cases ............................................................................................ 113
viii
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Reference Guide
8.2.1. Set Up .................................................................................................................................. 113
8.2.2. Convergence Tips ................................................................................................................. 114
8.2.3. Postprocessing ..................................................................................................................... 114
9. CFX Best Practices Guide for HVAC ..................................................................................................... 115
9.1. HVAC Simulations ......................................................................................................................... 115
9.1.1. Setting Up HVAC Simulations ................................................................................................ 115
9.1.1.1. Buoyancy .................................................................................................................... 115
9.1.1.2. Thermal Radiation ....................................................................................................... 116
9.1.1.2.1. Thermal Radiation Model .................................................................................... 116
9.1.1.2.2. Spectral Model .................................................................................................... 116
9.1.1.2.3. Scattering Model ................................................................................................ 116
9.1.1.3. CHT (Conjugate Heat Transfer) Domains ....................................................................... 117
9.1.1.4. Mesh Quality ............................................................................................................... 117
9.1.1.5. Fans ............................................................................................................................ 118
9.1.1.6. Thermostats ................................................................................................................ 118
9.1.1.7. Collections of Objects .................................................................................................. 118
9.2. Convergence Tips ......................................................................................................................... 118
10. CFX Best Practices Guide for Multiphase .......................................................................................... 119
10.1. Bubble Columns ......................................................................................................................... 119
10.1.1. Setup ................................................................................................................................. 119
10.1.2. Convergence Tips ............................................................................................................... 120
10.1.3. Postprocessing ................................................................................................................... 120
10.2. Mixing Vessels ............................................................................................................................. 120
10.2.1. Setup ................................................................................................................................. 120
10.3. Free Surface Applications ............................................................................................................ 121
10.3.1. Setup ................................................................................................................................. 121
10.3.2. Convergence Tips ............................................................................................................... 121
10.4. Multiphase Flow with Turbulence Dispersion Force ...................................................................... 122
11. CFX Best Practices Guide for Turbomachinery .................................................................................. 123
11.1. Gas Compressors and Turbines .................................................................................................... 123
11.1.1. Setup for Simulations of Gas Compressors and Turbines ...................................................... 123
11.1.2. Convergence Tips ............................................................................................................... 124
11.1.3. Computing Speedlines for a Machine .................................................................................. 124
11.1.4. Postprocessing ................................................................................................................... 125
11.2. Liquid Pumps and Turbines ......................................................................................................... 126
11.2.1. Setup for Simulations of Liquid Pumps and Turbines ........................................................... 126
11.2.2. Convergence Tips ............................................................................................................... 127
11.2.3. Postprocessing ................................................................................................................... 127
11.3. Fans and Blowers ........................................................................................................................ 127
11.3.1. Setup for Simulations of Fans and Blowers .......................................................................... 127
11.3.2. Convergence Tips ............................................................................................................... 127
11.3.3. Postprocessing ................................................................................................................... 128
11.4. Frame Change Models ................................................................................................................. 128
11.4.1. Frozen Rotor ....................................................................................................................... 128
11.4.2. Stage ................................................................................................................................. 129
11.4.3. Transient Rotor-Stator ......................................................................................................... 129
11.5. Domain Interface Setup .............................................................................................................. 129
11.5.1. General Considerations ...................................................................................................... 129
11.5.2. Case 1: Impeller/Volute ....................................................................................................... 130
11.5.3. Case 2: Step Change Between Rotor and Stator ................................................................... 130
11.5.4. Case 3: Blade Passage at or Close to the Edge of a Domain ................................................... 131
11.5.5. Case 4: Impeller Leakage ..................................................................................................... 132
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
ix
Reference Guide
11.5.6. Case 5: Domain Interface Near Zone of Reversed Flow ......................................................... 133
11.6. Transient Blade Row .................................................................................................................... 134
11.6.1. Steady versus Transient Blade Row Analysis ......................................................................... 134
11.6.2. Full Model Simulation versus Reduced Geometry Simulation (Pitch Change Models) ............ 134
11.6.3. Selecting an Appropriate Transient Blade Row Model with Pitch Change ............................. 135
11.6.3.1. Profile Transformation ................................................................................................ 135
11.6.3.2. Time Transformation .................................................................................................. 135
11.6.3.3. Fourier Transformation ............................................................................................... 136
11.6.4. Convergence and Solution Monitoring of Transient Blade Row Flow Problems ..................... 136
11.6.5. Boundary Conditions in Blade Row Simulation .................................................................... 137
11.6.5.1. Steady-state Analysis ................................................................................................. 137
11.6.5.2. Transient Analysis ...................................................................................................... 137
12. Best Practices: Scale-Resolving Simulations in ANSYS CFD .............................................................. 139
12.1. Scale-Resolving Simulation (SRS) Models – Basic Formulations ..................................................... 141
12.1.1. Scale-Adaptive Simulation (SAS) ......................................................................................... 141
12.1.2. Detached Eddy Simulation (DES) ......................................................................................... 143
12.1.3. Large Eddy Simulation (LES) ................................................................................................ 145
12.1.3.1. Limitations of Large Eddy Simulation (LES) ................................................................. 145
12.1.4. Wall Modeled Large Eddy Simulation (WMLES) .................................................................... 154
12.1.5. Embedded/Zonal LES (ELES, ZLES) ...................................................................................... 156
12.1.6. Unsteady Inlet/Interface Turbulence ................................................................................... 157
12.2. Generic Flow Types and Basic Model Selection ............................................................................. 158
12.2.1. Globally Unstable Flows ...................................................................................................... 158
12.2.1.1. Flow Physics .............................................................................................................. 158
12.2.1.2. Modeling ................................................................................................................... 159
12.2.1.3. Meshing Requirements .............................................................................................. 160
12.2.1.4. Numerical Settings .................................................................................................... 160
12.2.1.5. Examples ................................................................................................................... 161
12.2.1.5.1. Flow around a Fighter Aircraft ........................................................................... 161
12.2.1.5.2. Flow around a Triangular Cylinder ...................................................................... 162
12.2.1.5.3. ITS Combustion Chamber .................................................................................. 164
12.2.2. Locally Unstable Flows ........................................................................................................ 169
12.2.2.1. Flow Physics .............................................................................................................. 169
12.2.2.2. Modeling ................................................................................................................... 170
12.2.2.3. Meshing Requirements .............................................................................................. 171
12.2.2.4. Numerical Settings .................................................................................................... 172
12.2.2.5. Examples ................................................................................................................... 172
12.2.2.5.1. Backward-Facing Step I ..................................................................................... 172
12.2.3. Stable Flows and Wall Boundary Layers ............................................................................... 176
12.2.3.1. Flow Physics .............................................................................................................. 176
12.2.3.2. Modeling ................................................................................................................... 176
12.2.3.3. Meshing Requirements .............................................................................................. 177
12.2.3.4. Numerical Settings .................................................................................................... 179
12.2.3.5. Examples ................................................................................................................... 179
12.2.3.5.1. Periodic Channel ............................................................................................... 179
12.2.3.5.2. Wall Boundary Layer .......................................................................................... 182
12.2.3.5.3. NASA Hump Flow .............................................................................................. 187
12.2.3.5.4. T-Junction with Thermal Mixing ......................................................................... 189
12.3. Numerical Settings for SRS .......................................................................................................... 197
12.3.1. Spatial Discretization .......................................................................................................... 197
12.3.1.1. Momentum ............................................................................................................... 197
12.3.1.2. Turbulence Equations ................................................................................................ 199
x
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Reference Guide
12.3.1.3. Gradients (ANSYS Fluent) ........................................................................................... 199
12.3.2. Pressure (ANSYS Fluent) ...................................................................................................... 199
12.3.3. Time Discretization ............................................................................................................. 199
12.3.3.1. Time Integration ........................................................................................................ 199
12.3.3.2. Time Advancement and Under-Relaxation (ANSYS Fluent) .......................................... 200
12.4. Initial and Boundary Conditions .................................................................................................. 200
12.4.1. Initialization of SRS ............................................................................................................. 200
12.4.2. Boundary Conditions for SRS .............................................................................................. 201
12.4.2.1. Inlet Conditions ......................................................................................................... 201
12.4.2.2. Outlet Conditions ...................................................................................................... 201
12.4.2.3. Wall Conditions .......................................................................................................... 201
12.4.3. Symmetry vs. Periodicity ..................................................................................................... 201
12.5. Postprocessing and Averaging .................................................................................................... 202
12.5.1. Visual Inspection ................................................................................................................ 202
12.5.2. Averaging .......................................................................................................................... 203
12.6. Summary .................................................................................................................................... 204
12.6.1. Acknowledgment ............................................................................................................... 205
12.6.2. Appendix 1: Summary of Numerics Settings with ANSYS Fluent ........................................... 205
12.6.3. Appendix 2: Summary of Numerics Settings With ANSYS CFX .............................................. 206
12.6.4. Appendix 3: Models ............................................................................................................ 206
12.6.5. Appendix 4: Generic Flow Types and Modeling .................................................................... 209
12.7. Scale-Resolving Simulations References ....................................................................................... 212
13. CFX Command Language (CCL) ......................................................................................................... 215
13.1. CFX Command Language (CCL) Syntax ........................................................................................ 215
13.1.1. Basic Terminology .............................................................................................................. 216
13.1.2. The Data Hierarchy ............................................................................................................. 216
13.1.3. Simple Syntax Details ......................................................................................................... 216
13.1.3.1. Case Sensitivity .......................................................................................................... 216
13.1.3.2. CCL Names Definition ................................................................................................ 217
13.1.3.3. Indentation ............................................................................................................... 217
13.1.3.4. End of Line Comment Character ................................................................................. 217
13.1.3.5. Continuation Character .............................................................................................. 217
13.1.3.6. Named Objects .......................................................................................................... 217
13.1.3.7. Singleton Objects ...................................................................................................... 218
13.1.3.8. Parameters ................................................................................................................ 218
13.1.3.9. Lists ........................................................................................................................... 218
13.1.3.10. Parameter Values ..................................................................................................... 218
13.1.3.10.1. String .............................................................................................................. 218
13.1.3.10.2. String List ........................................................................................................ 219
13.1.3.10.3. Integer ............................................................................................................ 219
13.1.3.10.4. Integer List ...................................................................................................... 219
13.1.3.10.5. Real ................................................................................................................ 219
13.1.3.10.6. Real List .......................................................................................................... 219
13.1.3.10.7. Logical ............................................................................................................ 219
13.1.3.10.8. Logical List ...................................................................................................... 220
13.1.3.11. Escape Character ..................................................................................................... 220
14. CFX Expression Language (CEL) ........................................................................................................ 221
14.1. CEL Fundamentals ...................................................................................................................... 221
14.1.1. Values and Expressions ....................................................................................................... 221
14.1.1.1. Using Locators in Expressions ..................................................................................... 222
14.1.2. CFX Expression Language Statements ................................................................................. 222
14.1.2.1. Use of Constants ........................................................................................................ 223
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
xi
Reference Guide
14.1.2.2. Expression Syntax ...................................................................................................... 223
14.1.2.3. Multiple-Line Expressions .......................................................................................... 224
14.2. CEL Operators, Constants, and Expressions ................................................................................... 224
14.2.1. CEL Operators .................................................................................................................... 224
14.2.2. Conditional if Statement ..................................................................................................... 225
14.2.3. CEL Constants .................................................................................................................... 226
14.2.4. Using Expressions ............................................................................................................... 226
14.2.4.1. Use of Offset Temperature .......................................................................................... 226
14.3. CEL Examples .............................................................................................................................. 227
14.3.1. Example: Reynolds Number Dependent Viscosity ................................................................ 227
14.3.2. Example: Feedback to Control Inlet Temperature ................................................................. 228
14.3.3. Examples: Using Expressions in CFD-Post ............................................................................ 229
14.4. CEL Technical Details ................................................................................................................... 230
15. Functions in ANSYS CFX .................................................................................................................... 231
15.1. CEL Mathematical Functions ....................................................................................................... 231
15.2. Quantitative CEL Functions in ANSYS CFX .................................................................................... 233
15.3. Functions Involving Coordinates ................................................................................................. 236
15.4. CEL Functions with Multiphase Flow ............................................................................................ 236
15.5. Quantitative Function List ........................................................................................................... 237
15.5.1. area ................................................................................................................................... 241
15.5.1.1. Tools > Command Editor Example .............................................................................. 242
15.5.1.2. Tools > Function Calculator Example .......................................................................... 242
15.5.2. areaAve .............................................................................................................................. 242
15.5.2.1. Tools > Command Editor Example .............................................................................. 243
15.5.2.2. Tools > Function Calculator Examples ......................................................................... 243
15.5.3. areaInt ............................................................................................................................... 243
15.5.3.1. Tools > Command Editor Example .............................................................................. 244
15.5.3.2. Tools > Function Calculator Examples ......................................................................... 244
15.5.4. ave ..................................................................................................................................... 244
15.5.4.1. Tools > Command Editor Example .............................................................................. 245
15.5.4.2. Tools > Function Calculator Example .......................................................................... 245
15.5.5. count ................................................................................................................................. 245
15.5.5.1. Tools > Command Editor Example .............................................................................. 245
15.5.5.2. Tools > Function Calculator Example .......................................................................... 246
15.5.6. countTrue .......................................................................................................................... 246
15.5.6.1.Tools > Command Editor Examples ............................................................................. 246
15.5.6.2. Tools > Function Calculator Example .......................................................................... 246
15.5.7. force .................................................................................................................................. 246
15.5.7.1. Tools > Command Editor Example .............................................................................. 247
15.5.7.2. Tools > Function Calculator Examples ......................................................................... 247
15.5.8. forceNorm .......................................................................................................................... 247
15.5.8.1. Tools > Command Editor Example .............................................................................. 248
15.5.8.2. Tools > Function Calculator Example .......................................................................... 248
15.5.9. inside ................................................................................................................................. 248
15.5.9.1. Tools > Command Editor Example .............................................................................. 248
15.5.10. length .............................................................................................................................. 248
15.5.10.1. Tools > Command Editor Example ............................................................................ 249
15.5.10.2. Tools > Function Calculator Example ........................................................................ 249
15.5.11. lengthAve ........................................................................................................................ 249
15.5.11.1. Tools > Command Editor Example ............................................................................ 249
15.5.11.2. Tools > Function Calculator Example ........................................................................ 249
15.5.12. lengthInt .......................................................................................................................... 250
xii
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Reference Guide
15.5.12.1. Tools > Command Editor Example ............................................................................ 250
15.5.13. mass ................................................................................................................................ 250
15.5.14. massAve ........................................................................................................................... 250
15.5.15. massFlow ......................................................................................................................... 250
15.5.15.1. Mass Flow Sign Convention ...................................................................................... 251
15.5.15.2. Tools > Command Editor Example ............................................................................ 251
15.5.15.3. Tools > Function Calculator Example ........................................................................ 251
15.5.16. massFlowAve ................................................................................................................... 252
15.5.16.1. Tools > Command Editor Example ............................................................................ 252
15.5.16.2. Tools > Function Calculator Example ........................................................................ 252
15.5.17. massFlowAveAbs .............................................................................................................. 252
15.5.18. Advanced Mass Flow Considerations ................................................................................. 253
15.5.19. Mass Flow Technical Note ................................................................................................. 253
15.5.20. massFlowInt ..................................................................................................................... 254
15.5.20.1. Tools > Command Editor Example ............................................................................ 255
15.5.20.2. Tools > Function Calculator Example ........................................................................ 255
15.5.21. massInt ............................................................................................................................ 255
15.5.22. maxVal ............................................................................................................................. 255
15.5.22.1. Tools > Command Editor Example ............................................................................ 255
15.5.22.2. Tools > Function Calculator Example ........................................................................ 255
15.5.23. minVal .............................................................................................................................. 255
15.5.23.1. Tools > Command Editor Example ............................................................................ 256
15.5.23.2. Tools > Function Calculator Example ........................................................................ 256
15.5.24. probe ............................................................................................................................... 256
15.5.24.1. Tools > Command Editor Example ............................................................................ 256
15.5.24.2. Tools > Function Calculator Example ........................................................................ 256
15.5.25. rbstate ............................................................................................................................. 256
15.5.25.1. Expressions Details View Example ............................................................................ 257
15.5.26. rmsAve ............................................................................................................................. 257
15.5.27. sum .................................................................................................................................. 257
15.5.27.1. Tools > Command Editor Example ............................................................................ 258
15.5.27.2. Tools > Function Calculator Example ........................................................................ 258
15.5.28. torque .............................................................................................................................. 258
15.5.28.1. Tools > Command Editor Example ............................................................................ 258
15.5.28.2. Tools > Function Calculator Example ........................................................................ 258
15.5.29. volume ............................................................................................................................. 259
15.5.29.1. Tools > Command Editor Example ............................................................................ 259
15.5.29.2. Tools > Function Calculator Example ........................................................................ 259
15.5.30. volumeAve ....................................................................................................................... 259
15.5.30.1. Tools > Command Editor Example ............................................................................ 259
15.5.30.2. Tools > Function Calculator Example ........................................................................ 259
15.5.31. volumeInt ........................................................................................................................ 259
15.5.31.1. Tools > Command Editor Example ............................................................................ 260
15.5.31.2. Tools > Function Calculator Example ........................................................................ 260
16. Variables in ANSYS CFX ..................................................................................................................... 261
16.1. Hybrid and Conservative Variable Values ...................................................................................... 261
16.1.1. Solid-Fluid Interface Variable Values .................................................................................... 262
16.1.1.1. Conservative Values at 1:1 Interface ............................................................................ 262
16.1.1.2. Hybrid Values at 1:1 Interface ..................................................................................... 262
16.1.1.3. Conservative Values on a GGI Interface ....................................................................... 263
16.1.1.4. Hybrid Values on a GGI Interface ................................................................................ 263
16.2. List of Field Variables ................................................................................................................... 263
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
xiii
Reference Guide
16.2.1. Common Variables Relevant for Most CFD Calculations ....................................................... 264
16.2.2. Variables Relevant for Turbulent Flows ................................................................................ 268
16.2.3. Variables Relevant for Buoyant Flow .................................................................................... 271
16.2.4. Variables Relevant for Compressible Flow ............................................................................ 271
16.2.5. Variables Relevant for Particle Tracking ................................................................................ 272
16.2.6. Variables Relevant for Calculations with a Rotating Frame of Reference ................................ 272
16.2.7. Variables Relevant for Parallel Calculations .......................................................................... 273
16.2.8. Variables Relevant for Multicomponent Calculations ........................................................... 273
16.2.9. Variables Relevant for Multiphase Calculations .................................................................... 273
16.2.10. Variables Relevant for Radiation Calculations ..................................................................... 274
16.2.11. Variables for Total Enthalpies, Temperatures, and Pressures ................................................ 276
16.2.12. Variables and Predefined Expressions Available in CEL Expressions .................................... 277
16.2.12.1. System Variable Prefixes ........................................................................................... 287
16.2.12.2. CEL Variables r and theta .......................................................................................... 287
16.2.12.3. CEL Variable rNoDim ................................................................................................ 288
16.2.12.4. CEL Variable "subdomain" and CEL Function "inside" ................................................. 288
16.2.12.5. Timestep, Timestep Interval, and Iteration Number Variables ..................................... 288
16.2.12.5.1. Steady-State Runs ........................................................................................... 288
16.2.12.5.2. Transient Runs ................................................................................................. 289
16.2.12.5.3. ANSYS Multi-field Runs .................................................................................... 289
16.2.12.5.4. Timestep Variables in CFD-Post ........................................................................ 289
16.2.12.6. Expression Names .................................................................................................... 289
16.2.12.7. Scalar Expressions .................................................................................................... 289
16.2.12.8. Expression Properties ............................................................................................... 290
16.2.12.9. Available and Unavailable Variables .......................................................................... 290
16.3. Particle Variables Generated by the Solver ................................................................................... 290
16.3.1. Particle Track Variables ........................................................................................................ 291
16.3.2. Particle Field Variables ........................................................................................................ 294
16.3.2.1. Particle Sources into the Coupled Fluid Phase ............................................................. 294
16.3.2.2. Particle Radiation Variables ........................................................................................ 295
16.3.2.3. Particle Vertex Variables ............................................................................................. 295
16.3.2.3.1. Variable Calculations ......................................................................................... 297
16.3.2.4. Particle Boundary Vertex Variables .............................................................................. 298
16.3.2.5. Particle RMS Variables ................................................................................................ 299
16.3.2.5.1. Variable Calculations ......................................................................................... 300
16.4. Miscellaneous Variables ............................................................................................................... 300
17. Power Syntax in ANSYS CFX .............................................................................................................. 311
17.1. Examples of Power Syntax ........................................................................................................... 311
17.1.1. Example 1: Print the Value of the Pressure Drop Through a Pipe ........................................... 312
17.1.2. Example 2: Using a for Loop ................................................................................................ 313
17.1.3. Example 3: Creating a Simple Subroutine ............................................................................ 313
17.1.4. Example 4: Creating a Complex Quantitative Subroutine ..................................................... 314
17.2. Predefined Power Syntax Subroutines ......................................................................................... 315
17.2.1. Power Syntax Subroutine Descriptions ................................................................................ 315
17.2.2. Power Syntax Usage ........................................................................................................... 316
17.2.3. Power Syntax Subroutines .................................................................................................. 316
17.2.3.1. area(Location, Axis) .................................................................................................... 316
17.2.3.2. areaAve(Variable, Location, Axis) ................................................................................. 316
17.2.3.3. areaInt(Variable, Location, Axis) .................................................................................. 316
17.2.3.4. ave(Variable, Location) ............................................................................................... 317
17.2.3.5. calcTurboVariables() ................................................................................................... 317
17.2.3.6. calculate(function,...) .................................................................................................. 317
xiv
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Reference Guide
17.2.3.7. calculateUnits(function,...) .......................................................................................... 317
17.2.3.8. collectTurboInfo() ...................................................................................................... 317
17.2.3.9. comfortFactors() ........................................................................................................ 317
17.2.3.10. compressorPerform(Location, Location, Location, Var, Args) ....................................... 317
17.2.3.11. compressorPerformTurbo() ...................................................................................... 317
17.2.3.12. copyFile(FromPath, ToPath) ...................................................................................... 317
17.2.3.13. count(Location) ....................................................................................................... 317
17.2.3.14. countTrue(Expression, Location) ............................................................................... 318
17.2.3.15. cpPolar(Location, Var, Arg, Var, Location, Arg) ............................................................. 318
17.2.3.16. evaluate(Expression) ................................................................................................ 318
17.2.3.17. evaluateInPreferred(Expression) ............................................................................... 318
17.2.3.18. exprExists(Expression) .............................................................................................. 318
17.2.3.19. fanNoiseDefault() ..................................................................................................... 319
17.2.3.20. fanNoise() ................................................................................................................ 319
17.2.3.21. force(Location, Axis) ................................................................................................. 319
17.2.3.22. forceNorm(Location, Axis) ........................................................................................ 319
17.2.3.23. getBladeForceExpr() ................................................................................................. 319
17.2.3.24. getBladeTorqueExpr() .............................................................................................. 319
17.2.3.25. getCCLState() ........................................................................................................... 319
17.2.3.26. getChildrenByCategory(Category) ............................................................................ 319
17.2.3.27. getChildren(Object Name, Child Type) ...................................................................... 319
17.2.3.28. getExprOnLocators() ................................................................................................ 320
17.2.3.29. getExprString(Expression) ........................................................................................ 320
17.2.3.30. getExprVal(Expression) ............................................................................................. 320
17.2.3.31. getObjectName(Object Path) ................................................................................... 320
17.2.3.32. getParameterInfo(Object Name, Parameter Name, Info Type) ..................................... 320
17.2.3.33. getParameters(Object Name) ................................................................................... 320
17.2.3.34. getTempDirectory() ................................................................................................. 320
17.2.3.35. getType(Object Name) ............................................................................................. 320
17.2.3.36. getValue(Object Name, Parameter Name) ................................................................. 321
17.2.3.36.1. Example .......................................................................................................... 321
17.2.3.37. getViewArea() .......................................................................................................... 321
17.2.3.38. isCategory(Object Name, Category) .......................................................................... 321
17.2.3.39. Length(Location) ..................................................................................................... 321
17.2.3.40. lengthAve(Variable, Location) ................................................................................... 322
17.2.3.41. lengthInt(Variable, Location) .................................................................................... 322
17.2.3.42. liquidTurbPerformTurbo() ........................................................................................ 322
17.2.3.43. liquidTurbPerform() ................................................................................................. 322
17.2.3.44. massFlow(Location) ................................................................................................. 322
17.2.3.45. massFlowAve(Variable, Location) .............................................................................. 322
17.2.3.46. massFlowAveAbs(Variable, Location) ........................................................................ 322
17.2.3.47. massFlowInt(Variable, Location) ............................................................................... 322
17.2.3.48. maxVal(Variable, Location) ....................................................................................... 322
17.2.3.49. minVal(Variable, Location) ........................................................................................ 322
17.2.3.50. objectExists(Object Name) ....................................................................................... 323
17.2.3.51. probe(Variable, Location) ......................................................................................... 323
17.2.3.52. pumpPerform() ........................................................................................................ 323
17.2.3.53. pumpPerformTurbo() ............................................................................................... 323
17.2.3.54. range(Variable, Location) .......................................................................................... 323
17.2.3.55. reportError(String) ................................................................................................... 323
17.2.3.56. reportWarning(String) .............................................................................................. 323
17.2.3.57. showPkgs() .............................................................................................................. 323
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
xv
Reference Guide
17.2.3.58. showSubs(packageName) ........................................................................................ 323
17.2.3.59. showVars(packageName) ......................................................................................... 324
17.2.3.60. spawnAsyncProcess(command, arguments) ............................................................. 324
17.2.3.61. sum(Variable, Location) ............................................................................................ 324
17.2.3.62. torque(Location, Axis) .............................................................................................. 324
17.2.3.63. turbinePerform() ...................................................................................................... 324
17.2.3.64. turbinePerformTurbo() ............................................................................................. 324
17.2.3.65. verboseOn() ............................................................................................................. 324
17.2.3.66. volume(Location) ..................................................................................................... 324
17.2.3.67. volumeAve(Variable, Location) ................................................................................. 324
17.2.3.68. volumeInt(Variable, Location) ................................................................................... 324
18. Bibliography ...................................................................................................................................... 327
18.1. References 1-20 .......................................................................................................................... 327
18.2. References 21-40 ......................................................................................................................... 330
18.3. References 41-60 ......................................................................................................................... 333
18.4. References 61-80 ......................................................................................................................... 336
18.5. References 81-100 ....................................................................................................................... 339
18.6. References 101-120 ..................................................................................................................... 341
18.7. References 121-140 ..................................................................................................................... 344
18.8. References 141-160 ..................................................................................................................... 347
18.9. References 161-180 ..................................................................................................................... 350
18.10. References 181-200 ................................................................................................................... 353
18.11. References 201 – ....................................................................................................................... 356
Glossary ................................................................................................................................................... 361
xvi
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 1: ANSYS CFX Launcher
This chapter describes the ANSYS CFX Launcher in detail:
1.1.The ANSYS CFX Launcher Interface
1.2. Customizing the ANSYS CFX Launcher
1.1. The ANSYS CFX Launcher Interface
The layout of the ANSYS CFX Launcher is shown below:
Figure 1.1: ANSYS CFX Launcher
The launcher consists of a menu bar, a toolbar for launching applications, a working directory selector,
and an output window where messages are displayed. On Windows platforms, an icon to start Windows
Explorer in the working directory appears next to the directory selector.
1.1.1. Menu Bar
The ANSYS CFX Launcher menus provide the following capabilities:
1.1.1.1. File Menu
Saves the contents of the text output window and to close the ANSYS CFX Launcher.
1.1.1.1.1. Save As
Saves the contents of the output window to a file.
1.1.1.1.2. Quit
Shuts down the ANSYS CFX Launcher. Any programs already launched will continue to run.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
1
ANSYS CFX Launcher
1.1.1.2. Edit Menu
Clears the text output window, finds text in the text output window and sets options for the ANSYS
CFX Launcher.
1.1.1.2.1. Clear
Clears the output window.
1.1.1.2.2. Find
Displays a dialog box where you can search the text in the output window.
1.1.1.2.3. Options
Presents the Options dialog box, which enables you to change the appearance of the ANSYS CFX
Launcher.
1.1.1.2.3.1. User Interface Style
You can choose any one of several user interface styles; each style is available on all platforms. For example, choosing Windows will change the look and feel of the user interface to resemble that of a
Windows application. You can select from Windows, Motif, CDE (Solaris), Plastique, and Cleanlooks styles.
Once you have selected a style, click Apply to test.
1.1.1.2.3.2. Application Font and Text Window Font
The button to the right of Application Font sets the font used anywhere outside the text output window.
The button to the right of Text Window Font applies only to the text output window. Clicking either
of these buttons opens the Select Font dialog box.
1.1.1.3. CFX Menu
Enables you to launch CFX-Pre, CFX-Solver Manager, CFD-Post, and, if they are installed, other CFX
products (such as ANSYS TurboGrid).
1.1.1.3.1. CFX-Pre
Runs CFX-Pre, with the working directory as specified in Working Directory Selector (p. 4).
1.1.1.3.2. CFX-Solver Manager
Runs CFX-Solver Manager, with the working directory as specified in Working Directory Selector (p. 4).
1.1.1.3.3. CFD-Post
Runs CFD-Post, in the current working directory as specified in Working Directory Selector (p. 4).
1.1.1.3.4. Other CFX Applications
The ANSYS CFX Launcher also searches for other CFX applications (for example, ANSYS TurboGrid) and
provides a menu entry to launch the application. If an application is not found, you can add it; for details,
see Customizing the ANSYS CFX Launcher (p. 5).
2
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
The ANSYS CFX Launcher Interface
1.1.1.4. Show Menu
Enables you to show system, installation, and other information.
1.1.1.4.1. Show Installation
Displays information about the version of CFX that you are running.
1.1.1.4.2. Show All
Displays all of the available information, including information about your system, installation, and
variables.
1.1.1.4.3. Show System
Displays information about the CFX installation and the system on which it is being run.
1.1.1.4.4. Show Variables
Displays the values of all the environment variables that are used in CFX.
1.1.1.5. Tools Menu
Enables you to access license-management tools and a command line for running other CFX utilities.
1.1.1.5.1. ANSYS Client Licensing Utility
Enables you to configure connections to ANSYS License Managers.
1.1.1.5.2. Command Line
Starts a command window from which you can run any of the CFX commands via the command line
interface. The command line will be set up to run the correct version of CFX and the commands will
be run in the current working directory.
If you do not use the Tools > Command Line command to open a command window, then you will
have to either type the full path of the executable in each command, or explicitly set your operating
system path to include the <CFXROOT>/bin directory.
You may want to start components of CFX from the command line rather than by clicking the appropriate
button on the ANSYS CFX Launcher for the following reasons:
• CFX contains some utilities (for example, a parameter editor) that can be run only from the command line.
• You may want to specify certain command line arguments when starting up a component so that it starts
up in a particular configuration.
• If you are having problems with a component, you may be able to get a more detailed error message by
starting the component from the command line than you would get if you started the component from the
launcher. If you start a component from the command line, any error messages produced are written to the
command line window.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
3
ANSYS CFX Launcher
1.1.1.5.3. Configure User Startup Files (Linux only)
Information about creating startup files can be found in the installation documentation.
1.1.1.5.4. Edit File
Opens a platform-native text editor. Which text editor is opened is controlled by the settings in <CFXROOT>/etc/launcher/shared.ccl.
1.1.1.5.5. Edit Site-wide Configuration File
Opens the site-wide configuration file in a text editor. Which text editor is called is controlled by the
settings in <CFXROOT>/etc/launcher/CFX5.ccl.
1.1.1.6. User Menu
The User menu is provided as an example. You can add your own applications to this menu, or create
new menus; for details, see Customizing the ANSYS CFX Launcher (p. 5).
1.1.1.7. Help Menu
The Help menu has the following commands:
CFX-Launcher
Opens CFX-Launcher help (this chapter), which describes the launcher interface as well as how to customize
the launcher to, for example, add a menu entry that runs your own application.
CFX
You can select various topics including Contents, which will open up help documentation that describes
the CFX documentation set, Tutorials, and several topics.
About CFX-Launcher
This gives the point releases and software patches that are installed.
Help on Help
Opens documentation about the help system: Help On Help
Guidance on accessing CFX documentation is provided in Accessing Help.
1.1.2. Toolbar
The toolbar contains shortcuts to the main components of CFX, for example CFX-Pre, CFX-Solver Manager
and CFD-Post. Pressing any of the buttons will start up the component in the specified working directory.
The equivalent menu entries for launching the components also show a keyboard shortcut that can be
used to launch the component.
1.1.3. Working Directory Selector
While running CFX, all the files that are created will be stored in the working directory. To change the
working directory, you can do any of the following:
• Type the directory name into the box and press Enter.
• Click the down-arrow icon (
4
) next to the directory name. This displays a list of recently used directories.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Customizing the ANSYS CFX Launcher
• Click Browse
to browse to the directory that you want.
1.1.4. Output Window
The output window is used to display information from commands in the Show menu. You can rightclick in the output window to show a shortcut menu with the following options:
• Find: Displays a dialog box where you can enter text to search for in the output.
• Select All: Selects all the text.
• Copy Selection: Copies the selected text.
• Save As: Saves the output to a file.
• Clear: Clears the output window.
1.2. Customizing the ANSYS CFX Launcher
Many parts of the ANSYS CFX Launcher are driven by CCL commands contained in configuration files.
Some parts of the launcher are not editable (such as the File, Edit and Help menus), but others parts
enable you to edit existing actions and create new ones (for example, launching your own application
from the User menu). The following sections outline the steps required to configure the launcher. The
configuration files are located in the <CFXROOT>/etc/launcher/ directory (where <CFXROOT> is
the path to your installation of CFX). You can open these files in any text editor, but you should not
edit any of the configuration files provided by CFX, other than the User.ccl configuration file.
1.2.1. CCL Structure
The configuration files contain CCL objects that control the appearance and behavior of menus and
buttons that appear in the ANSYS CFX Launcher. There are three types of CCL objects: GROUP, APPLIC
ATION and DIVIDER objects. The fact that there are multiple configuration files is not important; applications in one file can refer to groups in other files.
An example of how to add a menu item for the Windows calculator to the launcher is given in Example:
Adding the Windows Calculator (p. 8).
1.2.1.1. GROUP
GROUP objects represent menus and toolbar groups in the ANSYS CFX Launcher. Each new GROUP
creates a new menu and toolbar. Nothing will appear in the menu or toolbar until you add APPLICA
TION or DIVIDER objects to the group. An example of a GROUP object is given below:
GROUP: CFX
Position = 200
Menu Name = &CFX
Show In Toolbar = Yes
Show In Menu = Yes
Enabled = Yes
END
• The group name is set after the colon. In this case, it is "CFX". This is the name that APPLICATION and
DIVIDER objects will refer to when you want to add them to this group. This name should be different to
all other GROUP objects.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
5
ANSYS CFX Launcher
• Position refers to the position of the menu relative to others. The value should be an integer between 1
and 1000. Groups with a higher Position value, relative to other groups, will have their menu appear
further to the right in the menu bar. Referring to Figure 1.1: ANSYS CFX Launcher (p. 1), CFX has a lower
position value than the ANSYS group. The File and Edit menus are always the first two menus and the Help
menu is always the last menu.
• The title of the menu is set under Menu Name (this menu has the title CFX). The optional ampersand is
placed before the letter that you want to have act as a menu accelerator (for example, Alt+C displays the
CFX menu). You must be careful not to use an existing menu accelerator.
• The creation of the menu or toolbar can be toggled by setting the Show in Menu and Show in
Toolbar options to Yes or No respectively. For example, you may want to create a menu item but not an
associated toolbar icon.
• Enabled sets whether the menu/toolbar is available for selection or is disabled. Set the option to No to
disable it.
1.2.1.2. APPLICATION
APPLICATION objects create entries in the menus and toolbars that will launch an application or run
a process. Two examples are given below with an explanation for each parameter. The first example
creates a menu entry in the Tools menu that opens a command line window. The second example
creates a menu entry and toolbar button to start CFX-Solver Manager.
APPLICATION: Command Line 1
Position = 300
Group = Tools
Tool Tip = Start a window in which CFX commands can be run
Menu Item Name = Command Line
Command = <windir>\system32\cmd.exe
Arguments = /c start
Show In Toolbar = No
Show In Menu = Yes
Enabled = Yes
OS List = winnt
END
APPLICATION: CFXSM
Position = 300
Group = CFX
Tool Tip = Launches ANSYS CFX-Solver Manager
Menu Item Name = CFX-Solver Manager
Command = cfx5solve
Show In Toolbar = Yes
Show In Menu = Yes
Enabled = Yes
Toolbar Name = ANSYS CFX-Solver Manager
Icon = LaunchSolveIcon.xpm
Shortcut = CTRL+S
END
• The application name is set after the colon, in the first example it is "Command Line 1". This name should
be different from all other APPLICATION objects.
• Position: sets the relative position of the menu entry. The value should be an integer between 1 and
1000. The higher the value, relative to other applications that have the same group, the further down the
menu or the further to the right in a toolbar the entry will appear. If you do not specify a position, the object
assumes a high position value (so it will appear at the bottom of a menu or at the right of a group of buttons).
• Group: sets the GROUP object to which this application belongs. The value must correspond to the name
that appears after "GROUP:" in an existing GROUP object. The menu and/or toolbar entry will not be created
6
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Customizing the ANSYS CFX Launcher
if you do not specify a valid group name. The GROUP object does not have to be in the same configuration
file.
• Tool Tip: displays a message when the mouse pointer is held over a toolbar button. In the "Command
Line 1" example above, the Tool Tip entry is not used because a toolbar button is not created. This
parameter is optional.
• Menu Item Name: sets the name of the entry that will appear in the menu. If you do not specify a name,
the name is set to the name of the APPLICATION: object. The optional ampersand is placed before the
letter that you want to have act as a menu accelerator (for example, Alt+C then S will start CFX-Solver
Manager. Alt+C selects the CFX menu and S selects the entry from the menu). You must be careful not to
use an existing menu accelerator.
• Command: contains the command to run the application. The path can be absolute (that is, use a forward
slash to begin the path on Linux, or a drive letter on Windows). If an absolute path is not specified, a relative
path from <CFXROOT>/bin/ is assumed. If no command is specified, the menu item/toolbar button will
not appear in the ANSYS CFX Launcher. The path and command are checked when the launcher is started.
If the path or command does not exist, the menu item/toolbar button will not appear in the launcher. You
may find it useful to include environment variables in a command path; for details, see Including Environment
Variables (p. 8).
• Arguments: specifies any arguments that need to be passed to the application. The arguments are appended
to the value you entered for Command. You do not need to include this parameter as there are no arguments
to pass. You may find it useful to include environment variables in the arguments; for details, see Including
Environment Variables (p. 8).
Distinct arguments are space-separated. If you need to pass an argument that contains spaces (such
as a Windows filepath) you should include that argument in double quotes, for example:
Arguments = “C:\Documents and Settings\User” arg2 arg3
• Show In Toolbar: determines if a toolbar button is created for the application. This optional parameter
has a default value of Yes.
• Show In Menu: determines if a menu entry is created for the application. This optional parameter has a
default value of Yes.
• Enabled: controls the menu entry and toolbar button. Set this parameter to No to disable the application.
This optional parameter has a default value of Yes.
• OS List is an optional parameter that enables you to set which operating system the application is suitable
for. If OS List is not supplied, the launcher will attempt to create the menu item and toolbar button on
all platforms.
For example, the command to open a command line window varies depending on the operating
system. In the ‘Command Line 1’ example above, the application only applies to Windows platforms.
To complete the OS coverage, the launcher configuration files contain more ‘Command Line’ applications that apply to different operating systems.
• Toolbar Name: sets the name that appears on the toolbar button. This parameter is optional (because
you may want to show only an icon).
• Icon: specifies the icon to use on the toolbar button and in the menu item. The path can be absolute (that
is, use a forward slash to begin the path on Linux, or a drive letter on Windows). If an absolute path is not
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
7
ANSYS CFX Launcher
specified, a relative path from <CFXROOT>/etc/icons is assumed. The following file formats are supported
for icon image files: Portable Network Graphics (png), Pixel Maps (ppm, xpm) and Bitmaps (bmp). Other icons
used in the launcher are 32 pixels wide and 30 pixels high. This parameter is optional. If it is not included,
an icon will not appear.
• Shortcut: specifies the keyboard shortcut that can be pressed to launch the application. You must be
careful not to use a keyboard shortcut that is used by any other APPLICATION object.
1.2.1.2.1. Including Environment Variables
In can be useful to use environment variables in the values for some parameters. You can specify an
environment variable value in any parameter by including its name between the < > symbols. In the
‘Command Line 1’ example above, <windir> is used in the Command parameter so that the command
would work on different versions of Windows. <windir> is replaced with the value held by the windir
environment variable. The Command and Argument parameters are the only parameters that are likely
to benefit from using environment variables. Environment variables included in the Arguments parameter are expanded before they are passed to the application.
1.2.1.3. DIVIDER
DIVIDER objects create a divider in a menu and/or toolbar (see the Tools menu for an example). An
example of the CCL for DIVIDER objects is shown below.
DIVIDER: Tools Divider 1
Position = 250
Group = Tools
OS List = winnt
END
The Position, Group and OS List parameters are the same as those used in APPLICATION objects.
For details, see APPLICATION (p. 6).
1.2.2. Example: Adding the Windows Calculator
The following CCL is the minimum required to add the Windows calculator to the ANSYS CFX Launcher:
GROUP: Windows Apps
Menu Name = Windows
END
APPLICATION: Calc
Group = Windows Apps
Command = <windir>\system32\calc.exe
Toolbar Name = Calc
END
Although the parameter Toolbar Name is not strictly required, you would end up with a blank toolbar
button if it were not set.
8
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 2: Volume Mesh Import API
The Mesh Import Application Programming Interface (API) enables you to build a customized executable
that reads a 3-dimensional mesh from a 3rd-party mesh file into CFX-Pre and to extend the number of
file formats that CFX-Pre can understand and read beyond those supplied as part of the standard installation.
The communication between the executable and CFX-Pre is via a communications channel that is controlled by use of routines in the API provided.
For details on using the Volume Mesh Import API, see User Import.
This chapter describes:
2.1. Valid Mesh Elements in CFX
2.2. Creating a Custom Mesh Import Executable for CFX-Pre
2.3. Details of the Mesh Import API
2.4. An Example of a Customized C Program for Importing Meshes into CFX-Pre
2.5. Import Programs
2.1. Valid Mesh Elements in CFX
The CFX-Solver technology works with unstructured meshes. This does not prohibit the use of structured
meshes. However a structured mesh will always be dealt with internally as an unstructured mesh.
The CFX-Solver can solve flows in any mesh comprising one or more of the following element types:
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
9
Volume Mesh Import API
You must write the program using the API to translate the mesh read from the 3rd-party file into a
format that can be processed by CFX-Pre.
2.2. Creating a Custom Mesh Import Executable for CFX-Pre
You can create your own customized program using the 'C' programming language or Fortran programming language. A number of API functions are provided in a library supplied with the ANSYS CFX installation. For details, see Details of the Mesh Import API (p. 12).
The installation contains a C source code example file that can be used as the basis of your custom
executable. This file, ImportTemplate.c, is provided in <CFXROOT>/examples/, and is listed in:
An Example of a Customized C Program for Importing Meshes into CFX-Pre (p. 26).
The basic structure of a program written to import a 3rd-party mesh into CFX-Pre is as follows:
1.
Inclusion of the cfxImport.h header file (for C programs and not Fortran programs).
2.
Initialization for import with the cfxImportInit routine.
3.
Definition of node data with cfxImportNode.
4.
Definition of element data with cfxImportElement.
5.
Optionally, definitions of 2D and 3D regions with either cfxImportRegion or the following three
functions: cfxImportBegReg, cfxImportAddReg, cfxImportEndReg
6.
Data transfer with cfxImportDone.
10
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating a Custom Mesh Import Executable for CFX-Pre
The header files associated with the API are located in <CFXROOT>/include/. If you do not use the
header file cfxImport.h, the functionality of the routines contained within the API may not follow
defined behavior.
After writing the program, you will need to compile the source code. For details, see Compiling Code
with the Mesh Import API (p. 11).
You will also need to link your routine with the API routine libraries. For details, see Linking Code with
the Mesh Import API (p. 11).
After a customized executable has been produced, it can be run in CFX-Pre. For details, see User Import.
2.2.1. Compiling Code with the Mesh Import API
Compilation of a customized executable must be performed using an appropriate compiler and compiler
flags.
The customized executable must also be linked with the provided mesh import API library and the
provided I/O library as detailed in Linking Code with the Mesh Import API (p. 11).
Note
Windows users should note that custom mesh import programs must be compiled as multithreaded applications.
2.2.2. Linking Code with the Mesh Import API
In order to build a customized import utility routine, it must be linked with several libraries. These libraries are located in <CFXROOT>/lib/<os>/:
• libmeshimport.lib (on Windows), or libmeshimport.a (on Linux)
• libratlas_api.lib (on Windows), or libratlas_api.a (on Linux)
• libratlas.lib (on Windows), or libratlas.a (on Linux)
• libpgtapi.lib (on Windows), or libpgtapi.a (on Linux)
• libunits.lib (on Windows), or libunits.a (on Linux)
• libcclapilt.lib (on Windows), or libcclapilt.a (on Linux)
• libio.lib (on Windows), or libio.a (on Linux)
2.2.2.1. Linking a Customized C Mesh Import Executable on a Linux Platform
On most Linux systems you should be able to build the executable with the command:
gcc myimport.c -I<CFXROOT>/include/ -o myimport -L<CFXROOT>/lib/<os> \
-lmeshimport -lratlas_api -lratlas -lpgtapi -lunits -lcclapilt -lio \
-lm -lc
Here, -lmeshimport, -lratlas_api, -lratlas, -lpgtapi, -lunits, -lcclapillt, and -lio
indicate the libraries mentioned above, while -lm and -lc are system libraries.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
11
Volume Mesh Import API
In this example, your own import program is named myimport.c and the executable file will be called
myimport. You should ensure that the libraries to which you are linking (which are in the path given
after -L) appear on the command line after the source file (or object file if you are just linking to an
existing object).
You can use the GCC compiler v4.6.1 with ANSYS CFX 15.0 or greater.
2.2.2.2. Linking a Customized Fortran Mesh Import Executable on a UNIX Platform
The following is an example of how to build the executable on Linux, when the source code for the
executable is written in Fortran:
pgf95 myimport.F -L<CFXROOT>/lib/linux-amd64 -lmeshimport -lratlas_api -lratlas \
-lpgtapi -lunits -lcclapilt -lio -lm -o myimport.exe
Note
The officially supported pgf compiler is required.
2.2.2.3. Linking a Customized Mesh Import Executable on a Windows Platform
You can build the executables on Windows systems that have the C++ compiler of Microsoft Visual
Studio 2010. An example command line follows:
cl /MD /I "C:\Program Files\Ansys Inc\v162\CFX\include" ImportTemplate.c
/link /libpath:"C:\Program Files\Ansys Inc\v162\CFX\lib\winnt-amd64"
libcclapilt.lib libio.lib libmeshimport.lib libunits.lib libpgtapi.lib
libratlas_api.lib libratlas.lib
You can also write the import program in Fortran and then compile it using the recommended Fortran
compiler on Windows. An example command line follows:
ifort /MD /I "C:\Program Files\Ansys Inc\v162\CFX\include" /threads
/iface:mixed_str_len_arg ImportTemplate.F /exe:ImportTemplate.exe /libs:dll
/link /libpath:"C:\Program Files\Ansys Inc\v162\CFX\lib\winnt-amd64"
libcclapilt.lib libio.lib libmeshimport.lib libunits.lib libpgtapi.lib
libratlas_api.lib libratlas.lib
2.3. Details of the Mesh Import API
This section contains information about the functions that are used to write a customized import executable in the Mesh Import API.
Before trying to use any of the routines listed in this section, it is highly recommended that you read
Creating a Custom Mesh Import Executable for CFX-Pre (p. 10).
This section contains details of:
• Defined Constants (p. 13)
• Initialization Routines (p. 14)
• Termination Routines (p. 15)
12
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Details of the Mesh Import API
• Error Handling Routines (p. 15)
• Node Routines (p. 16)
• Element Routines (p. 16)
• Primitive Region Routines (p. 19)
• Composite Regions Routines (p. 21)
• Explicit Node Pairing (p. 21)
• Fortran Interface (p. 22)
• Unsupported Routines Previously Available in the API (p. 25)
Note
In past releases of ANSYS CFX the API has defined IDs of nodes and elements as integers
(int). This release now uses a datatype ID_t to represent these quantities. This type is currently
defined as an unsigned integer (unsigned int). This allows a greater number of nodes and
elements to be imported than in the past.
2.3.1. Defined Constants
The following are defined in the header file cfxImport.h, which should be included in the import
program.
2.3.1.1. Element Types
There are currently 4 types of elements, which are identified by the number of nodes: Tetrahedrons (4
nodes), pyramids (5 nodes), wedges or prisms (6 nodes), and hexahedrons (8 nodes). The element types
may be identified by the defined constants:
#define
#define
#define
#define
cfxELEM_TET
cfxELEM_PYR
cfxELEM_WDG
cfxELEM_HEX
4
5
6
8
The element node ordering and local face numbering follow Patran Neutral file conventions for element
descriptions.
2.3.1.2. Region Types
Regions may be defined in terms of nodes, faces or elements, based on the type argument to the
cfxImportBegReg or cfxImportRegion routines. The three types are defined by the defined
constants:
#define cfxImpREG_NODES
#define cfxImpREG_FACES
#define cfxImpREG_ELEMS
1
2
3
Node and Face regions define 2D regions of the imported mesh. Element regions define 3D regions of
the imported mesh.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
13
Volume Mesh Import API
It is best to use face regions to define 2D regions of the mesh and element regions to define 3D regions
of the mesh.
Node regions will be automatically transformed into a face region by the import process. This transformation requires the node IDs specified to define vertices of valid element faces. If no element faces can
be constructed from the defined node region the node region will be deleted.
Note
Due to the limited topological information recoverable from a set of nodes it is not advisable
to define 2D regions internal to a 3D region using nodes. In this case it is advisable to use
Face regions.
Node regions are specified by a list of node IDs.
Face regions are defined by a list of face IDs. These face IDs are a combination of an element ID and a
local face number in the element.
2.3.2. Initialization Routines
The following routines check and initialize the Import API. With the exception of cfxImportStatus
the first call to the Import API must be either cfxImportInit for communication with CFX, or cfx
ImportTest for testing the import routine in stand-alone mode.
2.3.2.1. cfxImportStatus
int cfxImportStatus ()
Returns 0 if descriptor is not opened and -1 if not opened for writing. In the normal case, 1 is returned
if opened for writing to CFX, and 2 if opened for writing to a file.
2.3.2.2. cfxImportInit
void cfxImportInit ()
Performs initialization to begin communicating with CFX. This routine should be called early on in the
import program to let CFX know that data is to be sent. If not called within 60 seconds, CFX will terminate
the import process. If called and there is no connection with CFX, then the routine cfxImport
Test("/dev/null") (UNIX) or cfxImportTest("null") (Windows) will be called. This routine
will be automatically called by most of the API routines if not already called.
There is no return value for this routine. In the case of an error, cfxImportFatal will be called.
2.3.2.3. cfxImportTest
int cfxImportTest (filename)
char *filename;
This routine allows testing of import program in isolation from CFX by writing data to a file filename
instead of attempting to write it to the CFX communication channel.
The routine will return the file descriptor of the output file or will terminate with a call to cfxImport
Fatal on error.
14
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Details of the Mesh Import API
2.3.3. Termination Routines
With the exception of cfxImportTotals the last call to the Import API must always be cfxIm
portDone. This function performs the final processing of the import data, and then transfers the data
to CFX.
2.3.3.1. cfxImportDone
long cfxImportDone ()
Indicate to the import API that all mesh data has been given and the API should now send the data to
CFX. Except for cfxImportTotals, this should be last call made to the API. Returns the total number
of bytes transferred to CFX by the import program.
2.3.3.2. cfxImportTotals
long cfxImportTotals (counts)
size_t counts[cfxImpCNT_SIZE];
Get the total number of nodes, elements, regions and other useful information given to the mesh import
API by the program. This information is returned in the array counts, which should be of size at least
cfxImpCNT_SIZE (currently defined as 9). The values returned in counts may be indexed by the
enum list in cfxImport.h, which is:
counts[cfxImpCNT_NODE]
counts[cfxImpCNT_ELEMENT]
counts[cfxImpCNT_REGION]
counts[cfxImpCNT_UNUSED]
counts[cfxImpCNT_DUP]
counts[cfxImpCNT_TET]
counts[cfxImpCNT_PYR]
counts[cfxImpCNT_WDG]
counts[cfxImpCNT_HEX]
=
=
=
=
=
=
=
=
=
number
number
number
number
number
number
number
number
number
of
of
of
of
of
of
of
of
of
nodes
elements
regions
unused nodes
duplicate nodes
tetrahedral elements
pyramid elements
wedge elements
hexahedral elements
The return value for the function is the total number of bytes of data sent to CFX or written to the test
file given when cfxImportTest was called.
2.3.4. Error Handling Routines
The first error handling routine allows the programmer to define an error callback function that is called
when a fatal error is generated by the API or explicitly by the programmers code.
The second routine performs a method for clean termination of the program, shutting down the program
and communication with ANSYS CFX.
2.3.4.1. cfxImportError
void cfxImportError (callback)
void (*callback)(char *errmsg);
Define a user routine to be called before terminating due to a fatal error. callback is the applicationsupplied function to be called in the case of an error. The callback routine takes a single argument,
errmsg, which will be passed by cfxImportFatal and should be processed by the callback function
as a brief message describing the error that has occurred. If this function is not called or callback is not
specified, then the normal termination behavior of the mesh import API will be that the any fatal errors
will write the error message to stderr as well as being sent to CFX.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
15
Volume Mesh Import API
2.3.4.2. cfxImportFatal
void cfxImportFatal (errmsg)
char *errmsg;
Terminate with an error message, errmsg. This routine will send the message to CFX, shut down the
communication channel or test file and call the user callback function (if specified by a call to cfxImportError).
There is no return from this call. The import program will terminate immediately after clean up tasks
have been performed.
2.3.5. Node Routines
These routines define the 3D coordinates of points in space(nodes) that will be used to define elements
or 2D regions that are to be imported to CFX. Each node has a unique identifier called a node ID.
2.3.5.1. cfxImportNode
ID_t cfxImportNode (nodeid, x, y, z)
ID_t nodeid;
double x, y, z;
Define a node in the import API to be subsequently imported into CFX. The unique identifier of the
node is given by nodeid, and the coordinates of the node by x, y, and z.
Returns 0 if nodeid is invalid (less than 1), or nodeid is successfully defined. If a node with the same
identity has already been defined, the coordinate values will alter to the supplied values.
2.3.5.2. cfxImportGetNode
ID_t cfxImportGetNode (nodeid, x, y, z)
ID_t nodeid;
double *x, *y, *z;
Get the coordinates for the node identified by nodeid and return the values in x, y, and z. Returns 0
if the node has not been defined or the node ID for the node.
2.3.5.3. cfxImportNodeList
ID_t * cfxImportNodeList ()
Returns an array of all node identifiers currently defined or NULL if no nodes have been defined. The
first entry in the array is the number of nodes currently defined.
The memory for the array returned is allocated using malloc by the routine, consequently it should
be destroyed when no longer required by calling free.
2.3.6. Element Routines
The following routines define the topology of elements (using node IDs) that are to be imported to
CFX. Also included here are routines that get the local face number and vertices of an element.
2.3.6.1. cfxImportElement
ID_t cfxImportElement (elemid, elemtype, nodelist)
ID_t elemid, *nodelist; int elemtype;
16
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Details of the Mesh Import API
Define a new element to be imported to CFX. The unique identifier of the element is given by elemid,
the element type by elemtype and the list of vertices by nodelist. If an element with the same ID
has already been defined, it will be replaced by the new element being defined.
Only volume elements are currently supported by CFX; these may be tetrahedrons (4 vertices), pyramids
(5 vertices), prisms (6 vertices) or hexahedrons (8 vertices). elemtype is the number of vertices for the
element.
The following defines are included in the header file, cfxImport.h for convenience:
#define
#define
#define
#define
cfxELEM_TET
cfxELEM_PYR
cfxELEM_WDG
cfxELEM_HEX
4
5
6
8
/*
/*
/*
/*
tet element (4 nodes)
pyramid element (5 nodes)
wedge element (6 nodes)
hex element (8 nodes)
*/
*/
*/
*/
The list of vertices in nodelist refers to IDs of nodes that on termination of the import program by
a call to cfxImportDone must have been defined by calls to cfxImportNode. If this is not the case
a fatal error will be reported and the API will terminate.
The vertex ordering for the elements follows Patran Neutral File element conventions, and is shown in
the following figure.
Note
The vertex ordering for the export API is different. For details, see cfxExportElementList (p. 52).
Returns 0 in the case of an elemid is invalid (less than 1) or an unsupported value is given by elem
type, or elemid if the element is successfully defined. If the element already exists the vertices of the
element will be redefined.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
17
Volume Mesh Import API
2.3.6.2. cfxImportGetElement
ID_t cfxImportGetElement (elemid, nodelist)
ID_t elemid, nodelist[];
Get the node IDs for corresponding to the vertices of element identified by elemid and store in the
array nodelist. This array must be at least as large the number of vertices for the element (a size of 8
will handle all possible element types).
Returns 0 if the element is not defined, or the element type (number of vertices). The node IDs will be
ordered in the order expected by cfxImportElement if the program was to redefine the element.
2.3.6.3. cfxImportElementList
ID_t * cfxImportElementList ()
Returns an array of all the currently defined element IDs or NULL if no elements have been defined.
The first entry in the array is the number of elements.
The memory for the array returned is allocated using malloc by the routine, consequently it should
be destroyed when no longer required by calling free.
2.3.6.4. cfxImportGetFace
ID_t cfxImportGetFace (elemid, facenum, nodelist)
ID_t elemid, nodelist[]; int facenum;
Gets the node IDs for the local facenum’th face of the element identified by elemid.
The node IDs are returned in nodelist, which should be of at least of size 4. The nodes correspond
to the vertices of the face and are ordered counter-clockwise such that the normal for the face points
away from the element. The face numbers and associated node indices are modeled after Patran
Neutral File elements, and are tabulated here:
Element Type
Face
Nodes
tetrahedron
1
1
3
2
2
1
2
4
3
2
3
4
4
1
4
3
1
1
4
3
2
1
2
5
3
2
3
5
4
3
4
5
5
1
5
4
1
1
3
2
2
4
5
6
3
1
2
5
4
4
1
4
6
3
5
2
3
6
5
1
1
2
6
5
pyramid
prism
hexahedron
18
2
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Details of the Mesh Import API
Element Type
Face
Nodes
2
3
4
8
7
3
1
4
3
2
4
2
3
7
6
5
5
6
7
8
6
1
5
8
4
Note
The face numbers and associated node indices are different when exporting elements. For
details, see cfxExportFaceNodes (p. 54).
Returns -1 if the element has not been defined, 0 if the face number is out of range, or the number of
nodes for the face (3 or 4):
2.3.6.5. cfxImportFindFace
ID_t cfxImportFindFace (elemid, nnodes, nodeid)
ID_t elemid, nodeid[]; int nnodes;
Gets the local face number in element identified by elemid that contains all the nodes supplied by
the calling routine in nodeid. nnodes is the number of nodes for the face (3 or 4).
Returns -1 if the element is not found or nodeid is not supplied or nnodes is greater than 4 or less
than 3. Returns 0 if there is no match, or the local face number (1 to 6) of the element.
2.3.7. Primitive Region Routines
The following routines enable the specification of 2D regions as a group of nodes or faces, or a 3D region
as a group of elements. In the case of nodes and faces, only those that define faces of valid imported
elements will be imported; others are ignored by CFX.
2.3.7.1. cfxImportBegReg
int cfxImportBegReg (regname, regtype)
char *regname;
int regtype;
Initialize for the specification of a region. If a region is currently being defined, cfxImportEndReg
will be called.
The name of the region is given by regname. If the region name is NULL, the name Unnamed Region
2D or Unnamed Region 3D, with a sequential integer appended, will be used. If a region named
regname has already been defined, then additional objects will be added to the previous region.
The type of region is given by regtype, which should be one of cfxImpREG_NODES, cfxIm
pREG_FACES or cfxImpREG_ELEMS depending on whether the region is to be defined by nodes,
faces or elements, respectively. It is not currently possible to mix types in a region; doing so will cause
the import API to terminate with an error message.
Returns the number of objects (node, faces or elements) currently in the region.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
19
Volume Mesh Import API
2.3.7.2. cfxImportAddReg
int cfxImportAddReg (numobjs, objlist)
int numobjs, *objlist;
Add IDs of objects being defined to the current region.
A region must be currently defined or reactivated by cfxImportBegReg or an error will occur, and
the API will terminate.
The number of objects to add is given by numobjs and the IDs of the objects are supplied in objlist.
The objects are interpreted as node IDs, face IDs, or element IDs, depending on the type of the region
indicated when cfxImportBegReg was called.
On calling cfxImportDone, any node IDs , face IDs or element IDs specified in the object list must
have been defined by the appropriate routine or they will be removed from the region.
Returns the total number of objects in the current region after the object IDs have been added.
2.3.7.3. cfxImportEndReg
int cfxImportEndReg ()
End the specification of the current region.
Returns the number of objects (nodes, faces or elements) in the region.
2.3.7.4. cfxImportRegion
int cfxImportRegion (regname, regtype, numobjs, objlist)
char *regname;
int regtype, numobjs, *objlist;
Import a region named regname of type regtype. The number of objects to add to the region is
given by numobjs, and the list of object IDs by objlist. This routine combines calls to cfxImport
BegReg, cfxImportAddReg and cfxImportEndReg.
Returns the total number of objects in the region on termination of the routine.
2.3.7.5. cfxImportRegionList
char ** cfxImportRegionList ()
Return a NULL terminated list of currently defined region names.
The memory for the array and each character string in the array returned is allocated using malloc
by the routine, consequently each array member and the array itself should be destroyed when no
longer required by calling free.
2.3.7.6. cfxImportGetRegion
int * cfxImportGetRegion (regname)
char *regname;
Returns a list of objects in the region named regname, or NULL if the region does not exist. The first
entry in the returned list is the region type and the second entry is the number of object IDs.
20
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Details of the Mesh Import API
The memory for the array is allocated using malloc by the routine, consequently the array itself should
be destroyed when no longer required by calling free.
2.3.8. Composite Regions Routines
The following routines enable composite regions to be defined in terms of primitive regions or other
composite regions.
2.3.8.1. cfxImportBegCompRegion
cfxImportBegCompReg()
char *regionName;
Begin defining a composite region with the name regionName,
Returns -1 if a primitive region regionName is already defined or memory couldn’t be allocated, or 0
if successfully created.
2.3.8.2. cfxImportAddCompRegComponents
int cfxImportAddCompRegComponents(componentCount,components)
int componentCount;
char **components;
Add a set of component region names specified in components to the composite region currently
being defined. componentCount specified how many components are specified in the components
array,
Returns -1 if a composite region is not being defined or insufficient memory is available to add the
components of the composite region, or 0 if the components were successfully added.
2.3.8.3. cfxImportEndCompReg
int cfxImportEndCompReg()
Finish defining the current composite region.
Returns -1 if a composite region is not currently being defined or 0 otherwise.
2.3.8.4. cfxImportCompositeRegion
int cfxImportCompositeRegion(regionName, componentCount, components)
char *regionName, **components;
int componentCount;
Define a composite region named regionName with componentCount components supplied in
character array components.
Returns 0 if successful or -1 if an error occurred preventing the composite region being defined.
2.3.9. Explicit Node Pairing
The following routine provides a method for explicitly marking two nodes as being identical (or in the
same position in space).
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
21
Volume Mesh Import API
2.3.9.1. cfxImportMap
ID_t cfxImportMap (nodeid, mapid)
ID_t nodeid, mapid;
Explicitly map the node identified by nodeid to the node identified by mapid.
On calling cfxImportDone the Mesh Import API will update regions and elements referencing the
mapped node to the node it is mapped to. This therefore reduces the total node count imported to
CFX and eliminates the duplicate nodes.
Duplicate nodes may also be removed by CFX if the appropriate options are selected in the CFX interface
and an appropriate tolerance set. For details, see Importing Meshes in the CFX-Pre User's Guide.
2.3.10. Fortran Interface
The following routines are callable from Fortran, and interface with the corresponding C routine. There
are currently no return values.
2.3.10.1. cfxinit
call cfxinit
Interface to cfxImportInit. Initializes for import.
2.3.10.2. cfxtest
CHARACTER*n filename
call cfxtest(filename)
Interface to cfxImportTest. filename is a CHARACTER*n value that gives the name of the file to
dump the output to.
2.3.10.3. cfxunit
CHARACTER*n units
call cfxunit(units)
Interface to cfxImportUnits. Specify the units the mesh is specified in.
2.3.10.4. cfxwarn
CHARACTER*n mesg
call cfxwarn(mesg)
Interface to cfxImportWarning. Emit a warning message mesg.
2.3.10.5. cfxfatl
CHARACTER*n mesg
call cfxfatl(mesg)
Interface to cfxImportFatal. Emit a warning message mesg and terminate the program cleanly.
2.3.10.6. cfxdone
call cfxdone
Interface to cfxImportDone. Terminates the program and transfers the data to CFX-Pre.
22
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Details of the Mesh Import API
2.3.10.7. cfxnode
INTEGER idnode
DOUBLE PRECISION x,y,z
call cfxnode(idnode,x,y,z)
Interface to cfxImportNode. Imports a node with the specified coordinates. idnode is an INTEGER
value for the node ID, and x, y, and z are the DOUBLE PRECISION coordinates of the node.
2.3.10.8. cfxnodg
INTEGER idnode
DOUBLE PRECISION x,y,z
call cfxnodg(idnode,x,y,z)
Interface to cfxImportGetNode. Queries the current coordinates or a node referenced by idnode.
idnode is an INTEGER value for the node ID, and x, y, and z are the DOUBLE PRECISION coordinates
of the node.
2.3.10.9. cfxnods
INTEGER ids(*)
call cfxnods(ids)
Interface to cfxImportNodeList. Retrieves the list of all valid node IDs having been imported into
the API. ids is an INTEGER array that must be at least as large as the number of nodes currently imported.
2.3.10.10. cfxelem
INTEGER idelem,itelem,nodes(*)
call cfxelem(idelem,itelem,nodes)
Interface to cfxImportElement. idelem is element ID, and itelem is the element type (number
of nodes - 4,5,6, or 8). Both are of type INTEGER. nodes is an array of INTEGER node IDs dimensioned
of size at least itelem.
2.3.10.11. cfxeleg
INTEGER idelem,itelem,nodes(*)
call cfxeleg(idelem,itelem,nodes)
Interface to cfxImportGetElement. Queries the current node ids that define the vertices of the
element referenced by the id idelem. idelem is element ID, and itelem is the element type (number
of nodes - 4, 5, 6, or 8). Both are of type INTEGER. nodes is an array of INTEGER values that will contain
the node IDs on successful return. It should be dimensioned of size at least itelem.
2.3.10.12. cfxeles
INTEGER ids(*)
call cfxeles(ids)
Interface to cfxImportElemList. Retrieves the list of all valid element IDs having been imported
into the API. ids is an INTEGER array that must be at least as large as the number of elements currently
imported.
2.3.10.13. cfxfacd
INTEGER eleid, elefc, id
call cfxfacd(eleid, elefc, id)
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
23
Volume Mesh Import API
Interface to cfxImportFaceID. Defines a face id (id) in terms of an element ID (eleid) and local
face (elefc) of that element.
2.3.10.14. cfxface
INTEGER eleid, elefc, vtx(*)
INTEGER cfxface(eleid, elefc, vtx)
Interface to cfxImportGetFace. Returns the node IDs of the vertices defining a face located by the
element ID (eleid) and local face (elefc) of that element.
2.3.10.15. cfxffac
INTEGER eleid, nvtx, vtx(*), elefc
call cfxffac(eleid, nvtx, vtx, elefc)
Interface to cfxImportFindFace. Returns the local face (elefc) of an element (eleid) that is
defined by the vertices (vtx).
2.3.10.16. cfxregn
CHARACTER*n regname
INTEGER type,nobjs,objs(*)
call cfxregn(regname,type,nobjs,objs)
Interface to cfxImportRegion. Regname is a CHARACTER*n string defining the region name, type
is an INTEGER value specifying the type of region, either 1 for nodes, 2 for faces, or 3 for elements.
nobjs is an INTEGER value that gives the number of objects in the region, and objs is an INTEGER array
of object IDs dimensioned at least size nobjs.
2.3.10.17. cfxregb
CHARACTER*n regname
INTEGER type
call cfxregb(regname,type)
Interface to cfxImportBegReg. Start defining a new region or make an existing region of the same
name the current one if it already exists and is of the same type. regname is a CHARACTER*n string
defining the region name, type is an INTEGER value specifying the type of region, either 1 for nodes, 2
for faces, or 3 for elements.
2.3.10.18. cfxrega
INTEGER nobjs,objs(*)
call cfxrega(nobjs,objs)
Interface to cfxImportAddReg. Add the objects (objs) to the current region. nobjs is an INTEGER
value that gives the number of objects to add to the region, and objs is an INTEGER array of object
IDs dimensioned at least size nobjs.
2.3.10.19. cfxrege
call cfxrege()
Interface to cfxImportEndReg. Finish defining the current region (after the call there will be no
current region).
24
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Details of the Mesh Import API
2.3.10.20. cfxregs
CHARACTER*n regname
INTEGER numobj
call cfxregs(regname,numobj)
Query how many objects (returned in numobj) are referenced by the region regname. regname is a
CHARACTER*n string specifying the region name.
2.3.10.21. cfxregg
CHARACTER*n regname
INTEGER type, obj(*)
call cfxregg(regname, type, objs)
Get the type (type) and object IDs (objs) referenced by the region regname. regname is a CHARACTER*n string specifying the region name. type is INTEGER and objs is an INTEGER array at least of the
size returned by cfxregs.
2.3.10.22. cfxcmpb
CHARACTER*n regname
call cfxcmpb(regname)
Interface to cfxImportBegCompReg. Start defining a new composite region or make an existing
composite region of the same name as the current one if it already exists. regname is a CHARACTER*n
string defining the region name.
2.3.10.23. cfxcmpa
INTEGER nregs
CHARACTER*(n) regs
call cfxcmpa(nregs,regs)
Interface to cfxImportAddCompReg. Add the region names (regs) to the current composite region
being defined. nregs is an INTEGER value that gives the number of regions to add to the region, and
regs is a CHARACTER*(*) array of region names dimensioned at least size nregs.
2.3.10.24. cfxcmpe
call cfxcmpe()
Interface to cfxImportEndCompReg. Finish defining the current composite region (after the call there
will be no current composite region).
2.3.11. Unsupported Routines Previously Available in the API
In ANSYS CFX 16.2 certain functionality available in previous releases is no longer supported. These
routines have been removed because they are directly implemented in CFX.
The following is a list of routines removed from the mesh import API:
cfxImportFixElements
cfxImportTolerance
cfxImportGetTol
cfxImportSetCheck
cfxImportRange
cfxImportCheck
cfxtol
cfxset
cfxchk
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
25
Volume Mesh Import API
2.4. An Example of a Customized C Program for Importing Meshes into
CFX-Pre
An example, ImportTemplate.c, can be found in <CFXROOT>/examples.
2.5. Import Programs
The following sections detail the standard import programs currently available within CFX-Pre and their
command line equivalents.
Information about importing meshes from the CFX-Pre interface is given in Importing Meshes in the
CFX-Pre User's Guide.
If you want to use command line options that cannot be specified through the CFX-Pre User Interface,
then you may want to run these programs as user-defined mesh import programs. User Import details
how to run a mesh import program.
The executables are located in <CFXROOT>/bin/<os>.
• ANSYS (p. 26)
• CFX Def/Res (p. 27)
• CFX-4 (p. 27)
• CFX-5.1 (p. 27)
• CFX-TfC (p. 29)
• CGNS (p. 29)
• Fluent (p. 30)
• GridPro/az3000 (p. 30)
• I-DEAS (p. 31)
• ICEM CFX (p. 31)
• PATRAN (p. 31)
• NASTRAN (p. 32)
• CFX-TASCflow (p. 32)
2.5.1. ANSYS
Imports an ANSYS file. The external import routine is ImportANSYS. Available options are:
-v Verbose output. Echo additional data to stdout during the import.
-E Import Elements of the same type as regions.
-A Import ANSA parts as regions.
26
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Import Programs
-S Display a list of all supported element types.
2.5.2. CFX Def/Res
Imports the mesh from a CFX-Solver input or results file. The external import routine is ImportDef.
Available options are:
-v Verbose output. Echo additional data to stdout during the import.
-I Read mesh from the initial timestep in the file.
-L Read mesh from the last timestep in the file.
-T<timestep> Read mesh from the timestep specified (Transient files)
2.5.3. CFX-4
Imports a CFX-4 grid file. The external import routine is ImportCFX4.
Available options are:
-v Verbose output. Echo additional data to stdout during the import.
-C Read coordinates as being in cylindrical coordinates.
-i Included interfaces in regions.
-3 Include USER3D and POROUS regions as 3D regions.
-c Import blocked-off conducting solid regions as 3D regions.
-l Include blocked-off solid regions as 3D regions.
-X Import axisymmetric problem with default values in geometry file.
-a <nk> Override the number of planes created in the k direction by nk (for example, split theta with
nk planes) for axisymmetric import.
-A <theta> Create a total sector of theta degrees for axisymmetric import.
-S Rename multiple symmetry planes with the same name to conform to CFX-Solver requirements
(that is, must lie in a plane).
2.5.4. CFX-5.1
Imports a CFX-5.1 results file. The external import routine is ImportCFX5.
Available options are:
-v Verbose output. Echo additional data to stdout during the import.
-f Input file is formatted.
-u Input file is unformatted (Fortran).
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
27
Volume Mesh Import API
-M <machine type> Set the machine type in the case of a binary or unformatted file so that data
conversion may be done if needed. The default file format is 32-bit IEEE (Iris, Sun, HP, IBM). The currently
recognized machine types are:
• IEEE - generic 32-bit IEEE machine.
• BSIEEE - generic 32-bit byteswapped IEEE machine.
• IBM - IBM 32-bit IEEE.
• IRIS - Iris 32-bit IEEE.
• HP - HP 32-bit IEEE.
• SUN - Sun 32-bit IEEE.
• ALPHA - Compaq Tru64 UNIX Alpha 64-bit byte-swapped IEEE.
• DOS - DOS 16-bit byte-swapped IEEE.
• Compaq Tru64 UNIX - Compaq Tru64 UNIX 32-bit byte-swapped IEEE.
• CRAY - Cray 64-bit format.
• CONVEX - native Convex floating point format.
• Windows - 32-bit Windows.
The argument machine type is case insensitive, and only the first 2 characters are needed (any others
are ignored).
-M <machine type> Set the machine type in the case of a binary or unformatted file so that data
conversion may be done if needed. The default file format is 32-bit IEEE (Iris, Sun, HP, IBM). The currently
recognized machine types are:
• IEEE - generic 32-bit IEEE machine.
• BSIEEE - generic 32-bit byteswapped IEEE machine.
• IBM - IBM 32-bit IEEE.
• IRIS - Iris 32-bit IEEE.
• HP - HP 32-bit IEEE.
• SUN - Sun 32-bit IEEE.
• ALPHA - Compaq Tru64 UNIX Alpha 64-bit byte-swapped IEEE.
• DOS - DOS 16-bit byte-swapped IEEE.
• Compaq Tru64 UNIX - Compaq Tru64 UNIX 32-bit byte-swapped IEEE.
• CRAY - Cray 64-bit format.
• CONVEX - native Convex floating point format.
28
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Import Programs
• Windows - 32-bit Windows.
The argument machine type is case-insensitive, and only the first two characters are needed (any others
are ignored).
2.5.5. CFX-TfC
Imports a CFX-TfC 1.3 mesh file. The external import routine is ImportGEM.
Available options are:
-v Verbose output. Echo additional data to stdout during the import.
-f Input file is formatted.
-u Input file is unformatted (Fortran).
-r Read regions from a BFI file.
-b <file> Use file as a BFI filename instead of default name.
-M <machine type> Set the machine type in the case of a binary or unformatted file so that data
conversion may be done if needed. The default file format is 32-bit IEEE (Iris, Sun, HP, IBM). The currently
recognized machine types are:
• IEEE - generic 32-bit IEEE machine.
• BSIEEE - generic 32-bit byteswapped IEEE machine.
• IBM - IBM 32-bit IEEE.
• IRIS - Iris 32-bit IEEE.
• HP - HP 32-bit IEEE.
• SUN - Sun 32-bit IEEE.
• ALPHA - Compaq Tru64 UNIX Alpha 64-bit byte-swapped IEEE.
• DOS - DOS 16-bit byte-swapped IEEE.
• Compaq Tru64 UNIX - Compaq Tru64 UNIX 32-bit byte-swapped IEEE.
• CRAY - Cray 64-bit format.
• CONVEX - native Convex floating point format.
• Windows - 32-bit Windows.
The argument machine type is case insensitive, and only the first 2 characters are needed (any others
are ignored).
2.5.6. CGNS
Imports a CGNS file. The external import routine is ImportCGNS. Available options are:
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
29
Volume Mesh Import API
-v Verbose output. Echo additional data to stdout during the import.
-b Read a grid from the specific CGNS base.
-B Read all CGNS bases. (default)
-c Read BOCO information as 2D regions.
-f Import Family Information as regions.
-E Import each Element Section as a separate region.
-I Import each side of a connection as a separate region.
-P Do not add the Zone name as a prefix to any region being defined.
2.5.6.1. SplitCGNS.exe
The SplitCGNS.exe program will take a single CGNS file and split it into multiple files on a "file per
problem basis". The method for running this is:
SplitCGNS.exe [ -l ] <filename> <basename>
If the file contains two problems called "Pipe" and "Elbow", the import filter will only currently read
"Pipe", but using SplitCGNS will produce two files called basename_Pipe.cgns and basename_Elbow.cgns each containing a single problem that can then be selected for import via the normal
method.
Specifying the "-l" option "links" the part of the data in the original file to the created file using a relative pathname. The created file does not therefore need to duplicate data.
The "-l" option should only be used if the original file and resulting files are going to be kept relative
to each other (that is, if when SplitCGNS was run the original file was in ../../example.cgns, it
must always remain in this position relative to the created files).
2.5.7. Fluent
Imports Fluent msh and cas files. The external import routine is ImportFluent. The import routine
will read the mesh information from the .cas or .msh file.
Available command line options are:
-v Verbose output. Echo additional data to stdout during the import.
-I Import interior boundary conditions.
2.5.8. GridPro/az3000
Imports a GridPro/az3000 grid and connectivity file from Program Development Corporation (PDC).
The external import routine is ImportPDC. The import routine will attempt to determine the connectivity
file associated with the grid file by appending the extension conn to the grid filename. If the file is not
found, then the grid filename extension will be replaced by conn and the new file checked for. If neither
of these are found, the import routine will look for a file named conn.tmp, and if found will use it. A
command line option (-c) is also available to explicitly name the connectivity file.
30
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Import Programs
If a connectivity file is found, the interface information in the file will be used to eliminate the duplicate
nodes at block interfaces, and boundaries conditions will be imported as regions into CFX. If the
boundary condition is named in the connectivity file, then that name will be used for the region name,
else the default name UnnamedRegionX with the X replaced by a number will be used. If a connectivity
file is not found, or the command line option to ignore the connectivity file is given (-i), then only the
grid file will be imported, resulting in duplicate nodes at the block interfaces. You may then want to
eliminate these duplicate nodes with the command line option (-d or -D).
Available options are:
-v Verbose output. Echo additional data to stdout during the import.
-i Ignore the connectivity file. Duplicate nodes will result and no regions will be imported.
-c <connfile> Set the name of the connectivity file associated with the grid file to connfile.
-p Include periodic boundary conditions as regions. These are not normally included in the import.
Setting this flag will result in these being imported as regions.
-q Read from the property file
-P <propfile> Set the name of the property file associated with the grid file to propfile.
-3 Import grid blocks as 3D regions
2.5.9. I-DEAS
Imports an I-DEAS Universal file from SDRC. The external import routine is ImportIDEAS. Reads datasets
781 and 2411 (nodes) as nodes, 780 and 2412 (elements) as elements, and nodes (type 7) from datasets
752 and 2417 (permanent groups) as regions. All other datasets are read, but not processed.
Available options are:
-v Verbose output. Echo additional data to stdout during the import.
-n Import nodes in a PERMANENT group as a 2D region.
-l Import elements in a PERMANENT group as a 3D region.
-f Import faces in a PERMANENT group as a 2D region.
2.5.10. ICEM CFX
Imports a file written for CFX by ICEM Tetra. The external import routine is ImportICEM. Available
options are:
-v Verbose output. Echo additional data to stdout during the import.
-P Read coordinate data from a binary file as double precision.
2.5.11. PATRAN
Imports a PATRAN Neutral file. The external import routine is ImportPatran. Reads packet 01 (nodes)
as nodes, packet 02 (elements) as elements, and nodes (type 5) from packet 21 (named groups) as regions.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
31
Volume Mesh Import API
A command line option is available to read packet 06 (loads) as regions also. All other packets are read,
but not processed.
Available options are:
-v Verbose output. Echo additional data to stdout during the import.
-l Import packet 06 (distributed loads) as regions. The regions will be assigned the name PatranLoadX
where the X is replaced by the load ID number.
2.5.12. NASTRAN
Imports a NASTRAN file. The external import routine is ImportMSC. Currently reads only nodes (GRID),
tet (CTETRA) and hex (CHEXA) elements.
Available options are:
-v Verbose output. Echo additional data to stdout during the import.
-l Import PLOAD4 datasets as 2D regions.
-s Import PSOLID datasets as 3D regions.
2.5.13. CFX-TASCflow
Imports TASCflow Version 2 files. The external import routine is ImportGRD. The import routine will
read the mesh information from the GRD file and automatically remove duplicate nodes where interfaces
are defined and are 1:1.
Available command line options are:
-v Verbose output. Echo additional data to stdout during the import.
-V More verbose output.
-i Ignore the blockoff file (BCF).
-c Ignore GCI file.
-o Old style 2.4 format.
-b <file> Specifies a bcf file that contains blocked-off regions (boundary condition information is
ignored). For details, see CFX-TASCflow Files in the CFX-Pre User's Guide.
-g <file> Specifies the gci file to import. For details, see CFX-TASCflow Files in the CFX-Pre User's
Guide.
-f Formatted (ASCII) GRD file.
-u Fortran unformatted GRD file.
-3 Import labelled 3D regions.
32
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 3: Mesh and Results Export API
This chapter describes how to create a custom program for exporting mesh and results data. Information
on using such a program is given in Using a Customized Export Program.
This chapter describes:
3.1. Creating a Customized Export Program
3.2. Compiling Code with the Mesh and Results Export API
3.3. Linking Code with the Mesh and Results Export API
3.4. Details of the Mesh Export API
3.1. Creating a Customized Export Program
The mesh and results contained within an ANSYS CFX results file can be exported in many formats,
ready for input into postprocessing software other than CFD-Post, MSC/PATRAN, EnSight and Fieldview.
To do this, you would write a customized export program that calls routines from the Export Application
Programming Interface (API). However, this is recommended only for advanced users, because it involves
at least some knowledge of C or C++ programming language.
Once an export program has been created, it can be used by any number of users; so if other ANSYS
CFX users at a site regularly use a different postprocessor, it may be worth contacting a system administrator to find out if such a format has already been defined.
To define a new format, use the export API. The general steps to follow are:
1.
Create a file that contains instructions needed to build the format in C.
This is most easily done by editing the template file provided (which is written in C). For details,
see An Example of an Export Program (p. 34).
2.
Compile your C program.
For details, see Compiling Code with the Mesh and Results Export API (p. 45).
3.
Link the C program into the CFX code.
For details, see Linking Code with the Mesh and Results Export API (p. 45).
4.
Use the program.
For details, see Using a Customized Export Program.
Numerous keywords are required for development and use of custom export files. For details, see
cfx5export Arguments.
An example source routine can be used as the basis of a customized program; one is given in the next
section.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
33
Mesh and Results Export API
3.1.1. An Example of an Export Program
The following is an annotated listing of the C source code for a reasonably simple example of a customized Export program. The full source code is available for use as a template and is located in CFX/examples/ExportTemplate.c, where CFX is the directory in which CFX is installed.
The example program is a reasonably simple example of an export program, which opens a CFX results
file, writes a geometry file (ignoring pyramid elements) and several files containing results. After the
program listing, a sample of the output produced is shown.
3.1.1.1. File Header
The file header uses several #include entries. The first set includes standard header files.
#include
#include
#include
#include
<stdio.h>
<string.h>
<stdlib.h>
<io.h>
The second set includes cfx5export header files.
#include "cfxExport.h"
#include "getargs.h"
Obtaining CFX-Mesh and Results Export API header files is described in more detail. For details, see
Linking Code with the Mesh and Results Export API (p. 45).
3.1.1.2. Allowed Arguments
The definition of allowed arguments appears as:
static char options[] = "u:d:t:cif";
The following piece of code simply defines the message that is printed if you enter incorrect options
to the program.
static char *usgmsg[] = {
"usage: ExportTemplate [options] res_file [basename]",
" options are:",
" -u<level>
= user level of interest",
" -d<domain>
= domain of interest (default is 0 - all the domains",
"
are combined into a single domain)",
" -t<timestep> = timestep of interest (if set to -1, all timesteps",
"
are exported)"
" -c
= use corrected boundary node data",
" -i
= include boundary node only data",
" -f
= get info on the res_file (No output is created)",
" <basename> is the base filename for Template file output.",
"If not specified, it defaults to ‘res_file’. The Template",
"geometry file will be written to <basename>.geom, the",
"results file to <basename>.res, and the variables to",
"<basename>.s## or <basename>.v## where ## is the variable",
"number and s indicates a scalar and v a vector.",
NULL
};
3.1.1.3. Main Program Initialization
As is standard, the variables argc and argv are the number of arguments and a pointer to the argument
list. The variable cfxCNT_SIZE and the types cfxNode and cfxElement are defined in the header
file cfxExport.h as are all variables and functions starting with the letters cfx. For details, see Mesh
34
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating a Customized Export Program
and Results Export API (p. 33). The variables level, zone, alias, bndfix and bnddat are used for
setting the default values for the various parameters that can be set on the command line of the program.
void main (int argc, char *argv[])
{
char *pptr;
char baseFileName[256], fileName[256], errmsg[256];
int i, n, counts[cfxCNT_SIZE], dim, length, namelen;
int nnodes, nelems, nscalars, nvectors, nvalues;
int level = 1, zone = 0, alias = 1, bndfix = 0, bnddat = 0;
int timestep = -1, infoOnly = 0;
int ts, t, t1, t2;
int nTimeDig = 1;
/* number of digits in transient file suffix */
char zoneExt[256];
/* zone extension added to the base filename */
int isTimestep = 0;
float timeVal = 0.0; /* time value in the single timestep mode */
char *wildcard = { "******" }; /* used in transient file specification */
FILE *fp;
cfxNode *nodes;
cfxElement *elems;
float *var;
The variable cfxCNT_SIZE and the types cfxNode and cfxElement are defined in the header file
cfxExport.h as are all variables and functions starting with the letters cfx. For details, see Mesh
and Results Export API (p. 33). The variables level, zone, alias, bndfix and bnddat are used for
setting the default values for the various parameters that can be set on the command line of the program.
The following line prints an error message if there are not enough arguments to proceed.
if (argc < 2)
cfxUsage (usgmsg, NULL);
The following piece of code reads the specified options and assigns values to certain variables accordingly.
If an invalid or incomplete option is specified, then getargs prints an error message and the export
program stops.
while ((n = getargs (argc, argv, options)) > 0) {
switch (n) {
case ‘u’:
level = atoi (argarg);
break;
case ‘d’:
zone = atoi (argarg);
break;
case ‘t’:
timestep = atoi (argarg);
isTimestep = 1;
break;
case ‘c’:
bndfix = 1;
break;
case ‘i’:
bnddat = 1;
break;
case ‘f’:
infoOnly = 1;
break;
}
}
After this, the level variable contains the user level specified. All results are output if they are of this
user level or below it. The zone variable contains the domain number that you specified. The variable
alias determines whether the variables are referred to by their long names or short names. The default
here is for short names to be used because some post-processors need variable names to contain no
spaces, but you are encouraged to use long variable names wherever possible. The variable bndfix
determines whether the variables are exported with corrected boundary node values - if bndfix is set
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
35
Mesh and Results Export API
to 1, then corrected values are used. Finally, bnddat determines whether variables that contain
meaningful values only on the boundary (such as Yplus) are exported or not; if bnddat is set to 1, then
these variables are exported.
3.1.1.4. Checking File Names
The following code checks to make sure that a CFX results file has been specified, and that it can be
read by the export program. If this is not the case, the export program exits.
/* CFX-5 results file */
if (argind >= argc)
cfxUsage (usgmsg, "CFX-5 results file not specified");
if (access (argv[argind], 0)) {
fprintf (stderr, "result file <%s> does not exist\n", argv[argind]);
exit (1);
}
The following code writes the basename specified to the character array baseFileName. If one was
not specified, then it defaults to the name of the results file specified. A basename name may be specified
in another directory (for example, “../template/output”). However, later in the code this basename
without the preceding directory information is required (in this example “output”); and so the pointer
pptr is assigned to point to the first character of this name.
/* base file name */
if (argind + 1 < argc)
strcpy (baseFileName,
else
strcpy (baseFileName,
if (NULL != (pptr = strrchr
pptr++;
else if (NULL != (pptr =
pptr++;
else
pptr = baseFileName;
argv[argind+1]);
argv[argind]);
(baseFileName, ‘/’)))
strrchr (baseFileName, ‘\\’)))
The following code checks that the results file that will be produced by the export program will not
overwrite an existing results file.
/* don’t overwrite results file */
sprintf (fileName, "%s.res", baseFileName);
if (0 == strcmp (argv[argind], fileName)) {
fprintf (stderr, "Template res file would overwrite CFX results file\n");
fprintf (stderr, "Need to select new Template output base file name\n");
exit (1);
}
3.1.1.5. Opening the CFX Results File
The following code prints a message to the screen telling you that the program is reading the results
file. It then calls cfxExportInit, which must always be called before any of the other export routines.
The variable n is set to equal the number of zones in the results file. If the -f option has been selected,
information about the results file will be displayed. The number of domains to be exported is also determined so that the format of the exported file includes the appropriate suffix. Finally, a check is made
to make sure that the zone (if any) that you specified in the program options is a valid zone for this
results file.
/* open CFX-5 results file */
printf ("\nreading CFX results from <%s>\n", argv[argind]);
n = cfxExportInit (argv[argind], NULL);
if (infoOnly) {
int nt;
printf("\n%d domains:\n", n);
for(i = 1; i <= n; i++)
36
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating a Customized Export Program
printf(" %d
%s\n", i, cfxExportZoneName(i));
nt = cfxExportTimestepCount();
printf("%d timesteps:\n", nt);
if(nt) {
for(i = 1; i <= nt; i++)
printf(" %d\n", cfxExportTimestepNumGet(i));
}
cfxExportDone();
exit (0);
}
/* determine the zone suffix for the export files */
strcpy(zoneExt, "");
if(zone == 0) {
printf ("processing all domains\n");
cfxExportSetVarParams(bndfix, level);
}
else {
printf ("processing domain %d\n", zone);
if(n != 1) {
float f;
int nZoneDig = 0;
/* count number of digits needed to fit any zone number */
f = (float) n;
while((f /= 10) >= 1) nZoneDig++;
sprintf(zoneExt, "_d%*.*d", nZoneDig, nZoneDig, zone);
}
}
if (cfxExportZoneSet (zone, counts) < 0)
cfxExportFatal ("invalid zone number");
The following code is ignoring any pyramid elements (elements with 5 nodes) and decreases nelems
by the number of pyramid elements. It then checks to make sure that neither the number of nodes nor
the number of elements is zero; if so, the program exits with return code -1.
The first two lines focus on the number of nodes in the zone and the number of elements in the zone.
nnodes = cfxExportNodeCount();
nelems = cfxExportElementCount();
if (counts[cfxCNT_PYR]) {
printf ("%d pyramid elements found - they are being ignored\n",
counts[cfxCNT_PYR]);
nelems -= counts[cfxCNT_PYR];
}
if (!nnodes || !nelems)
cfxExportFatal ("no nodes and/or elements");
3.1.1.6. Timestep Setup
The following code determines whether all of the timesteps, a specific timestep or the final timestep
(steady-state) have been selected for export.
if(isTimestep && timestep == -1 && !cfxExportTimestepCount()) {
isTimestep = 0;
}
if(isTimestep) {
int i;
float f;
if(timestep == -1) {
printf("processing all timesteps\n");
t1 = 1;
t2 = cfxExportTimestepCount() + 1;
}
else {
int isFound = 0;
printf("processing timestep %d\n", timestep);
for(i = 1; i <= cfxExportTimestepCount() + 1; i++)
if(cfxExportTimestepNumGet(i) == timestep) {
timeVal = cfxExportTimestepTimeGet(i);
t1 = t2 = i;
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
37
Mesh and Results Export API
isFound = 1;
break;
}
if(!isFound) {
sprintf(errmsg, "\nTimestep %d not found. "
"Use -f to see the list of valid timesteps.\n", timestep);
cfxExportFatal (errmsg);
}
}
/* count number of digits needed to fit any timestep number */
f = (float) cfxExportTimestepCount();
while((f /= 10) >= 1) nTimeDig++;
}
else {
timeVal = cfxExportTimestepTimeGet(cfxExportTimestepCount() + 1);
timestep = cfxExportTimestepNumGet(cfxExportTimestepCount() + 1);
t1 = t2 = cfxExportTimestepCount() + 1;
}
3.1.1.7. Geometry File Output
The following code opens the geometry file basename.geom, printing an error if it cannot be opened
for any reason. A message is then displayed informing you that the application is writing the geometry
file.
/* Template geometry output */
sprintf (fileName, "%s.geom", baseFileName);
if (NULL == (fp = fopen (fileName, "w+"))) {
sprintf (errmsg, "can’t open <%s> for output", fileName);
cfxExportFatal (errmsg);
}
printf ("writing Template Geometry file to <%s>\n", fileName);
The header of this file is shown after the program listing.
/* write header
fprintf( fp,
fprintf( fp,
fprintf( fp,
fprintf( fp,
*/
"Template Geometry file exported from CFX\n");
" \n");
"node id given\n");
"element id off\n");
The following code writes first the word "coordinates" and the number of nodes that will be written.
The pointer nodes is initialized to point at the data for the first node and the node data is written into
the geometry file. For each node, a node number is written, followed by the three coordinates of that
node. Note that n ranges between 0 and nnodes-1. This program adds 1 to each node number so
that the nodes in the geometry file are numbered between 1 and nnodes. When it has finished, the
cfxExportNodeFree routine frees the memory that was used to store the node data, and finally the
word "done" is printed on the screen to alert you that it has finished writing the node data.
/* write nodes */
fprintf( fp, "coordinates\n");
fprintf( fp, "%8d\n", nnodes );
nodes = cfxExportNodeList();
printf (" writing %d nodes ...", nnodes);
fflush (stdout);
for (n = 0; n < nnodes; n++, nodes++) {
fprintf( fp, "%8d %12.5e %12.5e %12.5e\n", n + 1, nodes->x,
nodes->y, nodes->z );
}
cfxExportNodeFree();
printf (" done\n");
Next, the data for each element must be written.
Firstly, some general information is written. Then the data for each element type is written in turn.
38
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating a Customized Export Program
/* write elements */
fprintf( fp, "part 1\n" );
fprintf( fp, "volume elements\n");
printf (" writing %d elements...", nelems);
fflush (stdout);
For tetrahedral elements, the word "tetra4" is written to the file, followed by the number of tetrahedral
elements written.
/* tets */
fprintf( fp, "tetra4\n");
fprintf( fp, "%8d\n", counts[cfxCNT_TET] );
The following code is executed only if the number of tetrahedral elements is non-zero. Assuming this,
elems is set to point to the list of elements stored in the results file. The index n loops over all the
elements. For each element, the following step is carried out: “If the element is a tetrahedron, then loop
over its four vertices and write their node numbers to the geometry file, then start a new line (ready
for the next set of data).” The output produced can be seen in the examples of the exported files in
the next section.
if (counts[cfxCNT_TET]) {
elems = cfxExportElementList();
for (n = 0; n < nelems; n++, elems++) {
if (cfxELEM_TET == elems->type) {
for (i = 0; i < elems->type; i++)
fprintf (fp, "%8d", elems->nodeid[i]);
putc (‘\n’, fp);
}
}
}
For wedges (triangular prisms) and hexahedral elements, the same procedure is followed. However,
there is a slight difference in the way that the fprintf line is written for hexahedral elements. This
is because the order that the element nodes are written to the geometry file is different to the order
in which they were read from the results file. This may need to be done if a post-processor has a different
convention for node order than the one that the cfx5export node routines have. The order the nodes
are written in will affect which node is connected to which. The node ordering for exported elements
is illustrated in cfxExportElementList (p. 52).
/* wedges */
fprintf( fp, "penta6\n");
fprintf( fp, "%8d\n", counts[cfxCNT_WDG] );
if (counts[cfxCNT_WDG]) {
elems = cfxExportElementList();
for (n = 0; n < nelems; n++, elems++) {
if (cfxELEM_WDG == elems->type) {
for (i = 0; i < elems->type; i++)
fprintf (fp, "%8d", elems->nodeid[i]);
}
putc (‘\n’, fp);
}
}
/* hexes */
fprintf( fp, "hexa8\n");
fprintf( fp, "%8d\n", counts[cfxCNT_HEX] );
if (counts[cfxCNT_HEX]) {
elems = cfxExportElementList();
for (n = 0; n < nelems; n++, elems++) {
if (cfxELEM_HEX == elems->type)
fprintf (fp, "%8d%8d%8d%8d%8d%8d%8d%8d\n",
elems->nodeid[0], elems->nodeid[1],
elems->nodeid[3], elems->nodeid[2],
elems->nodeid[4], elems->nodeid[5],
elems->nodeid[7], elems->nodeid[6]);
}
}
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
39
Mesh and Results Export API
Then the geometry file is closed and the memory occupied by the element data is freed.
printf (" done\n");
fclose (fp);
cfxExportElementFree();
3.1.1.8. Template Results File
Despite its name, the Template results file does not contain any actual values of results. It simply contains
information about how many variables there are and in which file each is stored.
The first job is to make sure that there are some results for export. First, the code checks that there is
a nonzero number of variables that have the specified user level. Then it counts the number of scalar
and vector variables that will be exported. To be exported, a variable must:
1.
Have a dimension of 1 (scalar variable) or 3 (vector variable) and,
2.
Either be a variable with useful values everywhere in the zone or be a variable that has values only on the
boundaries (in which case it will be exported only if you asked to "include boundary node only data" by
specifying the option -i when starting the export program, which translated to setting bnddat = 1
when the arguments were processed).
Review the cfxExportVariableSize routine if this logic is unclear. For details, see cfxExportVariableSize (p. 58).
Once results are identified, the code calculates the variable namelen, which is the length of the longest
variable name to be exported (the alias variable was set when processing the arguments passed to
the export program, and depends upon whether you wanted to use long names or short names). If
there are no vector or scalar variables to be exported, the export program exits.
/* output results file */
nscalars = nvectors = namelen = 0;
if ((nvalues = cfxExportVariableCount(level)) > 0) {
for (n = 1; n <= nvalues; n++) {
cfxExportVariableSize (n, &dim, &length, &i);
if ((1 != dim && 3 != dim) ||
(length != nnodes && length != bnddat))
continue;
if (1 == dim)
nscalars++;
else
nvectors++;
i = strlen (cfxExportVariableName (n, alias));
if (namelen < i)
namelen = i;
}
}
if (0 == (nscalars + nvectors)) {
cfxExportDone ();
exit (0);
}
The following code checks that the results file can be opened for writing to, and exits if not. The number
of scalar and vector variables are written to the file, followed by some numbers (which EnSight, for example, requires) that are always the same for any export of this kind.
sprintf (fileName, "%s.res", baseFileName);
if (NULL == (fp = fopen (fileName, "w+"))) {
sprintf (errmsg, "can’t open <%s> for writing", fileName);
cfxExportFatal (errmsg);
}
printf ("writing Template results file to <%s>\n", fileName);
fflush (stdout);
40
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating a Customized Export Program
fprintf( fp, "%d %d 0\n", nscalars, nvectors );
fprintf( fp, "%d\n", t2 - t1 + 1 );
for(i = t1; i <= t2; i++) {
fprintf( fp, "%13.4e", cfxExportTimestepTimeGet(i));
if(!(i % 6)) fprintf( fp, "\n");
}
fprintf( fp, "\n");
if(isTimestep && t1 != t2)
fprintf( fp, "0 1\n");
Next, for each scalar variable, a line is written that contains the filename where the scalar will be written,
and then the name of the variable. Note that the filename is not the basename, but the basename with
all the directory structure (if any) stripped off the front. For details, see Checking File Names (p. 36).
This is done because these file will be written in the same directory as this Template results file, so there
is no need for directory information.
if ( nscalars ) {
for (n = 1; n <= nvalues; n++) {
cfxExportVariableSize (n, &dim, &length, &i);
if (1 == dim && (length == nnodes || length == bnddat))
if(!isTimestep)
fprintf (fp, "%s%s.s%2.2d %s\n", pptr, zoneExt,
n, cfxExportVariableName(n, alias));
else if(t1 == t2)
fprintf (fp, "%s%s_t%d.s%2.2d %s\n", pptr, zoneExt,
cfxExportTimestepNumGet(t1), n,
cfxExportVariableName(n, alias));
else
fprintf (fp, "%s%s_t%*.*s.s%2.2d %s\n", pptr, zoneExt,
nTimeDig, nTimeDig, wildcard, n,
cfxExportVariableName(n, alias));
}
}
The same information is then written for each vector variable and the Template results file is closed.
if ( nvectors ) {
for (n = 1; n <= nvalues; n++) {
cfxExportVariableSize (n, &dim, &length, &i);
if (3 == dim && (length == nnodes || length == bnddat))
if(!isTimestep)
fprintf (fp, "%s%s.v%2.2d %s\n", pptr, zoneExt,
n, cfxExportVariableName(n, alias));
else if(t1 == t2)
fprintf (fp, "%s%s_t%d.v%2.2d %s\n", pptr, zoneExt,
cfxExportTimestepNumGet(t1), n,
cfxExportVariableName(n, alias));
else
fprintf (fp, "%s%s_t%*.*s.v%2.2d %s\n", pptr, zoneExt,
nTimeDig, nTimeDig, wildcard, n,
cfxExportVariableName(n, alias));
}
}
fclose( fp );
3.1.1.9. Creating Files with Results for Each Variable
The results for each variable are written to separate files, called <basename>.s01, <basename>.s02,
<basename>.v03, for example. Each file with an extension containing a letter “s” contains a scalar
variable, and each with a “v” contains a vector variable. Which variable is written to each file is tabulated
in the Template results file that has just been written.
The following code reads the information for each variable, after you decide that it should be exported
- the logic is very similar to that used when counting the relevant variables when creating the Template
results file. The marked if loop executes if the variable needs to be exported. It checks to make sure
that the variable information can be read, and (assuming it can) then builds the filename and checks
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
41
Mesh and Results Export API
to see if it can be opened. Continuing, it writes to the screen where it is putting the variable, and then
loops through all the values, writing them to the file, inserting a new line every six values. After each
variable, the memory used to store that variable is restored.
After all the variable files have been written, the program calls the cfxExportDone routine, which
close the CFX results file, and frees up any remaining memory. This routine must be the last call to any
of the API routines. The program then exits.
Note
This program makes no use of any of the region routines, which enable access to boundary
condition data, nor the volume routines that enable access to the subdomains that are
defined for a problem.
• Region Routines (p. 53)
• Volume Routines (p. 55)
/* output each timestep to a different file */
for(t = t1; t <= t2; t++) {
ts = cfxExportTimestepNumGet(t);
if(cfxExportTimestepSet(ts) < 0) {
continue;
}
/* build file name and open file */
if(!isTimestep)
sprintf( fileName, "%s%s.%c%2.2d", baseFileName, zoneExt,
1 == dim ? ‘s’ : ‘v’, n);
else if(t1 == t2)
sprintf( fileName, "%s%s_t%d.%c%2.2d", baseFileName, zoneExt,
ts, 1 == dim ? ‘s’ : ‘v’, n);
else
sprintf( fileName, "%s%s_t%*.*d.%c%2.2d", baseFileName, zoneExt,
nTimeDig, nTimeDig, t-1, 1 == dim ? ‘s’ : ‘v’, n);
if (NULL == (fp = fopen (fileName, "w+"))) {
sprintf (errmsg, "can’t open <%s> for writing\n", fileName);
cfxExportFatal (errmsg);
}
printf (" %-*s -> %s ...", namelen,
cfxExportVariableName(n, alias), fileName);
fflush (stdout);
fprintf( fp, "%s\n", cfxExportVariableName(n, alias));
length = nnodes * dim;
for ( i = 0; i < length; i++, var++ ) {
fprintf( fp, "%12.5e ", *var );
if ( i && 5 == (i % 6) )
putc (‘\n’, fp);
}
if ( 0 != ( nvalues % 6 ) )
putc( ‘\n’, fp );
fclose( fp );
cfxExportVariableFree (n);
printf (" done\n");
}
}
} /* loop for each timestep */
cfxExportDone();
exit (0);
}
42
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Creating a Customized Export Program
3.1.2. Example of Output Produced
If the export program is correctly compiled and run, the following output is obtained. For details, see
Using a Customized Export Program.
In this example, the CFX results file contains three variables at user level 1: pressure, temperature and
velocity. This is in a file named file.res. No timesteps or domains were specified, and the basename was
specified as an example.
The following is displayed on screen:
reading CFX results from <file.res>
processing all domains
writing Template Geometry file to <example.geom>
writing 2365 nodes ... done
writing 11435 elements... done
writing Template results file to <example.res>
writing variable output files
Pressure
-> example.s01 ... done
Temperature -> example.s02 ... done
Velocity
-> example.v03 ... done
Five files are produced: the geometry file example.geom, the Template results file example.res,
and three variable files called example.s01, example.s02 and example.v03, which contain the
results for pressure, temperature and velocity, respectively. For details, see:
• example.geom (p. 43)
• example.res (p. 44)
• example.s01 (p. 44)
3.1.2.1. example.geom
The content of this file appears as:
Template Geometry file exported from CFX
node id given
element id off
coordinates
2365
1 2.00000e+00 0.00000e+00 0.00000e+00
2-2.00000e+00-6.51683e-07 0.00000e+00
3 2.00000e+00 0.00000e+00 2.00000e+00
4-2.00000e+00-6.51683e-07 2.00000e+00
5 3.00000e+00 1.00000e+00 5.00000e-01
....
....
....
2362-1.13337e+00 2.18877e-01 4.02491e-01
2363-1.12115e+00-3.66598e-01 2.22610e-01
2364 1.36924e+00 4.78359e-01 1.22588e-01
2365-3.30703e-01 1.38487e+00 2.23515e+00
part 1
volume elements
tetra4
11435
754
230
12
145
755
216
8
122
756
212
125
215
....
....
....
2365
496
475
474
penta6
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
43
Mesh and Results Export API
0
hexa8
0
3.1.2.2. example.res
The content of this file appears as:
2 1 0
1
0.0
0 1
example.s01 Pressure
example.s02 Temperature
example.v03 Velocity
3.1.2.3. example.s01
The content of this file appears as:
Pressure
1.42748e+04 1.42621e+04 1.43425e+04 1.43350e+04 1.44118e+04 1.44777e+04
1.38639e+04 1.37352e+04 1.44130e+04 1.44755e+04 1.37733e+04 1.37626e+04
....
....
....
1.39092e+04 1.40699e+04 1.24139e+04 1.34786e+04 1.34859e+04 1.37959e+04
3.1.3. Source Code for getargs.c
The following code is the C code that defines the functions cfxUsage and getargs, both of which
are called by the example listing above. You do not need to include this code with your custom export
program (it is automatically linked in if you use the compiler as described in the next section).
#include <stdio.h>
#include <string.h>
#include <ctype.h>
#include "getargs.h"
/*---------- usage -------------------------------------------------* display usage message and exit
*-------------------------------------------------------------------*/
void cfxUsage (
#ifdef PROTOTYPE
char **usgmsg, char *errmsg)
#else
usgmsg, errmsg)
char **usgmsg, *errmsg;
#endif
{
int n;
if (NULL != errmsg)
fprintf (stderr, "ERROR: %s\n", errmsg);
for (n = 0; NULL != usgmsg[n]; n++)
fprintf (stderr, "%s\n", usgmsg[n]);
exit (NULL != errmsg);
}
/*---------- getargs --------------------------------------------------* get option letter from argument vector or terminates on error
* this is similar to getopt()
*----------------------------------------------------------------------*/
int argind = 0; /* index into argv array */
char *argarg;
/* pointer to argument string */
int getargs (
#ifdef PROTOTYPE
int argc, char **argv, char *ostr)
#else
argc, argv, ostr)
int argc;
44
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Linking Code with the Mesh and Results Export API
char **argv, *ostr;
#endif
{
int argopt;
char *oli;
static char *place;
static int nextarg;
/* initialisation */
if (!argind)
nextarg = 1;
if (nextarg) { /* update scanning pointer */
nextarg = 0;
/* end of arguments */
if (++argind >= argc || ‘-’ != argv[argind][0])
return (0);
place = argarg = &argv[argind][1];
}
/* check for valid option */
if ((argopt = *place++) == ‘:’ ||
(oli = strchr (ostr, argopt)) == NULL) {
fprintf (stderr, "invalid command line option `%c’\n", argopt);
exit (1);
}
/* check for an argument */
if (*++oli != ‘:’) {
/* don’t need argument */
argarg = NULL;
if (!*place)
nextarg = 1;
}
else {
/* need an argument */
if (!*place) {
if (++argind >= argc) {
fprintf (stderr, "missing argument for option `%c’\n", argopt);
exit (1);
}
place = argv[argind];
}
argarg = place;
nextarg = 1;
}
return (argopt);
/* return option letter */
}
3.2. Compiling Code with the Mesh and Results Export API
Compilation of a customized executable must be performed using an appropriate compiler and compiler
flags.
The customized executable must also be linked with the provided Mesh and Results Export API library
and the provided i/o library as detailed in Linking Code with the Mesh and Results Export API (p. 45).
3.3. Linking Code with the Mesh and Results Export API
In order to build a customized export utility, it must be linked with several libraries. These libraries are
located in <CFXROOT>/lib/<os>/:
• libmeshexport.lib (on Windows), or libmeshexport.a (on Linux)
• libratlas_api.lib (on Windows), or libratlas_api.a (on Linux)
• libratlas.lib (on Windows), or libratlas.a (on Linux)
• libpgtapi.lib (on Windows), or libpgtapi.a (on Linux)
• libunits.lib (on Windows), or libunits.a (on Linux)
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
45
Mesh and Results Export API
• libcclapilt.lib (on Windows), or libcclapilt.a (on Linux)
• libio.lib (on Windows), or libio.a (on Linux)
3.3.1. Linux
On most Linux systems, build the executable with the command:
gcc export.c -o export.exe -I<CFXROOT>/include/ -L<CFXROOT>/lib/<OSDIR> -lmeshexport -lratlas_api -lratlas -lpgtapi
where <CFXROOT> is the directory in which CFX is installed and <OSDIR> is a directory name corresponding to the architecture of the machine. In this example, your own export program is named export.c and the executable file will be called export.exe.
The compiler flags and required libraries may vary, depending on the compiler and the custom program.
You can use the GCC compiler v4.6.1 with ANSYS CFX 15.0 or greater.
3.3.2. Windows
You can build the executables on Windows systems that have the C++ compiler of Microsoft Visual
Studio 2010. An example command line follows:
cl /MD /I "C:\Program Files\Ansys Inc\v162\CFX\include" ExportTemplate.c
/link /libpath:"C:\Program Files\Ansys Inc\v162\CFX\lib\winnt-amd64"
libcclapilt.lib libio.lib libmeshexport.lib libunits.lib libpgtapi.lib
libratlas_api.lib libratlas.lib
You can also write the export program in Fortran and then compile it using the recommended Fortran
compiler on Windows. An example command line follows:
ifort /MD /I "C:\Program Files\Ansys Inc\v162\CFX\include" /threads
/iface:mixed_str_len_arg ExportTemplate.F /exe:ExportTemplate.exe /libs:dll
/link /libpath:"C:\Program Files\Ansys Inc\v162\CFX\lib\winnt-amd64"
libcclapilt.lib libio.lib libmeshexport.lib libunits.lib libpgtapi.lib
libratlas_api.lib libratlas.lib
3.4. Details of the Mesh Export API
The full list of constants, data structures, types and functions available to the programmer are given in
the following sections:
3.4.1. Defined Constants and Structures
3.4.2. Initialization and Error Routines
3.4.3. Zone Routines
3.4.4. Node Routines
3.4.5. Element Routines
3.4.6. Region Routines
3.4.7. Face Routines
3.4.8. Volume Routines
3.4.9. Boundary Condition Routines
3.4.10. Variable Routines
46
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Details of the Mesh Export API
3.4.1. Defined Constants and Structures
The following constants and data structures are defined in the header file cfxExport.h, which should
be included in the export program.
3.4.1.1. Element Types
CFX can use 4 types of element, which are identified by the number of nodes: tetrahedrons (4 nodes),
pyramids (5 nodes), prisms/wedges (6 nodes), and hexahedrons (8 nodes). The element types are
identified in the Export API by the following constants:
#define
#define
#define
#define
cfxELEM_TET
cfxELEM_PYR
cfxELEM_WDG
cfxELEM_HEX
4
5
6
8
3.4.1.2. Volume List Types
The Export API contains functions that enable you to query how volumes are defined in the results file.
It is possible to request how a volume is defined in terms of nodes or elements. (For details, see Volume
Routines (p. 55).)
The following constants are defined in the header file and should be used as arguments to the Volume
routines:
#define cfxVOL_NODES 0
#define cfxVOL_ELEMS 1
3.4.1.3. Region List Types
The Export API contains functions that enable you to query how regions are defined in the results file.
It is possible to request how a region is defined in terms of nodes or faces. (For details, see Region
Routines (p. 53).)
The following constants are defined in the header file and should be used as arguments to the Region
routines:
#define cfxREG_NODES 0
#define cfxREG_FACES 1
In the case of nodes, the global node number is returned, while in the case of faces, the returned value
is a combination of the global element number and local face number of the element. The following
macros are available to enable you to extract the element and face number from the combined value:
#define cfxFACENUM(face) ((face) & 7)
#define cfxELEMNUM(face) ((face) >> 3)
3.4.1.4. Count Entries
Two routines exist for initializing the Export API (see cfxExportInit (p. 48)) and requesting the totals of
certain quantities in a zone (see cfxExportZoneSet (p. 49)). The array returned from both of these
routines requires the following constants to be used by the calling program to reference the correct
quantities.
enum cfxCounts {
cfxCNT_NODE = 0, /* number of nodes */
cfxCNT_ELEMENT, /* number of elements */
cfxCNT_VOLUME,
/* number of volumes */
cfxCNT_REGION, /* number of regions */
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
47
Mesh and Results Export API
cfxCNT_VARIABLE, /* number of variables */
cfxCNT_TET, /* number of tetrahedral elements */
cfxCNT_PYR, /* number of pyramid elements */
cfxCNT_WDG, /* number of wedge elements */
cfxCNT_HEX, /* number of hexahedral elements */
cfxCNT_SIZE /* size of count array */
};
3.4.1.5. Node Data Structure
Nodes are represented in the Export API using the following structure (note the change in data type
of x, y and z):
typedef struct cfxNode {
float x, y, z;
} cfxNode;
where x, y, and z are the coordinates of the node. A pointer to an array of these structures is returned
by cfxExportNodeList. For details, see cfxExportNodeList (p. 51).
3.4.1.6. Element Data Structure
Elements are represented by the Export API using the following structure:
typedef struct cfxElement {
int type;
int *nodeid;
} cfxElement;
where type is the element type and nodeid is an array of node numbers that define the topology of
the element. A pointer to an array of these structures is returned by cfxExportElementList. For
details, see Element Types (p. 47) and cfxExportElementList (p. 52).
3.4.2. Initialization and Error Routines
The following routines open and close the CFX results file, initialize the Export API, and handle fatal
error processing. The first call to any of the API routines must be cfxExportInit and the last call
should be cfxExportDone. For details, see:
• cfxExportInit (p. 48)
• cfxExportDone (p. 48).
3.4.2.1. cfxExportInit
int cfxExportInit (char *resfile, int counts[cfxCNT_SIZE])
Opens the CFX results file named resfile and initializes the Export API. This should be the first call
made to the API.
The routine returns the total number of zones. If the array counts is supplied to the routine (that is,
it is not NULL), the array is filled with values representing the total number of nodes, elements, volumes,
regions and variables for all the zones are returned in this array.
3.4.2.2. cfxExportDone
void cfxExportDone ()
48
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Details of the Mesh Export API
Closes the CFX results file and destroys any internal storage used by the API. This should be the final
call made to the Export API.
3.4.2.3. cfxExportError
void cfxExportError (void (*callback) (char *errmsg))
Specify a callback function that will be executed when a fatal error is generated by a call to cfxIm
portFatal (see cfxImportFatal (p. 16)). The argument, callback, is the function that will be called, it
should take an argument that is the error message passed to cfxImportFatal. It is the responsibility of
the function to terminate the application if required.
3.4.2.4. cfxExportFatal
void cfxExportFatal (char *errmsg)
Generate a fatal error message (errmsg) and close the ANSYS CFX results file. This routine also calls a
callback function, if one has been specified by cfxExportError (see cfxExportError (p. 49)). If no
callback function has been specified the function also terminates the application. There is no return
from this call.
3.4.3. Zone Routines
A zone is defined as groups of nodes or faces that are located on the external boundaries of the domain.
The following routines provide functionality for returning the number of zones in the open CFX results
file specifying and requesting the current zone, and destroying any internal storage associated with a
zone. All other routines in the Export API refer to quantities in the current zone being accessed by the
API. By default the current zone is the global zone (a combination of all zones in the ANSYS CFX results
file), but this can be the current zone can be altered by making a call to cfxExportZoneSet (see
cfxExportZoneSet (p. 49)). Once this call has been made, any other function returns information about
this zone until a subsequent call is made.
3.4.3.1. cfxExportZoneCount
int cfxExportZoneCount ()
Return the number of zones in the CFX results file.
3.4.3.2. cfxExportZoneSet
int cfxExportZoneSet (int zone, int counts[cfxCNT_SIZE])
Set the current zone being accessed by the Export API.
The value of zone should be between 1 and the value returned by cfxExportZoneCount (see cfxExportZoneCount (p. 49)) or 0 if the global zone is to be accessed.
The function returns 0 if the value of zone is invalid or the value zone if setting of the zone was successful.
The argument counts can be passed as a NULL pointer. In this case no information is returned to the
calling function other than the return value mentioned above. If counts is specified it must be at least
cfxCNT_SIZE in size, not specifying an array large enough can result in errors. In the case when counts
is supplied correctly the total number of nodes, elements, volumes, regions and variables will be returned.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
49
Mesh and Results Export API
3.4.3.3. cfxExportZoneGet
int cfxExportZoneGet ()
Returns the current zone number.
3.4.3.4. cfxExportZoneFree
void cfxExportZoneFree ()
While a zone is being accessed, internal storage is allocated, this storage should be deallocated when
no longer required. This can be done by calling cfxExportZoneFree or by calling cfxExportNode
Free, cfxExportElementFree, cfxExportVolumeFree, cfxExportRegionFree and cfxEx
portVariableFree. Details on each of these routines is available; see:
• cfxExportNodeFree (p. 51)
• cfxExportElementFree (p. 53)
• cfxExportVolumeFree (p. 56)
• cfxExportRegionFree (p. 54)
• cfxExportVariableFree (p. 60).
3.4.3.5. cfxExportZoneIsRotating
int cfxExportZoneIsRotating(double rotationAxis[2][3], double *angularVelocity)
Query whether the current zone is rotating and describe axis and angular velocity of the rotation if
applicable. Returns 1 if the current zone is rotating and 0 if it is not; for the combined zone the return
value is always -1. If successful the rotation axis is returned in rotationAxis and the velocity in an
gularVelocity in radians/second.
3.4.3.6. cfxExportZoneMotionAction
int cfxExportZoneMotionAction(const int zone, const int flag)
Specify whether grid coordinates and variables should have the appropriate rotation applied to them
if the zone is rotating so that grid coordinates appear in their correct locations and velocities (for examples) take this rotation into consideration. If cfxExportZoneList and cfxExportVariableList
should return rotated values, flag should be set to cfxMOTION_USE. The default behavior for a particular zone will be used if cfxMOTION_IGNORE is specified or this function is not called. If zone is not
valid or flag is not cfxMOTION_USE, cfxMOTION_IGNORE the return value will be -1 otherwise 0 is
returned.
3.4.4. Node Routines
Accessing nodes within the current zone (see cfxExportZoneSet (p. 49)) is performed by making calls
to the following functions.
It should be noted that the nodes for a zone are not loaded into the Export API until either cfxExport
NodeList (see cfxExportNodeList (p. 51)) or cfxExportNodeGet (see cfxExportNodeGet (p. 51))
are called. This reduces memory overheads in the API by not allocating space until required.
50
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Details of the Mesh Export API
When access to nodes in the current zone is no longer required, a call to cfxExportNodeFree (see
cfxExportNodeFree (p. 51)) should be made to deallocate any internal storage.
3.4.4.1. cfxExportNodeCount
int cfxExportNodeCount ()
Query the number of nodes defined in the current zone.
3.4.4.2. cfxExportNodeList
cfxNode *cfxExportNodeList ()
Return a pointer to an array of cfxNode elements (see cfxnode (p. 23)) containing the coordinate values
of each node in the current zone. The first node in the zone is the first element of the array, the second
is the second and so on.
The memory allocated to represent this information should be deallocated using cfxExportNodeFree
(see cfxExportNodeFree (p. 51)) when no longer required.
3.4.4.3. cfxExportNodeGet
int cfxExportNodeGet (int nodeid, double *x, double *y, double *z)
Query the coordinates of a specific node in the current zone.
The index (nodeid) is specified between 1 and the number of nodes returned by cfxExportNodeCount
(see cfxExportNodeCount (p. 51)). If the value of nodeid is out of range the return value is 0 otherwise
it is nodeid.
3.4.4.4. cfxExportNodeFree
void cfxExportNodeFree ()
Deallocate any internal storage allocated by the Export API after calls to cfxExportNodeList (see
cfxExportNodeList (p. 51)) and cfxExportNodeGet (see cfxExportNodeGet (p. 51)) have been made
in the current zone.
3.4.5. Element Routines
Accessing elements within the current zone (see cfxExportZoneSet (p. 49)) is performed by making calls
to the following functions. It should be noted that the elements for a zone are not loaded into the Export
API until either cfxExportElementList (see cfxExportElementList (p. 52)) or cfxExportElement
Get (see cfxExportElementGet (p. 52)) are called. This reduces memory overheads in the API by not
allocating space until required.
When access to elements in the current zone is no longer required a call to cfxExportElementFree
(see cfxExportElementFree (p. 53)) should be made to deallocate any internal storage.
3.4.5.1. cfxExportElementCount
int cfxExportElementCount ()
Query the number of elements defined in the current zone.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
51
Mesh and Results Export API
3.4.5.2. cfxExportElementList
cfxElement *cfxExportElementList ()
Return a pointer to an array of cfxElement elements (see cfxelem (p. 23)) containing the type and vertices
of each element in the current zone. The first element in the zone is the first element of the array, the
second the second and so on.
The memory allocated to represent this information should be deallocated using cfxExportElement
Free (see cfxExportElementFree (p. 53)) when no longer required.
The following diagrams show the order of the nodes and connections that ANSYS CFX uses for exporting
elements:
Note
The vertex ordering for the import API is different. For details, see cfxImportElement (p. 16).
3.4.5.3. cfxExportElementGet
int cfxExportElementGet (int elemid, int elemtype, int *nodelist)
Query the type and vertices of a specific element in the current zone.
The index (elemid) is specified between 1 and the number of elements returned by cfxExportEle
mentCount (see cfxExportElementCount (p. 51)). If the value of elemid is out of range the return value
is 0 otherwise it is elemid.
52
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Details of the Mesh Export API
The type of the element is returned in elemtype and the vertices defining the element in nodelist. Note
that nodelist must be large enough to hold the element number of vertices in the element (normally
an array of 8 integers is used as this allows space enough for all element types to be handled).
3.4.5.4. cfxExportElementFree
void cfxExportElementFree ()
Deallocates any internal storage allocated by making calls to cfxExportElementList (see cfxExportElementList (p. 52)) or cfxExportElementGet (see cfxExportElementGet (p. 52)).
3.4.6. Region Routines
Regions are groups of faces in an ANSYS CFX results file. Accessing regions within the current zone (see
cfxExportZoneSet (p. 49)) is performed by making calls to the following functions. It should be noted
that the region information is not loaded into the Export API until either cfxExportRegionList
(see cfxExportRegionList (p. 53)) or cfxExportRegionGet (see cfxExportRegionGet (p. 54)) are called.
This reduces memory overheads in the API by not allocating space until required.
When access to region in the current zone is no longer required a call to cfxExportRegionFree
(see cfxExportRegionFree (p. 54)) should be made to deallocate any internal storage.
3.4.6.1. cfxExportRegionCount
int cfxExportRegionCount ()
Query the number of regions defined in the current zone.
3.4.6.2. cfxExportRegionSize
int cfxExportRegionSize (int regnum, int type)
Query the number of faces (if type is cfxREG_FACES) or nodes (if type is cfxREG_NODES) defined
in the region identified by regnum in the current zone.
The function returns the number of faces or nodes in the current zone or 0 if either regnum is out of
range or type is invalid.
3.4.6.3. cfxExportRegionName
char *cfxExportRegionName (int regnum)
Query the name of the region in the current zone identifies by regnum.
The function returns the name of the region or NULL if the region number supplied is out of range.
The pointer returned points to static storage, which will be overwritten by the next call to cfxExport
RegionName.
3.4.6.4. cfxExportRegionList
int *cfxExportRegionList (int regnum, int type)
Query the nodes (type is cfxREG_NODES) or faces (cfxREG_FACES) that define a region. This function
returns a pointer to an array of node ids or face ids that define the region identified by regnum or NULL
if the region number is out of range or the type is not recognized. If type is specified as cfxREG_FACES,
the returned ids will represent faces. The element number and local element face number may be exRelease 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
53
Mesh and Results Export API
tracted from each face id returned by using the macros cfxELEMNUM and cfxFACENUM. The node
numbers for the face may be obtained by calling cfxExportFaceNodes. For details, see cfxExportFaceNodes (p. 54).
3.4.6.5. cfxExportRegionGet
int cfxExportRegionGet (int regnum, int type, int index, int *id)
Query the index’th element (type is cfxREG_ELEM) or index’th node (type is cfxREG_NODE) that
defines a region regnum in the current zone.
If regnum is out of range or type is not recognized or index is out of range, 0 is returned.
Otherwise id will contain the id of the appropriate node or face defining the region and the function
will return index.
If type is specified as cfxREG_FACES, the returned id will represent the identity of a face. The element
number and local element face number may be extracted from the id by using the macros cfxELEMNUM
and cfxFACENUM.
3.4.6.6. cfxExportRegionFree
void cfxExportRegionFree (int regnum)
Deallocate any internal data storage associated with the region defined by regnum.
3.4.7. Face Routines
Faces are 2 dimensional (2D) units of mesh. Each global face ID is returned from cfxExportBound
aryList (see cfxExportBoundaryList (p. 57)) or cfxExportRegionList (see cfxExportRegionList (p. 53)).
Within CFX faces are either represented as Triangles (three vertices) or Quadrilaterals (two vertices).
Each face in a CFX .res file will be parented by a single 3D element. The parent element of a face can
be returned by the cfxELEMNUM macro with the global face ID, and the local face of that element can
be determined by calling cfxFACENUM with the same global face ID
3.4.7.1. cfxExportFaceNodes
int cfxExportFaceNodes (int faceid, int *nodes)
Requests the vertices for the face identified by faceid. The argument faceid should be constructed
from the element number and local face number using the following formula:
(element_number << 3) & local_face_number
Values returned from cfxExportRegionGet and cfxExportRegionList can be supplied directly
to this function.
The number of vertices defining the face are returned if faceid is valid, otherwise 0 is returned. The
node numbers are returned in the array nodes, which should be dimensioned to a minimum size of 4
in the calling routine.
The face numbers and associated node indices are tabulated here:
54
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Details of the Mesh Export API
Element Type
Face
Nodes
tetrahedron
1
0
1
2
2
0
3
1
3
1
3
2
4
0
2
3
1
0
3
4
2
1
4
2
3
0
4
1
4
2
4
3
5
0
1
2
3
1
0
2
5
3
2
0
3
4
1
3
1
4
5
2
4
0
1
2
5
3
5
4
1
0
2
6
4
2
1
5
7
3
3
0
4
5
1
4
2
3
7
6
5
0
1
3
2
6
4
6
7
5
pyramid
prism
hexahedron
Note
The face numbers and associated node indices are different when importing elements. For
details, see cfxImportGetFace (p. 18).
3.4.8. Volume Routines
Volumes are groups of elements in a CFX results file. Accessing volumes within the current zone (see
cfxExportZoneSet (p. 49)) is performed by making calls to the following functions. It should be noted
that the volume definitions for a zone are not loaded into the Export API until either cfxEx
portVolumeList (see cfxExportVolumeList (p. 56)) or cfxExportVolumeGet (see cfxExportVolumeGet (p. 56)) are called. This reduces memory overheads in the API by not allocating space until required.
When access to volume information in the current zone is no longer required a call to cfxEx
portVolumeFree (see cfxExportVolumeFree (p. 56)) should be made to deallocate any internal storage.
3.4.8.1. cfxExportVolumeCount
int cfxExportVolumeCount ()
Query the number of volumes defined in the current zone.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
55
Mesh and Results Export API
3.4.8.2. cfxExportVolumeSize
int cfxExportVolumeSize (int volnum, int type)
Query the number of nodes (if type is cfxVOL_NODES) or number of elements (if type is cfx
VOL_ELEMS) defining the volume indexed by volnum in the current zone. The return value will be 0
if volnum is out of range or type is invalid.
3.4.8.3. cfxExportVolumeName
char *cfxExportVolumeName (int volnum)
Query the name of the volume in the current zone indexed by volnum. Returns NULL if the volnum
is out of range.
Note
The returned pointer points to internal storage, which will be overwritten by the next call
to cfxExportVolumeName.
3.4.8.4. cfxExportVolumeList
int *cfxExportVolumeList (int volnum, int type)
Query the nodes (type is cfxVOL_NODES) or elements (cfxVOL_ELEMS) that define a volume.
This function returns a pointer to an array of node ids or element ids that define the volume identified
by volnum or NULL if the volume number is out of range or the type is not recognized.
3.4.8.5. cfxExportVolumeGet
int cfxExportVolumeGet (int volnum, int type, int index, int *id)
Query the [index]th element (type is cfxVOL_ELEM) or [index]th node (type is cfxVOL_NODE) that
defines a volume volnum in the current zone.
If volnum is out of range or type is not recognized or index is out of range, 0 is returned.
Otherwise id will contain the id of the appropriate node or element in defining the volume and the
function will return index.
3.4.8.6. cfxExportVolumeFree
void cfxExportVolumeFree (int volnum)
Deallocate any internal data storage associated with the volume defined by volnum.
3.4.9. Boundary Condition Routines
Boundary condition are located on groups of faces in a CFX results file. Accessing boundary condition
locations within the current zone (see cfxExportZoneSet (p. 49)) is performed by making calls to the
following functions. It should be noted that the boundary condition location information is not loaded
into the Export API until either cfxExportBoundaryList (see cfxExportBoundaryList (p. 57)) or
cfxExportBoundaryGet (see cfxExportBoundaryGet (p. 58)) are called. This reduces memory overheads in the API by not allocating space until required. When access to regions in the current zone are
56
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Details of the Mesh Export API
no longer required a call to cfxExportBoundaryFree (see cfxExportBoundaryFree (p. 58)) should
be made to deallocate any internal storage.
3.4.9.1. cfxExportBoundaryCount
int cfxExportBoundaryCount ()
Query the number of boundary conditions defined in the current zone.
The function returns the number of boundary conditions in the current zone.
3.4.9.2. cfxExportBoundaryName
const char *cfxExportBoundaryName (const int bcidx)
Query the name of the boundary condition in the current zone identified by bcidx.
The function returns the name of the boundary condition or NULL if the bcidx supplied is out of
range.
The pointer returned points to static storage, which will be overwritten by the next call to cfxExport
BoundaryName.
Note
The following routines use bcidx, which must lie between 1 and cfxExportBoundary
Count() and use index which must lie between 1 and cfxExportBoundarySize (bcidx,
type).
3.4.9.3. cfxExportBoundaryType
const char *cfxExportBoundaryType (const int bcidx)
Query the type (for example, Inlet, Outlet, and so on) of the boundary condition in the current zone
identified by bcidx.
The function returns the type of the boundary condition or NULL if the bcidx supplied is out of range.
The pointer returned points to static storage, which will be overwritten by the next call to cfxExport
BoundaryType.
3.4.9.4. cfxExportBoundarySize
int cfxExportBoundarySize (const int bcidx, const int type)
Query the number of faces (if type is cfxREG_FACES) or nodes (if type is cfxREG_NODES) defined
in the boundary condition identified by bcidx in the current zone.
The function returns the number of faces or nodes or 0 if either bcidx is out of range or type is invalid.
3.4.9.5. cfxExportBoundaryList
int *cfxExportBoundaryList (const int bcidx, const int type)
Query the faces (if type is cfxREG_FACES) or nodes (if type is cfxREG_NODES) that define a
boundary condition.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
57
Mesh and Results Export API
This function returns a pointer to an array of node ids or face ids that define the location of the
boundary condition identified by bcidx or NULL if bcidx is out of range or the type is not recognized.
If type is specified as cfxREG_FACES, the returned ids will represent faces. The element number and
local element face number may be extracted from each face id returned by using the macros cfxEL
EMNUM and cfxFACENUM respectively. The node numbers for the face may be obtained by calling
cfxExportFaceNodes. For details, see cfxExportFaceNodes (p. 54).
The returned pointer points to static data that should be destroyed using cfxExportBoundaryFree.
Subsequent calls to cfxExportBoundaryList will overwrite the array.
3.4.9.6. cfxExportBoundaryGet
int cfxExportBoundaryGet (const int bcidx, const int type, const int index, int *id)
Query the index'th face (type is cfxREG_FACES) or index'th node (type is cfxREG_NODES) that defines
the boundary condition location indexed by bcidx in the current zone. If bcidx is out of range or
type is not recognized or index is out of range (not between 1 and cfxExportBoundarySize), 0
is returned. Otherwise id will contain the identifier of the appropriate node or face defining the
boundary condition location and the function will return index.If type is specified as cfxREG_FACES,
the returned id will represent the identity of a face. The element number and local element face
number may be extracted from the id by using the macros cfxELEMNUM and cfxFACENUM respectively.
3.4.9.7. cfxExportBoundaryFree
void cfxExportBoundaryFree (const int bcidx)
Deallocate any internal data storage associated with the boundary condition defined by bcidx.
3.4.10. Variable Routines
These routines access the variable data defined on the current zone as defined by cfxExportZoneSet.
For details, see cfxExportZoneSet (p. 49). The variable data arrays are not loaded into memory until
either cfxExportVariableList or cfxExportVariableGet are called, and remain in memory
until cfxExportVariableFree is called. For details, see:
• cfxExportVariableList (p. 59)
• cfxExportVariableGet (p. 59)
• cfxExportVariableFree (p. 60).
3.4.10.1. cfxExportVariableCount
int cfxExportVariableCount(int usr_level)
Query the number of variables at interest level usr_level or below. If usr_level is 0, then the
total number of variables is returned.
3.4.10.2. cfxExportVariableSize
int cfxExportVariableSize (int varnum, int *dimension, int *length, int *bdnflag)
Query the dimension, dimension, and length, length, for the variable identified by varnum, which
should be from 1 to the number of variables, returned by cfxExportVariableCount (cfxExportVariableCount (p. 58)). The length, length, will either be 1 or the same as the number of nodes returned
58
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Details of the Mesh Export API
by cfxExportNodeCount (see cfxExportNodeCount (p. 51)). If 1, then the variable has meaningful
values only at the boundary nodes, with a constant value in the interior.
The function also returns bdnflag, which indicates if the variable contains corrected boundary node
values (1) or not (0).
The function returns varnum if successful, or 0 if the variable number is out of range.
3.4.10.3. cfxExportVariableName
char *cfxExportVariableName (int varnum, int alias)
Query the name of the variable identified by varnum.
The return value of the function is NULL if the variable number is out of range or the name of the
variable.
The pointer returned points to static storage, which will be overwritten by the next call to cfxEx
portVariableName.
The argument alias indicates whether the short name (alias=0) or long name (alias=1) should
be returned. For example, the short and long names for the total temperature variable are TEMPTOT
and Total Temperature, respectively.
3.4.10.4. cfxExportVariableList
float *cfxExportVariableList (int varnum, int correct)
Query the results data for a variable identified by varnum.
Returns NULL if the variable number is out of range or the variable data if successful.
The flag correct indicates whether to correct boundary node data (correct=1) or not (correct=0), assuming that it exists.
The data is in the same order as the nodes returned from cfxExportNodeList (see cfxExportNodeList (p. 51)).
For multidimensional variables, the data is stored with dimension consecutive values for each node.
The storage for the data is created by the Export API when this function is called. When the data is no
longer required a call to cfxExportVariableFree (see cfxExportVariableFree (p. 60)) should be
made by the calling function.
3.4.10.5. cfxExportVariableGet
int cfxExportVariableGet (int varnum, int correct, int index, float *value)
Request the values of the variable identified by varnum at the location given by index, which should
be from 1 to the length of the variable, inclusively.
The flag correct indicates whether to correct boundary node data (correct=1) or not (correct=0),
assuming that it exists.
The function returns index, or 0 if the location is out of range.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
59
Mesh and Results Export API
3.4.10.6. cfxExportVariableFree
void cfxExportVariableFree (int varnum)
Deallocates the internal data storage for the variable identified by varnum for the current zone.
60
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 4: Remeshing Guide
Periodic remeshing is an important part of running analyses that involve significant mesh deformation.
Remeshing is often required simply to maintain acceptable mesh quality, as described in Discretization
Errors in the CFX-Solver Theory Guide and Measures of Mesh Quality in the CFX-Solver Modeling Guide.
A schematic illustrating the integration of remeshing into the general simulation workflow is shown in
the figure below.
Figure 4.1: Integration of a Remeshing Loop into the General Simulation Workflow
As shown in Figure 4.1: Integration of a Remeshing Loop into the General Simulation Workflow (p. 61),
in addition to the Preprocessing and Solution steps of the standard simulation workflow, the
remeshing loop includes three additional steps:
• Data Extraction
• Geometry Modification
• Mesh Recreation.
In the context of remeshing, those steps are responsible for completing the following sub-steps;
• Data Extraction: Extract any data needed to guide geometry modifications and mesh re-creation from
the most recent analysis results and monitor point values.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
61
Remeshing Guide
• Geometry Re-Creation: Update the analysis’ geometry so that it conforms to that of the most recent
analysis results (that is, account for mesh deformation).
• Mesh Re-Creation: Generate new mesh(es) that correspond to the updated geometry.
• Preprocessing: Insert the new mesh(es) into the analysis definition, and generate an updated CFXSolver Input File.
• Solution: Interpolate the previously generated analysis results onto the new mesh, re-partition the
mesh if a parallel run mode is selected, and continue the solution process.
As described in Remeshing Tab in the CFX-Pre User's Guide, there are two options available for remeshing:
User Defined and ICEM CFD Replay. As outlined in the discussions that follow, the Preprocessing and
Solution steps (and their respective sub-steps) are automatically executed for both remeshing options.
Although the remaining steps are automatically executed for the ICEM CFD Replay remeshing option,
they become the responsibility of a user defined external command for the User Defined remeshing
option.
4.1. User Defined Remeshing
User Defined remeshing offers the greatest flexibility to customize the remeshing process. This comes
at the expense of requiring that the data extraction, and geometry and mesh re-creation steps are executed by a user-specified external command, as illustrated in the figure below where the dashed line
identifies steps that must be executed by the user-specified External Command.
Figure 4.2: Schematic for User Defined remeshing
This remeshing option is ideally suited for users who have previously completed an ‘in-house’ remeshing
solution involving scripts or varying degrees of manual user-intervention. When this option is used, the
following steps are automatically executed:
62
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
User Defined Remeshing
• Run the specified external command to generate a new mesh(es)
• Insert the new mesh(es) into the analysis definition, and generate an updated CFX-Solver Input file
• Interpolate the previously generated analysis results onto the new mesh, re-partition the mesh if a
parallel run mode is selected, and continue the solution process.
The following examples outline the use of the User Defined remeshing option:
• Remeshing with Key-Frame Meshes (p. 63)
• Remeshing with Automatic Geometry Extraction (p. 63).
4.1.1. Remeshing with Key-Frame Meshes
In some analyses involving mesh deformation, the motion of various boundaries and sub-domains is
known beforehand. Thus, the iteration or time step number at which unacceptable mesh quality will
occur due to mesh motion is also known. A sequence of ‘key-frame’ meshes (of any mesh file type)
corresponding to these instances of poor mesh quality can consequently be generated and applied
during the analysis.
Once the sequence of key-frame meshes has been generated, they should be placed in a location that
will be accessible during the analysis’ execution. The analysis definition is then modified to include one
or more control conditions that will interrupt the solver at the iteration or time step at which a keyframe mesh should be inserted. A configuration is subsequently defined (unless this has already been
done), and a remeshing definition is created with the following settings:
• Set Option to User Defined.
• Set the Activation Condition(s) to the previously created interrupt control condition(s).
• Set the Location to the mesh region that will be replaced.
• Set the External Command to the command that will be used to generate the replacement mesh file.
• Set the Replacement File to the name of the file that will be generated by the external command.
The External Command is typically a shell script or batch file that completes the following tasks:
• Determine which key-frame mesh to use. This will require parsing the run’s output file for the iteration
or time step number, or the actual simulation time. Output generated from the cfx5mondata executable can also be parsed instead of the run’s output file. For details, see Exporting Monitor Data from
the Command Line in the CFX-Solver Manager User's Guide.
• Copy the key-frame mesh to the path the specified by the Replacement File setting.
4.1.2. Remeshing with Automatic Geometry Extraction
In some analyses involving mesh deformation, the motion of various boundaries and sub-domains is
not known beforehand and the key-frame remeshing strategy presented above is not applicable. In
these analyses, geometrical information must be extracted from the most recent analysis results and
applied in the remeshing process.
In such cases, the analysis definition is modified to include one or more control conditions that will interrupt the solver when, for example, mesh quality deteriorates significantly. A configuration is subRelease 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
63
Remeshing Guide
sequently defined (unless this has already been done), and a remeshing definition is created with the
following settings:
• Set Option to User Defined.
• Set the Activation Condition(s) to the previously created interrupt control condition(s).
• Set the Location to the mesh region that will be replaced.
• Set the External Command to the command that will be used to generate the replacement mesh file.
• Set the Replacement File to the name of the file that will be generated by the external command.
The External Command is typically a shell script or batch file that completes the following tasks:
• Extract geometry data from the most recent solution of the analysis, and either update or replace the
original geometry. This may be done using mesh-to-geometry conversion tools available in software
such as ANSYS ICEM CFD, or by extracting monitor point data values (for example, the Total Centroid
Displacement variable) using the cfx5mondata executable. For details, see Exporting Monitor Data
from the Command Line in the CFX-Solver Manager User's Guide.
• Create a replacement mesh file using the updated or newly generated geometry. This may be done in
any suitable mesh generation application.
Note that some mesh-to-geometry conversion tools are unable to extract the latest mesh coordinates
from the most recent CFX-Solver Results file. If this is the case, then introduce a call to CFX-Pre (within
the External Command) that executes a session file that simply loads the latest CFX-Solver Results file
and writes a new CFX-Solver Input file. That CFX-Solver Input file will contain the required, latest mesh
coordinates.
4.2. ICEM CFD Replay Remeshing
ICEM CFD Replay remeshing provides a highly automated remeshing process that is ideally suited for
users of the ANSYS ICEM CFD mesh generation software and cases that involve translational mesh
motion only (that is, no rotation or general deformation). When this option is used, a master replay file
is assembled from other task-oriented replay files and submitted to the ANSYS ICEM CFD mesh generator for batch execution. These replay files are illustrated in the figure below, along with the general
process flow for this remeshing option. The dashed line in the figure highlights components of the
master replay file and identifies files and steps that you can modify. Unless otherwise noted, files are
contained in the <CFXROOT>/etc/Remeshing directory.
64
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
ICEM CFD Replay Remeshing
Figure 4.3: Schematic for ICEM CFD Replay remeshing
When this option is used, the following steps are automatically executed:
• Extract geometry and mesh control data and write them to the cfx_params.rpl replay file in the
run directory. The data includes:
– Centroid displacements for boundaries that are included in ANSYS ICEM CFD Part Maps
– Mesh control parameters (for example, ehgt and emax)
– Scalar parameters.
• Run (in batch) the ANSYS ICEM CFD mesh generation program using the master replay file. This master
replay file executes the following tasks:
– Read the cfx_params.rpl file.
– Load the reference geometry from the Geometry File identified in the Remesh definition.
– Apply displacements (including scaling and any offsets) corresponding to all ANSYS ICEM CFD Part
Map definitions contained in the Remesh definition. This is done using the default geometry replay
file provided, or using the user defined replay file if specified in the ICEM CFD Geometry Control
setting.
– Apply ICEM CFD Mesh Controls defined in the Remesh definition. This is done using the provided
controls, or using the user-defined replay file if specified in the ICEM CFD Mesh Control setting.
– Load your Mesh Replay File, specified in the Remesh definition.
– Export a new mesh for ANSYS CFX.
• Insert the new mesh(es) into the analysis definition, and generate an updated CFX-Solver Input file.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
65
Remeshing Guide
• Interpolate the previously generated analysis results onto the new mesh, re-partition the mesh if a
parallel run mode is selected, and continue the solution process.
You must create the reference Geometry File and the Mesh Replay File because these are specific to
each case. However, the generic default replay files (icemcfd_Remesh.rpl, icemcfd_GeomMod.rpl,
and icemcfd_MeshMod.rpl) used by this option are provided in the <CFXROOT>/etc/Remeshing
directory. These files may be edited to provide installation-wide changes to the ICEM CFD Replay
remeshing behavior. Alternatively, the geometry and mesh modification files may be copied and edited
to provide case-specific changes.
Note
As indicated previously, only translational mesh motion is automatically handled by the ICEM
CFD Replay remeshing option. This is accomplished by applying the displacements of centroids
of boundaries in the ANSYS CFX analysis definition to parts in the ANSYS ICEM CFD geometry.
All other mesh motion (such as rotation about the centroid or another point, or general deformation) will not be applied, and an inconsistency in the analysis geometry before and
after remeshing will be introduced.
4.2.1. Steps to Set Up a Simulation Using ICEM CFD Replay Remeshing
The following discussion presents the three general steps required to set up a simulation using the
ICEM CFD Replay remeshing option.
The first step involves creating the reference Geometry File within the ANSYS ICEM CFD environment.
If the geometry was not created within that environment, use one of the File > Import Geometry options
in the ANSYS ICEM CFD environment. At this point, ensure that all required Parts (or Families) are defined
and named so that they can be referenced when completing the ICEM CFD Replay remeshing definition
later in CFX-Pre. Finally, store the geometry in the ICEM CFD native geometry file format (namely, a
.tin file).
The second step involves generating the Mesh Replay File, again, from within the ANSYS ICEM CFD
environment. Start with the previously created geometry loaded, and work sequentially through the
mesh generation process until acceptable mesh controls have been specified. This may require fine
tuning, which will involve the regeneration of your mesh after moving the geometry through its expected
range of motion. Once you are satisfied with the mesh control settings, purge the last mesh using File
> Mesh > Close Mesh, and reload the original reference geometry. Complete the following tasks to
generate the required Mesh Replay File:
1.
Use File > Replay Scripts > Replay Control to begin recording the commands for the Mesh Replay File.
The Replay Control dialog box is displayed.
2.
Revisit all of the mesh related tabs and settings used to generate the mesh, clicking either the Apply or
OK to commit the settings into the Replay Control panel.
3.
Generate the mesh.
4.
In the Replay Control panel, clear the Record (after current) toggle and select Save to write the settings
to replay file.
You may also want to export the mesh that was (re)generated for use in the simulation definition (as
in the next step).
66
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Directory Structure and Files Used During Remeshing
The third step involves defining the simulation within CFX-Pre. Complete the following tasks to prepare
the simulation:
1.
Start a new simulation and import the (previously generated) mesh.
2.
Define expressions for the motion of the geometry (for example, see the expressions for the ball movement
in Modeling a Ball Check Valve using Mesh Deformation and the CFX Rigid Body Solver in the CFX Tutorials).
Note
See also the discussion in Mesh Re-Initialization During Remeshing (p. 68).
3.
Define the flow analysis including the definition of one or more solver interrupt controls, as described in
Interrupt Control in the CFX-Pre User's Guide, to identify the condition(s) under which solver execution
will be interrupted.
4.
Define a configuration and complete the ICEM CFD Replay remeshing setup as described in ANSYS ICEM
CFD Replay Remeshing in the CFX-Pre User's Guide. The Geometry File and Mesh Replay File created
above are referenced here. Note also, that references to one or more of the previously defined solver interrupt control conditions are required to activate remeshing.
5.
Complete any execution controls for the simulation and either start the solver or write the CFX-Solver
Input file for later use.
4.3. Directory Structure and Files Used During Remeshing
CFX-Solver runs that include remeshing will have a slightly non-standard directory structure during execution. For example, using a CFX-Solver input file named case.def, a directory structure similar to
the following will exist just after solution execution is interrupted and the second instance of remeshing
begins:
case.def
case_001/
1_full.trn
0_full.trn
2_full.trn
3_oldmesh.res
3_remesh.out
case_001.dir/
3_full.trn
4_full.trn res mon
The first instance of remeshing occurred when the solver was interrupted after the third time step.
Following this instance of remeshing, all CFX-Solver Results files (such as transient, backup, and
remeshing) contained in the run directory, case_001.dir, were moved into the final solution directory,
case_001. The results file written when the solver was interrupted before remeshing was renamed to
3_oldmesh.res. Any text output to the console window during remeshing was redirected to the file
named 3_remesh.out, which is also placed in the final solution directory.
The second, and currently running, instance of remeshing began when the solver was interrupted after
the fifth time step. The results file written by the solver still has the generic name, res, and monitor
data (contained in the mon file) has not yet been inserted into the results file.
Just after inserting the new mesh(es) into the analysis definition, the files contained in the final solution
and run directories change slightly. The results and console output files are renamed (to
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
67
Remeshing Guide
5_oldmesh.res and 5_remesh.out, respectively) and moved from the run directory into the final
solution directory. An automatically generated session file, meshUpdate.pre, is used by CFX-Pre to
generate the updated the solver input file, 5_newmesh.def, and each of these files are present in the
run directory. These files are, however, replaced or removed during the next instance of remeshing or
when the analysis ends and the run directory is deleted.
4.4. Additional Considerations
This section discusses additional considerations for remeshing.
4.4.1. Mesh Re-Initialization During Remeshing
4.4.2. Software License Handling
4.4.3. Results File Option
4.4.1. Mesh Re-Initialization During Remeshing
The following points are important to note during remeshing:
• The total mesh displacement variable is relative to a specific mesh topology. Because the mesh topology
changes, this variable is reset each time remeshing occurs.
• The new variable called total centroid displacement tracks the displacement of each
boundary’s centroid since the beginning of the analysis (that is, relative to the original mesh).
• The specified displacement based mesh motion is relative to the initial mesh and must therefore include
an offset to account for mesh re-initialization. The Mesh Initialisation Time variable corresponds
to the time at which mesh re-initialization last occurred. This can be used to evaluate the required offset
for time varying mesh displacement.
Note
Total Centroid Displacement is the sum of total mesh displacement and an offset
vector. The value of the offset is determined by the displacement of the boundary’s centroid
from its original position to its initial position. When using Total Centroid Displace
ment in a non-remeshing case, the original and the initial position are the same, resulting
in an offset value of zero. In this case, there seems to be no difference between the variables,
Total Centroid Displacement and Total Mesh Displacement. However, when
using Total Centroid Displacement in a remeshing case, the original position is
defined at the start of the simulation, while the initial position is defined after the last remesh;
this results in an offset contribution that is non-zero.
An example of the expressions used to evaluate an applied displacement that includes the required
offset to account for mesh re-initialization is given below. In this example, the applied displacement is
evaluated as the desired displacement minus the value of the desired displacement at the Mesh
Initialisation Time.
Disp Desired = 1[m]*0.5*(1-cos(2.[s^-1]*pi*t))
Disp Mesh ReInit = 1[m]*0.5*(1-cos(2.[s^-1]*pi*Mesh Initialisation Time ))
Disp Applied = Disp Desired - Disp Mesh ReInit
4.4.2. Software License Handling
Several software components (for example, CFX-Pre, the CFX-Solver, ANSYS ICEM CFD, and so on) are
used while executing steps in the overall remeshing process. Rather than holding all of these licenses
68
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Additional Considerations
for the entire duration of the analysis, they are only ‘checked out’ as required. Although this frees up
the licenses for other users when remeshing is not executing, it also introduces the possibility that required licenses are not available when they are needed for remeshing.
This model for software license handling may cause problems in multi-user environments, but work is
underway to provide a broader range of handling options for future releases.
4.4.3. Results File Option
In order for remeshing to proceed, results files must be of type Standard, Essential, or Refiner.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
69
70
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 5: Reference Guide for Mesh Deformation and
Fluid-Structure Interaction
This guide is part of a series that provides advice for using CFX in specific engineering application areas.
It is aimed at users with little or moderate experience using CFX for applications involving Mesh Deformation and/or Fluid Structure Interaction.
This guide describes:
5.1. Mesh Deformation
5.2. Fluid Structure Interaction
5.1. Mesh Deformation
Mesh deformation is an important part of executing simulations with changing domain geometry. In
CFX, this capability is available in fluid and solid domains. Motion can be specified on selected regions
via CEL or an external solver coupling (for example, ANSYS Multi-field MFX), or on all nodes in an entire
domain via a user-Fortran junction box routine.
5.1.1. Mesh Folding: Negative Sector and Element Volumes
It is not uncommon for the mesh to become folded (or tangled) during the mesh deformation process.
When this occurs, a message indicating the existence and location of either negative sector volumes
or negative (that is, topologically invalid) elements is written to the simulation output file. Notification
of negative sector volumes highlights the existence of non-convex mesh elements that still have a
positive volume. Although the existence of negative sector volumes is not a fatal condition, it does indicate that:
• Mesh elements are only barely positive
• Further mesh deformation is likely to yield elements with negative volumes, which is a fatal condition
Some of the most common causes for mesh folding during deformation are identified in the following
sections.
5.1.2. Applying Large Displacements Gradually
In many simulations that require mesh deformation, the motion is known a priori. In these cases, the
motion can be applied gradually, by relating it to the iteration or timestep counters, to reduce the
likelihood of mesh folding. Mesh folding is often avoided with this strategy because the mesh displacement equations are assembled using the updated meshes from each deformation step (that is, outer
iteration or timestep). In general, the desired total mesh deformation should be split up so that regions
where motion is specified move through less than approximately 5 adjacent elements per step.
In some simulations, the motion is not known a priori. Fluid Structure Interaction is an excellent example
of this. In these cases, mechanisms available for under-relaxing the displacements applied per deformation step should be used. For details, see Solver Controls, External Coupling Tab in the CFX-Solver
Modeling Guide.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
71
Reference Guide for Mesh Deformation and Fluid-Structure Interaction
5.1.3. Consistency of Mesh Motion Specifications
Mesh motion options such as Specified Displacement may be applied on multiple boundary
and subdomain regions. Because the specified motion is applied directly to mesh nodes, rather than
control volume integration points, care is required to ensure that motion specified on adjacent regions
is self-consistent. For example, the motion specified on one moving wall should be reduced to zero for
any nodes that are shared with another stationary wall. If this is not done, then the motion applied to
the shared nodes will be either the moving or stationary condition, depending on which was applied
last during the equation assembly process.
Folded meshes often result from the application of inconsistent motion specifications.
5.1.4. Solving the Mesh Displacement Equations and Updating Mesh Coordinates
During each outer iteration or timestep, the mesh displacement equations are solved to the specified
convergence level and the resulting displacements are applied to update the mesh coordinates. This
occurs before proceeding to solve the general transport (for example, hydrodynamics, turbulence, and
so on) equations.
Unlike other equation classes, the convergence level (that is, controls and criteria) applied to mesh
displacement equations is unaffected by changes made to the basic settings for all other equations.
The default convergence controls and criteria for the mesh displacement equation are tabulated below,
and are changed by visiting the Mesh Displacement entry in the Equation Class Settings tab under
Solver Control.
Setting
Value
Maximum Number of Coefficient
Loops
5
Minimum Number of Coefficient
Loops
1
Residual Type
RMS
Residual Target
1.0E-4
Mesh folding occurs and is detected when the displacements are used to update the mesh coordinates.
Folded meshes can occur if the displacement equations are incompletely solved. In this case, the unconverged displacement solution field does not vary smoothly enough to ensure that adjacent mesh nodes
move by similar amounts.
5.1.5. Mesh Displacement Diffusion Scheme
A number of numerical schemes are available for the solution of the mesh displacement diffusion
equation. In many cases the default scheme is appropriate, but in some situations mesh folding can be
avoided and improved mesh quality can be obtained by using a different scheme. The expert parameter
meshdisp diffusion scheme controls which numerical scheme is used. For details, see Discretization Parameters. Setting meshdisp diffusion scheme to 3 can be helpful if the mesh folds unexpectedly at sharp corners or if uniform mesh deformation is expected but non-uniform deformation
is observed. The figures below show an example of using different mesh displacement diffusion schemes.
72
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Mesh Deformation
Figure 5.1: Original Undeformed Mesh
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
73
Reference Guide for Mesh Deformation and Fluid-Structure Interaction
Figure 5.2: Deformed Mesh with the Default Diffusion Scheme
74
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Mesh Deformation
Figure 5.3: Deformed Mesh with "meshdisp diffusion scheme = 3"
5.1.6. Mesh Displacement vs. Total Mesh Displacement
A number of new variables become available when executing simulations with mesh deformation. Two
of these variables are Mesh Displacement and Total Mesh Displacement.
Mesh Displacement is the principal variable that is solved for by the mesh motion model (see Mesh
Deformation in the CFX-Solver Modeling Guide). This variable represents the displacement relative to the
previous mesh locations. Conversely, Total Mesh Displacement is a derived quantity that represents
the displacement relative to the initial mesh.
5.1.7. Simulation Restart Behavior
The following table summarizes the behavior that occurs when simulations with (or without) mesh deformation are restarted with (or without) mesh deformation. With only the exception noted, the simulation type (that is, steady-state or transient) used for the initial or restart run does not affect behavior.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
75
Reference Guide for Mesh Deformation and Fluid-Structure Interaction
Initial Simulation
Restart Simulation
Restart Behavior
No Deformation
Deformation
Mesh from initial run
serves as initial mesh
for restart run
Deformation
No Deformation
Final mesh from initial
run serves as mesh for
restart run
Deformation
Deformation
Initial mesh from initial
run serves as initial
mesh for restart runa
a
If the restart is a transient run with the initial time set to Value, then the final mesh from the initial run will serve as the initial mesh
for the restart simulation.
5.2. Fluid Structure Interaction
CFX provides the ability to solve, or take part in the solution of cases that involve the coupling of
solution fields in fluid and solid domains. This coupling is commonly referred to as Fluid Structure Interaction (FSI). One example of FSI is the simulation of an internal combustion engine, which involves the
solution of fluid flow, conjugate heat transfer and combustion problems on deforming meshes.
In the discussion that follows, examples are presented to demonstrate the FSI capabilities using CFX
by itself or with other CAE packages like ANSYS Mechanical and ANSYS Multiphysics. These examples
are grouped according to the degree of coupling that must be maintained during the simulation in
order to ensure that accurate results are obtained.
5.2.1. Unidirectional (One-Way) FSI
In many FSI simulations, the coupling between the solution fields is predominantly unidirectional; a
given field may strongly affect, but not be affected by other fields. In CFX, there are a variety of strategies
to efficiently execute such simulations. These strategies are identified in the following examples.
5.2.1.1. Using CFX Only
One of the most useful examples of unidirectional FSI within CFX involves prescribed mesh deformation
of fluid or solid domains. This is possible using the CEL to specify the motion of sub-domains or domain
boundaries, or by reading a sequence of pre-defined meshes.
5.2.1.2. Using CFX and the Mechanical Application
In many FSI simulations, the capabilities of additional solvers are required to compliment those of CFX.
In these circumstances, CFX provides tools to facilitate the import and export of solution data in a
variety of formats.
5.2.1.2.1. Importing Data from the Mechanical Application Solver
The recommended method for importing boundary condition data from the Mechanical application
into CFX is via boundary profile data. For information about the creation and use of profile data files,
refer to Unidirectional Load Transfer in the Mechanical APDL Coupled-Field Analysis Guide and Use Profile
Data in the CFX-Pre User's Guide.
76
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Fluid Structure Interaction
5.2.1.2.2. Export Data to Other ANSYS Software Products
Two methods exist for exporting data from CFX for use in other ANSYS software products. The first
method requires the use of the MFS variant of the ANSYS Multi-field solver and the second method
does not.
• For information about exporting mechanical and thermal surface data and thermal volumetric data for use
with the MFS solver, refer to Export to ANSYS Multi-field Solver Dialog Box in the CFX-Solver Manager User's
Guide. For information about using the exported results and the MFS Solver, refer to The ANSYS Multi-field
(TM) Solver - MFS Single-Code Coupling in the Mechanical APDL Coupled-Field Analysis Guide.
• For information about exporting mechanical and thermal surface data for general use, refer to Mechanical
Import/Export Commands in the CFD-Post User's Guide. This method involves reading a Mechanical Coded
Database (CDB) file and interpolating CFX solution data onto the mesh contained in that file. For more information about how these steps are automated in the Mechanical application, see Custom Systems in the
Workbench User's Guide.
5.2.1.2.3. Mechanical Import/Export Example: One-Way FSI Data Transfer
You can perform one-way FSI operations manually (by exporting CDB files from the Mechanical APDL
application, importing the surface in CFD-Post, and exporting the SFE commands).
To create a Mechanical load file using CFD-Post to transfer FSI data:
1.
Load the fluids results file, from which you want to transfer results, into CFD-Post
2.
Select File > Import > Import Mechanical CDB Surface. The Import Mechanical CDB Surface dialog
box appears.
3.
In the Import Mechanical CDB Surface dialog box, either:
• Select the CDB file that specifies the surface mesh of the solid object to which to transfer data. Also
select the Associated Boundary for the surface to map onto, and make other selections as appropriate.
• Select the XML document that provides all transfer information. Click OK, and the surface data is loaded.
4.
Select File > Export > Export Mechanical Load File. The Export Mechanical Load File dialog box appears.
5.
In the Export Mechanical Load File dialog box, select a filename to which to save the data. For the Location parameter value, select the imported ANSYS mesh object. Under File Format select ANSYS Load
Commands (FSE or D). (Alternatively, you can select WB Simulation Input (XML) to get XML output.)
Also select the appropriate data to export: Normal Stress Vector, Tangential Stress Vector, Stress Vector,
Heat Transfer Coefficient, Heat Flux, or Temperature. Click Save, and the data file is created.
The one-way FSI data transfer described above is performed automatically when using the FSI: Fluid
Flow (CFX) > Static Structural custom system in ANSYS Workbench. For details, see the FSI: Fluid Flow
(ANSYS CFX) > Static Structural in the Workbench User's Guide section in the ANSYS documentation.
5.2.1.3. Using CFX and Other CAE Software
Solution data can be exported from CFX in a variety of general formats during or after execution of the
CFX-Solver. For information about the export of data in CGNS format during the execution of the solver,
refer to Export Results Tab in the CFX-Pre User's Guide. For information about the extraction and export
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
77
Reference Guide for Mesh Deformation and Fluid-Structure Interaction
of CGNS, MSC Patran, FIELDVIEW, EnSight and custom data from CFX results files, refer to Generic Export
Options in the CFX-Solver Manager User's Guide.
5.2.2. Bidirectional (Two-Way) FSI
In some simulations, there is a strong and potentially nonlinear relationship between the fields that are
coupled in the Fluid Structure Interaction. Under these conditions, the ability to reach a converged
solution will likely require the use of bidirectional FSI. As for unidirectional interaction, examples are
provided below that demonstrate the variety of strategies to execute such simulations.
5.2.2.1. Using CFX Only
Conjugate heat transfer is an example of bidirectional interaction that can be solved using the CFXSolver only.
5.2.2.2. Using CFX and the Mechanical Application
Communicating data between CFX and the Mechanical application is automated by the MFX branch of
the ANSYS Multi-field solver. In this branch of the ANSYS Multi-field solver, data is communicated
between the CFX and the Mechanical application field solvers through standard internet sockets using
a custom client-server communication protocol. This custom solution maximizes execution efficiency
and robustness, and greatly facilitates future extensibility.
Setup requires creation of the fluid and solid domain/physical models in the CFX-Pre and the Mechanical application user interfaces, respectively, and the specification of coupling data transfers and controls
in the CFX-Pre user interface. Execution and run-time monitoring of the coupled simulation is performed
from the CFX-Solver Manager. Note that a dedicated MFX-ANSYS/CFX tab is also provided in the ANSYS
Product Launcher to begin execution of the coupled simulation (see General Procedure in the CFXSolver Manager User's Guide).
Refer to the following sections for more information:
• Coupling CFX to an External Solver: ANSYS Multi-field Simulations in the CFX-Solver Modeling Guide
• Multi-field Analysis Using Code Coupling in the Mechanical APDL Coupled-Field Analysis Guide.
Coupled simulations begin with the execution of the Mechanical application and CFX field solvers. The
Mechanical application solver acts as a coupling master process to which the CFX-Solver connects. Once
that connection is established, the solvers advance through a sequence of six pre-defined synchronization
points (SPs), as illustrated in Figure 5.4: Sequence of Synchronization Points (p. 79). At each of these
SPs, each field solver gathers the data it requires from the other solver in order to advance to the next
point.
The first three SPs are used to prepare the solvers for the calculation intensive solution process, which
takes place during the final three SPs. These final SPs define a sequence of coupling steps, each of
which consists of one or more stagger/coupling iterations. During every stagger iteration, each field
solver gathers the data it requires from the other solver, and solves its field equations for the current
coupling step. Stagger iterations are repeated until a maximum number of stagger iterations is reached
or until the data transferred between solvers and all field equations have converged. The latter guarantees
an implicit solution of all fields for each coupling step.
78
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Fluid Structure Interaction
Figure 5.4: Sequence of Synchronization Points
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
79
Reference Guide for Mesh Deformation and Fluid-Structure Interaction
5.2.2.3. Using CFX and Other CAE Software
Third-party code-coupling software or proprietary interfaces provided by the CAE software vendors can
also be used in conjunction with CFX. Contact those software providers and your CFX service representative for more information.
80
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 6: CFX Best Practices Guide for Numerical Accuracy
This guide provides best practice guidelines for Computational Fluid Dynamics (CFD) simulation and
documentation of the verification, validation, and demonstration test cases. It describes:
• An Approach to Error Identification, Estimation and Validation (p. 81)
• Definition of Errors in CFD Simulations (p. 82)
• General Best Practice Guidelines (p. 91)
• Selection and Evaluation of Experimental Data (p. 101)
This guide is aimed at users who have moderate or little experience using ANSYS CFX. It is part of a
series that provides advice for using ANSYS CFX in specific engineering application areas. The current
guidelines are adapted from Best Practice Guidelines developed for the nuclear reactor safety applications
[143 (p. 348)].
6.1. An Approach to Error Identification, Estimation and Validation
An evaluation of CFD capabilities has to ensure that the different types of errors are identified and, as
far as possible, treated separately. It is known from single-phase studies that the quantification and
documentation of modeling errors (as in turbulence models, for example) can be achieved only if the
other major sources of errors are reduced below an “acceptable” level. In an ideal world, this would
mean, among other demands, that solutions are provided for grids and with timesteps that are fine
enough so that numerical errors can be neglected. This is not a trivial task and the separation of errors
cannot always be achieved. These difficulties will be greatly increased by the inclusion of multi-phase
physics and unsteady effects. Nevertheless, the worst strategy would be to avoid the subject and to
provide solutions on a single grid, with a single timestep, and with other uncertainties in initial conditions
and boundary conditions not evaluated. This would result in solutions that would be of little use for
the validation goals.
An essential quantity in the quality assurance procedure is the definition of target variables. They will
mainly be scalar (integral) quantities (for instance, forces, heat transfer rates, and maximum temperature)
or one-dimensional distributions, such as the wall heat transfer along a certain line. Convergence
studies can be based on these variables without a reference to the grid used in the simulation. They
can also be used for an asymptotic evaluation of convergence on unstructured meshes. Even more
important, these quantities are of immediate meaning to engineers and enable them to understand
the uncertainty from a physical standpoint. A danger of integral or local scalar quantities is that they
might not be sensitive enough to detect local changes in the solutions under grid refinement. This
should be kept in mind during the analysis.
In order to tackle the problem, it is necessary to first define the different type of errors that can impact
a CFD simulation. It is then required that you list the most promising strategies in order to reduce or
avoid these errors. Based on these strategies, procedures have to be defined that can be used for the
test case simulations.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
81
CFX Best Practices Guide for Numerical Accuracy
It might be not possible to rigorously perform the error estimation and reduction procedures described
in the following sections for the complex demonstration cases. However, the best attempt should be
made to follow the principal ideas and to avoid single grid solutions without sensitivity studies. For
these cases, it is even more important to follow a stringent documentation procedure and to list the
possible deficiencies and uncertainties in the simulations.
The strategies for the reduction and evaluation of numerical errors have been developed for singlephase flows. There is no principal difference between the single- and multi-phase flow formulations.
They are both based on (ensemble) averaged equations, and are mathematically similar. From a physical
standpoint, there are however significant additional challenges due to the presence of the different
phases, besides the obviously higher demands on model formulation. One of the additional complication
lies in the presence of sharp interfaces between the phases, which require a higher degree of grid resolution than usually necessary for single-phase flows. In addition, multi-phase flows have a higher affinity
to physical instabilities that might be suppressed on coarse grids, but appear under grid refinement.
(This effect is sometimes also observed in single-phase flows. An example is the blunt trailing edge of
an airfoil, where extreme grid refinement will eventually capture the vortex shedding of the mixing
layer). It is to be kept in mind that the brute application of procedures might not lead to the desired
results. Also in these cases, the spirit behind the guidelines should be followed and carried as far as
possible.
Validation studies have to be based on experimental data. These data can introduce significant errors
into the comparison. It is therefore required to select the project test cases with attention to potential
error sources and experimental uncertainties. Definitions on the different types of test cases as well as
on the requirements for the project are given in Selection and Evaluation of Experimental Data (p. 101).
6.2. Definition of Errors in CFD Simulations
CFD simulations have the following potential sources for errors or uncertainties:
• Numerical Errors (p. 83)
Numerical errors result from the differences between the exact equations and the discretized equations
solved by the CFD code. For consistent discretization schemes, these errors can be reduced by an
increased spatial grid density and/or by smaller timesteps.
• Modeling Errors (p. 88)
Modeling errors result from the necessity to describe flow phenomena such as turbulence, combustion,
and multi-phase flows by empirical models. For turbulent flows, the necessity for using empirical
models derives from the excessive computational effort to solve the exact equations1 with a Direct
Numerical Simulation (DNS) approach. Turbulence models are therefore required to bridge the gap
between the real flow and the statistically averaged equations. Other examples are combustion
models and models for interpenetrating continua, for example, two-fluid models for two-phase flows.
• User Errors (p. 89)
User errors result from incorrect use of CFD software and are usually a result of insufficient expertise
by the CFD user. Errors can be reduced or avoided by additional training and experience in combination with high-quality project management and by provision and use of Best Practice Guidelines
and associated checklists.
• Application Uncertainties (p. 90)
1
The Navier-Stokes equations for single-phase, Newtonian fluids
82
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Definition of Errors in CFD Simulations
Application uncertainties are related to insufficient information to define a CFD simulation. A typical
example is insufficient information on the boundary conditions.
• Software Errors (p. 90).
Software errors are the result of an inconsistency between the documented equations and the actual
implementation in the CFD software. They are usually a result of programming errors.
A more detailed definition of the different errors follows.
6.2.1. Numerical Errors
Numerical Errors are of the following types:
• Solution Errors (p. 83)
• Spatial Discretization Errors (p. 84)
• Time Discretization Errors (p. 84)
• Iteration Errors (p. 85)
• Round-off Error (p. 86)
• Solution Error Estimation (p. 86)
6.2.1.1. Solution Errors
The most relevant errors from a practical standpoint are solution errors2. They are the difference between
the exact solution of the model equations and the numerical solution. The relative solution error can
be formally defined as:
(6.1)
Equation 6.1 (p. 83) is valid for every grid point for which the numerical solution exists. A global number
can be defined by applying suitable norms, as:
(6.2)
The goal of a numerical simulation is to reduce this error below an acceptable limit.
Obviously, this is not a straightforward task, as the exact solution is not known and the error can
therefore not be computed. Exceptions are simple test cases for code verification where an analytical
solution is available.
Given a grid spacing , and the truncation error order of a consistent discretization scheme, , a Taylor
series can be written to express the exact solution as:
(6.3)
2
Sometimes also called ‘discretization errors’
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
83
CFX Best Practices Guide for Numerical Accuracy
In other words, the numerical solution converges towards the exact solution with the
grid spacing. Analogous definitions are available for time discretization errors.
power of the
6.2.1.2. Spatial Discretization Errors
Spatial discretization errors are the result of replacing the analytical derivatives or integrals in the exact
equations by numerical approximations that have a certain truncation error. The truncation error can
be obtained by inserting a Taylor series expansion of the numerical solution into the different terms of
the discretized equations:
(6.4)
where
is the
derivative of the exact solution at a given location. An example is a central difference
for a spatial derivative:
(6.5)
This formulation has a truncation error of order 2 and is therefore second-order accurate. The overall
truncation error order of the spatial discretization scheme is determined by the lowest order truncation
error after all terms have been discretized.
In the
term of Equation 6.5 (p. 84), the leading term is proportional to
upwind differencing of the convective terms yields truncation errors
. First-order
with leading term propor-
tional to
. This term then contributes to the diffusion term (numerical/false diffusion), which is
most dangerous in 3D problems with grid lines not aligned to the flow direction. These schemes enhance
the dissipation property of the numerical algorithm (see for example, Ferziger and Peric [141 (p. 347)])
and are not desirable in high-quality CFD simulations.
From a practical standpoint, it is important to understand that for a first-order method, the error is reduced to 50% by a doubling of the grid resolution in each spatial direction. For a second-order method,
it is reduced to 25% for the same grid refinement.
6.2.1.3. Time Discretization Errors
Time adds another dimension to a CFD simulation. The definition of time discretization errors is therefore
similar to the definition of the spatial discretization errors. The spatial discretization usually results in a
system of nonlinear algebraic equations of the form:
(6.6)
The error in the time discretization can again be obtained by a Taylor series expansion of the numerical
formulation of this equation. With the example of a backward Euler integration:
(6.7)
84
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Definition of Errors in CFD Simulations
the discretization error is:
(6.8)
The error is therefore first-order for the time derivative.
An additional complication for implicit methods comes from the inclusion of the unknown
in the
right hand side of Equation 6.7 (p. 84). In order to benefit from an implicit method, a linearization of
has to be included:
(6.9)
The resulting discretized equation is therefore:
(6.10)
This constitutes an implicit formulation with first-order accuracy. A second-order time differencing is
not compatible with this linearization of the right hand side, as the linearization introduced a first-order
error in
. In order to be able to satisfy the implicit dependency of the right hand side on the time
level
more closely, inner iterations (or coefficient loops) are frequently introduced:
(6.11)
where an additional iteration over the index
is carried out. This equation can be reformulated as:
(6.12)
This equation can be converged completely (left hand side goes to zero) in in order to solve the
original exact implicit formulation given by Equation 6.7 (p. 84). It is obvious that it is not necessary to
converge the coefficient loop to zero, while the right hand side has a finite (first-order) error in
. It
can be shown that for a first-order time integration, one coefficient loop is consistent with the accuracy
of the method. In a case where a second-order accurate scheme is used in the time derivative, two
coefficient loops will ensure overall second-order accuracy of the method. Note, however, that this is
correct only if the coefficient loops are not under-relaxed in any way.
For explicit methods, no coefficient loops are required and the time discretization error is defined solely
from a Taylor series expansion.
6.2.1.4. Iteration Errors
The iteration error is similar to the coefficient loop error described above. It occurs in a case where a
steady-state solution is sought from an iterative method. In most CFD codes, the iteration is carried out
via a (pseudo-) timestepping scheme as given in this example, which also appears above:
(6.13)
Zero iteration error would mean that the left hand side is converged to zero, leading to the converged
solution
. However, in practical situations, the iterative process is stopped at a certain level, in
order to reduce the numerical effort. The difference between this solution and the fully converged
solution defines the iteration error.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
85
CFX Best Practices Guide for Numerical Accuracy
The iteration error is usually quantified in terms of a residual or a residual norm. This can be the maximum absolute value of the right hand side,
, for all grid points, or a root mean square of this
quantity. In most CFD methods, the residual is nondimensionalized to enable a comparison between
different applications with different scaling. However, the non-dimensionalization is different for different
CFD codes, making general statements as to the required absolute level of residuals impractical. Typically,
the quality of a solution is measured by the overall reduction in the residual, compared to the level at
the start of the simulation.
The iteration error should be controlled with the use of the target variables. The value of the target
variable can be plotted as a function of the convergence level. In case of iterative convergence, the
target variable should remain constant with the convergence level. It is desirable to display the target
variable in the solver monitor during the simulation.
6.2.1.5. Round-off Error
Another numerical error is the round-off error. It results from the fact that a computer only solves the
equations with a finite number of digits (around 8 for single-precision and around 16 for double-precision). Due to the limited number of digits, the computer cannot differentiate between numbers that
are different by an amount below the available accuracy. For flow simulations with large-scale differences
(for instance, extent of the domain vs. cell size), this can be a problem for single-precision simulations.
Round-off errors are often characterized by a random behavior of the numerical solution.
6.2.1.6. Solution Error Estimation
The most practical method to obtain estimates for the solution error is systematic grid refinement or
timestep reduction. In the following, the equations for error estimation are given for grid refinement.
The same process can be used for timestep refinement.
If the asymptotic range of the convergence properties of the numerical method is reached, the difference
between solutions on successively refined grids can be used as an error estimator. This allows the application of Richardson extrapolation to the solutions on the different grids (Roache [139 (p. 347)]). In
the asymptotic limit, the solution can be written as follows:
(6.14)
In this formulation,
is the grid spacing (or a linear measure of it) and the
are functions independent
of the grid spacing. The subscript, , refers to the current level of grid resolution. Solutions on different
grids are represented by different subscripts.
The assumption for the derivation of an error estimate is that the order of the numerical discretization
is known. This is usually the case. Assuming a second-order accurate method, the above expansion can
be written for two different grids:
(6.15)
Neglecting higher-order terms, the unknown function
timate for the exact solution is therefore:
can be eliminated from this equation. An es-
(6.16)
86
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Definition of Errors in CFD Simulations
The difference between the fine grid solution and the exact solution (defining the error) is therefore:
(6.17)
For an arbitrary order of accuracy, , of the underlying numerical scheme, the error is given by:
(6.18)
In order to build the difference between the solutions
and , it is required that the coarse and the
fine grid solution is available at the same location. In the case of a doubling of the grid density without
a movement of the coarse grid nodes, all information is available on the coarse grid nodes. The application of the correction to the fine-grid solution requires an interpolation of the correction to the fine
grid nodes (Roache [139 (p. 347)]). In the case of a general grid refinement, the solutions are not available
on the same physical locations. An interpolation of the solution between the different grids is then required for a direct error estimate. It has to be ensured that the interpolation error is lower than the
solution error in order to avoid a contamination of the estimate.
Richardson interpolation can also be applied to integral quantities (target variables), such as lift or drag
coefficients. In this case, no interpolation of the solution between grids is required.
Note that the above derivation is valid only if the underlying method has the same order of accuracy
everywhere in the domain and if the coarse grid is already in the asymptotic range (the error decreases
with the order of the numerical method). In addition, the method magnifies round-off and iteration
errors.
The intention of the Richardson interpolation was originally to improve the solution on the fine grid.
This requires an interpolation of the correction to the fine grid and introduces additional inaccuracies
into the extrapolated solution, such as errors in the conservation properties of the solution. A more
practical use of the Richardson extrapolation is the determination of the relative solution error, :
(6.19)
An estimate,
, of this quantity can be derived from Equation 6.16 (p. 86):
(6.20)
It can be shown (Roache [139 (p. 347)]) that the exact relative error and the approximation are related
by:
(6.21)
Equation 6.20 (p. 87) can also be divided by the range of
prevent the error to become infinite as
or another suitable quantity in order to
goes to zero.
In order to arrive at a practical error estimator, the following definitions are proposed:
Field error:
(6.22)
Maximum error:
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
87
CFX Best Practices Guide for Numerical Accuracy
(6.23)
RMS error:
(6.24)
Target variable error:
(6.25)
where is the defined target variable (list, drag, heat transfer coefficient, maximum temperature, mass
flow, and so on).
Similar error measures can be defined for derived variables, which can be specified for each test case.
Typical examples would be the total mass flow, the pressure drop, or the overall heat transfer. This will
be the recommended strategy, as it avoids the interpolation of solutions between the coarse and the
fine grid.
For unstructured meshes, the above considerations are valid only in cases of a global refinement of the
mesh. Otherwise, the solution error will not be reduced continuously across the domain. For unstructured
refinement the refinement level, , can be defined as follows:
(6.26)
where
is the number of grid points and
is the dimension of the problem.
It must be emphasized that these definitions do not impose an upper limit on the real error, but are
estimates for the evaluation of the quality of the numerical results. Limitations of the above error estimates are:
• The solution has to be smooth
• The truncation error order of the method has to be known
• The solution has to be sufficiently converged in the iteration domain
• The coarse grid solution has to be in the asymptotic range.
For three-dimensional simulations, the demand that the coarse grid solution be in the asymptotic range
is often hard to ensure. It is therefore required to compute the error for three different grid levels, to
avoid fortuitous results. If the solution is in the asymptotic range, the following indicator should be
close to constant:
(6.27)
6.2.2. Modeling Errors
In industrial CFD methods, numerous physical and chemical models are incorporated. Models are usually
applied to avoid the resolution of a large range of scales, which would result in excessive computing
requirements.
88
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Definition of Errors in CFD Simulations
The classical model used in almost all industrial CFD applications is a turbulence model. It is based on
time or ensemble averaging of the equations resulting in the so-called Reynolds Averaged Navier-Stokes
(RANS) equations. Due to the averaging procedure, information from the full Navier-Stokes equations
is lost. It is supplied back into the code by the turbulence model. The most widely used industrial
models are two-equation models, such as the
or
models.
The statistical model approach reduces the resolution requirements in time and space by many orders
of magnitude, but requires the calibration of model coefficients for certain classes of flows against experimental data. There is a wide variety of models that are introduced to reduce the resolution requirements for CFD simulations, including:
• Turbulence models
• Multi-phase models
• Combustion models
• Radiation models.
In combustion models, the reduction can be both in terms of the chemical species and in terms of the
turbulence-combustion interaction. In radiation, the reduction is typically in terms of the wavelength
and/or the directional information. For multi-phase flows, it is usually not possible to resolve a large
number of individual bubbles or droplets. In this case, the equations are averaged over the different
phases to produce continuous distributions for each phase in space and time.
As all of these models are based on a reduction of the ‘real’ physics to a reduced ‘resolution’, information
has to be introduced from outside the original equations. This is usually achieved by experimental calibration, or by available DNS (p. 82) results.
Once a model has been selected, the accuracy of the simulation cannot be increased beyond the capabilities of the model. This is the largest factor of uncertainty in CFD methods, as modeling errors can
be of the order of 100% or more. These large errors occur in cases where the CFD solution is very
sensitive to the model assumptions and where a model is applied outside its range of calibration.
Because of the complexity of industrial simulations, it cannot be ensured that the models available in
a given CFD code are suitable for a new application. While in most industrial codes a number of different
models are available, there is no a priori criterion as to the selection of the most appropriate one. Successful model selection is largely based on the expertise and the knowledge of the CFD user.
6.2.3. User Errors
User errors result from the inadequate use of the resources available for a CFD simulation. The resources
are given by:
• Problem description
• Computing power
• CFD software
• Physical models in the software
• Project time frame.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
89
CFX Best Practices Guide for Numerical Accuracy
According to the ERCOFTAC Best Practice Guidelines [140 (p. 347)], some of the sources for user errors
are:
• Lack of experience
• Lack of attention to detail or other mistakes.
Often, user errors are related to management errors when insufficient resources are assigned to a project,
or inexperienced users are given a too complex application. Typical user errors are:
• Oversimplification of a given problem; for example, geometry, equation system, and so on
• Poor geometry and grid generation
• Use of incorrect boundary conditions
• Selection of non-optimal physical models
• Incorrect or inadequate solver parameters; for example, timestep, and so on
• Acceptance of non-converged solutions
• Postprocessing errors.
6.2.4. Application Uncertainties
Application uncertainties result from insufficient knowledge to carry out the simulation. This is in most
cases a lack of information on the boundary conditions or of the details of the geometry. A typical example is the lack of detailed information at the inlet. A complete set of inlet boundary conditions is
composed of inflow profiles for all transported variables (momentum, energy, turbulence intensity,
turbulence length scale, volume fractions, and so on). This information can be supplied from experiments
or from a CFD simulation of the upstream flow. In most industrial applications, this information is not
known and bulk values are given instead. In some cases, the detailed information can be obtained from
a separate CFD simulation (for instance a fully developed pipe inlet flow). In other cases, the boundaries
can be moved far enough away from the area of interest to minimize the influence of the required assumptions for the complete specification of the boundary conditions.
Typical application uncertainties are:
• Lack of boundary condition information
• Insufficient information on the geometry
• Uncertainty in experimental data for solution evaluation.
6.2.5. Software Errors
Software errors are defined as any inconsistency in the software package. This includes the code, its
documentation, and the technical service support. Software errors occur when the information you
have on the equations to be solved by the software is different from the actual equations solved by
the code. This difference can be a result of:
• Coding errors (bugs)
• Errors in the graphical user interface (GUI)
90
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
General Best Practice Guidelines
• Documentation errors
• Incorrect support information.
6.3. General Best Practice Guidelines
In order to reduce the numerical errors, it is necessary to have procedures for the estimation of the
different errors described in Definition of Errors in CFD Simulations (p. 82). The main goal is to reduce
the solution error to a minimum with given computer resources.
6.3.1. Avoiding User Errors
User errors are directly related to the expertise, the thoroughness, and the experience of the user. For
a given user, these errors can only be minimized by good project management and thorough interaction
with others. In case of inexperienced users, day-to-day interaction with a CFD expert/manager is required
to avoid major quality problems. A structured work plan with intermediate results is important for intermediate and long-term projects.
A careful study of the CFD code documentation and other literature on the numerical methods as well
as the physical models is highly recommended. Furthermore, benchmark studies are recommended to
enable you to understand the capabilities and limitations of CFD methods. A comparison of different
CFD methods is desirable, but not always possible.
6.3.2. Geometry Generation
Before the grid generation can start, the geometry has to be created or imported from CAD-data. In
both cases, attention should be given to:
• The use of a correct coordinate system
• The use of the correct units
• The use of geometrical simplification, for example, symmetry planes
• Local details. In general, geometrical features with dimensions below the local mesh size (for example, wall
roughness or porous elements) are not included in the geometrical model. These should be incorporated
through a suitable model.
In the case that the geometry is imported from CAD-data, the data should be checked beforehand.
Frequently, after the import of CAD-data, the CAD-data has to be adapted (cleaned) before it can be
used for mesh generation. It is essential for mesh generation to have closed volumes. The various CADdata formats do not always contain these closed volumes. Therefore, the CAD-data has to be altered
in order to create the closed volumes. It has to be ensured that these changes do not influence the
flow to be computed.
6.3.3. Grid Generation
In a CFD analysis, the flow domain is subdivided in a large number of computational cells. All these
computational cells together form the so-called mesh or grid. The number of cells in the mesh should
be taken sufficiently large, such that an adequate resolution is obtained for the representation of the
geometry of the flow domain and the expected flow phenomena in this domain.
A good mesh quality is essential for performing a good CFD analysis. Therefore, assessment of the mesh
quality before performing a large and complex CFD analysis is very important. Most of the mesh generRelease 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
91
CFX Best Practices Guide for Numerical Accuracy
ators and CFD solvers offer the possibility of checking the mesh on several cells or mesh parameters,
such as aspect ratio, internal angle, face warpage, right handiness, negative volumes, cracks, and tetrahedral quality. The reader is referred to the user's guides of the various mesh generators and CFD
solvers for more information on these cells and mesh parameters.
Recommendations for grid generation are:
• Avoid high grid stretching ratios.
– Aspect ratios should not be larger than 20 to 50 in regions away from the boundary.
– Aspect ratios may be larger than that in unimportant regions.
– Aspect ratios may, and should, be larger than that in the boundary layers. For well resolved boundary
layers at high Re numbers, the near-wall aspect ratios can be of the order of 105-106.
• Avoid jumps in grid density.
– Growth factors should be smaller than 1.3.
• Avoid poor grid angles.
• Avoid non-scalable grid topologies. Non-scalable topologies can occur in block-structured grids and are
characterized by a deterioration of grid quality under grid refinement.
• Avoid non-orthogonal, for example, unstructured tetrahedral meshes, in (thin) boundary layers.
• Use a finer and more regular grid in critical regions, for example, regions with high gradients or large changes
such as shocks.
• Avoid the presence of arbitrary grid interfaces, mesh refinements, or changes in element types in critical
regions. An arbitrary grid interface occurs when there is no one-to-one correspondence between the cell
faces on both sides of a common interface, between adjacent mesh parts.
If possible, determine the size of the cells adjacent to wall boundaries where turbulence models are
used, before grid generation has started.
Numerical diffusion is high when computational cells are created that are not orthogonal to the fluid
flow. If possible, avoid computational cells that are not orthogonal to the fluid flow.
Judge the mesh quality by using the possibilities offered by the mesh generator. Most mesh generators
offer checks on mesh parameters, such as aspect ratio, internal angle, face warpage, right handiness,
negative volumes, cracks, and tetrahedral quality.
It should be demonstrated that the final result of the calculations is independent of the grid that is
used. This is usually done by comparison of the results of calculations on grids with different grid sizes.
Some CFD methods enable the application of grid adaptation procedures. In these methods, the grid
is refined in critical regions (high truncation errors, large solution gradients, and so on). In these methods,
the selection of appropriate indicator functions for the adaptation is essential for the success of the
simulations. They should be based on the most important flow features to be computed.
As a general rule, any important shear layer in the flow (boundary layer, mixing layer, free jets, wakes,
and so on) should be resolved with at least 10 nodes normal to the layer. This is a very challenging requirement that often requires the use of grids that are aligned with the shear layers.
92
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
General Best Practice Guidelines
6.3.4. Model Selection and Application
Modeling errors are the most difficult errors to avoid, as they cannot be reduced systematically. The
most important factor for the reduction of modeling errors is the quality of the models available in the
CFD package and the experience of the user. There is also a strong interaction between modeling errors
and the time and space resolution of the grid. The resolution has to be sufficient for the model selected
for the application.
In principle, modeling errors can only be estimated in cases where the validation of the model is ‘close’
to the intended application. Model validation is essential for the level of confidence you can have in a
CFD simulation. It is therefore required that you gather all available information on the validation of
the selected model, both from the open literature and from the code developers (vendors). In case that
CFD is to be applied to a new field, it is recommended that you carry out additional validation studies,
in order to gain confidence that the physical models are adequate for the intended simulation.
If several modeling options are available in the code (as is usually the case for turbulence, combustion
and multi-phase flow models), it is recommended that you carry out the simulation with different
models in order to test the sensitivity of the application with respect to the model selection.
In case you have personal access to a modeling expert in the required area, it is recommended that
you interact with the model developer or expert to ensure the optimal selection and use of the model.
6.3.4.1. Turbulence Models
There are different methods for the treatment of turbulent flows. The need for a model results from
the inability of CFD simulations to fully resolve all time and length scales of a turbulent motion. In
classical CFD methods, the Navier-Stokes equations are usually time- or ensemble-averaged, reducing
the resolution requirements by many orders of magnitude. The resulting equations are the RANS (p. 89)
equations. Due to the averaging procedure, information is lost, which is then fed back into the equations
by a turbulence model.
The amount of information that has to be provided by the turbulence model can be reduced if the
large time and length scales of the turbulent motion are resolved. The equations for this so-called Large
Eddy Simulation (LES) method are usually filtered over the grid size of the computational cells. All scales
smaller than the resolution of the mesh are modeled and all scales larger than the cells are computed.
This approach is several orders of magnitude more expensive than a RANS (p. 89) simulation and is
therefore not used routinely in industrial flow simulations. It is most appropriate for free shear flows,
as the length scales near the solid walls are usually very small and require small cells even for the
LES (p. 93) method.
RANS (p. 89) methods are the most widely used approach for CFD simulations of industrial flows. Early
methods, using algebraic formulations, have been largely replaced by more general transport equation
models, for both implementation and accuracy considerations. The use of algebraic models is not recommended for general flow simulations, due to their limitations in generality and their geometric restrictions. The lowest level of turbulence models that offer sufficient generality and flexibility are twoequation models. They are based on the description of the dominant length and time scale by two independent variables. Models that are more complex have been developed and offer more general
platforms for the inclusion of physical effects. The most complex RANS (p. 89) model used in industrial
CFD applications are Second Moment Closure (SMC) models. Instead of two equations for the two main
turbulent scales, this approach requires the solution of seven transport equations for the independent
Reynolds stresses and one length (or related) scale.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
93
CFX Best Practices Guide for Numerical Accuracy
The challenge for the user of a CFD method is to select the optimal model for the application at hand
from the models available in the CFD method. In most cases, it cannot be specified beforehand which
model will offer the highest accuracy. However, there are indications as to the range of applicability of
different turbulence closures. This information can be obtained from validation studies carried out with
the model.
In addition to the accuracy of the model, consideration has to be given to its numerical properties and
the required computer power. It is often observed that more complex models are less robust and require
many times more computing power than the additional number of equations would indicate. Frequently,
the complex models cannot be converged at all, or, in the worst case, the code becomes unstable and
the solution is lost.
It is not trivial to provide general rules and recommendations for the selection and use of turbulence
models for complex applications. Different CFD groups have given preference to different models for
historical reasons or personal experiences. Even turbulence experts cannot always agree as to which
model offers the best cost-performance ratio for a new application.
6.3.4.1.1. One-equation Models
A number of one-equation turbulence models based on an equation for the eddy viscosity have been
developed over the last years. Typical applications are:
• Airplane- and wing flows
• External automobile aerodynamics
• Flow around ships.
These models have typically been optimized for aerodynamic flows and are not recommended as general-purpose models.
6.3.4.1.2. Two-equation Models
The two-equation models are the main-stand of industrial CFD simulations. They offer a good compromise
between complexity, accuracy and robustness. The most popular models are the standard model and
different versions of the
model, see Wilcox [30 (p. 331)]. The standard
model of Wilcox is the
most well known of the
based models, but shows a severe free-stream dependency. It is therefore
not recommended for general industrial flow simulations, as the results are strongly dependent on the
user input. Alternative formulations are available, see for example, the Shear Stress Transport (SST)
model, Menter [9 (p. 328)].
An important weakness of standard two-equation models is that they are insensitive to streamline
curvature and system rotation. Particularly for swirling flows, this can lead to an over-prediction of turbulent mixing and to a strong decay of the core vortex. There are curvature correction models available,
but they have not been generally validated for complex flows.
The standard two-equation models can also exhibit a strong build-up of turbulence in stagnation regions,
due to their modeling of the production terms. Several modifications are available to reduce this effect,
for instance by Kato and Launder [128 (p. 345)]. They should be used for flows around rods, blades, airfoils,
and so on.
94
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
General Best Practice Guidelines
6.3.4.1.3. Second Moment Closure (SMC) Models
SMC (p. 93) models are based on the solution of a transport equation for each of the independent
Reynolds stresses in combination with the - or the -equation. These models offer generally a wider
modeling platform and account for certain effects due to their exact form of the turbulent production
terms. Some of these models show the proper sensitivity to swirl and system rotation, which have to
be modeled explicitly in a two-equation framework. SMC (p. 93) models are also superior for flows in
stagnation regions, where no additional modifications are required.
One of the weak points of the SMC (p. 93) closure is that the same scale equations are used as in the
two-equation framework. As the scale equation is typically one of the main sources of uncertainty, it is
found that SMC (p. 93) models do not consistently produce superior results compared to the simpler
models. In addition, experience has shown that SMC (p. 93) models are often much harder to handle
numerically. The model can introduce a strong nonlinearity into the CFD method, leading to numerical
problems in many applications.
SMC (p. 93) models are usually not started from a pre-specified initial condition, but from an already
available solution from a two-equation (or simpler) model. This reduces some of the numerical problems
of the SMC (p. 93) approach. In addition, it offers an important sensitivity study, as it allows quantifying
the influence of the turbulence model on the solution. It is therefore recommended that you fully
converge the two-equation model solution and save it for a comparison with the SMC (p. 93) model
solution. The difference between the solutions is a measure of the influence of the turbulence model
and therefore an indication of the modeling uncertainty. This is possible only in steady-state simulations.
For unsteady flows, the models usually have to be started from the initial condition.
6.3.4.1.4. Large Eddy Simulation Models
LES (p. 93) models are based on the numerical resolution of the large turbulence scales and the modeling of the small scales. LES (p. 93) is not yet a widely used industrial approach, due to the large cost
of the required unsteady simulations. For certain classes of applications, LES (p. 93) will be applicable
in the near future. The most appropriate area will be free shear flows, where the large scales are of the
order of the solution domain (or only an order of magnitude smaller). For boundary layer flows, the
resolution requirements are much higher, as the near-wall turbulent length scales become much smaller.
The internal flows (pipe flows, channel flows) are in between, as they have a restricted domain in the
wall normal direction, but small scales have to be resolved in the other two directions.
LES (p. 93) simulations do not easily lend themselves to the application of grid refinement studies both
in the time and the space domain. The main reason is that the turbulence model adjusts itself to the
resolution of the grid. Two simulations on different grids are therefore not comparable by asymptotic
expansion, as they are based on different levels of the eddy viscosity and therefore on a different resolution of the turbulent scales. From a theoretical standpoint, the problem can be avoided, if the LES (p. 93)
model is not based on the grid spacing, but on a pre-specified filter-width. This would enable reaching
grid-independent LES (p. 93) solutions above the DNS (p. 82) limit. However, LES (p. 93) is a very expensive method and systematic grid and timestep studies are prohibitive even for a pre-specified filter.
It is one of the disturbing facts that LES (p. 93) does not lend itself naturally to quality assurance using
classical methods. This property of the LES (p. 93) also indicates that (nonlinear) multigrid methods of
convergence acceleration are not suitable in this application.
On a more global level, the grid convergence can be tested using averaged quantities resulting from
the LES (p. 93) simulation. The averaged LES (p. 93) results can be analyzed in a similar way as
RANS (p. 89) solutions (at least qualitatively). Again, it is expensive to perform several LES (p. 93) simulations and grid refinement will therefore be more the exception than the rule.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
95
CFX Best Practices Guide for Numerical Accuracy
Due to the high computing requirements of LES (p. 93), modern developments in the turbulence
models focus on a combination of RANS (p. 89) and LES (p. 93) models. The goal is to cover the wall
boundary layers with RANS (p. 89) and to enable unsteady (LES (p. 93)-like) solutions in largely separated
and unsteady flow regions (for example, flow behind a building, or other blunt bodies). There are two
alternatives of such methods available in ANSYS CFX.
The first alternative is called Scale-Adaptive-Simulation (SAS) model (Menter and Egorov [130 (p. 346)],
[131 (p. 346)], [144 (p. 348)], [145 (p. 348)]). It is essentially an improved Unsteady RANS (URANS) method
that develops LES (p. 93)-like solutions in unstable flow regimes.
The second alternative is called Detached Eddy Simulation (DES) (Spalart [146 (p. 348)]), implemented in
the version of Strelets [58 (p. 335)]. The current recommendation is to use the SAS (p. 96) model, as it
has less grid sensitivity than the DES (p. 96) formulation. In case that SAS (p. 96) does not provide an
unsteady solution, the DES (p. 96) model should be applied. It should be noted that both model formulations require small timesteps with a Courant number of CFL<1. You are encouraged to read the original references before applying these models.
6.3.4.1.5. Wall Boundary Conditions
There are generally three types of boundary conditions that can be applied to a RANS (p. 89) simulation:
• Wall Function Boundary Conditions (p. 96)
• Integration to the wall (low-Reynolds number formulation) (p. 96)
• Mixed formulation (automatic near-wall treatment) (p. 97).
6.3.4.1.5.1. Wall Function Boundary Conditions
Standard wall functions are based on the assumption that the first grid point off the wall (or the first
integration point) is located in the universal law-of-the-wall or logarithmic region. Wall functions eliminate the need to resolve the very thin viscous sublayer, leading to a reduction in the number of cells
and to a more moderate (and desirable) aspect ratio of the cells (ratio of the longest to the smallest
side in a structured grid). High aspect ratios can result in numerical problems due to round-off errors.
On the other hand, standard wall function formulations are difficult to handle, because you have to
ensure that the grid resolution near the wall satisfies the wall function requirements. If the grid becomes
too coarse, the resolution of the boundary layer is no longer ensured. If the resolution becomes too
fine, the first grid spacing can be too small to bridge the viscous sublayer. In this case, the logarithmic
profile assumptions are no longer satisfied. You have to ensure that both limits are not overstepped in
the grid generation phase.
The lower limit on the grid resolution for standard wall functions is a severe detriment to a systematic
grid refinement process, as required by the best practice approach. That is, instead of an improved accuracy of the solution with grid refinement, the solution will deteriorate from a certain level on, leading
eventually to a singularity of the numerical method. Standard wall functions are therefore not recommended for systematic grid refinement studies. Recently, alternative formulations (scalable wall functions)
have become available, Menter and Esch [142 (p. 347)], which enable a systematic grid refinement when
using wall functions.
6.3.4.1.5.2. Integration to the wall (low-Reynolds number formulation)
The use of low-Reynolds (low-Re) number formulations of turbulence models for the integration of the
equations through the viscous sublayer is generally more accurate, as no additional assumptions are
96
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
General Best Practice Guidelines
required concerning the variation of the variables near the wall. On the downside, most low-Re extensions
of turbulence models are quite complex and can reduce the numerical performance or even destabilize
the numerical method. In addition, classical low-Re models require a very fine near-wall resolution of
at all wall nodes. This is very hard to ensure for all walls of a complex industrial application. In
the case that significantly coarser grids are used, the wall shear stress and the wall heat transfer can be
reduced significantly below their correct values.
6.3.4.1.5.3. Mixed formulation (automatic near-wall treatment)
In ANSYS CFX, hybrid methods are available for all -equation based turbulence models (automatic
near-wall treatment), which automatically switch from a low-Re formulation to wall functions based on
the grid spacing you provide. These formulations provide the optimal boundary condition for a given
grid. From a best practice standpoint, they are the most desirable, as they enable an accurate near-wall
treatment over a wide range of grid spacings. However, accurate boundary layer simulations do not
depend only on the
near-wall spacing, but also require a minimum of at least 10 grid nodes inside
the boundary layer.
6.3.4.1.5.4. Recommendations for Model Selection
• Avoid the use of classical wall functions, as they are inconsistent with grid refinement.
• Avoid strict low-Re number formulations, unless it is ensured that all near-wall cells are within the resolution
requirements of the formulation.
• In combination with the
model, use scalable wall functions. They can be applied to a range of grids
without immediate deterioration of the solution (default in ANSYS CFX).
• For more accurate simulations, use an automatic wall treatment in combination with SST (p. 94) turbulence
model (default in ANSYS CFX).
6.3.4.2. Heat Transfer Models
The heat transfer formulation is strongly linked to the underlying turbulence model. For eddy viscosity
models, the heat transfer simulation is generally based on the analogy between heat and momentum
transfer. Given the eddy viscosity of the two-equation model, the heat transfer prediction is based on
the introduction of a molecular and a turbulent Prandtl number. The treatment of the energy equation
is therefore similar to the treatment of the momentum equations. No additional transport equations
are required for the turbulent heat transfer prediction. The boundary conditions are the same as for
the momentum equations and follow the same recommendations.
For SMC (p. 93) models, three additional transport equations must be solved for the turbulent heat
transfer vector in order to be consistent with the overall closure level. Only a few CFD methods offer
this option. In most cases, the heat transfer is computed from an eddy diffusivity with a constant turbulent
Prandtl number.
6.3.4.3. Multi-Phase Models
Multi-phase models are required in cases where more than one phase is involved in the simulation
(phases can also be non-miscible fluids). There is a wide variety of multi-phase flow scenarios, with the
two extremes of small-scale mixing of the phases or a total separation of the phases by a sharp interface.
Depending on the flow simulation, different types of models are available. The main distinction of the
models is given below.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
97
CFX Best Practices Guide for Numerical Accuracy
Lagrange models solve a separate equation for individual particles, bubbles, or droplets in a surrounding
fluid. The method integrates the three-dimensional trajectories of the particles based on the forces
acting on them from the surrounding fluid and other sources. Turbulence is usually accounted for by
a random motion, superimposed on the trajectory.
Lagrange models are usually applied to flows with low particle (bubble) densities. In these flows, the
interaction between the particles can usually be neglected, thereby reducing the complexity of the
problem significantly.
The Euler-Euler formulation is based on the assumption of interpenetrating continua. A separate set of
mass, momentum, and energy conservation equations is solved for each phase. Interphase transfer
terms have to be modeled to account for the interaction of the phases. Euler-Euler methods can be
applied to separated and dispersed flows by changing the interface transfer model.
Additional models are required for flows with mass transfer between the phases (condensation, evaporation, boiling). These models can be applied in the form of correlations for a large number of particles
(bubbles) in a given control volume, or directly at the interface between the resolved phase boundary.
6.3.5. Reduction of Application Uncertainties
Application uncertainties cannot always be avoided because the missing information can frequently
not be recovered. The uncertainty can be minimized by interaction with the supplier of the test case.
The potential uncertainties have to be documented before the start of the CFD application.
In the case that the assumptions have to be made concerning any input to a CFD analysis, they have
to be communicated to the partners in the project. Alternative assumptions have to be proposed and
the sensitivity of the solution to these assumptions has to be evaluated by case studies (alteration of
inflow profiles, different locations for arbitrary boundary conditions, and so on).
Recommendations are:
• Identify all uncertainties in the numerical setup:
– Geometry reduction
– Boundary condition assumptions
– Arbitrary modeling assumptions, for example, bubble diameter, and so on.
• Perform a sensitivity analysis with at least two settings for each arbitrary parameter.
• Document the sensitivity of the solution on the assumptions.
6.3.6. CFD Simulation
This section provides recommendations concerning the optimal application of a CFD method, once the
grids are available and the basic physical models have been defined.
6.3.6.1. Target Variables
In order to monitor numerical errors, it is recommended that you define target variables. The convergence
of the numerical scheme can then be checked more easily and without interpolation between different
grids. You should select target variables that:
98
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
General Best Practice Guidelines
1.
Are representative of the goals of the simulation.
2.
Are sensitive to numerical treatment and resolution.
This criteria should help to avoid the use of measures that are insensitive to the resolution, such
as pressure-based variables in boundary layer simulations.
3.
Can be computed with existing postprocessing tools.
4.
Can be computed inside the solver and displayed during run time (optimal).
It is optimal if the variable can be computed during run time and displayed as part of the convergence
history. This enables you to follow the development of the target variable during the iterative process.
6.3.6.2. Minimizing Iteration Errors
A first indication of the convergence of the solution to steady-state is the reduction in the residuals.
Experience shows, however, that different types of flows require different levels of residual reduction.
For example, it is found regularly that swirling flows can exhibit significant changes even if the residuals
are reduced by more than 5 - 6 orders of magnitude. Other flows are well converged with a reduction
of only 3 - 4 orders.
In addition to the residual reduction, it is therefore required to monitor the solution during convergence
and to plot the pre-defined target quantities of the simulation as a function of the residual (or the iteration number). A visual observation of the solution at different levels of convergence is recommended.
It is also recommended that you monitor the global balances of conserved variables, such as mass,
momentum and energy, vs. the iteration number.
Convergence is therefore monitored and ensured by the following steps:
• Reduce residuals by a pre-specified level and provide residual plots.
• Plot evolution of r.m.s. and maximum residual with iteration number.
• Report global mass balance with iteration number.
• Plot target variables as a function of iteration number or residual level.
• Report target variables as a function of r.m.s. residual (table).
It is desirable to have the target variable written out at every timestep in order to display it during the
simulation run.
Depending on the numerical scheme, the recommendations may also be relevant to the iterative convergence within the timestep loop for transient simulations.
6.3.6.3. Minimizing Spatial Discretization Errors
Spatial discretization errors result from the numerical order of accuracy of the discretization scheme
and from the grid spacing. It is well known that only second- and higher-order space discretization
methods are able to produce high quality solutions on realistic grids. First-order methods should
therefore be avoided for high quality CFD simulations.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
99
CFX Best Practices Guide for Numerical Accuracy
As the order of the scheme is usually given (mostly second-order), spatial discretization errors can be
influenced only by the provision of an optimal grid. It is important for the quality of the solution and
the applicability of the error estimation procedures defined in Solution Error Estimation (p. 86), that
the coarse grid already resolves the main features of the flow. This requires that the grid points are
concentrated in areas of large solution variation. For the reduction of spatial discretization errors, it is
also important to provide a high-quality numerical grid.
For grid convergence tests, the simulations are carried out for a minimum of three grids. The target
quantities will be given as a function of the grid density. In addition, an error estimate based on the
definition given in Solution Error Estimation (p. 86) (Equation 6.25 (p. 88)) will be carried out. It is also
recommended that you compute the quantity given by Equation 6.27 (p. 88) to test the assumption of
asymptotic convergence.
It is further recommended that the graphical comparison between the experiments and the simulations
show the grid influence for some selected examples. The following information should be provided:
• Define target variable as given in Target Variables (p. 98).
• Provide three (or more) grids using the same topology (or for unstructured meshes, a uniform refinement
over all cells).
• Compute solution on these grids:
– Ensure convergence of the target variable in the time- or iteration domain. See Iteration Errors (p. 85)
and Minimizing Iteration Errors (p. 99).
– Compute target variables for these solutions.
• Compute and report error measure for target variable(s) based on Equation 6.25 (p. 88).
• Plot selected variables for the different grids in one picture.
• Check if the solution is in the asymptotic range using Equation 6.27 (p. 88).
6.3.6.4. Minimizing Time Discretization Errors
In order to reduce time integration errors for unsteady-state simulations, it is recommended that you
use at least a second-order-accurate time-discretization scheme. Usually, the relevant frequencies can
be estimated beforehand and the timestep can be adjusted to provide at least 10 - 20 steps for each
period of the highest relevant frequency. In case of unsteadiness due to a moving front, the timestep
should be chosen as a fraction of:
(6.28)
with the grid spacing
and the front speed
.
It should be noted that under strong grid and timestep refinement, sometimes flow features are resolved
that are not relevant for the simulation. An example is the (undesirable) resolution of the vortex shedding
at the trailing edge of an airfoil or a turbine blade in a RANS (p. 89) simulation for very fine grids and
timesteps. Another example is the gradual switch to a DNS (p. 82) for the simulation of free surface
flows with a Volume of Fluid (VOF) method (for example, drop formation, wave excitation for free
surfaces, and so on). This is a difficult situation, as it usually means that no grid/timestep converged
solution exists below the DNS (p. 82) range, which can usually not be achieved.
100
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Selection and Evaluation of Experimental Data
In principle, the time dependency of the solution can be treated as another dimension of the problem
with the definitions in Solution Error Estimation (p. 86). However, a four-dimensional grid study would
be very demanding. It is therefore more practical to carry out the error estimation in the time domain
separately from the space discretization. Under the assumption that a sufficiently fine space discretization
is available, the error estimation in the time domain can be performed as a one-dimensional study.
Studies should be carried out with at least two and if possible three different timesteps for one given
spatial resolution. Again, the error estimators given in Solution Error Estimation (p. 86) (Equation 6.25 (p. 88)) can be used, if is replaced by the timestep. The following information should be
provided:
• Unsteady target variables as a function of timestep (graphical representation)
• Error estimate based on Equation 6.25 (p. 88) for (time averaged) target variables
• Comparison with experimental data for different timesteps.
6.3.6.5. Avoiding Round-Off Errors
Round-off errors are usually not a significant problem. They can occur for high-Reynolds number flows
where the boundary layer resolution can lead to very small cells near the wall. The number of digits of
a single precision simulation can be insufficient for such cases. The only way to avoid round-off errors
with a given CFD code is the use of a double precision version. In case of an erratic behavior of the
CFD method, the use of a double precision version is recommended.
6.3.7. Handling Software Errors
Software errors can be detected by verification studies. They are based on a systematic comparison of
CFD results with verified solutions (in the optimal case analytical solutions). It is the task of the software
developer to ensure the functionality of the software by systematic testing.
In most cases, pre-existing software will be used. It is assumed that all CFD packages have been sufficiently tested to ensure that no software verification studies have to be carried out in the project (except
for newly developed modules). In case that two CFD packages give different results for the same application, using the same physical models, the sources for these differences will have to be evaluated. In
case of code errors, they will be reported to the code developers and if possible removed.
6.4. Selection and Evaluation of Experimental Data
Because of the necessity to model many of the unresolved details of technical flows, it is necessary to
assess the accuracy of the CFD method with the help of experimental data. Experiments are required
for the following tasks and purposes:
• Verification of model implementation
• Validation and calibration of statistical models
• Demonstration of model capabilities.
There is no philosophical difference between the different types of test cases. The same test case can
be used for the different phases of model development, implementation, validation, and application,
depending on the status of the model and the suitability of the data.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
101
CFX Best Practices Guide for Numerical Accuracy
6.4.1. Verification Experiments
The purpose of verification tests is to ensure the correct implementation of all numerical and physical
models in a CFD method. The best verification data would be the analytical solutions for simple cases
that enable the testing of all relevant implementation aspects of a CFD code and the models implemented. As analytical solutions are not always available, simple experimental test cases are often used instead.
6.4.1.1. Description
For CFD code verification, convergence can be tested against exact analytical solutions like:
• Convection of disturbances by a given flow
• Laminar Couette flow
• Laminar channel flow.
For the verification of newly implemented models, verification can only in limited cases be based on
analytical solutions. An example is the terminal rise velocity of a spherical bubble in a calm fluid.
In most other cases, simple experiments are used for the verification. It is recommended that you
compute the test cases given by the model developer in the original publication of the model, or other
trustworthy publications. Quite often experimental correlations can be applied, without the need for
comparison with one specific experiment. For instance for turbulence model verification, the most frequently used correlations are those for flat plate boundary layers.
6.4.1.2. Requirements
The only requirement for verification data is that they enable a judgement of the correct implementation
of the code and/or the models. This requires information from other sources concerning the performance
of the model for the test case. Strictly speaking, it is not required that the simulations are in good
agreement with the data, but that the differences between the simulations and the data are as expected.
The test suite for model verification must be diverse enough to check all aspects of the implementation.
As an example, a fully developed channel flow does not enable a test of the correct implementation
of the convective terms of a transport equation. The test suite should also enable testing the correct
interaction of the new model with other existing features of the software.
Software verification for physical models should be carried out in the same environment that the enduser has available. Testing of the new features in an expert environment might miss some of error
sources, such as the GUI.
Verification cases should be selected before the model is implemented. They must be considered an
integral part of the model implementation.
6.4.2. Validation Experiments
The purpose of validation tests is to check the quality of a statistical model for a given flow situation.
Validation tests are the only method to ensure that a new model is applicable with confidence to certain
types of flows. The more validation tests a model passes with acceptable accuracy, the more generally
it can be applied to industrial flows. The goal of validation tests is to minimize and quantify modeling
errors. Validation cases are often called building block experiments, as they test different aspects of a
CFD code and its physical models. The successful simulation of these building blocks is a prerequisite
for a complex industrial flow simulation.
102
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Selection and Evaluation of Experimental Data
6.4.2.1. Description
Examples of validation cases are flows with a high degree of information required to test the different
aspects of the model formulation. In an ideal case, a validation test case should be sufficiently complete
to enable an improvement of the physical models it was designed to evaluate. Increasingly, validation
data are obtained from DNS (p. 82) studies. The main limitation here is in the low-Reynolds number
and the limited physical complexity of DNS (p. 82) data. Typically, validation cases are geometrically
simple and often based on two-dimensional or axisymmetric geometries.
6.4.2.2. Requirements
Validation cases are selected to be as close as possible to the intended application of the model. As an
example, the validation of a turbulence model for a flat plate boundary layer does not ensure the applicability of the model to flows with separation (as is known from the
model). It is well accepted
by the CFD community and by model developers that no model (turbulence, multi-phase or other) will
be able to cover all applications with sufficient accuracy. This is the reason why there are always multiple
models for each application. The validation cases enable the CFD user to select the most appropriate
model for the intended type of application.
Test case selection requires that the main features of the CFD models that are to be tested be clearly
identified. They must then be dominant in the validation case. Validation cases are often ‘single physics’
cases, but it will be more and more necessary to validate CFD methods for combined effects.
The requirements for validation cases are that there should be sufficient detail to be able to compute
the flow unambiguously and to evaluate the performance of the CFD method for a given target application.
Completeness of information is one of the most important requirements for a validation test case. This
includes all information required to run the simulation, like:
• Geometry
• Boundary conditions
• Initial conditions (for unsteady flows)
• Physical effects involved.
While the first three demands are clearly necessary to be able to set up and run the simulation, the
knowledge of all physical effects taking place in the experiment is not always considered. However, it
is crucial to have a clear understanding of the overall flow in order to be able to judge the quality of
a test case. Typical questions are:
• Is the flow steady-state or does it have a large-scale unsteadiness?
• Is the flow two-dimensional (axisymmetric, for example)?
• Are all the relevant physical effects known (multi-phase, transition, and so on)?
• Have any corrections been applied to the data and are they appropriate?
• Was there any measurement/wind or water tunnel interference?
Completeness of information is also essential for the comparison of the simulation results with the experimental data. A validation case should have sufficient detail to identify the sources for the discrepRelease 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
103
CFX Best Practices Guide for Numerical Accuracy
ancies between the simulations and the data. This is a vague statement and cannot always be ensured,
but a validation experiment should provide more information than isolated point measurements. Profiles
and distributions of variables at least in one space dimension should be available (possibly at different
locations). More desirable is the availability of field data in two-dimensional measuring planes including
flow visualizations.
Completeness also relates to the non-dimensionalization of the data. Frequently the information provided
is not sufficient to reconstruct the data in the form required by the validation exercise.
In case that the data provided are not sufficient, the impact of the missing information has to be assessed.
Most crucial is the completeness of the data required to set up the simulation. In case of missing information, the influence of this information deficit has to be assessed. Typical examples are incomplete inlet
boundary conditions. While the mean flow quantities are often provided, other information required
by the method, as profiles for turbulent length scales and volume fractions is frequently missing. The
importance of this deficit can be estimated by experience with similar flows and by sensitivity studies
during the validation exercise.
Next to the completeness of the data, their quality is of primary importance for a successful validation
exercise. The quality of the data is mainly evaluated by error bounds provided by the experimentalists.
Unfortunately, most experiments still do not provide this information. Moreover, even if error estimates
are available, they cannot exclude systematic errors by the experimentalist.
In addition to error bounds, it is therefore desirable to have an overlap of experimental data that enable
testing the consistency of the measurements. Examples are the same data from different experimental
techniques. It is also a quality criterion when different experimental groups in different facilities have
carried out the same experiment. Consistency can also be judged from total balances, like mass, momentum and energy conservation. Quality and consistency can frequently be checked if validation exercises have already been carried out by other CFD groups, even if they used different models.
The availability of the data has to be considered before any CFD validation is carried out. This includes
questions of ownership. For most CFD code developers, data that cannot be shown publicly are much
less valuable than freely available experimental results.
6.4.3. Demonstration Experiments
The purpose of a demonstration exercise is to build confidence in the ability of a CFD method to simulate
complex flows. While validation studies have shown for a number of building block experiments that
the physical models can cover the basic aspects of the target application, the demonstration cases test
the ability of a method to predict combined effects, including geometrical complexity.
6.4.3.1. Description
For an aerodynamic study, a typical hierarchy would be:
• Verification - Flat plate
• Validation - Airfoil or wing
• Demonstration - Complete aircraft.
Similar hierarchies can be established for other industrial areas.
104
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Selection and Evaluation of Experimental Data
6.4.3.2. Requirements
Typically, the detail of the experimental data is much lower than for verification or validation cases.
Completeness of information to set up the test case is of similar importance as for validation cases and
involves the same aspects as listed below:
• Geometry
• Boundary conditions
• Initial conditions (for unsteady flows)
• Physical effects involved.
Typically, the level of completeness of the data for demonstration cases is much lower than for validation
cases. It is therefore even more essential to identify the missing information and to carry out sensitivity
studies with respect to these data.
In terms of postprocessing, demonstration cases often do not provide a high degree of detail. They are
usually not appropriate to identify specific weaknesses in the physical models or the CFD codes. Typically,
only the point data or global parameters, as efficiencies, are provided.
Even though the density of data is usually lower, the quality should satisfy the same criteria as for validation cases. Error estimates are desirable and so are independent measurements.
Due to the limited amount of data available, the information is usually not sufficient to carry out consistency checks.
The requirements in terms of availability/openness are usually lower than for validation cases, as the
demonstration applies usually to a smaller audience. A demonstration case might be carried out for a
single customer or one specific industrial sector. It has to be ensured, as in all cases, that the data can
be shown to the target audience of the simulation.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
105
106
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 7: CFX Best Practices Guide for Cavitation
This guide is part of a series that provides advice for using CFX in specific engineering application areas.
It is aimed at users with moderate or little experience using CFX for applications involving cavitation.
This guide describes Liquid Pumps (p. 107).
Cavitation is the formation of vapor bubbles within a liquid where flow dynamics cause the local static
pressure to drop below the vapor pressure. The bubbles of vapor usually last a short time, collapsing
when they encounter higher pressure. Cavitation should not be confused with boiling. When a liquid
boils, thermal energy drives the local temperature to exceed the saturation temperature.
Cavitation is a concern in several application areas, including pumps, inducers, marine propellers, water
turbines, and fuel injectors. One of the major problems caused by cavitation is a loss of pressure rise
across a pump. Other problems include noise, vibration, and damage to metal components.
The next section discusses the effects of cavitation on the performance of liquid pumps.
7.1. Liquid Pumps
Water pumps must take in water and deliver it at a higher total pressure with an acceptable flow rate.
Under certain conditions, cavitation may occur on the low pressure side of the pump, causing a loss of
pressure rise and/or flow rate.
Both pump performance without cavitation and the affects of cavitation on performance will be discussed.
7.1.1. Pump Performance without Cavitation
As long as the static pressure remains sufficiently high everywhere in the system, cavitation will not
occur. In this case, for a given pump RPM, the pressure rise and flow rate are directly coupled, and can
be plotted in a pump performance diagram, as shown below.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
107
CFX Best Practices Guide for Cavitation
Figure 7.1: Flow Rate vs Pressure Rise for a Liquid Pump
7.1.2. Pump Performance with Cavitation
If the inlet total pressure is below the critical value for a particular flow rate and RPM, cavitation will
occur causing the pressure rise to diminish. The following performance diagram shows the effect of
cavitation on pressure rise.
Figure 7.2: Cavitation Performance at Constant RPM and Flow Rate
NPSH is the Net Positive Suction Head, a quantity directly related to the inlet total pressure by the relation:
(7.1)
108
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Liquid Pumps
where pT,inlet is the inlet total pressure, pv is the vapor pressure, is density, and g is the acceleration
due to gravity. As the inlet total pressure drops, so does the NPSH value, and the amount of cavitation
increases.
To generate this diagram, RPM and flow rate are fixed, and the pressure rise is measured at progressively
lower inlet total pressures. For the part of the test where the inlet total pressure is sufficiently high to
prevent cavitation, the pressure rise across the pump is constant, equal to the amount predicted by
the first performance diagram. This results in a horizontal trend in the performance curve as the inlet
total pressure is dropped. Because the pressure rise remains constant, the total pressure at the outlet
drops by the same amount as at the inlet. Using CFX software, a mass flow outlet boundary condition
can be specified to fix the flow rate while the inlet total pressure is varied.
When the inlet total pressure reaches a sufficiently low value, cavitation occurs. A further reduction in
inlet total pressure causes more cavitation, which almost always causes a large loss of pressure rise. In
rare cases, pressure rise can actually increase slightly with small amounts of cavitation. Even in such
cases, however, a further increase in cavitation causes a sudden loss of pressure rise. In the lab, the
pressure rise will eventually become insufficient to maintain the required flow rate. Using CFX software,
the solution will eventually fail to converge. Before this point, data should be collected with a sufficient
resolution (sufficiently small changes in inlet pressure) to resolve the part of the performance curve
where the pressure starts to drop. The point of cavitation is often marked by the NPSH at which the
pressure rise has fallen by a few percent.
7.1.3. Procedure for Plotting Performance Curve
1.
Set up a simulation with cavitation turned on and pressure levels set high enough to avoid levels of
cavitation that significantly affect pressure rise.
If you have trouble getting a converged solution, try running a simulation with cavitation turned
off, then use the result as an initial guess for a simulation with cavitation turned on.
2.
Run the solver to obtain a solution.
3.
Calculate the pressure rise across the pump and the NPSH value, then plot a point in the performance
diagram.
4.
Lower the pressure boundary condition by about 5% to 10%.
5.
Repeat starting from step 2, using the previous solution as the initial guess, until cavitation has caused a
significant loss of pump head.
7.1.4. Setup
To facilitate setting up typical domain settings for the cavitation of water, you may load a single-domain
mesh, then run the template .ccl file:
CFX/etc/model-templates/cavitating_water.ccl
This file should be examined in a text editor before using it so that you understand which settings it
specifies.
For the domain fluids list, specify both a liquid and a vapor for the same material. In most cases, it is
sufficient to use a constant-density vapor.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
109
CFX Best Practices Guide for Cavitation
Under Fluid Models for the domain, it is strongly recommended that you select Homogeneous Model
under Multiphase Options. You do not need to select Free Surface Model for the purpose of simulating
cavitation.
Under Fluid Pairs for the domain, select the fluid pair from the list and, for Mass Transfer, set Option
to Cavitation. Select the Rayleigh Plesset cavitation model or a User Defined Cavitation Model.
For the Rayleigh Plesset model, the Mean Diameter for cavitation bubbles represents the mean nucleation site diameter and must be specified. The default value of 2e-06 m is a reasonable value in most
cases. The Saturation Pressure must be defined unless the materials you have selected are the components of a homogeneous binary mixture. In the latter case, the saturation properties will already be
defined in the mixture definition, but you may still choose to override the Saturation Pressure by
specifying it on the Fluid Pairs tab.
When initializing the domain, set the volume fraction of vapor to zero and the volume fraction of liquid
to unity. These settings (represented by the Automatic setting for Volume Fraction) are used by
default in CFX.
Set up the problem with one of the following boundary condition combinations:
1.
Inlet total pressure and outlet mass flow (recommended)
2.
Inlet velocity profile and outlet static pressure
The inlet boundary condition should specify that the volume fraction of vapor is zero.
Turbulence models should be chosen as usual (for example, k-epsilon or SST). For turbulence induced
cavitation, consider using the DES model.
For advection scheme, use high resolution, or a specified blend factor of unity.
If editing a material, remember that the vapor pressure is on an absolute scale; it does not depend on
the specified reference pressure.
Cavitation models cannot be combined with other types of interphase mass transfer, such as thermal
phase changes.
7.1.5. Convergence Tips
If performing a single solution, initially turn off cavitation, then turn on cavitation and use the first set
of results as an initial guess.
If performing a series of simulations using one solution to initialize the next, solve the cases in order
of decreasing pressure (for example, approaching cavitation).
7.1.6. Postprocessing
A contour plot of volume fraction for the vapor can show where cavitation bubbles exist.
To calculate the inlet and outlet pressures, use the function calculator.
110
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 8: CFX Best Practices Guide for Combustion
This guide is part of a series that provides advice for using CFX in specific engineering application areas.
It is aimed at users with moderate or little experience using CFX for applications involving combustion.
This guide describes:
• Gas Turbine Combustors (p. 111)
• Combustion Modeling in HVAC Cases (p. 113)
8.1. Gas Turbine Combustors
Gas turbines are widely used in stationary and aircraft applications. The combustor receives the working
fluid in a compressed state, burns fuel to increase its temperature, and passes it to the turbine. One of
the key design goals for the combustor is to achieve a stable combustion process. Another key design
goal is to minimize the emission of pollutants, particularly oxides of nitrogen.
8.1.1. Setup
8.1.1.1. Steady-state vs. Transient
Most simulations are steady-state, particularly for stationary gas turbines that operate at a constant
load.
8.1.1.2. Turbulence Model
The
turbulence model is used in many applications, but the SST model should be considered for
flows with separated boundary layers, and the Reynolds stress model is the best choice for highly
swirling flows.
8.1.1.3. Reference Pressure
Because of the high inlet pressure, a reference pressure between 4 and 20 atmospheres is common,
and depends upon the type of simulation you are running.
8.1.1.4. Combustion Model
The choice of combustion model depends of whether the fuel/oxidant combination is premixed. The
following table outlines some of the differences.
Premixed Combustion
Non-Premixed Combustion
Commonly used for recent stationary gas
turbines in power generation.
Typically used for flight engines because it is
easier to control variable operating
conditions.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
111
CFX Best Practices Guide for Combustion
Premixed Combustion
Non-Premixed Combustion
Combustion Models: EDM with product limiter
and/or extinction submodels, FRC/EDM
combined, Partially Premixed (Turbulent Flame
Speed Closure (TFC))
Combustion Models: EDM, FRC/EDM
combined, Flamelet (and, for some cases, also
the Premixed model).
Note that the EDM model usually needs
adjusting for premixed combustion (for example,
extinction by temperature or by mixing/chemical
time scales).
For the preliminary analysis of high speed turbulent flow, the Eddy Dissipation combustion model is a
sensible choice, but cannot simulate burning velocities or flame position.
The Laminar Flamelet model is applicable for turbulent flow with non-premixed combustion, and
provides a robust solution at a low computational expense for multi-step reactions. The Flamelet
model uses a chemistry library, meaning that only two additional transport equations are solved to
calculate multiple species. As a result, the Flamelet model is a very good choice for modeling the
formation of various pollutants during the combustion process. The Flamelet model predicts incomplete
combustion to some extent (CO in exhaust gas), which helps to predict reduction in temperature (unlike
EDM).
8.1.2. Reactions
During the initial analysis of a combustor, the highest values of temperature and outgoing heat flux
are likely to be of primary concern. For this purpose, a single-step Eddy Dissipation reaction can be
used. Such a reaction is likely to overpredict the temperature, and will not predict emissions correctly,
but can provide a conservative indicator of the expected temperature levels.
Other reaction steps might then be added to the simulation to account for the formation of combustion
byproducts. Each reaction step has its own separate time scale. As a result, convergence can become
very difficult when a multi-step reaction contains more than about 5 steps.
8.1.3. Convergence Tips
The Equation Class Settings tab in CFX-Pre can be used to set different advection schemes and time
scales for each class of equation you are solving. For multi-step Eddy Dissipation reactions, convergence
can be improved by temporarily increasing the mass fraction time scale by a factor of about 5-10.
For the Eddy Dissipation Model, multistep convergence can be aided by first running a simplified singlestep simulation and using the results from the run as an initial values file for a multi-step run.
You may restart a Flamelet model from a cold solution. You should avoid restarting with the Flamelet
model from an EDM solution. You may restart an EDM case from a Flamelet model solution.
The High Resolution advection scheme is always recommended for combustion simulations because it
is bounded and prevents over/undershoots. Care must be taken, however, to provide a mesh of sufficient
quality to resolve most of the flow features. A very poor mesh will result in the scheme using a blend
factor close to zero (therefore not providing a solution as accurate as expected).
For simulations that include Finite Rate Chemistry, small temperature variations can result in large
changes in reaction rate. When a solution is converging, temperature values may change sufficiently
112
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Combustion Modeling in HVAC Cases
to make the solution unstable. To aid convergence, add a TEMPERATURE DAMPING CCL structure
within a SOLVER CONTROL block, as follows:
FLOW:
SOLVER CONTROL:
TEMPERATURE DAMPING:
Option = Temperature Damping
Temperature Damping Limit = <Real number>
Under Relaxation Factor = <Real number>
END
END
END
Depending on the location of the SOLVER CONTROL block, the temperature damping may be applied
to a particular domain or phase. Set the Temperature Damping Limit to 0 so that positive
damping is always applied. The Under Relaxation Factor can be set to multiply changes in
temperature by a value between 0 and 1. You should try a factor of 0.2 if you are having trouble converging a solution.
8.1.4. Postprocessing
Some of the most common plots to create in CFD-Post include:
• Mass Fractions: fuel, O2, products, intermediate species (CO), pollutants (NO)
• Turbulent Mixing Time Scale (Eddy Dissipation / Turbulent Kinetic Energy)
• Reaction Rates
The variable "<my reaction>.Molar Reaction Rate" is available for every "Single Step" reaction (EDM,
FRC or combined model).
• Plots of the turbulent Damköhler number (the ratio of the turbulent time scale to the chemical time scale)
8.2. Combustion Modeling in HVAC Cases
This section deals with the setup of combustion cases for HVAC simulations, where it is important to
accurately model the combustion process. Such processes are known as "combusting fire" simulations,
as opposed to "inert fire" simulations.
Using a combusting fire simulation is the most accurate way to model fires in all HVAC cases. It is particularly important in cases when the fire is under-ventilated, or when the ventilation cannot be easily
predicted. The drawback is the additional computational expense involved in solving a full combustion
model as part of the main solution.
8.2.1. Set Up
Most simulations are set up as transient. The choice of timestep is generally model dependent, but will
usually fall into the range 0.5 s to 2 s. The Total Energy heat transfer model should be selected to fully
model buoyancy.
Note
When modeling buoyancy, it is very important to correctly specify the buoyancy reference
density when opening boundary conditions are used.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
113
CFX Best Practices Guide for Combustion
The RNG
turbulence model is a good choice for combusting flows, with either no buoyancy terms
in equations or buoyancy terms in both the equations (with C3=1). The SST model is also reasonable,
but may not converge well for natural convection. The SSG model is accurate, but convergence may
be very slow.
The most common fuels used are hydrocarbons such as methane, diesel and petroleum. Cellulosic materials, plastics and wood are also used. The simulation will dictate the type of materials to use as a
fuel.
The Eddy Dissipation Model is widely used, combined with an Additional Variable for toxins. The
flamelet model is more rigorous, and is a better choice when the fire is under ventilated.
8.2.2. Convergence Tips
Convergence can be slowed if care is not taken in the setup of buoyancy and openings.
The presence of an instantaneous fuel supply is sometimes not physical, and can slow convergence. In
many transient cases, the amount of fuel available can be controlled by using time-dependent expressions.
8.2.3. Postprocessing
The most common parameters of interest in a combusting fire model are simulation-dependent, but
will usually include one of more of the following:
• Temperature
• Products (including carbon monoxide and other toxins)
• Visibility
• Wall Temperature
• Wall convective and radiative heat fluxes
114
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 9: CFX Best Practices Guide for HVAC
This guide discusses best practices for setting up, solving, and postprocessing an HVAC simulation:
9.1. HVAC Simulations
9.2. Convergence Tips
This guide is part of a series that provides advice for using CFX in specific engineering application areas.
It is aimed at users with moderate or little experience using CFX for HVAC1 applications.
9.1. HVAC Simulations
HVAC studies range in scale from single components (such as a radiator) to large and complicated systems
(such as a climate control system for a large building).
Physical processes that are commonly modeled in HVAC simulations include:
• Buoyancy
• Thermal radiation
• Conjugate heat transfer (CHT) between fluids and solids.
Typical HVAC systems include the following components:
• Heating/cooling units such as furnaces, heaters, air conditioners, and radiators
• Fans/pumps
• Thermostats.
9.1.1. Setting Up HVAC Simulations
This section discusses how to set up various physical processes, CFD features, and components involved
in HVAC simulations.
9.1.1.1. Buoyancy
Most HVAC cases involve flow that is affected by buoyancy. Buoyancy can be activated on the Basic
Settings tab of the Domain details view.
Two buoyancy models are available: Full and Boussinesq. These models are automatically selected according to the properties of the selected fluid(s).
• The Full buoyancy model is used if fluid density is a function of temperature and/or pressure (which includes
all ideal gases and real fluids). In this case, a Buoyancy Reference Density must be set as the expected average
density of the domain.
1
HVAC is a reference to Heating, Ventilation (or Ventilating), and Air Conditioning. Often, it is also used as a reference to refrigeration.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
115
CFX Best Practices Guide for HVAC
• The Boussinesq model is used if fluid density is not a function of temperature or pressure. In this case, a
Buoyancy Reference Temperature must be set as the expected average temperature of the domain.
When fluid properties are functions of pressure, the absolute pressure is used to evaluate them. The
calculation of absolute pressure requires a Buoyancy Reference Location to be defined, preferably by
specifying coordinates.
When modeling fire, it is recommended that you choose a compressible fluid because density variations
will be significant. An incompressible fluid should be chosen only if density variations are small (a few
percent or less).
9.1.1.2. Thermal Radiation
To set the radiation model for a fluid domain, visit the Fluid Models panel for that domain and set the
following:
9.1.1.2.1. Thermal Radiation Model
For HVAC studies, select either Monte Carlo or Discrete Transfer. If directed radiation is to be modeled,
Monte Carlo must be used.
9.1.1.2.2. Spectral Model
Select either Gray or Multiband. Spectral bands are used to discretize the spectrum and should therefore
be able to adequately resolve all radiation quantities that depend on wavelength (or frequency or wave
number). For HVAC, two bands will usually suffice.
9.1.1.2.3. Scattering Model
A scattering model should not be used if you are modeling clear air. The isotropic scattering model
should be used if you are modeling air that contains dust or fog.
To set up radiation for a solid domain, visit the Solid Models panel for that domain (each solid domain
must be set up separately). The only radiation model available for solid domains is Monte Carlo.
Note
If any solid domain uses the Monte Carlo radiation model (that is, if it uses radiation at all),
then all fluid domains using a radiation model must use the Monte Carlo model.
The material used in a domain that transmits radiation has radiation properties that specify Absorption
Coefficient, Scattering Coefficient, and the Refractive Index. These properties may be edited in the
Materials details view.
Note
Radiation modeling cannot be used with Eulerian multiphase simulations.
Thermal radiation properties are specified on the Boundary Details panel for each boundary of a domain
that transmits radiation. For opaque surfaces, the properties that must be specified are: Emissivity and
Diffuse Fraction. For inlets, outlets, and openings, you may specify either the Local Temperature or
an External Blackbody Temperature.
116
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
HVAC Simulations
The Monte Carlo and Discrete Transfer models allow radiation sources to be specified on the Sources
panel for any subdomain or wall boundary. For subdomains, radiation sources per unit volume are
specified; for boundaries, radiation fluxes are specified. Radiation sources may be directed or isotropic.
Multiple isotropic sources and up to one directed source may be specified for any given wall boundary
or subdomain.
Material properties related to radiation, thermal radiation properties for boundaries, and source strengths
can be specified as expressions that depend on one or more of the built-in variables: Wavelength in
Vacuum (or wavelo), Frequency (or freq), Wavenumber in Vacuum (or waveno).
A domain representing an opaque solid should not have a radiation model set. The boundaries of radiation-transmitting domains that interface with such a solid domain should be specified as opaque.
External windows of a room can be modeled as solid domains which interface with the room (air) domain;
they may also be modeled as an external boundary of the room domain. In either case, the exterior
boundary must be modeled as an opaque wall. A diffuse and a directed radiation source emitted from
the opaque surface can be used to simulate sunlight. In order to simulate the motion of the sun, the
direction vector for directed radiation can be specified by CEL expressions that depend on time (t).
Radiation escaping through a window can be modeled by specifying a non-zero emissivity (to cause
radiation absorption) and either:
• Specifying a heat transfer coefficient via a CEL expression that accounts for the thermal energy lost
• Specifying a fixed wall temperature.
When using solid domains that transmit radiation, a spectral radiation model is recommended. If a
simulation contains no solid domains that transmit radiation, a gray radiation model can be used for
rough calculations but a spectral model should be used for more detailed modeling.
9.1.1.3. CHT (Conjugate Heat Transfer) Domains
CHT domains are solid domains that model heat transfer. In CFX, all solid domains must model heat
transfer, and are therefore CHT domains. If you do not want to model heat transfer in a particular region,
do not assign the mesh for that region to any domain.
Boundaries between domains that model heat transfer have temperatures and thermal fluxes calculated
automatically, and should not have thermal boundary conditions specified. External boundaries (which
can represent solids that are not explicitly modeled) require the specification of a thermal boundary
condition.
Boundary conditions other than thermal boundary conditions (for example, wall roughness) may be
specified on the boundaries of a fluid domain that interface with a solid domain.
Sources of thermal energy and/or radiation can be added to a subdomain of a CHT domain.
9.1.1.4. Mesh Quality
Ensure that wall boundary layers have adequate mesh resolution. This is important regardless of the
type of wall heat transfer: adiabatic, specified temperature, specified heat flux, or heat transfer coefficient.
The mesh resolution in a boundary layer affects the prediction of convective heat transfer and the
temperature gradient near the wall. For walls without a specified temperature, the temperature gradient
near the wall affects the calculated wall temperature and, consequently, the amount of radiation emitted
(provided that the emissivity of the wall is non-zero).
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
117
CFX Best Practices Guide for HVAC
9.1.1.5. Fans
Fans should be represented by momentum sources if they are embedded in the domain. Fans can also
be represented by an inlet or outlet boundary condition or both.
9.1.1.6. Thermostats
A Thermostat can be defined using a User Fortran routine. Refer to Air Conditioning Simulation in the
CFX Tutorials for details.
9.1.1.7. Collections of Objects
If your HVAC simulation models a large number of people/equipment/items, consider volumetric sources
of heat, CO2, and resistances.
9.2. Convergence Tips
Buoyancy and coupling between the relevant equations often make convergence difficult. Smaller
timesteps may help convergence.
118
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 10: CFX Best Practices Guide for Multiphase
This guide is part of a series that provides advice for using CFX in specific engineering application areas.
It is aimed at users with moderate or little experience using CFX for applications involving multiphase
flows.
In the context of CFX, a multiphase flow is a flow composed of more than one fluid. Each fluid may
possess its own flow field, or all fluids may share a common flow field. Unlike multicomponent flow1,
the fluids are not mixed on a microscopic scale; rather, they are mixed on a macroscopic scale, with a
discernible interface between the fluids. CFX includes a variety of multiphase models to allow the simulation of multiple fluid streams, bubbles, droplets, and free surface flows.
This guide describes:
• Bubble Columns (p. 119)
• Mixing Vessels (p. 120)
• Free Surface Applications (p. 121)
• Multiphase Flow with Turbulence Dispersion Force (p. 122)
10.1. Bubble Columns
Bubble columns are tall gas-liquid contacting vessels and are often used in processes where gas absorption is important (for example, bioreactors to dissolve oxygen in broths) and to limit the exposure of
micro-organisms to excessive shear imparted by mechanically driven mixers. There are two types of
bubble columns in general use: airlift reactors that use a baffle to separate the riser and downcomer
regions, and other columns that do not use a baffle.
10.1.1. Setup
The choice of a steady-state or transient simulation depends on the type of simulation you want to
analyze. For example, an analysis using a steady-state simulation is often satisfactory for monitoring
global quantities. A transient simulation can be used to observe transient effects, such as recirculation
zones.
Most bubble columns use two fluids: one continuous fluid and one dispersed fluid. The
model is
typically used in the continuous fluid, and the dispersed phase zero equation is used for the dispersed
phase.
Non-drag forces become less significant with increasing size of the bubble column. For smaller columns,
non-drag forces may be significant.
The Grace drag model is recommended, especially for modeling air/water.
1
Note that a fluid in a multiphase flow may be a multicomponent mixture.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
119
CFX Best Practices Guide for Multiphase
A degassing boundary condition is generally employed at the top of the bubble column. The degassing
boundary behaves as an outlet boundary to the dispersed phase, but as a wall to the continuous phase.
A reasonable estimate of the time scale is given by a factor of the length of the domain divided by the
velocity scale (for example, 0.5 * L/U).
10.1.2. Convergence Tips
Sometimes, physical instabilities (such as recirculation zones) can result in slow or stalled convergence.
In these cases, you can still obtain an indicator of convergence for a global quantity by creating a
monitor point at some point in the domain. As a result, you can determine whether values for selected
global quantities (such as gas hold-up) are meaningful.
10.1.3. Postprocessing
The main design objective for bubble columns is efficient mixing, which is strongly influenced by the
dispersed phase. Mixing efficiency can be measured in a number of ways. One example is to measure
the gas hold-up in the riser as a function of the superficial gas velocity. This would require solving for
the gas volume fraction for a number of simulations, each with a different mass flow rate of the dispersed
phase at the sparger. Another option would be to use the same input parameters, this time measuring
the liquid velocity in the downcomer.
10.2. Mixing Vessels
Mixing vessels are widely used in the chemical industry to optimize mixing and/or heat transfer between
fluids. Mixing must be efficient, precise and repeatable to ensure optimum product quality. Quantities
of interest may include mixing times, gas hold-up, power draw, local shear and strain rates, and solids
distribution. The application of Computational Fluid Dynamics to address these needs results in faster
and lower cost design through reduced experimentation, more reliable scale-up, and better understanding
of the processes, leading to higher yields and reduced waste.
10.2.1. Setup
Mixing vessels generally use two domains. The impeller domain is a small, rotating domain that encloses
the impeller. The rest of the tank is represented by a stationary domain. Different types of domain interfaces are available for the connection between the stationary and the rotating domains. The recommended types are:
• Frozen Rotor: faster but cruder
• Transient: slower (transient analysis) but much more accurate
The choice of a steady-state or transient simulation is dependent on the type of interface that exists
between the two domains. Where a Frozen Rotor interface is used, a steady-state simulation is usually
carried out. Performing a transient simulation allows you to use the transient rotor/stator frame change
model to account for transient effects.
The initial guess for velocity can be set to zero in the relative frame for each domain.
120
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Free Surface Applications
10.3. Free Surface Applications
Free Surface flow refers to a multiphase situation where the fluids (commonly water and air) are separated
by a distinct resolvable interface. Such flows occur, for example, around the hull of a ship, or in a
breaking wave.
10.3.1. Setup
The choice of using a steady-state or transient simulation is problem-dependent. There are two models
available for free surface flow: homogeneous and inhomogeneous. The homogeneous model can be
used when the interface between the two phases remains well defined and none of the dispersed phase
becomes entrained in the continuous phase. An example of homogeneous free surface flow is flow in
an open channel. A breaking wave is one example of an inhomogeneous flow case.
The same choice of turbulence model as for single phase simulations is appropriate. When using the
inhomogeneous model, you should use the homogeneous turbulence option in CFX-Pre. The Buoyancy
Reference Density should be set to the density of the least dense fluid.
When setting boundary conditions, the volume fractions can be set up using step functions to set the
liquid height at each boundary. An outlet boundary having supercritical flow should use the Supercritical option for Mass And Momentum. This requires that you set the relative pressure of the gas above
the free surface at the outlet.
For most free surface applications, the initial conditions can use step functions to set the volume fractions
of the phases as a function of height. The initial condition for pressure should be set to hydrostatic
conditions for the specified volume fraction initialization and the buoyancy reference density.
The timestep for free surface flows should be based on a L/U (Length/Velocity) scale. The length scale
should be a geometric length scale. The velocity scale should be the maximum of a representative flow
velocity and a buoyant velocity, which is given by:
In addition, it is sometimes helpful to reduce the timestep for the volume fraction equations by an order
of magnitude below that of the other equations.
10.3.2. Convergence Tips
The interface between the liquid and gas phase can sometimes become blurry. This could be due to
physical properties (such as a breaking wave or sloshing in a vessel). Where the dispersed phase becomes
entrained in the continuous phase, the inhomogeneous model is a better choice.
A technique to increase the mesh density in the region of a liquid-gas interface is to create a subdomain
that occupies the same region as the liquid (or gas) phase, and inflate the mesh in both directions from
the edge of the subdomain, as shown in Figure 10.1: An exaggerated view of three inflation layers on
each side of the uppermost subdomain boundary surface. (p. 122). The inflation layers can increase the
resolution in the region of the interface and enhance the results.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
121
CFX Best Practices Guide for Multiphase
Figure 10.1: An exaggerated view of three inflation layers on each side of the uppermost
subdomain boundary surface.
10.4. Multiphase Flow with Turbulence Dispersion Force
For Release 14, in order to reduce convergence difficulties encountered in some multiphase flow
problems, the value of the expert parameter ggi ap relaxation is multiplied internally by 0.75.
This occurs in the following situation only:
• Multiphase flow
• Nontrivial turbulence dispersion force included
• Coupled volume fraction solution algorithm.
In this situation, the default value of 1.0 is converted internally to 0.75. If you override the default with
a smaller value, the new value is also multiplied internally by 0.75. This ensures that you retain some
control over this parameter. The above restrictions ensure that the numerics changes are focused on a
narrow range of problems and do not deteriorate convergence of other classes of problems.
122
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 11: CFX Best Practices Guide for Turbomachinery
Turbomachinery applications can generally be divided into three main categories: gas compressors and
turbines, liquid pumps and turbines, and fans and blowers. Each category is discussed in a separate
section below.
This guide describes best practices for setting up simulations involving:
11.1. Gas Compressors and Turbines
11.2. Liquid Pumps and Turbines
11.3. Fans and Blowers
11.4. Frame Change Models
11.5. Domain Interface Setup
11.6.Transient Blade Row
This guide is part of a series that provides advice for using CFX in specific engineering application areas.
It is aimed at users with moderate or little experience using CFX for applications involving turbomachinery.
11.1. Gas Compressors and Turbines
This section describes:
• Setup for Simulations of Gas Compressors and Turbines (p. 123)
• Convergence Tips (p. 124)
• Computing Speedlines for a Machine (p. 124)
• Postprocessing (p. 125)
11.1.1. Setup for Simulations of Gas Compressors and Turbines
Heat transfer and viscous work are involved, and can be modeled by using the Total Energy heat
transfer model and enabling the Viscous Work Term option in CFX-Pre.
The industry-standard Shear Stress Transport model is the recommended choice for these cases. When
using the Shear Stress Transport model, ensure a resolution of the boundary layer of more than 10
points. For details, see The k-omega and SST Models in the CFX-Solver Modeling Guide.
A common boundary condition configuration is to specify the total pressure and total temperature at
the inlet and either the mass flow, exit corrected mass flow, or static pressure at the outlet, depending
on the flow condition. Other configurations are also commonly used.
A good estimate of the timestep is within the region
to
, where is the angular velocity
of the rotating domain in radians per second. Selecting an automatic timestep will result in a timestep
of
.
The second-order high-resolution advection scheme is generally recommended.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
123
CFX Best Practices Guide for Turbomachinery
11.1.2. Convergence Tips
For high speed compressors and turbines, where the machine mass flow is choked, it is generally not
possible to specify the specified mass flow at the outlet to match the numerical choked mass flow value.
For choked flow conditions, you can either specify static pressure or exit corrected mass flow at the
outlet. Both these conditions allow the mass flow through the machine to adjust to the numerical
choked mass flow value.
If you have trouble converging a simulation involving real gases, try to obtain a solution first using an
ideal gas. Ideal gases are available in the real gas library.
If you have trouble converging a problem with many stages, you may find that solving for a reduced
number of stages can give you a better understanding of the physics, and may allow you to restart a
multi-stage problem with a better initial guess. You can also try ramping up boundary conditions and
the RPM.
Low pressure ratio Gas compressors (1.1 or less) can be treated more like liquid pumps. For details, see
Liquid Pumps and Turbines (p. 126).
11.1.3. Computing Speedlines for a Machine
Most turbomachinery simulations examine the machine performance across a range of operating points.
A speedline involves varying the mass flow rate from choke to stall at a fixed rotational speed. This is
often accomplished by varying the exit mass flow rate or exit pressure while maintaining a constant,
stationary frame total temperature and pressure at the inlet. If total conditions are not maintained at
the inlet, the resulting inlet mass flow rate must be corrected to a standard reference condition.
Performance along a speedline is typically measured in terms of a pressure ratio and an efficiency. A
full performance map is obtained by examining the performance across a range of rotation rates; that
is, multiple speedlines. A plot containing multiple speedlines is called the performance map of the machine. Computing speedlines and performance maps requires many individual computations (one per
mass flow), therefore it is desirable to automate the process.
Depending on the machine type, you can use the following boundary conditions to effectively compute
speedlines:
• For low speed compressors and turbines (subsonic), liquid pumps: Specify Total Pressure and Temperature
at the inlet and a Mass Flow Rate condition or a Exit Corrected Mass Flow Rate condition at the
outlet. This enables you to easily vary the mass flow across the full speedline while maintaining stationary
inlet total conditions. For compressors, the specification of the mass flow rate at the outlet is essential
towards the low flow end of a speedline where the machine pressure ratio is insensitive to the mass
flow rate. For this reason, you should not specify a Static Pressure condition at the outlet boundary
for these machines.
• For high speed turbines and compressors (transonic): In these machines, the mass flow through the system
is limited by a choked condition. If the specifed exit mass flow exceeds the choke flow rate, the net
mass downstream of the choke condition will decrease until it reaches zero density, causing the solver
to fail. It is therefore important to avoid an exit mass flow near choke.
Similarly, at lower mass flow rates, close to stall, the pressure ratio is either constant or decreasing.
A pressure specified outlet is generally unstable in this regime because there are multiple mass
flow rates that may satisfy the outlet condition. Therefore a pressure boundary condition should
be avoided in this range.
124
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Gas Compressors and Turbines
This presents a problem with running speedlines using pressure and mass flow conditions, because
neither boundary condition can be used across the entire speedline.
While the exit pressure and mass flow rate may be asymptotic over portions of a speedline, the
exit corrected mass flow remains non-asymptotic and is therefore applicable across the entire
operating range. Thus, it is recommended that you use the Exit Corrected Mass Flow Rate
outlet boundary condition for running speedlines.
Some advantages of using the Exit Corrected Mass Flow Rate outlet boundary condition are:
• It allows you to specify the exit corrected mass flow, which is a function of the outlet mass flow rate, total
conditions, and a user-supplied reference condition.
• It makes it possible to automate the speedline analysis by enabling you to specify one boundary condition
type that functions well across the entire speedline.
• It improves stability when a run is started with poor initial conditions, allowing for the use of a much larger
timescale factor, so that all runs can be started from a simple or automatic initial guess. This allows points
along the speedline to be computed independently rather than using each existing solution to initialize the
next.
• Typically in compressor operations, a fixed value of Exit Corrected Mass Flow Rate represents a fixed running
or “op” line. As a result, you could keep the Exit Corrected Mass Flow Rate boundary condition fixed and
vary the rotational speed to generate the compressor performance along an op line. This is useful when
comparing designs.
For more details on the mathematical treatment of exit corrected mass flow rate as an outlet boundary
condition, see Exit Corrected Mass Flow Rate in the CFX-Solver Theory Guide.
11.1.4. Postprocessing
CFD-Post offers a powerful array of postprocessing tools for turbomachinery applications, including
turbo-specific plots and performance calculation macros. To use many of the Turbo Post tools, you must
first initialize each domain by specifying the locations of turbo regions and instancing information.
The Turbo Calculator from the Turbo menu in CFD-Post allows you to perform calculations on the type
of application you are modeling. The macro prints a report in HTML showing a number of calculated
variables, including torque, head and flow coefficients, blade loading, and efficiency.
You can also create your own macros to customize postprocessing using Power Syntax, which is based
on the Perl language.
The optimal performance characteristics can be determined by creating a curve of pressure ratio versus
flow rate.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
125
CFX Best Practices Guide for Turbomachinery
Figure 11.1: Flow Rate vs Pressure Rise for a Gas Compressor
In Figure 11.1: Flow Rate vs Pressure Rise for a Gas Compressor (p. 126), Region 1 shows an area where
a large change in mass flow rate represents a small change in pressure rise. When modeling flow in
this region, a mass flow rate specified outlet is better than a pressure specified outlet. Region 2 shows
an area where a small change in flow rate represents a large pressure variation. This region is close to
“choking”, and a pressure-specified or exit corrected mass flow rate outlet is the best choice. For details,
see Convergence Tips (p. 124).
CFD-Post provides a performance macro for gas compressors and turbines.
11.2. Liquid Pumps and Turbines
This section describes:
• Setup for Simulations of Liquid Pumps and Turbines (p. 126)
• Convergence Tips (p. 127)
• Postprocessing (p. 127)
11.2.1. Setup for Simulations of Liquid Pumps and Turbines
Heat transfer is not significant in most cases, so the heat transfer option can be set to None in CFX-Pre.
The
and Shear Stress Transport models are appropriate choices for modeling turbulence. When
using the Shear Stress Transport model, ensure a resolution of the boundary layer of more than 10
points. For details, see The k-epsilon Model in the CFX-Solver Modeling Guide.
When setting boundary conditions, a total pressure specified inlet and a mass flow outlet are a recommended practice. The total pressure inlet condition is often more appropriate than the uniform velocity
or massflow inlet condition for cases that assume that the machine is drawing fluid directly from a
static reservoir.
126
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Fans and Blowers
As with gas compressors, a good estimate of the timestep is within the region
to
, where
is the angular velocity of the rotating domain in radians per second. Selecting an automatic timestep
will result in a timestep of
.
The high-resolution advection scheme is recommended.
This document deals with obtaining solutions for cases without cavitation, but cavitation may be present.
For advice on how to deal with cavitation, see CFX Best Practices Guide for Cavitation (p. 107).
11.2.2. Convergence Tips
When only a poor initial guess is available, it may be helpful to first run with a specified mass flow inlet
and a static pressure outlet. The outlet pressure in this case is fairly arbitrary and is usually set at, or
close to zero to reduce round-off error. The specification of a mass flow inlet may be more robust.
However, a mass flow inlet assumes a uniform inlet velocity—which may not be appropriate. Once the
overall flow is established, the boundary conditions may then be changed to total pressure at the inlet
and mass flow at the outlet.
11.2.3. Postprocessing
If a total pressure inlet boundary condition is used (recommended where possible), it will also provide
a useful starting point for streamlines that are colored by total pressure during postprocessing. The
uniform total pressure distribution means lines will begin with a uniform color. It may be harder to
visually resolve these pressure values if an inlet velocity profile is used.
CFD-Post provides a performance macro for liquid pumps and turbines.
11.3. Fans and Blowers
This section describes:
• Setup for Simulations of Fans and Blowers (p. 127)
• Convergence Tips (p. 127)
• Postprocessing (p. 128)
11.3.1. Setup for Simulations of Fans and Blowers
Fans and blowers behave like liquid pumps, and require a similar model setup. The flow is generally
modeled as incompressible and isothermal. The fluid is typically air as a general fluid or as an ideal gas
at a specified temperature. The
or SST model is used to model turbulence.
Boundary conditions, turbulence models and choice of timestep are the same as for liquid pumps and
turbines.
11.3.2. Convergence Tips
The use of the alternate rotation model is an important consideration when modeling fans and blowers.
Where long axisymmetric inlets exist, the absolute frame velocity has less swirl than the relative frame
velocity. Because the alternate rotation model solves for the absolute frame velocity, it can reduce numerical error in such inlet sections. The model may introduce errors in the exit stream if the flow is
highly swirling. Hence, the length of the inlet and exit sections can be an important factor when
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
127
CFX Best Practices Guide for Turbomachinery
choosing whether to implement the model. The alternate rotation model is generally recommended,
especially for axial fans. In most realistic flow situations, this model reduces (or at least will not increase)
numerical errors.
Air foil drag is significant and boundary layer friction is an important modeling issue for fans and blowers.
A good resolution of the boundary layer, requiring a high concentration of nodes close to the blade
surfaces, is therefore important. The Shear Stress Transport model can provide relatively accurate results
where the boundary layer is sufficiently resolved by the mesh.
11.3.3. Postprocessing
A similar postprocessing approach to pumps and turbines is also useful for fans and blowers. For details,
see Postprocessing (p. 127). See the following figure for a plot of flow rate vs pressure rise for a blower.
11.4. Frame Change Models
When specifying domain interfaces in CFX-Pre, you must select the type of analysis that will be carried
out in the solver. The choices are:
• Frozen Rotor (p. 128)
• Stage (p. 129)
• Transient Rotor-Stator (p. 129)
11.4.1. Frozen Rotor
The Frozen Rotor model treats the flow from one component to the next by changing the frame of
reference while maintaining the relative position of the components. Usually, periodicity is used to reduce
the number of components to a subset that has approximately the same pitch ratio as the full geometry.
To account for differences in pitch ratio between the subset and the full geometry, the flow passing
through the interface is scaled according to the net pitch ratio of the subsets.
128
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Domain Interface Setup
The Frozen Rotor model must be used for non-axisymmetric flow domains, such as impeller/volute,
turbine/draft tube, propeller/ship and scroll/volute cases. It can also be used for axial compressors and
turbines. The Frozen Rotor model has the advantages of being robust, using less computer resources
than the other frame change models, and being well suited for high blade counts. The drawbacks of
the model include inadequate prediction of physics for local flow values and sensitivity of the results
to the relative position of the rotor and stator for tightly coupled components.
11.4.2. Stage
The Stage model circumferentially averages the fluxes in bands and transmits the average fluxes to the
downstream component. Possible applications include axial turbines, compressors and pumps, as well
as fans and torque converters. The model is useful for large pitch ratios and still takes a relatively short
time to solve. The model is not suitable for applications with tight coupling of components and/or
significant wake interaction effects and may not accurately predict loading.
11.4.3. Transient Rotor-Stator
The Transient Rotor-Stator model takes into account all of the transient flow characteristics. A sliding
interface is used to allow a smooth rotation between components. As with the Frozen Rotor model, the
Transient Rotor-Stator model scales the flow from one component to the next in order to account for
a non-unity net pitch ratio. This model is robust and yields high accuracy predictions of loading. The
drawbacks include high computational cost and large amounts of storage required to hold the transient
data.
Note
The dynamic re-intersection of the interface at the start of each time step may result in a
different interface topology, which in turn may require more or less memory. Unlike the
static interfaces (Frozen Rotor, Stage), which are only intersected once (first time step of a
serial run or partitioner in a parallel run), the initial memory estimate might not be sufficient
for the whole run. To avoid potential memory problems, it might be necessary to start the
simulation with more conservative (larger) memory factors.
11.5. Domain Interface Setup
The setup of domain interfaces is an important consideration when defining a problem. The following
section outlines some approved practices for use in turbomachinery applications.
11.5.1. General Considerations
• Domain interfaces should typically be placed midway between the rotor and stator for turbomachinery
cases.
• To avoid numerical errors, the aspect ratio of elements on the domain interface should be between 0.1:1
and 10:1, as measured by x/y in Figure 11.2: Element Aspect Ratio at Domain Interface (p. 130).
• Where circular domain interfaces exist, they must be axisymmetric in shape as shown in Figure 11.3: Impeller/Volute (p. 130).
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
129
CFX Best Practices Guide for Turbomachinery
Figure 11.2: Element Aspect Ratio at Domain Interface
11.5.2. Case 1: Impeller/Volute
A basic impeller/volute sketch is shown in Figure 11.3: Impeller/Volute (p. 130). The edge of the inner
circle shows the maximum extent of the impeller blades. A good practice here is to create the domain
interface halfway across the narrowest gap between the blade and volute wall. This usually occurs
around the cut-off or “tongue” illustrated in the diagram.
Figure 11.3: Impeller/Volute
11.5.3. Case 2: Step Change Between Rotor and Stator
For the case shown, there is a step change in the passage height between the rotor and stator. A
common choice for placement of the interface would be choice 1. However, take care with this setup
because the non-overlap regions of the interface should be specified as walls. A better alternative may
be to use a domain interface upstream or downstream of the step change, at position 2 or position 3.
130
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Domain Interface Setup
Figure 11.4: Possible Domain Interface Positions with Step Change in Passage Height
11.5.4. Case 3: Blade Passage at or Close to the Edge of a Domain
Figure 11.5: Radial Compressor (p. 132) shows a blade that extends to the edge of the rotating domain.
Although it is convenient to place a domain interface at the blade edge (1), this can result in unrealistic
results (The area of the interface would be reduced on one side where the interface is displaced by the
blade edge, resulting in an inaccurate pitch change calculation. Also, in the case of a stage interface,
the wake would be mixed out at the trailing edge.) A better arrangement is to extend the rotating domain
away from the blade edge. Domain Interfaces can then be created at (2), (3), and (4).
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
131
CFX Best Practices Guide for Turbomachinery
Figure 11.5: Radial Compressor
11.5.5. Case 4: Impeller Leakage
A close-up view of part of Figure 11.5: Radial Compressor (p. 132), which models flow leaking from a
volute back into the impeller region. To model the feature, you can use two domain interfaces (at positions 1 and 2), or a single domain interface downstream of the leak (position 3).
132
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Domain Interface Setup
Figure 11.6: Flow Leakage Through Gap Near Impeller Inlet
11.5.6. Case 5: Domain Interface Near Zone of Reversed Flow
Be wary of flow moving backwards across stage or frozen rotor interfaces. Because of the approximations
implied by these interfaces, flow moving upstream and downstream on the same interface will lead to
unphysical results. Try relocating the interface to prevent this from occurring.
As an example, Figure 11.7: Domain Interface Between Blade Rows in an Axial Machine (p. 134) shows
two blade rows of an axial machine with a frozen rotor interface between them. The flow moves from
left to right everywhere except in a small region just downstream of the trailing edge of the first row
of blades. In this case, the domain interface, shown as a dashed line, should be located to the right of
this region, as shown.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
133
CFX Best Practices Guide for Turbomachinery
Figure 11.7: Domain Interface Between Blade Rows in an Axial Machine
11.6. Transient Blade Row
This section describes the following topics:
11.6.1. Steady versus Transient Blade Row Analysis
11.6.2. Full Model Simulation versus Reduced Geometry Simulation (Pitch Change Models)
11.6.3. Selecting an Appropriate Transient Blade Row Model with Pitch Change
11.6.4. Convergence and Solution Monitoring of Transient Blade Row Flow Problems
11.6.5. Boundary Conditions in Blade Row Simulation
11.6.1. Steady versus Transient Blade Row Analysis
For many turbomachinery problems, steady-state stage simulations involving frame change/mixing
models such as Stage or Frozen Rotor, are sufficient to obtain machine performance and analyze flow
details. However, when turbomachine component interactions are strong due to close proximity or high
speed flow, transient blade row simulation become necessary to improve the prediction of turbomachine
aerodynamic performance.
A transient blade row simulation is also needed for aeromechanical (for example, flutter and forced response), aerothermodynamic (for example, hot streak analysis) and aeroacoustics analysis.
In general, a transient blade row analysis is more demanding on computer resources than a steadystate analysis.
11.6.2. Full Model Simulation versus Reduced Geometry Simulation (Pitch
Change Models)
To reduce costs (CPU & memory) of a transient blade row simulation, you can model a turbomachinery
flow on a small sector of the machine and apply a pitch change model (such as Profile Transformation,
Time Transformation or Fourier Transformation) to account for the difference in pitch between blade
rows.
In general, the transient blade row simulation becomes more efficient on the small sector model with
respect to the full wheel model as the number of blade counts in the original machine increases. For
example, in some cases it is better to do a transient blade row simulation on a full wheel rather than
134
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Transient Blade Row
a reduced geometry with pitch change models if the blade count is very small. Axial machines can have
a large number of blades per row (for example, 100 blades or more) so the cost savings with transient
blade row methods can be very large (of the order of 100x for such a machine). For radial machines,
the blade count is typically much smaller (for example, 5-20 blades) resulting in reduced potential cost
savings for the pitch change models.
11.6.3. Selecting an Appropriate Transient Blade Row Model with Pitch Change
ANSYS CFX provides a variety of transient blade row pitch change models to be used on a diverse range
of turbomachinery flow problems:
11.6.3.1. Profile Transformation
11.6.3.2.Time Transformation
11.6.3.3. Fourier Transformation
11.6.3.1. Profile Transformation
The Profile Transformation method should be used to predict performance and improve on steady-state
stage simulations. It can be used to capture the strong interactions between components.
The Profile Transformation method can be used for single-stage or multistage machines for all flow
physics including liquids and gases, at any range of Mach number.
The Profile Transformation method can be used on small to moderate pitch-ratio configurations. There
is no formal limit on the pitch ratio for the Profile Transformation method, but the model error grows
proportionally with the pitch ratio between components. For large pitch-ratio modeling, the error can
be minimized by adding more than one blade passage per row to reduce the pitch ratio of the ensemble.
The Profile Transformation method can also be mixed freely with stage interfaces, as well as with the
Time Transformation method, making it a highly useful and flexible approximation.
11.6.3.2. Time Transformation
The Time Transformation method should be used to predict both performance and blade passing frequency.
For small to moderate pitch-ratios (0.75-1.4), usually one blade passage per row is needed. However,
this pitch-ratio range can be substantially reduced for a very low rotation machine. If stability of the
method is reached, then adding a second blade passage may be necessary to regain stability.
The Time Transformation method usually reaches periodically established flow regimes after just a few
blade passing periods.
The Time Transformation method does not make any prior assumptions about the main frequencies
involved in the simulation. However, this pitch-change method is only applicable to compressible flows.
For multistage modeling, the Time Transformation TRS interface can be combined with Profile Transformation TRS. Sometimes the accuracy provided by the Time Transformation method can impact performance predictions. For subsonic compressors, the Time Transformation method gives a more accurate
resolution of the surge point, but perhaps gives a similar performance prediction as Profile Transformation and even steady-state analysis away from stall. For transonic compressors, the Time Transformation
method can give an overall improvement in the accuracy of the performance map due to the strong
interactions between components. This is caused by the shocks interacting between components. The
choked mass flow and the surge point may both change noticeably for the Time Transformation
method compared to Profile Transformation method and steady-state method.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
135
CFX Best Practices Guide for Turbomachinery
Time Transformation TRS can be combined with stage interfaces to model multistage turbomachines.
11.6.3.3. Fourier Transformation
The Fourier Transformation method is similar to the Time Transformation method however, it can be
used on very large pitch ratio configurations (for example, fan inlet distortion problems or fan bypass
regions where the pitch ratio between the fan blade and the downstream stator row is very large).
The Fourier Transformation method is capable of modeling both compressible and incompressible flows.
For optimum computational efficiency, it is recommended that you use the Fourier Transformation
method when the pitch ratio is too large to be modeled sensibly with the Time Transformation method.
The Fourier Transformation method is the best method to use for blade flutter analysis. The Fourier
Transformation method allows you to specify the phase shift (nodal diameter) as a simple input parameter between fluttering blade rows.
A transient blade row simulation with the Fourier Transformation method is more efficient with respect
to the reference solution when the machine has a large number of blades per row. Therefore, it may
not be useful to perform transient blade row simulation with the Fourier Transformation method on
turbomachines with a low blade count.
The Fourier Transformation TRS interface can be combined with stage interfaces to model multistage
turbomachines but can not be combined with Profile Transformation TRS or Time Transformation TRS
interfaces.
11.6.4. Convergence and Solution Monitoring of Transient Blade Row Flow
Problems
Due to the periodic nature of the flow in blade row configurations, ensure that the solution is monitored
sufficiently in order to determine when a transient periodic state has been reached. The following
monitoring options can be used:
• Use flow field monitors to check pressure, temperature and velocity variation. The solution is usually
deemed converged when the monitor repeats the same pattern over a common period. Sometimes
local flow field monitors do not show perfect repeatability within a common period due to local flow
instabilities. The Frequency Filtering option was added to the Fourier Transformation model to avoid
instabilities. The setting for enabling frequency filtering is described in Frequency Filtering in the CFXPre User's Guide.
• Use monitors of integrated quantities such as pressure surface loads, stage pressure ratio, or stage efficiency. Integrated quantity monitors tend to be less influenced by local instabilities and can give a
better sense of the overall solution convergence than local flow field monitors. Monitoring of instantaneous integrated quantities is not recommended for Time Transformation. Instead, you should monitor integrated quantities using monitor averaging.
• Use monitors on inlet and outlet flow rates.
• Use monitor averaging to assess the convergence of the periodic monitors. By selecting an appropriate
averaging range, you can monitor the average of the variation to determine if the solution has reached
a transient periodic state.
Ensure that a transient solution is converging properly at each time step:
• Check that the residuals of all equations are converging sufficiently at every time step.
136
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Transient Blade Row
• For time accurate solutions, convergence must be achieved without reaching the maximum number
of coefficient loops. If convergence is not achieved, a mesh issue could be the problem preventing the
solution from converging, requiring a re-examination of the mesh quality.
Also see Using Interrupt Control in Cases with Transient Convergence Behavior in the CFX-Solver Modeling
Guide.
11.6.5. Boundary Conditions in Blade Row Simulation
The following sections provide advice on applying boundary conditions:
11.6.5.1. Steady-state Analysis
11.6.5.2.Transient Analysis
11.6.5.1. Steady-state Analysis
To obtain the speed line performance of a turbomachine stage in steady-state analysis you can use one
of the following approaches:
• At the exit use a mass flow boundary from a stall point toward a near-choke point and pressure
boundary from a near-choke point to a deep-choke point.
• Use the exit corrected mass flow rate boundary condition, which enables you to traverse the speed line
without changing the boundary condition type.
11.6.5.2. Transient Analysis
In a transient simulation it is recommended that you use a pressure boundary to traverse the speed
line. This is particularly true when you are modeling a blade row flow problem on small sector of the
wheel and using one of the pitch-change models.
It is very important to note that a mass flow boundary at the exit should not be used with an incompressible flow setting. For a more accurate representation of the pressure field at the outlet of an axial
machine, use a radially distributed pressure profile. If you want to compare a transient solution obtained
from reduced geometry having pitch-change models (for example, Time Transformation or Fourier
Transformation) with a solution obtained from a full domain model, then it is best to select a boundary
condition setup that minimizes the differences between the two simulations. Therefore, on the exit
boundary it is recommended that you use a pressure profile without circumferential variation (thus, set
Pressure Profile Blend = 1). The pressure profile can vary radially.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
137
138
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 12: Best Practices: Scale-Resolving Simulations in ANSYS
CFD
While today’s CFD simulations are mainly based on Reynolds-Averaged Navier-Stokes (RANS) turbulence
models, it is becoming increasingly clear that certain classes of flows are better covered by models in
which all or a part of the turbulence spectrum is resolved in at least a portion of the numerical domain.
Such methods are termed Scale-Resolving Simulation (SRS) models in this paper.
There are two main motivations for using SRS models in favor of RANS formulations. The first reason
for using SRS models is the need for additional information that cannot be obtained from the RANS
simulation. Examples are acoustics simulations where the turbulence generates noise sources, which
cannot be extracted with accuracy from RANS simulations. Other examples are unsteady heat loading
in unsteady mixing zones of flow streams at different temperatures, which can lead to material failure,
or multi-physics effects like vortex cavitation, where the unsteady turbulence pressure field is the cause
of cavitation. In such situations, the need for SRS can exist even in cases where the RANS model would
in principle be capable of computing the correct time-averaged flow field.
The second reason for using SRS models is related to accuracy. It is known that RANS models have their
limitations in accuracy in certain flow situations. RANS models have shown their strength essentially
for wall-bounded flows, where the calibration according to the law-of-the-wall provides a sound
foundation for further refinement. For free shear flows, the performance of RANS models is much less
uniform. There is a wide variety of such flows, ranging from simple self-similar flows such as jets, mixing
layers, and wakes to impinging flows, flows with strong swirl, massively separated flows, and many
more. Considering that RANS models typically already have limitations covering the most basic selfsimilar free shear flows with one set of constants, there is little hope that even the most advanced
Reynolds stress models (RSM) will eventually be able to provide a reliable foundation for all such flows.
(For an overview of RANS modeling, see Durbin, Pettersson and Reif, 2003 [5] (p. 212); Wilcox, 2006
[38] (p. 214); or Hanjalic and Launder, 2011 [13] (p. 212).)
For free shear flows, it is typically much easier to resolve the largest turbulence scales, as they are of
the order of the shear layer thickness. In contrast, in wall boundary layers the turbulence length scale
near the wall becomes very small relative to the boundary layer thickness (increasingly so at higher Re
numbers). This poses severe limitations for Large Eddy Simulation (LES) as the computational effort required is still far from the computing power available to industry (Spalafrt, 1997 [29] (p. 213)). (For an
overview of LES modeling, see Guerts, 2004 [12] (p. 212), and Wagner et al., 2007 [35] (p. 214).) For this
reason, hybrid models are under development where large eddies are resolved only away from walls
and the wall boundary layers are covered by a RANS model. Examples of such global hybrid models
are Detached Eddy Simulation (DES, see Spalart, 2000 [30] (p. 213)) or Scale-Adaptive Simulation (SAS,
see Menter and Egorov, 2010 [18] (p. 213)). A further step is to apply a RANS model only in the innermost
part of the wall boundary layer and then to switch to a LES model for the main part of the boundary
layer. Such models are termed Wall-modeled LES (WMLES) (see Shur et al., 2008 [26] (p. 213)). Finally,
for large domains, it is frequently necessary to cover only a small portion with SRS models, while the
majority of the flow can be computed in RANS mode. In such situations, zonal or embedded LES
methods are attractive as they enable you to specify ahead of time the region where LES is required.
Such methods are typically not new models in the strict sense, but enable the combination of existing
models/technologies in a flexible way in different portions of the flowfield. Important elements of
zonal models are interface conditions, which convert turbulence from RANS mode to resolved mode
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
139
Best Practices: Scale-Resolving Simulations in ANSYS CFD
at pre-defined locations. In most cases, this is achieved by introducing synthetic turbulence based on
the length and time scales from the RANS model.
There are many hybrid RANS-LES models, often with somewhat confusing naming conventions, that
vary in the range of turbulence eddies they can resolve. On close inspection, many of these models are
only slight variations of the Detached Eddy Simulation (DES) concept of Spalart, 2000 [30] (p. 213) and
have very similar performance. For a general overview of SRS modeling concepts, see Fröhlich and von
Terzi, 2008 [8] (p. 212), and Sagaut et al., 2006 [24] (p. 213).
SRS models are very challenging in their proper application to industrial flows. The models typically
require special attention to various details such as:
• Model selection
• Grid generation
• Numerical settings
• Solution interpretation
• Postprocessing
• Quality assurance
Unfortunately, there is no unique model covering all industrial flows, and each individual model poses
its own set of challenges. In general, when using a CFD code, you must understand the intricacies of
the SRS model formulation in order to be able to select the optimal model and to use it efficiently. This
report is intended to support you in the basic understanding of such models and to provide best
practice guidelines for their usage. The discussion is focused on the models available in the ANSYS CFD
software.
This report is intended as an addition to the code-specific Theory and User Documentation available
for both ANSYS Fluent and ANSYS CFX . The Theory and User Documentation describes in detail how
to select and activate these models, so that information is not repeated here. This report is intended
to provide you with a general understanding of the underlying principles and the associated limitations
of each of the described modeling concepts. It also covers the types of flows for which the models are
suitable as well as flows where they will likely not work well. Finally, the impact of numerical settings
on model performance is discussed.
In accordance with the intention of providing you with recommendations for your day-to-day work,
several Appendices can be found at the end of the document for quick reference of the most important
points.
This chapter discusses:
12.1. Scale-Resolving Simulation (SRS) Models – Basic Formulations
12.2. Generic Flow Types and Basic Model Selection
12.3. Numerical Settings for SRS
12.4. Initial and Boundary Conditions
12.5. Postprocessing and Averaging
12.6. Summary
12.7. Scale-Resolving Simulations References
140
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Scale-Resolving Simulation (SRS) Models – Basic Formulations
12.1. Scale-Resolving Simulation (SRS) Models – Basic Formulations
In the ANSYS CFD codes the following SRS models are available:
1. Scale-Adaptive Simulation (SAS) models
• SAS-SST model (Fluent, CFX)
2. Detached Eddy Simulation (DES) models
• DES-SA (DDES) model (Fluent)
• DES-SST (DDES) model (Fluent, CFX)
• Realizable
DES model (Fluent)
3. Large Eddy Simulation (LES)
• Smagorinsky-Lilly model (+dynamic) (Fluent, CFX)
• WALE model (Fluent, CFX)
• Kinetic energy subgrid model dynamic (Fluent)
• Algebraic Wall Modeled LES (WMLES) (Fluent, CFX)
4. Embedded LES (ELES) mode
• Combination of all RANS models with all non-dynamic LES models (Fluent)
• Zonal forcing model (CFX)
5. Synthetic turbulence generator
• Vortex method (Fluent)
• Harmonic Turbulence Generator (HTG) (CFX)
12.1.1. Scale-Adaptive Simulation (SAS)
In principle, all RANS models can be solved in unsteady mode (URANS). Experience shows, however,
that classical URANS models do not provide any spectral content, even if the grid and time step resolution
are sufficient for that purpose. It has long been argued that this behavior is a natural outcome of the
RANS averaging procedure (typically time averaging), which eliminates all turbulence content from the
velocity field. By that argument, it has been concluded that URANS can work only in situations of a
"separation of scales," where only time variations that are of much lower frequency than turbulence
are resolved. An example would be the flow over a slowly oscillating airfoil, where the turbulence is
modeled entirely by the RANS model and only the slow super-imposed motion is resolved in time. A
borderline case for this scenario is the flow over bluff bodies, like a cylinder in crossflow. For such flows,
the URANS simulation provides unsteady solutions even without an independent external forcing. The
frequency of the resulting vortex shedding is not necessarily much lower than the frequencies of the
largest turbulent scales. This scenario is depicted in Figure 12.1 (p. 142), which shows that URANS
models (in this case SST) produce a single mode vortex shedding even at a relatively high
number
of
. The vortex stream extends far into the cylinder wake, maintaining a single frequency. This
result is in contradiction to experimental observations of a broadband turbulence spectrum.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
141
Best Practices: Scale-Resolving Simulations in ANSYS CFD
As shown in a series of publications (for example, Menter and Egorov, 2010 [18] (p. 213), Egorov et al.,
2010 [6] (p. 212)), a class of RANS models can be derived based on a theoretical concept dating back to
Rotta (see Rotta, 1972 [23] (p. 213)). These models perform like standard RANS models in steady flows,
but enable the formation of a broadband turbulence spectrum for certain types of unstable flows (for
the types of flows, see Section 12.2 (p. 158)). Such models are termed Scale-Adaptive Simulation (SAS)
models. This scenario is illustrated by Figure 12.2 (p. 142), which shows the same simulation as in Figure
12.1 (p. 142) but with the SAS-SST model. The behavior seen in Figure 12.1 (p. 142) is therefore not inherent
to all RANS models, but only to those derived in a special fashion.
Figure 12.1: URANS computations of a flow past a circular cylinder (SST model)
Figure 12.2: SAS simulation of flow past a circular cylinder (SAS-SST model)
The SAS concept is described in much detail in the cited references and will not be repeated here.
However, the basic model formulation must be provided for a discussion of the model’s characteristics.
The difference between standard RANS and SAS models lies in the treatment of the scale-defining
equation (typically -, -, or -equation). In classic RANS models, the scale equation is modeled based
on an analogy with the -equation using simple dimensional arguments. The scale equation of SAS
models is based on an exact transport equation for the turbulence length scale as proposed by Rotta.
This method was re-visited by Menter and Egorov, 2010 [18] (p. 213) and avoids some limitations of the
original Rotta model. As a result of this re-formulation, it was shown that the second derivative of the
velocity field must be included in the source terms of the scale equation. The original SAS model (Menter
142
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Scale-Resolving Simulation (SRS) Models – Basic Formulations
and Egorov, 2010 [18] (p. 213)) was formulated as a two-equation model, with the variable
the scale equation:
for
(12.1)
(12.2)
(12.3)
The main new term is the one including the von Karman length scale
, which does not appear in
any standard RANS model. The second velocity derivative allows the model to adjust its length scale
to those structures already resolved in the flow. This functionality is not present in standard RANS
models. This leads to the behavior shown in Figure 12.2 (p. 142), which agrees more closely with the
experimental observations for such flows.
The
term can be transformed and implemented into any other scale-defining equation resulting in
SAS capabilities as in the case of the SAS-SST model. For the SAS-SST model, the additional term in the
-equation resulting from the transformation has been designed to have no effect on the SST model’s
RANS performance for wall boundary layers. It can have a moderate effect on free shear flows (Davidson,
2006 [4] (p. 212)).
The SAS model will remain in steady RANS mode for wall bounded flows, and can switch to SRS mode
in flows with large and unstable separation zones (see Section 12.2 (p. 158)).
12.1.2. Detached Eddy Simulation (DES)
Detached Eddy Simulation (DES) was introduced by Spalart and co-workers (Spalart et al., 1997
[29] (p. 213), 2000 [30] (p. 213), Travin et al., 2000 [33] (p. 214), Strelets, 2001 [32] (p. 214)), to eliminate the
main limitation of LES models by proposing a hybrid formulation that switches between RANS and LES
based on the grid resolution provided. By this formulation, the wall boundary layers are entirely covered
by the RANS model and the free shear flows away from walls are typically computed in LES mode. The
formulation is mathematically relatively simple and can be built on top of any RANS turbulence model.
DES has attained significant attention in the turbulence community as it was the first SRS model that
allowed the inclusion of SRS capabilities into common engineering flow simulations.
Within DES models, the switch between RANS and LES is based on a criterion like the following:
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
143
Best Practices: Scale-Resolving Simulations in ANSYS CFD
(12.4)
where
is the maximum edge length of the local computational cell. The actual formulation for a
two-equation model (for example, the -equation of the
model) is:
(12.5)
(12.6)
As the grid is refined below the limit
the DES-limiter is activated and switches the model from
RANS to LES mode. The intention of the model is to run in RANS mode for attached flow regions, and
to switch to LES mode in detached regions away from walls. This switch suggests that the original DES
formulation, as well as its later versions, require a grid and time step resolution to be of LES quality
once they switch to the grid spacing as the defining length scale. Once the limiter is activated, the
models lose their RANS calibration and all relevant turbulence information must be resolved. For this
reason, for example in free shear flows, the DES approach offers no computational savings over a
standard LES model. However, it allows you to avoid the high computing costs of covering the wall
boundary layers in LES mode.
It is also important to note that the DES limiter can already be activated by grid refinement inside attached boundary layers. This is undesirable as it affects the RANS model by reducing the eddy viscosity;
this can lead to Grid-Induced Separation (GIS), as discussed by Menter and Kuntz, 2002 [19] (p. 213),
where the boundary layers can separate at arbitrary locations depending on the grid spacing. In order
to avoid this limitation, the DES concept has been extended to Delayed-DES (DDES) by Spalart et al.,
2006 [31] (p. 214), following the proposal of Menter and Kuntz, 2002 [19] (p. 213) of “shielding” the
boundary layer from the DES limiter. The DDES extension was also applied to the DES-SA formulation
resulting in the DDES-SA model, as well as to the SST model giving the DDES-SST model.
For two-equation models, the dissipation term in the -equation is thereby re-formulated as follows:
(12.7)
(12.8)
The function
is designed in such a way as to give
inside the wall boundary layer and
away from the wall. The definition of this function is intricate as it involves a balance between
proper shielding and not suppressing the formation of resolved turbulence as the flow separates from
the wall.
144
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Scale-Resolving Simulation (SRS) Models – Basic Formulations
There are a number of DDES models available in ANSYS CFD. They follow the same principal idea with
respect to switching between RANS and LES mode. The models differ therefore mostly by their RANS
capabilities and should be selected accordingly.
12.1.3. Large Eddy Simulation (LES)
The details of different LES models can be found in the User and Theory documentation of the corresponding solvers. As described in Section 12.1.3.1 (p. 145), the main purpose of LES models is to provide
sufficient damping for the smallest (unresolved) scales. For this reason, it is not advisable to use complex
formulations, but to stay with simple algebraic models. The most widely used LES model is the
Smagorinsky, 1963 [28] (p. 213) model:
(12.9)
The main deficiency of the Smagorinsky model is that its eddy-viscosity does not go to zero for laminar
shear flows (only
). For this reason, this model also requires a near-wall damping function
in the viscous sublayer. It is desirable to have a LES formulation that automatically provides zero eddyviscosity for simple laminar shear flows. This is especially important when computing flows with laminar
turbulent transition, where the Smagorinsky model would negatively affect the laminar flow. The simplest
model to provide this functionality is the WALE (Wall-Adapting Local Eddy-viscosity) model of Nicoud
and Ducros, 1999 [21] (p. 213). The same effect is also achieved by dynamic LES models, but at the cost
of a somewhat higher complexity. None of the classical LES models addresses the main industrial
problem of excessive computing costs for wall-bounded flows at moderate to high Reynolds numbers.
There are numerous cases at very low Reynolds numbers where LES can be an industrial option. Under
such conditions, the wall boundary layers are likely laminar and turbulence forms only in separated
shear layers and detached flow regions. Such situations can be identified by analyzing RANS eddy viscosity solutions for a given flow. In the case where the ratio of turbulence to molecular viscosity
is smaller than
inside the boundary layer, it can be assumed that the boundary layers
are laminar and no resolution of near-wall turbulence is required. Such conditions are observed for
flows around valves or other small-scale devices at low Reynolds numbers.
LES can also be applied to free shear flows, where resolution requirements are much reduced relative
to wall-bounded flows.
12.1.3.1. Limitations of Large Eddy Simulation (LES)
In order to understand the motivation for hybrid models, one has to discuss the limitations of Large
Eddy Simulation (LES). LES has been the most widely used SRS model over the last decades. It is based
on the concept of resolving only the large scales of turbulence and to model the small scales. The
classical motivation for LES is that the large scales are problem-dependent and difficult to model,
whereas the smaller scales become more and more universal and isotropic and can be modeled more
easily.
LES is based on filtering the Navier-Stokes equations over a finite spatial region (typically the grid
volume) and aimed at only resolving the portions of turbulence larger than the filter width. Turbulence
structures smaller than the filter are then modeled, typically by a simple Eddy Viscosity model.
The filtering operation is defined as:
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
145
Best Practices: Scale-Resolving Simulations in ANSYS CFD
(12.10)
where is the spatial filter. Filtering the Navier-Stokes equations results in the following form (density
fluctuations neglected):
(12.11)
The equations feature an additional stress term due to the filtering operation:
(12.12)
Despite the difference in derivation, the additional sub-grid stress tensor is typically modeled as in RANS
using an eddy viscosity model:
(12.13)
The important practical implication from this modeling approach is that the modeled momentum
equations for RANS and LES are identical if an eddy-viscosity model is used in both cases. The modeled
Navier-Stokes equations have no knowledge of their derivation. The only information they obtain from
the turbulence model is the size of the eddy viscosity. Depending on that, the equations will operate
in RANS or LES mode (or in some intermediate mode). The formal identity of the filtered Navier-Stokes
and the RANS equations is the basis of hybrid RANS-LES turbulence models, which can obviously be
introduced into the same set of momentum equations. Only the model (and the numerics) have to be
switched.
Classical LES models are of the form of the Smagorinsky, 1963 [28] (p. 213) model:
(12.14)
where is a measure of the grid spacing of the numerical mesh, is the strain rate scalar and
is a
constant. This is obviously a rather simple formulation, indicating that LES models will not provide a
highly accurate representation of the smallest scales. From a practical standpoint, a very detailed
modeling might not be required. A more appropriate goal for LES is not to model the impact of the
unresolved scales onto the resolved ones, but to model the dissipation of the smallest resolved scales.
This can be seen from Figure 12.3 (p. 147) showing the turbulence energy spectrum of a Decaying Isotropic Turbulence (DIT) test case; that is, initially stirred turbulence in a box, decaying over time (ComteBellot and Corrsin, 1971 [3] (p. 212)).
is the turbulence energy as a function of wave number .
Small values represent large eddies and large values represent small eddies. Turbulence moves
down the turbulence spectrum from the small wave number to the high wave numbers. In a fully resolved
simulation (Direct Numerical Simulation, or DNS), the turbulence is dissipated into heat at the smallest
scales (
in Figure 12.3 (p. 147)), by viscosity. The dissipation is achieved by:
146
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Scale-Resolving Simulation (SRS) Models – Basic Formulations
(12.15)
where is typically a very small kinematic molecular viscosity. The dissipation
as the velocity gradients of the smallest scales are very large.
is still of finite value
LES computations are usually performed on numerical grids that are too coarse to resolve the smallest
scales. In the current example, the cut-off limit of LES (resolution limit) is at around
. The velocity
gradients of the smallest resolved scales in LES are therefore much smaller than those at the DNS limit.
The molecular viscosity is then not sufficient to provide the correct level of dissipation. In this case, the
proper amount of dissipation can be achieved by increasing the viscosity, using an eddy-viscosity:
(12.16)
The eddy viscosity is calibrated to provide the correct amount of dissipation at the LES grid limit. The
effect can be seen in Figure 12.3 (p. 147), where a LES of the DIT case is performed without a LES model
and with different LES models. When the LES models are activated, the energy is dissipated and the
models provide a sensible spectrum for all resolved scales. LES is not modeling the influence of unresolved
small scale turbulence onto the larger, resolved scales, but the dissipation of turbulence into heat (the
dissipated energy is typically very small relative to the thermal energy of the fluid and does not have
to be accounted for, except for high Mach number flows).
Figure 12.3: Turbulence spectrum for DIT test case after t=2. Comparison of results without
Sub-Grid Scale model (no LES) with WALE and Smagorinsky LES model simulations
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
147
Best Practices: Scale-Resolving Simulations in ANSYS CFD
This discussion shows that LES is a fairly simple technology, which does not provide a reliable backbone
for modeling. This is also true for more complex LES models like dynamic models. Dynamic eddy viscosity
LES models (see Guerts, 2004 [12] (p. 212)) are designed to estimate the required level of dissipation at
the grid limit from flow conditions at larger scales (typically twice the filter width), thereby reducing
the need for model calibration. Such models, however, also only provide a suitable eddy viscosity level
for energy dissipation. Within the LES framework, all features and effects of the flow that are of interest
and relevance to engineers have to be resolved in space and time. This requirement makes LES in
principle a very CPU-expensive technology.
Even more demanding is the application of LES to wall-bounded flows, which is the typical situation in
engineering flows. The turbulent length scale, , of the large eddies can be expressed as:
(12.17)
where is the wall distance and a constant. Even the (locally) largest scales become very small near
the wall and require a high resolution in all three space dimensions and in time.
The linear dependence of on indicates that the turbulence length scales approach zero near the
wall, which would require an infinitely fine grid to resolve them. This is not the case in reality, as the
molecular viscosity prevents scales smaller than the Kolmogorov limit. This is manifested by the viscous
or laminar sublayer, a region very close to the wall, where turbulence is damped and does not need to
be resolved. However, the viscous sublayer thickness is a function of the Reynolds number, Re, of the
flow. At higher Re numbers, the viscous sublayer becomes decreasingly thinner and thereby allows the
survival of smaller and smaller eddies, which need to be resolved. This is depicted in Figure 12.4 (p. 149)
showing a sketch of turbulence structures in the vicinity of the wall (for example, channel flow with
flow direction normal to observer). The upper part of the picture represents a low Re number and the
lower part a higher Re number. The gray box indicates the viscous sublayer for the two Re numbers.
The structures inside the viscous sublayer (circles inside the gray box) are depicted but not present in
reality due to viscous damping. Only the structures outside of the viscous sublayer (that is, above the
gray box) exist and need to be resolved. Due to the reduced thickness of the viscous sublayer in the
high Re case, substantially more resolution is required to resolve all active scales. Wall-resolved LES is
therefore prohibitively expensive for moderate to high Reynolds numbers. This is the main reason why
LES is not suitable for most engineering flows.
148
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Scale-Resolving Simulation (SRS) Models – Basic Formulations
Figure 12.4: Sketch of turbulence structures for wall-bounded channel flow with viscous sublayer
(a) Low Re number (b) High Re number (Grey area: viscous sublayer)
The Reynolds number dependence of wall-resolved LES can be estimated for a simple periodic channel
flow as shown in Figure 12.5 (p. 149) ( -streamwise, -wall-normal, -spanwise, is the channel height).
(12.18)
Figure 12.5: Turbulence structures in a channel flow
The typical resolution requirements for LES are:
(12.19)
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
149
Best Practices: Scale-Resolving Simulations in ANSYS CFD
where
is the non-dimensional grid spacing in the streamwise direction,
the number of cells across half of the channel height. With the definitions:
in the spanwise and
(12.20)
one can find the number,
of cells required as a function of
domain of simple flow (see Table 12.1 (p. 150)).
, for resolving this limited
(12.21)
Table 12.1: Number of cells,
, vs Reynolds number for channel flow
500
(For the practitioner: the Reynolds,
103
104
105
, number based on the bulk velocity is around a factor of ten
larger than the Reynolds number,
, based on friction velocity. Note that
is based on
).
The number of cells increases strongly with
number, demanding high computing resources even
for very simple flows. The CPU power scales even less favorably, as the time step must also be reduced
to maintain a constant CFL number (
).
The Re number scaling for channel flows could be reduced by the application of wall functions with
increasing
values for higher
numbers. However, wall functions are a strong source of modeling
uncertainty and can undermine the overall accuracy of simulations. Furthermore, the experience with
RANS models shows that the generation of high quality wall-function grids for complex geometries is
a very challenging task. This task is even more challenging for LES applications, where you would have
to control the resolution in all three space dimensions to conform to the LES requirements (for example,
and
then depend on
).
For external flows, there is an additional Re number effect resulting from the relative thickness of the
boundary layer (for example, boundary layer thickness relative to chord length of an airfoil). At high Re
numbers, the boundary layer becomes very thin relative to the body’s dimensions. Assuming a constant
resolution per boundary layer volume, Spalart et al., 1997 [29] (p. 213), 2000 [30] (p. 213) provided estimates
of computing power requirements for high Reynolds number aerodynamic flows under the most favorable
assumptions. Even then, the computing resources are excessive and will not be met even by optimistic
estimates of computing power increases for several decades.
While the computing requirements for high Re number flows are dominated by the relatively thin
boundary layers, the situation for low Re number technical flows is often equally unfavorable, as effects
such as laminar-turbulent transition dominate and need to be resolved. Based on reduced geometry
150
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Scale-Resolving Simulation (SRS) Models – Basic Formulations
simulations of turbomachinery blades (see Michelassi, 2003 [20] (p. 213)), an estimate for a single turbine
blade with end-walls is given in Table 12.2 (p. 151).
Table 12.2: Computing power estimate for a single turbomachinery blade with end-walls
Method
Cells
Time steps
Inner
loops per
time step
Ratio to
RANS
RANS
~106
~102
1
1
LES
~108–109
~104–105
10
105–107
Considering that the goal of turbomachinery companies is the simulation of entire machines (or parts
of them), it is unrealistic to assume that LES will become a major element of industrial CFD simulations
even for such low Re number (
) applications. However, LES can play a role in the detailed analysis of elements of such flows like cooling holes or active flow control.
All the above does not mean that LES of wall-bounded flows is not feasible at all, but just that the costs
of such simulations are high. Figure 12.6 (p. 152) shows the grid used for a LES around a NACA 0012
airfoil using the WALE model. The computational domain is limited in the spanwise direction to 5% of
the airfoil chord length using periodic boundary conditions in that direction. At a Reynolds number of
a spanwise extent of 5% has been estimated as the minimum domain size that allows
turbulence structures to develop without being synchronized across the span by the periodic boundary
conditions. The estimate was based on the boundary layer thickness at the trailing edge as obtained
from a precursor RANS computation. This boundary layer thickness is about 2% chord length. The grid
had 80 cells in the spanwise direction and overall
cells. The simulation was carried out at an
angle of attack of
, using ANSYS Fluent in incompressible mode. The chord length was set to
, the freestream velocity,
and the fluid is air at standard conditions. The
time step was set to
giving a Courant number of
inside the boundary layer.
Figure 12.7 (p. 153) shows turbulence structures near the leading edge (a) and the trailing edge (b). Near
the leading edge, the laminar-turbulent transition can clearly be seen. The transition is triggered by a
laminar separation bubble. Near the trailing edge, the turbulence structures are already relatively large,
but still appear unsynchronized in the spanwise direction (no large scale 2D structures with axis orientation in the spanwise direction). The simulation was run for ~104 time steps before the averaging procedure was started. The time averaging was conducted for
time steps. Figure 12.8 (p. 153)
shows a comparison of the wall pressure coefficient
and Figure 12.9 (p. 154) of the wall shear stress
coefficient
on the suction side of the airfoil in comparison to a RANS computation using the SST
model (Menter, 1994 [16] (p. 213)). No detailed discussion of the simulation is intended here, but the
comparison of the wall shear stress with the well-calibrated RANS model indicates that the resolution
of the grid is still insufficient for capturing the near-wall details. For this reason, the wall shear stress is
significantly underestimated by about 30% compared to the SST model in the leading edge area. As
the trailing edge is approached, the comparison improves, mainly because the boundary layer thickness
is increased whereas the wall shear stress is decreased, which produces a higher relative resolution in
the LES. Based on this simulation, it is estimated that a refinement by a factor of 2, in both streamwise
and spanwise directions, would be required in order to reproduce the correct wall shear stress. While
such a resolution is not outside the realm of available computers, it is still far too high for day-to-day
simulations.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
151
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.6: Details of grid around a NACA 4412 airfoil (a) Grid topology (b) Leading edge area
(c) Trailing edge area
152
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Scale-Resolving Simulation (SRS) Models – Basic Formulations
Figure 12.7: Turbulence structures of WALE LES computation around a NACA 4412 airfoil (a)
Leading edge (b) Trailing edge (Q-criterion, color- spanwise velocity component)
Figure 12.8: Wall pressure coefficient Cp on the suction side of a NACA 4412 airfoil: comparison
of RANS-SST and LES-WALE results
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
153
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.9: Wall shear stress coefficient Cf on the suction side of a NACA 4412 airfoil: comparison
of RANS-SST and LES-WALE results
Overall, LES for industrial flows will be restricted in the foreseeable future to flows not involving wall
boundary layers, or wall-bounded flows in strongly reduced geometries, preferentially at low Re numbers.
The limitations of the conventional LES approach are the driving force behind the development of hybrid
RANS-LES models that are described in the later parts of this report.
12.1.4. Wall Modeled Large Eddy Simulation (WMLES)
Wall Modeled LES (WMLES) is an alternative to classical LES and reduces the stringent and
numberdependent grid resolution requirements of classical wall-resolved LES (Section 12.1.3.1 (p. 145)) The
principle idea is depicted in Figure 12.10 (p. 155). As described in Section 12.1.3.1 (p. 145), the near-wall
turbulence length scales increase linearly with the wall distance, resulting in smaller and smaller eddies
as the wall is approached. This effect is limited by molecular viscosity, which damps out eddies inside
the viscous sublayer (VS). As the
number increases, smaller and smaller eddies appear, since the
viscous sublayer becomes thinner. In order to avoid the resolution of these small near-wall scales, RANS
and LES models are combined such that the RANS model covers the very near-wall layer, and then
switches over to the LES formulation once the grid spacing becomes sufficient to resolve the local
scales. This is seen in Figure 12.10 (b) (p. 155), where the RANS layer extends outside of the VS, thus
avoiding the need to resolve the inner second row of eddies depicted in the sketch.
154
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Scale-Resolving Simulation (SRS) Models – Basic Formulations
Figure 12.10: Concept of WMLES for high Re number flows (a) Wall-resolved LES. (b) WMLES
The WMLES formulation in ANSYS CFD is based on the formulation of Shur et al., 2008 [26] (p. 213):
(12.22)
where
is the wall distance,
is the von Karman constant,
is the strain rate and
is a near-wall
damping function. This formulation was adapted to suit the needs of the ANSYS general purpose CFD
codes. Near the wall, the min-function selects the Prandtl mixing length model whereas away from the
wall it switches over to the Smagorinsky model. Meshing requirements for the WMLES approach are
given in Section 12.2.3.3 (p. 177).
For wall boundary layer flows, the resolution requirements of WMLES depend on the details of the
model formulation. In ANSYS Fluent and ANSYS CFX they are (assuming for this estimate that is the
streamwise, the wall normal and the spanwise direction as shown in Figure 12.11 (p. 156)):
(12.23)
where ,
, and
are the numbers of cells per boundary layer thickness, , in the streamwise, wall
normal, and spanwise directions respectively, (see Figure 12.11 (p. 156)). About 6000-8000 cells are
needed to cover one boundary layer volume
. This is also the minimal resolution for classical
LES models at low Reynolds numbers. Actually, for low Reynolds numbers, WMLES turns essentially into
classical LES. The advantage of WMLES is that the resolution requirements relative to the boundary
layer thickness remain independent of the Reynolds number.
While WMLES is largely Reynolds number-independent for channel and pipe flows (where the boundary
layer thickness must be replaced by half of the channel height) there remains a Reynolds number
sensitivity for aerodynamic boundary layer flows, where, the ratio of the boundary layer thickness, ,
to a characteristic body dimension, , is decreasing with increasing Reynolds number. In aerodynamic
boundary layer flows, there are more boundary layer volumes to consider at increased Reynolds numbers.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
155
Best Practices: Scale-Resolving Simulations in ANSYS CFD
It should also be noted that despite the large cost savings of WMLES compared to wall-resolved LES,
the cost increase relative to RANS models is still high. Typical RANS computations feature only one cell
per boundary layer thickness in streamwise and spanwise directions (
). In addition, RANS
steady-state simulations can be converged in the order of ~102–103 iterations, whereas unsteady simulations typically require ~104–105.
For wall-normal resolution in WMLES, it is recommended that you use grids with
If this cannot be achieved, the WMLES model is formulated to tolerate coarser
itive formulation) as well.
at the wall.
values (
-insens-
Figure 12.11: Sketch of boundary layer profile with thickness , x-streamwise direction, y-normal
direction, and z-spanwise direction
For channel and pipe flows, the above resolution requirements for the boundary layer should be applied,
only replacing the boundary layer thickness, , with half the channel height, or with the pipe radius in
the grid estimation. This estimate would result in a minimum of ~120 cells in the circumferential direction
(
) for a fully developed pipe flow.
It should be noted that reductions in grid resolution similar to WMLES can be achieved with classical
LES models when using LES wall functions. However, the generation of suitable grids for LES wall
functions is very challenging as the grid spacing normal to the wall and the wall-parallel grid resolution
requirements are coupled and strongly dependent on
number (unlike RANS where only the wallnormal resolution must be considered).
In ANSYS Fluent, the WMLES formulation can be selected as one of the LES options; in ANSYS CFX it is
always activated inside the LES zone of the Zonal Forced LES (ZFLES) method.
12.1.5. Embedded/Zonal LES (ELES, ZLES)
The idea behind ELES is to predefine different zones with different treatments of turbulence in the
preprocessing stage. The domain is split into a RANS and a LES portion ahead of the simulation. Between
the different regions, the turbulence model is switched from RANS to LES/WMLES. In order to maintain
consistency, synthetic turbulence is generally introduced at RANS-LES interfaces. ELES is actually not a
new model, but an infrastructure that combines existing elements of technology in a zonal fashion. The
recommendations for each zone are therefore the same as those applicable to the individual models.
156
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Scale-Resolving Simulation (SRS) Models – Basic Formulations
In ANSYS Fluent, an Embedded LES formulation is available (Cokljat et al., 2009 [2] (p. 212)). It allows the
combination of most RANS models with all non-dynamic LES models in the predefined RANS and LES
regions respectively. The conversion from modeled turbulence to resolved turbulence is achieved at
the RANS-LES interface using the Vortex Method (Mathey et al., 2003 [15] (p. 213)).
In CFX, a similar functionality is achieved using a method called Zonal Forced LES (ZFLES) (Menter et
al., 2009 [17] (p. 213)). The simulation is based on a pre-selected RANS model. In a LES zone, specified
via a CEL expression, forcing terms in the momentum and turbulence equations are activated. These
terms push the RANS model into a WMLES formulation. In addition, synthetic turbulence is generated
at the RANS-LES interface,
An additional option in ANSYS Fluent involves using a global turbulence model (SAS or DDES), and activates the generation of synthetic turbulence at a pre-defined interface. The code takes care of balancing
the resolved and modeled turbulence through the interface. This option can be used to force global
hybrid models (like SAS or DDES) into unsteadiness for cases where the natural flow instability is not
sufficient. Unlike ELES, the same turbulence model is used upstream and downstream of the interface.
In ELES, different models are used in different zones on opposite sides of the interface.
Such forcing can also by achieved in ANSYS CFX by specifying a thin LES region and using the SAS or
DDES model globally.
12.1.6. Unsteady Inlet/Interface Turbulence
Classical LES requires providing unsteady fluctuations at turbulent inlets/interfaces (RANS-LES interface)
to the LES domain. This makes LES substantially more demanding than RANS, where profiles of the
mean turbulence quantities ( and or and ) are typically specified. An example is a fully turbulent
channel (pipe) flow. The flow enters the domain in a fully turbulent state at the inlet, so you are therefore
required to provide suitable resolved turbulence at such an inlet location through unsteady inlet velocity
profiles. The inlet profiles have to be composed in such a way that their time average corresponds to
the correct mean flow inlet profiles, as well as to all relevant turbulence characteristics (turbulence time
and length scales, turbulence stresses, and so on). For fully turbulent channel and pipe flows, this requirement can be circumvented by the application of periodic boundary conditions in the flow direction.
The flow is thereby driven by a source term in the momentum equation acting in the streamwise direction. By that trick, the turbulence leaving the domain at the outlet enters the domain again at the inlet,
thereby avoiding the explicit specification of unsteady turbulence profiles. This approach can be employed
for only very simple configurations. It requires a sufficient length of the domain (at least ~8–10h, see
Figure 12.5 (p. 149)) in the streamwise direction to enable the formation inside the domain of turbulence
structures independent of the periodic boundaries.
In most practical cases, the geometry does not enable fully periodic simulations. It can however feature
fully developed profiles at the inlet (again typically pipe/channel flows). In such cases, you can perform
a periodic precursor simulation on a separate periodic domain and then insert the unsteady profiles
obtained at any cross-section of that simulation to the inlet of the complex CFD domain. This approach
requires either a direct coupling of two separate CFD simulations or the storage of a sufficient number
of unsteady profiles from the periodic simulation to be read in by the full simulation.
In a real situation, however, the inlet profiles might not be fully developed and no simple method exists
for producing consistent inlet turbulence. In such cases, synthetic turbulence can be generated, based
on given inlet profiles from RANS. These are typically obtained from a precursor RANS computation of
the domain upstream of the LES inlet.
There are several methods for generating synthetic turbulence. In ANSYS Fluent, the most widely used
method is the Vortex Method (VM) (see Mathey et al., 2003 [15] (p. 213)), where a number of discrete
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
157
Best Practices: Scale-Resolving Simulations in ANSYS CFD
vortices are generated at the inlet. Their distribution, strength, and size are modeled to provide the
desirable characteristics of real turbulence. The input parameters to the VM are the two scales (k and
or k and ) from the upstream RANS computation. CFX uses the generation of synthetic turbulence
by using suitable harmonic functions as an alternative to the VM (see Menter et al., 2009 [17] (p. 213)).
The characteristic of high-quality synthetic turbulence in wall-bounded flows is that it recovers the timeaveraged turbulent stress tensor quickly downstream of the inlet. This can be checked by plotting
sensitive quantities like the time-averaged wall shear stress or heat transfer coefficient and observing
their variation downstream of the inlet. It is also advisable to investigate the turbulence structures
visually by using, for example, an isosurface of the -criterion,
(where is the Strain
rate, and is the vorticity rate). This can be done even after a few hundred time steps into the simulation.
Because synthetic turbulence will never coincide in all aspects with true turbulence, avoid putting an
inlet/interface at a location with strong non-equilibrium turbulence activity. In boundary layer flows,
that means that the inlet or RANS-LES interface should be located several (at least 3) boundary layer
thicknesses upstream of any strong non-equilibrium zone (such as a separation). The boundary layers
downstream of the inlet/interface need to be resolved with a sufficiently high spatial resolution (see
Section 12.2.3.3 (p. 177)).
12.2. Generic Flow Types and Basic Model Selection
There is a wide range of complex industrial turbulent flows and there is no single SRS approach to
cover all of them with high efficiency. The most difficult question as you use the software is therefore
how to select the optimal model combination for a given simulation. For this task, it is useful to categorize
flows into different types. Although such a categorization is not always easy and by no means scientifically
exact (there are many flows that do not exactly fall into any one of the proposed categories or fall into
more than one) it might still help in the selection of the most appropriate SRS modeling approach.
This section discusses:
12.2.1. Globally Unstable Flows
12.2.2. Locally Unstable Flows
12.2.3. Stable Flows and Wall Boundary Layers
12.2.1. Globally Unstable Flows
12.2.1.1. Flow Physics
The classical example of a globally unstable flow is a flow past a bluff body. Even when computed with
a classical URANS model, the simulation will typically provide an unsteady output. Figure 12.14 (p. 163)
shows the flow around a triangular cylinder in crossflow as computed with both the SAS-SST and the
DES-SST model. It is important to emphasize that the flow is computed with steady-state boundary
conditions (as would be employed for a RANS simulation). Still, the flow downstream of the obstacle
turns quickly into unsteady (scale-resolving) mode, even though no unsteadiness is introduced by any
boundary or interface condition.
From a physical standpoint, such flows are characterized by the formation of new turbulence downstream
of the body. This turbulence is independent from, and effectively overrides, the turbulence coming from
the thin, attached boundary layers around the body. The turbulence in the attached boundary layers
has very little effect on the turbulence in the separated zone. The attached boundary layers can, however,
define the separation point/line on a smoothly curved body and so affect the size of the downstream
separation zone. This effect can be tackled by a suitable underlying RANS model.
158
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
Typical members of this family of flows are given in the list below. Such flows are very common in engineering applications and are also the type of flows where RANS models can exhibit a significant deterioration of their predictive accuracy.
Examples of globally unstable flows include:
• Flows past bluff bodies include:
– Flow past buildings
– Landing gears of airplanes
– Baffles in mixers
– Side mirrors of cars
– Stalled wings/sails
– Re-entry vehicles
– Trains/trucks/cars in crossflow
– Tip gap of turbomachinery blades
– Flows past orifices, sharp nozzles
– Cavities
– Flows with large separation zones (relative to attached boundary layer thickness)
• Flows with strong swirl instabilities include:
– Flow in combustion chambers of gas turbines
– Flows past vortex generators
– Some tip vortex flows in adverse pressure gradients
• Flows with strong flow interaction include:
– Impinging/colliding jets
– Jets in crossflow
The color scheme of the preceding points above identifies flows that are clearly within the definition
of globally unstable flows (black) and those where the type of the flow depends on details of its regime/geometry (gray). Such flows fall in-between globally and locally unstable flows (see Section 12.2.2 (p. 169)).
12.2.1.2. Modeling
Of all flows where SRS modeling is required, globally unstable flows are conceptually the easiest to
handle. They can be typically captured by a global RANS-LES model such as SAS or DDES. Such models
cover the attached and mildly separated boundary layers in RANS mode, thereby avoiding the high
costs of resolving wall turbulence. Due to the strong flow instability past the separation line, there is
no need for specifying unsteady inlet turbulence nor to define specific LES zones. Globally unstable
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
159
Best Practices: Scale-Resolving Simulations in ANSYS CFD
flows are also the most beneficial for SRS, as experience shows that RANS models can fail with significant
margins of error for such flows. A large number of industrial flows fall into this category.
The safest SRS model for such flows is the SAS approach. It offers the advantage that the RANS model
is not affected by the grid spacing and thereby avoids the potential negative effects of (D)DES (gray
zones or grid induced separation). The SAS concept reverts back to (U)RANS in case the mesh/time step
is not sufficient for LES and thereby preserves a backbone of modeling that is independent of space
and time resolution, though at the increased cost that is associated with any transient SRS calculation.
SAS also avoids the need for shielding, which for internal flows with multiple walls can suppress turbulence formation in DDES models.
The alternative to SAS is DDES. If proper care is taken to ensure LES mesh quality in the detached flow
regions, the model will be operating in the environment for which it was designed, typically providing
high-quality solutions. DDES has shown advantages for flows at the limit of globally unstable flows (see
Figure 12.43 (p. 192)) where the SAS model can produce URANS-like solutions. In cases like these, DDES
still provides SRS in the separated regions.
For globally unstable flows, the behavior of SAS and DDES is often very similar and they should both
be tried.
12.2.1.3. Meshing Requirements
The part of the domain where the turbulence model acts in RANS mode has to be covered by a suitable
RANS grid. It is especially important that all relevant boundary layers are covered with sufficient resolution
(typically a minimum of 10–15 structured cells across the boundary layer). It is assumed that you are
familiar with grid requirements for RANS simulations.
The estimate for the lowest possible mesh resolution in the detached SRS region is based on the assumption that the largest relevant scales are similar in size to the width of the instability zone. For a
bluff body, the width is the diameter D of the body; for a combustor, the width is the diameter of the
core vortex; for a jet in crossflow, the width is the diameter of the jet; and so on. Experience shows that
the minimum resolution for such flows is of the order:
(12.24)
This resolution requires more than 20 cells per characteristic diameter, (in some applications with
very strong instabilities, even 10 cells across the layer may be sufficient). As is generally the case for
SRS, it is best to provide isotropic (cubic) cells, or at least to avoid large aspect ratios (aspect ratios
smaller than 5 would be optimal, but cannot always be achieved in complex geometries).
With the above estimate for
, there is a good chance of resolving the main flow instability and the
resulting strong turbulent mixing processes associated with the global flow instability (an effect often
missed by RANS models). For acoustics simulations, it might also be important to resolve the turbulence
generated in the (often thin) shear layer that is separating from the body. Resolving this turbulence
poses a much more stringent demand on grid resolution on the simulation, as the shear layer scales
with the boundary layer thickness at separation and so can be much smaller than the body dimension.
This situation is covered in Section 12.2.2 (p. 169).
12.2.1.4. Numerical Settings
The general numerical settings are described in Section 12.3 (p. 197). Globally unstable flows are relatively
forgiving with respect to numerics, at least as far as the mean flow characteristics are concerned. The
recommended choice for the advection terms is the Bounded Central Difference (BCD) scheme, especially
160
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
for complex geometries and flows. For such flows, the classical Central Difference (CD) scheme can be
unstable or produce unphysical wiggles in the solution (see Figure 12.51 (p. 198)). The BCD scheme is
slightly more dissipative, but is substantially more robust and is therefore frequently the optimal choice.
If a visual inspection of the flow (see Section 12.5.1 (p. 202)) shows that turbulence structures are not
produced in agreement with the expectations for the flow, you can switch to CD. If this switch is made,
it is advisable to closely monitor the solution (visually and numerically through residuals) to ensure that
wiggles are not dominating the simulation. With SAS the “Least Square Cell Based” or the “Node-Based
Green Gauss” gradient method should be used in ANSYS Fluent. The latter allows a slightly better representation of the second derivative of the velocity field that is required for the model formulation (von
Karman length scale).
In ANSYS CFX, the default hybrid numerical option switches explicitly between the High Resolution
Scheme (in the RANS region) and the CD scheme (in the LES region). For most applications, it appears
that the use of the BCD scheme should also be favored in ANSYS CFX (see also Section 12.3.1.1 (p. 197))
12.2.1.5. Examples
12.2.1.5.1. Flow around a Fighter Aircraft
Figure 12.12 (p. 162) shows a highly complex, globally unstable flow field, around a generic fighter aircraft
geometry at high angle of attack as computed with the SAS-SST model. The grid consists of 108 hybrid
cells. This simulation is currently in progress within the EU project ATAAC and no detailed discussion
of this flow is intended. Figure 12.12 (p. 162) demonstrates the complex regional appearance of resolved
turbulence around the aircraft. It is obvious that the application of global models like SAS or DDES
greatly simplifies the set up for such flows compared to using ELES/ZLES, where you would have to
define the LES regions and suitable interfaces between the RANS and LES regions in a preprocessing
step. In contracts, when using global models, the simulation is first carried out in standard RANS mode.
Starting from that RANS solution, the model is then simply switched to the SAS or DDES variant of the
RANS model, the solver is set to unsteady mode, and the numeric is adjusted according to Section 12.2.1.4 (p. 160). No further adjustment is required in order to produce the solutions shown in Figure
12.12 (p. 162).
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
161
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.12: Turbulence structures for flow around a generic fighter aircraft (Q-criterion) as
computed by SAS-SST model
12.2.1.5.2. Flow around a Triangular Cylinder
Figure 12.13 (p. 163) shows the grid around a triangular cylinder in crossflow. The Reynolds number
based on the freestream velocity (17.3 [m/s]) and the edge length is 45,500. Periodic boundary conditions
have been applied in the spanwise direction. The simulations have been run with ANSYS Fluent using
the BCD (Bounded Central Difference) and CD (Central Difference) advection schemes and a time step
of
(CFL~1 behind cylinder). The grid features 26 cells across its base. It is extended in the
spanwise direction to cover 6 times the edge length of the triangle with 81 cells in that direction. Due
to the strong global instability of this flow, such resolution was sufficient and has produced highly accurate solutions for mean flow and turbulence quantities (Figure 12.14 (p. 163)).
It should be noted that not all flows produce such strong instability as the triangular cylinder, and a
higher grid resolution might be required for flows with less instability. Figure 12.14 (p. 163) shows that
the grid does not provide resolution of the boundary layer on the walls of the triangular body. This is
not a problem in the current case because the wall boundary layer has no influence on the global flow,
as it separates at the corners of the triangle. In real flows, this might not always be the case and the
boundary layer should be resolved with a RANS-type mesh (that is, a finer mesh in the near-wall region
with higher aspect ratios being acceptable).
162
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
Figure 12.13: Grid around cylinder in crossflow
Figure 12.14 (p. 163) shows a visual representation of the flow using the DDES-SST and the SAS-SST
models with the Q-criterion (see Section 12.5.1 (p. 202)). Both simulations have been carried out using
the BCD scheme. Both models generate resolved turbulence structures in agreement with the expectation
for the grid provided. Figure 12.15 (p. 164) shows a comparison with the experimental data (Sjunnesson
et al., 1992 [27] (p. 213)) for the wake velocity profiles as well as for turbulence characteristics.
Figure 12.14: Turbulence structures for flow around a cylinder in crossflow
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
163
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.15: Velocity profiles and turbulence RMS profiles for three different stations downstream
of the triangular cylinder (x/a=0.375, x/a=1.53, x/a=3.75). Comparison of SAS-SST, DES-SST models,
and experiment. (a) U-velocity, (b) urms, (c) vrms, (d) u’v’
Figure 12.16 (p. 164) shows a comparison of the CD and the BCD scheme for the triangular cylinder using
the SAS-SST model. The turbulence content is almost identical, except that some smaller scales are
present in the CD simulation downstream of the body. A comparison with experimental data showed
results that are almost identical to the ones shown in Figure 12.15 (p. 164) and independent of whether
the CD or the BCD scheme was used.
Figure 12.16: SAS-SST simulation for flow around a triangular cylinder using the BCD and the CD
scheme for the convective fluxes
12.2.1.5.3. ITS Combustion Chamber
The SAS-SST model is applied to the flow in a single swirl burner investigated experimentally by
Schildmacher et al., 2000 [25] (p. 213) at ITS (Institut für Thermische Strömungsmaschinen) of the University
of Karlsruhe. The ITS burner is a simplified industrial gas turbine combustor. It concentrates on the swirl
flow in the combustion region. Similar to the triangular cylinder test case, the wall boundary layers are
164
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
not important, which means that this test case is also accessible to pure LES simulations. However, in
many industrial combustion chambers wall boundary layers and auxiliary pipe flows have to be considered, which makes them unsuitable for pure LES.
There are two co-axial inlet streams and both are swirling in the same direction. The swirl is generated
by means of the two circumferential arrays of blades, which are not included in the current computational domain. The axisymmetric velocity profiles with the circumferential component corresponding
to the given swirl number are used as the inlet boundary conditions. The swirl gives the flow a strong
global instability, which can be captured well by global SRS models.
Figure 12.17 (p. 165) shows the geometry. The grid shown in Figure 12.18 (p. 166) consists of
tetrahedral elements. As stated, the wall boundary layers are not important and are therefore not resolved
on this tetrahedral mesh. The simulation was run with ANSYS CFX, which internally converts the grid
to a polyhedral grid with
control volumes around the grid points for the node-based solver. This
means that the polyhedral grid cells are larger than the visual impression from Figure 12.18 (p. 166) with
~20–30 cells covering the relevant length scale , shown in Figure 12.18 (p. 166). The grid does not
feature any near-wall boundary layer resolution. It is recommended that you provide such a boundary
layer grid for industrial flows (typically more than 10 structured cells across the boundary layer), as in
some geometries the separation characteristics near the burner entrance can depend on such details.
The convection scheme selected was the default hybrid scheme; however, BCD should also work well.
Figure 12.17: Computational domain for the ITS swirl burner
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
165
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.18: Unstructured grid on the symmetry plane and boundary locations for the ITS swirl
burner and relevant length scale, L
The flow structures from the SAS-SST computations of the non-reacting and the reacting flow at a given
instance in time are shown in Figure 12.19 (p. 167) using the
-criterion (
, see Sec-
tion 12.5.1 (p. 202)). The isosurface in Figure 12.19 (p. 167) is given by
. The
main turbulence structures seem to be captured well in the simulations. Clearly, small-scale turbulence
cannot be resolved on such a grid. The grid resolution used here should not be considered as a recommendation for combustion chambers, but as the lowest limit for which such SRS models can be applied.
Figure 12.20 (p. 168) shows a comparison of the standard
RANS and SAS results at a given distance
from the burner entrance. It shows the level of improvement that results from the application of SRS
methods. Many more details of this simulation can be found in Egorov et al., 2010 [6] (p. 212) or in a
more detailed analysis of a more complex combustion chamber in Widenhorn et al., 2009 [37] (p. 214).
166
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
Figure 12.19: SAS solution for ITS combustion chamber (a) Non-reacting, (b) Reacting flow
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
167
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.20: Reacting flow velocity profiles at the axial distance from the inlet x=103 mm (a)
Axial velocity, (b) Tangential velocity
168
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
12.2.2. Locally Unstable Flows
12.2.2.1. Flow Physics
The expression “locally unstable flows” is not easily defined, as every turbulent flow is by nature unstable.
It is meant to characterize flows that also produce new turbulence, typically downstream of a geometry
change, but where the flow instability producing this turbulence is significantly weaker than for globally
unstable flows.
Consider the computation of a mixing layer starting from two wall boundary layers in RANS mode (see
Figure 12.21 (p. 169)). As the flat plate ends, the two boundary layers form a turbulent mixing layer,
which quickly becomes independent of the turbulence of the two boundary layers on the flat plate
(yellow circles). The mixing layer instability (red) provides for a de-coupling of the boundary layer and
the mixing layer turbulence. For this reason, you can neglect the boundary layer turbulence downstream
of the trailing edge (the dashed yellow boundary layer turbulence sketched in Figure 12.21 (p. 169)) and
concentrate on using SRS mode to resolve the mixing layer turbulence, which will quickly dominate
the flow.
Figure 12.21: Schematic of locally unstable flow: Mixing layer originating from a flat plate with
two boundary layers of different freestream velocity. Full yellow circles are boundary layer
turbulence. Dashed yellow circles are remains of the boundary layer turbulence. Red arrows are
new mixing layer turbulence
Examples of locally unstable flows:
• Generic Flows
– All equilibrium free-shear flows emanating from walls (jets, wakes, mixing layers)
– Backward-facing step flow
– Weakly interacting equilibrium flows
– Flows with weak swirl
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
169
Best Practices: Scale-Resolving Simulations in ANSYS CFD
12.2.2.2. Modeling
The goal in SRS is to cover the boundary layer turbulence (solid yellow circles in Figure 12.21 (p. 169))
in RANS and the mixing layer turbulence (red in Figure 12.21 (p. 169)) in resolved mode. This can only
be achieved if the impact of the RANS turbulence model is significantly reduced downstream of the
trailing edge; otherwise the formation of unsteady structures would be suppressed.
The SAS model will typically not switch to SRS mode in such situations, independent of the mesh
provided, as the eddy-viscosity produced in the mixing layer will be too large for the flow instability at
hand. From a pure turbulence modeling standpoint, this is often acceptable, as such flows are typically
covered with reasonable accuracy by using RANS models (mixing layers, wakes, back step, and so on).
However, in cases where unsteady information is required for other reasons (for example, acoustics),
the SAS model will likely not be suitable, unless an interface is used that converts modeled turbulence
energy into resolved energy (see Section 12.1.5 (p. 156)).
DDES allows SRS behavior, as the shielding function is turned off past the trailing edge of the plate,
and the eddy-viscosity is reduced, assuming a fine (LES) grid is provided downstream of the plate. The
DDES model then switches to LES mode in the wake, and the mixing-layer instability is strong enough
to generate resolved turbulence relative quickly (within a few boundary layer thicknesses). It is important
to point out that the ability of the DDES model to generate unsteady structures in the mixing layer
depends on the grid provided in that area. Assuming an overly coarse grid (for example, in the spanwise
direction), the DES limiter would not engage and the model would stay in RANS mode, which will not
enable the formation of resolved structures. Remember that the DES length scale is defined as:
(12.25)
where
is the largest edge length for each cell. For this case, assume that the grid in the
plane
shown in Figure 12.21 (p. 169) is very fine (of LES quality), and
is the grid resolution in the
spanwise ( ) direction. Conversely, if
is very coarse, the DES limiter would always select the RANS
length scale and the model would remain in RANS mode in the wake region. No unsteady structures
would develop as the RANS model will damp them out. As the grid in the -direction is refined, the
DES limiter will be activated at some location downstream of the trailing edge where
(note
that grows as the mixing layer becomes thicker). With further grid refinement, the location of the
implicit RANS-LES interface would move closer to the trailing edge. Eventually, the entire mixing layer
would be covered by LES. This behavior of (D)DES is both a disadvantage and an advantage. The disadvantage and the danger lie in the strong grid sensitivity introduced explicitly into the turbulence
model. As a result, you must be very careful to provide a suitable grid for a given application when
using DDES. The advantage is that the model can be applied to locally unstable flows without the
definition of an explicit RANS-LES interface. However, the grid sensitivity can be reduced by employing
an interface which converts modeled turbulence to resolved turbulence using the DDES model upstream
and downstream of the interface (see Section 12.1.5 (p. 156)).
The most general approach to the flows discussed here is the use of the embedded or zonal RANS-LES
methods, where the boundary layers are covered by a RANS model and the mixing layer by a LES
model. The models are explicitly switched from RANS to LES at a pre-defined interface upstream or at
the trailing edge. In order to obtain a proper LES solution, a grid with LES resolution is required in the
mixing layer. Frequently a non-conformal interface between the RANS and the LES part is used to reduce
the grid resolution in the upstream RANS region. For a fully consistent simulation, one must introduce
synthetic turbulence at the RANS-LES interface. By such injection of synthetic turbulence, the balance
between RANS and LES turbulence across the interface is preserved (that is, the yellow dashed circles
in Figure 12.21 (p. 169) are accounted for).
170
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
The recommendation for flows with local instabilities is to use ELES/ZLES models if the geometry and
the application enable the definition of well-defined interfaces (for example, internal flows, like pipe
flows). Synthetic turbulence should be introduced at these interfaces in order to preserve the balance
between the RANS and LES turbulence content. Should the geometry/application be complex such that
the definition of explicit RANS and LES zones is not easily possible (for example, turbomachinery flows,
external flows), apply the DDES model. However, ensure careful tailoring of the grid with sufficient
resolution on the LES region to avoid undefined model behavior somewhere between RANS and LES
mode. It is advisable to refrain from using conventional DES in flows with extensive boundary layers,
as the danger of affecting the boundary layers is too high.
It is very important to understand that for locally unstable flows, failure to capture the instability of the
Separating Shear Layer (SSL) can have a pronounced effect on the solution downstream. The turbulence
field is a result of this initial instability and missing it can severely limit the resolved content of the
simulation and contaminate an expensive SRS solution. This danger is much reduced with ELES/ZLES
models, (relative to DDES) because the flow enters the SSL with a prescribed synthetic turbulent content
from the RANS-LES interface.
12.2.2.3. Meshing Requirements
In order to generalize the concepts discussed for the mixing layer example (Figure 12.21 (p. 169)), we
introduce the terminology of a Separating Shear Layer (SSL). It refers to the shear layer that starts at
the point of separation from the body and moves into a free shear flow (we are not considering small
separation bubbles embedded within the boundary layer). In Figure 12.21 (p. 169) the SSC would be the
mixing layer forming downstream of the plate. In other flows it can be a separating boundary layer
from a corner. In the case of locally unstable flows, the
spacing should be sufficiently small to
enable resolution of the initial flow instability of the SSL. The main quantity of relevance is the ratio of
RANS to grid length scale:
(12.26)
It is important to emphasize that this quantity must be evaluated based on a precursor RANS solution.
This implies that such a solution exists and is meaningful. If the precursor solution is not available, then
you can estimate the ratio based on the thickness of SSL. For equilibrium mixing layers, the following
ratio is approximately correct:
(12.27)
where
is the thickness of the mixing layer. The value of RL should be:
(12.28)
where 0.2 should be considered an extreme lower limit of resolution and 0.1 the desirable lower limit.
Again, higher grid resolution should be used if computing power permits. The value of
corresponds to a resolution of 15 cells across the mixing layer. This amount of cells is not a very fine grid
resolution, but equal resolution should ideally be provided in all three space dimensions. In addition,
the SSL can be thin relative to the body dimensions, resulting in very high computational costs. The
initial SSL instability is akin to a Helmholtz instability and is initially two-dimensional. Two times the
coarser grid spacing in the spanwise direction is therefore acceptable.
It is not always possible to achieve such resolution directly from the onset of the separating shear layer,
especially if this layer is very thin relative to the body dimensions. This inability is not necessarily a
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
171
Best Practices: Scale-Resolving Simulations in ANSYS CFD
problem as, typically, the thickness of the SSL increases strongly downstream of the separation point/line.
Therefore
is decreasing relatively quickly and reaches sufficiently low values to provide the required
resolution. It is important to note that for cases where the small scales play a significant role, such as
in acoustics simulations, the delay of the initial instability can result in a loss of spectral information at
high wave numbers (small scales). It is advisable to visually inspect the displayed results for the presence
of the unsteady turbulent structures at the intended locations.
Of special concern are geometries with high aspect ratios, meaning a large domain size in the direction
perpendicular to the SSL (long cylinders in crossflow, stalled wings of high aspect ratios, and so on). In
such situations, it is not always possible to sufficiently resolve the third direction. It might then be necessary to solve only a portion of the real flow domain in SRS mode, either by using suitable boundary
conditions (for example, periodicity in the spanwise direction), or by restricting the SRS to a limited
portion of the domain.
12.2.2.4. Numerical Settings
The general numerical settings described in Section 12.3 (p. 197) should be applied. In addition, locally
unstable flows can be very sensitive with respect to numerics. For the application of the DDES model,
the recommended choice for the advection terms is the Bounded Central Difference (BCD) in the entire
domain. The PRESTO pressure interpolation should be avoided in such simulations, as it has been observed that this option can suppress the initial formation of resolved turbulence.
Experience suggests that the BCD scheme is also the most suitable choice when using ELES/ZLES
methods. In some applications with high demands on accuracy and where a high quality isotropic mesh
can be provided in the LES region, the application of the CD scheme in the LES zone might be advantageous.
12.2.2.5. Examples
12.2.2.5.1. Backward-Facing Step I
The backward-facing step flow experimentally investigated by Vogel and Eaton, 1985 [34] (p. 214) was
computed. In this flow, the height of the channel upstream of the step is equal to four step heights
( ). A summary of the physical parameters is given in Shur et al., 2008 [26] (p. 213):
Table 12.3: Parameters for simulation of a backward-facing step
28 000
0.02
1.0
The computational domain for the test case is shown in Figure 12.22 (p. 173). The characteristic length
is the step height, , which is equal to 1 [m] in the current study. The domain dimension in -direction
is equal to
. The domain upstream of the step has dimensions in the - and -directions of
and
respectively. The downstream domain has dimensions in the - and -direction, of
and
respectively.
172
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
Figure 12.22: The computational domain for the Backward-Facing Step test case
An example of the computational grid used for the test case is shown in Figure 12.23 (p. 173). The grid
has 2.25 million hexahedral cells (2.3 million nodes) providing a near-wall resolution in wall units to be
less than one. A non-dimensional time step (based on step height and inlet velocity) of
ensures
that the CFL number is less than unity in the unsteady mixing zone downstream of the step. The
number of cells in the spanwise direction is 80. The solution was averaged over 5000 time steps.
In Figure 12.23 (b) (p. 173) all boundary conditions are shown. In the spanwise direction (cyan colored
boundary), a periodic boundary condition was applied; on the red-colored boundaries, no-slip wall
conditions were applied; on the blue-colored boundary, an outlet condition was applied; and on the
green-colored boundary, an inlet condition was applied. The latter was provided in the form of steadystate RANS profiles. Therefore, unsteadiness resulted solely from the local flow instability past the step.
Figure 12.23: Computational grid (a), (c) and applied boundary conditions (b) for Backward-Facing
Step test case
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
173
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.24 (p. 174) shows turbulent structures visualized by an isosurface of the -criterion colored
with the streamwise velocity. It can be seen that these structures develop quickly downstream of the
step due to the local flow instability.
Figure 12.24: Isosurface of Q-criterion equal to Q=1 [non-dimensional with Uinlet and H] colored
by velocity using the DDES-SST model
While test cases of the type discussed in Section 12.2.1 (p. 158) with strong global instabilities are relatively
insensitive to modeling and numerical details, cases with only local instabilities are much more fragile.
Figure 12.25 (p. 175) to Figure 12.27 (p. 175) show a comparison of the time-averaged skin-friction coefficient distribution for different model variants and solver settings. In particular, Figure 12.25 (p. 175)
shows that the details of the formulation of the DDES shielding function can have a strong effect on
such flows. The use of the conservative function
of the SST model delays the formation of resolved
turbulence structures and so delays flow reattachment. For this reason, the shielding functions of the
DDES-SST model have recently been optimized and the new DDES-SST shielding function proposed in
Gritskevich et al., 2012 [11] (p. 212) is recommended (and used in the current simulation).
The selection of the Central Difference (CD) scheme vs. the Bounded Central Difference (BCD) scheme
did not show any significant impact on the solution as is seen in Figure 12.26 (p. 175).
However, the selection of the pressure interpolation scheme proved to be quite influential as shown
in Figure 12.27 (p. 175). Figure 12.28 (p. 176) shows the consequences of missing or delaying the flow
instability of the SSL. The model does not really operate in LES mode through a significant part of the
recirculating region as shown in Figure 12.28 (b) (p. 176). Similar behavior can be observed on underresolved grids. It is worth re-iterating that this effect is less likely to be a problem in globally unstable
flows. The effect can largely be avoided by using the ELES formulation, where unsteady structures are
introduced at the RANS-LES interface. The solution does not depend as critically on the resolution of
the first few shear layer thicknesses downstream of the step and on the numerical settings as critically
as it does with DDES.
174
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
Figure 12.25: Skin friction coefficient for different turbulence models (F1 is the first SST model
blending function, F2 is the second SST model blending function, FD is the new DDES shielding
function)
Figure 12.26: Skin friction coefficient for DDES with different advection schemes
Figure 12.27: Skin friction coefficient for DDES with different pressure interpolation schemes
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
175
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.28: Strongly delayed shear layer instability due to numerics settings (a) Standard
pressure interpolation (b) PRESTO scheme
12.2.3. Stable Flows and Wall Boundary Layers
12.2.3.1. Flow Physics
Stable flows in this context are characterized by a continuous development of the turbulence field. For
such flows, the turbulence at a certain location depends strongly/entirely on the turbulence upstream
of it. There is no mechanism for quickly generating new turbulence and over-riding the upstream turbulence field. Stable flows in the context of this discussion are essentially wall-bounded flows, which
are either attached or have small separation bubbles.
• Generic Flows
– Channel and pipe flows (attached and mildly separated)
– Boundary layers (attached and mildly separated)
12.2.3.2. Modeling
For stable flows, the use of embedded or zonal RANS-LES methods with a well-defined interface between
the RANS and the LES zone is essential. Synthetic turbulence must be introduced at the RANS-LES interface to ensure a proper balance between the modeled and the resolved content of turbulence. The introduction of resolved turbulence allows the balance between RANS and LES turbulence across the interface to be preserved (assuming the synthetic turbulence is of sufficient quality). Neither DDES nor
176
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
SAS-type models are able to switch from RANS to SRS mode in such stable situations. Even in cases
where resolved turbulence is specified at the inlet (or an interface) these models will typically switch
back to their underlying RANS mode after some boundary layer thicknesses (see Davidson, 2006
[4] (p. 212)).
Even an explicit switch from a RANS to a LES model (and the corresponding grid refinement in the LES
zone) at the interface without an introduction of synthetic turbulence does not work well. If sufficient
resolution is provided in the LES zone, the flow would eventually go through a transitional process and
recover the fully turbulent state. However, such a process would require many boundary layer thicknesses,
with an entirely unbalanced model formulation in-between. This method is not acceptable in most
technical flows and must be avoided.
In such stable flows, the most suitable selection of hybrid RANS-LES models are Embedded- or Zonal
models, where the RANS and the LES zones are user-defined and synthetic turbulence is injected at the
RANS-LES interface. As mentioned previously, the RANS-LES interface should be placed in a non-critical
region of the flow (equilibrium flow), since existing synthetic turbulence generators do not provide
realistic turbulent fluctuations for strongly non-equilibrium flows. As a result, placing the interface in
such regions results in a too-slow relaxation from synthetic to "real" turbulence (typically, several
boundary layer thicknesses).
As an alternative, the RANS and LES simulations can be carried out separately. The RANS domain would
include the full geometry whereas the LES solution can be carried out on a smaller portion of the original domain. This separate LES domain would be identical to the LES zone in the equivalent ELES setup. The information from the larger RANS solution can then be mapped onto the boundaries of the
LES domain. Synthetic turbulence should be introduced at the inlet of the LES domain. This approach
can be used if you are confident that the physical decoupling has very little or no effect onto the
overall flow topology. The advantage of the decoupled method over the ELES approach is that the
RANS solution does not have to carry the burden of the excessive temporal resolution that the LES
domain would have otherwise required. However, you should be aware that some scripting is required
for mapping the results from RANS to LES in the decoupled approach.
The models selected in the RANS and LES zone depend on the flow physics. In the RANS zone, a suitable
model for the flow should be selected. In the LES zone, the use of a WMLES formulation is typically recommended for wall boundary layers in order to avoid the unfavorable Reynolds number scaling of
classical LES models. For free shear flows, the WALE model should provide optimal performance.
12.2.3.3. Meshing Requirements
Figure 12.29 (p. 178) shows the schematic of an ELES set-up. There is a central area (red), which is the
domain of interest (for example, a boundary layer with a separation bubble). This area is not specifically
defined in the ELES set-up, but is just used to demonstrate how such a zone would be handled. Clearly,
you would not place the LES zone (green) directly at the start of the zone of interest, but extend it
upstream and downstream of that region by several boundary layer thicknesses as indicated in Figure
12.29 (p. 178). For fully developed pipe/channel flow, the boundary layer thickness should be estimated
as half of the pipe diameter/channel height. The LES zone is then embedded into a larger RANS zone
(blue).
The meshing requirements are those of the underlying turbulence models. In the RANS zone typical
RANS resolution requirements should be satisfied (20–30 cells across the wall boundary layer with
possibly a
and 15–20 cells across free shear flows).
In the LES zone, the resolution requirements depend on the details of the LES model formulation and
the flow type. For free shear flows, cubic grid cells with a minimum of
cells per shear layer
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
177
Best Practices: Scale-Resolving Simulations in ANSYS CFD
thickness should be used. For wall-bounded flows, the resolution requirements are those described in
Section 12.1.3.1 (p. 145) for classical LES and in Section 12.1.4 (p. 154) for WMLES.
Figure 12.29: Sketch of embedded LES (ELES) domain
For wall-bounded flows, it is clear that large domains cannot be covered in SRS mode, even when using
WMLES. In most cases you would limit the domain size of the LES zone by one or more of the following
concepts:
• Use only a limited spanwise domain size.
– Apply periodic boundary conditions where appropriate. The domain size has to cover a minimum of 3–5
boundary layer thicknesses in the spanwise direction to avoid inaccuracies caused by the spanwise periodicity condition. Care must be taken that this requirement is satisfied for the entire LES domain. In case
the boundary layer grows in the streamwise direction, the most downstream location is relevant for the
estimate.
– In cases where no periodicity can be applied, place the spanwise interfaces into a region of limited interest.
• Place the upstream RANS-LES interface economically to reduce the size of the LES domain. However, the
interface should be located in a zone of undisturbed equilibrium flow. Place the RANS-LES interface at a
minimum of ~3 boundary layer thicknesses upstream of the zone of interest (for example, a separation region).
Limit the size of the RANS-LES interface to the shear layer you want to capture; that is, do not extend the
interface far into the freestream, as the code will then generate resolved turbulence in freestream regions
where no LES is required. The Vortex Method (VM) would also generate a large number of vortices if the
RANS-LES interface were too large.
• Place the downstream LES-RANS interface economically to reduce the size of LES domain. However, do not
place the interface immediately downstream of the zone of interest, but place it several boundary layer
thicknesses farther downstream to avoid any negative influence of the downstream RANS model (this approach enables the boundary layer to recover several boundary layer thicknesses downstream of a separation
before switching back to RANS)
• Limit the height of the LES zone, but allow for some space above the boundary layer. Typically the LES zone
should be about twice as thick as the boundary layer.
178
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
In order to check the quality of the simulation, sensitive quantities like time-averaged wall shear stress
should be plotted across the RANS-LES zones. There should be no large jump in those quantities and
the unavoidable disturbance caused by the interface should be recovered before entering the zone of
interest.
12.2.3.4. Numerical Settings
Zonal methods typically enable a separate selection of numerical settings in the RANS and LES zones.
For very sensitive simulations, you can therefore select a pure Central Difference (CD) in the LES domain,
while using an appropriate numerical scheme in the RANS parts. However, you can also select a global
scheme, in which case the Bounded Central Difference (BCD) scheme is recommended.
12.2.3.5. Examples
12.2.3.5.1. Periodic Channel
The periodic channel flow is not an ELES, but a WMLES application. This section of the report shows
that as WMLES is typically used in the LES portion of ELES/ZLES applications. The entire domain is
WMLES and there are no RANS-LES interfaces. Simulations of this flow have been carried out assuming
incompressible fluid at several Reynolds numbers based on friction velocity
and channel height
, Re = 395, 760, 1100, 2400, and 18000. The flow is driven by a constant pressure gradient
, where is the pressure and is the density. This pressure gradient is taken into
account in the governing equations via a source term in the momentum equations, which allows imposing periodic boundary conditions not only in the spanwise direction , but also in the streamwise
direction . Note that within such an approach, the bulk velocity of the flow is not specified and should
be obtained as a part of the solution, which means that it could be different with different turbulence
models. Alternatively, you can specify the mass flow and the solver will adjust the imposed pressure
gradient accordingly.
The size of the computational domain shown in Figure 12.30 (p. 180) is equal to
in the streamwise
direction and
in the spanwise direction. For all considered Reynolds numbers, the computational
grid is unchanged in the streamwise and spanwise directions with a uniform grid-spacing of
and
respectively. This gives 10 cells per channel half width,
, ( being the relevant boundary
layer thickness) in the streamwise and 20 cells per in the spanwise direction. Different grids have
been used in the wall-normal direction. This arrangement provides a sufficient resolution (
near
the wall) at different Reynolds numbers. Note, however, that all simulations could have been performed
on the finest grid. The non-dimensional time step is
, which ensures that the CFL number
is
in the entire domain. The solution was averaged in time over 5000 time steps.
Table 12.4 (p. 180) gives the details of the grids used in the simulations and the resulting non-dimensional
grid spacing. Note that classical wall-resolved LES would require values of
,
, demonstrating the substantial savings that can be achieved with WMLES for higher Re numbers. The
range
in Table 12.4 (p. 180) covers the range of
values in the wall normal direction, with the largest values
located at the center of the channel.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
179
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.30: Computational domain and grid for WMLES of channel flow
Table 12.4: Grid resolution for WMLES channel flow simulations
Cell Number
Node
Number
395
384 000
40.0
20.0
760
384 000
76.9
38.5
1100
480 000
111.4
55.7
2400
528 000
243.0
121.5
18000
624 000
1822.7
911.4
Figure 12.31 (p. 180) shows the turbulence structures using the
are colored, and show the streamwise velocity.
-criterion (
). The isosurfaces
Figure 12.31: Turbulence structures for WMLES of channel flow at lowest Reynolds number (Q=350
[s-2])
Figure 12.32 (p. 181) shows the flow in a horizontal cut through the domain for the lowest and the
highest Reynolds numbers. The thin region of RANS modeling near the wall for the high Reynolds
number is indicated by the high eddy-viscosity (note the different scales in the plot for the eddy-viscosity
ratio for the different Reynolds numbers). RANS modeling in this context is as described in Section 12.1.4 (p. 154), based on the near-wall mixing length formulation.
180
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
Figure 12.32: Flow visualization for WMLES of channel flow (a) Vorticity rate Omega, (b) Absolute
value of velocity U, (c) Ratio of eddy-viscosity to molecular viscosity
Results of the WMLES formulation and their comparison with the empirical correlation of Reichart, 1951
[22] (p. 213) are shown in Figure 12.33 (p. 182). You can see that the WMLES solutions reproduce the
logarithmic layer with good accuracy. There is a slight kink at the switch from the RANS to the LES formulation, but it is moderate and does not affect global properties such as the wall shear stress.
The above simulations have been carried out with ANSYS Fluent. Similar results can be obtained with
ANSYS CFX where WMLES is the default formulation inside the LES zone of the ZFLES method.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
181
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.33: Resolved normal stresses, turbulent kinetic energy, and mean velocity profiles for
WMLES at different Reynolds numbers
12.2.3.5.2. Wall Boundary Layer
The zero pressure gradient wall boundary layer is a benchmark test case that is commonly used for
turbulence model investigation due to its geometric and physical simplicity. Unlike the periodic channel
test case, the wall boundary layer needs unsteady boundary conditions because there is no periodicity
in the streamwise direction. In the current simulations, the Vortex Method (VM) was used for these
purposes (Mathey et al., 2003 [15] (p. 213)).
A computational domain for this test case is shown in Figure 12.34 (p. 183). The characteristic length,
which determines the geometry, is the plate length, , of 1 [m] in the current study. Dimensions of the
computational domain in , , and directions are equal to ,
, and
respectively.
182
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
Figure 12.34: Computational domain for a Wall Boundary Layer test case
The simulations have been performed for an incompressible fluid. A summary of physical parameters
is presented in Table 12.5 (p. 183).
Table 12.5: Properties for flat plate boundary layer simulations
Inlet boundary layer
thickness
1000
10 000
0.032
0.032
0.001
0.001
1.0
1.0
The geometry and the computational grid used for the test case are shown in Figure 12.35 (p. 184). The
base grid is uniform in the - and -directions with steps 0.004 [m] and 0.002 [m] respectively. In the
wall normal direction the grid was expanded by a factor of 1.15. For all computations the value of
is less than 1, which means that the governing equations are integrated to the wall. A complete summary
of all used grids is presented in Table 12.6 (p. 184).
Figure 12.35 (b) (p. 184) presents all the boundary condition types used in the simulations. The cyan
color shows one of the periodic planes, the red color the no-slip wall boundary, the blue color the
outlet boundary, the green color the inlet boundary, and the yellow color the symmetry boundary.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
183
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.35: Computational grid (a), (c) and applied boundary conditions (b)
Table 12.6: Information on grids for flat plate test case
Cell Number
Node Number
1000
1 085 000
68.0
34.0
10 000
1 333 000
680.0
340.0
Two cases have been computed using the numerical grids with the parameters shown in
Table 12.6 (p. 184). They have different inlet Reynolds numbers that are based on the boundary layer
momentum thickness (
).
The Non-Iterative Time Advancement (NITA) algorithm based on the Fractional Time Step method was
applied with the second order scheme for the approximation of time derivatives. The convective terms
in the momentum equations have been approximated with the second order Central Difference scheme
and the Green-Gauss cell-based method was used for interpolation of variables on cell faces. The
Standard option was selected for the pressure interpolation scheme.
Visualizations of the flow at two values of
are shown in Figure 12.36 (p. 185). Isosurfaces of the
-criterion that are equal to
and colored with the velocity magnitude are depicted. It can be
seen that the turbulence structures are well-developed and do not show any visual decay or disruption
downstream of the inlet. This indicates that the Vortex Method provides sufficiently realistic turbulent
content at the inlet boundary.
184
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
Figure 12.36: Isosurfaces of Q-criterion (Q=200 [s–2]) colored with velocity for a flat plate at two
different Reynolds numbers
Figure 12.37 (p. 186) shows the skin-friction coefficient for the two Reynolds numbers. The results
demonstrate that the inlet wall friction provided by the RANS inlet velocity profiles is maintained without
any major disruption. This indicates again that the vortex method produces sensible synthetic inlet
turbulence. In addition, the models react properly to the Reynolds number variation, suggesting that
the WMLES can maintain a boundary layer accurately even at high Reynolds numbers, where standard
LES models would fail due to a lack of resolution. Figure 12.37 (a) (p. 186) shows the impact of the
pressure interpolation scheme, which has proven to be critical for locally stable flows. As seen in Figure
12.37 (p. 186), the effect of the PRESTO scheme turns out to be not as pronounced in the fully developed
turbulent boundary layers as it has been in the backward-facing step example shown in Figure
12.37 (p. 186). It is worth re-iterating that the PRESTO scheme requires slightly more running length to
recover the correct levels of turbulence and wall shear stress.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
185
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.37: Skin friction distributions along a flat plate predicted by WMLES at two Reynolds
numbers (a) Re theta=1000 with different numerical settings (b) Re theta =10 000
Figure 12.38 (p. 187) shows Reynolds stresses and velocity profiles from the simulations. The figure
suggests that, just as for the channel flow, the quality of the simulations is fairly high in terms of both
the mean flow prediction (the logarithmic profile is reproduced faithfully) and Reynolds stresses (they
are well within the range expected from known DNS studies of the flat plate boundary layer).
186
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
Figure 12.38: Profiles of resolved normal and shear Reynolds stresses and mean velocity in the
flat plate boundary layer predicted by WMLES at two Reynolds numbers (a) Re theta=1000 with
different numerical settings (b) Re theta=10 000 with the second order pressure interpolation
The above simulations have been carried out with ANSYS Fluent. Similar results can be obtained with
ANSYS CFX where WMLES is the default formulation inside the LES zone of the ZFLES method.
12.2.3.5.3. NASA Hump Flow
A challenging test case for ELES in combination with WMLES was computed within the EU project
ATAAC. The case models the flow over a hump with a relatively large separation zone on the leeward
side. Figure 12.39 (p. 187) shows the experimental set-up (Greenblatt et al., 2005). Due to the limited
separation zone, this flow would be categorized as a stable flow in the present context.
Figure 12.39: Experimental set-up for NASA hump flow experiment
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
187
Best Practices: Scale-Resolving Simulations in ANSYS CFD
The flow was computed with ANSYS Fluent 13.0 using the SST model in the RANS zone, the vortex
method at the RANS-LES interface and the algebraic WMLES option in the LES zone. The Reynolds
number, based on the free-stream velocity,
, and hump chord, , is equal to
. The simulation
was carried out in the full domain, which extends from
to
(0 corresponds to the hump beginning). In the spanwise direction, the extent of the domain is
. The inflow boundary conditions
for RANS have been set based on the preliminary flat plate boundary layer computations up to the flow
section
(
), where the parameters of the incoming boundary layer have been
measured in the experiment. At the upper wall of the channel, free-slip wall conditions have been
specified.
The grid in the LES zone (see Figure 12.40 (p. 188)) consists of
cells and was designed
to provide
cells per boundary layer volume in the streamwise, wall normal, and spanwise
directions. The RANS grid is much coarser, especially in the spanwise direction. Figure 12.40 (p. 188) also
presents a visualization of the turbulent structures in the LES zone that suggests a high resolution
provided by the simulation (note that the momentum thickness Reynolds number at the inlet to the
LES domain is relatively high (
)). In retrospect, the set-up might not be fully optimal, as the
RANS-LES interface is placed relatively close to the non-equilibrium/separation zone of the boundary
layer. There are only about two boundary layer thicknesses between the interface and the bend of the
geometry. A more optimal grid should cover more of the upstream boundary layer and enable the
synthetic turbulence to develop over a longer running length.
Figure 12.40: (a) Grid used for the NASA hump simulation (b) Turbulent structures in the LES
domain (Q-criterion colored with spanwise velocity component)
Figure 12.41 (p. 189) shows the skin-friction and wall-pressure coefficient distributions from the simulations.
It can be seen that the use of ELES combined with the WMLES model in the LES zone results in very
close agreement with the data, even though the skin-friction is known to be very sensitive to simulation
details. A comparison of the results obtained using WMLES with those obtained using the standard
WALE model in the LES zone is shown in Figure 12.41 (p. 189). The results suggest that the latter performs
considerably worse than the former. In particular, in the simulations using the WALE model, the wall
shear stress drops immediately after the RANS-LES interface to unrealistically small values due to the
lack of resolution. The results with this model further downstream are therefore no longer reliable as
the wall shear stress has a strong influence on the overall boundary layer development. Further investigations of this flow are on-going, so the results should not be considered final, but are provided to
demonstrate the basic concepts.
188
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
Figure 12.41: (a) Skin-friction, cf, and (b) Wall pressure coefficients, cp, from NASA hump flow
simulations. Comparison of WMLES and WALE LES methods in the LES domain
12.2.3.5.4. T-Junction with Thermal Mixing
The following example is a flow through a pipe T-junction with two streams at different temperatures
Westin et al., 2006 [36] (p. 214). This test case was used as a benchmark of the OECD to evaluate CFD
capabilities for reactor safety applications. This flow is not easily categorized in the current framework.
It can be placed somewhere between a globally and a locally unstable flow. As shown below, this flow
can be modeled with SAS and DDES, but special care must be taken in choosing the numerical settings.
The set-up consists of a horizontal pipe for the cold water flow, and a vertically oriented pipe for the
hot water flow. The hot water pipe is attached to the upper side of the horizontal cold water pipe. In
the experiments, the length of the straight pipes upstream of the T-junction is more than 80 diameters
for the cold water inlet, and approximately 20 diameters for the hot water inlet. The flow conditions
are listed in Table 12.7 (p. 189).
Table 12.7: Flow conditions for T-Junction test case
Diameter
Bulk velocity
Mass
flow
Temperature
Re number
Hot
Pipe
Cold
Pipe
A sketch of the domain is depicted in Figure 12.42 (p. 191). The domain dimensions are as follows. The
hot leg inlet is located at the
section, the cold leg inlet is located at the
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
section,
189
Best Practices: Scale-Resolving Simulations in ANSYS CFD
and the outlet is located at
, with being the diameter of the cold leg of the pipe. When
ELES was used, two additional interfaces have been introduced in the domain, where the synthetic
fluctuations generated with the use of the Vortex Method have been specified. These sections have
been placed at
in the hot leg and at
in the cold leg.
The computational grid for this flow comprises about 4.9 million hexahedral cells (see Figure
12.42 (p. 191)). The wall normal grid spacing was set to 0.0001 [m], which yields
in the
entire domain. The grid spacing in the axial and circumferential directions was set as follows:
• For the cold water pipe where the inlet boundary layer thickness
spacing was chosen
and
and
is equal to 0.07 [m], the grid
, which yields
.
• For the hot water pipe the inlet boundary layer thickness
was chosen
and
was set to 0.022 [m] and the grid spacing
, which yields
and
.
• In wall units, the grid spacing is (
,
) (195, 80) for the hot water pipe and (
) (115, 70) for the cold water pipe, which means that the flow requires near-wall turbulence modeling. The time step was set to 0.001 [s], which leads to CFL~1 in the central mixing zone.
190
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
,
Generic Flow Types and Basic Model Selection
Figure 12.42: Geometry and grid of T-Junction test case with measurement planes
The boundary conditions for this case have been specified as follows. For the inlet boundaries, the
precursor simulations of the pipe flow have been performed using the SST model. For the cold water
pipe, a fully developed pipe flow was calculated using the SST model and the profiles of velocity and
turbulence quantities have been specified at the inlet boundary. For the hot leg and the pipe, the profiles
in the experiments were not fully developed. For this reason, a separate pipe flow simulation was conducted using constant inlet values for velocity and turbulence. The inlet profiles for the hot leg have
then been extracted from this precursor simulation at the location where they matched the experimental
profiles most closely.
It bears repeating that this flow is not easily categorized into one of the three groups described above,
but might be described as between globally unstable and locally unstable. It was originally computed
with the global SAS and DDES models. Although both simulations turn into a proper SRS mode in the
interaction zone of the two streams, the results turned out to be very sensitive to numerical details and
solver settings, especially for the SAS model. As an illustration, in Figure 12.43 (p. 192), the turbulence
structures are shown as predicted by the SAS-SST model with the use of the CD and BCD numerical
schemes. The effect of the scheme on the resolved flow is striking. This effect is an indication that the
underlying flow instability is not very strong and can only be represented by the SAS model with the
use of a low dissipative numerical scheme such as CD in this particular case. Under such conditions, it
is not advisable to apply global methods like SAS (and to a lesser extent, DDES), as will be seen from
the temperature distributions later. It is important to emphasize that in more unstable flows, the difference between CD and BCD is not nearly as strong and often barely noticeable.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
191
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.43: Turbulence structures for SAS-SST model (a) Central Difference (CD) scheme, (b)
Bounded Central Difference (BCD) scheme
It is therefore recommended to apply the ELES model with synthetic turbulence specified at predefined
RANS-LES interfaces located in both pipes upstream of the interaction zone. Switch from the RANS to
LES at these interfaces using the vortex method. In this case, the SST model was employed in the RANS
zone and the WMLES approach was used in the LES part of the domain. As seen in Figure 12.44 (p. 193),
with this approach resolved turbulence is generated well-upstream of the interaction zone and is then
maintained through the interaction zone independent of the numerical scheme (CD or BCD).
192
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
Figure 12.44: Vorticity contours for ELES/WMLES simulation (a) CD scheme, (b) BCD scheme
Figure 12.45 (p. 194) shows velocity profiles of different velocity components at different measurement
locations (see Figure 12.42 (p. 191)). Figure 12.45 (a) (p. 194) shows results for the DDES, ELES/WMLES,
and SAS simulations using the CD scheme. All simulations agree well with each other and with the experimental data. Figure 12.45 (b) (p. 194) shows the same models, but computed using the BCD scheme.
As discussed, the SAS/BCD model shows marked differences compared to the experimental data, as
already expected from Figure 12.43 (p. 192). It stays in URANS mode, which for this case turns out to be
inadequate. The other models are less sensitive to the numerical set-up and provide almost identical
results when using the BCD and the CD scheme.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
193
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.45: Comparison of the experimental and computational velocity profiles for T-Junction
flow for different turbulence models (a) CD scheme (b) BCD scheme (note that scales of coordinate
axes change by large factors between curves)
From an application-oriented standpoint, the most important outcome of these simulations is the
thermal mixing and the resulting wall temperature distributions. Results for the different simulations
are shown in Figure 12.46 (p. 195) to Figure 12.49 (p. 196). The comparison is depicted for four lines located
on the wall of the main pipe downstream of the intersection at the Top ( ), Front ( ), Bottom (
),
and Rear (
) (see Figure 12.42 (p. 191)). One can find significant differences between the global and
the ELES formulations, especially on the top wall. The temperature mixing is more accurately predicted
with the ELES model because the transitional process between RANS and LES is not well-defined in
global models. While the solution of global hybrid models is much better than URANS (not shown here),
the details can still be missed in the initial mixing zone. The ELES method is more consistent, as it
provides a clear interface where modeled and resolved turbulence are exchanged (RANS-LES interface
with synthetic turbulence). Because of that, well-defined resolved turbulence is already present upstream
of the junction, thereby avoiding the ambiguities of the formation of resolved turbulence in the interaction zone.
194
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Generic Flow Types and Basic Model Selection
Figure 12.46: Comparison of the experimental and computational wall temperature distributions
for T-Junction flow at the Top wall (0 degrees, see Figure 12.42 (p. 191)) of the main pipe
Figure 12.47: Comparison of the experimental and computational wall temperature distributions
for T-Junction flow at the Front wall (90 degrees, see Figure 12.42 (p. 191)) of the main pipe
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
195
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Figure 12.48: Comparison of the experimental and computational wall temperature distributions
for T-Junction flow at the Bottom wall (180 degrees, see Figure 12.42 (p. 191)) of the main pipe
Figure 12.49: Comparison of the experimental and computational wall temperature distributions
for T-Junction flow at the Rear wall (270 degrees, see Figure 12.42 (p. 191)) of the main pipe
Details of the resolved turbulence can be seen in Figure 12.50 (p. 197), which shows the region just
downstream of the pipe intersection on the Top wall ( - Figure 12.42 (p. 191)) where the temperature
predictions between ELES and DDES differ the most (Figure 12.46 (p. 195)). ELES shows significantly
stronger resolved turbulence activity than DDES, confirming the arguments above.
196
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Numerical Settings for SRS
Figure 12.50: Comparison of turbulence structures on the Top wall downstream of the pipe
intersection (a) DDES model (b) ELES model
12.3. Numerical Settings for SRS
This chapter discusses:
12.3.1. Spatial Discretization
12.3.2. Pressure (ANSYS Fluent)
12.3.3.Time Discretization
12.3.1. Spatial Discretization
12.3.1.1. Momentum
SRS models, as described in Scale-Resolving Simulation (SRS) Models – Basic Formulations (p. 141), serve
the main purpose of dissipating the energy out of the turbulence spectrum at the limit of the grid resolution. The eddy viscosity is defined to provide the correct dissipation at the larger LES scales. This
assumes that the numerical scheme is non-dissipative and that all dissipation results from the LES
model. For this reason, one is required to select a numerical scheme in the LES region with low dissipation, relative to the dissipation provided by a subgrid LES model. Another strategy is to avoid the introduction of the LES (subgrid) eddy viscosity and provide all damping through the numerical scheme.
This approach is called MILES (Monotone Integrated Large Eddy Simulation) (Boris et al., 1992 [1] (p. 212)).
In ANSYS CFD, the standard LES methodology is followed, whereby the dissipation is introduced by a
LES eddy viscosity model and the numerical dissipation is kept at a low value.
In order to achieve low numerical dissipation, you cannot use the standard numerical schemes for
convection that were developed for the RANS equations (Second Order Upwind Schemes, or SOU),
which are dissipative by nature. In contrast, LES is carried out using Central Difference (CD) schemes.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
197
Best Practices: Scale-Resolving Simulations in ANSYS CFD
In industrial simulations, second order schemes are typically employed, however, in complex geometries
with non-ideal grids, CD methods are frequently unstable and produce unphysical wiggles (see Figure
12.51 (p. 198)), which can eventually destroy the solution. To overcome this problem, variations of CD
schemes have been developed with more dissipative character, but still much less dissipative than Upwind
Schemes. An example is the Bounded Central Difference (BCD) scheme of Jasak et al., 1999 [14] (p. 213).
Figure 12.51: Example of scheme oscillations in T-Junction flow shown by vorticity: (a) CD, (b)
BCD
The CD scheme can be used successfully for (WM)LES of simple flows on optimal grids (typically hexahedral grids with low skew) such as channel or pipe flows. For more complex geometries, ELES allows
the reduction of the LES domain to a limited region with high quality grids. Under such conditions, CD
can be employed inside the LES portion of the grid, while using a standard upwind biased scheme for
the RANS part of the domain.
For global models, like SAS or DDES, involving RANS and LES portions without a well-defined interface
between them, most cases require the use of the BCD scheme, which can also handle both the RANS
and LES domains with acceptable accuracy.
When using ELES in ANSYS Fluent, one can also switch the numerical scheme between the RANS and
the LES regions (see Cokljat et al., 2009 [2] (p. 212)) by hand.
In ANSYS CFX, the default for the SAS and DDES models is a numerical scheme that switches explicitly
between a second order upwind and the CD scheme, based on the state of the flow, using a switch
proposed by Strelets, 2001 [32] (p. 214). This switching scheme is relatively complex and it is advisable
to apply the less complex BCD scheme that is also available in the code. In ANSYS CFX there is an additional parameter for the BCD scheme that allows a continuous variation of the scheme from BCD to
CD. The parameter is called CDS Bound. CDS Bound=1 applies only to BCD and CDS Bound=0 applies
only to CD.
198
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Numerical Settings for SRS
12.3.1.2. Turbulence Equations
The spatial discretization of the convection terms of the turbulence model is not critical in SRS, as the
models are dominated by their source terms. The first order upwind scheme is therefore sufficient for
these equations, but second order is also suitable.
12.3.1.3. Gradients (ANSYS Fluent)
The selection of a specific gradient method is not of much relevance to SRSs on high quality hexahedral
meshes. For skewed or polyhedral meshes, the Least Square Method (LSM) is recommended. For the
SAS model one should use the LSM or the Green-Gauss Node Based (GGNB). The latter allows a slightly
higher sensitivity to initial instabilities.
12.3.2. Pressure (ANSYS Fluent)
SRS can be relatively sensitive to the pressure interpolation. Validation studies have shown that the
PRESTO scheme is more dissipative than the other options and should be avoided unless required for
other reasons. For the validation studies, the standard pressure interpolation was typically used.
12.3.3. Time Discretization
12.3.3.1. Time Integration
Time integration should be carried out with the second order backward Euler scheme. This has proven
to have sufficient accuracy for a wide range of applications. For turbulence (and other positive) variables,
use the Bounded Second Order Implicit Euler scheme (this must be selected in ANSYS Fluent and is the
default in ANSYS CFX).
The time steps should be selected to achieve a Courant number of
in the LES part of the domain.
For complex geometries and grids with high stretching factors, the definition of the CFL number is not
always very reliable (for example, if the flow passes through a region of highly stretched cells). In such
situations, estimates can be built upon the physical dimensions of the shear layer to be resolved. If
cubic cells are required for resolving a shear layer (say
across a mixing layer of thickness )
and a certain CFL number is to be achieved, then a time step of
(12.29)
is required. Considering that is proportional to the RANS turbulent length scale
of order 1), this estimate may be further simplified to:
(with a constant
(12.30)
where
simulation.
. This simplification means that the time step
can be estimated on a pre-cursor RANS
You can also apply a more global estimate by assessing the through flow time, which is the time required
by a fluid element to pass through the LES domain of length
timate of how many cells,
with velocity
:
, will be passed along this trajectory, one obtains
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
. With an es.
199
Best Practices: Scale-Resolving Simulations in ANSYS CFD
12.3.3.2. Time Advancement and Under-Relaxation (ANSYS Fluent)
There are several different settings for time advancement in ANSYS Fluent. The first choice is between
the Iterative (ITA) and the Non-Iterative Time Advancement (NITA). NITA should be checked for any new
application as it can result in significant CPU savings. As a general guideline, NITA works well on high
quality grids and for flows with limited additional physical coupling between the equations. Within
NITA, the fractional step scheme is recommended; however, one must be very cautious and conservative
with the assessment of the time step size. An attempt to perform a simulation with CFL>1 can lead to
an incorrect solution. In addition, one should reduce residual tolerance for all equations to 0.0001.
For the ITA schemes (everything except NITA), the segregated solvers are typically faster than the
coupled solver. The optimal choice is in most cases the SIMPLEC scheme. The default under-relaxation
parameters for this scheme are set for steady-state simulations. For SRS model simulations, they should
be changed to values as close as possible to 1 to improve iterative convergence. Typically, the number
of inner iteration loops (
10–20) required with SIMPLEC depends on the complexity of the flow
problem. The most critical quantity is the mass conservation. Mass residuals should decrease by at least
one order of magnitude every time step.
The coupled solver is slower per iteration, but it can lead to more robust convergence, and for complex
cases can be advantageous. For the coupled solver, one would typically also specify under-relaxation
values of (or close to) 1. The number of inner loops is typically
5-10. In ANSYS CFX, the coupled
solver is used in all simulations.
For flows with additional physics (multiphase, combustion, and so on), the number of inner iterations
per time step can increase significantly for all solvers.
It is important to emphasize that the optimal under-relaxation factors and the optimal number of inner
iterations is case-dependent. Some optimization might be required for achieving the most efficient
results.
12.4. Initial and Boundary Conditions
This chapter discusses:
12.4.1. Initialization of SRS
12.4.2. Boundary Conditions for SRS
12.4.3. Symmetry vs. Periodicity
12.4.1. Initialization of SRS
In most cases it is best to initialize the SRS model using a RANS model solution. This recommendation
is especially true for global hybrid RANS-LES models (SAS, DDES), which are based on an underlying
RANS model.
For pure LES or WMLES, ANSYS Fluent offers an option for initializing the flow by converting turbulence
from RANS to LES mode (solve/initialize/init-instantaneous-vel) using a synthetic
turbulence generation routine. This option should be used with caution as it can, at times, have a detrimental effect on the robustness of the simulation. It should be executed mainly for cases where no
synthetic turbulence is generated at an inlet/interface and where the inherent flow instability is not
strong enough to generate resolved turbulence on its own. A typical example would be the LES of a
channel flow with periodic boundary conditions in the streamwise direction. For such flows, the solver
could return a laminar solution even at super-critical (turbulent) Reynolds numbers if no initial disturbance
is provided.
200
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Initial and Boundary Conditions
In ANSYS CFX, synthetic turbulence is generated automatically in the first time step inside the LES region
of a ZLES set-up.
12.4.2. Boundary Conditions for SRS
12.4.2.1. Inlet Conditions
Inlet conditions should be selected based on the physics of the flow and applied in a similar manner
as RANS computations.
For global models (SAS, DDES), use standard (typically steady-state) RANS inlet conditions.
For LES or WMLES, provide synthetic turbulence at the inlet.
12.4.2.2. Outlet Conditions
If possible, outflow or average pressure is better than constant pressure outlets as vortices carry nonconstant pressure distributions across the boundary. For certain acoustics calculations, like jet noise,
use non-reflecting boundary conditions.
12.4.2.3. Wall Conditions
For all models except LES, use low
values of around
. The models are formulated in a -insensitive fashion, so larger values of
can be tolerated as long as the overall boundary layer resolution is
sufficient.
For LES, one would typically have to apply wall functions in order to avoid the large resolution requirements near the wall. The wall resolution in streamwise ( ), normal ( ) and spanwise ( ) directions are
coupled.
(12.31)
12.4.3. Symmetry vs. Periodicity
In most cases, periodicity or slip conditions cannot be employed in regions that border on zones of
resolved turbulence, even if the geometry and the time-averaged flow are symmetric with respect to
a given plane. The reason is that unsteady turbulence does not obey symmetry instantaneously. The
application of symmetry boundaries would therefore impose an unphysical constraint onto the resolved
scales. It is therefore essential to either compute the full domain, or to apply periodicity at such planes
if possible (for example, if there is a matching plane at the other end of the domain).
Symmetry and slip wall conditions can be used if the resolved turbulence is confined to regions not
touching these boundaries.
Periodicity conditions can lead to problems for axi-symmetric situations. As the radius approaches zero,
the circumferential size of the domain goes to zero, and periodicity conditions would not enable turbulence structures of finite size to exist. An example is the flow in an axi-symmetric pipe. If you were to
compute that flow in a pipe segment with periodicity conditions in the circumferential direction, you
would restrict the size of the resolved eddies to zero near the axis. This effect is not correct and would
substantially alter the solution. Such a simulation would therefore have to be carried out in full
mode. Note that the situation would be different in the case of the flow through a ring segment, where
the axis is excluded from the SRS domain. Periodicity could be applied in the case of
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
201
Best Practices: Scale-Resolving Simulations in ANSYS CFD
with
being the outer radius,
1 or larger.
the inner radius of the segment and
being a constant of the order
12.5. Postprocessing and Averaging
This chapter discusses:
12.5.1. Visual Inspection
12.5.2. Averaging
12.5.1. Visual Inspection
The first and most important step in any SRS model is the visual inspection of the turbulence structures.
This is typically done using an isosurface of the -criterion. The definition of is:
(12.32)
where in different definitions the constant might be different (for historic reasons,
in ANSYS
Fluent and
in ANSYS CFD-Post). The value of the constant
is typically unimportant as we
are only interested in visual impressions when using this quantity. In this definition, is the absolute
value of the Strain Rate and is the absolute value of vorticity.
(12.33)
The rationale behind this definition is that we want to visualize vorticity, which characterizes turbulence
vortices, but also to subtract the mean shear rate in order to avoid displaying steady shear layers (where
).
There are different definitions of , some of them non-dimensional. Avoid using non-dimensional
values as they can be mainly used for visualization of free vortices and their dynamics (for example, tip
vortex of an airplane wing). In turbulent flows, they can elevate very weak turbulence structures to the
same level as the strong ones and thereby produce an incorrect picture.
In ANSYS Fluent, the variable is called “ criterion” (under Turbulence) and in ANSYS CFD-Post “Velocity.Invariant ” in the variable list. Both codes also have a non-dimensional version of (ANSYS Fluent:
“Normalized q criterion ,” ANSYS CFD-Post: “Location / Vortex Core Region, Method = -Criterion”),
which are not suitable for turbulence vortex fields.
The dimensional
to
-values can be very large and can vary greatly in the domain. Frequently, values up
can be found in high Re number flows. In such cases, isosurfaces in the range of
are typically sensible. You must experiment with some values for the isosurface before
obtaining a suitable picture. It might be helpful to first plot on a fixed surface as a contour plot and
select the correct scaling from that contour plot. Use positive values for the isosurface. Do not use
for visualization, as it will show very weak structures not relevant to turbulence visualizations.
202
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Postprocessing and Averaging
It is also advisable to color the isosurface of
with some other variable. Interesting quantities are the
eddy-viscosity ratio (
), or a velocity component that is small or zero in RANS (such as the spanwise
velocity), or the CFL number, and so on. The visual inspection should be done continuously during the
entire start-up and run time of the simulations (once per day or after every 1000 time steps). It serves
the following purposes (see for example Figure 12.13 (p. 163) and Figure 12.14 (p. 163)): • Check if unsteady turbulence develops at all and at the expected locations.
• Check large scale symmetries/asymmetries of the flow.
• Check the solution for numerical wiggles (odd-even decoupling)
• Check the size of the resolved eddies and see if they are as one would expect from the grid resolution.
• Check the CFL number on these eddies. It should be smaller than CFL 1. Check the eddy-viscosity ratio. It
should be much smaller than RANS.
• Check for global SRS turbulence models (SAS/DDES) if the turbulence structures develop early in the separating shear layer or if a noticeable delay is observed (see Figure 12.28 (b) (p. 176)).
• Check for ELES/Unsteady inlet conditions, if synthetic turbulence is reasonable and does not decay (such
as in Figure 12.36 (p. 185)).
• Check the progress of the simulation towards a statistically converged solution. This means that the resolved
turbulence requires some time until it has developed and has been transported through the domain. Timeaveraging has to wait until that stage has been achieved.
• Include pictures of turbulence structures in any reports of the test case (slides, reports, publications, service
requests).
• If possible make animations, which help to understanding of the flow physics and is also helpful for others
to understand the flow.
• Add monitoring points at interesting locations and plot their development in time to demonstrate statistical
convergence.
For all examples in this report, visual representations of the flows are included. These serve as a guideline
on how to process the results.
12.5.2. Averaging
Unsteady simulations with scale resolution require special care in postprocessing and averaging. Engineers
are usually interested only in time-averaged results and not in the details of the unsteady flowfield. It
is therefore important to follow a systematic approach when computing such quantities.
The typical process is to start from a RANS solution (or reasonable initial condition). When switching to
any SRS model, the flow will require some time to statistically settle into a new state for the following
reasons: • The resolved turbulence requires some time to develop and be transported through the domain.
• The global flow topology might change from the initial (RANS) solution.
• Other physical effects might require longer start-up times (such as multi-phase).
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
203
Best Practices: Scale-Resolving Simulations in ANSYS CFD
The general strategy is therefore to run the simulation for some start-up time
, before activating
the averaging process (or initiating the acquisition of, for example, acoustics information). When should
this process be started and how long does it take until the flow is statistically steady? This is the stage
where any increase in
would not change the averaged solutions. Unfortunately
depends
strongly on the flowfield and no general guidelines can be given. For some flows, the flow develops
quickly (in a few thousand time steps). For others it takes tens of thousands of steps to reach that point.
However, a first estimate can be obtained by estimating throughflow time,
. This is the time that
the mean flow requires to pass one time through the domain
where
is the length
of the domain and
is the mean flow velocity. The turbulence statistics typically require several (35) throughflow times to establish themselves. Again, this is just a rough estimate and can depend on
the particular flow.
In order to determine
more systematically, one must monitor the simulation. It is advisable to
monitor some local and some global quantities. • Continuously inspect the solution visually with the aid of regular images and updated animations.
• Inspect solution variables at monitor points in the critical zone of simulation (pressure, velocity, temperature,
and so on) as a function of time. The amplitude and frequency of local oscillations should become regular
before the averaged statistics can be gathered.
• Monitor global quantities (forces on body, massflow, integrated swirl, and so on). Interesting quantities are
often those that would be zero for RANS (spanwise forces, and so on) as they are sensitive to the SRS characteristics. They also help to evaluate the overall symmetry of the solution (they should fluctuate around
zero) and to determine slow transients (quantities that fluctuate around zero but with low overlaid frequencies).
Only when all indicators show that the flow is no longer changing statistically (meaning only the details
of the turbulence structures are a function of time) should the averaging be activated. It is important
to document the number of steps that have already occurred when averaging was started and how
many steps have been averaged. With respect to averaged quantities: • Monitor time-averaged quantities and ensure that they are not “drifting.” They will drift initially, but should
then settle to an asymptotic value.
• Ensure that they satisfy the symmetry conditions of the flow. Any asymmetry is an indicator of non-convergence (exceptionally, there are flows that develop physical asymmetries despite a symmetric set-up. Example:
some symmetric diffusers separate from one side and stay attached on the other).
• Ensure that the averaged quantities are smooth.
• In zonal/embedded simulations, check if averaged quantities are reasonably smooth across RANS-LES interfaces (they will never be perfectly smooth, but should also not change drastically).
12.6. Summary
An overview of hybrid Scale-Resolving Simulation (SRS) technologies was given. Due to the nature of
the subject, only a rough outline of the models could be provided. The rational and the advantages/disadvantages of each model family have been discussed. Based on the description of the models, an attempt has been made to categorize flows into sub-classes, and to map the modeling strategies onto
these classes. It should be emphasized again, that the proposed categories are not easily and clearly
defined and have significant overlap. Still it is considered necessary to explain that no single SRS model
204
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Summary
is suitable for all applications and it is not possible to generalize about which model should be used
for which type of flow.
In principle, ELES and ZFLES, in combination with WMLES are suitable for all flows, but require a substantial amount of preprocessing work to define the corresponding zones and provide suitable grids
for all of them. For complex applications, this is not always feasible/practical and the global models
(SAS, DDES) are favored. However, as detailed, they work only if a sufficient level of instability is present
in the flow. If in doubt, it is better to select the safer option, over the more convenient one.
Details on many aspects of SRS have been provided, ranging from numerics, to grid resolution all the
way to postprocessing. Numerous examples have been shown to enable the reader to properly place
the intended application into this framework. It is anticipated that the document will evolve over time,
as new questions are posed by users and as the SRS models themselves will evolve.
A brief summary of the more important points is provided in the Appendices.
12.6.1. Acknowledgment
The material in this report was prepared with the help of members of the turbulence team at ANSYS
Jochen Schütze, Yuri Egorov, Richard Lechner, as well as with the help of the colleagues at NTS in St.
Petersburg Mikhail Gritskevich and Andrey Garbaruk. Aleksey Gerasimov at ANSYS has provided a very
thorough review, which has resulted in the removal of numerous inconsistencies and has significantly
improved the quality and readability of the document. Some of the test cases have been run in the
framework of the EU projects DESIDER and ATAAC.
12.6.2. Appendix 1: Summary of Numerics Settings with ANSYS Fluent
Unsteady Simulation
Comment
Convection
Terms
CD / BCD
CD on simple geometries (also inside LES
regions). In case of wiggles in solution
use BCD (most industrial cases)
Pressure
Discretization
Any except PRESTO
Use PRESTO only if required for other
reasons. Note that the initial formation
of turbulence structures can be delayed
(inhibited) with PRESTO.
Velocity
Gradients
Least Squares Cell Based
No significant impact on SRS, typically
Least Square Cell Based. For the SAS
model one should use the Least Square
Cell Based, or the Green-Gauss Node
Based (GGNB). The latter allows a slightly
higher sensitivity to initial instabilities.
Iterative
Method
SIMPLEC
NITA/Fractional step only for simple flows
Monitor convergence: at least 1 order in
mass conservation. SIMPLEC with 5–10
inner loops.
For cases that are difficult to converge
try the coupled solver. More expensive,
but potentially lower inner iterations
required.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
205
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Unsteady Simulation
Comment
Increase Under-Relaxation Factors to
values ~1
Under-relaxation URF 1
Start with all URF 1 (typically 0.8–0.95).
Reduce in case of convergence problems.
Lower values for additional physics
(combustion, multi-phase, and so on).
Time
Discretization
Use CFL<1 in LES zones if possible. This
condition can also be relaxed depending
on the flow and CFL~5 was used for the
T-junction test case successfully.
Second order backward
Euler
Bounded for second order turbulence
quantities ( , , ) and other positive
quantities (volume fraction, and so on).
12.6.3. Appendix 2: Summary of Numerics Settings With ANSYS CFX
Convection
Terms
Unsteady Simulation
Comment
CD / BCD
CD on simple geometries (also inside LES
regions). In case of wiggles in solution
use BCD
The default scheme for DDES and SAS is
a hybrid scheme that switches
automatically between High Res and CD.
Recent experience indicates that BCD is
generally easier to apply and often yields
the same accuracy.
CDS Bound enables shifting between the
classical BCD scheme and the Central
Difference scheme.
Time
discretization
Second order backward
Euler
Use CFL<1 in LES zones if possible. This
condition can also be relaxed depending
on the flow.
Bounded for second order turbulence
quantities is default ( , , ) and other
positive quantities (volume fraction, and
so on).
12.6.4. Appendix 3: Models
Scale-Adaptive
Simulation
(SAS)
Applications
Comments
• Use for globally unstable
flows
• Safest SRS model, as it has URANS
fallback position on coarse grids/time
steps
• Use CFL~1 for best
results (higher CFL
206
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Summary
Applications
possible but less
resolution)
Comments
• Danger of falling into URANS mode if
flow instability is not strong
• Avoid PRESTO scheme
• Check Q-criterion
carefully during run time
to ensure SRS structures
Detached
Eddy
Simulation
(DES)
• Use for globally unstable
flows and with care also
for locally unstable flows
• Always use DDES to
avoid impact of DES
limiter on attached
boundary layers, use
DDES shielding function
• More aggressive than SAS in terms of
unsteadiness
• Careful grid generation important,
otherwise danger of gray zones or
grid-induced separation
• Grid in SRS region must
be of LES quality, no
RANS fallback position
• Use CFL~1
• Avoid PRESTO scheme
• Check -criterion
carefully during run time
to ensure SRS structures
Large
Eddy
Simulation
(LES)
• Use for free shear flows
• Typically too expensive for
wall-bounded flows
• Use if boundary layers
are laminar
• Use for turbulent
boundary layers only
with high grid resolution
at low Reynolds
numbers
• Use CFL~1
• Apply synthetic
turbulence at inlets
• Check -criterion
carefully during run time
to ensure SRS structures
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
207
Best Practices: Scale-Resolving Simulations in ANSYS CFD
Wall
Modeled
LES
(WMLES)
Applications
Comments
• Use for wall boundary
layers at moderate and
high Reynolds numbers
• Scales much more favorably with
Reynolds number than standard LES but
still very expensive
• Resolve boundary layer
volume (
) by
cells
• Limit wall region to a small portion of
flow domain (ELES)
• Use CFL~1
• Apply synthetic
turbulence at inlets
• Check -criterion
carefully during run time
to ensure SRS structures
Embedded
LES (ELES)
Zonal
Forced
LES
(ZFLES)
• Use for wall boundary
layers at moderate and
high Reynolds numbers
• Resolve boundary layer
volume (
) by
cells
• Allows flexible combination of models
in different parts of the domain.
• If wall boundary layers in LES domain,
consider using WMLES (default in CFX)
• Use CFL~1
• Apply synthetic
turbulence at RANS-LES
interface
• Check -criterion
carefully during run time
to ensure SRS structures
Vortex
Method
(VM) –
Fluent
• Use to generate
synthetic turbulence at
RANS-LES interface or
LES (WMLES) inlet
• Grid in LES region of interface must be
of LES quality
• Restrict interface zone to
the minimal section
where turbulence must
be converted (do not
extend LES zone far into
the freestream)
• If large RANS-LES
interface cannot be
avoided increase (and
check) the number of
208
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Summary
Applications
Comments
vortices specified. Can
be as high as 104.
• Use CFL~1
• Check Q-criterion
carefully during run time
to ensure SRS structures
Harmonic
Turbulence
Generator
(HTG) CFX
• Restrict inlet zone to the
LES minimal section
where turbulence must
be converted (do not
extend LES zone far into
the freestream)
• Grid in LES region of interface must be
of LES quality
12.6.5. Appendix 4: Generic Flow Types and Modeling
Table 12.8: Globally Unstable Flows
Examples
• Flows past bluff bodies
– Flow past buildings
– Landing gears of airplanes
– Baffles in mixers
– Side mirrors of cars
– Stalled wings/sails
– Trains/trucks/cars in crossflow
– Tip gap of turbomachinery blades
– Flows past orifices, sharp nozzles, and so on.
• Flows with strong swirl instabilities
– Flow in combustion chambers of gas turbines
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
209
Best Practices: Scale-Resolving Simulations in ANSYS CFD
– Some tip vortex flows in adverse pressure gradients
– Flows past vortex generators
• Flows with strong flow interaction
– Impinging/colliding jets
Modeling
• SAS model is safest option as it has RANS fall-back
position
• DDES in case SAS does not show sufficient content
of resolved turbulence. Provide suitable LES grid in
LES region
• Often SAS and DDES give very similar solutions.
• ELES typically not required
Critical
• Visually check turbulent structures
• Run flow until statistically converged
Table 12.9: Locally Unstable Flows
Examples
• Flows with large separation zones (< boundary layer
thickness)
– Backward-facing step type flows
– Bump flows with large separation
– Cavity flows
– Mixing layer leaving plate/trailing edge
• Flows with weak swirl instabilities
– Flames with low or zero swirl
• Flows with weak flow interaction
210
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Summary
– Jet in crossflow with low momentum ratio
Modeling
• Use ELES where geometry permits
• DDES on high quality grids and low dissipation
numerics (CD/BCD)
Critical
• Instability of Separating Shear Layer (SSL) must be
resolved with DDES quickly. ELES is safer as it provides
unsteady inlet to separation zone but generally much
more expensive
• Visually check turbulent structures in SSL
Table 12.10: Stable Flows
Examples
• Attached and mildly separated wall bounded flows
– Boundary layers
– Channel/pipe flows
Modeling
• LES in separate domain if possible
– WMLES for higher Re numbers
– Maybe interpolate larger domain RANS solution
onto LES zone boundaries
– Use unsteady (synthetic) turbulence at inlet,
preferred Vortex Method
• ELES in combined RANS-LES simulation
– Define LES zone as detailed in
Section 12.2.3 (p. 176). Extend LES zone to leave
space around critical area.
– Place RANS-LES interface into region of uncritical
flows (such as equilibrium boundary layers)
Critical
• Visually check turbulent structures
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
211
Best Practices: Scale-Resolving Simulations in ANSYS CFD
• Provide sufficient grid resolution in (WM)LES zones
especially for wall-bounded flows
(Section 12.2.3.3 (p. 177)).
• CFL number<1.
12.7. Scale-Resolving Simulations References
[1] Boris, J. P., Grinstein, F. F., Oran, E. S., and Kolbe, R. S. “New insights into Large Eddy Simulation”. Fluid
Dynamic Research. Vol. 10. 199-228. 1992.
[2] Cokljat D., Caradi D., Link G., Lechner R., and Menter F.R. “Embedded LES Methodology for GeneralPurpose CFD Solvers”. 22-24 June 2009. Proc. Turbulent Shear Flow Phenomena, 6th Int. Symp.
Turbulence and Shear Flow Phenomena. Seoul, Korea. . 1191-1196.
[3] Comte-Bellot, G., and Corrsin, S. “Simple Eulerian time correlation of full- and narrow-band velocity
signals in grid-generated, “isotropic” turbulence”. Journal of Fluid Mechanics. Vol. 48, Part 2. 273337. 1971.
[4] Davidson, L. “Evaluation of the SAS-SST Model Channel Flow, Asymmetric Diffuser and Axi-Symmetric
Hill”. Proceedings European Conference on Computational Fluid Dynamics . ECCOMAS CFD. .
2006.
[5] Durbin, P., and Pettersson Reif, B.A. Statistical theory of turbulent flows. John Wiley and Sons, Ltd. UK.
2003.
[6] Egorov Y., Menter F.R., and Cokljat D. “Scale-Adaptive Simulation Method for Unsteady Flow Predictions.
Part 2: Application to Aerodynamic Flow”. Flow Turbulence and Combustion. Vol. 85, No. 1. 139165. 2010.
[7] Fröhlich J., Mellen C.P., Rodi W., Temmerman L., and Leschziner M. “Highly resolved large-eddy simulation of separated flow in a channel with streamwise periodic constrictions”. Journal of Fluid
Mechanics. Vol. 526. 19–66. 2005.
[8] Fröhlich J., and von Terzi, D. “Hybrid LES/RANS methods for simulation of turbulent flows”. Progress in
Aerospace Sciences. Vol. 44, Issue 5. 349-377. 2008.
[9] Girimaji, S. S. “Partially-Averaged Navier-Stokes Method: A RANS to DNS Bridging Method”. 2004.
[10] Girimaji, S., and Abdul-Hamid, K.S. “Partially-averaged Navier-Stokes model for turbulence: implementation and validation”. AIAA Aerospace Sciences Meeting and Exhibit. Reno, Nevada. . 2005-0502.
2005.
[11] Gritskevich, M.S. Garbaruk, A.V., Schütze, J., and Menter F.R. “Sensitization of DDES and IDDES Formulations to the
Shear-Stress Transport Model”. Flow Turbulence and Combustion. 2012.
[12] Guerts, J. B. Elements of direct and large-eddy simulation. Edwards Inc. Philadelphia, USA. 2004.
[13] Hanjalic, K., and Launder, B. Modelling Turbulence in Engineering and the Environment. Cambridge
University Press. Cambridge, UK. 2011.
212
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Scale-Resolving Simulations References
[14] Jasak H., Weller H.G., and Gosman A.D. “High Resolution Differencing Scheme for Arbitrarily Unstructured
Meshes”. International Journal for Numerical Methods in Fluids. Vol. 31. 431-449. 1999.
[15] Mathey, F., Cokljat, D., Bertoglio, J.P., and Sergent, E. “Specification of LES Inlet Boundary Condition
Using Vortex Method. 4th International Symposium on Turbulence, Heat and Mass Transfer. Antalya, Turkey. . 2003.
[16] Menter, F. R. “Two-equation eddy-viscosity turbulence models for engineering applications”. AIAA
Journal. Vol. 32, No. 8. 1598–1605. 1994.
[17] Menter F.R., Garbaruk A., and Smirnov P. “Scale adaptive simulation with artificial forcing”. Proc. 3rd
Symposium on Hybrid RANS-LES Methods . . 2009.
[18] Menter, F.R., and Egorov, Y. “Scale-Adaptive Simulation Method for Unsteady Flow Predictions. Part 1:
Theory and Model Description”. Flow, Turbulence and Combustion . Vol. 85, No. 1. 113– 138. 2010.
[19] Menter, F.R., and Kuntz, M. “Adaptation of Eddy-Viscosity Turbulence Models to Unsteady Separated
Flow Behind Vehicles”. Proc. Conf. The Aerodynamics of Heavy Vehicles: Trucks, Busses and Trains.
Asilomar, California. Springer . . 2002.
[20] Michelassi V., Wissink, J. G., and Rodi W. “Direct numerical simulation, large eddy simulation and unsteady Reynolds-averaged Navier-Stokes simulations of periodic unsteady flow in a low-pressure
turbine cascade: A comparison”. Journal of Power and Engineering . Vol 217, Number 4. 403– 411.
2003.
[21] Nicoud, F., and Ducros, F. “Subgrid-scale stress modelling based on the square of the velocity gradient
tensor”. Flow, Turbulence and Combustion . Vol. 62. 183– 200. 1999.
[22] Reichardt, H. “Vollstandige Darstellung der turbulenten Geschwindigkeitsverteilung in glatten Leitungen”.
Zeitschrift fur Angewandte Mathematik und Mechanik . Vol. 31. 208– 219. 1951.
[23] Rotta, J.C. “Turbulente Strömumgen”. BG Teubner Stuttgart. 1972.
[24] Sagaut, P., Deck, S., and Terracol, M. Multiscale and multiresolution approaches in turbulence. Imperial College Press. London. 2006.
[25] Schildmacher, K.-U., Koch, R., Wittig, S., Krebs, W., and Hoffmann, S. “Experimental investigations of
the temporal air-fuel mixing fluctuations and cold flow instabilities of a premixing gas turbine
burner”. ASME Paper 2000-GT-0084. 2000.
[26] Shur, M.L., Spalart, P.R., Strelets, M.K., and Travin, A.K. “A hybrid RANS-LES approach with delayed-DES
and wall-modeled LES capabilities”. International Journal of Heat and Fluid Flow . Vol. 29. 16381649. 2008.
[27] Sjunnesson, A., Henriksson, R., and Lofstrom, C. “CARS measurements and Visualization of Reacting
Flows in Bluff Body Stabilized Flame”. AIAA Paper 1992–3650. 1992.
[28] Smagorinsky, J. “General Circulation Experiments with the Primitive Equations”. Monthly Weather Review.
Vol. 91. 99 – 165. 1963.
[29] Spalart, P.R., Jou, W., Strelets, M., and Allmaras, S. “Comments on the feasibility of LES for wings, and
on a hybrid RANS/LES approach”. Advances in DNS/LES. 1st AFOSR Int. Conf. on DNS/LES. . 1997.
[30] Spalart, P. R. “Strategies for turbulence modelling and simulations”. International Journal of Heat and
Fluid Flow. Vol. 21. 2. 2000.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
213
Best Practices: Scale-Resolving Simulations in ANSYS CFD
[31] Spalart, P., Deck, S., Shur, M., Squires, K., Strelets, M., and Travin, A. “A New Version of Detached Eddy
Simulation, Resistant to Ambiguous Grid Densities”. Journal of Theoretical and Computational Fluid
Dynamics. Vol. 20. 181 –195. 2006.
[32] Strelets, M. “Detached Eddy Simulation of massively separated flows”. AIAA Paper 2001-879. 2001.
[33] Travin, A., Sur M., Strelets, M., and Spalart P. “Physical and numerical upgrades in the detached eddy
simulation of complex turbulent flows , In Advances in LES of complex flows ”. eds. R. Friedrich, W.
Rodi . Kluwer Acad. New York. 239-254. 2000.
[34] Vogel, J.C., and Eaton, J.K. “Combined heat transfer and fluid dynamic measurements downstream of
a backward-facing step”. Journal of Heat and Mass Transfer. Vol. 107. 922 –929. 1985.
[35] Wagner, C., Hüttl, T., and Sagaut, P. “Large-eddy simulation for acoustics”. Cambridge University Press.
2007.
[36] Westin, J., Alavyoon F., Andersson, L. Veber, P., Henriksson, M., and Andersson, C. “Experiments and
Unsteady CFD-Calculations of Thermal Mixing in a T-Junction” . OECD/NEA/IAEA Workshop on the
Benchmarking of CFD Codes for Application to Nuclear Reactor Safety (CFD4NRS). Munich, Germany. . 1–15. 2006.
[37] Widenhorn, A., Noll, B., and Aigner, M. “Numerical Study of a Non-Reacting Turbulent Flow in a Turbine
Model Combustor”. AIAA Paper 2009-647, Orlando Florida . 2009.
[38] Wilcox, D.C. “Turbulence Modeling for CFD”. DCW Industries Inc. 3rd Edition. 2006.
214
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 13: CFX Command Language (CCL)
The CFX Command Language (CCL) is the internal communication and command language of ANSYS
CFX. It is a simple language that can be used to create objects or perform actions in the post-processor.
All CCL statements can be classified into one of three categories:
• Object and parameter definitions, which are described in Object Creation and Deletion.
• CCL actions, which are commands that perform a specific task (such as reading a session file) and which are
described in Command Actions in the CFD-Post User's Guide.
• Power Syntax programming, which uses the Perl programming language to allow loops, logic, and custom
macros (subroutines). Power Syntax enables you to embed Perl commands into CCL to achieve powerful
quantitative postprocessing. For details, see Power Syntax in ANSYS CFX (p. 311).
State files and session files contain object definitions in CCL. In addition, session files can also contain
CCL action commands. You can view and modify the CCL in these files by using a text editor.
For more information, see Object Creation and Deletion.
13.1. CFX Command Language (CCL) Syntax
The following topics will be discussed:
• Basic Terminology (p. 216)
• The Data Hierarchy (p. 216)
• Simple Syntax Details (p. 216)
– Case Sensitivity (p. 216)
– CCL Names Definition (p. 217)
– Indentation (p. 217)
– End of Line Comment Character (p. 217)
– Continuation Character (p. 217)
– Named Objects (p. 217)
– Singleton Objects (p. 218)
– Parameters (p. 218)
– Lists (p. 218)
– Parameter Values (p. 218)
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
215
CFX Command Language (CCL)
– Escape Character (p. 220)
13.1.1. Basic Terminology
The following is an example of a CCL object that defines an isosurface.
ISOSURFACE: Iso1
Variable = Pressure
Value = 15000 [Pa]
Color = 1,0,0
Transparency = 0.5
END
• ISOSURFACE is an object type
• Iso1 is an object name
• Variable = Pressure is a parameter
• Variable is a parameter name
• Pressure is a parameter value
• If the object type does not need a name, it is called a singleton object. Only one object of a given singleton
type can exist.
13.1.2. The Data Hierarchy
Data is entered via parameters. These are grouped into objects that are stored in a tree structure.
OBJECT1: object name
name1 = value
name2 = value
END
Objects and parameters may be placed in any order, provided that the information is set prior to being
used further down the file. If data is set in one place and modified in another, the latter definition
overrides the first.
In CFD-Post, all object definitions are only one object level deep (that is, objects contain parameters,
but not other objects).
13.1.3. Simple Syntax Details
The following applies to any line that is not a Power Syntax or action line (that is, the line does not
start with a ! or >).
13.1.3.1. Case Sensitivity
Everything in the file is sensitive to case.
Case sensitivity is not ideal for typing in many long parameter names, but it is essential for bringing
the CFX Expression Language (CEL) into CCL. This is because some names used to define CCL objects
(such as Fluids, Materials and Additional Variables) are used to construct corresponding
CEL names.
For simplicity and consistency, the following is implemented:
216
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
CFX Command Language (CCL) Syntax
• Singletons and object types use upper case only.
• Parameter names, and predefined object names, are mixed case. The CFX Expression Language tries to follow
the following conventions:
1. Major words start with an upper case letter, while minor words such as prepositions and conjunctions
are left in lower case (for example, Mass Flow in).
2. Case is preserved for familiar names (for variables k or r), or for abbreviation RNG.
• User object names conventions can be chosen arbitrarily by you.
13.1.3.2. CCL Names Definition
Names of singletons, types of object, names of objects, and names of parameters all follow the same
rules:
• In simple syntax, a CCL name must be at least one character. This first character must be alphabetic; there
may be any number of subsequent characters and these can be alphabetic, numeric, space or tab.
• The effects of spaces in CCL names are:
– Spaces appearing before or after a name are not considered to be part of the name.
– Single spaces appearing inside a name are significant.
– Multiple spaces and tabs appearing inside a name are treated as a single space.
13.1.3.3. Indentation
Nothing in the file is sensitive to indentation, but indentation can be used for easier reading.
13.1.3.4. End of Line Comment Character
The # character is used for this. Any text to the right of this character will be treated as comments. Any
characters may be used within comments.
13.1.3.5. Continuation Character
If a line ends with the character \, the following line will be linked to the existing line. There is no restriction on the number of continuation lines.
13.1.3.6. Named Objects
A named object consists of an object type at the start of a line, followed by a : and an object name.
Subsequent lines may define parameters and child objects associated with this object. The object
definition is terminated by the string END on a line by itself.
Object names must be unique within the given scope, and the name must not contain an underscore.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
217
CFX Command Language (CCL)
13.1.3.7. Singleton Objects
A singleton object consists of an object type at the start of a line, followed by a :. Subsequent lines
may define parameters and child objects associated with this object. The object definition is terminated
by the string END on a line by itself.
The difference between a singleton object and a named object is that (after the data has been processed),
a singleton can appear just once as the child of a parent object. However, there may be several instances
of a named object of the same type defined with different names.
13.1.3.8. Parameters
A parameter consists of a parameter name at the start of a line followed by an = character followed by
a parameter value. A parameter may belong to many different object types. For example, U Velocity
= 1.0 [m/s] may belong to an initial value object and U Velocity = 2.0 [m/s] may belong
to a boundary condition object. Both refer to the same definition of U velocity in the rules file.
13.1.3.9. Lists
Lists are used within the context of parameter values and are comma separated.
13.1.3.10. Parameter Values
All parameter values are initially handled as data of type String, and should first of all conform to the
following definition of allowed String values:
13.1.3.10.1. String
• Any characters can be used in a parameter value.
• String values or other parameter type values are normally unquoted. If any quotes are present, they are
considered part of the value. Leading and trailing spaces are ignored. Internal spaces in parameter values
are preserved as given, although a given application is free to subsequently assume a space condensation
rule when using the data.
• The characters $ and # have a special meaning. A string beginning with $ is evaluated as a Power Syntax
variable, even if it occurs within a simple syntax statement. This is useful for performing more complex
Power Syntax variable manipulation, and then using the result as part of a parameter or object definition.
The appearance of # anywhere in the CCL file denotes the start of a comment.
• The characters such as [, ], {, and } are special only if used in conjunction with $. Following a $, such
characters terminate the preceding Perl variable name.
• Other characters that might be special elsewhere in power syntax are escaped automatically when they
appear in parameter values. For example, @, % and & are escaped automatically (that is, you do not need to
precede these characters with the escape character \ when using them in parameter values).
• Parameter values can contain commas, but if the string is processed as a List or part of a List then the commas
may be interpreted as separators (see below under List data types).
Some examples of valid parameter values using special characters in power syntax are:
Estimated cost = \$500
Title = Run\#1
Sys Command = "echo ’Starting up Stress solver’ ; fred.exe &"
218
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
CFX Command Language (CCL) Syntax
Pressure = $myArray[4]
Option = $myHash{"foo"}
Fuel = C${numberCatoms}H${numberHatoms}
Parameter values for data types other than String will additionally conform to one of the following
definitions.
13.1.3.10.2. String List
A list of string items separated by commas. Items in a String List should not contain a comma unless
contained between parentheses. One exception can be made if the String List to be is interpreted as a
Real List (see below). Otherwise, each item in the String List follows the same rules as String data.
names = one, two, three, four
13.1.3.10.3. Integer
Sequence of digits containing no spaces or commas. If a real is specified when an integer is needed,
the real is rounded to the nearest integer.
13.1.3.10.4. Integer List
List of integers, separated by commas.
13.1.3.10.5. Real
A single-precision real number that may be specified in integer, floating point, or scientific format, followed optionally by a dimension. Units use the same syntax as CEL.
Expressions are allowed to include commas inside function call argument lists.
Example usage:
a = 12.24
a = 1.224E01
a = 12.24 [m s^-1]
A real may also be specified as an expression such as:
a = myvel^2 + b
a = max(b,2.0)
13.1.3.10.6. Real List
List of reals, comma separated. Note that all items in the list must have the same dimensions. Items
that are expressions may include commas inside function call argument lists, and the enclosed commas
will be ignored when the list is parsed into individual items. Example usage:
a = 1.0 [m/s], 2.0 [m/s], 3.0 [m/s], 2.0*myvel, 4.0 [cm/s]
The list syntax 5*2.0 to represent 5 entries of the value 2.0 is not supported within CCL and hence
within CFD-Post.
13.1.3.10.7. Logical
Several forms are acceptable: YES, TRUE, 1 or ON are all equivalent; NO or FALSE or 0 or OFF are all
equivalent; initial letter variants Y, T, N, F are accepted (O is not accepted for On/Off); all case variants
are accepted. Logical strings are also case insensitive (YeS, nO).
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
219
CFX Command Language (CCL)
13.1.3.10.8. Logical List
List of logicals, separated by commas.
13.1.3.11. Escape Character
The \ character to be used as an escape character, for example, to allow $ or # to be used in strings.
220
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 14: CFX Expression Language (CEL)
CFX Expression Language (CEL) is an interpreted, declarative language that has been developed to enable
CFX users to enhance their simulations without recourse to writing and linking separate external Fortran
routines.
You can use CEL expressions anywhere a value is required for input in ANSYS CFX.
CEL can be used to:
• Define material properties that depend on other variables.
• Specify complex boundary conditions.
• Add terms to the solved equations.
You can also monitor the value of an expression during the solution using monitor points.
Note
CFX-Pre and CFD-Post evaluate CEL expressions with single (not double) precision.
Important
There is some CEL that works elsewhere in ANSYS CFX, but not in CFD-Post. Any expression
created in CFX-Pre and used as a Design Exploration output parameter could potentially
cause fatal errors during the Design Exploration run, so you should create all expressions for
Design Exploration output parameters in CFD-Post.
This chapter describes:
14.1. CEL Fundamentals
14.2. CEL Operators, Constants, and Expressions
14.3. CEL Examples
14.4. CEL Technical Details
14.1. CEL Fundamentals
The following topics will be discussed:
• Values and Expressions (p. 221)
• CFX Expression Language Statements (p. 222)
14.1.1. Values and Expressions
CEL can be used to generate both values and expressions. Values are dimensional (that is, with units)
or dimensionless constants. The simplest type of definition is the dimensionless value, for example:
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
221
CFX Expression Language (CEL)
b = 3.743
You can also specify a value with units, for example:
g = 9.81 [m s^-2]
The dimensions of the quantities of interest for CFD calculations can be written in terms of mass, length,
time, temperature and angle. The concept of units is fundamental to the behavior of values and expressions.
Values can be used directly, or they can be used as part of an expression. For example, you can use an
expression to add two values together:
<Expr_1> = <Value_1> + <Value_2>
In this example, you may want to predefine <Value_1> and <Value_2>, but this is not required.
However, in order to add two quantities together, they must have the same dimension; that is, it is
meaningful to add a quantity in inches to one expressed in meters, but it is not meaningful to add one
expressed in kilograms to one in square feet.
Expressions can also be functions of other (predefined) expressions:
<Expr_2> = <Expr_1> + <Value_3>
Units follow the conventions in the rest of CFX, in that a calculation has a set of solution units (by default,
SI units), and that any quantity can be defined either in terms of the solution units, or any other set of
units with the correct form.
An expression does not have its own units string, but if it references quantities that have dimensions,
these will determine the resulting units for the expression. For example, if an expression depends inversely
on the square of the x coordinate, then it has implied dimensions of length to the power -2.
14.1.1.1. Using Locators in Expressions
A CFX simulation has physics areas and mesh areas; physics areas are boundaries while mesh areas are
regions. These two types of area can occupy completely different spaces in a simulation; however, there
is no requirement that area names be unique between physics and mesh. This can lead to ambiguities
when you use these names in expressions.
To avoid these ambiguities, ANSYS CFX first checks to see if "@<locator>" is a physics name; if this is
not found, the name is checked in the list of mesh names. Thus if "in1" is both the name of a physics
area and the name of a mesh area, "@<locator>" is taken to indicate the physics area.
ANSYS CFX also has @REGION CEL syntax so that you can identify a named area as being a mesh area.
Thus to identify the mesh area in1, you would use the syntax:
@REGION:in1
Note that if <locator> does not appear as a physics name or a mesh name, the expression fails.
14.1.2. CFX Expression Language Statements
The CFX Expression Language is declarative. You declare the name and definition of the expression
using expression language statements. The statements must conform to a predefined syntax that is
similar to Fortran mathematical statements and to C statements for logical expressions.
222
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
CEL Fundamentals
The statement must consist of the following:
• a number, optionally with associated units. This defines a constant. Constants without units are termed dimensionless.
• for mathematical expressions, one or more references to mathematical constants, system variables, or existing
user variables, separated by + (addition), - (subtraction), * (multiplication), / (division) and ^ (exponentiation),
with optional grouping of these by parentheses. The syntax rules for these expressions are the same as
those for conventional arithmetic.
• for logical expressions involving relational operators, one or more references to mathematical constants or
results from mathematical expressions, separated by <= (is less than or equal to), < (is less than), == (is equal
to), != (is not equal to), > (is greater than) and >= (is greater than or equal to) with optional grouping of
these by parentheses.
• for logical expressions involving logical operators, one or more references to logical constants or results
from relational operations separated by ! (negation), && (logical AND) and || (logical OR), with optional
grouping by parentheses.
14.1.2.1. Use of Constants
Constants do not need to be defined prior to being used in an expression. For example, you could
choose to evaluate the expression x + 5 [m]. Or, you could define a constant, b = 5 [m] and
then create an expression x + b.
The logical constants are false and true. Results of logical expressions are either false or true, which
are evaluated as 0 and 1 (corresponding to false and true, respectively) when a numerical representation is required.
The use of constants may be of benefit in generating complicated expressions or if you have several
expressions that use the same constants.
14.1.2.2. Expression Syntax
All numbers are treated as real numbers.
The precedence of mathematical operators is as follows (from highest to lowest):
• The power operator ^ as in x^y.
• The unary minus or negation operator - as in -x.
• Multiplication and division as in x*y/z.
• Addition and subtraction as in x+y-z.
The precedence of logical and relational operators is as follows (from highest to lowest):
• The negation operator ! as in !x.
• The relational operators involving less than or greater than (<=, <, > and >=) as in x >= y.
• The relational operator is equal to and is not equal to (== and !=) as in x != y.
• The logical AND operator (&&) as in x && y.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
223
CFX Expression Language (CEL)
• The logical OR operator (||) as in x || y.
14.1.2.3. Multiple-Line Expressions
It is often useful, particularly with complex expressions, to use more than one line when creating your
expression. CFX allows you to use multiple lines to generate an expression, provided each line is separated
by an appropriate operator.
For example, you may have an equation, A + B/C, that consists of three complex terms, A, B, and C. In
this case, you could use three lines to simplify creating the expression:
A +
B
/ C
Note that the operator may be used at the end of a line (A +) or at the beginning of a line (/ C). You
do not need to enter the operator twice.
Once the expression has been created, it will appear in the Existing Definitions list box as if it were
generated on a single line (A + B/C).
14.2. CEL Operators, Constants, and Expressions
The following topics are discussed:
• CEL Operators (p. 224)
• Conditional if Statement (p. 225)
• CEL Constants (p. 226)
• Using Expressions (p. 226)
14.2.1. CEL Operators
CFX provides a range of mathematical, logical and operational operators as built-in functions to help
you create complex expressions using the Expression details view.
Table 14.1: CEL Operators
Operator
First
Operand’s
Dimensions
[x]
-x
Any
x+y
Any
x-y
Second
Operand’s
Dimensions
[y]
Operands’
Values
Result’s
Dimensions
(Approx)a
Any
[x]
[x]
Any
[x]
Any
[x]
Any
[x]
x*y
Any
Any
Any
[x]*[y]
x/y
Any
Any
0
[x]/[y]
x^y (if y is a
simple,
constant,
Any
Dimensionless
224
Anyb
[x]^y
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
CEL Operators, Constants, and Expressions
Operator
First
Operand’s
Dimensions
[x]
Second
Operand’s
Dimensions
[y]
Operands’
Values
Result’s
Dimensions
x^y (if y is
any simple,
constant,
expression)
Any
Dimensionless
x>0
[x]^y
x^y (if y is
not simple
and
constant)
Dimensionless
Dimensionless
x>0
Dimensionless
!x
Dimensionless
false or
true
Dimensionless
x <= y
Any
[x]
false or
true
Dimensionless
x<y
Any
[x]
false or
true
Dimensionless
x>y
Any
[x]
false or
true
Dimensionless
x >= y
Any
[x]
false or
true
Dimensionless
x == y
Any
[x]
false or
true
Dimensionless
x != y
Any
[x]
false or
true
Dimensionless
x && y
Dimensionless
Dimensionless
false or
true
Dimensionless
x || y
Dimensionless
Dimensionless
false or
true
Dimensionless
(Approx)a
integer
expression)
a
The logical constants true and false are represented by "1" and "0" when a numerical representation is required.
For y < 0, x must be non-zero.
b
14.2.2. Conditional if Statement
CEL supports the conditional if statement using the following syntax:
if( cond_expr, true_expr, false_expr )
where:
• cond_expr: is the logical expression used as the conditional test
• true_expr: is the mathematical expression used to determine the result if the conditional test is
true.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
225
CFX Expression Language (CEL)
• false_expr : is the mathematical expression used to determine the result if the conditional test is
false.
Note
The expressions true_expr and false_expr are always evaluated independent of
whether the evaluation of cond_expr is true or false. As a consequence, a conditional
statement cannot be used to avoid division by zero as in if( x>0, 1/x, 1.0). In this
case, when x=0.0, a division by zero will still occur because the expression 1/x is evaluated
independent of whether x>0 is satisfied or not.
14.2.3. CEL Constants
Right-click in the Expression details view to access the following useful constants when developing
expressions:
Table 14.2: CEL Constants
Constant
Units
Description
R
J K^-1 mol^-1
Universal Gas Constant: 8.314472
avogadro
mol^-1
6.02214199E+23
boltzmann
J K^-1
1.3806503E-23
clight
m s^-1
2.99792458E+08
e
Dimensionless
Constant: 2.7182817
echarge
As
Constant: 1.60217653E-19
epspermo
1./(clight*clight*mupermo)
g
m s^-2
Acceleration due to gravity:
9.8066502
mupermo
N A^-2
4*pi*1.E-07
pi
Dimensionless
Constant: 3.141592654
planck
Js
6.62606876E-34
stefan
W m^-2 K^-4
5.670400E-08
14.2.4. Using Expressions
The interaction with CEL consists of two phases:
• a definition phase, and,
• a use phase.
The definition phase consists of creating a set of values and expressions of valid syntax. The purpose
of the Expression details view is to help you to do this.
14.2.4.1. Use of Offset Temperature
When using temperature values in expressions, it is generally safer to use units of [K] only. When units
are used that posses an offset (for example, [C]), they are converted internally to [K]. For terms that
226
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
CEL Examples
have temperature to the power of unity, any unit conversion will include the offset between temperature
scales. However, in all other cases the offset is ignored because this is usually the most appropriate
behavior. You should therefore take care when specifying an expression involving non-unit powers of
temperature. For example, each of the expressions below is equivalent:
Temperature
Temperature
Temperature
Temperature
=
=
=
=
30 [C]
303.15 [K]
0 [C] + 30 [K]
273.15 [K] + 30 [K]
These are only equivalent because all units are to the power of unity and units other than [K] appear
no more than once in each expression. The following expression will not produce the expected result:
Temperature = 0 [C] + 30 [C]
This is equivalent to 576.30 [K] because each value is converted to [K] and then summed. The two
expression below are equivalent (as expected) because the offset in scales is ignored for non-unit powers
of temperature:
Specific Heat = 4200 [J kg^-1 C^-1]
Specific Heat = 4200 [J kg^-1 K^-1]
14.3. CEL Examples
The following examples are included in this section:
• Example: Reynolds Number Dependent Viscosity (p. 227)
• Example: Feedback to Control Inlet Temperature (p. 228)
14.3.1. Example: Reynolds Number Dependent Viscosity
In this example it is assumed that some of the fluid properties, including the dynamic viscosity, are not
known. However the Reynolds number, inlet velocity and a length scale are known. The flow is compressible and therefore the density is variable.
Given this information it is possible to calculate the fluid dynamic viscosity based on the Reynolds
number. The Reynolds number is given by:
where is density, U a velocity scale, L a length scale and the dynamic viscosity. The velocity scale
is taken as the inlet velocity, the length scale as the inlet width and the density is calculated as the average density over the inlet area.
The LIBRARY section of the CCL (CFX Command Language) file appears as follows:
LIBRARY :
CEL :
EXPRESSIONS :
Re = 4.29E6 [ ]
Vel = 60 [m s^-1]
L=1.044[m]
Visc=areaAve(density)@in*Vel*L/Re
END
END
MATERIAL : Air Ideal Gas
Option = Pure Substance
PROPERTIES :
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
227
CFX Expression Language (CEL)
Option = Ideal Gas
Molar Mass = 2.896E1 [kg kmol^-1]
Dynamic Viscosity = Visc
Specific Heat Capacity = 1.E3 [J kg^-1 K^-1]
Thermal Conductivity = 2.52E-2 [W m^-1 K^-1]
END
END
END
This shows that four CEL expressions have been created. The first three expressions define constant
values that are used in the Visc expression. The Visc expression calculates the dynamic viscosity
based on the equation for Reynolds number given above. Within the expression the function
areaAve(density)@in is used to evaluate the average density at the inlet.
The Visc expression can now be used to replace the value of Dynamic Viscosity in the MATER
IAL > PROPERTIES section.
14.3.2. Example: Feedback to Control Inlet Temperature
In this example a feedback loop is used to control the outlet temperature by varying the temperature
at an inlet. To illustrate the example consider the geometry shown below:
Figure 14.1: Temperature Feedback Loop
Fluid from a main and a side inlet enter at temperatures of 275 K and 375 K respectively. The temperature
of the fluid entering from the third inlet depends on the outlet temperature. When the outlet temperature is greater than 325 K, the fluid from the third inlet is set to 275 K. When the outlet temperature
is less than 325 K, the fluid from the third inlet is set to 375 K. In addition an expression is used to set
the dynamic viscosity to be a linear function of temperature.
The LIBRARY section of the .ccl (CFX Command Language) file appears as follows. Note that the “\”
character indicates a line continuation in CCL.
LIBRARY:
MATERIAL: Water at STP Modified
Option = Pure Substance
PROPERTIES:
Option = General Fluid
Density = 9.999E2 [kg m^-3]
Dynamic Viscosity = VisT
Specific Heat Capacity = 4.21E3 [J kg^-1 K^-1]
Thermal Conductivity = 5.69E-1 [W m^-1 K^-1]
END # PROPERTIES
END # MATERIAL Water at STP Modified
CEL:
EXPRESSIONS:
Tupper = 375.0 [ K ] # Upper temp.
Tlower = 275.0 [ K ] # Lower temp.
Visupper = 0.000545 [ N s m^-2 ] # Vis. at Tupper
Vislower = 0.0018 [ N s m^-2 ] # Vis. at Tlower
VisT = Vislower+(Visupper-Vislower)*(T-Tlower)/ \
(Tupper-Tlower)
228
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
CEL Examples
# Vis.-Temp. relationship
Tm=(Tupper+Tlower)/2
Tout=areaAve(Water at STP Modified.T)@outlet
Tcontrol=Tlower*step((Tout-Tm)/1[K]) \
+Tupper*step((Tm-Tout)/1[K])
END # EXPRESSIONS
END # CEL
END # LIBRARY
The first four expressions, Tupper, Tlower, Visupper and Vislower are simply constant values to
define temperature and viscosity values. The expression VisT produces a linear function for the dynamic
viscosity taking a value of Visupper at Tupper and a value of Vislower at Tlower. The expression
Tm sets the desired value of the outlet temperature. In this case it is set to a mean value of the two
inlet temperatures.
Tout calculates the outlet temperature using the areaAve function.
Finally the expression Tcontrol is used to set the temperature of the third inlet. Two step functions
are used so that the temperature is equal to Tlower when Tout-Tm is positive (that is, the outlet
temperature is greater than Tm), and is equal to Tupper when Tout-Tm is positive.
14.3.3. Examples: Using Expressions in CFD-Post
The first example is a single-valued expression that calculates the pressure drop through a pipe. The
names of inlet and outlet boundaries are “inlet” and “outlet”.
Create a new expression named “dp”:
dp = massFlowAve(Pressure)@inlet – massFlowAve(Pressure)@outlet
When you click Apply, the value is shown below the editor.
Tip
Alternatively, type the expression in a table cell and prefix with ‘=’ sign. The cell displays the
result when you click outside of the cell.
The second example is a variable expression that plots the pressure coefficient variation on a surface
or a line:
1.
Click the Expressions tab, then right-click in the Expressions area and select New.
2.
Create these three expressions:
RefPressure = 100000 [Pa]
dynHead = 0.5 * areaAve(Density)@inlet * areaAve(Velocity)@inlet^2
cpExp = (Pressure - RefPressure)/dynHead
3.
Click the Variables tab, then right-click and select New.
4.
Create a user variable defined by cpExp.
5.
Select Insert > Location > Line and use the details view to position the line in the simulation.
From the details view Color tab, plot the user variable on a surface or a line (just as you would
with any other variable).
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
229
CFX Expression Language (CEL)
14.4. CEL Technical Details
CEL is a byte code compiled language. Compiled languages, such as Fortran, rely on a translation program
to convert them into the native machine language of the host platform. Interpreted languages are of
two types: the fully interpreted languages such as the UNIX C shell, and the byte code compiled languages
such as CEL. With byte codes, host machines are loaded with a client program (written in a compiled
language and compiled for that machine architecture) that interprets the byte stream. The advantage
of the byte code is that they can be the same on all host platforms, obviating the need for platform
dependent codes.
Because the byte codes are interpreted, there is no need to re-link executable programs to perform a
different calculation. Furthermore, many of the problems encountered by writing and linking in separate
routines, for instance in C or Fortran, are averted, and the time taken to set up and debug complicated
problems reduced considerably.
The link between CEL and the CFX-Solver is accomplished through an internal program called genicode.
Genicode generates intermediate code from your CEL definitions and writes to a file that is then interpreted by the CFX-Solver during the solution process.
230
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 15: Functions in ANSYS CFX
This chapter describes predefined functions in ANSYS CFX:
15.1. CEL Mathematical Functions
15.2. Quantitative CEL Functions in ANSYS CFX
15.3. Functions Involving Coordinates
15.4. CEL Functions with Multiphase Flow
15.5. Quantitative Function List
15.1. CEL Mathematical Functions
The following mathematical functions are available for use with all CEL expressions.
Note
In the Function column in the table below, [a] denotes any dimension of the first operand.
Table 15.1: Standard Mathematical CEL Functions
Function
Operand’s Values
Result’s Dimensions
abs( [a] )
Any
[a]
acos( [ ] )
Radians
asin( [ ] )
Radians
atan( [ ] )a
Any
Radians
atan2( [a], [a] )a
Any
Radians
besselJ( [ ], [ ] )b
Dimensionless
besselY( [ ], [ ] )b
Dimensionless
cos( [radians] )
Any
Dimensionless
cosh( [ ] )
Any
Dimensionless
exp( [ ] )
Any
Dimensionless
int([ ])c
Dimensionless
Dimensionless
loge( [ ] )d
Dimensionless
log10( [ ] )e
Dimensionless
min( [a], [a] )
Any
[a]
max( [a], [a] )
Any
[a]
mod( [a], [a] )f
Any
[a]
nint([ ])g
Dimensionless
Dimensionless
sin( [radians] )
Any
Dimensionless
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
231
Functions in ANSYS CFX
Function
Operand’s Values
Result’s Dimensions
sinh( [ ] )
Any
Dimensionless
sqrt( [a] )
[a]^0.5
Any
Dimensionless
tan( [radians] )i
Any
Dimensionless
tanh( [ ] )
Any
Dimensionless
step( [ ] )
h
a
atan does not determine the quadrant of the result, but atan2 does.
The value of the first dimensionless operand n, also referred to as the order of the Bessel function, must be an integer (n=0, 1, 2,
....). The second argument is a dimensionless real number.
c
The int() function truncates the dimensionless argument to its integer part.
b
Examples:
int(1) = 1
int(2.5) = 2
int(-3.1) = -3
int(-4.8) = -4
The int() function requires a dimensionless argument but will not report an error if the argument of the function has a dimension
of radians or degrees.
d
ln(x) is valid as an alias for loge(x)
e
log(x) is valid as an alias for log10(x)
f
mod(x, y) returns the remainder on dividing x by y; the function is not defined for y = 0.
g
The nint function requires a dimensionless argument and is defined as:
int(x + 0.5) if x >= 0
int(x - 0.5) if x < 0
See the implementation of int( ) function in the table above.
Examples:
nint(2.6) = 3
nint(2.5) = 3
nint(2.4) = 2
nint(1) = 1
nint(-1) = -1
nint(-2.4) = -2
nint(-2.5) = -3
nint(-2.6) = -3
Note that the nint() function will not report an error if the argument of the function has a dimension of radians or degrees.
h
step(x) is 0 for negative x, 1 for positive x and 0.5 for x=0. x must be dimensionless.
i
tan(x) is undefined for x=n /2, where n=1, 3, 5, ...
232
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Quantitative CEL Functions in ANSYS CFX
15.2. Quantitative CEL Functions in ANSYS CFX
CEL expressions can incorporate specialized functions that are useful in CFD calculations. All CEL functions
are described in Quantitative Function List (p. 237). For a description of the full CFX Expression Language,
see CFX Expression Language (CEL) (p. 221).
Important
You must use consistent units when adding, subtracting, or comparing values.
There are some differences between CEL functions in CFX-Pre and CFX-Solver and those in
CFD-Post. For details, see below.
The syntax used for calling these functions when used within CEL expressions is:
[<Phase_Name>.][<Component_Name>.]<Function>([<Operand>])@<Location>
where:
• Terms enclosed in square brackets [ ] are optional and terms in angle brackets < > should be replaced
with the required entry.
• <Phase_Name>: specifies a valid name of a phase. The phase can be fluid, particle, solid, fluid pair, or
polydispersed fluid. For multi-phase cases in CFX-Pre, if the phase name is not specified in the <Operand>,
then the phase name associated with the domain, subdomain, domain boundary, initialization or function
in which the operand is being evaluated will be used. For multi-phase cases in CFX-Pre, a discussion of the
handling of the phase name when it is not used to qualify (prepended to) <Function> and/or <Operand>
can be found in CEL Functions with Multiphase Flow (p. 236). For multi-phase cases in CFD-Post, if the phase
name is not specified then the bulk quantity (if available for the CFX-Solver Results file) is used.
• <Component_Name>: specifies a valid name of a component material, size group, or reaction
• <Function>: specifies the CEL function to evaluate. See Quantitative Function List (p. 237). The function
can be further qualified by appending _Coordinate_Direction. In CFX-Pre, if the coordinate frame is
not specified (in _Coordinate_Direction ) then the function will use the coordinate frame associated
with the object (such as for a material, domain, subdomain, domain boundary, source point, monitor point,
initialization, reference location or spark ignition object) in which it is being invoked.
• <Coordinate_Direction>: specifies a particular coordinate direction. The syntax of the coordinate
direction is [x|y|z][_<Coordinate_Frame>] where the coordinate frame can be the global coordinate
frame or any user defined coordinate frame. In CFD-Post, if the coordinate frame is not specified then the
global frame is used. See Coordinate Frame Command in the CFD-Post User's Guide, for discussion of creating
a coordinate frame in CFD-Post.
• <Operand>: specifies the argument of the function (if required). The operand can be either a valid mathematical CEL expression (only in CFD-Post) or specified using the following general variable syntax:
[<Phase_Name>.][<Comp_Name>.]<Var_Name>[.<Var_Operator>][.Difference]
where <Comp_Name>, <Var_Name>, and <Var_Operator> represent <Component_Name>, <Vari
able_Name>, and <Variable_Operator>, respectively.
In CFX-Pre the operand cannot be a CEL expression or any operand qualified by <Variable_Oper
ator>. However, you can create an Additional Variable based on any expression and then use the
Additional Variable as the operand. The operand always uses the conservative values unless the
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
233
Functions in ANSYS CFX
Boundcon variable operator is specified (for details, see Data Acquisition Routines in the CFX-Solver
Modeling Guide). For primitive or composite mesh regions, conservative values will be used even if
the Boundcon variable operator is specified.
The operand must be valid for the physical models being used over the entire location. For example,
if the location spans fluid and solid domains, then the operand cannot be Pressure.
For some functions the operand must be left blank as in area()@Inlet.
In CFD-Post, difference variables created during case comparison are appended by .Difference.
• <Variable_Name>: specifies the base name of the variable. You can use the short or long form for variable
names. In CFX-Pre the variable name can be further qualified by appending _<Coordinate_Direction>.
This is useful for specifying a particular component of a vector or tensor, for example Velocity_y_myLoc
alFrame. In CFX-Pre, if the variable name corresponds to that of a component of a vector or a tensor and
coordinate frame is not prescribed (as part of the coordinate direction) then the global coordinate frame is
used. An exception applies for the position vector x, y, z (or r, theta, z) components, which are always
local, see Functions Involving Coordinates (p. 236).
• <Variable_Operator> specifies the name of the variable operator. The variable operators are.
Long Name
Short Name
Magnitude
magnitude
Gradient
grad
Curl
curl
Laplacian
laplacian
Time Derivative
dt
Transient Minimum
Trnmin
Transient Maximum
Trnmax
Transient Std Deviation
Trnsdv
Transient RMS
Trnrms
Transient Average
Trnavg
Boundcon
hybrid
All but the <Derived> operator are available in CFX-Pre and the CFX-Solver. See Data Acquisition
Routines in the CFX-Solver Modeling Guide. The <Derived> variable operator is available only in
CFD-Post, for example Absolute Helicity derived for use with Vortex Cores, see Vortex Core
Region in the CFD-Post User's Guide. In CFX-Pre the variable operator can be further qualified by appending _<Coordinate_Direction>.
The Magnitude and Curl operators may only be applied to vector variables. All other operators
may be applied to scalar variables and vector components.
• <Location>: specifies the location over which the function is to be applied. The syntax of location is:
[Case:<Case_Name>.][REGION:]<Location_Name>
The case syntax [Case:<Case_Name>.] is only available in CFD-Post. When multiple cases are
loaded, this syntax is used to narrow down the locator to the desired case.
234
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Quantitative CEL Functions in ANSYS CFX
In CFX-Pre [<Location_Name>] must be a domain boundary, domain, subdomain, or, primitive
or composite mesh region. If the location name of a mesh region is the same as the name of a named
boundary, domain or subdomain, then the mesh location name must be prepended by REGION:.
For primitive or composite mesh regions, conservative values will be used even if the name of the
mesh region is the same as that of a named boundary.
In CFD-Post [<Location_Name>] can be any loaded or user-defined location (for example, a point,
domain boundary, plane, mesh region, and so on). The syntax REGION:<Region Name> can also
be used in CFD-Post to refer to any mesh region. If a mesh region is present with the same name as,
for example, a domain boundary, then the mesh region is imported into CFD-Post with a Region
suffix. For example, if there is both a domain boundary and a mesh region called in1 in the CFXSolver Results file, then in CFD-Post the mesh region will appear in CFD-Post as in1 Region. The
syntax in1 will refer to the domain boundary, and either of in1 Region or REGION:in1 can be
used to refer to the mesh region as desired.
Note
You cannot use a composite region that consists of a mixture of 2D and 3D regions.
Table 15.2: Examples of the Calling Syntax for an Expression
areaAve(p)@Inlet
This results in the area-weighted average
of pressure on the boundary named In
let.
area()@REGION:myCompositeMeshRegion
This results in the area of a 2D mesh region
named myCompositeMeshRegion.
areaAve(Pressure - 10000 [Pa])@out
let
This syntax is appropriate only for
CFD-Post.
area_x()@inlet
Water at RTP.force_z()@Default
area()@CASE:newcase.myplane
This syntax is appropriate only for CFD-Post
and is used when multiple files are loaded.
It follows the general form func
tion()@CASE:case name.location.
This example results in the area of the part
of myplane that is located within the case
newcase.
probe(Pressure)@CASE:1.Point 1
This syntax is used only for CFD-Post, when
two cases are loaded in the comparison
mode. This example results in the
difference in pressure between cases 1 and
2, where the pressure for Case 1 and the
pressure for Case 2 are evaluated at the
same point. The general syntax, func
tion()@CASE:[1|2].location, is
used when performing file comparisons.
probe(Pressure)@CASE:2.Point 1
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
235
Functions in ANSYS CFX
15.3. Functions Involving Coordinates
The CEL variables x, y, z, r and theta, representing the local coordinates, cannot be used as the
variable. However, the variables xGlobal, yGlobal and zGlobal can be used. For example, the
following is a valid expression definition:
z*areaAve(xGlobal)@inlet
15.4. CEL Functions with Multiphase Flow
Note
These functions are available in CFX-Pre and CFX-Solver without restrictions, and in CFD-Post
with the restriction that you cannot use short names.
If the function is fluid-specific, various behaviors are possible depending on the function type:
• For massFlow and massFlowAve, if the phase name is not specified for the function, then the bulk mass
flows will be used. See cases 1 to 7 in the table below.
• For other fluid-specific functions:
– if a fluid-specific operand is specified and no fluid is specified for the function, then the fluid specified for
the operand will be assumed for the function as well. See case 8 in the table below.
– if the function is specified and no fluid is specified for the operand, then the fluid specified for the function
will be assumed for the operand as well. See cases 7 and 9 in the table below.
• If both the function or operand are fluid-specific, and a phase name is not given for either, the solver will
stop with an error. See case 10 in the table below.
Table 15.3: CEL Multiphase Examples
Case
CEL Function - Multiphase
Behavior
1
massFlow()@inlet
Bulk mass flow rate through inlet
2
Air.massFlow()@inlet
Air mass flow rate through inlet
3
massFlowAve(Pressure)@inlet
Bulk mass flow averaged pressure on inlet
4
Air.massFlowAve(Pressure)@in
let
Air mass flow averaged pressure on inlet
5
massFlowAve(Air.Volume Frac
tion)@inlet
Bulk mass flow averaged air volume fraction
on inlet
6
Air.massFlowAve(Air.Volume
Fraction)@inlet
Air mass flow averaged air volume fraction
on inlet
7
Air.massFlowAve(Volume Frac
tion)@inlet
Same as Air.massFlowAve(Air.Volume
Fraction)@ inlet
8
massInt(Air.Volume Frac
tion)@domain1
Same as Air.massInt(Air.Volume
Fraction)@ domain1
9
Air.massInt(Volume Frac
tion)@domain1
Same as Air.massInt(Air.Volume
Fraction)@ domain1
236
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Quantitative Function List
Case
CEL Function - Multiphase
Behavior
10
massFlowAve(Volume Frac
tion)@inlet
Error because no fluid specified
15.5. Quantitative Function List
The available quantitative functions are outlined in the sections that follow.
In the table that follows, <Expression> applies to CFD-Post only. CFX-Pre and CFX-Solver can only accept
variables as arguments to quantitative functions. Note that for CFX-Pre and CFX-Solver, an Additional
Variable can be used to pass an expression indirectly into a quantitative function.
The behavior of the functions in the table below depends on the type of <Location>. Typically:
• On domains and subdomains, the functions use vertex (node) values for the operand.
• On a boundary, the functions use conservative values for the operand unless this is overridden by the
Boundcon variable operator in CFX-Pre.
• On user locations in CFD-Post, the functions use values interpolated from nodal values.
Table 15.4: CEL Functions in CFX-Pre/CFX-Solver and in CFD-Post
Function Name and Syntax
<required> [<optional>]
Operation
Availability
area( )
Area of a boundary or interface.
All
Supports “@<Location>”.
See area (p. 241).
area_x[_<Coord Frame>]( )
area_y[_<Coord Frame>]( )
area_z[_<Coord Frame>]( )
The (signed) component of the normal area
vector in the local X, Y, or Z direction. The
normal area vectors are always directed out of
the domain, therefore you may obtain positive
or negative areas depending on the orientation
of your domain and the boundary you are
operating on. The area of a closed surface will
always be zero.
Alla
Supports “@<Location>”.
areaAve(<Variable|Expression>)
Area-weighted average of
<Variable|Expression> on a boundary.
All
Supports “@<Location>”.
See areaAve (p. 242).
areaAve_x[_<Coord
Frame>]( )
areaAve_y[_<Coord
Frame>]( )
The (signed) component of the normal area
vector weighted average in the local X, Y or Z
direction. The normal area vectors are always
directed out of the domain, therefore you may
obtain positive or negative areas depending
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
CFD-Post
237
Functions in ANSYS CFX
Function Name and Syntax
<required> [<optional>]
Operation
areaAve_z[_<Coord
Frame>]( )
on the orientation of your domain and the
boundary you are operating on. The area of a
closed surface will always be zero.
Availability
Supports “@<Location>”.
areaInt(<Variable|Expression>)
Area-weighted integral of
<Variable|Expression> on a boundary.
All
The areaInt function projects the location
onto a plane normal to the specified direction
(if the direction is not set to None) and then
performs the calculation on the projected
location (the direction specification can also
be None). The direction of the normal vectors
for the location is important and will cancel
out for surfaces such as closed surfaces.
Supports “@<Location>”.
See areaInt (p. 243).
areaInt_x[_<Coord Frame>](
)
areaInt_y[_<Coord Frame>](
)
areaInt_z[_<Coord Frame>](
)
The (signed) component of the normal area
vector weighted integral in the local X, Y, or Z
direction. The normal area vectors are always
directed out of the domain, therefore you may
obtain positive or negative areas depending
on the orientation of your domain and the
boundary you are operating on. The area of a
closed surface will always be zero.
All
Supports “@<Location>”.
ave(<Variable|Expression>)
Arithmetic average of <Variable|Expression>
over nodes within a domain or subdomain.
All
Supports “@<Location>”.
See ave (p. 244).
count( )
Counts the number of evaluation points (for
example, nodes) on the named region.
All
See count (p. 245).
countTrue(<Variable|Expression>) Counts the number of nodes at which the
Variable or logical expression evaluates to true.
All
Supports “@<Location>”.
See countTrue (p. 246).
force( )
The magnitude of the force vector on a
boundary.
Supports “[<Phase>.]” and “@<Location>”.
238
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
All
Quantitative Function List
Function Name and Syntax
<required> [<optional>]
Operation
Availability
See force (p. 246).
forceNorm
[_<Axis>[_<Coord Frame>]](
)
The length of the normalized force on a curve
in the specified direction.
CFD-Post
Supports “[<Phase>.]” and “@<Location>”.
See forceNorm (p. 247).
force_x[_<Coord Frame>]( )
The (signed) component of the force vector in
the local X, Y, or Z direction.
Alla
force_y[_<Coord Frame>]( )
Supports “[<Phase>.]” and “@<Location>”.
force_z[_<Coord Frame>]( )
inside()
Similar to the subdomain variable, but allows
a specific 2D or 3D location to be given.
CFX-Pre,
CFX-Solver
Supports “@<Location>”.
See inside (p. 248).
length()
Length of a curve.
CFD-Post
Supports “@<Location>”.
See length (p. 248).
lengthAve(<Variable|Expression>) Length-weighted average.
CFD-Post
Supports “@<Location>”.
See lengthAve (p. 249).
lengthInt(<Variable|Expression>)
Length-weighted integration.
CFD-Post
Supports “@<Location>”.
See lengthInt (p. 250).
mass()
The total mass within a domain or subdomain.
This is fluid-dependent.
CFX-Pre,
CFX-Solver
Supports “@<Location>”.
See mass (p. 250).
massAve(<Variable|Expression>)
Mass-weighted average of
<Variable|Expression> on a domain or
subdomain.
CFX-Pre,
CFX-Solver
Supports “@<Location>”.
See massAve (p. 250).
massFlow()
Mass flow through a boundary.
All
Supports “[<Phase>.]” and “@<Location>”.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
239
Functions in ANSYS CFX
Function Name and Syntax
<required> [<optional>]
Operation
Availability
See massFlow (p. 250).
massFlowAve(<Variable|Expression>)
Mass flow weighted average of
<Variable|Expression> on a boundary.
All
Supports “[<Phase>.]” and “@<Location>”.
See massFlowAve (p. 252).
massFlowAveAbs(<Variable|Expression>)
Absolute mass flow weighted average of
<Variable|Expression> on a boundary.
All
Supports “[<Phase>.]” and “@<Location>”.
See massFlowAveAbs (p. 252).
massFlowInt(<Variable|Expression>)Mass flow weighted integration of
<Variable|Expression> on a boundary.
All
Supports “[<Phase>.]” and “@<Location>”.
See massFlowInt (p. 254).
massInt(<Variable|Expression>)
The mass-weighted integration of
<Variable|Expression> within a domain or
subdomain.
CFX-Pre,
CFX-Solver
Supports “@<Location>”.
See massInt (p. 255).
maxVal(<Variable|Expression>)
Maximum value of <Variable|Expression> within
a domain or subdomain.
All
Supports “@<Location>”.
See maxVal (p. 255).
minVal(<Variable|Expression>)
Minimum value of <Variable|Expression> within
a domain or subdomain.
All
Supports “@<Location>”.
See minVal (p. 255).
probe(<Variable|Expression>)
Returns the value of the specified variable or
expression on the specified Point object.
All
Supports “@<Location>”.
See probe (p. 256).
rbstate(<rbvar>[<axis>])
240
Returns the position/velocity/acceleration or
orientation/angular velocity/angular
acceleration (or axis components of these) of
a rigid body object or immersed solid that is
governed by a rigid body solution. These
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
CFX-Pre,
CFX-Solver
Quantitative Function List
Function Name and Syntax
<required> [<optional>]
Operation
Availability
quantities are with respect to the global
coordinate frame.
See rbstate (p. 256).
rmsAve(<Variable|Expression>)
RMS average of <Variable|Expression> on a 2D
boundary or within a 3D domain or subdomain.
CFX-Pre,
CFX-Solver
Supports “@<Location>”.
See rmsAve (p. 257).
sum(<Variable|Expression>)
Sum of <Variable|Expression> over all 2D
boundaries or 3D domains or subdomains.
All
Supports “@<Location>”.
See sum (p. 257).
torque( )
Magnitude of the torque vector on a boundary.
All
Supports “[<Phase>.]” and “@<Location>”.
See torque (p. 258).
torque_x[_<Coord Frame>]()
The (signed) components of the torque vector
about the local x, y, or z coordinate axis.
Alla
torque_y[_<Coord Frame>]()
Supports “[<Phase>.]” and “@<Location>”.
torque_z[_<Coord Frame>]()
volume( )
The total volume of a domain or subdomain.
All
Supports “@<Location>”.
See volume (p. 259).
volumeAve(<Variable|Expression>) Volume-weighted average of
<Variable|Expression> on a domain.
All
Supports “@<Location>”.
See volumeAve (p. 259).
volumeInt(<Variable|Expression>) Volume-weighted integration of
<Variable|Expression> within a domain or
subdomain.
All
Supports “@<Location>”.
See volumeInt (p. 259).
a
See the definition for [_<Coordinate_ Direction>]] in Quantitative CEL Functions in ANSYS CFX (p. 233)
15.5.1. area
The area function is used to calculate the area of a 2D locator.
area[_<Axis>[_<Coord Frame>] ]()@<Location>
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
241
Functions in ANSYS CFX
where:
• <Axis> is x, y, or z
• <Coord Frame> is the coordinate frame
• <Location> is any 2D region (such as a boundary or interface).
An error is raised if the location specified is not a 2D object. If an axis is not specified, the total area of
the location is calculated.
area()@Isosurface1 calculates the total area of the location, and Isosur
face1.area_y()@Isosurface1 calculates the projected area of Isosurface1 onto a plane
normal to the Y axis.
15.5.1.1. Tools > Command Editor Example
>calculate area, <Location>, [<Axis>]
The specification of an axis is optional. If an axis is not specified, the value held in the object will be
used. To calculate the total area of the location, the axis specification should be left blank (that is, type
a comma after the location specification).
>calculate area, myplane calculates the area of the locator myplane projected onto a plane
normal to the axis specification in the CALCULATOR object.
>calculate area, myplane, calculates the area of the locator myplane. Note that adding the
comma after myplane removes the axis specification.
15.5.1.2. Tools > Function Calculator Example
The following example will calculate the total area of the locator Plane1:
Function: area, Location: Plane1.
15.5.2. areaAve
The areaAve function calculates the area-weighted average of a variable or expression on a 2D location.
The area-weighted average of a variable or expression is the average value of the variable or expression
on a location with the mesh element sizes taken into account. Without the area weighting function,
the average of all the nodal variable or expression values would be biased towards values in regions
of high mesh density.
areaAve[_<Axis>[_<Coord Frame>] ](<Variable|Expression>)@<Location>
where:
• <Axis> is x, y, or z.
• <Coord Frame> is available in CFD-Post only.
• <Variable|Expression> is a variable or expression.
• <Location> is any 2D region (such as a boundary or interface). An error is raised if the location specified
is not a 2D object.
242
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Quantitative Function List
To calculate the pressure coefficient Cp, use:
(Pressure - 1[bar])/(0.5*Density*(areaAve(Velocity)@inlet)^2)
You can create an expression using this, and then create a user variable using the expression. The user
variable can then be plotted on objects like any other variable.
Note
Projected areaAve (for example, areaAve_x) works as expected only for surfaces that do not
fold in the selected direction. In extreme case, if the surface is fully closed, the projected
average will result in a randomly large number, as the projected area will be zero.
15.5.2.1. Tools > Command Editor Example
>calculate areaAve, <Expression>, <Location>, <Axis>
15.5.2.2. Tools > Function Calculator Examples
• This example will calculate the average magnitude of Velocity on outlet.
Function: areaAve, Location: outlet, Variable: Velocity.
Note that flow direction is not considered because the magnitude of a vector quantity at each node
is calculated.
• You can use the scalar components of Velocity (such as Velocity u) to include a directional sign. This
example will calculate the area-weighted average value of Velocity u, with negative values of Velocity
u replaced by zero. Note that this is not the average positive value because zero values will contribute to
the average.
Function: areaAve, Location: outlet, Variable: max(Velocity u, 0.0[m s^-1]).
15.5.3. areaInt
The areaInt function integrates a variable over the specified 2D location. To perform the integration
over the total face area, select the None option from the Axis drop-down menu. If a direction is selected,
the result is an integration over the projected area of each face onto a plane normal to that direction.
Each point on a location has an associated area that is stored as a vector and therefore has direction.
By selecting a direction in the function calculator, you are using only a single component of the vector
in the area-weighting function. Because these components can be positive or negative, depending on
the direction of the normal on the location, it is possible for areas to cancel out. An example of this
would be on a closed surface where the projected area will always be zero (the results returned will
not in general be exactly zero because the variable values differ over the closed surface). On a flat surface,
the normal vectors always point in the same direction and never cancel out.
areaInt[_<Axis>[_<Coord Frame>] ](<Variable|Expression>)@<Location>
where:
• <Axis> is x, y, or z.
Axis is optional; if not specified the integration is performed over the total face area. If axis is specified,
then the integration is performed over the projected face area. A function description is available.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
243
Functions in ANSYS CFX
• <Coord Frame> is the coordinate frame.
• <Variable|Expression> is a variable or expression.
• <Location> is any 2D region (such as a boundary or interface). An error is raised if the location specified
is not a 2D object.
areaInt_y_Frame2(Pressure)@boundary1 calculates the pressure force acting in the Y direction
of the coordinate frame Frame2 on the locator boundary1. This differs from a calculation using the
force function, which calculates the total force on a wall boundary (that is, viscous forces on the
boundary are included).
15.5.3.1. Tools > Command Editor Example
>calculate areaInt, <Expression>, <Location>, [<Axis>]
Axis is optional. If it is not specified, the value held in the object will be used. To perform the integration
over the total face area, the axis specification should be blank (that is, type a comma after the location
name). A function description is available in areaInt (p. 243).
15.5.3.2. Tools > Function Calculator Examples
• This example integrates Pressure over Plane 1. The returned result is the total pressure force acting
on Plane 1. The magnitude of each area vector is used and so the direction of the vectors is not considered.
Function: areaInt, Location: Plane 1, Variable: Pressure, Direction: None
• This example integrates Pressure over the projected area of Plane 1 onto a plane normal to the X axis.
The result is the pressure force acting in the X direction on Plane 1. This differs slightly from using the
force function to calculate the X-directional force on Plane 1. The force function includes forces due to
the advection of momentum when calculating the force on an internal arbitrary plane or a non-wall
boundary (inlets, and so on).
Function: areaInt, Location: Plane 1, Variable: Pressure, Direction: Global X.
15.5.4. ave
The ave function calculates the arithmetic average of a variable or expression on the specified location.
Note
CFD-Post and CFX-Solver may compute slightly different average values due to differences
in how the average is computed:
• CFD-Post computes the arithmetically averaged vertex value for the location. Specifically, the
average is computed by summing the vertex values and then dividing by the number of vertices.
• CFX-Solver computes the arithmetically averaged face value for the location. Specifically, the
average is computed by summing the face values and then dividing by the number of faces. The
value for a particular face is computed by arithmetically averaging the vertex values of the face.
• Computation in CFX-Solver and CFD-Post can be made more consistent by using expert parameter
bcp arithmetic aver sum option. For details, see Discretization Parameters in the CFXSolver Modeling Guide.
244
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Quantitative Function List
Results will be biased towards areas of high nodal density on the location. To obtain a mesh independent
result, you should use the lengthAve, areaAve, volumeAve or massFlowAve functions.
ave(<Variable|Expression>)@<Location>
where:
• <Variable|Expression> is a variable or expression.
• <Location> is any 3D region (such as a domain or subdomain).
The ave function can be used on point, 1D, 2D, and 3D locations.
ave(Yplus)@Default calculates the mean Yplus values from each node on the default walls.
15.5.4.1. Tools > Command Editor Example
>calculate ave, <Variable|Expression>, <Location>
Note
To obtain a mesh-independent result, you should use the lengthAve, areaAve, volumeAve
or massFlowAve functions.
The average of a vector value is calculated as an average of its magnitudes, not the magnitude of
component averages. As an example, for velocity:
(15.1)
where
(15.2)
15.5.4.2. Tools > Function Calculator Example
This example calculates the mean temperature at all nodes in the selected domain.
Function: ave, Location: MainDomain, Variable: Temperature.
15.5.5. count
The count function returns the number of nodes on the specified location.
count()@<Location>
where:
• <Location> is valid for point, 1D, 2D, and 3D locations.
count()@Polyline1 returns the number of points on the specified polyline locator.
15.5.5.1. Tools > Command Editor Example
>calculate count, <Location>
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
245
Functions in ANSYS CFX
15.5.5.2. Tools > Function Calculator Example
This example returns the number of nodes in the specified domain.
Function: count, Location: MainDomain.
15.5.6. countTrue
The countTrue function returns the number of mesh nodes on the specified region that evaluate to
“true”, where true means greater than or equal to 0.5. The countTrue function is valid for 1D, 2D, and
3D locations.
countTrue(<Expression>)@<Location>
where <Expression> is:
• In CFD-Post, an expression that contains the logical operators =, >, <, <=, or >=.
• In CFX-Solver, an Additional Variable that you define. For example:
TemperatureLE = Temperature > 300[K]
countTrue(TemperatureLE)@Polyline1 returns the number of nodes on the specified polyline
locator that evaluate to true.
15.5.6.1. Tools > Command Editor Examples
In CFD-Post:
>calculate countTrue(Temperature > 300[K]), Domain1
In CFX-Solver:
>calculate countTrue(TemperatureLE), Domain1
15.5.6.2. Tools > Function Calculator Example
This example returns the number of nodes that evaluate to “true” in the specified domain.
Function: countTrue, Location: MainDomain, Expression: Temperature > 300[K].
15.5.7. force
This function returns the force exerted by the fluid on the specified 2D locator in the specified direction.
[<Phase>.]force[_<Axis>[_<Coord Frame>] ]()@<Location>
where:
• [<Phase>.] is an optional prefix that is not required for single-phase flows. For details, see CEL Functions
with Multiphase Flow (p. 236).
• <Axis> is x, y, or z
• <Coord Frame> is the coordinate frame
• <Location> is any 2D region (such as a boundary or interface).
246
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Quantitative Function List
Force calculations on boundaries require additional momentum flow data.
Water at RTP.force_x()@wall1 returns the total force in the X direction acting on wall1 due
to the fluid Water at RTP.
The force on a boundary is calculated using momentum flow data from the results file, if it is available.
The result can be positive or negative, indicating the direction of the force. For non-boundary locators,
an approximate force is always calculated.
CFD-Post calculates the approximate force as follows:
• If the locator is a wall boundary, the force is equal to the pressure force.
• For all other locators, the force is equal to the pressure force plus the mass flow force (due to the advection
of momentum).
• In all cases, if wall shear data exists in the results file, the viscous force is added to the calculated force.
The force function enables you to select the fluids to use when performing your calculation. The
result returned is the force on the locator due to that fluid/those fluids. Because the pressure force is
the same at each node irrespective of the choice of fluids, the only difference is in the viscous forces
(on wall boundaries) or the mass flow forces.
It is important to note that forces arising as a result of the reference pressure are not included in the
force calculation. You can include reference pressure effects in the force calculation in the CFX-Solver
by setting the expert parameter include pref in forces = t.
When performing transient simulations with rotating reference frames, forces may be reported in either
the stationary frame or the rotating frame. The forces reported by the CFX-Solver out file are always
given in the rotating frame. The forces reported by CFD-Post are reported in the stationary frame if the
‘Angular shift for Transient Rotating Domains’ option is active, as discussed in Angular Shift for Transient
Rotating Domains in the CFD-Post User's Guide.
15.5.7.1. Tools > Command Editor Example
>calculate force, <Location>, <Axis>, [<Phase>]
15.5.7.2. Tools > Function Calculator Examples
• This calculates the total force on the default wall boundaries in the X direction. Pressure and viscous forces
are included.
Function: force, Location: Default, Direction: Global X, Phase: All Fluids.
• This calculates the forces on inlet1 due to pressure and the advection of momentum.
Function: force, Location: inlet1, Direction: Global X, Phase: Water at RTP.
15.5.8. forceNorm
Returns the per unit width force on a line in the direction of the specified axis. It is available only for a
polyline created by intersecting a locator on a boundary. Momentum data must also be available. The
magnitude of the value returned can be thought of as the force in the specified direction on a polyline,
if the polyline were 2D with a width of one unit.
[<Phase>.]forceNorm[_<Axis>[_<Coord Frame>] ]()@<Location>
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
247
Functions in ANSYS CFX
where:
• [<Phase>.] is an optional prefix that is not required for single-phase flows. For details, see CEL Functions
with Multiphase Flow (p. 236).
• <Axis> is x, y, or z
• <Coord Frame> is available in CFD-Post only
• <Location> is any 1D location. An error will be raised if the location specified is not one-dimensional.
forceNorm_y()@Polyline1 calculates the per unit width force in the Y direction on the selected
polyline.
15.5.8.1. Tools > Command Editor Example
>calculate forceNorm, <Location>, <Axis>, [<Phase>]
15.5.8.2. Tools > Function Calculator Example
The result from this calculation is force per unit width on Polyline1 in the X direction.
Function: forceNorm, Location: Polyline1, Direction: Global X, Phase: All Fluids.
15.5.9. inside
The inside CEL function is essentially a step function variable, defined to be unity within a subdomain
and zero elsewhere. This is useful for describing different initial values or fluid properties in different
regions of the domain. It is similar to the CEL subdomain variable, but allows a specific 2D or 3D location
to be given. For example, 273 [K] * inside()@Subdomain 1 has a value of 273 [K] at points
in Subdomain 1 and 0 [K] elsewhere. The location does not need to be a subdomain, but can be any
2D or 3D named sub-region of the physical location on which the expression is evaluated. For immersed
solids simulations, the location can also be a specific immersed solid domain, and the inside function
will be updated automatically at the beginning of each time step.
inside()@<Location>
where:
• <Location> is any 2D or 3D named sub-region of the physical location on which the expression is evaluated.
• <Location> can also be an immersed solid domain on which the expression is evaluated dynamically.
Note
The inside CEL function is not available in CFD-Post.
15.5.9.1. Tools > Command Editor Example
>calculate inside, <Location>
15.5.10. length
Computes the length of the specified line as the sum of the distances between the points making up
the line.
248
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Quantitative Function List
length()@<Location>
where:
• <Location> is any 1D location. Specifying a 2D location will not produce an error; the sum of the edge
lengths from the elements in the locator will be returned.
length()@Polyline1 returns the length of the polyline.
15.5.10.1. Tools > Command Editor Example
>calculate length, <Location>
Note
While using this function in Power Syntax, the leading character is capitalized to avoid confusion with the Perl internal command “length”.
15.5.10.2. Tools > Function Calculator Example
This example calculates the length of a polyline.
Function: length, Location: Polyline1.
15.5.11. lengthAve
Computes the length-based average of the variable or expression on the specified line. This is the 1D
equivalent of the areaAve function. The results is independent of the nodal distribution along the
line because a weighting function assigns a higher weighting to areas of sparse nodal density.
lengthAve(<Variable|Expression>)@<Location>
where:
• <Variable|Expression> is a variable or expression.
• <Location> is any 1D or 2D location.
lengthAve(T)@Polyline1 calculates the average temperature on Polyline1 weighted by the
distance between each point (T is the system variable for temperature).
15.5.11.1. Tools > Command Editor Example
>calculate lengthAve, <Expression>, <Location>
15.5.11.2. Tools > Function Calculator Example
This calculates the average velocity on the location Polyline1 using a length-based weighting function
to account for the distribution of points along the line.
Function: lengthAve, Location: Polyline1, Variable: Velocity.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
249
Functions in ANSYS CFX
15.5.12. lengthInt
Computes the length-based integral of the variable or expression on the specified line. This is the 1D
equivalent of the areaInt function.
lengthInt(<Variable|Expression>)@<Location>
where:
• <Variable|Expression> is a variable or expression.
• <Location> is any 1D location.
15.5.12.1. Tools > Command Editor Example
>calculate lengthInt, <Expression>, <Location>.
15.5.13. mass
mass()@<Location>
where:
• <Location> is any 3D region (such as a domain or subdomain).
15.5.14. massAve
massAve(<Variable|Expression>)@<Location>
where:
• <Variable|Expression> is a variable or expression.
• <Location> is any 3D region (such as a domain or subdomain).
15.5.15. massFlow
Computes the mass flow through the specified 2D location.
[<Phase>.]massFlow()@<Location>
where:
• [<Phase>.] is an optional prefix that is not required for single-phase flows. For details, see CEL Functions
with Multiphase Flow (p. 236).
• <Location> is any fluid surfaces (such as Inlets, Outlets, Openings and fluid-fluid interfaces).
Air at STP.massFlow()@DegassingOutlet calculates the mass flow of Air at STP through
the selected location.
For boundary locators:
250
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Quantitative Function List
• The mass flow is calculated using mass flow data from the results file, if it is available1. Otherwise, an approximate mass flow is calculated.
• For multiphase cases, the mass flow through a boundary on a GGI interface evaluated in CFD-Post is an approximation to the 'exact' mass flow evaluated by the solver. This approximation vanishes as the mesh is
refined or as the volume fraction on the interface becomes uniform.
For non-boundary locators (that is, internal locators):
• If the locator is an edge based locator (such as a slice plane or isosurface), the domain mass flow data from
the results file will be used.
• In all other cases, an approximate mass flow is calculated.
• There is a limitation with the massFlow function on isosurfaces and slice planes that cross non-matching
(that is, not 1-to-1) periodic interfaces. In such cases, the computed mass flow may not be accurate. To
perform a more accurate mass flow calculation, the following expression can be used:
areaInt_x(Velocity u * Density)@myLoc + areaInt_y(Velocity v * Density)@my
Loc + areaInt_z(Velocity w * Density)@myLoc
The massFlow function enables you to select the fluids to use when performing your calculation. The
result returned is the mass flow of the selected fluids through the locator.
If a user specifies a boundary mass source, this mass source is not included in the massFlow calculator.
This will affect all massFlow related calculations, such as massFlowInt().
15.5.15.1. Mass Flow Sign Convention
The mass flow through a surface is defined by
where is the velocity vector and is the surface
normal vector. By convention, the surface normal at a domain boundary is directed out of the domain.
Therefore, the mass flow is positive at an inlet boundary with the velocity directed into the domain.
For planes and surfaces that cut through a domain, the normal of the plane or surface is determined
by from the right-hand rule and the manner in which the plane or surface is constructed. For example,
the surface normal for a Z-X plane has the same sense and direction as the Y axis.
15.5.15.2. Tools > Command Editor Example
>calculate massFlow, <Location>, [<Phase>]
15.5.15.3. Tools > Function Calculator Example
This calculates the mass flow for all fluids in the domains through the location outlet2:
Function: massFlow, Location: outlet2, Phase: All Fluids.
1
The availability depends on the setting for Output Boundary Flows for the file (see Output Boundary Flows Check Box in the CFX-Pre
User's Guide for details).
In addition to this, mass flow information written to a backup file at time zero is not accurate. To calculate accurate mass flow
from a backup file, use information from the backup file written after the first timestep/iteration of the run.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
251
Functions in ANSYS CFX
15.5.16. massFlowAve
Computes the average of a variable or expression on the specified 2D location. The massFlowAve
function enables you to select the fluids to use for the calculation. The returned result is the average
variable or expression value, evaluated according to the formula:
(15.3)
where represents the variable or expression being averaged and represents the local mass flow
(net local mass flow if more than one fluid is selected). Each summation term is evaluated on, and corresponds to, a node on the 2D locator. The mass flow for each term is derived from summing contributions from the surrounding solver integration points. As a result, the denominator evaluates to the
conservative net mass flow through the 2D locator.
In cases where there is significant flow, but little or no net flow through the 2D locator (as can happen
with recirculation), the denominator of the averaging formula becomes small, and the resulting average
value may become adversely affected. In such cases, the massFlowAveAbs (see massFlowAveAbs (p. 252)) function is a viable alternative to the massFlowAve function.
[<Phase>.]massFlowAve(<Variable|Expression>)@<Location>
where:
• [<Phase>.] is an optional prefix that is not required for single-phase flows. For details, see CEL Functions
with Multiphase Flow (p. 236).
• <Variable|Expression> is a variable or expression.
• <Location> is any fluid surfaces (such as Inlets, Outlets, Openings and fluid-fluid interfaces). An error is
raised if the location specified is not 2D.
massFlowAve(Density)@Plane1 calculates the average density on Plane1 weighted by the mass
flow at each point on the location.
See the Advanced Mass Flow Considerations (p. 253) and Mass Flow Technical Note (p. 253) sections
under massFlowAveAbs (p. 252) for more information.
15.5.16.1. Tools > Command Editor Example
>calculate massFlowAve, <Variable|Expression>, <Location>, [<Phase>]
15.5.16.2. Tools > Function Calculator Example
This example calculates the average velocity on Plane1 weighted by the mass flow for all fluids assigned
to each point on Plane1:
Function: massFlowAve, Location: Plane1, Variable: Velocity, Phase: All Fluids
15.5.17. massFlowAveAbs
This function is similar to the massFlowAve function (see massFlowAve (p. 252)), except that each
local mass flow value used in the averaging formula has the absolute function applied. That is:
(15.4)
252
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Quantitative Function List
[<Phase>.]massFlowAveAbs(<Variable|Expression>)@<Location>
where:
• [<Phase>.] is an optional prefix that is not required for single-phase flows. For details, see CEL Functions
with Multiphase Flow (p. 236).
• <Variable|Expression> is a variable or expression.
• <Location> is any fluid surfaces (such as Inlets, Outlets, Openings and fluid-fluid interfaces). An error is
raised if the location specified is not 2D.
massFlowAve(Density)@Plane1 calculates the average density on Plane1 weighted by the mass
flow at each point on the location.
In cases where there is significant flow, but little or no net flow through the 2D locator (as can happen
with recirculation), the massFlowAveAbs function is a viable alternative to the massFlowAve function
(see massFlowAve (p. 252)).
15.5.18. Advanced Mass Flow Considerations
Note that the massFlowAveAbs and massFlowAve functions provide the same result, and that the
denominator evaluates to the net mass flow through the 2D locator, only when all of the flow passes
through the 2D locator in the same general direction (that is, when there is no backflow). If there is any
backflow through the 2D locator, the denominator in the function for massFlowAveAbs evaluates to
a value of greater magnitude than the conservative net mass flow through the 2D locator (although
this is not necessarily harmful to the resulting average value).
The values of variables other than mass flow are stored at the mesh nodes and are applied to the locator nodes by linear interpolation. For the mass flow variable, CFD-Post uses the integration point mass
flow data if it is available; otherwise, it will approximate mass flow values based on mesh node values
of velocity (and density, if available).
15.5.19. Mass Flow Technical Note
When integration point mass flow data is stored, backflow through the 2D locator may occur as an artifact of how the mass flow data is applied to the locator nodes, even though there may be no actual
backflow (as evidenced by a vector plot on the locator). The figure below illustrates how this may occur.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
253
Functions in ANSYS CFX
Figure 15.1: Backflow
In order to visualize this type of backflow through a locator, try making a contour plot of the variable
Mass Flow, setting a user defined Range from 0 to 1 and the # of Contours to 3. This will produce
a contour plot with two color bands: one for each general flow direction. This visualization technique
works because the method of applying integration-point mass-flow data to locator nodes is the same
for all uses of the mass flow variable involving a 2D locator (contour plots, massFlowAve, massFlowAveAbs, and so on).
15.5.20. massFlowInt
Integrates a variable or expression over the specified 2D location. A weighting function is applied to
the variable or expression value at each point based on the mass flow assigned to that point. You can
also specify the fluid(s) used to calculate the mass flow at each locator point.
[<Phase>.]massFlowInt(<Variable|Expression>)@<Location>
where:
• [<Phase>.] is an optional prefix that is not required for single-phase flows. For details, see CEL Functions
with Multiphase Flow (p. 236).
• <Variable|Expression> is a variable or expression.
• <Location> is any fluid surfaces (such as Inlets, Outlets, Openings and fluid-fluid interfaces). An error is
raised if the location specified is not 2D.
254
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Quantitative Function List
15.5.20.1. Tools > Command Editor Example
>calculate massFlowInt, <Variable|Expression>, <Location>, [<Phase>]
15.5.20.2. Tools > Function Calculator Example
This example integrates pressure over Plane1. The result is the pressure force acting on Plane1 weighted
by the mass flow assigned to each point on Plane1:
Function: massFlowInt, Location: Plane1, Variable: Pressure, Phase: All Fluids
15.5.21. massInt
The mass-weighted integration of a variable or expression within a domain or subdomain.
massInt(<Variable|Expression>)@<Location>
where:
• <Variable|Expression> is a variable or expression.
• <Location> is any 3D region (such as a domain or subdomain).
15.5.22. maxVal
Returns the maximum value of the specified variable or expression on the specified locator. You should
create a user variable if you want to find the maximum value of an expression.
maxVal(<Variable|Expression>)@<Location>
where:
• <Variable|Expression> is a variable or expression.
• <Location> is, in the context of CFX-Solver, a 2D region or 3D region (such as a domain or subdomain)
or, in the context of CFD-Post, a Point object or a 1D, 2D, or 3D locator.
15.5.22.1. Tools > Command Editor Example
>calculate maxVal, <Variable|Expression>, <Location>
15.5.22.2. Tools > Function Calculator Example
This will return the maximum Yplus value on the default wall boundaries:
Function: maxVal, Location: Default, Variable: Yplus
15.5.23. minVal
Returns the minimum value of the specified variable or expression on the specified locator. You should
create a user variable if you want to find the minimum value of an expression.
minVal(<Variable|Expression>)@<Location>
where:
• <Variable|Expression> is a variable or expression.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
255
Functions in ANSYS CFX
• <Location> is, in the context of CFX-Solver, a 2D region or 3D region (such as a domain or subdomain)
or, in the context of CFD-Post, a Point object or a 1D, 2D, or 3D locator.
15.5.23.1. Tools > Command Editor Example
>calculate minVal, <Variable|Expression>, <Location>
15.5.23.2. Tools > Function Calculator Example
These settings will return the minimum temperature in the domain:
Function: minVal, Location: MainDomain, Variable: Temperature
15.5.24. probe
Returns the value of the specified variable or expression on the specified Point object.
probe(<Variable|Expression>)@<Location>
where:
• <Variable|Expression> is a variable or expression.
• <Location> is any point object (such as a Source Point or Cartesian Monitor Point).
Important
This calculation should be performed only for point locators described by single points. Incorrect solutions will be produced for multiple point locators.
15.5.24.1. Tools > Command Editor Example
>calculate probe, <Expression>, <Location>
15.5.24.2. Tools > Function Calculator Example
This example returns the density value at Point1:
Function: probe, Location: Point1, Variable: Density
15.5.25. rbstate
Returns the value of the specified rigid body state variable, or axis component thereof, on the specified:
• Rigid Body object (for a standard rigid body definition), or
• Immersed Solid domain that is governed by a rigid body solution.
The rigid body state variables are:
• Position
• Linear Velocity
• Linear Acceleration
256
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Quantitative Function List
• Euler Angle
• Angular Velocity
• Angular Acceleration
Syntax:
rbstate(<rbvar>[<Axis>])@<Location>
where:
• <rbvar> is a rigid body state variable.
• <Axis> is X, Y, or Z.
For the Euler Angle rigid body state variable, an axis must be specified. For all of the other rigid
body state variables, the axis is optional. If you do not specify an axis, the magnitude of the vector
is returned. For example, if the variable is Position and you do not specify an axis, the distance
from the origin will be returned.
• <Location> is any rigid body object or any immersed solid domain that is governed by a rigid body
solution.
Results are given with respect to the global coordinate frame (Coord 0).
15.5.25.1. Expressions Details View Example
rbstate(Linear Velocity Z)@Buoy
15.5.26. rmsAve
The rmsAve function calculates the RMS average of a variable or expression on the specified location.
• CFX-Solver computes the RMS average of the vertex values for a 3D location.
• CFX-Solver computes the RMS average of the face values for a 2D location. The value for a particular face is
computed by arithmetically averaging the vertex values of the face.
rmsAve(<Variable|Expression>)@<Location>
where:
• <Variable|Expression> is a variable or expression.
• <Location> is a 2D region or 3D region (such as a domain or subdomain).
15.5.27. sum
The sum function calculates the sum of a variable or expression on the specified location.
Note
CFD-Post and CFX-Solver compute the sum in different ways:
• CFD-Post computes the sum of the vertex values for the location.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
257
Functions in ANSYS CFX
• CFX-Solver computes the sum of the vertex values for a 3D location.
• CFX-Solver computes the sum of the face values for a 2D location. The value for a particular face
is computed by arithmetically averaging the vertex values of the face.
sum(<Variable|Expression>)@<Location>
where:
• <Variable|Expression> is a variable or expression.
• <Location> is, in the context of CFX-Solver, a 2D region or 3D region (such as a domain or subdomain)
or, in the context of CFD-Post, a Point object or a 1D, 2D, or 3D locator.
15.5.27.1. Tools > Command Editor Example
>calculate sum, <Variable|Expression>, <Location>
15.5.27.2. Tools > Function Calculator Example
This example returns the sum of the finite volumes assigned to each node in the location SubDomain1.
In this case, this sums to the volume of the subdomain:
Function: sum, Location: SubDomain1, Variable: Volume of Finite Volume
15.5.28. torque
Returns the torque on a 2D locator about the specified axis. The force calculated during evaluation of
the torque function has the same behavior as the force function. For details, see force (p. 246). You can
select the fluids involved in the calculation.
[<Phase>.]torque_[<Axis>[_<Coord Frame>] ]()@<Location>
where:
• [<Phase>.] is an optional prefix that is not required for single-phase flows. For details, see CEL Functions
with Multiphase Flow (p. 236).
• <Axis> is x, y, or z
• <Coord Frame>
• <Location> is any 2D region (such as a wall). If the location specified is not 2D, an error is raised.
15.5.28.1. Tools > Command Editor Example
>calculate torque, <Location>, <Axis>, [<Phase>]
15.5.28.2. Tools > Function Calculator Example
This example calculates the torque on Plane1 about the Z axis due to all fluids in the domain.
Function: torque, Location: Plane1, Axis: Global Z, Phase: All Fluids
258
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Quantitative Function List
15.5.29. volume
Calculates the volume of a 3D location.
volume()@<Location>
where:
• <Location> is any 3D region (such as a domain or subdomain). An error is raised if the location specified
is not a 3D object. For details, see volume (p. 259).
15.5.29.1. Tools > Command Editor Example
>calculate volume, <Location>
15.5.29.2. Tools > Function Calculator Example
This example returns the sum of the volumes of each mesh element included in the location Volume1.
Function: volume, Location: Volume1
15.5.30. volumeAve
Calculates the volume-weighted average of a variable or expression on a 3D location. This is the 3D
equivalent of the areaAve function. The volume-weighted average is the average value on a location
weighted by the volume assigned to each vertex on a location. Without the volume weighting function,
the average of all the nodal values would be biased towards values in regions of high mesh density.
The following example demonstrates use of the function.
volumeAve(<Variable|Expression>)@<Location>
where:
• <Variable|Expression> is a variable or expression.
• <Location> is any 3D region (such as a domain or subdomain).
15.5.30.1. Tools > Command Editor Example
>calculate volumeAve, <Variable|Expression>, <Location>
15.5.30.2. Tools > Function Calculator Example
This example calculates the volume-weighted average value of density in the region enclosed by the
location Volume1:
Function: volumeAve, Location: Volume1, Variable: Density
15.5.31. volumeInt
Integrates the specified variable or expression over the volume location. This is the 3D equivalent of
the areaInt function.
volumeInt(<Variable|Expression>)@<Location>
where:
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
259
Functions in ANSYS CFX
• <Variable|Expression> is a variable or expression.
• <Location> is any 3D region (such as a domain or subdomain). An error is raised if the location specified
is not a 3D object.
For example, volumeInt(Density)@StaticMixer will calculate the total fluid mass in the domain
StaticMixer.
Note
Because the Density variable represents the average density during the timestep rather than
the density at the end of the timestep, the volumeInt(Density) does not accurately
give the mass of fluid at the end of a timestep. Use the mass() function instead.
The volumeInt function does not take into account the porosity of the location specified for
porous domains. To include the porosity effect in your calculation, you need to manually
multiply your argument by:
• The Volume Porosity if you want to evaluate the integral on the fluid side
• (1-Volume Porosity) if you want to evaluate the integral on the solid side
15.5.31.1. Tools > Command Editor Example
>calculate volumeInt, <Variable|Expression>, <Location>
15.5.31.2. Tools > Function Calculator Example
This example calculates the integral of density (the total mass) in Volume1.
Function: volumeInt, Location: Volume1, Variable: Density
260
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 16: Variables in ANSYS CFX
This chapter describes the variables available in ANSYS CFX:
16.1. Hybrid and Conservative Variable Values
16.2. List of Field Variables
16.3. Particle Variables Generated by the Solver
16.4. Miscellaneous Variables
16.1. Hybrid and Conservative Variable Values
The CFX-Solver calculates the solution to your CFD problem using polyhedral finite volumes surrounding
the vertices of the underlying mesh elements (hexahedrons, tetrahedrons, prisms, pyramids). Analytical
solutions to the Navier-Stokes equations exist for only the simplest of flows under ideal conditions. To
obtain solutions for real flows, a numerical approach must be adopted whereby the equations are replaced by algebraic approximations that may be solved using a numerical method.
The solution values on the boundary vertices, called conservative values, are the values obtained from
solving the conservation equations for the boundary control volumes. These values are not necessarily
the same as the specified boundary condition values, although the specified boundary value is used to
close boundary fluxes for the boundary control volume. For example, on a no-slip wall, the wall velocity
is used to compute the viscous force for the boundary face of the boundary control volume, but the
resulting control volume equation solution will not necessarily be the wall velocity. The conservative
values are representative of the boundary control volume, not the boundary itself. For visualization
purposes, it is often useful to view the specified boundary condition value for the boundary vertices
rather than the conservative values. This is especially true when the value of a conservative solution
variable (such as pressure or temperature, for instance) is specified at a particular boundary condition.
The specified boundary values are called hybrid values. CFD-Post uses hybrid values by default for most
variables. Hybrid values are obtained by overwriting the conservative results on the boundary nodes
produced by the CFX-Solver with values based on the specified boundary conditions. This ensures, for
example, that the velocity is displayed as zero on no-slip walls. For quantitative calculations, the conservative values should normally be used because they are consistent with the discrete solutions obtained
by the solver. If you want to use these values in CFD-Post, you can select them from the Variables
Editor dialog box as described above. By default, CFD-Post uses conservative values when the Calculate
command is used.
The difference between hybrid and conservative values at wall boundaries can be demonstrated using
the following figure:
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
261
Variables in ANSYS CFX
Using velocity as an example, the velocity value calculated at a mesh node is based upon the ‘average’
in the control volume surrounding that node. For calculation purposes, the entire control volume is
then assumed to possess that velocity. At a boundary node, its surrounding control volume includes
an area in the bulk of the fluid (this area is highlighted around the boundary node marked 1). Hence,
the conservative velocity calculated at the wall node is not zero, but an ‘average’ over the control
volume adjacent to the boundary. At a wall boundary node the difference between conservative and
hybrid values can be illustrated by considering the case of the mass flow rate through the wall-adjacent
control volume. If a zero velocity was enforced at the boundary node, then this would produce zero
mass flow through the control volume, which is clearly not correct.
16.1.1. Solid-Fluid Interface Variable Values
16.1.1.1. Conservative Values at 1:1 Interface
At a solid-fluid 1:1 interface, duplicate nodes exist. The conservative value for the solid-side node is the
variable values averaged over the half on the control volume that lies inside the solid. The conservative
value for the fluid-side node is the variable values averaged over the half of the control volume that
lies in the fluid.
Consider the example of heat transfer from a hot solid to a cool fluid when advection dominates within
the fluid. If you create a plot across the solid-fluid interface using conservative values of temperature,
then you will see a sharp change in temperature across the interface. This is because values are interpolated from the interface into the bulk of the solid domain using the value for the solid-side node at
the interface, while values are interpolated from the interface into the bulk of the fluid domain using
the value for the fluid-side node at the interface. This results in a temperature discontinuity at the interface.
16.1.1.2. Hybrid Values at 1:1 Interface
When creating plots using hybrid variable values (the default in CFD-Post), the 1:1 interface is single
valued and takes the solid-side conservative value. You can therefore expect to see the same plot
within the solid, but the temperature profile between the interface and the first node in the fluid interpolates between the solid-side interface value and the first fluid node value. In this case, a discontinuity
does not exist because all nodes are single valued.
Conservative values should be used for all quantitative calculations.
262
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
List of Field Variables
16.1.1.3. Conservative Values on a GGI Interface
At a GGI interface, the CFX Solver calculates both fluid-side and solid-side temperatures based on heat
flux conservation. These values are representative of the temperature within the half-control volumes
around the vertices on the interface. The fluid-side and solid-side temperatures are generally not equal.
As a result, a plot of conservative values of temperature will generally show a discontinuity across a
GGI interface.
16.1.1.4. Hybrid Values on a GGI Interface
At a GGI interface, the CFX Solver calculates a "surface temperature" based on a flux-conservation
equation for the 'control surfaces' that lie between the fluid side and the solid side. The surface temperature is usually between the fluid-side and solid-side temperatures. Hybrid values of temperature on a
GGI interface are set equal to the surface temperature. As a result, there is no discontinuity in hybrid
values of temperature across a GGI interface.
16.2. List of Field Variables
This section contains a list of field variables that you may have defined in CFX-Pre or that are available
for viewing in CFD-Post and exporting to other files. Many variables are relevant only for specific
physical models.
The information given in this section includes:
• Long Variable Name: The name that you see in the user interface.
• Short Variable Name: The name that must be used in CEL expressions.
• Units: The default units for the variable. An empty entry [ ] indicates a dimensionless variable.
Note
The entries in the Units columns are SI but could as easily be any other system of units.
• In the Availability column:
– A number represents the user level (1 indicates that the variable appears in default lists, 2 and 3 indicate
that the variable appears in extended lists that you see when you click
). This number is useful when
using the CFX Export facility. For details, see File Export Utility in the CFX-Solver Manager User's Guide.
Note that the CFX-Solver may sometimes override the user-level setting depending on the physics of the
problem. In these cases, the User Level may be different from that shown in the tables that follow.
– Boundary (B): A B in this column indicates that the variable contains only non-zero values on the
boundary of the model. See Boundary-Value-Only Variables in the CFD-Post User's Guide for more details.
Boundary-Value-Only Variables in the CFD-Post User's Guide describes the useful things that you
can do with variables that are defined only on the boundaries of the model.
– A indicates the variable is available for mesh adaption
– C indicates the variable is available in CEL
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
263
Variables in ANSYS CFX
– DT indicates the variable is available for data transfer to ANSYS
– M indicates the variable is available for monitoring
– P indicates the variable is available for particle user-routine argument lists
– PR indicates the variable is available for particle results
– R indicates the variable is available to be output to the results, transient results, and backup files
– RA indicates the variable is available for radiation results
– TS indicates the variable is available for transient statistics
• Definition: Defines the variable.
This is not a complete list of variables. Information on obtaining details on all variables is available in
RULES and VARIABLES Files in the CFX-Solver Manager User's Guide.
Note
Variables with names shown in bold text are not output to CFD-Post. However, some of
these variables can be output to CFD-Post by selecting them from the Extra Output Variables
List on the Results tab of the Solver > Output Control details view of CFX-Pre.
16.2.1. Common Variables Relevant for Most CFD Calculations
The following table contains a list of variables (with both long and short variable names) that can be
used when working with CFD calculations. For an explanation of the column headings, see List of Field
Variables (p. 263).
Long
Variable
Name
Short
Variable
Name
Units
Availability
Definition
Density
density
[kg m^-3]
1
Mass per unit volume.
A, C, M,
P, R, TS
Note that for fixed
composition, variable
composition, and reacting
mixtures, when density is
governed by the Ideal
Mixture option, the
density is determined by a
mass-fraction-weighted
harmonic average:
2
Dynamic viscosity ( ), also
called absolute viscosity, is
a measure of the resistance
of a fluid to shearing
Dynamic
Viscosity
viscosity
[kg m^-1 s^-1]
A, C, M,
P, R, TS
264
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
List of Field Variables
Long
Variable
Name
Short
Variable
Name
Units
Availability
Definition
forces, and appears in the
momentum equations.
Using an expression to set
the dynamic viscosity is
possible. For details, see
Non-Newtonian Flow in
the CFX-Solver Modeling
Guide.
Velocitya
vel
[m s^-1]
1
Velocity vector.
A, C, M,
P, R, TS
Velocity
u
u
[m s^-1]
v
Velocity
v
1
Components of velocity.
A, C, M,
P, R, TS
w
Velocity
w
Pressure
p
[kg m^-1 s^-2]
1
A, C, M,
P, R, TS
Static
Pressure
pstat
[kg m^-1 s^-2]
3
Both Pressure and
Total Pressure are
measured relative to the
reference pressure that you
specified on the Domains
panel in CFX-Pre.
Additionally, Pressure is
the total normal stress,
which means that when
using the k-e turbulence
model, Pressure is the
thermodynamic pressure
plus the turbulent normal
stress. Static Pres
sure is the
thermodynamic pressure,
in most cases this is the
same as Pressure. For
details, see Modified
Pressure in the CFX-Solver
Theory Guide.
CFX solves for the relative
Static Pressure
(thermodynamic pressure)
in the flow field, and
is related to Absolute
Pressure
.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
265
Variables in ANSYS CFX
Long
Variable
Name
Short
Variable
Name
Units
Availability
Definition
Total
Pressure
ptot
[kg m^-1 s^-2]
2
The total pressure,
, is
defined as the pressure
that would exist at a point
if the fluid was brought
instantaneously to rest
such that the dynamic
energy of the flow
converted to pressure
without losses. The
following three sections
describe how total
pressure is computed for a
pure component material
with constant density, ideal
gas equation of state and
a general equation of state
(CEL expression or RGP
table). For details, see
Scalable Wall Functions in
the CFX-Solver Theory
Guide.
A, C, M,
P, R, TS
Wall
Shear
wall
shear
Pa
Volume
of Finite
Volume
X
coordinate
3,B
For details, see Scalable
Wall Functions in the
CFX-Solver Theory Guide.
3
Volume of finite volume.
For details, see
Discretization of the
Governing Equations in the
CFX-Solver Theory Guide.
C, DT, R,
TS
x
[m]
2
Cartesian coordinate
components.
C
Y
coordinate
y
[m]
2
C
Z
coordinate
z
[m]
2
C
Kinematic
Diffusivity
visckin
2
C, M, P,
R, TS
266
Kinematic diffusivity
describes how rapidly a
scalar quantity would
move through the fluid in
the absence of convection.
For convection-dominated
flows, the kinematic
diffusivity can have little
effect because convection
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
List of Field Variables
Long
Variable
Name
Short
Variable
Name
Units
Availability
Definition
processes dominate over
diffusion processes.
Shear
Strain
Rate
sstrnr
Specific
Heat
Capacity
at
Constant
Pressure
Cp
Specific
Heat
Capacity
at
Constant
Volume
Cv
Thermal
Conductivity
cond
[s^-1]
2
A, C, M,
R, TS
[m^2 s^-2
K^-1]
2
A, C, M,
R, TS
[m^2 s^-2
K^-1]
For details see
Non-Newtonian Flow in
the CFX-Solver Modeling
Guide.
For details, see Specific
Heat Capacity in the
CFX-Solver Modeling Guide.
2
A, C, M,
P, R, TS
[kg m s^-3
K^-1]
2
A, C, M,
R, TS
Thermal conductivity, , is
the property of a fluid that
characterizes its ability to
transfer heat by
conduction.
For details, see Thermal
Conductivity in the
CFX-Solver Modeling Guide.
Temperature
T
[K]
1
A, C, DT,
M, P, R,
TS
Total
Temperature
Ttot
[K]
1
A, C, M,
P, R, TS
The static temperature,
, is the
thermodynamic
temperature, and depends
on the internal energy of
the fluid. In CFX,
depending on the heat
transfer model you select,
the flow solver calculates
either total or static
enthalpy (corresponding
to the total or thermal
energy equations). For
details, see Static
Temperature in the
CFX-Solver Theory Guide.
The total temperature is
derived from the concept
of total enthalpy and is
computed exactly the
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
267
Variables in ANSYS CFX
Long
Variable
Name
Short
Variable
Name
Units
Availability
Definition
same way as static
temperature, except that
total enthalpy is used in
the property relationships.
For details, see Total
Temperature in the
CFX-Solver Theory Guide.
Wall
Heat
Flux
Qwall
Wall
Heat
Transfer
Coefficient
htc
Total
Enthalpy
htot
Static
Enthalpy
[W m^-2]
2,B
C, DT, R,
TS
[W m^-2
K^-1]
2,B
C, R, TS
A heat flux is specified
across the wall boundary.
A positive value indicates
heat flux into the domain.
For multiphase cases,
when the bulk heat flux
into both phases is set, this
option is labeled Wall Heat
Flux instead of Heat Flux.
When set on a per fluid
basis, this option is
labelled Heat Flux.
For details, see Heat
Transfer Coefficient and
Wall Heat Transfer
Coefficient in the
CFX-Solver Modeling Guide.
[m^2 s^-2]
enthalpy
[m^2 s^-2]
A, C, M,
R, TS
For details, see Transport
Equations in the CFX-Solver
Theory Guide.
2
For details, see Static
Enthalpy in the CFX-Solver
Theory Guide.
A, C, M,
P, R, TS
a
When a rotating frame of reference is used, all variables in the CFX-5 results file are relative to the rotating frame, unless specified
as a Stn Frame variable.
16.2.2. Variables Relevant for Turbulent Flows
The following table contains a list of variables (with both long and short variable names) that can be
used when working with turbulent flows. For an explanation of the column headings, see List of Field
Variables (p. 263).
A B in the Type column indicates that the variable contains only non-zero values on the boundary of
the model.
268
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
List of Field Variables
Long
Variable
Name
Short
Variable
Name
Units
Availability
Definition
Blending
Function
for DES
model
desbf
[]
2
Controls blending between
RANS and LES regimes for
the DES model
Turbulence
Kinetic
Energy
ke
Turbulence
Eddy
Dissipation
ed
Turbulent
Eddy
Frequency
tef
Eddy
Viscosity
eddy
viscosity
Reynolds
Stress
C, M, R,
TS
[m^2
s^-2]
1
A, C, M,
P, R, TS
[m^2
s^-3]
1
A, C, M,
P, R, TS
[s^-1]
For details, see The
k-epsilon Model in the
CFX-Solver Modeling Guide.
The rate at which the
velocity fluctuations
dissipate. For details, see
The k-epsilon Model in the
CFX-Solver Modeling Guide.
1
A, C, M,
P, R, TS
rs
[kg
m^-1
s-1]
2
[m^2
s^-2]
2
A, C, M,
P, R, TS
A, C, M,
P, R, TS
Statistical
Reynolds
Stress uu
rsstat
uu
Statistical
Reynolds
Stress vv
rsstat
vv
[m^2
s^-2]
3
M, R
[m^2
s^-2]
3
M, R
The “eddy viscosity model”
proposes that turbulence
consists of small eddies
that are continuously
forming and dissipating,
and in which the Reynolds
stresses are assumed to be
proportional to mean
velocity gradients. For
details, see Eddy Viscosity
Turbulence Models in the
CFX-Solver Theory Guide.
This is a tensor quantity
with six components. For
details, see Statistical
Reynolds Stresses in the
CFX-Solver Modeling Guide
and Reynolds Stress
Turbulence Models in the
CFX-Solver Theory Guide in
the ANSYS CFX
documentation.
In LES runs, Reynolds
Stress components are
automatically generated
using running statistics of
the instantaneous,
transient velocity field. For
details, see Statistical
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
269
Variables in ANSYS CFX
Long
Variable
Name
Short
Variable
Name
Units
Availability
Definition
Statistical
Reynolds
Stress
ww
rsstat
ww
[m^2
s^-2]
3
Reynolds Stresses in the
CFX-Solver Modeling Guide.
Statistical
Reynolds
Stress uv
rsstat
uv
Statistical
Reynolds
Stress
uw
rsstat
uw
Statistical
Reynolds
Stress
vw
rsstat
vw
Velocity
Correlation
uu
uu
Velocity
Correlation
vv
vv
Velocity
Correlation
ww
ww
Velocity
Correlation
uv
uv
Velocity
Correlation
uw
uw
Velocity
Correlation
vw
vw
Yplus
yplusstd
M, R
[m^2
s^-2]
3
M, R
[m^2
s^-2]
3
M, R
[m^2
s^-2]
3
M, R
[m^2
s^-2]
3
C, M, R
[m^2
s^-2]
3
C, M, R
[m^2
s^-2]
3
C, M, R
[m^2
s^-2]
3
C, M, R
[m^2
s^-2]
3
C, M, R
[m^2
s^-2]
3
C, M, R
[]
2,B
C, R, TS
Solver
Yplus
yplus
[]
2,B
C, R, TS
270
These variables represent
the instantaneous velocity
correlation and are used in
the first term on the right
hand side of Equation 4.10
in the CFX-Solver Modeling
Guide.
A variable based on the
distance from the wall to
the first node and the wall
shear stress. For details,
see Solver Yplus and Yplus
in the CFX-Solver Modeling
Guide.
A deprecated internal
variable. For details, see
Solver Yplus and Yplus in
the CFX-Solver Modeling
Guide.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
List of Field Variables
16.2.3. Variables Relevant for Buoyant Flow
The following table contains a list of variables (with both long and short variable names) that can be
used when working with buoyant flows. For an explanation of the column headings, see List of Field
Variables (p. 263).
Long
Variable
Name
Short
Variable
Name
Units
Availability
Definition
Thermal
Expansivity
beta
[K^ -1]
2
For details, see Buoyancy
in the CFX-Solver Modeling
Guide.
C
16.2.4. Variables Relevant for Compressible Flow
The following table contains a list of variables (with both long and short variable names) that can be
used when working with compressible flows.
Long
Variable
Name
Short
Variable
Name
Units
Availability
Isobaric
Compressibility
compisoP
[K^-1]
2
Isothermal
Compressibility
compisoT
Mach
Number
Mach
C, M, R
[m s^2 kg^-1]
2
C, M, R
[]
1
A, C, M,
R, TS
Shock
Indicator
shock
indicator
[]
2
A, C, M,
R, TS
Isentropic
Compressibility
Definition
compisoS
[m s^2 kg^-1]
2
C, M, R
Defines the rate of change
of the system volume with
pressure.
For details, see List of
Symbols in the CFX-Solver
Theory Guide.
The variable takes a value
of 0 away from a shock
and a value of 1 in the
vicinity of a shock.
The extent to which a
material reduces its volume
when it is subjected to
compressive stresses at a
constant value of entropy.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
271
Variables in ANSYS CFX
16.2.5. Variables Relevant for Particle Tracking
The following table contains a list of variables (with both long and short variable names) that can be
used when working with particle tracking.
Long
Variable
Name
Short
Variable
Name
Units
User
Level
Definition
Latent
Heat
lheat
[]
2
User-specified latent heat
for phase pairs involving a
particle phase.
C, R, M
Particle
Momentum
Source
ptmomsrc
Particle
Diameter
particle
diameter
[]
2
A, C, M,
P, R
[]
3
Momentum source from
particle phase to
continuous phase.
Diameter of a particle
phase.
A, C, M,
R
16.2.6.Variables Relevant for Calculations with a Rotating Frame of Reference
The following table contains a list of variables (with both long and short variable names) that can be
used when working with a rotating frame of reference. For an explanation of the column headings, see
List of Field Variables (p. 263).
Long
Variable
Name
Short
Variable
Name
Units
Availability
Definition
Total
Pressure
in Stn
Frame
ptotstn
[kg m^-1 s^-2]
2
The velocity in the rotating
frame of reference is
defined as:
Total
Temperature
in Stn
Frame
Ttotstn
Total
Enthalpy
in Stn
Frame
htotstn
Mach
Number
in Stn
Frame
Machstn
Velocity
in Stn
Frame
velstn
272
A, C, M,
P, R, TS
[K]
2
A, C, DT,
M, P, R,
TS
[kg m^2 s^-2]
2
A, C, M,
R, TS
[]
1
where is the angular
velocity, is the local
radius vector, and
is
velocity in the stationary
frame of reference. For
details, see Rotating Frame
Quantities in the CFX-Solver
Theory Guide.
A, C, M,
R, TS
[m s^-1]
1
A, C, M,
R, TS
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
List of Field Variables
16.2.7. Variables Relevant for Parallel Calculations
The following table contains a list of variables (with both long and short variable names) that can be
used when working with parallel calculations. For an explanation of the column headings, see List of
Field Variables (p. 263).
Long
Variable
Name
Short
Variable
Name
Real
Partition
Number
Units
Availability
Definition
[]
2
The partition that the node
was in for the parallel run.
C, M, R
16.2.8. Variables Relevant for Multicomponent Calculations
The following table contains a list of variables (with both long and short variable names) that can be
used when working with multicomponent calculations. For an explanation of the column headings, see
List of Field Variables (p. 263).
Long
Variable
Name
Short
Variable
Name
Units
Availability Definition
Mass
Fraction
mf
[]
1
The fraction of a component in
a multicomponent fluid by mass.
A, C,
M, P,
R, TS
Mass
Concentration
mconc
[kg
m^-3]
2
The concentration of a
component.
A, C,
M, P,
R, TS
16.2.9. Variables Relevant for Multiphase Calculations
The following table contains a list of variables (with both long and short variable names) that can be
used when working with multiphase calculations. For an explanation of the column headings, see List
of Field Variables (p. 263).
Long
Variable
Name
Short
Variable
Name
Units
Availability Definition
Interfacial
Area
Density
area
density
[m^-1]
3
Interphase
Mass
Transfer
Rate
ipmt
rate
C
[]
3
Interface area per unit volume
for Eulerian multiphase fluid
pairs.
Interface mass transfer rate for
Eulerian multiphase fluid pairs.
C
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
273
Variables in ANSYS CFX
Long
Variable
Name
Short
Variable
Name
Units
Availability Definition
Mean
Particle
Diameter
mean
particle
diameter
[m]
3
Volume
Fraction
vf
[]
A, C,
M
1
Mean particle diameter for an
Eulerian dispersed phase
(including Polydispersed Fluids).
For details, see Volume Fraction
in the CFX-Solver Modeling Guide.
A, C,
M, P,
R, TS
Conservative
Volume
Fraction
vfc
[]
Drift
Velocity
drift
velocity
2
For details, see Volume Fraction
in the CFX-Solver Modeling Guide.
A, C,
M, R,
TS
[]
2
C, M,
R, TS
Slip
Reynolds
Number
slip
Re
[]
Slip
Velocity
slipvel
3
Velocity of an algebraic slip
component relative to the
mixture.
Reynolds number for Eulerian
multiphase fluid pairs.
C
[]
1
C, M,
R, TS
Surface
Tension
Coefficient
surface
tension
coefficient
[N
m^-1]
Unclipped
Interfacial Area
Density
unclipped
area
density
[m^-1]
Superficial
Velocity
volflx
[m
s^-1]
2
Velocity of an algebraic slip
component relative to the
continuous component.
Surface tension coefficient
between fluids in a fluid pair.
C
3
C
1
Similar to area density, but
values are not clipped to be
non-zero.
The Fluid.Volume Fraction
multiplied by the Fluid.Velocity.
A, C,
M, R,
TS
16.2.10. Variables Relevant for Radiation Calculations
The following table contains a list of variables (with both long and short variable names) that can be
used when working with radiation calculations. For an explanation of the column headings, see List of
Field Variables (p. 263).
274
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
List of Field Variables
A B in the Type column indicates that the variable contains only non-zero values on the boundary of
the model.
Long
Variable
Name
Short
Variable
Name
Units
Availability Definition
Wall
Radiative
Heat
Flux
Qrad
[W
m^-2]
2,B
Wall
Heat
Flux
Qwall
Wall
Irradiation
Flux
irrad
Radiation
Intensity
radint
DT, R,
TS
[W
m^-2]
2,B
C, DT,
R, TS
[W
m^-2]
2,B
C, DT,
R, TS
[W
m^-2
sr^-1]
RA, R,
A, M,
C, P,
TS
Wall Radiative Heat Flux represents
the net radiative energy flux leaving
the boundary. It is computed as the
difference between the radiative
emission and the incoming radiative
flux (Wall Irradiation Flux).
Wall Heat Flux is sum of the Wall
Radiative Heat Flux and the Wall
Convective Heat Flux. For an
adiabatic wall, the sum should be
zero.
Wall Irradiation Flux represents the
incoming radiative flux. It is
computed as the solid angle integral
of the incoming Radiative Intensity
over a hemisphere on the boundary.
For simulations using the multiband
model, the Wall Irradiation Flux for
each spectral band is also available
for postprocessing.
Radiation Intensity represents the
radiative energy flow (in units of
energy per time) per unit solid angle
(solid angle of the outgoing or
incoming radiation, measured in
steradians) and per unit area (area
of a surface that is normal to the ray
direction).
Note
This quantity should not
be used for quantitative
calculations when
computed using
surface-to-surface models,
since it has been
agglomerated and it
represents an average
value over the whole
domain.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
275
Variables in ANSYS CFX
Long
Variable
Name
Short
Variable
Name
Units
Availability Definition
Wall
Absorbed
Radiation
Flux
sabsor
[W
m^-2]
2,B
Incident
Radiation
radinc
DT, R,
TS
[kg
s^-3]
1
C, DT,
M, R,
TS
Absorption
Coefficient
absorp
[m^-1]
1
C, M,
R, TS
Scattering
Coefficient
scatter
[m^-1]
Wall Absorbed Radiation Flux
represents the absorbed heat flux
due to radiation, and is computed
as Wall Radiative Heat Flux minus
reflection and emission.
The integral of Radiation In
tensity over a full sphere of unit
radius. For isotropic radiation, it is a
factor of
greater than the Radi
ation Intensity.
For details, see Table 16.2: Common CEL
Field Variables and Predefined
Expressions (p. 278)
1
C, M,
R, TS
Refractive
Index
refrac
[
]
1
C, R,
TS
Radiative
Emission
rademis
[kg
s^-3]
1
RA
Extinction
Coefficient
extinct
[m^-1]
1
C
Emissivity
emis
[
]
1
C
16.2.11. Variables for Total Enthalpies, Temperatures, and Pressures
The following table lists the names of the various total enthalpies, temperatures, and pressures when
visualizing results in CFD-Post or for use in CEL expressions. For an explanation of the column headings,
see List of Field Variables (p. 263).
Long
Variable
Name
Short
Variable
Name
Units
Availability Definition
Total
Enthalpy
htot
[m^2
s^-2]
A, C,
M, R,
TS
276
For details, see Transport
Equations in the
CFX-Solver Theory Guide.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
List of Field Variables
Long
Variable
Name
Short
Variable
Name
Units
Availability Definition
Rothalpy
rothalpy
[m^2
s^-2]
A, C,
M, R,
TS
Total
Enthalpy in
Stn Frame
htotstn
[m^2
s^-2]
A, C,
M, R,
TS
Total
Temperature
in Rel
Frame
Ttotrel
[K]
A, C,
DT,
M, P,
R, TS
Total
Temperature
Ttot
[K]
A, C,
DT,
M, P,
R, TS
Total
Temperature
in Stn
Frame
Ttotstn
[K]
A, C,
DT,
M, P,
R, TS
Total
Pressure in
Rel Frame
ptotrel
[kg m^-1 s^-2] A, C,
M, P,
R, TS
Total
Pressure
ptot
[kg m^-1 s^-2] A, C,
M, P,
R, TS
Total
Pressure in
Stn Frame
ptotstn
[kg m^-1 s^-2] A, C,
M, P,
R, TS
16.2.12. Variables and Predefined Expressions Available in CEL Expressions
The following is a table of the more common variables and predefined expressions that are available
for use with CEL when defining expressions. To view a complete list, open the Expressions workspace.
For an explanation of the column headings, see List of Field Variables (p. 263).
Many variables and expressions have a long and a short form (for example, Pressure or p).
Additional Variables and expressions are available in CFD-Post. For details, see CFX Expression Language
(CEL) in CFD-Post in the CFD-Post User's Guide.
Table 16.1: Common CEL Single-Value Variables and Predefined Expressions
Long Variable
Name
Short
Variable
Name
Units
Availability
Definition
Accumulated
Coupling
Step
acplgstep
[]
2
These single-value variables
enable access to timestep,
timestep interval, and
C
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
277
Variables in ANSYS CFX
Long Variable
Name
Short
Variable
Name
Units
Availability
Definition
Accumulated
Iteration
Number
aitern
[]
2
Accumulated
Time Step
atstep
iteration number in CEL
expressions. They may be
useful in setting parameters
such as the Physical
Timescale via CEL
expressions. For details, see
Timestep, Timestep Interval,
and Iteration Number
Variables (p. 288).
C
[]
2
C
Current
Iteration
Number
citern
Current
Stagger
Iteration
cstagger
Current
Time Step
ctstep
[]
2
C
[]
2
C
[]
2
C
Sequence
Step
sstep
[]
2
C
Time Step
Size
dtstep
[s]
2
C
Time
t
[s]
2
C
Note
Variables with names shown in bold text in the tables that follow are not output to CFDPost. However, some of these variables can be output to CFD-Post by selecting them from
the Extra Output Variables List on the Results tab of the Solver > Output Control details
view in CFX-Pre.
Table 16.2: Common CEL Field Variables and Predefined Expressions
Long Variable
Name
Short
Variable
Name
Units
Availability
Definition
Axial
Distance
aaxis
[m]
2
Axial spatial location
measured along the
locally-defined axis
from the origin of the
latter. When the
locally-defined axis
happens to be the Z
axis, z and aaxis are
identical.
C
278
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
List of Field Variables
Long Variable
Name
Short
Variable
Name
Units
Availability
Definition
Absorption
Coefficient
absorp
[m^-1]
1
The property of a
medium that describes
the amount of
absorption of thermal
radiation per unit path
length within the
medium. It can be
interpreted as the
inverse of the mean
free path that a
photon will travel
before being absorbed
(if the absorption
coefficient does not
vary along the path).
C, M, R,
TS
Boundary
Distance
bnd
distance
[m]
2
A, C, M,
R, TS
Boundary
Scale
bnd
scale
[m^-2]
3
C, M, R,
TS
Contact
Area Fraction
af
[]
[AV name]
[AV
name]
Thermal
Expansivity
beta
3
M
Additional Variable
name
[K^-1]
2
C
Effective
Density
deneff
[kg m^-3]
3
A, C, M,
R, TS
Density
density
[kg m^-3]
2
A, C, M,
P, R, TS
Turbulence
Eddy
Dissipation
ed
[m^2 s^-3]
Eddy
Viscosity
eddy
viscosity
1
A, C, M,
P, R, TS
[kg m^-1
s^-1]
1
A, C, M,
P, R, TS
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
279
Variables in ANSYS CFX
Long Variable
Name
Short
Variable
Name
Units
Availability
Definition
Emissivity
emis
[]
1
A characteristic of a
surface that describes
the fraction of emitted
radiation with respect
to the blackbody
emission at the same
temperature.
C
Extinction
Coefficient
extinct
Initial
Cartesian
Coordinates
initcartcrd
Turbulence
Kinetic
Energy
ke
Mach
Number
Mach
[m^-1]
1
C
[m]
2
C
[m^2 s^-2]
The property of a
medium that describes
the amount of
absorption and
scattering of thermal
radiation per unit path
length for propagation
in the medium.
The position of each
node as it was at the
start of the simulation
(that is, the current
position with Total
Mesh Displacement
subtracted). The
individual components
are referred to as
"Initial X", "Initial Y"
and "Initial Z".
1
A, C, M,
P, R, TS
[]
1
A, C, M,
R, TS
Mach
Number in
Stn Frame
Machstn
Mass
Concentration
mconc
[]
1
Mach Number in
Stationary Frame
A, C, M,
R, TS
[m^-3 kg]
2
Mass concentration of
a component
A, C, M,
P, R, TS
Mass
Fraction
mf
[]
1
A, C, M,
P, R, TS
280
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
List of Field Variables
Long Variable
Name
Short
Variable
Name
Units
Availability
Conservative Mass
Fraction
mfc
[]
2
Mean
Particle
Diameter
mean
particle
diameter
[m]
Mesh
Displacement
meshdisp
[m]
Definition
A, C, M,
R, TS
3
C, P
3
C, M, R,
TS
Mesh
Expansion
Factor
mesh
exp fact
Mesh
Initialisation
Time
meshinittime
Mixture
Fraction
mixfrc
[]
2
C, M, R,
TS
[s]
2
C
[]
1
The displacement
relative to the previous
mesh
Ratio of largest to
smallest sector
volumes for each
control volume.
Simulation time at
which the mesh was
last re-initialized (most
often due to
interpolation that
occurs as part of
remeshing)
Mixture Fraction Mean
A, C, M,
R, TS
Mixture
Model
Length
Scale
mixture
length
scale
[m]
Mixture
Fraction
Variance
mixvar
[]
Molar
Concentration
molconc
3
M
1
A, C, M,
R, TS
[m^-3 mol]
2
A, C, M,
P, R, TS
Molar
Fraction
molf
[]
2
A, C, M,
P, R, TS
Molar
Mass
mw
[kg
mol^-1]
3
C, P
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
281
Variables in ANSYS CFX
Long Variable
Name
Short
Variable
Name
Units
Availability
Definition
Orthogonality
Angle
orthangle
[rad]
2
A measure of the
average mesh
orthogonality angle
C, M, R,
TS
Orthogonality
Angle
Minimum
orthanglemin
Orthogonality
Factor
orthfact
[rad]
2
C, M, R,
TS
2
C, M, R,
TS
Orthogonality
Factor
Minimum
orthfactmin
Pressure
p
2
C, M, R,
TS
[kg m^-1 s^-2]
A measure of the worst
mesh orthogonality
angle
A non-dimensional
measure of the
average mesh
orthogonality
A measure of the worst
mesh orthogonality
angle
1
A, C, M,
P, R, TS
Absolute
Pressure
pabs
[kg m^-1 s^-2]
2
A, C, M,
R, TS
Reference
Pressure
pref
[kg m^-1 s^-2]
2
C
Distance
from local
Z axis
r
[m]
Radius
raxis
[m]
2
Radial spatial location.
C
. For details,
see CEL Variables r and
theta (p. 287).
2
Radial spatial location
measured normal to
the locally-defined axis.
When the
C
282
The Reference
Pressure is the
absolute pressure
datum from which all
other pressure values
are taken. All relative
pressure specifications
in CFX are relative to
the Reference
Pressure. For details,
see Setting a Reference
Pressure in the
CFX-Solver Modeling
Guide.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
List of Field Variables
Long Variable
Name
Short
Variable
Name
Units
Availability
Definition
locally-defined axis
happens to be the Z
axis, r and raxis are
identical.
Radiative
Emission
rademis
[kg s^-3]
1
RA
Incident
Radiation
radinc
[kg s^-3]
1
C, DT, M,
R, TS
Radiation
Intensity
radint
[kg s^-3]
1
A, C, M,
P, R, TS
Refractive
Index
refrac
[]
1
C, R, TS
Non dimensional radius
rNoDim
[]
2
C
Blackbody radiative
emission is defined as
* Refractive Index^2
* Temperature^4,
where represents the
Stefan-Boltzmann
constant.
This is a volumetric
quantity and has no
relevance at
boundaries. For
relevant radiation
quantities at
boundaries, see the
definitions for Wall
Radiative Heat
Flux and Wall Ir
radiation Flux in
Variables Relevant for
Radiation
Calculations (p. 274).
This is written to the
results file for all
radiation models. For
Monte Carlo
simulations, the Radi
ation Intens
ity.Normalized
Std Deviation is
also written. This
variable represents the
statistical deviation
with respect to the
mean for the Monte
Carlo model.
A non-dimensional
parameter defined as
the ratio of the speed
of light in a vacuum to
that in a material.
Non-dimensional
radius (available only
when a rotating
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
283
Variables in ANSYS CFX
Long Variable
Name
Short
Variable
Name
Units
Availability
Definition
domain exists). For
details, see CEL
Variable
rNoDim (p. 288).
Reynolds
Stress
rs
rs
rs
rs
rs
rs
uu,
vv,
ww,
uv,
uw,
vw
Statistical
Reynolds
Stress
rsstat
rsstat
rsstat
rsstat
rsstat
rsstat
uu,
vv,
ww,
uv,
uw,
vw
Scattering
Coefficient
scatter
[m^2 s^-2]
2
A, C, M,
P, R, TS
[m^2 s^-2]
3
M, R
[m^-1]
1
C, M, R,
TS
Soot Mass
Fraction
sootmf
The six Reynolds Stress
components
[]
The six Statistical
Reynolds Stress
components
The property of a
medium that describes
the amount of
scattering of thermal
radiation per unit path
length for propagation
in the medium. It can
be interpreted as the
inverse of the mean
free path that a
photon will travel
before undergoing
scattering (if the
scattering coefficient
does not vary along
the path).
1
A, C, M,
R, TS
Soot
Nuclei
Specific
Concentration
sootncl
Specific
Volume
specvol
[m^-3]
1
A, C, M,
R, TS
[m^3
kg^-1]
3
A, C, M,
R, TS
Local
Speed of
Sound
284
speedofsound
[m s^-1]
2
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
List of Field Variables
Long Variable
Name
Short
Variable
Name
Units
Availability
Definition
C, M, R,
TS
Subdomain
subdomain
[]
2
C
inside()
@<Locations>
inside()
@<Locations>
Theta
taxis
inside variable (1.0 in
subdomain, 0.0
elsewhere). For details,
see CEL Variable
"subdomain" and CEL
Function
"inside" (p. 288).
[rad]
2
C
Turbulence
Eddy
Frequency
tef
Angle
around
local Z axis
theta
Total
Mesh
Displacement
meshdisptot
Velocity u
u
Velocity v
v
Velocity w
w
Subdomain variable
(1.0 in subdomain, 0.0
elsewhere). For details,
see CEL Variable
"subdomain" and CEL
Function
"inside" (p. 288).
[s^-1]
taxis is the angular
spatial location
measured around the
locally-defined axis,
when the latter is
defined by the
Coordinate Axis option.
When the locally
defined axis is the
z(/x/y)-axis, taxis is
measured from the
x(/y/z)-axis, positive
direction as per
right-hand rule.
1
A, C, M,
P, R, TS
[rad]
2
C
[m]
1
C, DT, M,
R, TS
[m s^-1]
1
Angle, arctan(y/x). For
details, see CEL
Variables r and
theta (p. 287).
The total displacement
relative to the initial
mesh
Velocity in the x, y, and
z coordinate directions
A, C, M,
P, R, TS
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
285
Variables in ANSYS CFX
Long Variable
Name
Short
Variable
Name
Units
Availability
Definition
Velocity in
Stn Frame
u
velstn u
[m s^-1]
1
Velocity in Stationary
Frame in the x, y, and
z coordinate directions
Velocity in
Stn Frame
v
velstn w
velstn v
A, C, M,
R, TS
Velocity in
Stn Frame
w
Volume
Fraction
vf
[]
1
A, C, M,
P, R, TS
Conservative
Volume
Fraction
vfc
[]
Kinematic
Viscosity
visckin
2
A, C, M,
R, TS
[m^2 s^-1]
The variable <flu
id>.Conservative
Volume Fraction
should not usually be
used for
postprocessing.
2
A, C, M,
P, R, TS
Wall
Distance
wall
distance
[m]
2
A, C, M,
P, R, TS
Wall
Power
Density
wall
powerdens
[W m^-2]
2
C, DT, R,
TS
Power done by a
moving wall onto the
fluid per unit area
This variable is 0 at
stationary walls.
Wall Work
Density
wall
workdens
[J m^-2]
2
C, DT, R,
TS
Work done by a
moving wall onto the
fluid per unit area
This variable is 0 at
stationary walls.
Wall Scale
wall
scale
[m^2]
3
M, R, TS
286
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
List of Field Variables
16.2.12.1. System Variable Prefixes
In order to distinguish system variables of the different components and fluids in your CFX model,
prefixes are used. For example, if carbon dioxide is a material used in the fluid air, then some of the
system variables that you might expect to see are:
• air.density - the density of air
• air.viscosity - the viscosity of air
• air.carbondioxide.mf - the mass fraction of carbon dioxide in air
• air | water.surface tension coefficient – the surface tension coefficient between air and
water
• air | water.area density – the interfacial area density between air and water.
In a single phase simulation the fluid prefix may be omitted.
For multiphase cases, a fluid prefix indicates either a specific fluid, or a specific fluid pair. The absence
of a prefix indicates a bulk or fluid independent variable, such as pressure.
For porous solids, those variables that exist in the solid are prefixed by the name of the solid phase.
16.2.12.2. CEL Variables r and theta
r is defined as the normal distance from the third axis with respect to the reference coordinate frame.
theta is defined as the angular rotation about the third axis with respect to the reference coordinate
frame. For details, see Coordinate Frames in the CFX-Solver Modeling Guide.
The variables Radius and theta are available only when the rotational axis has been defined. The
rotational axis can either be defined in the results file or in CFD-Post through the Initialization panel
in the Turbo workspace.
Note
theta is expressed in radians and will have values between
and .
r and theta are particularly useful for describing radial distributions, for instance the velocity profile
at the inlet to a pipe.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
287
Variables in ANSYS CFX
Figure 16.1: r and theta with Respect to the Reference Coordinate Frame
16.2.12.3. CEL Variable rNoDim
rNoDim is a dimensionless system variable that can be useful for rotating machinery applications. It is
a ratio of radii, defined to be zero at the minimum radius and unity at the maximum radius, so that in
general:
where R is the radius of any point in the domain from the axis of rotation. rNoDim is only available for
domains defined with a rotating frame of reference.
16.2.12.4. CEL Variable "subdomain" and CEL Function "inside"
subdomain is essentially a step function variable, defined to be unity within a subdomain and zero
elsewhere. This is useful for describing different initial values or fluid properties in different regions of
the domain. It works in all subdomains but cannot be applied to specific subdomains (for example, an
expression for temperature in a subdomain could be 373*subdomain [K]).
The inside CEL function can be used in a similar way to the subdomain variable, but allows a specific 2D or 3D location to be given. For example, 273 [K] * inside()@Subdomain 1 has a value
of 273 [K] at points in Subdomain 1 and 0 [K] elsewhere. Furthermore, the location can be any 2D or
3D named sub-region of the physical location on which the expression is evaluated. The location can
also be an immersed solid domain.
16.2.12.5. Timestep, Timestep Interval, and Iteration Number Variables
These variables enable access to timestep, timestep interval, and iteration number in CEL expressions.
They may be useful in setting parameters such as the Physical Timescale via CEL expressions.
16.2.12.5.1. Steady-State Runs
In steady-state runs, only Accumulated Iteration Number (or, equivalently Accumulated Time Step) and
Current Iteration Number (or, equivalently Current Time Step) are of use. Current Iteration Number gives
the outer iteration number of the current run. The outer iteration number begins at 1 for each run, irrespective of whether it is a restarted run. Accumulated Iteration Number gives the accumulated outer
iteration number, which accumulates across a restarted run.
288
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
List of Field Variables
16.2.12.5.2. Transient Runs
In transient runs, Accumulated Time Step and Current Time Step are used for the accumulated and
current timestep numbers of the outer timestep loop. Current Iteration Number gives the current
coefficient loop number within the current timestep. Thus, Current Iteration Number will cycle between
1 and n for each timestep during a transient run, where n is the number of coefficient loops. Accumulated
Iteration Number is equivalent to Current Iteration Number for transient runs.
16.2.12.5.3. ANSYS Multi-field Runs
For ANSYS Multi-field runs, Current Stagger Iteration and Accumulated Coupling Step are also available.
Current Stagger Iteration gives the current stagger iteration, which will cycle between 1 and n for each
coupling step of the run. Accumulated Coupling Step gives the accumulated coupling step. This gives
the multi-field timestep number or "coupling step" number for the run, and accumulates across a restarted
run. For transient ANSYS Multi-field runs where the CFX timestep is the same as the multi-field timestep,
Accumulated Coupling Step is equivalent to Accumulated Time Step.
16.2.12.5.4. Timestep Variables in CFD-Post
In CFD-Post, Sequence Step (sstep) is the 'global' sequence timestep. It is equivalent to the Step value
in Timestep Selector in the CFD-Post User's Guide.
Accumulated Time Step (atstep) and Current Time Step (ctstep) are available for both steady-state
and transient runs, with Current Time Step being set to the same value as Accumulated Time Step.
Accumulated Iteration Number (aitern), Current Iteration Number (citern), Accumulated Coupling
Step (acplgstep), and Current Stagger Iteration (cstagger) are not available in CFD-Post.
If multiple cases are loaded, the values obtained from evaluating these timestep-related variables relate
to the last loaded case.
16.2.12.6. Expression Names
Your CEL expression name can be any name that does not conflict with the name of a CFX system
variable, mathematical function, or an existing CEL expression. The RULES and VARIABLES files provide
information on valid options, variables, and dependencies. Both files are located in <CFXROOT>/etc/
and can be viewed in any text editor.
16.2.12.7. Scalar Expressions
A scalar expression is a real valued expression using predefined variables, user variables, and literal
constants (for example, 1.0). Note that literal constants have to be of the same dimension. Scalar expressions can include the operators + - * / and ^ and several of the mathematical functions found in
standard Fortran (for example, sin() and exp()).
An expression’s value is a real value and has specified dimensions (except where it is dimensionless but this is also a valid dimension setting).
For example, if t is time and L is a length then the result of L/t has the same dimensions as speed.
The + and - operators are only valid between expressions with the same dimensions and result in an
expression of those dimensions.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
289
Variables in ANSYS CFX
The * and / operators combine the dimensions of their operands in the usual fashion. X^I, where I is
an integer, results in an expression whose dimensions are those of X to the power I. The trigonometric
functions all work in terms of an angle in radians and a dimensionless ratio.
16.2.12.8. Expression Properties
There are three properties of expressions:
• An expression is a simple expression if the only operations are +, -, *, / and there are no functions used in
the expression.
• An expression is a constant expression if all the numbers in the expression are explicit (that is, they do not
depend on values from the solver).
• An expression is an integer expression if all the numbers in the expression are integers and the result of
each function or operation is an integer.
For example, (3+5)/2 is a simple, constant, integer expression. However, 2*(1/2) is not a constant integer
expression because the result of 1/2 is 0.5, not an integer. Also 3.*4 is not a constant integer expression
because 3 is not an integer. Moreover, 2^3 is not a simple, constant, integer expression because ^ is
not in the list (+, -, *, /).
Expressions are evaluated at run time and in single precision floating point arithmetic.
16.2.12.9. Available and Unavailable Variables
CFX System Variables and user-defined expressions will be available or unavailable depending on the
simulation you are performing and the expressions you want to create. In some circumstances, System
Variables are logically unavailable; for instance, time (t) is not available for steady-state simulations. In
others, the availability of a System Variable is not allowed for physical model reasons. For example,
density can be a function of pressure (p), temperature (T) and location (x, y, z), but no other system
variables.
Information on how to find dependencies for all parameters is available in the RULES and VARIABLES
files. Both files are located in <CFXROOT>/etc/ and can be viewed in any text editor.
The expression definition can depend on any system variable. If, however, that expression depends on
a system variable that is unavailable for a particular context, then that expression will also be unavailable.
16.3. Particle Variables Generated by the Solver
This section describes the following types of particle variables that you may have defined in CFX-Pre
or that are available for viewing in CFD-Post and exporting to other files. Many variables are relevant
only for specific physical models.
16.3.1. Particle Track Variables
16.3.2. Particle Field Variables
Some variables are defined only on the boundaries of the model. When using these variables in CFDPost, there are a limited number of useful things that you can do with these. For details, see BoundaryValue-Only Variables in the CFD-Post User's Guide.
The following information is given for particle variables described in this section:
• Long Variable Name: The name that you see in the user interface.
290
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Particle Variables Generated by the Solver
• Short Variable Name: The name that must be used in CEL expressions.
• Units: The default units for the variable. An empty entry [ ] indicates a dimensionless variable.
Note
The entries in the Units columns are SI but could as easily be any other system of units.
• Type (User Level, Boundary)
User Level: This number is useful when using the CFX Export facility. For details, see File Export
Utility in the CFX-Solver Manager User's Guide. Note that the CFX-Solver may sometimes override the
user-level setting depending on the physics of the problem. In these cases, the User Level may be
different from that shown in the table below.
Boundary (B): A B in this column indicates that the variable contains only non-zero values on the
boundary of the model. See Boundary-Value-Only Variables in the CFD-Post User's Guide for more
details.
This section does not cover the complete list of variables. For information on obtaining details on all
variables, see RULES and VARIABLES Files in the CFX-Solver Manager User's Guide.
16.3.1. Particle Track Variables
Particle track variables are particle variables that are defined directly on each track. These variables are
defined on the particle positions for which track information is written to the results file. Direct access
to the particle track variables outside of CFD-Post is possible only if the raw track file is kept after a
particle run.
You can do the following with particle track variables:
• Export them from particle tracks in CFD-Post
• Use them to color particle tracks in CFD-Post
• Use them in particle histograms
• Use them as input to Particle User Fortran
Particle track variables are not available for use in CEL expressions and general User Fortran. In addition,
they cannot be monitored during a simulation.
The following table lists particle track variables that are available in general, including in CFD-Post:
Long Variable
Name
Short
Variable
Name
Units
Description
Availability
<Particle
Type>.Mean Particle
Diameter
mean
particle
diameter
[m]
Particle diameter
3
<Particle
Type>.<Particle
PR
[-]
Note: Only available for
multi-component particles.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
291
Variables in ANSYS CFX
Long Variable
Name
Short
Variable
Name
Units
Component>.Mass
Fraction
Description
Availability
Fraction of mass of a particular
particle component
<Particle
Type>.Particle
Number Rate
particle
number
rate
[s^-1]
<Particle
Type>.Particle Time
pttime
[s]
Particle number rate
3
PR
Simulation time
2
PR
<Particle
Type>.Particle
Traveling Distance
ptdist
[m]
<Particle
Type>.Particle
Traveling Time
[s]
<Particle
Type>.Particle Weber
Number
[-]
Distance along the particle track
measured from the injection
point
2
Time measured from the time of
injection of the particle. For
steady-state simulations only, this
time is identical to <Particle
Type>.Particle Time.
2
PR
PR
Note: Only available if a
secondary droplet breakup model
is active.
Particle Weber number along
track
where
<Particle
Type>.Temperature
T
[K]
Particle temperature
1
PR
<Particle Type>.Total
Particle Mass
ptmasst
[kg]
Particle total mass
2
PR
<Particle
Type>.Velocity
[m
s^-1]
Particle velocity
1
PR
<Particle
Type>.Velocity u
u
[m
s^-1]
Particle velocity components in
X, Y, and Z direction
v
292
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
1
Particle Variables Generated by the Solver
Long Variable
Name
Short
Variable
Name
<Particle
Type>.Velocity v
w
Units
Description
Availability
PR
<Particle
Type>.Velocity w
For Particle User Fortran, these additional track variables, which are not available in CFD-Post, can be
specified in the argument list for the user routine:
Long Variable Name
Short
Variable
Name
Units
Particle Eotvos Number
pteo
[]
Definition
Availability
2
PR
Particle Morton Number
ptmo
[]
2
PR
Particle Nusselt Number
ptnu
[]
2
PR
Particle Ohnesorge Number
pton
[]
2
PR
Particle Reynolds Number
ptre
[]
2
PR
Particle Slip Velocity
ptslipvel
[m
s^-1]
2
PR
Particle Position
ptpos
[m]
Cartesian coordinates of
current particle position
2
PR
Particle Impact Angle
a
a
particle
impact
angle
[radian]
3
PR
Note: The impact angle is measured from the wall.
The following particle variables are available only in particle histograms:
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
293
Variables in ANSYS CFX
Long Variable
Name
Short
Variable
Name
Units
Description
Availability
<Particle
Type>.Particle Mass
Flow Rate
[kg
s^-1]
Particle mass flow rate = Particle
Total Mass * Particle Number Rate
3
<Particle
Type>.Velocity
Magnitude
[m
s^-1]
PR
Particle Speed
2
PR
16.3.2. Particle Field Variables
Particle field variables are particle variables that are defined at the vertices of the fluid calculation. In
contrast to track variables, these variables can be used in the same way as “standard” Eulerian variables.
This means that particle field variables are available for use in CEL expressions and User Fortran, they
can be monitored during a simulation, and are available for general post-processing in CFD-Post. Additionally, particle field variables can be used in the same way as particle track variables as input to particle
User Fortran and for coloring tracks. When used for coloring tracks, the field variables have to be interpolated onto the tracks, and so this operation will be slower than coloring with a track variable.
The following particle variables are available as field variables:
16.3.2.1. Particle Sources into the Coupled Fluid Phase
For fully-coupled particle simulations involving energy, momentum and mass transfer to the fluid phase,
the following variables are written to the results file:
Long Variable Name
Short Variable Name
Units
Availability
Particle Energy Source
ptenysrc
[W m^-3]
2
A, C, M, P,
R
Particle Energy Source Coefficient
ptenysrcc
[W m^-3 K^-1] 2
A, C, M, P,
R
Particle Momentum Source
ptmomsrc
[kg m^-2 s^-2] 2
A, C, M, P,
R
Particle Momentum Source
Coefficient
ptmomsrcc
[kg m^-3 s^-1] 2
A, C, M, P,
R
Total Particle Mass Source
ptmassrctot
[kg s^-1 m^-3] 2
A, C, M, P,
R
Total Particle Mass Source Coefficient
294
ptmassrcctot
[kg s^-1 m^-3] 2
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Particle Variables Generated by the Solver
Long Variable Name
Short Variable Name
Units
Availability
A, C, M, P,
R
For multi-component mass transfer, the following Additional Variables are available a:
Particle Mass Source
ptmassrc
[kg s^-1 m^-3] 2
A, C, M, P,
R
Particle Mass Source Coefficient
ptmassrcc
[kg s^-1 m^-3] 2
A, C, M, P,
R
a
The variables for multi-component take the following form: <Particle Type>.<Particle Component>.<Variable Name>
Particle source terms are accumulated along the path of a particle through a control volume and stored
at the corresponding vertex. A smoothing procedure can be applied to the particle source terms, which
may help with convergence or grid independence. For details, see Particle Source Smoothing in the
CFX-Solver Modeling Guide.
16.3.2.2. Particle Radiation Variables
Long Variable Name
Short Variable
Name
Units
Availability
Particle Radiative Emission
ptremiss
[W m^-3]
2
A, C, M,
P, R
Particle Absorption Coefficient
ptabscoef
[m^-1]
2
A, C, M,
P, R
Particles can also interact with the radiation field and either emit or absorb radiation.
16.3.2.3. Particle Vertex Variables
By default, particle vertex variables are not written to the results file, except for the Averaged Volume
Fraction. The other vertex variables can be written to the results file if they are selected from the
Extra Output Variables List in the Output Control section of CFX-Pre or if they are used in a monitor
point, CEL expression or in (Particle) User Fortran.
The following particle variables are available:
Long Variable Name
Short Variable
Name
Units
Availability
Averaged Velocity
averaged vel
[m s^-1]
1
A, C, M,
P, PR, R
Averaged Volume Fraction
vfpt
[]
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
1
295
Variables in ANSYS CFX
Long Variable Name
Short Variable
Name
Units
Availability
A, C, M,
P, PR, R
Averaged Temperature
averaged
temperature
[K]
1
A, C, M,
P, PR, R
Averaged Mass Fraction
a
averaged mf
[]
1
A, C, M,
P, PR, R
Averaged Particle Time
averaged
pttime
[s]
2
A, C, M,
P, PR, R
Averaged Mean Particle Diameter (D43)
Averaged Arithmetic Mean Particle Diameter
(D10)
Averaged Surface Mean Particle Diameter
(D20)
Averaged Volume Mean Particle Diameter
(D30)
Averaged Sauter Mean Particle Diameter
(D32)
Averaged Mass Mean Particle Diameter (D43)
Averaged Particle Number Rate
averaged
mean particle
diameter
[m]
averaged
arithmetic
mean particle
diameter
[m]
averaged
surface mean
particle
diameter
[m]
averaged
volume mean
particle
diameter
[m]
averaged
sauter mean
particle
diameter
[m]
averaged mass
mean particle
diameter
[m]
averaged
particle
number rate
[s^-1]
2
A, C, M,
P, PR, R
2
A, C, M,
P, PR, R
2
A, C, M,
P, PR, R
2
A, C, M,
P, PR, R
2
A, C, M,
P, PR, R
2
A, C, M,
P, PR, R
2
A, C, M,
P, PR, R
For simulations with the particle wall film model activated, the following additional vertex variables
are available:
Averaged Volume Fraction Wall
296
vfptw
[]
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
1
Particle Variables Generated by the Solver
Long Variable Name
Short Variable
Name
Units
Availability
A, C, M,
P, PR, R
Averaged Film Temperature
averaged film
temperature
[K]
1
A, C, M,
P, PR, R
a
This variable takes the following form: <Particle Type>.<Particle Component>.<Variable Name>
The following are the formulae for particle vertex fields' size distributions:
Arithmetic Mean Diameter
Surface Mean Diameter
Volume Mean Diameter
Sauter Mean Diameter
Mass Mean Diameter
16.3.2.3.1. Variable Calculations
Particle vertex variables are calculated using the following averaging procedure:
(16.1)
With:
•
: Sum over all particles and time steps in a control volume
•
: Particle integration time step
•
: Particle number rate
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
297
Variables in ANSYS CFX
•
: Particle mass
•
: Particle quantity
Slightly different averaging procedures apply to particle temperature and particle mass fractions:
Averaged Particle Temperature
(16.2)
With:
Averaged Mass Fraction
•
•
: Particle specific heat capacity
: Particle temperature
(16.3)
With:
•
: Mass of species c in the particle
Due to the discrete nature of particles, vertex variables may show an unsmooth spatial distribution,
which may lead to robustness problems. To reduce possible problems a smoothing option is available.
For details, see Vertex Variable Smoothing in the CFX-Solver Modeling Guide.
16.3.2.4. Particle Boundary Vertex Variables
Particle-boundary vertex variables are particle variables that are defined on the vertices of domain
boundaries. They are normalized with the face area of the corresponding boundary control volume.
You can use these variables to color boundaries and to compute average or integrated values of the
corresponding particle quantities.
You cannot use these variables in CEL expressions or User Fortran, and you cannot monitor them during
a simulation.
Long Variable Name
Units
Availability
[kg m^-2 s^-1]
2
Available at inlet, outlet, openings and interfaces:
Mass Flow Density
B, R
Momentum Flow Density
[kg m^-1 s^-2]
2
B, R
Energy Flow Density
298
[kg s^-3]
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
2
Particle Variables Generated by the Solver
Long Variable Name
Units
Availability
B, R
Available at walls only:
Wall Stress
[kg m^-1 s^-2]
2
B, R
Wall Energy Flow Density
[kg s^-3]
2
B, R
Wall Mass Flow Density
[kg m^-2 s^-1]
2
B, R
Erosion Rate Density
[kg m^-2 s^-1]
2
B, R
Available in transient runs:
Time Integrated Mass Flow Density
[kg m^-2]
2
B, R
Time Integrated Momentum Flow Density
[kg m^-1 s^-1]
Time Integrated Energy Flow Density
[kg s^-2]
2
B, R
Time Integrated Wall Energy Flow Density
[kg s^-2]
2
B, R
Time Integrated Wall Mass Flow Density
[kg m^-2]
2
B, R
Time Integrated Erosion Rate Density
[kg m^-2]
2
B, R
16.3.2.5. Particle RMS Variables
For some applications, it may be necessary to not only provide the mean values of particle quantities,
but also their standard deviation in the form of particle RMS variables. Similar to particle vertex variables,
these variables are also defined at the vertices of the fluid calculation. Particle RMS variables are available
for use in CEL expressions and User Fortran; they can be monitored during a simulation, and are available
for general postprocessing in CFD-Post. Additionally, particle RMS variables can be used in the same
way as particle track variables as input to particle User Fortran and for coloring tracks.
By default, particle RMS variables are not written to the results file; unless, they have been explicitly
requested by you (selected from the Extra Output Variables List in the Output Control section of
CFX-Pre, usage in a CEL expression or in User Fortran) or if the stochastic particle collision model is used
in a simulation.
The following particle variables are available as field variables, particularly useful for simulations that
use the stochastic particle collision model:
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
299
Variables in ANSYS CFX
Long Variable Name
Short Variable
Name
Units
Availability
RMS Velocity
rms velocity
[m s^-1]
1
A, C, M, P,
PR, R
RMS Temperature
rms
temperature
[K]
1
A, C, M, P,
PR, R
RMS Mean Particle Diameter
RMS Particle Number Rate
rms mean
particle
diameter
[m]
rms particle
number rate
[s^-1]
3
A, C, M, P,
PR, R
3
A, C, M, P,
PR, R
16.3.2.5.1. Variable Calculations
Particle RMS variables are calculated using the following procedure:
(16.4)
With:
•
: Instantaneous particle quantity
•
: Average particle quantity
•
: Fluctuating particle quantity
•
: Average of square of particle quantity
•
: Square of average of particle quantity
A smoothing option, as available for particle vertex variables, is available for particle RMS variables. For
details, see Vertex Variable Smoothing in the CFX-Solver Modeling Guide.
16.4. Miscellaneous Variables
Variable names in bold are not output to CFD-Post.
In the Availability column:
• A number represents the user level (1 indicates that the variable appears in default lists, 2 and 3 indicate
that the variable appears in extended lists that you see when you click
)
• A indicates the variable is available for mesh adaption
300
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Miscellaneous Variables
• C indicates the variable is available in CEL
• DT indicates the variable is available for data transfer to ANSYS
• M indicates the variable is available for monitoring
• P indicates the variable is available for particle user routine argument lists
• PR indicates the variable is available for particle results
• R indicates the variable is available to be output to the results, transient results, and backup files
• TS indicates the variable is available for transient statistics
Long
Variable
Name
Short
Variable
Name
Units
Availability
Aspect Ratio
aspect ratio
[]
2
Definition
C, M, R, TS
Autoignition
autoignition
[]
1
A, C, M, R, TS
Boundary
Scale
bnd scale
[]
3
C, M, R, TS
Burnt
Absolute
Temperature
burnt Tabs
Burnt Density
burnt density
[K]
Similar to wall
scale, this
variable is used
for controlling
mesh stiffness
near boundaries
for moving
mesh problems.
2
A, C, M, R, TS
[kg
m^-3]
2
A, C, M, R, TS
Clipped
Pressure
pclip
[Pa]
1
M, R, TS
Conservative
Size Fraction
sfc
[]
Negative
absolute values
clipped for
cavitation
2
A, C, M, R, TS
Courant
Number
courant
[]
2
C, M, R, TS
Cumulative
Size Fraction
csf
[]
2
A, C, M, R, TS
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
301
Variables in ANSYS CFX
Long
Variable
Name
Short
Variable
Name
Current
Density
jcur
Units
Availability
Definition
1
C, M, R, TS
Dynamic Diffusivity
diffdyn
2
C, M, P, R, TS
Electric Field
elec
1
C, M, R, TS
Electric
Potential
epot
1
C, M, R, TS
Electrical
Conductivity
conelec
3
C, M, R, TS
Electrical
Permittivity
permelec
3
C, M, R, TS
Electromagnetic
Force Density
bfemag
3
R
Equivalence
Ratio
equivratio
[]
2
A, C, M, R, TS
External
Magnetic
Induction
bmagext
First Blending
Function for
BSL and SST
model
sstbf1
Second
Blending
Function for
SST model
sstbf2
Flame
Surface
Density
fsd
Specific
Flame
Surface
Density
spfsd
Frequency
freq
302
[]
1
M, R, TS
[]
External
magnetic
induction field
specified by the
user.
3
C, M, R, TS
[]
3
C, M, R, TS
[m^-1]
1
A, C, M, R, TS
2
A, C, M, R, TS
Combustion
with flame
surface density
models.
Combustion
with flame
surface density
models.
3
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Miscellaneous Variables
Long
Variable
Name
Short
Variable
Name
Units
Availability
Definition
C
Fuel Tracer
trfuel
[]
1
A, C, M, R, TS
Granular
Temperature
grantemp
[m^2
s^-2]
Residual
material model
or exhaust gas
recirculation
(EGR)
1
A, C, M, R, TS
Group I Index
groupi
[]
2
C
Group J Index
groupj
[]
2
C
Group I Diameter
diami
2
C
Group J Diameter
diamj
2
C
Group I
Mass
massi
2
C
Group J
Mass
massj
2
C
Group I
Lower Mass
massi lower
2
C
Group J
Lower Mass
massj lower
2
C
Group I Upper Mass
massi upper
2
C
Group J Upper Mass
massj upper
2
C
Ignition
Delay
Elapsed
Fraction
ignfrc
Ignition
Delay Time
tigndelay
[]
2
A, C, M, R, TS
[s]
2
A, C, M, R, TS
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
303
Variables in ANSYS CFX
Long
Variable
Name
Short
Variable
Name
Units
Availability
Particle
Integration
Timestep
particle
integration
timestep
[s]
3
Isentropic
Compressibility
compisoS
[m s^2 kg^-1]
Definition
P
2
C, M, R
Isentropic
Compression
Efficiency
icompeff
Isentropic
Expansion
Efficiency
iexpeff
Isentropic
Total
Enthalpy
htotisen
Isentropic
Static
Enthalpy
enthisen
Isobaric
Compressibility
compisoP
Isothermal
Compressibility
compisoT
LES Dynamic
Model
Coefficient
dynmc
Laminar
Burning
Velocity
velburnlam
Lighthill
Stress
lighthill stress
tensor
[]
2
C, M, R, TS
[]
2
C, M, R, TS
2
C, M, R, TS
2
C, M, R, TS
[K^-1]
2
C, M, R
[m s^2 kg^-1]
2
C, M, R
[]
1
A, C, M, P, R, TS
[m s^-1]
2
A, C, R, TS
2
A, C, M, R, TS
Magnetic
Induction
bmag
1
C, M, R, TS
Magnetic
Field
hmag
2
C, M, R, TS
Magnetic
Vector
Potential
bpot
Magnetic
Permeability
permmag
1
C, M, R, TS
3
C, M, R, TS
304
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Miscellaneous Variables
Long
Variable
Name
Short
Variable
Name
External
Magnetic
Induction
bmagext
Mass Flux
mfflux
Units
Availability
Definition
1
C, M, R, TS
2
R
Mesh
Diffusivity
diffmesh
[m^2
s^-1]
2
C, M, R, TS
Normal Area
normarea
[]
2
Normal area
vectors.
C
Total Force
Density
forcetden
3
DT
Total
Pressure in
Rel Frame
ptotrel
Turbulent
Burning
Velocity
velburnturb
Mesh Velocity
meshvel
2
A, C, M, P, R, TS
[m s^-1]
Based on
relative frame
total enthalpy.
2
A, C, R, TS
1
C, M, R, TS
Mixture
Fraction
Scalar
Dissipation
Rate
mixsclds
Molar
Reaction Rate
reacrate
[s^-1]
3
A, C, M, R, TS
2
C, R, TS
Nonclipped
Absolute
Pressure
pabsnc
Nonclipped
Density
densitync
3
A, C, M, R, TS
[kg
m^-3]
2
C
Normal Vector
normal
[]
Nonclipped
absolute
pressure for
cavitation
source. This is
written to the
.res file for all
cases that have
cavitation.
Nonclipped
density for
cavitation source
2
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
305
Variables in ANSYS CFX
Long
Variable
Name
Short
Variable
Name
Units
Availability
Definition
C
Orthogonality Factor
Minimum
orthfactmin
Orthogonality Factor
orthfact
[]
2
C, M, R, TS
[]
2
C, M, R, TS
Orthogonality Angle
Minimum
orthanglemin
Orthogonality
Angle
orthangle
2
C, M, R, TS
2
C, M, R, TS
Particle
Laplace
Number
ptla
Particle
Turbulent
Stokes
Number
ptstt
Polytropic
Compression
Efficiency
pcompeff
Polytropic
Expansion
Efficiency
pexpeff
Polytropic
Total
Enthalpy
htotpoly
Polytropic
Static
Enthalpy
enthpoly
Reaction
Progress
reacprog
[]
2
P
[]
2
P
[]
2
C, M, R, TS
[]
2
C, M, R, TS
2
C, M, R, TS
2
C, M, R, TS
[]
1
A, C, M, R, TS
Weighted
Reaction
Progress
wreacprog
Weighted
Reaction
Progress
Source
wreacprogsrc
306
[]
2
A, C, M, R, TS
3
A, C, R, TS
For premixed or
partially
premixed
combustion.
For premixed or
partially
premixed
combustion.
For premixed or
partially
premixed
combustion.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Miscellaneous Variables
Long
Variable
Name
Short
Variable
Name
Units
Availability
Definition
Residual
Products
Mass Fraction
mfresid
[]
1
Residual
material model
or exhaust gas
recirculation
(EGR)
Residual
Products
Molar
Fraction
molfresid
Restitution
Coefficient
restitution
coefficient
A, C, M, R, TS
[]
2
A, C, M, R, TS
[]
Residual
material model
or exhaust gas
recirculation
(EGR)
3
C, M, R, TS
Rotation
Velocity
rotvel
2
C, R, TS
Rotational
Energy
rotenergy
2
C, R, TS
Shear Velocity
ustar
2
C
Size Fraction
sf
[]
1
A, C, M, R, TS
Solid Bulk
Viscosity
solid bulk
viscosity
[kg m^-1 s^-1] 3
C, M, R, TS
Solid
Pressure
solid pressure
[Pa]
3
A, C, M, R, TS
Solid
Pressure
Gradient
solid pressure
gradient
Solid Shear
Viscosity
solid shear
viscosity
[]
3
C, M, R, TS
[kg m^-1 s^-1] 3
C, M, R, TS
Static
Entropy
entropy
3
A, C, M, P, R, TS
Temperature
Variance
Tvar
1
A, C, M, R, TS
Time This
Run
trun
2
C
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
307
Variables in ANSYS CFX
Long
Variable
Name
Short
Variable
Name
Total
Boundary
Displacement
bnddisptot
Total Density
dentot
Units
Availability
1
C, DT, M, R, TS
[kg m^-3]
2
A, C, M, R
Total Density
in Stn Frame
Definition
dentotstn
[kg m^-3]
Total Density is
the density
evaluated at the
Total
Temperature
and Total
Pressure.
2
A, C, M, R
Total Density
in Rel Frame
dentotrel
[kg
m^-3]
2
A, C, M, R
Total Force
forcet
3
DT
Unburnt
Absolute
Temperature
unburnt Tabs
Unburnt
Density
unburnt
density
[K]
2
A, C, M, R, TS
[kg m^-3]
2
A, C, M, R, TS
Unburnt
Thermal
Conductivity
unburnt cond
Unburnt
Specific Heat
Capacity at
Constant
Pressure
unburnt Cp
Volume
Porosity
volpor
[W m^-1 K^-1] 2
A, C, M, R, TS
[J kg^-1 K^-1]
2
A, C, M, R, TS
[]
2
C, M, R, TS
Volume of
Finite
Volumes
volcvol
Vorticity
vorticity
3
C, R, TS
2
A, C, M, R, TS
Vorticity in
Stn Frame
vortstn
Note that
Vorticity is the
same as
Velocity.Curl.
2
A, C, M, R, TS
308
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Miscellaneous Variables
Long
Variable
Name
Short
Variable
Name
Wall External
Heat Transfer
Coefficient
htco
Wall Adjacent
Temperature
tnw
Units
Availability
Definition
2
R, TS
[K]
2
C, DT, R, TS
Wall Distance
wall distance
[m]
2
A, C, M, P, R, TS
Wall External
Temperature
tnwo
[K]
2
DT, R, TS
Wall Film
Thickness
film thickness
[m]
User-specified
external wall
temperature for
heat transfer
coefficient
boundary
conditions.
2
C, R
Wall Heat
Transfer
Coefficient
htc
Wall Heat
Flow
QwallFlow
2
C, R, TS
3
C, DT, R, TS
Wall Normal
Velocity
nwallvel
2
C, R, TS
Wall Scale
wall scale
3
R, M, TS
Wavelength
in Vacuum
wavelo
3
C
Wavenumber
in Vacuum
waveno
3
C
Normalized
Droplet
Number
spdropn
Droplet
Number
spdrop
[m^-3]
2
C, M, R, TS
1
C, M, R, TS
Dynamic Bulk
Viscosity
dynamic bulk
viscosity
1
A, C, M, R, TS
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
309
Variables in ANSYS CFX
Long
Variable
Name
Short
Variable
Name
Units
Availability
Total MUSIG
Volume
Fraction
vft
[]
2
Smoothed
Volume
Fraction
vfs
Temperature
Superheating
Tsuperheat
Definition
A, C, M, R, TS
[]
2
A, C, M, R, TS
3
Temperature
above saturation
C
Temperature
Subcooling
Tsubcool
3
Temperature
below saturation
C
310
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 17: Power Syntax in ANSYS CFX
Programming constructs can be used within CCL for advanced usage. Rather than invent a new language,
CCL takes advantage of the full range of capabilities and resources from an existing programming language, Perl. Perl statements can be embedded in between lines of simple syntax, providing capabilities
such as loops, logic, and much, much more with any CCL input file.
A line of Power Syntax is identified in a CCL file by an exclamation mark (!) in the first column of a line.
In between Perl lines, simple syntax lines may refer to Perl variables and lists.
A wide range of additional functionality is made available to expert users with the use of Power Syntax
including:
• Loops
• Logic and control structures
• Lists and arrays
• Subroutines with argument handling (useful for defining commonly re-used plots and procedures)
• Basic I/O processing
• System functions
• Many other procedures (Object programming, World Wide Web access, simple embedded graphical user
interfaces).
Any of the above may be included in a CCL input file or CFD-Post session file.
Important
You should be wary when entering certain expressions because Power Syntax uses Perl
mathematical operators. For example, in CEL, is represented as 2^2, but in Perl, it would
be written 2**2. If you are unsure about the validity of an operator, you should check a Perl
reference guide.
There are many good reference books on Perl. Two examples are Learning Perl (ISBN 1-56592042-2) and Programming Perl (ISBN 1-56592-149-6) from the O’Reilly series.
This chapter describes:
17.1. Examples of Power Syntax
17.2. Predefined Power Syntax Subroutines
17.1. Examples of Power Syntax
The following are some examples in which the versatility of power syntax is demonstrated. They become
steadily more complex in the later examples.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
311
Power Syntax in ANSYS CFX
Some additional, more complex, examples of Power Syntax subroutines can be found by viewing the
session files used for the Macro Calculator. These are located in CFX/etc/. You can execute these
subroutines from the Command Editor dialog box the same as calling any other Power Syntax subroutine.
The required argument format is:
!cpPolar(<"BoundaryList">, <"SliceNormalAxis">,
<"SlicePosition">, <"PlotAxis">, <"InletLocation">,
<"ReferencePressure">)
!compressorPerform(<"InletLocation">, <"OutletLocation">,
<"BladeLocation">, <"MachineAxis">, <"RotationalSpeed">,
<"TipRadius">, <"NumBlades">, <"FluidGamma">)
These subroutines are loaded when CFD-Post is launched, so you do not need to execute the session
files before using the functions.
Additional information on these macro functions is available in Gas Compressor Performance Macro
and Cp Polar Plot Macro.
All arguments passed to subroutines should be enclosed in quotations, for example Plane 1 must be
passed as “Plane 1” and Eddy Viscosity should be entered as “Eddy Viscosity”. Any legal
CFX Command Language characters that are illegal in Perl need to be enclosed in quotation marks.
17.1.1. Example 1: Print the Value of the Pressure Drop Through a Pipe
!
!
!
!
$Pin = massFlowAve("Pressure","inlet");
$Pout = massFlowAve("Pressure","outlet");
$dp = $Pin-$Pout;
print "The pressure drop is $dp\n";
Note
Function-specific Perl subroutines do not allow phase-specific evaluations; that is, you can
get only bulk results (such as mass flow for all phases). A workaround is to use "evaluate"
subroutine, which evaluates any CEL expression.
For example instead of
! $val = massFlow("Inlet", "Water")
# Does NOT work
you need to use:
! ($val, $units) = evaluate( "Water.massFlow()\@Inlet");
312
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Examples of Power Syntax
17.1.2. Example 2: Using a for Loop
This example demonstrates using Power Syntax that wraps a for loop around some CCL Object
definitions to repetitively change the visibility on the outer boundaries.
# Make the outer boundaries gradually transparent in
# the specified number of steps.
!$numsteps = 10;
!for ($i=0; $i < $numsteps; $i++) {
! $trans = ($i+1)/$numsteps;
BOUNDARY:in
Visibility = 1
Transparency = $trans
END
BOUNDARY:out
Visibility = 1
Transparency = $trans
END
BOUNDARY:Default
Visibility = 1
Transparency = $trans
END
!}
The first line of Power Syntax simply defines a scalar variable called numsteps. Scalar variables (that
is, simple single-valued variables) begin with a $ symbol in Perl. The next line defines a for loop that
increments the variable i up to numsteps. Next, you determine the fraction you are along in the loop
and assign it to the variable trans. The object definitions then use trans to set their transparency
and then repeat. Note how Perl variables can be directly embedded into the object definitions. The final
line of Power Syntax (!}) closes the for loop.
Note
Function-specific Perl subroutines do not allow phase-specific evaluations; that is, you can
get only bulk results (such as mass flow for all phases). A workaround is to use "evaluate"
subroutine, which evaluates any CEL expression.
For example instead of
! $val = massFlow("Inlet", "Water")
# Does NOT work
you need to use:
! ($val, $units) = evaluate( "Water.massFlow()\@Inlet");
17.1.3. Example 3: Creating a Simple Subroutine
The following example defines a simple subroutine to make two planes at specified locations. The
subroutine will be used in the next example.
!sub makePlanes {
PLANE:plane1
Option = Point and Normal
Point = 0.09,0,-0.03
Normal = 1,0,0
Draw Lines = On
Line Color = 1,0,0
Color Mode = Variable
Color Variable = Pressure
Range = Local
END
PLANE:plane2
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
313
Power Syntax in ANSYS CFX
Option = Point and Normal
Point = 0.08,-0.038,-0.0474
Normal = 1,0,0
Draw Faces = Off
Draw Lines = On
Line Color = 0,1,0
END
!}
Although this subroutine is designed for use with the next example, you can execute it on its own by
typing !makePlanes(); in the Command Editor dialog box.
17.1.4. Example 4: Creating a Complex Quantitative Subroutine
This example is a complex quantitative subroutine that takes slices through the manifold geometry, as
shown below, compares the mass flow through the two sides of the initial branch, and computes the
pressure drop through to the four exit locations.
! sub manifoldCalcs{
# call the previously defined subroutine (Example 3) make the
# upstream and downstream cutting planes
! makePlanes();
#
# Bound the two planes so they each just cut one side of the branch.
PLANE:plane1
Plane Bound = Circular
Bound Radius = 0.025
END
PLANE:plane2
Plane Bound = Circular
Bound Radius = 0.025
END
# Calculate mass flow through each using the predefined
# 'evaluate' Power Syntax subroutine and output the results
! ($mass1, $mfunits) = evaluate( "massFlow()\@plane1" );
! ($mass2) = evaluate( "massFlow()\@plane2" );
! $sum = $mass1+$mass2;
! print "Mass flow through branch 1 = $mass1 [$mfunits]\n";
! print "Mass flow through branch 2 = $mass2 [$mfunits]\n";
! print "Total = $sum [$mfunits]\n";
# Now calculate pressure drops and mass flows through the exits
# calculate the average pressure at the inlet
!($Pin, $punits) = evaluate( "massFlowAve(Pressure)\@in1" );
314
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Predefined Power Syntax Subroutines
# Set-up an array that holds the approximate X location of each
# of the 4 exits. We then loop over the array to move the outlet
# plane and re-do the pressure drop calculation at each exit.
! @Xlocs = (0.15,0.25,0.35,0.45);
! $sum = 0;
! for ($i=0;$i<4;$i++) {
PLANE:outlet
Option = Point and Normal
Normal = 0,-1,-1
Point = $Xlocs[$i],-0.06,-0.2
Plane Bound = Circular
Bound Radius = 0.05
END
! ($Pout, $punits) = evaluate( "massFlowAve(Pressure)\@outlet" );
! ($massFl) = evaluate( "massFlow()\@outlet" );
! $sum += $massFl;
! $Dp = $Pin-$Pout;
! $ii = $i+1;
! print "At outlet \#$ii: Dp=$Dp [$punits], Mass Flow=$massFl [$mfunits]\n";
! } # end loop
! print "Total Mass Flow = $sum [$mfunits]\n";
!} # end subroutine
After processing these commands to define the subroutine, you can execute it, in the same way as any
other subroutine, by typing !manifoldCalcs(); in the Command Editor dialog box.
17.2. Predefined Power Syntax Subroutines
CFD-Post provides predefined subroutines that add Power Syntax functionality. You can view a list of
these subroutines by entering !showSubs(); in the Command Editor dialog box. The list is printed
to the console window. The list shows all currently loaded subroutines, so it will include any custom
subroutines that you have processed in the Command Editor dialog box.
These subroutines provide access to the quantitative functionality of CFD-Post. Most of these routines
provide results in a single return value. For example, if the Perl variable $verbose = 1, then the
result is also printed to the screen. Information on the calculations performed by the subroutines is
available. For details, see Function Selection.
The following sections describe these predefined subroutines:
• Power Syntax Subroutine Descriptions (p. 315)
• Power Syntax Usage (p. 316)
• Power Syntax Subroutines (p. 316)
17.2.1. Power Syntax Subroutine Descriptions
In the next section, each subroutine will appear in the following format:
Each of the subroutines contains an argument list (in brackets, separated by commas). If any argument
contains more than one word (for example, Plane 1), it must be within quotes. You should enclose
all arguments within quotes to avoid making possible syntax errors.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
315
Power Syntax in ANSYS CFX
Each subroutine is preceded by its return value(s). For example:
real, string evaluate("Expression", "Locator")
will return two values, a real number and a string.
The return values will always be in the solution units of the CFX-Solver results file, even if you have
changed the display units in the Edit menu. This means that if you have a plot of temperature in degrees
C on Plane 1, the area averaged value of temperature on Plane 1 returned by the areaAve
command will still be in degrees K.
17.2.2. Power Syntax Usage
All lines of power syntax must have an exclamation mark as the first character so that they are not
treated as CCL statements. The statements must also end with a semicolon.
Assuming you have a plane named Plane 1, the following example returns the area of this plane:
! $areaVal = area("Plane 1");
! print "The area of Plane 1 is $areaVal \n";
Some subroutines return more than one value. To store return values for a subroutine that returns two
variables (such as the evaluate function), you could use the following:
! ($value, $units) = evaluate('area()@Plane 1');
! print "The area of Plane 1 is $value in units of $units \n";
Note
In this case, if single quotes are not used around the expression, area()@Plane 1, when
calling the function, evaluate(), the @ symbol must be escaped (made literal) using the
following power syntax instead:
! ($value, $units) = evaluate("area()\@Plane 1");
! print "The area of Plane 1 is $value in units of $units \n";
This is used to avoid Perl treating the @ symbol as a special character. See evaluate(Expression) (p. 318) for details.
17.2.3. Power Syntax Subroutines
17.2.3.1. area(Location, Axis)
real area("Location", "Axis")
Returns the area of a 2D locator. For details, see area (p. 241).
17.2.3.2. areaAve(Variable, Location, Axis)
real areaAve("Variable", "Location", "Axis")
Returns the area-weighted average of the variable at a 2D locator. For details, see areaAve (p. 242).
17.2.3.3. areaInt(Variable, Location, Axis)
real areaInt("Variable", "Location", "Axis")
Returns the result of the variable integrated over the 2D location. For details, see areaInt (p. 243).
316
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Predefined Power Syntax Subroutines
17.2.3.4. ave(Variable, Location)
real ave("Variable", "Location")
Returns the arithmetic average of the variable at a location. For details, see ave (p. 244).
17.2.3.5. calcTurboVariables()
void calcTurboVariables()
Calculates all 'extra' turbo variables. (Works only in turbo mode.)
17.2.3.6. calculate(function,...)
real calculate(function,...)
Evaluates the named function with the supplied argument list, and returns the float result. The function
name is a required argument, which can be followed by a variable length list of arguments.
17.2.3.7. calculateUnits(function,...)
string,string calculateUnits(function,...)
Evaluates the named function with the supplied argument list, and returns the value and units.
17.2.3.8. collectTurboInfo()
This is an internal subroutine that is used only to initialize report templates.
17.2.3.9. comfortFactors()
This is an internal subroutine that is used only to initialize report templates.
For details, see Comfort Factors Macro.
17.2.3.10. compressorPerform(Location, Location, Location, Var, Args)
This is a special macro; for details, see Gas Compressor Performance Macro. For example:
compressorPerform("Inlet", "Outlet", "Blade", "X", 600, 0.03, 10, 1.2)
17.2.3.11. compressorPerformTurbo()
This is an internal subroutine that is used only to initialize report templates.
17.2.3.12. copyFile(FromPath, ToPath)
void copyFile("FromPath", "ToPath")
A utility function for copying files.
17.2.3.13. count(Location)
real count("Location")
Returns the number of nodes on the location. For details, see count (p. 245).
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
317
Power Syntax in ANSYS CFX
17.2.3.14. countTrue(Expression, Location)
real countTrue("Expression", "Location")
Returns the number of mesh nodes on the specified region that evaluate to “true”, where true means
greater than or equal to 0.5. "Expression" should contain one of the logical operators =, >, <, <=,
or >=. The countTrue function is valid for 1D, 2D, and 3D locations. For details, see countTrue (p. 246).
17.2.3.15. cpPolar(Location, Var, Arg, Var, Location, Arg)
This is a special macro; for details, see Cp Polar Plot Macro. For example:
cpPolar("Plane 1", "Y", 0.3, "X", "Inlet", 10000)
17.2.3.16. evaluate(Expression)
real,string evaluate("Expression")
Returns the value of the expression and the units. Only one expression can be evaluated each time the
subroutine is executed. The main advantage of using evaluate is that it takes any CEL expression.
This means that you do not have to learn any other quantitative power syntax routines described in
this section. Also, evaluate will return the result units in addition to the value.
An example is:
evaluate("areaAve(Velocity v)\@Location 1")
In this case, another subroutine is evaluated. The evaluate command takes an any expression as the
argument, or more precisely, any expression that resolves to a quantity. This means that you cannot
use:
"2*Pressure"
but you can use:
"2*minVal(Pressure)\@locator 1"
or
"100 [m]"
This is simply an alternative way of typing:
! $myVal = 2 * minVal("Pressure", "Location");
The reason that the @ is escaped calling evaluate() is to avoid Perl treating it as a special character.
17.2.3.17. evaluateInPreferred(Expression)
real,string evaluateInPreferred("Expression")
Returns the value of the expression in your preferred units. Preferred units are the units of the data that
CFD-Post uses when information is displayed to you and are the default units when you enter information
(as contrasted with units of the data that are stored in results files). Use the Edit > Options > Common
> Units dialog box to set your preferred units.
17.2.3.18. exprExists(Expression)
bool exprExists("Expression")
318
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Predefined Power Syntax Subroutines
Returns true if an expression with this name exists; false otherwise.
17.2.3.19. fanNoiseDefault()
This is an internal subroutine that is used only to initialize report templates.
17.2.3.20. fanNoise()
This is an internal subroutine that is used only to initialize report templates.
17.2.3.21. force(Location, Axis)
real force("Location", "Axis")
Returns the force on a 2D locator. For details, see force (p. 246).
17.2.3.22. forceNorm(Location, Axis)
real forceNorm("Location", "Axis")
Returns the per unit width force on a line in the direction of the specified axis. It is available only for a
polyline created by intersecting a locator on a boundary. For details, see forceNorm (p. 247).
17.2.3.23. getBladeForceExpr()
This is an internal subroutine that is used only to initialize report templates.
17.2.3.24. getBladeTorqueExpr()
This is an internal subroutine that is used only to initialize report templates.
17.2.3.25. getCCLState()
This is an internal debugging call.
17.2.3.26. getChildrenByCategory(Category)
string getChildrenByCategory("Category")
Returns the children of an object that belong to the specified category in a comma-separated list. Each
object type (for example, a PLANE) can have multiple categories associated with it such as "geometry",
"surface", and so on). Categories are specified in <CFXROOT>/etc/CFXPostRules.ccl.
For example, to get a comma-separated list of all surfaces in a state at the top level (that is, not subobjects of other objects):
! $surfaces = getChildrenByCategory("/", "surface" );
Use 'split ","' to convert the string into an array of strings.
17.2.3.27. getChildren(Object Name, Child Type)
string getChildren("Object Name", "Child Type")
Returns the children of an object in a comma-separated list. If Child Type is not an empty string,
this subroutine return only children of the specified type.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
319
Power Syntax in ANSYS CFX
17.2.3.28. getExprOnLocators()
This is an internal subroutine that is used only to initialize report templates.
17.2.3.29. getExprString(Expression)
string getExprString("Expression")
Returns the value and the units of the expression in the form “value units”. For example: “100 m”.
17.2.3.30. getExprVal(Expression)
real getExprVal("Expression")
Returns only the "value" portion of the expression (units are not included).
17.2.3.31. getObjectName(Object Path)
string getObjectName("Object Path")
Extracts the name of an object from its full path. For example:
!string = getObjectName("/USER SURFACE:User Surface 1")
returns "User Surface 1". This is the form needed for evaluating a CEL expression.
17.2.3.32. getParameterInfo(Object Name, Parameter Name, Info Type)
string getParameterInfo("Object Name", "Parameter Name", "Info Type")
Returns the requested information for a parameter of an object. Object Name returns the name or
path of an object; "/" or an empty string specifies the root.Parameter Name returns the name of the
parameter. Info Type returns the type of data requested; this can be one of "type", "value", "default
value", or "allowed values". For example:
! $info = getParameterInfo("/USER DEFINED/POINT:Point 1", "Symbol Size", "default value");
! print "getParameterInfo returned=$info\n";
prints:
getParameterInfo returned=2.5
17.2.3.33. getParameters(Object Name)
string getParameters("Object Name")
Returns the parameters of an object in a comma-separated list. Use 'split ","' to convert the string
into an array of strings.
17.2.3.34. getTempDirectory()
string getTempDirectory()
Returns the temporary directory path.
17.2.3.35. getType(Object Name)
string getType("Object Name")
Returns the object type.
320
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Predefined Power Syntax Subroutines
17.2.3.36. getValue(Object Name, Parameter Name)
string getValue("Object Name", "Parameter Name")
Takes a CCL object and parameter name and returns the value of the parameter.
Returns the value stored in Parameter Name.
17.2.3.36.1. Example
1.
Create a text object called Text 1.
2.
In the Text String box, enter Here is a text string.
3.
Click Apply to create the text object.
4.
In the Command Editor dialog box, enter the following:
!string = getValue( "/TEXT:Text 1/TEXT ITEM: Text Item 1", "Text String");
! print $string;
5.
Click Process, and the string will be printed to your terminal window.
The same procedure can be carried out for any object.
17.2.3.37. getViewArea()
string,string getViewArea()
Calculates the area of the scene projected in the view direction. Returns the area and the units in an
array of strings.
17.2.3.38. isCategory(Object Name, Category)
bool isCategory("Object Name", "Category")
A return of 1 indicates that the object matches the passed category; 0 otherwise. Categories are specified
in <CFXROOT>/etc/CFXPostRules.ccl.
For example, the following prints "Plane 1 is a surface":
! if( isCategory( "Plane 1", "surface" )) {
!
print "Plane 1 is a surface\n";
! }
17.2.3.39. Length(Location)
real Length("Location")
Returns the length of a line locator. For details, see length (p. 248).
Note
While using this function in Power Syntax the leading character is capitalized to avoid confusion with the Perl internal command “length.”
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
321
Power Syntax in ANSYS CFX
17.2.3.40. lengthAve(Variable, Location)
real lengthAve("Variable", "Location")
Returns the length-based average of the variable on the line locator. For details, see lengthAve (p. 249).
17.2.3.41. lengthInt(Variable, Location)
real lengthInt("Variable", "Location")
Returns the length-based integral of the variable on the line locator. For details, see lengthInt (p. 250).
17.2.3.42. liquidTurbPerformTurbo()
This is an internal subroutine that is used only to initialize report templates.
17.2.3.43. liquidTurbPerform()
This is an internal subroutine that is used only to initialize report templates.
17.2.3.44. massFlow(Location)
real massFlow("Location")
Returns the mass flow through the 2D locator. For details, see massFlow (p. 250).
17.2.3.45. massFlowAve(Variable, Location)
real massFlowAve("Variable","Location")
Returns the average value of the variable, weighted by mass flow, through the 2D locator. For details,
see massFlowAve (p. 252).
17.2.3.46. massFlowAveAbs(Variable, Location)
real massFlowAveAbs("Variable","Location")
Returns the average value of the variable, weighted by absolute mass flow, through the 2D locator. For
details, see massFlowAveAbs (p. 252).
17.2.3.47. massFlowInt(Variable, Location)
real massFlowInt("Variable", "Location")
Returns the integral of the variable, weighted by mass flow, over the 2D locator. For details, see massFlowInt (p. 254).
17.2.3.48. maxVal(Variable, Location)
real maxVal("Variable", "Location")
Returns the maximum value of the variable at the location. For details, see maxVal (p. 255).
17.2.3.49. minVal(Variable, Location)
real minVal("Variable", "Location")
Returns the minimum value of the variable at the location. For details, see minVal (p. 255).
322
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Predefined Power Syntax Subroutines
17.2.3.50. objectExists(Object Name)
bool objectExists("Object Name")
A return of 1 indicates that the object exists; 0 otherwise.
17.2.3.51. probe(Variable, Location)
real probe("Variable", "Location")
Important
This calculation should only be performed for point locators described by single points. Incorrect solutions will be produced for multiple point locators.
Returns the value of the variable at the point locator. For details, see probe (p. 256).
17.2.3.52. pumpPerform()
This is an internal subroutine that is used only to initialize report templates.
17.2.3.53. pumpPerformTurbo()
This is an internal subroutine that is used only to initialize report templates.
17.2.3.54. range(Variable, Location)
real,real range("Variable", "Location")
Returns the minimum and maximum values of the variable at the location.
17.2.3.55. reportError(String)
void reportError("String")
Pops up an error dialog box.
17.2.3.56. reportWarning(String)
void reportWarning("String")
Pops up a warning dialog box.
17.2.3.57. showPkgs()
void showPkgs()
Prints to the console a list of packages available that may contain other variables or subroutines in
Power Syntax.
17.2.3.58. showSubs(packageName)
void showSubs("packageName")
Prints to the console a list of the subroutines available in the specified package. If no package is specified,
CFD-Post is used by default.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
323
Power Syntax in ANSYS CFX
17.2.3.59. showVars(packageName)
void showVars("packageName")
Prints to the console a list of the Power Syntax variables and their current value defined in the specified
package. If no package is specified, CFD-Post is used by default.
17.2.3.60. spawnAsyncProcess(command, arguments)
bool spawnAsyncProcess("command", "arguments")
Spawns a forked process. For example:
! spawnAsyncProcess("dir", "c:/");
Displays the contents of c:\ in the console window.
17.2.3.61. sum(Variable, Location)
real sum("Variable", "Location")
Returns the sum of the variable values at each point on the locator. For details, see sum (p. 257).
17.2.3.62. torque(Location, Axis)
real torque("Location", "Axis")
Returns the computed value of torque at the 2D locator about the specified axis. For details, see
torque (p. 258).
17.2.3.63. turbinePerform()
This is an internal subroutine that is used only to initialize report templates.
17.2.3.64. turbinePerformTurbo()
This is an internal subroutine that is used only to initialize report templates.
17.2.3.65. verboseOn()
bool verboseOn()
Returns 1 or 0 depending if the Perl variable $verbose is set to 1.
17.2.3.66. volume(Location)
real volume("Location")
Returns the volume of a 3D locator. For details, see volume (p. 259).
17.2.3.67. volumeAve(Variable, Location)
real volumeAve("Variable", "Location")
Returns the average value of a variable over the 3D locator. For details, see volumeAve (p. 259).
17.2.3.68. volumeInt(Variable, Location)
real volumeInt("Variable", "Location")
324
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Predefined Power Syntax Subroutines
Returns the integral of a variable over the 3D locator. For details, see volumeInt (p. 259).
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
325
326
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Chapter 18: Bibliography
This bibliography contains entries referenced in the CFX documentation.
• References 1-20 (p. 327)
• References 21-40 (p. 330)
• References 41-60 (p. 333)
• References 61-80 (p. 336)
• References 81-100 (p. 339)
• References 101-120 (p. 341)
• References 121-140 (p. 344)
• References 141-160 (p. 347)
• References 161-180 (p. 350)
• References 181-200 (p. 353)
• References 201 – (p. 356)
18.1. References 1-20
1
Hutchinson, B.R. and Raithby, G.D.,
“A Multigrid method Based on the Additive Correction Strategy”, Numerical Heat Transfer,
Vol. 9, pp. 511-537, 1986.
2
Rhie, C.M. and Chow, W.L.,
“A Numerical Study of the Turbulent Flow Past an Isolated Airfoil with Trailing Edge
Separation”,
AIAA Paper 82-0998, 1982
3
Raw, M.J.,
“A Coupled Algebraic Multigrid Method for the 3D Navier-Stokes Equations”,
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
327
Bibliography
10th GAMM Seminar, Kiel, 1994.
4
Launder, B.E., Reece, G.J. and Rodi, W.,
“Progress in the developments of a Reynolds-stress turbulence closure”,
J. Fluid Mechanics, Vol. 68, pp.537-566, 1975.
5
Speziale, C.G., Sarkar, S. and Gatski, T.B.,
“Modelling the pressure-strain correlation of turbulence: an invariant dynamical systems
approach”,
J. Fluid Mechanics, Vol. 277, pp. 245-272, 1991.
6
Schiller, L. and Naumann, A.,
VDI Zeits, 77, p. 318, 1933.
7
Hughmark, G.A.,
AIChE J., 13 p. 1219, 1967.
8
Modest, M.,
“Radiative Heat Transfer”, Second Edition
Academic Press, 2003.
9
Menter, F.R.,
“Two-equation eddy-viscosity turbulence models for engineering applications”,
AIAA-Journal., 32(8), pp. 1598 - 1605, 1994.
10
Grotjans, H. and Menter, F.R.,
“Wall functions for general application CFD codes”,
In K.D.Papailiou et al., editor, ECCOMAS 98 Proceedings of the Fourth European Computational Fluid Dynamics Conference, pp. 1112-1117. John Wiley & Sons, 1998.
11
328
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 1-20
Wilcox, D.C.,
“Multiscale model for turbulent flows”,
In AIAA 24th Aerospace Sciences Meeting. American Institute of Aeronautics and Astronautics, 1986.
12
Menter, F.R.,
“Multiscale model for turbulent flows”,
In 24th Fluid Dynamics Conference. American Institute of Aeronautics and Astronautics,
1993.
13
Launder, B.E. and Spalding, D.B.,
“The numerical computation of turbulent flows”,
Comp Meth Appl Mech Eng, 3:269-289, 1974.
14
White, F.M.,
“Viscous Fluid Flow”, Second Edition,
McGraw-Hill, 1991.
15
Kader, B.A.,
“Temperature and concentration profiles in fully turbulent boundary layers”,
International Journal of Heat and Mass Transfer, 24(9):1541-1544, 1981.
16
Huang, P.G., Bradshaw, P. and Coakley, T.J.,
“Skin friction and velocity profile family for compressible turbulent boundary layers”,
American Institute of Aeronautics and Astronautics Journal, 31(9):1600-1604, 1993.
17
Bouillard, J.X, Lyczkowski, R.W.and Gidaspow, D.,
“Porosity Distribution in a Fluidised Bed with an Immersed Obstacle”,
AIChE J., 35, 908-922, 1989.
18
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
329
Bibliography
Gidaspow, D.,
“Multiphase Flow and Fluidisation”, Academic Press, 1994.
19
Ishii, M. and Zuber, N.,
“Drag Coefficient and Relative Velocity in Bubbly, Droplet or Particulate Flows”,
AIChE J., 25, 843-855, 1979.
20
Lopez de Bertodano, M.,
“Turbulent Bubbly Flow in a Triangular Duct”,
Ph.D. Thesis, Rensselaer Polytechnic Institute, Troy New York, 1991.
18.2. References 21-40
21
Lopez de Bertodano, M.,
“Two Fluid Model for Two-Phase Turbulent Jet”,
Nucl. Eng. Des. 179, 65-74, 1998.
22
Sato, Y. and Sekoguchi, K.,
“Liquid Velocity Distribution in Two-Phase Bubbly Flow”,
Int. J. Multiphase Flow, 2, p.79, 1975.
23
Siegel, R and J.R. Howell,
“Thermal Radiation Heat Transfer”,
ISBN 0-89116-506-1.
24
Goldstein, M. and J.R. Howell,
“Boundary Conditions for the Diffusion Solution of Coupled Conduction-Radiation
Problems”,
NASA Technical Note, NASA TN D-4618.
25
330
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 21-40
Raw, M.J.,
“Robustness of Coupled Algebraic Multigrid for the Navier-Stokes Equations”,
AIAA 96-0297, 34th Aerospace and Sciences Meeting & Exhibit, January 15-18 1996,
Reno, NV.
26
Kee, R. J., Rupley, F. M. and Miller, J. A.,
“Chemkin -II: A Fortran Chemical Kinetics Package for the Analysis of Gas-Phase Chemical
Kinetics",
Sandia National Laboratories Report, SAND89-8009,(1991).
27
Brackbill, J.U, Kothe, D.B. and Zemach, C.,
“A Continuum Method for Modelling Surface Tension”,
Journal of Computational Physics 100:335-354, 1992.
28
Barth, T.J., and Jesperson, D.C,
“The Design and Application of Upwind Schemes on Unstructured Meshes”,
AIAA Paper 89-0366, 1989.
29
Bird, R.B., Stewart, W.E. and Lightfoot, E.N.,
“Transport Phenomena”,
John Wiley & Sons, Inc., 1960.
30
Wilcox, D.C.,
“Turbulence Modelling for CFD”,
DCW Industries, 2000, La Canada, CA 91011, p. 314.
31
Launder, B.E., Tselepidakis, D. P., Younis, B. A.,
“A second-moment closure study of rotating channel flow”,
J. Fluid Mech., Vol. 183, pp. 63-75, 1987.
32
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
331
Bibliography
Menter, F. R.,
“Eddy Viscosity Transport Equations and their Relation to the
Model”,
NASA Technical Memorandum 108854, November 1994.
33
Menter, F. R.,
“Eddy Viscosity Transport Equations and their Relation to the
Model”,
ASME J. Fluids Engineering, Vol. 119, pp. 876-884, 1997.
34
Smagorinsky, J.,
“General Circulation Experiments with the Primitive Equations”,
Month. Weath. Rev. Vol. 93, pp. 99-165, 1963.
35
Clift, R., Grace, J.R., Weber, M.E.,
“Bubbles, Drops and Particles”,
Academic Press, New York, U.S.A., 1978.
36
Liang, L., Michaelides, E. E.,
“The magnitude of Basset forces in unsteady multiphase flow computations”,
Journal of Fluids Engineering, Vol. 114, pp. 417-419, 1992.
37
Peters, N.,
“Turbulent Combustion”,
Cambridge monographs on mechanics, Cambridge University Press, 2000.
38
Zimont, V.L., Polifke, W., Bettelini, M. and Weisenstein, W.,
“An efficient Computational Model for Premixed Turbulent Combustion at High Reynolds
Numbers Based on a Turbulent Flame Speed Closure“,
J. Engineering for Gas Turbines and Power (Transactions of the ASME), Vol. 120, pp. 526532, 1998.
39
332
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 41-60
Hinze, J. O.,
“Turbulence”,
McGraw-Hill, New York, U.S.A., 1975.
40
Zimont, V.L.,
“Gas Premixed Combustion at High Turbulence. Turbulent Flame Closure Combustion
Model”,
Proceedings of the Mediterranean Combustion Symposium, Instituto di Richerche sulla
Combustione - CNR, Italy, pp. 1155-1165, 1999.
18.3. References 41-60
41
Zimont, V.L., Biagioli, F. and Syed, Khawar,
“Modelling turbulent premixed combustion in the intermediate steady propagation regime”,
Progress in Computational Fluid Dynamics, Vol. 1, pp. 14-28, 2001.
42
Linan, A.,
“On the internal structure of laminar diffusion flames”,
Technical note, Inst. nac. de tec. aeron., Esteban Terradas, Madrid, Spain, 1961.
43
Warnatz, J., Mass, U. and Dibble, R. W.,
“Combustion”,
Springer, Verlag, 1996, pp.219-221.
44
Magnussen, B. F.,
“The Eddy Dissipation Concept for Turbulent Combustion Modelling. Its Physical and
Practical Implications”,
Presented at the First Topic Oriented Technical Meeting, International Flame Research
Foundation, IJmuiden, The Netherlands, Oct. 1989.
45
Tesner, P. A., Snegirova, T. D., and Knorre, V. G.,
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
333
Bibliography
“Kinetics of Dispersed Carbon Formation”,
Combustion and Flame, Vol. 17, pp. 253-260, 1971.
46
Magnussen, B. F., and Hjertager, B. H.,
“On Mathematical Modeling of Turbulent Combustion with Special Emphasis on Soot
Formation and Combustion”,
Sixteenth Symp. (Int.) on Combustion, The Combustion Institute, p 719, 1976.
47
Vukalovich, M. P.,
“Thermodynamic Properties of Water and Steam”,
Mashgis, Moscow, 6th ed., 1958.
48
Hottel, H.C. and Sarofim, A.F.,
“Radiative transfer”,
McGraw-Hill, New York 1967.
49
Hadvig, S.,
“Gas emissivity and absorptivity”,
J. Inst. Fuel, 43, pp. 129-135., 1970.
50
Leckner, B.,
“Spectral and total emissivity of water vapour and carbon dioxide”,
Comb. Flame, 19, pp. 33-48., 1972.
51
Taylor, P.B. and Foster, P.J.,
“The total emissivities of luminous and non-luminous flames”,
Int. J. Heat Mass Transfer, 17, pp. 1591-1605., 1974.
52
Beer, J.M., Foster, P.J. and Siddall, R.G.,
334
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 41-60
“Calculation methods of radiative heat transfer”,
HTFS Design Report No. 22, AEA Technology (Commercial)., 1971.
53
Prakash, C.,
“Two phase model for binary liquid-solid phase change”,
Parts I and II, Numerical Heat Transfer, B 15, p. 171.
54
CFX Limited, Waterloo, Ontario, Canada,
CFX-TASCflow Theory Documentation,
Section 4.1.2, Version 2.12, 2002.
55
Menter, F. R. and Kuntz, M.,
“Development and Application of a Zonal DES Turbulence Model for CFX-5”,
CFX-Validation Report, CFX-VAL17/0503.
56
Menter, F.R., Kuntz, M.,
“Adaptation of Eddy-Viscosity Turbulence Models to Unsteady Separated Flow Behind
Vehicles”,
Proc. Conf. The Aerodynamics of Heavy Vehicles: Trucks, Busses and Trains, Asilomar, Ca,
2002.
57
Spalart, P.R, Jou, W.-H., Strelets, M. and Allmaras, S.R.,
“Comments on the feasibility of LES for wings, and on a hybrid RANS/LES approach”,
1st AFOSR Int. Conf. On DNS/LES, Aug.4-8, 1997, Ruston, LA. In Advances in DNS/LES, C.
Liu & Z. Liu Eds., Greyden Press, Colombus, OH.
58
Strelets, M.,
“Detached Eddy Simulation of Massively Separated Flows”,
AIAA Paper 2001-0879, 39th Aerospace Sciences Meeting and Exhibit, Reno, NV, 2001.
59
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
335
Bibliography
Ishii, M.,
“One-dimensional drift-flux model and constitutive equations for relative motion between
phases in various two-phase flow regimes”,
Argonne National Laboratory ANL-77-47, 1977.
60
Manninen, M. and Tavassalo, V.,
“On the Mixture Models for Multiphase Flow”,
VTT Publications, 1996.
18.4. References 61-80
61
Luo, S.M., and Svendsen, H.,
“Theoretical Model for Drop and Bubble Breakup in Turbulent Dispersions”,
AIChE Journal 42, 1225 -1233.
62
Prince, M. and Blanch, H.,
“Bubble Coalescence and Break-Up in Air-Sparged Bubble Columns”,
AIChE Journal 36, 1485-1499.
63
Hutchings, I.M.,
“Mechanical and metallurgical aspects of the erosion of metals”,
Proc. Conf. on Corrosion-Erosion of Coal Conversion System Materials, NACE (1979) 393.
64
Dosanjh, S., and Humphrey, J.A.C.,
“The influence of turbulence C on erosion by a particle laden fluid jet, Wear”,
V.102, 1985, pp. 309-330.
65
Aungier, R.H.,
“Centrifugal Compressors: A strategy for Aerodynamic Design and Analysis”,
ASME Press, New York, 2000.
336
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 61-80
66
Westbrook, C.K., Dryer, F.L.,
“Simplified Reaction Mechanisms for the Oxidation of Hydrocarbon Fuels in Flames”,
Combustion Science and Technology Vol. 27, pp. 31-43, 1981.
67
Faeth, G. M.,
“Mixing, transport and combustion in sprays”,
Process Energy Combustion Science, Vol. 13, pp. 293-345, 1987.
68
Mijnbeek, G.,
“Bubble column, airlift reactors and other reactor designs”, Operational Modes of Bioreactors, Chapter 4,
Butterworth and Heinemann, 1992.
69
Bello, R. A., Robinson, C. W., and Moo-Young, M.,
Canadian Journal of Chemical Engineering, Vol. 62, pp. 573. Chemical Institute of Canada
and Canadian Society for Chemical Engineering, 1984.
70
García-Calvo, E. and Letón, P.,
“Prediction of gas hold-up and liquid velocity in airlift reactors using two-phase flow
friction coefficients”,
Journal of Chemical Technology & Biotechnology, Vol. 67, pp. 388-396,
Wiley Interscience, 1996.
71
Maneri, C. C. and Mendelson, H. D.,
American Institute of Chemical Engineers Journal, Vol. 14, p. 295. American Institute of
Chemical Engineers, 1968.
72
Baker, J. L. L. and Chao, B. T.,
American Institute of Chemical Engineers Journal, Vol. 11, p. 268. American Institute of
Chemical Engineers, 1965.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
337
Bibliography
73
Hughmark, G. A.,
Industrial Engineering and Chemical Process Design and Development, Vol. 6, p. 218.
1967.
74
S. Lo, R. Bagatin and M. Masi.,
“The Development of a CFD Analysis and Design Tool for Air-lift Reactors”,
Proceedings of the SAIChE 2000 Conference, Secunda, South Africa, 2000.
75
Ranz, W.E. and Marshall, W.R.,
Chem. Eng. Prog. 48(3), p. 141, 1952.
76
Bardina, J.E., Huang, P.G. and Coakley, T.J.,
“Turbulence Modeling Validation Testing and Development”,
NASA Technical Memorandum 110446, 1997. (See also Bardina, J.E., Huang, P.G. and
Coakley, T.J., “Turbulence Modeling Validation”, AIAA Paper 97-2121.)
77
H. Schlichting.,
“Boundary Layer Theory”,
McGraw-Hill, 1979.
78
Badzioch, S., and Hawksley, P.G.W.,
“Kinetics of thermal decomposition of pulverised coal particles, Industrial Engineering
Chemistry Process Design and Development, 9 p. 521”, 1997.
79
S.J. Ubhayakar, D.B. Stickler, C.W. Von Rosenburg, and R.E. Gannon;
“Rapid devolatilization of pulverised coal in hot combustion gases”,
16th Symposium (International) on Combustion, The Combustion Institute, p. 426, 1976.
80
Wall, T.F., Phelan, W.J., and Bartz, S.,
338
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 81-100
“The prediction of scaling of burnout in swirled pulverised coal flames”,
InternationalFlame Research Foundation Report F388/a/3 IJmuiden, The Netherlands,
1976.
18.5. References 81-100
81
Sutherland, W.,
“The Viscosity of Gases and Molecular Force”,
Phil. Mag. 5:507-531, 1893.
82
Hirschfelder, J.O., Taylor, and M.H., Bird, R.B.,
“Molecular Theory of Gases and Liquids”,
Wiley, New York, 1954.
83
Chung, T.H., Lee, L.L., and Starling, K.E.,
“Applications of Kinetic Gas Theories and Multiparameter Correlation for Prediction of
Dilute Gas Viscosity and Thermal Conductivity”,
Ind. Eng. Chem. Fundam.
23:8, 1984.
84
Poling, B.E., Prausnitz, J.M., and O’Connell, J.P.,
“The Properties of Gases and Liquids”,
McGraw-Hill, New York, 2001.
85
Redlich, O., and Kwong, J.N.S.,
"On the Thermodynamics of Solutions. V. An Equation of State. Fugacities of Gaseous
Solutions.",
Chem Rev 44:233, 1949.
86
Saffman, P. G.,
“The lift on a small sphere in a slow shear flow”,
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
339
Bibliography
J. Fluid Mech., 22, p. 385, 1965.
87
Mei, R. and Klausner, J. F.,
“Shear lift force on spherical bubbles”,
Int. J. Heat and Fluid Flow, 15, p. 62, 1994.
88
Antal, S. P., Lahey, R. T., and Flaherty, J. E.,
“Analysis of phase distribution in fully developed laminar bubbly two-phase flow”,
Int. J. Multiphase Flow, 7, pp. 635-652, 1991.
89
Krepper, E., and Prasser, H-M.,
“Measurements and CFX Simulations of a bubbly flow in a vertical pipe”,
in AMIFESF Workshop, Computing Methods in Two-Phase Flow, 2000.
90
Burns, A.D.B., Frank, Th., Hamill, I., and Shi, J-M.,
“The Favre Averaged Drag Model for Turbulent Dispersion in Eulerian Multi-Phase Flows”,
5th International Conference on Multiphase Flow, ICMF-2004, Yokohama, Japan.
91
Moraga, J.F., Larreteguy, A.E., Drew, D.A., and Lahey, R.T.,
“Assessment of turbulent dispersion models for bubbly flows in the low Stokes number
limit”,
Int. J. Multiphase Flow, 29, p. 655, 2003.
92
CIBSE Guide A: Environmental Design
CIBSE, U.K., 1999.
93
ISO 7730-1984(E), Moderate thermal environments - Determination of the PMV and PPD
indices and specification of the conditions for thermal comfort
1984.
94
340
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 101-120
Yamada, T. and R.D. Gunn,
J. Chem Eng. Data, 18, p. 234, 1973.
95
Pitzer, K.S., D.Z. Lippmann, R.F. Curl, C.M. Huggins, and D.E. Petersen,
J. Am. Chem. Soc., 77: 3433 (1955).
96
Aungier, R.H.,
“A Fast, Accurate Real Gas Equation of State for Fluid Dynamic Analysis Applications”,
Journal of Fluids Engineering, Vol. 117, pp. 277-281, 1995.
97
H. Enwald, E. Peirano and A. E. Almstedt,
“Eulerian Two-Phase Flow Theory Applied to Fluidisation”,
Int. J. Multiphase Flow, 22 Suppl., pp. 21-66,1996.
98
J. Ding and D. Gidaspow,
“A Bubbling Fluidisation Model using Theory of Granular Flow”,
AIChEJ. 36, pp. 523-538, 1990.
99
C.K.K. Lun, S.B. Savage, D.J. Jeffery, and N. Chepurniy,
“Kinetic Theories for Granular Flow: Inelastic Particles in Couette Flow and Slightly Inelastic
Particles in a General Flow Field”,
J. Fluid Mech., 140, pp. 223-256, 1984.
100
C.K.K. Lun, and S.B. Savage,
“The Effects of an Impact Velocity Dependent Coefficient of Restitution on Stresses Developed by Sheared Granular Materials”,
Acta Mechanica., 63, pp. 15-44, 1986.
18.6. References 101-120
101
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
341
Bibliography
Menter, F.R., Langtry, R.B., Likki, S.R., Suzen, Y.B., Huang, P.G., and Völker, S.,
“A Correlation based Transition Model using Local Variables Part 1- Model Formulation”,
ASME-GT2004-53452, ASME TURBO EXPO 2004, Vienna, Austria.
102
Langtry, R.B., Menter, F.R., Likki, S.R., Suzen, Y.B., Huang, P.G., and Völker, S.,
“A Correlation based Transition Model using Local Variables Part 2 - Test Cases and Industrial Applications”,
ASME-GT2004-53454, ASME TURBO EXPO 2004, Vienna, Austria.
103
Langtry, R.B., Menter, F.R.,
“Transition Modeling for General CFD Applications in Aeronautics”,
AIAA paper 2005-522, 2005.
104
Mayle, R.E.,
“The Role of Laminar-Turbulent Transition in Gas Turbine Engines”,
ASME Journal of Turbomachinery, Vol. 113, pp. 509-537, 1991.
105
R. Schmehl,
“Advanced Modelling of Droplet Deformation and Breakup for CFD Analysis of Mixture
Preparation”,
ILASS-Europe 2002, 2002.
106
Miller A. and Gidaspow D,
AIChE Journal, Vol. 38, No. 11, p. 1811, 1992.
107
F.X. Tanner,
“Liquid Jet Atomization and Droplet Breakup Modeling of Non-Evaporating Diesel Fuel
Sprays”,
SAE Technical Paper Series, 970050, 1997.
108
342
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 101-120
B. Liu, D. Mather and R.D. Reitz,
“Effects of Drop Drag and Breakup on Fuel Sprays”,
SAE Technical Paper 930072, 1993.
109
L.P. Hsiang and G.M. Faeth,
“Near-Limit Drop Deformation and Secondary Breakup”,
International Journal of Multiphase Flow, Vol. 18, No. 5, pp. 635-652, 1992.
110
S. C. Kuensberg, S.-C., Kong and R. D. Reitz,
“Modelling the Effects of Injector Nozzle Geometry on Diesel Sprays”,
SAE Paper 1999-01-0912, 1999.
111
H. Hiroyasu and T. Kadota,
“Fuel droplet size distribution in diesel combustion chamber”,
SAE Technical Paper, 740715, 1974.
112
R. Schmehl, G. Maier and S. Wittig,
“CFD Analysis of Fuel Atomization, Secondary Droplet Breakup and Spray Dispersion in
the Premix Duct of a LPP Combustor”,
Proc. of 8th Int. Conf. on Liquid Atomization and Spray Systems, Pasadena, CA, USA,
2000.
113
Schlichting, H., and Gersten, K.,
“Grenzschicht-Theorie”.
9. Auflage, Springer-Verlag Berlin, Heidelberg, New York, 1997
114
W.H. Nurick,
“Orifice Cavitation and Its Effect on Spray Mixing”,
Journal of Fluids Engineering, Vol. 98, pp. 681-687, 1976.
115
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
343
Bibliography
R.D. Reitz and R. Diwakar,
“Structure of High-Pressure Fuel Sprays”,
SAE Technical Paper, 870598, 1987.
116
P.J.O'Rourke and A.A. Amsden,
“The TAB Method for Numerical Calculation of Spray Droplet Breakup”,
SAE Technical Paper 872089, 1987.
117
M. Pilch and C.A. Erdman,
“Use of Breakup Time Data and Velocity History Data to Predict the Maximum Size of
Stable Fragments for Acceleration-Induced Breakup of a Liquid Drop”,
Int. J. Multiphase Flow, Vol. 13, No. 6, pp. 741-757, 1987.
118
S.V. Patankar,
“Numerical Heat Transfer and Fluid Flow”,
Hemisphere Publishing Corp., 1980.
119
S. Majumdar,
“Role of Underrelaxation in Momentum Interpolation for Calculation of Flow with Nonstaggered Grids”,
Numerical Heat Transfer 13:125-132.
120
C. Baumgarten, H. Lettmann and G.P. Merker,
“Modelling of Primary and Secondary Break-Up Processes in High Pressure Diesel Sprays”,
Paper No. 7, CIMAC Congress, Kyoto 2004.
18.7. References 121-140
121
T. Iijima and T. Takeno,
“Effects of pressure and temperature on burning velocity”,
344
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 121-140
Combust. Flame, Vol. 65, pp. 35-43, 1986.
122
B. Lewis and G. v. Elbe,
“Combustion, Flames and Explosions of Gases”,
3rd Edition, Academic Press, London, 1987.
123
B. E. Milton and J.C. Keck,
“Laminar burning velocities in stoichiometric hydrogen and hydrogen-hydrocarbon gas
mixtures”,
Combust. Flame, Vol. 58, pp. 13-22, 1984.
124
M. Metghalchi and J.C. Keck,
“Burning Velocities of Mixtures of Air with Methanol, iso-octane and indolene at High
Pressure and Temperature”,
Combust. Flame, Vol. 48, pp. 191-210, 1982.
125
W. Wagner, and A. Kruse,
“The Industrial Standard IAPWS-IF97: Properties of Water and Steam”,
Springer, Berlin, 1998.
126
Senecal, P.K., Schmidt, D.P., Nouar, I., Rutland, C.J., Reitz, R.D. and Corradin, M.L.,
"Modeling High-Speed Viscous Liquid Sheet Atomization",
International Journal of Multiphase Flow, 25, pp. 1073-1097, 1999.
127
Han, Z., Perrish, S., Farrell, P.V. and Reitz R.D.,
"Modeling Atomization Processes of Pressure-Swirl Hollow-Cone Fuel Sprays",
Atomization and Sprays, Vol. 7, pp. 663-684, Nov.-Dec. 1997.
128
Kato, M., Launder, B.E.,
"The modelling of turbulent flow around stationary and vibrating square cylinders",
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
345
Bibliography
Ninth Symposium on "Turbulent Shear Flows", Kyoto, Japan, August 16-18, 1993.
129
Menter, F. R.,
"Zonal two equation
turbulence models for aerodynamic flows",
AIAA Paper 93-2906, 1993.
130
Menter F. R. and Egorov, Y.,
"Re-visiting the turbulent scale equation",
Proc. IUTAM Symposium; One hundred years of boundary layer research, Göttingen,
2004.
131
Menter, F.R. and Egorov, Y.,
"A Scale-Adaptive Simulation Model using Two-Equation Models",
AIAA paper 2005-1095, Reno/NV, 2005.
132
Menter, F. R, Kuntz, M., Bender R.,
"A scale-adaptive simulation model for turbulent flow predictions",
AIAA Paper 2003-0767, 2003.
133
Menter. F. R., Kuntz, M. and Durand. L.,
"Adaptation of eddy viscosity turbulence models to unsteady separated flow behind
vehicles",
The Aerodynamics Of Heavy Vehicles: Trucks, Buses And Trains, Monterey, Dec.2-6, 2002.
134
Rotta, J. C.,
"Turbulente Strömungen",
Teubner Verlag, Stuttgart, 1972.
135
Spalart P. R.,
"Young-Person's Guide to Detached-Eddy Simulation Grids",
346
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 141-160
NASA/CR-2001-211032, 2001.
136
Wilcox, D. C.,
"Turbulence Modelling for CFD",
DWC Industries, La Cañada, 1993.
137
Squires, K.,
"Detached eddy simulation: Current status and future perspectives",
Proc. DLES-5 Conference, München, 2004.
138
Jovic, S., Driver, D. M.,
"Backward-facing step measurement at low Reynolds number, Reh=5000",
NASA TM 108807, 1994.
139
Roache, P. J.,
“Verification and Validation in Computational Science and Engineering”,
Hermosa publishers, Albuquerque, New Mexico, 1998.
140
Casey, M. and Wintergerste W.,
“Best Practice Guidelines”,
ERCOFTAC Special Interest Group on Quality and Trust in Industrial CFD, Report, 2000.
18.8. References 141-160
141
Ferziger, J. H. and Peric, M.,
“Computational methods for fluid dynamics”,
Springer, Berlin.
142
Menter, F. R. and Esch T.,
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
347
Bibliography
“Elements of Industrial Heat Transfer Predictions”,
16th Brazilian Congress of Mechanical Engineering (COBEM), Nov. 2001, Uberlandia, Brazil.
143
Menter, F.,
“CFD Best Practice Guidelines for CFD Code Validation for Reactor Safety Applications”,
Evaluation of Computational Fluid Dynamic Methods for Reactor Safety Analysis (ECORA),
European Commission, 5th EURATOM FRAMEWORK PROGRAMME, 1998-2002.
144
Menter F. R. and Egorov, Y.,
“Turbulence Models based on the Length-Scale Equation”,
Fourth International Symposium on Turbulent Shear Flow Phenomena, Williamsburg,
2005 - Paper TSFP4-268, 2005.
145
Menter F. R. and Egorov, Y.,
“SAS Turbulence Modelling of Technical Flows”,
DLES 6 - 6th ERCOFTAC Workshop on Direct and Large Eddy Simulation September,
Poitiers, 2005.
146
Spalart P. R.,
“Strategies for turbulence modelling and simulations”,
Int. J. Heat Fluid Flow, 21, pp. 252-263, 2000.
147
A. D. Gosman and E. Ioannides,
“Aspects of computer simulation of liquid fuelled combustors”,
AIAA Paper, No. 81-0323,1981.
148
F. Bakir, R. Rey, A.G. Gerber, T. Belamri and B. Hutchinson,
“Numerical and Experimental Investigations of the Cavitating Behavior of an Inducer”,
Int J Rotating Machinery, Vol. 10, pp. 15-25, 2004.
149
348
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 141-160
Frank, Th.,
“Parallele Algorithmen für die numerische Simulation dreidimensionaler, disperser
Mehrphasenströmungen und deren Anwendung in der Verfahrenstechnik”,
Habilitationsschrift, Shaker Verlag Aachen, pp. 1-329, 2002.
150
Hussmann, B. et al.,
“A stochastic particle-particle collision model for dense gas-particle flows implemented
in the Lagrangian solver of ANSYS CFX and its validation”,
6th International Conference on Multiphase Flows, ICMF 2007, Leipzig, Germany, 2007.
151
Oesterlé, B., Petitjean, A.,
“Simulations of particle-to-particle interactions in gas-solid flows”,
Int. J. Multiphase Flow, Vol. 19(1), pp. 199-211, 1993.
152
Sommerfeld, M.,
“Modellierung und numerische Berechnung von partikelbeladenen Strömungen mit
Hilfe des Euler-Lagrange-Verfahrens”,
Habilitationsschrift, Shaker Verlag Aachen, 1996.
153
Lavieville, J., Deutsch, E. and Simonin, O.,
“Large eddy simulations of interactions between colliding particles and a homogeneous
isotropic turbulence field”,
ASME FED Vol. 228, pp. 359-369, 1995.
154
Sommerfeld, M.,
“Validation of a stochastic Lagrangian modeling approach for inter-particle collision in
homogeneous isotropic turbulence”,
Int. J. Multiphase Flow, Vol. 27, pp. 1829 – 1858, 2001.
155
Huh, K.Y., Lee, E.,
“Diesel Spray Atomization Models Considering Nozzle Exit Turbulence Conditions”,
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
349
Bibliography
Atomization and Sprays, Vol. 8, pp. 453-469, 1998.
156
Chryssakis, C.A., Assanis, D.N.,
“A Secondary atomization Model for Liquid Droplet Deformations and Breakup under
High Weber Number Conditions”,
ILASS Americas, 18th Annual Conference on Liquid Atomization and Spray Systems,
Irvine, CA, 2005.
157
Peng, D.Y. and Robinson, D.B.,
“A New Two-Constant Equation of State”,
Ind. Eng. Chem. Fundam., Vol. 15, No. 1, pp. 59 – 64, 1976.
158
Chung, T.H., M. Ajlan, L.L. Lee and K.E. Starling,
“Generalized Multiparameter Correlation for Nonpolar and Polar Fluid Transport Properties”,
Ind. Eng. Chem. Res., Vol. 27, pp. 671 – 679, 1988.
159
Kurul, N. and Podowski, M. Z.,
“On the modeling of multidimensional effects in boiling channels”,
ANS Proc. 27th National Heat Transfer Conference, Minneapolis, MN, July 28-31, 1991.
160
Kocamustafaogullari, G. and Ishii, M.,
“Interfacial area and nucleation site density in boiling systems”,
Int. J. Heat Mass Transfer, 26 p. 1377, 1983.
18.9. References 161-180
161
Podowski, M. Z., Alajbegovic, A., Kurul, N., Drew, D.A. and Lahey, R. T.,
“Mechanistic modelling of CHF in forced-convection sub-cooled boiling”,
Int. Conference on Convective Flow and Pool Boiling, Irsee, Germany, 1997a.
162
350
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 161-180
Podowski, R. M., Drew, D.A., Lahey, R. T. and Podowski, M. Z.,
“A mechanistic model of the ebullition cycle in forced-convection sub-cooled boiling”,
NURETH-8, Kyoto, Japan, 1997b.
163
Egorov, Y. and Menter, F.,
“Experimental implementation of the RPI boiling model in CFX-5.6”,
Technical Report ANSYS / TR-04-10., 2004.
164
Lemmert, M. and Chawla, J. M.,
“Influence of flow velocity on surface boiling heat transfer coefficient”,
Heat Transfer and Boiling (Eds. E. Hahne and U. Grigull), Academic Press, 1977.
165
Tolubinski, V. I. and Kostanchuk, D. M.,
“Vapour bubbles growth rate and heat transfer intensity at subcooled water boiling”,
4th. International Heat Transfer Conference, Paris, France, 1970.
166
Cole, R.,
“A photographic study of pool boiling in the region of CHF”,
AIChEJ, 6 pp. 533-542, 1960.
167
Mikic, B. B. and Rohsenow, W. M.,
“A new correlation of pool boiling data including the fact of heating surface characteristics”,
ASME J. Heat Transfer, 91 pp. 245-250, 1969.
168
Del Valle, V. H. and Kenning, D. B. R.,
“Subcooled flow boiling at high heat flux”,
Int. J. Heat Mass Transfer, 28 p. 1907, 1985.
169
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
351
Bibliography
Ceumern-Lindenstjerna, W. C.,
“Bubble Departure and Release Frequencies During Nucleate Pool Boiling of Water and
Aqueous NaCl Solutions”,
Heat Transfer in Boiling, Academic Press and Hemisphere, 1977.
170
Saffman, P. G.,
Corrigendum to: “The lift on a small sphere in a slow shear flow”,
J. Fluid Mech., 31, p. 624, 1968
171
Legendre, D. and Magnaudet, J.,
“The lift force on a spherical bubble in a viscous linear shear flow”,
J. Fluid Mech., 368, pp. 81–126, 1998.
172
Tomiyama, A.,
“Struggle with computational bubble dynamics”,
ICMF'98, 3rd Int. Conf. Multiphase Flow, Lyon, France, pp. 1-18, June 8-12, 1998.
173
Frank, Th., Shi, J. M. and Burns, A. D.,
“Validation of Eulerian Multiphase Flow Models for Nuclear Safety Applications”,
3rd International Symposium on Two-Phase Flow Modelling and Experimentation, Pisa,
Italy, 22-24, Sept. 2004.
174
Wellek, R. M., Agrawal, A. K. and Skelland, A. H. P.,
“Shapes of liquid drops moving in liquid media”,
AIChE J, 12, pp. 854-862, 1966.
175
G. Elsässer,
“Experimentelle Untersuchung und numerische Modellierung der freien Kraftstoffstrahlausbreitung und Wandinteraktion unter motorischen Randbedingungen”,
Dissertation, Logos Verlag, Berlin, 2001
352
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 181-200
176
C. Bai and A.D. Gosman,
“Prediction of spray wall impingement in reciprocating engines”,
ILASS-Europe, July 1999
177
Frank, Th., Zwart, P. J., Krepper, E., Prasser, H. -M. and Lucas,
“Validation of CFD models for mono- and polydisperse air-water two-phase flows in
pipes”
J. Nuclear Engineering & Design, Vol. 238, pp. 647–659, March 2008.
178
Lighthill, M. J.,
“On sound generated aerodynamically. I. General theory”
Proc. R. Soc. Series A, Vol. 211, p. 564, 1952.
179
Lighthill, M. J.,
“On sound generated aerodynamically. II. Turbulence as a source of sound”
Proc. R. Soc. Series A, Vol. 222, 1954.
180
Ffowcs-Williams, J. E. and Hawkings, D. L.,
“Theory relating to the noise of rotating machinery”
J. Sound Vib., Vol. 10, pp. 10-21, 1969.
18.10. References 181-200
181
Wen, C. Y. and Yu, Y. H.,
“Mechanics of Fluidization”
Chem. Eng. Prog. Symp. Ser. 62, pp. 100-111, 1966.
182
Choi, C. R. and Huh, K. Y.,
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
353
Bibliography
"Development and validation of a coherent flamelet model for a spark-ignited turbulent
premixed flame in a closed vessel,"
Combustion & Flame Vol. 114, No. 3-4, 336-348, 1998.
183
A. M. Douaud, P.Eyzat,
“Four-Octane-Number Method for Predicting the Anti-Knock Behavior of Fuels and Engines”,
SAE Technical Paper 780080, SAE, 1978.
184
M. P. Halstead, L. J. Kirsch, C. P. Quinn,
“The Autoignition of Hydrocarbon Fuels at High Temperatures and Pressures – Fitting
of a Mathematical Model”,
Combustion and Flame, Vol. 30, pp. 45-60, 1977.
185
H. O. Hardenberg, F.W. Hase,
“An Empirical Formula for Computing the Pressure Rise Delay of a Fuel from Its Cetane
Number and from the Relevant Parameters of Direct-Injection Diesel Engines”,
SAE Technical Paper 790493, SAE, 1979.
186
Meneveau, C., and Poinsot, T.,
“Stretching and quenching of flamelets in premixed turbulent combustion”,
Combustion and Flame, 86:311-332, 1991.
187
T. Poinsot, D. Veynante,
“Theoretical and Numerical Combustion”,
Edwards, 2001.
188
Wallin, S. and Johansson A.,
“A complete explicit algebraic Reynolds stress model for incompressible and compressible
flows”,
Journal of Fluid Mechanics, 403, pp. 89-132, 2000.
354
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 181-200
189
Wallin, S., and Johansson A.,
“Modelling streamline curvature effects in explicit algebraic Reynolds stress turbulence
models”,
International journal of Heat and Fluid Flow, 23(5), pp. 721-730, 2002.
190
Hellsten, A.,
“New advanced
turbulence model for high-lift aerodynamics”,
AIAA Paper 2004-1120, Reno, Nevada, 2004.
191
Spalart, P.R., and Shur, M.
“On the sensitization of turbulence models to rotation and curvature”,
Aerospace Sci. Tech., 1(5), pp. 297-302, 1997.
192
Smirnov, P.E., and Menter, F.R.
“Sensitization of the SST turbulence model to rotation and curvature by applying the
Spalart-Shur correction term”,
ASME Paper GT 2008-50480, Berlin, Germany, 2008.
193
Coleman, H.W., Hodge, B.K., Taylor, R.P.,
“A Re-Evaluation of Schlichting’s Surface Roughness Experiment”,
Journal of Fluids Engineering, Vol. 106, 1984.
194
Lechner, R., and Menter, F.,
“Development of a rough wall boundary condition for
-based turbulence models”,
Technical Report ANSYS / TR-04-04, 2004.
195
Pimenta, M.M., Moffat, R.J. and Kays, W.M.,
“ The Turbulent Boundary Layer: An Experimental Study of the Transport of Momentum
and Heat with the Effect of Roughness”,
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
355
Bibliography
Interim Report Stanford University, CA, 1975.
196
Launder, B.E.,
“Second-moment closure: present … and future”.
Int. J. Heat and Fluid Flow, Vol. 10, No. 4, pp. 282-300, 1989.
197
Egorov, Y., and Menter, F.,
“Development and Application of SST-SAS Turbulence Model in the DESIDER Project”,
Second Symposium on Hybrid RANS-LES Methods, Corfu, Greece, 2007.
198
Germano, M., Piomelli, U., Moin, P., Cabot, W.H.,
“A Dynamic Subgrid-Scale Eddy Viscosity Model”,
Phys. Fluids A 3 (7), pp. 1760-1765, 1991.
199
Lilly, D.K.,
“A Proposed Modification of the Germano Subgrid-Scale Closure Method”,
Phys. Fluids A 4 (3), pp. 633-635, 1992.
200
Nicoud, F., Ducros, F.,
“Subgrid-Scale Stress Modelling Based on the Square of the Velocity Gradient Tensor”,
Flow, Turbulence and Combustion, 62, pp. 183-200, 1999.
18.11. References 201 –
201
Abramzon, B. and Sirignano, W.A.,
“Droplet Vaporization Model for Spray Combustion Calculations”
Int. J. Heat Mass Transfer, 32, pp. 1605–1618, 1989.
202
Sazhin, Sergei S.,
“Advanced Models of Fuel Droplet Heating and Evaporation”
356
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 201 –
Progress in Energy and Combustion Science, 32, pp. 162–214, 2006.
203
Hughes, T.J.R.,
“The Finite Element Method”
Prentice-Hall, Englewood Cliffs, N.J., 1987.
204
Simo, J.C. and Wong, K.K.,
“Unconditionally Stable Algorithms for Rigid Body Dynamics that exactly Preserves Energy
and Momentum”
Int. J. Num. Methods in Eng., 31, pp. 19-52, 1991.
205
Hughes, Peter C.,
“Spacecraft Attitude Dynamic”
Dover, 2004.
206
Etkin, Bernard.,
“The Dynamics of Atmospheric Flight”
John Wiley & Sons, 1972.
207
Conaire, Marcus Ó, Curran, Henry J., Simmie, John M., Pitz, William J., Westbrook, Charles
K.,
“A Comprehensive Modeling Study of Hydrogen Oxidation”,
International Journal of Chemical Kinetics,
Volume 36, Issue 11, pp. 603-622, 2004.
208
Frank, Th.
"Numerische Simulation der feststoffbeladenen Gasströmung im horizontalen Kanal unter
Berücksichtigung von Wandrauhigkeiten"
Ph.D. Thesis, Techn. University Bergakademie Freiberg, Germany, 1992
209
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
357
Bibliography
Matsumoto, S., Saito, S., Maeda, S.
"Simulation of Gas-Solid Two-Phase Flow in Horizontal Pipe"
Journal of Chemical Engineering of Japan
Vol. 9, No. 1, pp. 23–28, 1976
210
Tsuji, Y., Oshima, T., Morikawa, Y.
"Numerical Simulation of Pneumatic Conveying in a Horizontal Pipe"
KONA Powder Science and Technology in Japan
No. 3, pp. 38–51, 1985
211
Frank, Th.
"Parallele Algorithmen für die numerische Simulation dreidimensionaler, disperser
Mehrphasenströmungen und deren Anwendung in der Verfahrenstechnik"
Doctorial Dissertation, Shaker Verlag, 2002
212
Sommerfeld, M.
"Numerical Simulation of the Particle Dispersion in Turbulent Flow: the Importance of
Particle Lift Forces and Particle/Wall Collision Models"
ASME Symposium on Numerical Methods for Multiphase Flows, Toronto, Canada
pp. 1–8, 1990
213
B. P. Leonard,
”The ULTIMATE conservative difference scheme applied to unsteady one-dimensional
advection,”
Comp. Methods Appl. Mech. Eng.,
88:17–74, 1991
214
Jasak, H.; Weller, H.G., Gosman, A.D.
“High resolution NVD differencing scheme for arbitrarily unstructured meshes,”
Int. J. Numer. Meth. Fluids, 1999,
358
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
References 201 –
pp. 413 – 449.
215
Erdos, J.A.
“Numerical Solution of Periodic Transonic Flow through a Fan Stage”
AIAA Journal, 1977.
pp. 1559-1568.
216
Gerolymos G.A.
“Analysis and Application of Chorochronic Periodicity in Turbomachinery Rotor/Stator
Interaction Computations”
Journal of Propulsion and Power, 2002.
pp. 1139-1152.
217
Giles, M.
“Calculation of Unsteady Wake/Rotor Interaction”
J. Propulsion, 1988.
pp. 356-362.
218
He, L.
“An Euler Solution for Unsteady Flows Around Oscillating Blades”
Transactions of the ASME, 1990.
pp. 714-722.
219
Apsley, D.D. and Leschziner, M.A.
“A new low-reynolds-number nonlinear two-equation turbulence model for complex
flows”
International Journal of Heat and Fluid Flow, 19, pp. 209-222, 1998.
220
Coffee, T. P.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
359
Bibliography
“Comment on Simplified Reaction Mechanisms for the Oxidation of Hydrocarbon Fuels in
Flames by C. K. Westbrook and F. T. Dryer”
Combustion Science and Technology, 43, pp. 333–339, 1985.
221
Spalart, P. R., Deck, S., Shur, M. L., Squires, K. D., Strelets, M. Kh., Travin, A.
“A new version of detached-eddy simulation, resistant to ambiguous grid densities”
Theoretical and Computational Fluid Dynamics, vol. 20, pp. 181-195.
222
C. Temperton
“Implementation of a Self-Sorting In-Place Prime Factor FFT Algorithm”
Journal of Computational Physics, 58, pp. 283–299, 1985.
360
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Glossary
Symbols
<CFDPOSTROOT>
The directory in which CFD-Post is installed; for example: C:\Program
Files\ANSYS Inc\v162\CFD-Post\
<CFXROOT>
The directory in which CFX is installed; for example: C:\Program
Files\ANSYS Inc\v162\CFX\
A
absolute pressure
The summation of solver pressure, reference pressure, and hydro-static
pressure (if a buoyant flow) in the cavitation model. The absolute pressure
is clipped to be no less than the vapor pressure of the fluid. It is used by
the solver to calculate pressure-dependent properties (such as density
for compressible flow).
absorption coefficient
A property of a medium that measures the amount of thermal radiation
absorbed per unit length within the medium.
adaption criteria
The criteria that are used to determine where mesh adaption takes place.
adaption level
The degree that a mesh element has been refined during adaption. Each
mesh element has an adaption level. Each time an element is split into
smaller elements, the new elements have an adaption level that is one
greater than the "parent" element. The maximum number of adaption
levels is controlled to prevent over-refinement.
adaption step
One loop of the adapt-solve cycle in the mesh adaption process.
Additional Variable
A non-reacting, scalar component. Additional Variables are used to
model the distribution of passive materials in the flow, such as smoke in
air or dye in water.
Additional Variables are typically specified as concentrations.
adiabatic
The description of any system in which heat is prevented from crossing
the boundary of the system. You can set adiabatic boundary conditions
for heat transfer simulations in ANSYS CFX or in Fluent.
Advancing Front and Inflation (AFI)
The default meshing mode in CFX. The AFI mesher consists of a triangular
surface/tetrahedral volume mesh generator that uses the advancing front
method to discretize first the surface and then the volume into an unstructured (irregular) mesh. Inflation can be applied to selected surfaces
to produce prismatic elements from the triangular surface mesh, which
combine with the tetrahedra to form a hybrid mesh.
all domains
In immersed-solids cases in CFD-Post, "all domains" refers to all of the
domains in the case excluding the immersed solid. This is done for
backwards compatibility.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
361
Glossary
Generally speaking, only the wireframe needs to keep track of both
"all domains" and the immersed solid.
ASM (Algebraic Slip Model)
A mathematical form in which geometry may be represented, known as
parametric cubic.
aspect ratio
Also known as normalized shape ratio. A measure of how close to a
regular tetrahedron any tetrahedron is. The aspect ratio is 1 for a regular
tetrahedron, but gets smaller the flatter the tetrahedron gets. Used for
judging how good a mesh is.
B
backup file
An intermediate CFX-Solver Results file that can be manually generated
during the course of a solution from the CFX-Solver Manager interface
by using the Backup action button. Backup files should be generated if
you suspect your solution may be diverging and want to retain the intermediate solution from which you can do a restart.
batch mode
A way to run some components of ANSYS CFX without needing to open
windows to control the process. When running in batch mode, a Viewer
is not provided and you cannot enter commands at a command prompt.
Commands are issued via a CFD-Post session file (*.cse), the name of
which is specified when executing the command to start batch mode.
The session file can be created using a text editor, or, more easily, by
recording a session while running in line-interface or user-interface mode.
blend factor
A setting that controls the degree of first/second order blending for the
advection terms in discrete finite volume equations.
body
A collection of surfaces that completely and unambiguously enclose a
finite volume. Modelers that create so-called B-Rep models create "bodies."
This term was coined to distinguish between the tri-parametric entities,
known herein as solids, and the shell-like representations produced by
most CAD systems.
boundary
A surface or edge that limits the extent of a space. A boundary can be
internal (the surface of a submerged porous material) or external (the
surface of an airfoil).
boundary condition
Physical conditions at the edges of a region of interest that you must
specify in order to completely describe a simulation.
buoyant flow
Flow that is driven wholly or partially by differences in fluid density. For
fluids where density is not a function of temperature, pressure, or Additional Variables, the Boussinesq approximation is employed. If density is
a function of one of these, then the Full Buoyancy model is employed.
C
CEL (CFX Expression Language)
362
A high level language used within CFX to develop expressions for use in
your simulations. CEL can be used to apply user-defined fluid property
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
dependencies, boundary conditions, and initial values. Expressions can
be developed within CFX using the Expression Editor.
CFD (Computational Fluid
Dynamics)
The science of predicting fluid flow, heat transfer, mass transfer (as in
perspiration or dissolution), phase change (as in freezing or boiling),
chemical reaction (as in combustion), mechanical movement (as in fan
rotation), stress or deformation of related solid structures (such as a mast
bending in the wind), and related phenomena by solving the mathematical equations that govern these processes using a numerical algorithm
on a computer.
CFX-Solver Input file
A file that contains the specification for the whole simulation, including
the geometry, surface mesh, boundary conditions, fluid properties, solver
parameters and any initial values. It is created by CFX and used as input
to CFX-Solver.
CHT (Conjugate Heat
Transfer)
Heat transfer in a conducting solid.
clipping plane
A plane that is defined through the geometry of a model, in front of
which no geometry is drawn. This enables you to see parts of the geometry that would normally be hidden.
command actions
Command actions are:
• Statements in session files
• Commands entered into the Tools > Command Editor dialog box
• Commands entered in Line Interface mode.
All such actions must be preceded with the > symbol. These commands force CFD-Post to undertake specific tasks, usually related to
the input and output of data from the system. See also Power Syntax (p. 372).
component
A substance containing one or more materials in a fixed composition.
The properties of a component are calculated from the mass fractions
of the constituent materials and are based on the materials forming an
ideal mixture.
compressible flow
Flow in which the fluid volume changes in response to pressure change.
Compressible flow effects can be taken into consideration when the Mach
number (M) approaches approximately 0.2.
computational mesh
A collection of points representing the flow field where the equations of
fluid motion (and temperature, if relevant) are calculated.
control volume
The volume surrounding each node, defined by segments of the faces
of the elements associated with each node. The equations of fluid flow
are solved over each control volume.
convergence
A state of a solution that occurs when the change in residual values from
one iteration to the next are below defined limits.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
363
Glossary
corrected boundary node
values
Node values obtained by taking the results produced by CFX-Solver
(called "conservative values") and overwriting the results on the boundary
nodes with the specified boundary conditions.
The values of some variables on the boundary nodes (that is, on the
edges of the geometry) are not precisely equal to the specified
boundary conditions when CFX-Solver finishes its calculations. For
instance, the value of velocity on a node on the wall will not be
precisely zero, and the value of temperature on an inlet may not be
precisely the specified inlet temperature. For visualization purposes,
it can be more helpful if the nodes at the boundary do contain the
specified boundary conditions and so "corrected boundary node
values" are used. Corrected boundary node values are obtained by
taking the results produced by CFX-Solver (called "conservative values") and overwriting the results on the boundary nodes with the
specified boundary conditions. This will ensure the velocity is display
as zero on no-slip walls and equal to the specified inlet velocity on
the inlet, for example.
coupled solver
A solver in which all of the hydrodynamic equations are solved simultaneously as a single system. The advantages of a coupled solver are that
it is faster than a traditional solver and fewer iterations are required to
obtain a converged solution. CFX-Solver is an example of a coupled
solver.
curve
A general vector valued function of a single parametric variable. In CFX,
a line is also a curve. By default, curves are displayed in yellow in ANSYS
CFX.
D
default boundary condition
The boundary condition that is applied to all surfaces that have no
boundary condition explicitly set. Normally, this is set to the No Slip
Adiabatic Wall boundary condition, although you can change the type
of default boundary condition in CFX.
Detached Eddy Simulation
(DES)
A model that covers the boundary layer by a RANS model and switches
to a LES model in detached regions.
Direct Numerical Simulation
(DNS)
A CFD simulation in which the Navier-Stokes equations are solved without
any turbulence model.
discretization
The equations of fluid flow cannot be solved directly. Discretization is
the process by which the differential equations are converted into a
system of algebraic equations, which relate the value of a variable in a
control volume to the value in neighboring control volumes.
domain
Regions of fluid flow and/or heat transfer in CFX are called domains.
Fluid domains define a region of fluid flow, while solid domains are regions occupied by conducting solids in which volumetric sources of energy can be specified. The domain requires three specifications:
364
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
• The region defining the flow or conducting solid. A domain is formed
from one or more 3D primitives that constrain the region occupied by
the fluid and/or conducting solids.
• The physical nature of the flow. This determines the modeling of specific
features such as heat transfer or buoyancy.
• The properties of the materials in the region.
There can be many domains per model, with each domain defined
by separate 3D primitives. Multidomain problems may be created
from a single mesh if it contains multiple 3D primitives or is from
multiple meshes.
dynamic viscosity
Dynamic viscosity, also called absolute viscosity, is a measure of the resistance of a fluid to shearing forces.
dynamical time
For advection dominated flows, this is an approximate timescale for the
flow to move through the Domain. Setting the physical time step (p. 371)
size to this value (or a fraction of it) can promote faster convergence.
E
eddy viscosity model
A turbulence model based on the assumption that Reynolds stresses are
proportional to mean velocity gradients and that the Reynolds stress
contribution can be described by the addition of a turbulent component
of viscosity. An example of an eddy viscosity model is the k- model.
edge
The edge entity describes the topological relationships for a curve. Adjacent faces share at least one edge.
emissivity
A property of an object that describes how much radiation it emits as
compared to that of a black body at the same temperature.
expansion factor
The rate of growth of volume elements away from curved surfaces and
the rate of growth of surface elements away from curved boundaries.
Expansion factor is also used to specify the rate of mesh coarsening from
a mesh control.
expression editor
An interactive, form-driven facility within CFX for developing expressions.
external flow
A flow field that is located outside of your geometry.
F
face
“Face” can have several meanings:
• A solid face is a surface that exists as part of a solid. It is also known as
an implicit surface.
• An element face is one side of a mesh element.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
365
Glossary
• A boundary face is an element face that exists on the exterior boundary
of the domain.
• Surfaces composed of edges that are connected to each other.
FLEXlm
The program that administers ANSYS licensing.
flow boundaries
The surfaces bounding the flow field.
flow region
A volumetric space containing a fluid. Depending on the flow characteristics, you may have a single, uninterrupted flow region, or several flow
regions, each exhibiting different characteristics.
flow symmetry
Flow where the conditions of the flow entering and leaving one half of
a geometry are the same as the conditions of the flow entering and
leaving the other half of the geometry.
fluid
A substance that tends to flow and assumes the shape of its domain,
such as a gas in a duct or a liquid in a container.
free edges
Element edges belonging to only one element.
G
gas or liquid surface
A type of boundary that exhibits no friction and fluid cannot move
through it. Also called a symmetry boundary.
general fluid
A fluid whose properties may be generally prescribed in ANSYS CFX or
Fluent. Density and specific heat capacity for general fluids may depend
on pressure, temperature, and any Additional Variables.
global model tolerance
The minimum distance between two geometry entities below which CFX
considers them to be coincident. The default setting of global model
tolerance, defined in the template database, is normally .005 in whichever
geometry units you are working.
geometric symmetry
The state of a geometry where each half is a mirror of the other.
group
A named collection of geometric and mesh entities that can be posted
for display in viewports. The group's definition includes:
• Group name
• Group status (current/not current)
• Group display attributes (modified under Display menu)
• A list of the geometric and mesh entities that are members of the group.
366
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
H
hexahedral element
A mesh element with the same topology as a hexahedron, with six faces
and eight vertices.
home directory
The directory on all Linux systems and some Windows NT systems where
each user stores all of their files, and where various set-up files are stored.
However, on some Windows NT systems, users do not have an
equivalent to the Linux home directory. In this case, the ANSYS CFX
set-up file cfx5rc can be placed in c:\winnt\profiles\<user>\Application Data\ANSYS CFX\<release>,
where <user> is the user name on the machine. Other files can be
put into a directory set by the variable HOME.
I
ideal gas
A fluid whose properties obey the ideal gas law. The density is automatically computed using this relationship and a specified molecular weight.
IGES (Initial Graphics Exchange Specification) file
An ANSI standard formatted file used to exchange data among most
commercial CAD systems. IGES files can be imported into CFX.
implicit geometry
Geometry that exists as part of some other entity. For example, the edges
of a surface are implicit curves.
import mesh
A meshing mode that enables import of volume meshes generated in
one of a number of external CFD packages. The volume mesh can contain
hexahedral, tetrahedral, prismatic, and pyramidal element types.
inactive region
A fluid or porous region where flow and (if relevant) temperatures are
not being calculated, or a solid region where temperatures are not being
calculated. By default, inactive regions are hidden from view in the
graphics window.
incompressible flow
Flow in which the density is constant throughout the domain.
incremental adaption
The method of mesh adaption used by CFX where an existing mesh is
modified to meet specified criteria. Incremental adaption is much faster
than remeshing; however, the mesh quality is limited by that of the initial
mesh.
inertial resistance coefficients
Mathematical terms used to define porous media resistance.
initial guess
The values of dependent variables at the start of a steady-state simulation.
These can set explicitly, read from an existing solution, or given default
values.
initial values
The values of dependent variables at the initial time of a transient simulation. These can be either set explicitly, or read from an existing solution.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
367
Glossary
inlet boundary condition
A boundary condition (p. 362) for which the quantity of fluid flowing into
the flow domain is specified, for example, by setting the fluid velocity or
mass flow rate.
instancing
The process of copying an object and applying a positional transform to
each of the copies. For example, a row of turbine blades can be visualized
by applying instancing to a single blade.
interior boundary
A boundary that enables flow to enter and exit. These types of boundaries
are useful to separate two distinct fluid regions from each other, or to
separate a porous region from a fluid region, when you still want flow
to occur between the two regions.
internal flow
Flow through the interior of your geometry, such as flow through a pipe.
interpolation
The process of transferring a solution from a results file containing one
mesh onto a second file containing a different mesh.
isentropic
The description of a process where there is no heat transfer and entropy
is held constant.
isosurface
A surface of constant value for a given variable.
A three-dimensional surface that defines a single magnitude of a
flow variable such as temperature, pressure, velocity, and so on.
Isovolume
A locator that consists of a collection of volume elements, all of which
take a value of a variable greater than a user-specified value.
J
JPEG file
A common graphics file type that is supported by CFD-Post output options.
K
k-epsilon turbulence model
A turbulence model (p. 377) based on the concept that turbulence consists
of small eddies that are continuously forming and dissipating. The k-epsilon turbulence model solves two additional transport equations: one
for turbulence generation (k), and one for turbulence dissipation (epsilon).
kinematic diffusivity
A function of the fluid medium that describes how rapidly an Additional
Variable would move through the fluid in the absence of convection.
L
laminar flow
Flow that is dominated by viscous forces in the fluid, and characterized
by low Reynolds Number.
A flow field is laminar when the velocity distributions at various
points downstream of the fluid entrance are consistent with each
other and the fluid particles move in a parallel fashion to each other.
368
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
The velocity distributions are effectively layers of fluid moving at
different velocities relative to each other.
Large Eddy Simulation
Model (LES)
The Large Eddy Simulation model decomposes flow variables into large
and small scale parts. This model solves for large-scale fluctuating motions
and uses “sub-grid” scale turbulence models for the small-scale motion.
legend
A color key for any colored plot.
line interface mode
A mode in which you type the commands that would otherwise be issued
by the user interface. A viewer is provided that shows the geometry and
the objects created on the command line. Line interface mode differs
from entering commands in the Command Editor dialog box in that line
interface action commands are not preceded by a > symbol. Aside from
that difference, all commands that work for the Command Editor dialog
box will also work in line interface mode, providing the correct syntax is
used.
locator
A place or object upon which a plot can be drawn. Examples are planes
and points.
M
MAlt key (Meta key)
The MAlt key (or Meta key) is used to keyboard select menu items with
the use of mnemonics (the underscored letter in each menu label). By
simultaneously pressing the MAlt key and a mnemonic is an alternative
to using the mouse to click a menu title. The MAlt key is different for
different brands of keyboards. Some examples of MAlt keys include the
" " key for Sun Model Type 4 keyboards, the "Compose Character" key
for Tektronix keyboards, and the Alt key on most keyboards for most
Windows-based systems.
mass fraction
The ratio of the mass of a fluid component to the total mass of the fluid.
Values for mass fraction range from 0 to 1.
material
A substance with specified properties, such as density and viscosity.
meridional
A term used in Fluent documentation that is equivalent to the ANSYS
CFX term constant streamwise location.
mesh
A collection of points representing the flow field where the equations of
fluid motion (and temperature, if relevant) are calculated.
mesh adaption
The process by which, once or more during a run, the mesh is selectively
refined at various locations, depending on criteria that you can specify.
As the solution is calculated, the mesh can automatically be refined in
locations where solution variables are changed rapidly, in order to resolve
the features of the flow in these regions.
There are two general methods for performing mesh adaption. Incremental adaption takes an existing mesh and modifies it to meet the
adaption criteria. The alternative is remeshing, in which the whole
geometry is remeshed at every adaption step according to the adaption criteria. In CFX, incremental adaption is used because this is
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
369
Glossary
much faster; however, this imposes the limitation that the resulting
mesh quality is limited by the quality of the initial mesh.
mesh control
A refinement of the surface and volume mesh in specific regions of the
model. Mesh controls can take the form of a point, line, or triangle.
meshing mode
The method you use to create your mesh of nodes and elements required
for analysis. There are two main meshing modes:
• Advancing Front and Inflation (AFI) (p. 361)
• import mesh (p. 367)
minimal results file
A file that contains only the results for selected variables, and no mesh.
It can be created only for transient calculations. It is useful when you are
only interested in particular variables and want to minimize the size of
the results for the transient calculation.
multicomponent fluid
A fluid consisting of more than one component. The components are
assumed to be mixed at the molecular level, though the proportions of
each component may vary in space or time. The properties of a multicomponent fluid are dependent on the proportion of constituent components.
N
Navier-Stokes equations
The fundamental equations of fluid flow and heat transfer, solved by
CFX-Solver. They are partial differential equations.
new model preferences
Preferential settings for your model that define the meshing mode (p. 370),
the geometry units, and the global model tolerance (p. 366).
node allocation parameter
A parameter that is used in mesh adaption (p. 369) to determine how
many nodes are added to the mesh in each adaption step (p. 361).
non-clipped absolute pressure
The summation of solver pressure, reference pressure, and hydro-static
pressure (if a buoyant flow). This pressure, used by the solver to calculate
cavitation sources, can be negative or positive.
non-Newtonian fluid
A fluid that does not follow a simple linear relationship between shear
stress and shear strain.
normal
The direction perpendicular to the surface of a mesh element or geometry.
The positive direction is determined by the cross-product of the local
parametric directions in the surface.
O
open area
The area in a porous region that is open to flow.
OpenGL
A graphics display system that is used on a number of different types of
computer operating systems.
370
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
outlet
A boundary condition where the fluid is constrained to flow only out of
the domain.
outline plot
A plot showing the outline of the geometry. By setting the edge angle
to 0, the surface mesh can be displayed over the whole geometry.
output file
A text file produced by CFX-Solver that details the history of a run. It is
important to browse the output file when a run is finished to determine
whether the run has converged, and whether a restart is necessary.
P
parallel runs
Separate solutions of sections (partitions) of your CFD model, run on
more than one processor.
parametric equation
Any set of equations that express the coordinates of the points of a curve
as functions of one parameter, or express the coordinates of the points
of a surface as functions of two parameters, or express the coordinates
of the points of a solid as functions of three parameters.
parametric solids
Six-sided solids parameterized in three normalized directions. Parametric
solids are colored blue ANSYS CFX.
parametric surfaces
Four sided surfaces parameterized in two normalized directions. Parametric surfaces are colored green ANSYS CFX.
Particle-Particle Collision
Model (LPTM-PPCM)
A model in ANSYS CFX that takes inter-particle collisions and their effects
on the particle and gas phase into consideration.
periodic pair boundary
condition
A boundary condition where the values on the first surface specified are
mapped to the second surface. The mapping can be done either by a
translation or a rotation (if a rotating frame of reference is used).
physical time step
The time represented in each iteration of the solution.
pick list
The list processor interprets the contents of all selected data boxes. All
selected data boxes in CFX expect character strings as input. The character
strings may be supplied by the graphics system when you select an entity
from a viewport, or you can type or paste in the string directly. The
character strings are called "pick lists."
plot
Any means of viewing the results in CFD-Post. Types of plots include
vectors, streamlines, and contour plots.
point
An ordered n-tuple, where n is the number of dimensions of the space
in which the point resides.
point probes
Points placed at specific locations in a computational domain where data
can be analyzed.
polyline
A locator that consists of user-defined points.
postprocessor
The component used to analyze and present the results of the simulation.
For ANSYS CFX, the postprocessor is CFD-Post.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
371
Glossary
Power Syntax
The CFX Command Language (CCL) is the internal communication and
command language of CFD-Post. It is a simple language that can be used
to create objects or perform actions in the postprocessor. Power Syntax
enables you to embed Perl commands into CCL to achieve powerful
quantitative postprocessing.
Power Syntax programming uses the Perl programming language
to enable loops, logic, and custom macros (subroutines). A Line of
Power Syntax is identified in a .ccl file by an exclamation mark (!)
in the first column of a line. In between Perl lines, simple syntax
lines may refer to Perl variables and lists.
For details, see Power Syntax in ANSYS CFX (p. 311).
preprocessor
The component used to create the input for the solver. For ANSYS CFX,
the preprocessor is CFX-Pre.
pressure
In the cavitation model, pressure is the same as solver pressure, but
clipped such that the absolute pressure is non-negative. It is used for
postprocessing only.
prism or prismatic element
A 3D mesh element shaped like a triangular prism (with six vertices).
Sometimes known as a wedge element.
PVM (Parallel Virtual Machine)
The environment that controls parallel processes.
PVMHosts file
The database file containing information about where ANSYS CFX, and
consequently PVM, have been installed on each PVM node. It is consulted
when the Parallel Virtual Machine is started to determine where PVM is
located on each slave node.
pyramid element
A 3D mesh element that has five vertices.
R
reference coordinate frame
The coordinate frame in which the principal directions of X or Y or Z are
taken. X is taken in the local X of that frame, and so on. If the coordinate
frame is a non-rectangular coordinate frame, then the principal axes 1,
2, and 3 will be used to define the X, Y, and Z directions, respectively.
The default is CFX global system (Coord 0).
For domains, boundary conditions, and initial values, the reference
coordinate frame is always treated as Cartesian, irrespective of coordinate frame type.
region
An area comprised of a fluid, a solid material, or a porous material.
residuals
The change in the value of certain variables from one iteration to the
next.
The discretized Navier-Stokes equations (p. 370) are solved iteratively.
The residual for each equation gives a measure of how far the latest
solution is from the solution in the previous iteration. A solution is
372
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
considered to be converged when the residuals are below a certain
value.
CFX-Solver writes the residuals to the output file (p. 371) so that they
can be reviewed. Fluent allows residuals to be plotted during the
solution process.
results file (CFX-Solver Results file)
A file produced by CFX-Solver that contains the full definition of the
simulation as well as the values of all variables throughout the flow domain and the history of the run including residuals (p. 372). A CFX-Solver
Results file can be used as input to CFD-Post or as an input file to CFXSolver, in order to perform a restart.
Reynolds averaged NavierStokes (RANS) equations
Time-averaged equations of fluid motion that are primarily used with
turbulent flows.
Reynolds stress
The stress added to fluid flow due to the random fluctuations in fluid
momentum in turbulent flows. When the Navier-Stokes equations (p. 370)
are derived for time averaged turbulent flow to take into account the
effect of these fluctuations in velocity, the resulting equations have six
stress terms that do not appear in the laminar flow equations. These are
known as Reynolds stresses.
Reynolds stress turbulence
model
A model that solves transport equations for the individual Reynolds stress
components. It is particularly appropriate where strong flow curvature,
swirl, and separation are present. Reynolds stress models in general tend
to be less numerically robust than eddy viscosity models such as the kepsilon turbulence model (p. 368).
RNG k-epsilon turbulence
model
An alternative to the standard k-epsilon turbulence model (p. 368). It is
based on renormalization group analysis of the Navier-Stokes equations.
The transport equations for turbulence generation and dissipation are
the same as those for the standard k-epsilon model, but the model constants differ, and the constant C 1 is replaced by the function C 1RNG.
Rotating Frame of Reference (RFR)
A coordinate system that rotates. ANSYS CFX and Fluent can solve for
fluid flow in a geometry that is rotating around an axis at a fixed angular
velocity.
run
A process that requires the specification of the CFX-Solver input file (and
an initial values file, if necessary), and produces an output file and a results
file (if successful).
S
Sampling Plane
A locator that is planar and consists of equally-spaced points.
scalar variable
A variable that has only magnitude and not direction. Examples are
temperature, pressure, speed (the magnitude of the velocity vector), and
any component of a vector quantity.
Scale Adaptive Simulation
(SAS) model
A shear stress transport model used primarily for unsteady CFD simulations, where steady-state simulations are not of sufficient accuracy and
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
373
Glossary
do not properly describe the true nature of the physical phenomena.
Cases that may benefit from using the SAS-SST model include:
• Unsteady flow behind a car or in the strong mixing behind blades and
baffles inside stirred chemical reactors
• Unsteady cavitation inside a vortex core (fuel injection system) or a fluidstructure interaction (unsteady forces on bridges, wings, and so on).
For these problems and others, the SAS-SST model provides a more
accurate solution than URANS models, where steady-state simulations
are not of sufficient accuracy and do not properly describe the true
nature of the physical phenomena.
Second Moment Closure
models
Models that use seven transport equations for the independent Reynolds
stresses and one length (or related) scale; other models use two equations
for the two main turbulent scales.
session file (CFX)
A file that contains the records of all the actions in each interactive CFX
session. It has the extension .ses.
Shear Stress Transport (SST)
A
based SST model that accounts for the transport of the turbulent
shear stress and gives highly accurate predictions of the onset and the
amount of flow separation under adverse pressure gradients.
singleton (CCL object)
A singleton object that consists of an object type at the start of a line,
followed by a : (colon). Subsequent lines may define parameters and
child objects associated with this object. The object definition is terminated by the string END on a line by itself. The singleton object for a session file is declared like this:
SESSION:
Session Filename = <filename>.cse
END
The difference between a singleton object and a named object is
that after the data has been processed, a singleton can appear just
once as the child of a parent object. However, there may be several
instances of a named object of the same type defined with different
names.
slice plane
A locator that is planar, and that consists of all the points that intersect
the plane and the mesh edges.
solid
A material that does not flow when a force or stress is applied to it.
The general class of vector valued functions of three parametric
variables.
solid sub-domain
A region of the fluid domain that is occupied by a conducting solid.
ANSYS CFX can model heat transfer in such a solid; this is known as CHT
(Conjugate Heat Transfer) (p. 363).
solver
The component that solves the CFD problem, producing the required
results.
374
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
solver pressure
The pressure calculated by solving conservative equations; it can be
negative or positive. In the .out file it is called Pressure.
spanwise coordinate
A term used in Fluent documentation that is equivalent to the ANSYS
CFX term constant span.
specific heat
The ratio of the amount of heat energy supplied to a substance to its
corresponding change in temperature.
specific heat capacity
The amount of heat energy required to raise the temperature of a fixed
mass of a fluid by 1 K at constant pressure.
speed of sound
The velocity at which small amplitude pressure waves propagate through
a fluid.
sphere volume
A locator that consists of a collection of volume elements that are contained in or intersect a user-defined sphere.
state files
Files produced by CFD-Post that contain CCL commands. They differ from
session files in that only a snapshot of the current state is saved to a file.
You can also write your own state files using any text editor.
STP (Standard Temperature
and Pressure)
Defined as 0°C (273.15 K) and 1 atm (1.013x105 Pa).
steady-state simulation
A simulation that is carried out to determine the flow after it has settled
to a steady state. Note that, even with time constant boundary conditions,
some flows do not have a steady-state solution.
stream plot
A plot that shows the streamlines of a flow. Stream plots can be shown
as lines, tubes, or ribbons.
streamline
The path that a small, neutrally-buoyant particle would take through the
flow domain, assuming the displayed solution to be steady-state.
subdomains
Regions comprising a solid or set of solids, within the region of bounding
solids for a fluid domain, that enable the prescription of momentum and
energy sources. They can be used to model regions of flow resistance
and heat source.
subsonic flow
The movement of a fluid at a speed less than the speed of sound.
surface plot
A plot that colors a surface according to the values of a variable. Additionally, you can choose to display contours.
symmetry-plane boundary
condition
A boundary condition where all variables except velocity are mathematically symmetric and there can be no diffusion or flow across the
boundary. Velocity parallel to the boundary is also symmetric and velocity
normal to the boundary is zero.
T
template fluid
One of a list of standard fluids with predefined properties that you can
use 'as is', or use as a template to create a fluid with your own properties.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
375
Glossary
thermal conductivity
The property of a fluid that characterizes its ability to transfer heat by
conduction.
A property of a substance that indicates its ability to transfer thermal
energy between adjacent portions of the substance.
thermal expansivity
The property of a fluid that describes how a fluid expands as the result
of an increase in temperature. Also known as the coefficient of thermal
expansion, β.
theta
The angular coordinate measured about the axis of rotation following
the right-hand rule. When looking along the positive direction of the
axis of rotation, theta is increasing in the clockwise direction. Note that
the theta coordinate in CFD-Post does not increase over 360°, even for
spiral geometries that wrap to more than 360°.
topology
The shape, node, edge, and face numbering of an element.
tracers
Particles that follow a flow pathline. Used in viewing CFD results in order
to visualize the mechanics of the fluid flow.
transitions
Portions of a mesh that are the result of meshing geometry with two
opposing edges that have different mesh seeds. This produces an irregular mesh.
turbulence intensity
The ratio of the root-mean-square of the velocity fluctuations to the mean
flow velocity.
A turbulence intensity of 1% or less is generally considered low and
turbulence intensities greater than 10% are considered high. Ideally,
you will have a good estimate of the turbulence intensity at the inlet
boundary from external, measured data. For example, if you are
simulating a wind-tunnel experiment, the turbulence intensity in
the free stream is usually available from the tunnel characteristics.
In modern low-turbulence wind tunnels, the free-stream turbulence
intensity may be as low as 0.05%.
For internal flows, the turbulence intensity at the inlets is totally
dependent on the upstream history of the flow. If the flow upstream
is under-developed and undisturbed, you can use a low turbulence
intensity. If the flow is fully developed, the turbulence intensity may
be as high as a few percent.
turbulence length scale
A physical quantity related to the size of the large eddies that contain
the energy in turbulent flows.
In fully-developed duct flows, the turbulence length scale is restricted
by the size of the duct because the turbulent eddies cannot be larger
than the duct. An approximate relationship can be made between
the turbulence length scale and the physical size of the duct that,
while not ideal, can be applied to most situations.
If the turbulence derives its characteristic length from an obstacle
in the flow, such as a perforated plate, it is more appropriate to base
376
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
the turbulence length scale on the characteristic length of the
obstacle rather than on the duct size.
turbulence model
A model that predicts turbulent flow (p. 377). The available turbulence
models in ANSYS CFX are:
• k-epsilon turbulence model (p. 368)
• RNG k-epsilon turbulence model (p. 373)
• Reynolds stress turbulence model (p. 373)
• zero equation turbulence model (p. 379)
Turbulence models enable a steady-state representation of (inherently unsteady) turbulent flow to be obtained.
turbulent
A flow field that is irregular and chaotic look. In turbulent flow, a fluid
particle's velocity changes dramatically at any given point in the flow
field, in time, direction, and magnitude, making computational analysis
of the flow more challenging.
turbulent flow
Flow that is randomly unsteady over time. A characteristic of turbulent
flow is chaotic fluctuations in the local velocity.
V
variable
A quantity such as temperature or velocity for which results have been
calculated in a CFD calculation.
See also Additional Variable (p. 361).
vector plot
A plot that shows the direction of the flow at points in space, using arrows. Optionally, the size of the arrows may show the magnitude of the
velocity of the flow at that point. The vectors may also be colored according to the value of any variable.
verification
A check of the model for validity and correctness.
viewer area
The area of ANSYS CFX that contains the 3D Viewer, Table Viewer, Chart
Viewer, Comment Viewer, and Report Viewer, which you access from
tabs at the bottom of the area.
viewport (CFX)
An assigned, named, graphics window definition, stored in the CFX
database, that can be used to display selected portions of a model's
geometry, finite elements, and analysis results. The viewport's definition
includes:
• The viewport name
• The status of the viewport (posted or unposted; current or not current)
• Viewport display attributes
• A definition of the current view
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
377
Glossary
• A current group
• A list of the posted groups for display
• A graphics environment accessed from Display, Preference, and Group
menus that is common to all viewports.
There are the following types of CFX viewports:
current viewport
The viewport currently being displayed. The following actions can be
performed only on the current viewport:
• Changing the view by using the View menu or mouse.
• Posting titles and annotations by using the Display menu.
posted viewport
A viewport that has been selected for display.
target viewport
A viewport selected for a viewport modify action. Any viewport (including the current viewport) can be selected as the target viewport.
viscosity
The ratio of the tangential frictional force per unit area to the velocity
gradient perpendicular to the flow direction.
viscous resistance coefficients
A term to define porous media resistance.
Volume of Fluid (VOF)
method
A technique for tracking a fluid-fluid interface as it changes its topology.
W
wall
A generic term describing a stationary boundary through which flow
cannot pass.
workspace area
The area of CFX-Pre and CFD-Post that contains the Outline, Variables,
Expressions, Calculators, and Turbo workspaces, which you access from
the tabs at the top of the area. Each workspace has a tree view at the
top and an editor at the bottom (which is often called the details view).
See also CFD-Post Graphical Interface.
Y
y+ (YPLUS)
378
A non-dimensional parameter used to determine a specific distance from
a wall through the boundary layer to the center of the element at a wall
boundary.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Z
zero equation turbulence
model
A simple model that accounts for turbulence by using an algebraic
equation to calculate turbulence viscosity. This model is useful for obtaining quick, robust solutions for use as initial fields for simulations using
more sophisticated turbulence models.
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
379
380
Release 16.2 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information
of ANSYS, Inc. and its subsidiaries and affiliates.
Was this manual useful for you? yes no
Thank you for your participation!

* Your assessment is very important for improving the work of artificial intelligence, which forms the content of this project

Download PDF

advertisement