Fluent For Catia Tutorials 19.2

ANSYS Fluent for Catia Tutorials

ANSYS, Inc. Southpointe 2600 ANSYS Drive Canonsburg, PA 15317 [email protected] http://www.ansys.com (T) 724-746-3304 (F) 724-514-9494

Release 19.2 January 2019 ANSYS, Inc. and ANSYS Europe, Ltd. are UL registered ISO 9001: 2015 companies.

Copyright and Trademark Information © 2018 ANSYS, Inc. Unauthorized use, distribution or duplication is prohibited. ANSYS, ANSYS Workbench, AUTODYN, CFX, FLUENT 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 located 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. FLEXlm and FLEXnet are trademarks of Flexera Software LLC.

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. and ANSYS Europe, Ltd. are UL registered ISO 9001: 2015 companies.

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, contact ANSYS, Inc. Published in the U.S.A.

Table of Contents 1. Getting Started ....................................................................................................................................... 1 1.1. CATIA V5 Environment Settings ......................................................................................................... 1 1.2. FfC Settings ...................................................................................................................................... 6 2. Internal Flow Calculation ........................................................................................................................ 9 2.1. Introduction ..................................................................................................................................... 9 2.2. Prerequisites ..................................................................................................................................... 9 2.3. Problem Description ......................................................................................................................... 9 2.4. Preparation ..................................................................................................................................... 10 2.5. Setting the Options ......................................................................................................................... 10 2.6. Reading the File .............................................................................................................................. 15 2.7. Starting FLUENT for CATIA V5 .......................................................................................................... 15 2.8. Extracting Flow Volume .................................................................................................................. 15 2.9. Meshing Parameters ....................................................................................................................... 17 2.10. Materials ....................................................................................................................................... 18 2.11. Physics ......................................................................................................................................... 19 2.12. Boundary Conditions .................................................................................................................... 20 2.13. Solution ........................................................................................................................................ 22 2.14. Postprocessing ............................................................................................................................. 24 2.15. Update Results for Geometrical Change ......................................................................................... 29 2.16. Summary ...................................................................................................................................... 33 3. Porous Medium in an Air Filter .............................................................................................................. 35 3.1. Introduction ................................................................................................................................... 35 3.2. Prerequisites ................................................................................................................................... 35 3.3. Problem Description ....................................................................................................................... 35 3.4. Preparation ..................................................................................................................................... 36 3.5. Setting the Options ......................................................................................................................... 36 3.6. Reading the File .............................................................................................................................. 41 3.7. Starting FLUENT for CATIA V5 .......................................................................................................... 41 3.8. Extracting Flow Volume .................................................................................................................. 41 3.9. Materials ........................................................................................................................................ 42 3.10. Meshing Parameters ..................................................................................................................... 43 3.11. Physics ......................................................................................................................................... 46 3.12. Boundary Conditions .................................................................................................................... 47 3.13. Defining Porous Flow Properties .................................................................................................... 48 3.14. Solution ........................................................................................................................................ 51 3.15. Postprocessing ............................................................................................................................. 53 3.16. Summary ...................................................................................................................................... 57 3.17. Appendix A: Creating Planes for Splitting Geometry ....................................................................... 57 3.18. Appendix B: Splitting the Flow Volume .......................................................................................... 58 4. Internal Flow and Temperature Calculations in a Manifold .................................................................. 61 4.1. Introduction ................................................................................................................................... 61 4.2. Prerequisites ................................................................................................................................... 61 4.3. Problem Description ....................................................................................................................... 61 4.4. Preparation ..................................................................................................................................... 62 4.5. Setting the Options ......................................................................................................................... 62 4.6. Reading the File .............................................................................................................................. 67 4.7. Starting FLUENT for CATIA V5 .......................................................................................................... 67 4.8. Extracting Flow Volume .................................................................................................................. 67 4.9. Meshing Parameters ....................................................................................................................... 68 4.10. Physics ......................................................................................................................................... 71 Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

iii

Fluent for Catia Tutorials 4.11. Materials ....................................................................................................................................... 72 4.12. Boundary Conditions .................................................................................................................... 73 4.13. Solution ........................................................................................................................................ 75 4.14. Postprocessing ............................................................................................................................. 76 4.15. Finding Average Temperature at the Outlet ................................................................................... 78 4.16. Case 2: Considering Solid Material of Walls ..................................................................................... 80 4.16.1. Opening FLUENT for CATIA V5 Workbench ............................................................................ 80 4.16.2. Flow Volume ........................................................................................................................ 81 4.16.3. Meshing Parameters ............................................................................................................. 81 4.16.4. Physics ................................................................................................................................. 81 4.16.5. Materials .............................................................................................................................. 81 4.16.6. Boundary Conditions ............................................................................................................ 83 4.16.7. Solution ............................................................................................................................... 83 4.16.8. Postprocessing ..................................................................................................................... 84 4.17. Case 3: Transient Analysis Without Considering Solid Material ........................................................ 87 4.17.1. Opening FLUENT for CATIA V5 Workbench ............................................................................ 87 4.17.2. Flow Volume ........................................................................................................................ 88 4.17.3. Meshing Parameters ............................................................................................................. 88 4.17.4. Physics ................................................................................................................................. 89 4.17.5. Materials .............................................................................................................................. 89 4.17.6. Boundary Conditions ............................................................................................................ 90 4.17.7. Solution ............................................................................................................................... 93 4.17.8. Postprocessing ..................................................................................................................... 96 4.18. Summary .................................................................................................................................... 102 5. External Flow Calculations Over a Blimp ............................................................................................ 103 5.1. Introduction ................................................................................................................................. 103 5.2. Prerequisites ................................................................................................................................. 103 5.3. Problem Description ..................................................................................................................... 103 5.4. Preparation ................................................................................................................................... 104 5.5. Setting the Options ....................................................................................................................... 104 5.6. Reading the File ............................................................................................................................ 109 5.7. Creating the External Flow Domain ............................................................................................... 109 5.8. Starting FLUENT for CATIA V5 ........................................................................................................ 111 5.9. Extracting Flow Volume ................................................................................................................. 112 5.10. Physics ........................................................................................................................................ 112 5.11. Meshing Parameters ................................................................................................................... 113 5.12. Materials ..................................................................................................................................... 118 5.13. Boundary Conditions .................................................................................................................. 119 5.14. Mesh Generation ........................................................................................................................ 120 5.15. Solution ...................................................................................................................................... 123 5.16. Postprocessing ............................................................................................................................ 126 5.17. Summary .................................................................................................................................... 128 5.18. Appendix A: Displaying Contours of only the Blimp Surface .......................................................... 128 5.19. Appendix B: Displaying Velocity Path Lines ................................................................................... 129 6. Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model .............................. 131 6.1. Introduction ................................................................................................................................. 131 6.2. Prerequisites ................................................................................................................................. 131 6.3. Problem Description ..................................................................................................................... 132 6.4. Preparation ................................................................................................................................... 132 6.5. Setting the Options ....................................................................................................................... 132 6.6. Reading the File ............................................................................................................................ 137 6.7. Starting FLUENT for CATIA V5 ........................................................................................................ 137

iv

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Fluent for Catia Tutorials 6.8. Extracting Flow Volume ................................................................................................................. 137 6.9. Physics ......................................................................................................................................... 139 6.10. Meshing Parameters ................................................................................................................... 140 6.11. Materials ..................................................................................................................................... 141 6.12. Naming the Fluid Zones .............................................................................................................. 142 6.13. Specify the MRF Zone .................................................................................................................. 144 6.14. Solution ...................................................................................................................................... 147 6.15. Postprocessing ............................................................................................................................ 148 6.16. Summary .................................................................................................................................... 152 7. Compressible Flow Nozzle .................................................................................................................. 153 7.1. Introduction ................................................................................................................................. 153 7.2. Prerequisites ................................................................................................................................. 153 7.3. Problem Description ..................................................................................................................... 153 7.4. Preparation ................................................................................................................................... 154 7.5. Setting the Options ....................................................................................................................... 154 7.6. Reading the File ............................................................................................................................ 159 7.7. Starting FLUENT for CATIA V5 ........................................................................................................ 159 7.8. Extracting Flow Volume ................................................................................................................. 159 7.9. Meshing Parameters ..................................................................................................................... 162 7.10. Physics ........................................................................................................................................ 164 7.11. Materials ..................................................................................................................................... 164 7.12. Boundary Conditions .................................................................................................................. 165 7.13. Operating Conditions .................................................................................................................. 166 7.14. Journal Customization ................................................................................................................ 167 7.15. ANSYS Fluent Solution Settings ................................................................................................... 167 7.16. Solution ...................................................................................................................................... 169 7.17. Postprocessing ............................................................................................................................ 170 7.18. Summary .................................................................................................................................... 171 8. Volatile Gas Emission Modeling Using Species Transport Model ....................................................... 173 8.1. Introduction ................................................................................................................................. 173 8.2. Prerequisites ................................................................................................................................. 173 8.3. Problem Description ..................................................................................................................... 173 8.4. Preparation ................................................................................................................................... 174 8.5. Setting the Options ....................................................................................................................... 174 8.6. Reading the File ............................................................................................................................ 179 8.7. Starting FLUENT for CATIA V5 ........................................................................................................ 179 8.8. Extracting Flow Volume ................................................................................................................. 179 8.9. Meshing Parameters ..................................................................................................................... 182 8.10. Physics ........................................................................................................................................ 183 8.11. Materials ..................................................................................................................................... 184 8.12. Modifying Boundary Groups ....................................................................................................... 187 8.13. Boundary Conditions .................................................................................................................. 189 8.14. Operating Conditions .................................................................................................................. 192 8.15. ANSYS Fluent Solution Settings ................................................................................................... 192 8.16. Solution ...................................................................................................................................... 194 8.17. Postprocessing ............................................................................................................................ 194 8.18. Summary .................................................................................................................................... 202 9. Cavitation Model ................................................................................................................................. 205 9.1. Introduction ................................................................................................................................. 205 9.2. Prerequisites ................................................................................................................................. 205 9.3. Problem Description ..................................................................................................................... 205 9.4. Preparation ................................................................................................................................... 206 Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

v

Fluent for Catia Tutorials 9.5. Setting the Options ....................................................................................................................... 206 9.6. Reading the File ............................................................................................................................ 211 9.7. Physics ......................................................................................................................................... 211 9.8. Materials ....................................................................................................................................... 211 9.9. Boundary Conditions .................................................................................................................... 212 9.10. Meshing Parameters ................................................................................................................... 214 9.11. Cavitation Model Solution ........................................................................................................... 214 9.12. Postprocessing ............................................................................................................................ 218 9.13. Summary .................................................................................................................................... 223 9.14. Appendix .................................................................................................................................... 223 9.14.1. Reading the File .................................................................................................................. 223 9.14.2. Starting FLUENT for CATIA V5 .............................................................................................. 224 9.14.3. Extracting Flow Volume ...................................................................................................... 224 9.14.4. Modifying Boundary Groups ............................................................................................... 225 9.14.5. Mesh Settings .................................................................................................................... 226 9.14.6. Generating the Mesh .......................................................................................................... 231 10. Using Periodic Boundary Conditions ................................................................................................ 235 10.1. Introduction ............................................................................................................................... 235 10.2. Prerequisites ............................................................................................................................... 235 10.3. Problem Description ................................................................................................................... 235 10.4. Preparation ................................................................................................................................. 236 10.5. Setting the Options ..................................................................................................................... 236 10.6. Reading the File .......................................................................................................................... 241 10.7. Starting FLUENT for CATIA V5 ...................................................................................................... 241 10.8. Extracting Flow Volume ............................................................................................................... 241 10.9. Physics ........................................................................................................................................ 243 10.10. Meshing Parameters .................................................................................................................. 244 10.11. Materials ................................................................................................................................... 245 10.12. Create a Separate Group for Faces of the Shaft ........................................................................... 245 10.13. Naming the Fluid Zones ............................................................................................................ 247 10.14. Specify MRF Zone ...................................................................................................................... 248 10.15. Specify Periodic Zone ................................................................................................................ 251 10.16. Solver Settings .......................................................................................................................... 253 10.17. Perform Computation ............................................................................................................... 254 10.18. Save Management .................................................................................................................... 254 10.19. Postprocessing .......................................................................................................................... 255 10.20. Summary .................................................................................................................................. 262 11. Using Moving Mesh Model ................................................................................................................ 263 11.1. Introduction ............................................................................................................................... 263 11.2. Prerequisites ............................................................................................................................... 263 11.3. Problem Description ................................................................................................................... 263 11.4. Preparation ................................................................................................................................. 264 11.5. Setting the Options ..................................................................................................................... 264 11.6. Reading the File .......................................................................................................................... 269 11.7. Starting FLUENT for CATIA V5 ...................................................................................................... 269 11.8. Extracting Flow Volume ............................................................................................................... 269 11.9. Materials ..................................................................................................................................... 271 11.10. Meshing Parameters .................................................................................................................. 272 11.11. Physics ...................................................................................................................................... 273 11.12. Naming the Fluid Zones ............................................................................................................ 273 11.13. Renaming Groups ..................................................................................................................... 273 11.14. Specify MRF Zone ...................................................................................................................... 275

vi

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Fluent for Catia Tutorials 11.15. Specify Boundary Conditions ..................................................................................................... 276 11.16. Operating Conditions ................................................................................................................ 278 11.17. Solver Settings .......................................................................................................................... 278 11.18. Perform Computation ............................................................................................................... 279 11.19. Save Management .................................................................................................................... 280 11.20. Applying Moving Mesh ............................................................................................................. 280 11.21. Solution .................................................................................................................................... 282 11.22. Postprocessing .......................................................................................................................... 283 11.23. Summary .................................................................................................................................. 291 12. Simulation of Water Flow in a Bath Tub Using VOF Model ................................................................ 293 12.1. Introduction ............................................................................................................................... 293 12.2. Prerequisites ............................................................................................................................... 293 12.3. Problem Description ................................................................................................................... 293 12.4. Preparation ................................................................................................................................. 294 12.5. Setting the Options ..................................................................................................................... 294 12.6. Reading the File .......................................................................................................................... 299 12.7. Starting FLUENT for CATIA V5 ...................................................................................................... 299 12.8. Extracting Flow Volume ............................................................................................................... 299 12.9. Split Flow Volume ....................................................................................................................... 302 12.10. Meshing Parameters .................................................................................................................. 303 12.11. Physics ...................................................................................................................................... 305 12.12. Materials ................................................................................................................................... 306 12.13. VOF Specifications ..................................................................................................................... 307 12.14. Operating Conditions ................................................................................................................ 307 12.15. Specify Boundary Conditions ..................................................................................................... 308 12.16. Patch the Secondary Phase ........................................................................................................ 310 12.17. Unsteady Settings ..................................................................................................................... 310 12.18. Solver Settings .......................................................................................................................... 311 12.19. Save Management .................................................................................................................... 312 12.20. Perform Computation ............................................................................................................... 312 12.21. Postprocessing .......................................................................................................................... 312 12.22. Summary .................................................................................................................................. 315

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

vii

viii

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

List of Figures 1.1. CATIA V5 Product Structure Workbench .................................................................................................. 2 2.1. Problem Schematic ............................................................................................................................... 10 2.2. Options Dialog Box — General ............................................................................................................. 11 2.3. Options Dialog Box — Data Management ............................................................................................. 12 2.4. Options Dialog Box — Advanced Parameters ......................................................................................... 13 2.5. Options Dialog Box — Customization .................................................................................................... 14 2.6. Highlighted Inlet Face ........................................................................................................................... 16 2.7. Scaled Residuals ................................................................................................................................... 24 2.8. Contours of Total Pressure (Fringe) ........................................................................................................ 25 2.9. Total Pressure Fringe (Without Mesh) .................................................................................................... 26 2.10. Pressure and Velocity Image ................................................................................................................ 27 2.11. Viewing the Results on a Cut Plane ...................................................................................................... 29 3.1. Problem Schematic ............................................................................................................................... 36 3.2. Options Dialog Box — General ............................................................................................................. 37 3.3. Options Dialog Box — Data Management ............................................................................................. 38 3.4. Options Dialog Box — Advanced Parameters ......................................................................................... 39 3.5. Options Dialog Box — Customization .................................................................................................... 40 3.6. Highlighting the Flow Property and the Corresponding Zone ................................................................ 49 3.7. Selecting Face on Filter Region .............................................................................................................. 50 3.8. Measuring the Thickness of the Filter Region ......................................................................................... 50 3.9. Scaled Residuals ................................................................................................................................... 53 3.10. Pressure Contours (Without Mesh) ...................................................................................................... 55 3.11. Velocity Path Lines .............................................................................................................................. 56 3.12. Pressure Contours on Interior Planes ................................................................................................... 56 3.13. Velocity Contours on Interior Planes .................................................................................................... 57 3.14. Plane Definition Using Tangent to surface Option ................................................................................ 58 3.15. Selection of Planes for Splitting the Flow Volume ................................................................................. 59 3.16. Specification Tree after Volume Split .................................................................................................... 59 4.1. Problem Schematic ............................................................................................................................... 62 4.2. Options Dialog Box — General ............................................................................................................. 63 4.3. Options Dialog Box — Data Management ............................................................................................. 64 4.4. Options Dialog Box — Advanced Parameters ......................................................................................... 65 4.5. Options Dialog Box — Customization .................................................................................................... 66 4.6. Scaled Residuals ................................................................................................................................... 77 4.7. Contours of Static Temperature ............................................................................................................. 77 4.8. Contours of Velocity .............................................................................................................................. 78 4.9. Velocity Path Lines ................................................................................................................................ 78 4.10. Scaled Residuals ................................................................................................................................. 84 4.11. Temperature Contours ........................................................................................................................ 84 4.12. Temperature (fringe) Contours ............................................................................................................ 85 4.13.Temperature Contours at Wall-Fluid Interface ....................................................................................... 85 4.14. Setting Up the Cut Plane ..................................................................................................................... 86 4.15. Velocity Contours at Wall-Fluid Interface .............................................................................................. 87 4.16. Scaled Residuals ................................................................................................................................. 97 4.17. Surface Monitor Plot ........................................................................................................................... 97 4.18. Contours of Static Temperature at 0.08 s .............................................................................................. 99 4.19. Contours of Static Temperature at 0.15 s .............................................................................................. 99 4.20. Contours of Static Temperature at 0.175 s .......................................................................................... 100 4.21. Contours of Static Temperature at the Final Time Step ........................................................................ 100 4.22. Velocity (fringe) Distribution at the Final Step .................................................................................... 101 Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

ix

Fluent for Catia Tutorials 4.23. Velocity Vectors in a Cut Plane Passing Through Two Inlets ................................................................. 101 5.1. Blimp Geometry .................................................................................................................................. 104 5.2. Options Dialog Box — General ........................................................................................................... 105 5.3. Options Dialog Box — Data Management ........................................................................................... 106 5.4. Options Dialog Box — Advanced Parameters ....................................................................................... 107 5.5. Options Dialog Box — Customization .................................................................................................. 108 5.6. External Flow Domain Extents (Blimp Length is 143 Units) ................................................................... 110 5.7. External Flow Domain Extents (Rear View) ........................................................................................... 110 5.8. Blimp and External Flow Domain ......................................................................................................... 111 5.9. The Geometry and Surface mesh Tab Settings ..................................................................................... 114 5.10. Selection of Blimp Edges as Mesh Constraints .................................................................................... 116 5.11. Mesh at Blimp Extremities after Constraining Geometry ..................................................................... 117 5.12. Mesh at Blimp Extremities Without Constraining Geometry ................................................................ 117 5.13. Cutting Plane Through Mesh ............................................................................................................. 122 5.14. Zoomed-in View of Mesh Near Blimp Surface ..................................................................................... 122 5.15. Cells Display Based on Skewness Criteria ........................................................................................... 123 5.16. Residuals .......................................................................................................................................... 125 5.17. Drag Monitor .................................................................................................................................... 125 5.18. Contours of Total Pressure ................................................................................................................. 126 5.19. Setting the Cut Plane Position ........................................................................................................... 127 5.20. Contours of Velocity Vectors on a Cut Plane ....................................................................................... 127 5.21. Velocity Path Lines ............................................................................................................................ 128 6.1. Mixing Tank Schematic ........................................................................................................................ 132 6.2. Options Dialog Box — General ........................................................................................................... 133 6.3. Options Dialog Box — Data Management ........................................................................................... 134 6.4. Options Dialog Box — Advanced Parameters ....................................................................................... 135 6.5. Options Dialog Box — Customization .................................................................................................. 136 6.6. Flow Volume ....................................................................................................................................... 138 6.7. Groups ............................................................................................................................................... 139 6.8. Shaft-Rotating-Zone ........................................................................................................................... 143 6.9. Rotor-Blades ....................................................................................................................................... 143 6.10. Tank-Outer-Wall ................................................................................................................................ 144 6.11. Shaft-Not-Rotating-Zone ................................................................................................................... 144 6.12. Residual Plot ..................................................................................................................................... 148 6.13. Cut Plane Analysis Dialog Box ............................................................................................................ 150 6.14. Velocity Vectors ................................................................................................................................. 151 7.1. Problem Schematic ............................................................................................................................. 154 7.2. Options Dialog Box — General ........................................................................................................... 155 7.3. Options Dialog Box — Data Management ........................................................................................... 156 7.4. Options Dialog Box — Advanced Parameters ....................................................................................... 157 7.5. Options Dialog Box — Customization .................................................................................................. 158 7.6. Selected Inlet Edges ............................................................................................................................ 161 7.7. Selected Outlet Edges ......................................................................................................................... 161 7.8. Figure showing a Quadrant of Symmetry ............................................................................................. 162 7.9. Contours of Static Pressure .................................................................................................................. 170 7.10. Contours of Mach number ................................................................................................................. 171 8.1. Problem Schematic ............................................................................................................................. 174 8.2. Options Dialog Box — General ........................................................................................................... 175 8.3. Options Dialog Box — Data Management ........................................................................................... 176 8.4. Options Dialog Box — Advanced Parameters ....................................................................................... 177 8.5. Options Dialog Box — Customization .................................................................................................. 178 8.6. Selected Inner Surface of Ceiling ......................................................................................................... 180

x

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Fluent for Catia Tutorials 8.7. Selected Inlet Edges ............................................................................................................................ 181 8.8. Selected Outlet Edges ......................................................................................................................... 182 8.9. Specification Tree Updated for Benzene-air.1 ..................................................................................... 187 8.10. Report Showing the Solver Status ...................................................................................................... 195 8.11. Report Showing the Mass Flow Rate at All Boundaries ........................................................................ 195 8.12. Report Showing Image of Residuals ................................................................................................... 196 8.13. Pathlines of Mass Fraction of Benzene-vapor ...................................................................................... 197 8.14. Velocity Vectors on a Cutting Plane through the Door, Middle Vent, and the Opening .......................... 199 8.15. Velocity Vectors on a Cutting Plane through the Human Body ............................................................ 200 8.16. Contours of Mass Fraction of Benzene ............................................................................................... 201 8.17. Contours of Mass Fraction of Benzene Vapor on a Cutting Plane Through a Benzene Inlet ................... 202 8.18. Contours of Static Temperature ......................................................................................................... 202 9.1. Problem Schematic ............................................................................................................................. 206 9.2. Options Dialog Box — General ........................................................................................................... 207 9.3. Options Dialog Box — Data Management ........................................................................................... 208 9.4. Options Dialog Box — Advanced Parameters ....................................................................................... 209 9.5. Options Dialog Box — Customization .................................................................................................. 210 9.6. Mesh With Boundary Layers on Outlet Side .......................................................................................... 214 9.7. Scaled Residuals for Cavitation Model .................................................................................................. 218 9.8. Contours of Static Pressure on the Hydrofoil ........................................................................................ 219 9.9. Cut Plane view of Contours of Static Pressure ....................................................................................... 221 9.10. Contours of Volume Fraction of Primary Phase (Liquid Water) ............................................................. 222 9.11. Contours of Volume Fraction on Secondary Phase (Water Vapor) ........................................................ 222 9.12. Contours of Volume Fraction of Secondary Phase (region where cavitation has occurred) ................... 223 9.13. Figure Showing Mesh Parts for Advanced Meshing ............................................................................ 228 9.14. Selection of Trailing Edge of Hydrofoil ............................................................................................... 230 9.15. Figure Showing Entire Mesh .............................................................................................................. 232 9.16. Figure Showing Hydrofoil Mesh ......................................................................................................... 232 9.17. Zoomed View of the Hydrofoil Mesh .................................................................................................. 232 10.1. Mixing Tank Schematic ...................................................................................................................... 236 10.2. Options Dialog Box — General ......................................................................................................... 237 10.3. Options Dialog Box — Data Management .......................................................................................... 238 10.4. Options Dialog Box — Advanced Parameters ..................................................................................... 239 10.5. Options Dialog Box — Customization ................................................................................................ 240 10.6. Flow Volume ..................................................................................................................................... 242 10.7. Shaft-Rotating-Zone ......................................................................................................................... 246 10.8. Rotor-Blades ..................................................................................................................................... 246 10.9. Shaft-Not-Rotating-Zone ................................................................................................................... 247 10.10. Tank-Outer-Wall .............................................................................................................................. 247 10.11. Motion Direction ............................................................................................................................. 249 10.12. Periodic Zone .................................................................................................................................. 252 10.13. Periodic Point — Shading with Material ........................................................................................... 253 10.14. Periodic Point — Shading with Edges .............................................................................................. 253 10.15. Residual Plot ................................................................................................................................... 255 10.16. Cut Plane Analysis Dialog Box .......................................................................................................... 257 10.17. Velocity Vectors ............................................................................................................................... 258 10.18. Velocity Vectors without Periodic Repeats ........................................................................................ 260 10.19. Velocity Vectors with Periodic Repeats ............................................................................................. 261 10.20. Static Pressure on Rotor Blade ......................................................................................................... 262 11.1. Problem Schematic ........................................................................................................................... 264 11.2. Options Dialog Box — General ......................................................................................................... 265 11.3. Options Dialog Box — Data Management .......................................................................................... 266 Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

xi

Fluent for Catia Tutorials 11.4. Options Dialog Box — Advanced Parameters ..................................................................................... 267 11.5. Options Dialog Box — Customization ................................................................................................ 268 11.6. Flow Volume ..................................................................................................................................... 270 11.7. Fan-Blades ........................................................................................................................................ 274 11.8. Outer Wall ......................................................................................................................................... 274 11.9. Inlet .................................................................................................................................................. 274 11.10. Outlet ............................................................................................................................................. 275 11.11. Residual Plot ................................................................................................................................... 280 11.12. Residuals — Unsteady ..................................................................................................................... 284 11.13. Mass Flow Rate at Inlet .................................................................................................................... 284 11.14. Mass Weighted Total Pressure at Outlet ............................................................................................ 285 11.15. Static Pressure — Fan Blade ............................................................................................................. 286 11.16. Total Pressure — Fan Blade .............................................................................................................. 286 11.17. Total Pressure and Static Pressure .................................................................................................... 287 11.18. Velocity Vectors on fan-blade ......................................................................................................... 287 11.19. Turbulent Kinetic Energy Over Blades .............................................................................................. 288 11.20. Moving Mesh at Different Intervals .................................................................................................. 291 12.1. Problem Schematic ........................................................................................................................... 294 12.2. Options Dialog Box — General ......................................................................................................... 295 12.3. Options Dialog Box — Data Management .......................................................................................... 296 12.4. Options Dialog Box — Advanced Parameters ..................................................................................... 297 12.5. Options Dialog Box — Customization ................................................................................................ 298 12.6. Dry reference Surface Face Selection ................................................................................................. 300 12.7. Inlet Edges Selection ......................................................................................................................... 301 12.8. Outlet Edge Selection ........................................................................................................................ 301 12.9. Extracted Flow Volume ...................................................................................................................... 302 12.10. Split Flow Volumes .......................................................................................................................... 303 12.11. Residual Plot ................................................................................................................................... 312 12.12. Volume fraction at time step 4 ......................................................................................................... 313 12.13. Volume fraction at time step 12 ....................................................................................................... 313 12.14. Volume fraction at time step 20 ....................................................................................................... 313 12.15. Cut Plane Image of Velocity Contours at Time Step 20 ...................................................................... 314 12.16. Cut Plane Image of Velocity Vectors ................................................................................................. 315

xii

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

List of Tables 1.1. Useful Mouse Actions ............................................................................................................................. 5 3.1. Velocity vs Pressure Drop ...................................................................................................................... 36 5.1. Parameter Values ................................................................................................................................ 115 8.1. Boundary Group Names ...................................................................................................................... 187 9.1. Boundary Group Types ........................................................................................................................ 225

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

xiii

xiv

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 1: Getting Started This document will help you make some important settings before you can start working on any of the tutorials. In this document, you will learn how to: • Check whether the correct version of Service Pack and Hot Fix are installed. • Enable appropriate licenses. • Set the path to the documentation files. • Set the path to the locations where files will be saved.

1.1. CATIA V5 Environment Settings 1.

Start the FfC environment using one of the following ways: • Double-click the FLUENT for CATIA V5 icon created on your desktop during the installation. • Click the Windows Start menu. Select the Programs submenu, and the Fluent Inc Products program item, and the FLUENT for CATIA V5 R28 5.X.X sub item. Start → Programs → Fluent Inc Products → FLUENT for CATIA R28 5.X.X → FLUENT for CATIA R28 5.X.X Where, x represents the FfC release number, e.g., 20 for FfC 5.X.20. Depending on the name you provide during FfC installation, the submenus in the Programs list will change. When you start FLUENT for CATIA V5, one of the CATIA V5 workbenches opens. The current workbench is indicated by the icon at the top-right corner of the window shown in Figure 1.1: CATIA V5 Product Structure Workbench (p. 2).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

1

Getting Started Figure 1.1: CATIA V5 Product Structure Workbench

The following icons represent the respective workbenches: Icon

Workbench Product Structure Material Library CATIA V5, V4, V3, V2 Catalog Editor Part Design Assembly Design Sketcher Drafting Healing Assistant

2

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

CATIA V5 Environment Settings Icon

Workbench Wireframe and Surface Design Generative Shape Design Advanced Meshing Tools General Structural Analysis FfC Product Engineering Optimizer

2.

Check whether you have the correct version of Service Pack and Hot Fix installed. For details, see the Installation Guide. •

Open the About CATIA V5 dialog box. Help → About CATIA V5

3.

Ensure that the appropriate licenses are selected to run FLUENT for CATIA V5.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

3

Getting Started

a.

Select General below the Options feature (in the specification tree on the left-hand side of the dialog box).

b.

Click the Licensing tab. Enable the check-boxes for the following licenses in the List of Available Configurations or Products group box: • Necessary Licenses – MD2 (for geometry operations) – GPS (part structural analysis) • Optional/Useful Licenses – FMD (for volume meshing) – FMS (for surface meshing) – GAS (for analysis of assemblies) – EST (for advanced postprocessing operations)

4

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

CATIA V5 Environment Settings – PEO (for optimization)

Note – If you do not have FMS and FMD, certain meshing options will not be available (FMS+FMD). However, Octree 2D and 3D will be available by default. – If you make any changes to the license-related settings, restart FfC. This makes the new settings effective.

4.

5.

Ensure that Restrict external selection with link to published elements is disabled.

a.

Select Part Infrastructure in the specification tree.

b.

In the General tab, ensure that Restrict external selection with link to published elements is disabled.

If you are new to CATIA V5, the following mouse actions are useful while working with FLUENT for CATIA V5: Table 1.1: Useful Mouse Actions To ...

Do this ...

Zoom

Middle-click (hold) and right-click (release) Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

5

Getting Started To ...

Do this ...

Rotate

Middle-click (hold) and right-click (hold)

Move

Middle-click (hold)

1.2. FfC Settings Make the settings required to run FfC. If you are running FfC for the first time, configure some of the parameters in FfC using the Options dialog box before running the tutorial. Tools → Options 1.

6

Set the path to the FLUENT for CATIA V5 documentation so that you can access it while you work on tutorials.

a.

Select General below the Options feature (in the specification tree on the left-hand side of the dialog box).

b.

Select the Help tab.

c.

Click

to open the Path Selection dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

FfC Settings

d.

Select the following path using the directory tree in the left-hand side of the dialog box: FfC Installation/CAADoc The documentation files are stored at this location.

e.

Click OK to close the Path Selection dialog box.

Note To access the User's Guide help regarding any dialog box, open the dialog box and press the F1 key on your keyboard. This opens your web browser and the User's Guide page containing the relevant information.

2.

Specify the path to the ANSYS Fluent solver and the location to the directory where you want to save the analysis files. a.

Select Analysis & Simulation below the Options feature (in the specification tree on the left-hand side of the dialog box).

b.

Click the Fluent Options tab.

c.

In the General tab, specify the complete path to the ANSYS Fluent solver for Folder for solver. • for 32-bit: /FfC installation folder/solver/Fluent.Inc/ntbin/ntx86 • for 64-bit: /FfC installation folder/solver/Fluent.Inc/ntbin/win64 The ANSYS Fluent solver is installed automatically during FLUENT for CATIA V5 installation. When you start the simulation in FLUENT for CATIA V5, ANSYS Fluent runs in the background. Therefore, it is necessary to set the path to the location where the ANSYS Fluent solver is installed (Windows XP only).

d.

In the Data Management tab, specify the complete path to the directory where you want to store the temporary files for Temporary files:.

e.

Similarly set the path to the directory in the text entry field for FLUAnalysisComputations file: and FLUAnalysisResults file:. Set an appropriate path before starting any new tutorial (or any new CFD simulation). When you iterate the solution, FLUENT for CATIA V5 automatically saves all the solver-related files at this location. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

7

Getting Started f.

Enable Automatic renaming of FLUAnalysisResults and FLUAnalysisComputations files.

3.

In the General tab, select Maximum CPU Time or Maximum number of iterations from the Default criterion to stop steady state solver: drop-down list depending on your case setup.

4.

Enter the appropriate Maximum CPU Time (eg., 1e+07 s) or Maximum number of iterations (eg., 1000). FfC will use this default time (in seconds) as the maximum CPU allotment or the maximum number of iterations, while computing the solution.

5.

In the Advanced Parameters tab, ensure that the Mesh size multiplication factor is set to 1 in the Mesh group box.

6.

Check if you have the correct FfC version in the Fluent Options tab in the Options dialog box. a.

Select Analysis & Simulation in the specification tree.

b.

Click the Fluent Options tab.

c.

View the version at the bottom of the dialog box.

Note Refer to the FLUENT for CATIA V5 5.1 User's Guide for more information on the options explained in this document.

8

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 2: Internal Flow Calculation 2.1. Introduction This tutorial illustrates the setup and solution of a 3D fluid flow through a flier volume. The aim of this tutorial is to make you familiar with the FfC (FLUENT for CATIA V5) user interface. This tutorial demonstrates how to do the following: • Read an existing geometry into CATIA V5. • Launch the FLUENT for CATIA V5 environment. • Apply a material, specify the meshing parameters, and set the boundary conditions. • Initialize the mesh and the fluid flow calculations simultaneously. • Examine the results by performing postprocessing. • Update the result after making a geometrical change. • Generate a simulation report.

2.2. Prerequisites This tutorial assumes that you are familiar with the menu structure in CATIA V5 and that you have read the Getting Started (p. 1) portion of the Tutorial Guide.

Note It is assumed that you have the FMS and FMD licenses available. If you do not have FMD and FMS (CATIA V5) licenses then you will not be able to generate mesh as explained in the tutorial.

2.3. Problem Description The schematic of the problem is shown in Figure 2.1: Problem Schematic (p. 10). Pressure difference is maintained between the inlet and the outlet of the pipe because of which the air flows with a high velocity. A butterfly valve is fixed inside the flow volume. The air flow is assumed to be turbulent.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

9

Internal Flow Calculation Figure 2.1: Problem Schematic

2.4. Preparation 1.

Copy the CATIA V5 part file, flier_r18.CATPart to your working directory.

2.

Start the FfC environment.

2.5. Setting the Options Tools → Options → Analysis & Simulation → Fluent Options 1.

10

Click the General tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 2.2: Options Dialog Box — General

a.

Enter the path for the ANSYS Fluent solver in the text entry box next to Folder for solver.

Note The ANSYS Fluent solver is provided with the installed FfC package. You can use the Browse button to specify the path for the solver: For 32 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/ntx86 For 64 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/win64 Similarly, specify the path for the external postprocessor, CFD-Post (or FloWizard) executable.

b.

Set the remaining parameters as shown in Figure 2.2: Options Dialog Box — General (p. 11).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

11

Internal Flow Calculation 2.

Click the Data Management tab in the Options dialog box. Figure 2.3: Options Dialog Box — Data Management

a.

Enter the path for Temporary files, FLUAnalysisComputations file and FLUAnalysisResults file in the External Storage folder group box. You can use the Browse button to specify the path. The analysis files will be saved in the temporary folders while FfC is computing the solution. The analysis will be saved to its permanent location when the computation is complete.

b. 3.

12

Set the remaining parameters as shown in Figure 2.3: Options Dialog Box — Data Management (p. 12).

Click the Advanced Parameters tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 2.4: Options Dialog Box — Advanced Parameters

• 4.

Set the parameters as shown in Figure 2.4: Options Dialog Box — Advanced Parameters (p. 13).

Click the Customization tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

13

Internal Flow Calculation Figure 2.5: Options Dialog Box — Customization

a.

Enable Advanced Turbulence Models.

Note If the Advanced Turbulence Models option is disabled, then the default turbulence model (k-epsilon, Realizable) for turbulent flows and Reynolds Stress Model for turbulence with strong swirl will be selected without any further access to more turbulence models.

b.

Enable Advanced Boundary Condition Parameters.

Note The Advanced Boundary Condition Parameters option allows specification of heat generation rate for the wall boundary.

14

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Extracting Flow Volume c.

Enable Use solution steering by default.

Note The Use solution steering by default option enables the solution steering mechanism to control the solution convergence automatically.

d.

Enable Control "Solver Accuracy Settings" based on slider position of "Mesh Definition". For more information on the Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" control, refer to the FLUENT for CATIA V5 User's Guide.

5.

Click OK to close the Options dialog box.

2.6. Reading the File 1.

Read the CATIA V5 file (flier_r18.CATPart) in FLUENT for CATIA V5. File → Open... This opens the File Selection dialog box, using which you can select the file to be read.

2.

Select the file, flier_r18.CATPart. By default, the file is opened in the Part or Product workbench of CATIA V5.

Tip To use the entire screen space, remove the specification tree on the left-hand side by selecting the View → Specifications menu item or pressing the F3 key on your keyboard.

2.7. Starting FLUENT for CATIA V5 1.

Launch the FfC workbench. Start → Analysis & Simulation → FLUENT for CATIA V5 This updates the graphics display. The specification tree on the left-hand side also gets updated and displays the analysis-related parameters.

2.

In the Options dialog box, specify the location of the directory where you want to store the solver files.

2.8. Extracting Flow Volume In this step, you will define the inlet and outlet faces, and extract the flow volume. 1.

Click the icon or double-click the Geometry Definition.1 option located below the Environment.1 feature in the specification tree to open the Geometry Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

15

Internal Flow Calculation

2.

Select solid model from the Geometry definition drop-down list.

3.

Click on the field next to Inlet, zoom-in the inlet side of the geometry, and select the circular (annular) face at the inlet. When you move the pointer near the inlet, the faces around the pointer gets highlighted. Select the appropriate face as shown in Figure 2.6: Highlighted Inlet Face (p. 16). Figure 2.6: Highlighted Inlet Face

4.

Similarly, define the outlet solid face. See Figure 2.1: Problem Schematic (p. 10) to locate the outlet face.

5.

Click OK to validate. This creates a flow volume for the geometry. The flow volume is displayed in the graphics window. The specification tree on the left-hand side also gets updated to show relevant parameters.

16

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Meshing Parameters

2.9. Meshing Parameters 1.

Click the icon or double-click the Mesh Definition.1 option located below the Environment.1 feature in the specification tree to open the Mesh Definition dialog box.

2.

Click Reset All.

3.

Retain the default position of the slider bar at 50.

Note Some of the parameters in the Mesh Definition dialog box are linked to the position of the slider bar. Therefore, depending on the mesh type, moving the slider changes the values of such parameters.

4.

Use the default Optimized Surface mesher as the Mesh Type.

5.

Enter 1 mm for Critical length.

6.

Click the Surface Mesh tab, enable Automatic mesh capture, and enter a value of 1 mm.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

17

Internal Flow Calculation

7.

Click OK to validate.

2.10. Materials 1.

Click the

icon to open the Library dialog box.

2.

Select the FLUENT for CATIA V5 fluids and mixtures materials library. To open the materials library, you have to specify the path where it is stored. For 32 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\intel_a\startup\materials\Fluids and Mixtures.CATmaterial For 64 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\win_b64\startup\materials\Fluids and Mixtures.CATmaterial where X-X.X.X represents the version used.

18

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Physics

3.

In the Fluid tab, click the

icon (Air).

4.

Hold the mouse button, and drag and drop the material on to the flow volume in the graphics window. This includes the selected material (Air) in your case setup.

5.

Close the Library dialog box.

2.11. Physics 1.

Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the FLUENT for CATIA V5 specification tree in the Physical Model Definition dialog box.

2.

Disable Accounting for Temperature Effect.

3.

Select Turbulent in the Flow Type drop-down list.

4.

Select k-epsilon, Realizable in the Turbulence Model drop-down list.

5.

Click OK to validate.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

19

Internal Flow Calculation

2.12. Boundary Conditions 1.

Specify the inlet boundary conditions.

a.

Click the

icon to open the Inlet Boundary Condition dialog box.

Note There is a single inlet and outlet boundary in this example, hence they are automatically selected in the Supports field in the Boundary Condition dialog boxes.

2.

20

b.

Ensure that 1 Inlet boundary is selected for Supports.

c.

Enable Gauge Pressure (Total) and set the value to 500 N_m2.

d.

Click OK to validate.

Specify the outlet boundary conditions.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Boundary Conditions

3.

4.

a.

Click the

icon to open the Outlet Boundary Condition dialog box.

b.

Ensure that 1 Outlet boundary is selected for Supports.

c.

Enable Gauge Pressure (Static) and set the value to 0 N_m2.

d.

Click OK to validate.

Specify the wall boundary conditions.

a.

Click the

icon.

b.

Ensure that 1 Wall boundary is selected for Supports.

c.

Keep the default settings and click OK to validate.

Save the CATIA V5 analysis files. File → Save Management...

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

21

Internal Flow Calculation

a.

Select the Analysis1.CATAnalysis file and click the Save As... button.

b.

Rename the Analysis1.CATAnalysis file to flier_Analysis1.CATanalysis.

c.

Click the Propagate directory button and then click OK to close the Save Management dialog box.

Note You specify the path where all the analysis files are saved. Using Save Management... saves the analysis file along with other solution files written by FfC.

2.13. Solution In this step, you will generate the mesh and iterate the solution. Though FfC allows you to generate the mesh and start the flow computations separately, here you will perform these steps simultaneously. 1.

22

Initialize the solution from the inlet. a.

Double-click on Initialization Values.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Initialization Values dialog box.

b.

Click Reset All.

c.

Click on the Compute From field and select Inlet.1 below the Boundary Conditions.1 feature in the specification tree.

d.

Click OK to validate.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Solution 2.

3.

Double-click on Fluent Solution.1 below the Fluent case feature in the specification tree to open the Fluent Solution dialog box.

a.

Click the Reset All button to restore the default settings.

b.

Ensure that Residuals + Fluxes&Delta option is selected as the Convergence Criterion.

c.

Ensure that Use solution steering is enabled.

d.

Ensure that Maximum CPU Time is enabled and enter 30000s.

e.

Click OK to validate.

Click the

icon to open the Compute dialog box.

a.

Select All and Default Solution Options in the two drop-down lists available.

b.

Click OK in the Compute dialog box to launch the computations.

c.

Click Stop Computation if you want to interrupt the calculations.

The solution should converge in approximately 160 iterations.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

23

Internal Flow Calculation

2.14. Postprocessing 1.

Click the

icon to display the scaled residuals (Figure 2.7: Scaled Residuals (p. 24)).

Figure 2.7: Scaled Residuals

2.

Display the contours of total pressure (fringe). a.

Click the

icon.

Note The images created during the postprocessing are listed under the Fluent Solution.1 option in the specification tree.

Double-click on the image label of your interest and edit its definition using the Image Edition dialog box.

b.

24

Double-click on Total Pressure in the Fluent Solution set to open the Image Edition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing c.

Select Fringe in the Type list, and click OK to validate. The FLUENT for CATIA V5 display gets updated and shows the total pressure plot (Figure 2.8: Contours of Total Pressure (Fringe) (p. 25)). Figure 2.8: Contours of Total Pressure (Fringe)

d.

Click the

icon.

This disables the mesh display imprint from the postprocessing image. Only the contours of pressure over the domain are displayed (Figure 2.9: Total Pressure Fringe (Without Mesh) (p. 26)).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

25

Internal Flow Calculation Figure 2.9: Total Pressure Fringe (Without Mesh)

3.

Display the contours of velocity (symbol) along with total pressure (Figure 2.10: Pressure and Velocity Image (p. 27)).

a.

Click the

icon.

Note Ensure that the velocity vector (symbol) image is already displayed. If not, select Symbol in the Visu tab in the Image Edition dialog box. To move the colormap, position the cursor on the color-map and click the left mouse button. Then drag the color-map to a suitable position. FLUENT for CATIA V5 display updates and the velocity vector plot is updated. The velocity image is superimposed on the pressure image. The color-bands are also not placed properly.

b.

Place both the images at an appropriate distance. Ensure that both the postprocessing images are active and are displayed in the graphics window. i.

26

Click the

icon to open the Images Layout dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing

ii.

Specify the parameters as shown in the dialog box and click OK to validate. This will place both the postprocessing images at some distance from each other and you can view each image individually (Figure 2.10: Pressure and Velocity Image (p. 27)). You may have to move the color-bands to appropriate positions manually.

Figure 2.10: Pressure and Velocity Image

4.

Right-click on the Total pressure (fringe.1) option located below the Fluent Solution.1 set and select Activate/Deactivate in the contextual menu.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

27

Internal Flow Calculation This deactivates the pressure image.

Note If the On boundary option is already disabled then do not perform the next step.

5.

Double-click the color map of velocity image to open the Color Map Edition dialog box.

6.

Disable On boundary and click OK. This displays the velocity vectors throughout the domain, instead of displaying them only on the boundaries.

7.

View the velocity image on a cut plane. a.

Click the

icon to open the Cut Plane Analysis dialog box.

A cut plane passing through the geometry is also displayed.

b.

Adjust the position of the plane (Figure 2.11: Viewing the Results on a Cut Plane (p. 29)) using the compass (

28

) in the graphics window.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Update Results for Geometrical Change Figure 2.11: Viewing the Results on a Cut Plane

8.

Save the session. File → Save Management This allows you to save the files modified during the two save commands. For details, see the FLUENT for CATIA V5 User's Guide.

2.15. Update Results for Geometrical Change In this step, you will change the angle of the valve and update the results for new valve position. Do not change any other parameter. 1.

Enable Parameters, in Options dialog box. Tools → Options → Infrastructure → Part Infrastructure → Display

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

29

Internal Flow Calculation

2.

Select flier_r18.CATPart in the Window pull-down menu. Window → 1 flier_r18.Part

3.

Double-click on the Angle.1 option below the Parameters feature in the specification tree to open the Edit Parameter dialog box.

4.

Change the angle to 55deg.

5.

Click OK to validate.

30

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Update Results for Geometrical Change

6.

Enter the FLUENT for CATIA V5 workbench and select the flier_Analysis1.CATanalysis file. Window → flier_Analysis1.CATanalysis

7.

Right-click on the Fluent Solution.1 option and select Local Update in the contextual menu.

This re-generates the mesh and computes the case again for the new valve position. The postprocessing data also gets updated for the new valve position. 8.

To activate the velocity image display, right-click on the velocity vector.1 located below Fluent Solution.1 and select Activate/Deactivate in the contextual menu.

Tip If the arrows in the velocity image are too small, change their size. To do so, perform the following: 1. Right-click velocity vector.1 located below Fluent Solution.1. Select velocity vector.1 object and Definition in the contextual menu to open the Image Edition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

31

Internal Flow Calculation 2. Click the Options button to open the Visualization Options dialog box.

3. Increase the Size parameters to appropriate values.

9.

Save this updated solution in a new folder.

Note This is important otherwise the previous solution will be overwritten and the files will be corrupted if the file is saved in the same folder.

10. Generate the report of the simulation. a.

Click the

icon to open the Report Generation dialog box.

b.

Specify the appropriate path to the directory where you want FLUENT for CATIA V5 to save the simulation report. This opens the web browser and displays the report page. A report is a summary of the simulation you have performed. It reports information about the mesh details, flow physics, boundary conditions, and results. For more details, refer to Volatile Gas Emission Modeling Using Species Transport Model (p. 173).

32

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Summary

2.16. Summary In this tutorial you learned how to start the FfC environment, create the flow volume using the geometry, specify basic meshing parameters, apply material to your case setup, and set the boundary conditions for the problem. You also learned how to start the calculations and perform the postprocessing. Some of the basic settings required to run FLUENT for CATIA V5 for the first time were also discussed.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

33

34

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 3: Porous Medium in an Air Filter 3.1. Introduction This tutorial illustrates the setup and solution of a 3D turbulent fluid flow in an air filter. This tutorial demonstrates how to do the following: This tutorial demonstrates how to do the following: • Separate the air filter zone by using planes created in CATIA V5 part workbench. • Use velocity and pressure drop data for the filter to provide porous media inputs. • Set convergence criteria. • Use monitors to determine mass flow rate at outlet, pressures across the filter element. • Examine the velocity and pressure distribution across the filter element through contour plots • Display pathlines. • Analyze results.

3.2. Prerequisites This tutorial assumes that you are familiar with the menu structure in FfC. It also assumes that you have read the Getting Started (p. 1) portion of the Tutorial Guide and completed Internal Flow Calculation (p. 9). Some of the steps in setup and solution procedure will not be shown explicitly.

Note It is assumed that you have the FMS and FMD licenses available. If you do not have FMD and FMS (CATIA V5) licenses then you will not be able to generate mesh as explained in the tutorial.

3.3. Problem Description The air filter considered in this tutorial is used in air induction systems in automobiles. The flow pattern in the air filter, pressure drop across the filter element and uniformity of the flow in the filter element are important aspects of study. The filter element can be modeled as porous media zones in FfC. For filter elements, normally the flow and pressure drop characteristics are known. This data can be used to define porous media input parameters. The schematic of the problem is shown in Figure 3.1: Problem Schematic (p. 36). Air enters the air filter at 0.208 kg/sec from inlet. The flow is assumed to be turbulent.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

35

Porous Medium in an Air Filter Figure 3.1: Problem Schematic

The experimental values of velocity vs. pressure drop across the filter element is found to be as follows: Table 3.1: Velocity vs Pressure Drop x (m/s)

y (Pa)

2.0685

133

3.1

249

4.15

390

5.18

598

6.21996

797

The objective of the simulation is to determine: 1. Pressure drop across the filter element. 2. Flow distribution in the filter element.

3.4. Preparation 1.

Copy the CATIA V5 part file, air-filter-tutorial-final.CATPart to your working directory.

2.

Start the FfC environment.

3.5. Setting the Options Tools → Options → Analysis & Simulation → Fluent Options 1.

36

Click the General tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options a.

Enter the path for the ANSYS Fluent solver in the text entry box next to Folder for solver.

Note The ANSYS Fluent solver is provided with the installed FfC package. You can use the Browse button to specify the path for the solver: Figure 3.2: Options Dialog Box — General

For 32 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/ntx86 For 64 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/win64 Similarly, specify the path for the external postprocessor, CFD-Post (or FloWizard) executable.

b. 2.

Set the remaining parameters as shown in Figure 3.2: Options Dialog Box — General (p. 37).

Click the Data Management tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

37

Porous Medium in an Air Filter Figure 3.3: Options Dialog Box — Data Management

a.

Enter the path for Temporary files, FLUAnalysisComputations file and FLUAnalysisResults file in the External Storage folder group box. You can use the Browse button to specify the path. The analysis files will be saved in the temporary folders while FfC is computing the solution. The analysis will be saved to its permanent location when the computation is complete.

b. 3.

38

Set the remaining parameters as shown in Figure 3.3: Options Dialog Box — Data Management (p. 38).

Click the Advanced Parameters tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 3.4: Options Dialog Box — Advanced Parameters

• 4.

Set the parameters as shown in Figure 3.4: Options Dialog Box — Advanced Parameters (p. 39).

Click the Customization tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

39

Porous Medium in an Air Filter Figure 3.5: Options Dialog Box — Customization

a.

Enable Advanced Turbulence Models.

Note If the Advanced Turbulence Models option is disabled, then the default turbulence model (k-epsilon, Realizable) for turbulent flows and Reynolds Stress Model for turbulence with strong swirl will be selected without any further access to more turbulence models.

b.

Enable Advanced Boundary Condition Parameters.

Note The Advanced Boundary Condition Parameters option allows specification of heat generation rate for wall boundary.

c.

Enable Use solution steering by default.

Note The Use solution steering by default option enables solution steering mechanism to control the solution convergence automatically.

40

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Extracting Flow Volume d.

Enable Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" . For more information on the Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" control, refer to the FLUENT for CATIA V5 User's Guide.

5.

Click OK to close the Options dialog box.

3.6. Reading the File 1.

Read the CATIA V5 file (air-filter-tutorial-final.CATPart) in FLUENT for CATIA V5. File → Open... This opens the File Selection dialog box, using which you can select the file to be read.

2.

Select the file, air-filter-tutorial-final.CATPart. By default, the file is opened in the Part or Product workbench of CATIA V5.

Tip To use the entire screen space, remove the specification tree on the left-hand side by selecting the View → Specifications menu item or pressing the F3 key on your keyboard.

3.7. Starting FLUENT for CATIA V5 •

Launch the FfC workbench. Start → Analysis & Simulation → FLUENT for CATIA V5 This updates the graphics display. The specification tree on the left-hand side also gets updated and displays the analysis-related parameters.

3.8. Extracting Flow Volume In this step, you will define the inlet and outlet faces, and extract the flow volume. 1.

Click the icon or double-click the Geometry Definition.1 option located below the Environment.1 feature in the specification tree to open the Geometry Definition dialog box.

2.

Select flow volume from the Geometry definition drop-down list. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

41

Porous Medium in an Air Filter 3.

Click on the field next to Inlet, zoom-in the inlet side of the geometry, and select the circular (annular) face at the inlet. When you move the pointer near the inlet, the faces around the pointer gets highlighted. Select the appropriate face as shown in Figure 3.1: Problem Schematic (p. 36).

4.

Similarly, define the outlet solid face. See Figure 3.1: Problem Schematic (p. 36) to locate the outlet face.

5.

Click OK to validate. This creates a flow volume for the geometry. The flow volume is displayed in the graphics window. The specification tree on the left-hand side also gets updated to show relevant parameters.

3.9. Materials 1.

Click the

icon to open the Library dialog box.

2.

Select the FLUENT for CATIA V5 fluids and mixtures materials library. To open the materials library, you have to specify the path where it is stored. For 32 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\intel_a\startup\materials\Fluids and Mixtures.CATmaterial For 64 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\win_b64\startup\materials\Fluids and Mixtures.CATmaterial where X-X.X.X represents the version used.

42

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Meshing Parameters

3.

Drag and drop the in the graphics window.

4.

Close the Library dialog box.

icon (Air) in the Library (Read Only) dialog box on to the flow volumes

3.10. Meshing Parameters 1.

Click the icon or double-click the Mesh Definition.1 option located below the Environment.1 feature in the specification tree to open the Mesh Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

43

Porous Medium in an Air Filter

a.

Click Reset All.

b.

Retain the default position of the slider bar at 50.

Note Some of the parameters in the Mesh Definition dialog box are linked to the position of the slider bar. Therefore, depending on the mesh type, moving the slider changes the values of such parameters.

44

c.

Use the default Optimized Surface mesher as the Mesh Type.

d.

Enable Critical length and set the value to 2 mm.

e.

Set the Mesh size to 20 mm.

f.

Click the Surface Mesh tab and disable Use Relative sag.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Meshing Parameters

g.

Enable Growth rate and retain the default value of 1.2.

h.

Click the Volume mesh tab and retain the default values.

i.

Click OK to validate.

2.

Compute the mesh.

3.

Click the

icon to open the Quality Analysis dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

45

Porous Medium in an Air Filter

The quality analysis is done to check the skewness of the mesh. 4.

Enable Skewness and disable all other options.

5.

Click Apply.

6.

Click the

icon to open the Quality Report dialog box.

The maximum skewness is approximately 0.94 and the mesh count is approximately 100 k.

Note The mesh count and maximum skewness may differ slightly depending on the architecture. However maximum skewness should be approximately around or less than 0.95.

3.11. Physics 1.

46

Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the FLUENT for CATIA V5 specification tree in the Physical Model Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Boundary Conditions

2.

Disable Accounting for Temperature Effect.

3.

Select Turbulent in the Flow Type drop-down list.

4.

Select k-epsilon, Realizable in the Turbulence Model drop-down list.

5.

Select steady from the Time drop-down list.

6.

Click OK to validate.

3.12. Boundary Conditions 1.

Specify the inlet boundary conditions. a.

Click the

icon to open the Inlet Boundary Condition dialog box.

Note There is a single inlet and outlet boundary in this example, hence they are automatically selected in the Supports field in Boundary Condition dialog boxes.

b.

Ensure that 1 Inlet boundary is selected for Supports.

c.

Enable Mass Flow Rate and enter a value of 0.208 kg_s. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

47

Porous Medium in an Air Filter

2.

d.

Select External Environment from the Source of Flow drop-down list.

e.

Click OK to validate.

Specify the outlet boundary conditions. a.

Click the

icon to open the Outlet Boundary Condition dialog box.

b.

Ensure that 1 Outlet boundary is selected for Supports.

c.

Enable Gauge Pressure (static) and set the value to 0 N_m2.

d.

Select External Environment from the Downstream conditions drop-down list.

e.

Click OK to validate.

3.13. Defining Porous Flow Properties 1.

48

Use the

icon to find the flow property corresponding to the filter zone.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Defining Porous Flow Properties Figure 3.6: Highlighting the Flow Property and the Corresponding Zone

Check the flow property for the filter, in the specification tree. In this case it is Flow Property.3 (Figure 3.6: Highlighting the Flow Property and the Corresponding Zone (p. 49)).

Note The central zone should be selected as the filter.

2.

Double-click Flow Property.3 to open the Flow Property Definition dialog box.

a.

Rename Flow Property.3 to filter in the Name text-entry box.

b.

Select Yes from the Porous Property drop-down list.

c.

Click the

icon to open the Porous Property Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

49

Porous Medium in an Air Filter Figure 3.7: Selecting Face on Filter Region

i.

Enable Velocity and Pressure Drop Data input method.

ii.

Select a face on the filter zone perpendicular to the flow as the surface for Support for direction calculation (Figure 3.7: Selecting Face on Filter Region (p. 50)). To perform this operation, you have to hide the zone next to the filter.

Note Based on this surface, FfC determines the flow direction which is updated in the direction field.

iii.

Enable Porous region thickness and enter a value of 42.5 mm.

Click the icon to open the Measure Between dialog box to find the thickness of the filter region (Figure 3.8: Measuring the Thickness of the Filter Region (p. 50)). Figure 3.8: Measuring the Thickness of the Filter Region

Note Selection of the Support for Direction specification also automatically updates Porous Region Thickness. However you can overwrite the calculated value as explained above.

50

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Solution iv.

Enable Data Mapping for Velocity and Pressure.

v.

Click the Browse button to open the File Selection dialog box.

A.

Select the file v-vs-pdrop.xls and click Open. The field below Data Mapping for Velocity and Pressure is updated with the path of the spreadsheet file.

vi. d.

B.

Click Show in the Porous Property Definition dialog box to verify the input data in the Imported Table dialog box.

C.

Close the Imported Table dialog box.

Click OK to close the Porous Property Definition dialog box.

Click OK to close the Flow Property Definition dialog box.

3.14. Solution In this step, you will define monitors, generate the mesh, and iterate the solution. Though FLUENT for CATIA V5 allows you to generate the mesh and start the flow computations separately, here you will perform these steps simultaneously.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

51

Porous Medium in an Air Filter 1.

Double-click on Initialization Values.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Initialization Values dialog box. •

2.

3.

4.

Click Reset All and OK to validate.

Double-click on Fluent Solution.1 below the Fluent case feature in the specification tree to open the Fluent Solution dialog box. a.

Click Reset All.

b.

Ensure that Residuals + Fluxes&Delta option is selected as the Convergence Criterion.

c.

Click OK to validate.

Define a surface monitor for mass flow rate at outlet. a.

Right-click on Monitors.1 in the Fluent Solution.1 set in the specification tree.

b.

Select Surface Monitor from the contextual menu to open the Surface Monitor dialog box.

i.

Select the outlet boundary below the Groups.1 feature in the specification tree as the support.

ii.

Select Mass Flow Rate as the report type and click OK.

Similarly, define mass-weighted average pressure monitors at the filter inlet and filter outlet faces. The monitors will appear in the Monitors.1 list below Fluent Case feature in the specification tree.

5.

Save the analysis file and propagate the directory to save all the files together. File → Save Management...

6.

Click the

a. 52

icon to open the Compute dialog box.

Select All and Default Solution Options from the two drop-down lists available. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing b.

Click OK in the Compute dialog box to launch the computations. This opens the Fluent Calculations Progression dialog box which provides information about solution convergence.

c.

Click Stop Computation if you want to interrupt the calculations. The solution should converge in approximately 180 iterations.

7.

Save the analysis files as air-filter-solution-Analysis.CATAnalysis file and propagate directory once the solution is converged. File → Save Management...

3.15. Postprocessing 1.

Click the

icon to display the scaled residuals (Figure 3.9: Scaled Residuals (p. 53)).

Figure 3.9: Scaled Residuals

2.

Display the surface monitor plots.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

53

Porous Medium in an Air Filter

54

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing

3.

Display the contours of total pressure (fringe). a.

Click the

icon.

The FLUENT for CATIA V5 display gets updated and shows the total pressure plot (Figure 3.10: Pressure Contours (Without Mesh) (p. 55)). b.

Click the

icon to disable the mesh display from the postprocessing image.

Figure 3.10: Pressure Contours (Without Mesh)

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

55

Porous Medium in an Air Filter 4.

Display the velocity path lines (Figure 3.11: Velocity Path Lines (p. 56)). Figure 3.11: Velocity Path Lines

5.

Display the pressure contours on interior planes (Figure 3.12: Pressure Contours on Interior Planes (p. 56)). •

Double-click on Pressure (nodal values).1 in the specification tree to open the Image Edition dialog box. i.

Select the interior boundaries in the Selections tab. These boundaries correspond to the walls of the filter.

ii.

Click OK. The pressure contours are displayed on the interior planes.

Figure 3.12: Pressure Contours on Interior Planes

6.

56

Similarly, display velocity contours on the interior planes (Figure 3.13: Velocity Contours on Interior Planes (p. 57)).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Appendix A: Creating Planes for Splitting Geometry The images created during the postprocessing are listed below the Fluent Solution.1 feature in the specification tree. Double-click on the image label of your interest and edit its definition using the Image Edition dialog box. Figure 3.13: Velocity Contours on Interior Planes

7.

Save the session. File → Save Management This allows you to save the files modified during the two save commands. For details, see the FLUENT for CATIA V5 User's Guide.

3.16. Summary In this tutorial you learned how to use the data mapping feature to provide inputs. You defined a porous medium to model the filter and defined monitors to determine mass flow rate at outlet, pressures across the filter element. You examined the velocity and pressure distribution across the sections of the domain and displayed the pathlines. You may want to generate the report of your simulation. For details on report generation, refer to Volatile Gas Emission Modeling Using Species Transport Model (p. 173). Refer to Appendix A: Creating Planes for Splitting Geometry (p. 57) and Appendix B: Splitting the Flow Volume (p. 58) to learn how to split the flow volumes.

3.17. Appendix A: Creating Planes for Splitting Geometry Important You can skip these step as the flow volume is already split in the .CATPart file provided. Follow this step only if flow volume is not split. When you read in the air-filter-tutorial-final.CATPart file into FfC, you will see in the specification tree that two planes are already created, plane.1 and plane.2. The following steps show you how to create planes for splitting the geometry. You can use the similar approach to create planes for splitting the geometry. 1.

Create two planes as supports for the splitting of geometry at a later stage. a.

Right-click on the solid bodies on either side of the filter and select the Hide/Show option in the contextual menu. Hiding these bodies will help you select the appropriate support to define the planes. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

57

Porous Medium in an Air Filter

b.

Click the

icon to open the Plane Definition dialog box.

Figure 3.14: Plane Definition Using Tangent to surface Option

i.

Select Tangent to surface from the Plane type drop-down list.

ii.

Select the surface and the point (see Figure 3.14: Plane Definition Using Tangent to surface Option (p. 58)).

iii.

Click OK. A plane is formed at the specified position.

c.

Similarly, define one more plane on the other side of the filter body.

2.

Save the changes and enter the FLUENT for CATIA V5 workbench.

3.

Disable the Keep Part Body Only option in the Transition group box in the General tab in the Options dialog box. Tools → Options...

3.18. Appendix B: Splitting the Flow Volume Important This step is to show how to split the flow volume. The specification tree will show all the flow properties. 1.

Right-click on Geometry.1 below the Environment.1 feature in the specification tree.

2.

Select the Split flow volumes item to open the Split Flow Volumes dialog box.

3.

Select the two planes defined in Appendix A: Creating Planes for Splitting Geometry (p. 57) (see Figure 3.15: Selection of Planes for Splitting the Flow Volume (p. 59)).

58

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Appendix B: Splitting the Flow Volume Figure 3.15: Selection of Planes for Splitting the Flow Volume

These planes will be found in the same position in the specification tree as they were in the CATIA V5 Part workbench. 4.

Click OK. The flow volume is split into three zones. You can view the new properties and new materials created below the Properties.1 feature and the Materials.1 feature respectively (see Figure 3.16: Specification Tree after Volume Split (p. 59)). Figure 3.16: Specification Tree after Volume Split

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

59

60

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 4: Internal Flow and Temperature Calculations in a Manifold 4.1. Introduction This tutorial illustrates the setup and solution of a 3D turbulent fluid flow and heat transfer in a manifold. The manifold configuration is encountered in piping systems in power plants and the automotive industries. It is often important to predict the flow field and temperature field in the neighborhood of the mixing region to properly design the locations of inlet pipes. In this tutorial, you will learn how to: • Extract the flow volume, define the physics, specify the meshing parameters, and define the boundary conditions for a given problem. • Solve the problem in the following three cases: – Steady state flow and heat transfer without considering the solid material. – Steady state flow and heat transfer considering the solid material. – Unsteady state flow and heat transfer without considering the solid material. • Initialize the calculations for mesh and flow. • Specify time varying boundary conditions using time modulation. • Create a local sensor and calculate the average temperature at the outlet. • Examine the results by performing postprocessing.

4.2. Prerequisites This tutorial assumes that you are familiar with the menu structure in FfC. It also assumes that you have read the Getting Started (p. 1) portion of the Tutorial Guide and completed Internal Flow Calculation (p. 9). Some of the steps in setup and solution procedure will not be shown explicitly.

Note It is assumed that you have the FMS and FMD licenses available. If you do not have FMD and FMS (CATIA V5) licenses then you will not be able to generate mesh as explained in the tutorial.

4.3. Problem Description The problem to be considered is shown in Figure 3.1. Air at different temperatures enters through three inlets and mixes in the manifold. The flow is assumed to be turbulent.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

61

Internal Flow and Temperature Calculations in a Manifold This tutorial is solved in three parts. In the first part, the problem is solved only for the fluid flow. In the second part, it is solved for heat transfer through the solid walls of the manifold. In the third part, the problem is solved for unsteady state flow and heat transfer without considering the solid material. Figure 4.1: Problem Schematic

4.4. Preparation 1.

Copy the CATIA V5 part file, manifold.CATPart to your working directory.

2.

Start the FfC environment.

Note While saving the analysis files, create separate folders for each case and save the solution files accordingly.

4.5. Setting the Options Tools → Options → Analysis & Simulation → Fluent Options 1.

Click the General tab in the Options dialog box. a.

Enter the path for the ANSYS Fluent solver in the text entry box next to Folder for solver.

Note The ANSYS Fluent solver is provided with the installed FfC package. You can use the Browse button to specify the path for the solver:

62

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 4.2: Options Dialog Box — General

For 32 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/ntx86 For 64 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/win64 Similarly, specify the path for the external postprocessor, CFD-Post (or FloWizard) executable.

b. 2.

Set the remaining parameters as shown in Figure 4.2: Options Dialog Box — General (p. 63).

Click the Data Management tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

63

Internal Flow and Temperature Calculations in a Manifold Figure 4.3: Options Dialog Box — Data Management

a.

Enter the path for Temporary files, FLUAnalysisComputations file and FLUAnalysisResults file in the External Storage folder group box. You can use the Browse button to specify the path. The analysis files will be saved in the temporary folders while FfC is computing the solution. The analysis will be saved to its permanent location when the computation is complete.

b. 3.

64

Set the remaining parameters as shown in Figure 4.3: Options Dialog Box — Data Management (p. 64).

Click the Advanced Parameters tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 4.4: Options Dialog Box — Advanced Parameters

• 4.

Set the parameters as shown in Figure 3.4: Options Dialog Box — Advanced Parameters (p. 39).

Click the Customization tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

65

Internal Flow and Temperature Calculations in a Manifold Figure 4.5: Options Dialog Box — Customization

a.

Enable Advanced Turbulence Models.

Note If the Advanced Turbulence Models option is disabled, then the default turbulence model (k-epsilon, Realizable) for turbulent flows and Reynolds Stress Model for turbulence with strong swirl will be selected without any further access to more turbulence models.

b.

Enable Advanced Boundary Condition Parameters.

Note The Advanced Boundary Condition Parameters option allows specification of heat generation rate for wall boundary.

c.

Enable Use solution steering by default.

Note The Use solution steering by default option enables solution steering mechanism to control the solution convergence automatically.

66

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Extracting Flow Volume d.

Disable Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" .

Note The Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" option uses second order solutions after 75% accuracy settings during mesh definition. If this option is disabled, then first order solution is computed for all slider positions.

5.

Click OK to close the Options dialog box.

4.6. Reading the File 1.

Read the CATIA V5 file (manifold.CATPart) in FLUENT for CATIA V5. File → Open... This opens the File Selection dialog box, using which you can select the file to be read.

2.

Select the file, manifold.CATPart. By default, the file is opened in the Part or Product workbench of CATIA V5.

Tip To use the entire screen space, remove the specification tree on the left-hand side by selecting the View → Specifications menu item or pressing the F3 key on your keyboard.

4.7. Starting FLUENT for CATIA V5 1.

Launch the FfC workbench. Start → Analysis & Simulation → FLUENT for CATIA V5 This updates the graphics display. The specification tree on the left-hand side also gets updated and displays the analysis-related parameters.

2.

Specify the path to the directory where you want to store the ANSYS Fluent solver files in the Options dialog box.

4.8. Extracting Flow Volume In this step, you will define the inlet and outlet faces, and extract the flow volume. 1.

Click the icon or double-click the Geometry Definition.1 option located below the Environment.1 feature in the specification tree to open the Geometry Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

67

Internal Flow and Temperature Calculations in a Manifold

2.

Select solid model from the Geometry definition drop-down list.

3.

Select Faces in the Selection mode drop-down list.

4.

Click on the field next to Inlet, zoom-in the inlet side of the geometry, and select the three circular (annular) faces as the inlet . When you move the pointer near the inlet, the faces around the pointer gets highlighted. Select the appropriate faces as shown in Figure 4.1: Problem Schematic (p. 62).

5.

Click on the field next to Outlet, zoom-in on the outlet side of the geometry, and select the annular circular face as the outlet.

6.

Click OK to validate. This creates a flow volume for the geometry. The flow volume is displayed in the graphics window. The specification tree on the left-hand side also gets updated to show relevant parameters.

4.9. Meshing Parameters •

68

Click the icon or double-click the Mesh Definition.1 option located below the Environment.1 feature in the specification tree to open the Mesh Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Meshing Parameters

a.

Click Reset All.

b.

Retain the default position of the slider bar at 50.

Note Some of the parameters in the Mesh Definition dialog box are linked to the position of the slider bar. Therefore, depending on the mesh type, moving the slider changes the values of such parameters.

c.

Use the default Optimized Surface mesher as the Mesh Type.

d.

Enable Critical length and enter 1.2 mm for the value.

e.

Enter 10 mm for Mesh Size.

f.

Click the Geometry tab and enter 0 for Angle between faces and Angle between curves.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

69

Internal Flow and Temperature Calculations in a Manifold

g.

Click the Surface Mesh tab and specify a value of 1 for Automatic mesh capture.

This parameter defines the coarsest settings for all surface mesh, and you use it to define the surface mesh size at the external flow boundaries. h.

70

Click the Volume mesh tab and enable Size progression and specify a value of 1.2.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Physics

This parameter controls the growth rate of mesh size. i.

Click OK to validate.

4.10. Physics 1.

Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the FLUENT for CATIA V5 specification tree in the Physical Model Definition dialog box.

2.

Enable Accounting for Temperature Effect.

3.

Disable Include Solid.

4.

Select Turbulent in the Flow Type drop-down list.

5.

Select k-epsilon, Realizable in the Turbulence Model drop-down list.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

71

Internal Flow and Temperature Calculations in a Manifold 6.

Select Incompressible ideal gas from the Flow Property drop-down list.

7.

Select steady from the Time drop-down list.

8.

Click OK to validate.

4.11. Materials 1.

Click the

icon to open the Library dialog box.

2.

Select the FLUENT for CATIA V5 fluids and mixtures materials library. To open the materials library, you have to specify the path where it is stored. For 32 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\intel_a\startup\materials\Fluids and Mixtures.CATmaterial For 64 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\win_b64\startup\materials\Fluids and Mixtures.CATmaterial where X-X.X.X represents the version used.

72

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Boundary Conditions

3.

Drag and drop the boundaries.

icon (Air) in the Library (Read Only) dialog box on any of the inlet/outlet

This includes air as the material for your case setup. 4.

Close the Library dialog box.

4.12. Boundary Conditions 1.

Specify the inlet boundary conditions. a.

Click the

icon to open the Inlet Boundary Condition dialog box.

b.

Click the Inlet Boundary option located below the Groups.1 feature in the specification tree This automatically updates the Supports field.

2.

c.

Enable Velocity and enter a value of 0.1 m_s.

d.

Select Long tube, pipe or duct from the Source of Flow drop-down list.

e.

Click OK to validate.

Similarly, specify boundary conditions for the other two inlets using the values displayed in the following table: Boundary

Velocity (m_s)

Temperature (K)

Inlet Boundary..2

0.1

400

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

73

Internal Flow and Temperature Calculations in a Manifold Inlet Boundary.3

3.

0.2

500

Specify the outlet boundary conditions. a.

Click the

icon to open the Outlet Boundary Condition dialog box.

b.

Ensure that 1 Outlet boundary is selected for Supports Since there is a single outlet boundary in this example it is automatically selected in the Supports field in Outlet Boundary Condition dialog box.

4.

74

c.

Enable Gauge Pressure (Static) and set the value to 0 N_m2.

d.

Click OK to validate.

Specify the wall boundary conditions. a.

Click

icon to open the Wall Boundary Conditions dialog box.

b.

Select Wall(FluidToSolid.1.1_1).1 as support from the Groups.1 feature in the specification tree.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Solution

5.

c.

Enable Temperature-dependent heat flux (convection).

d.

Enter 4 W_kdeg_m2 as the Heat transfer coefficient.

e.

Enter 298.15 kdeg as the Ambient temperature.

f.

Click OK to close the Wall Boundary Condition dialog box.

Save the CATIA V5 analysis files in a new folder as manifold_case1.CATAnalysis. File → Save Management...

4.13. Solution In this step, you will generate the mesh, and iterate the solution. Though FLUENT for CATIA V5 allows you to generate the mesh and start the flow computations separately, here you will perform these steps simultaneously. 1.

Double-click on Initialization Values.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Initialization Values dialog box. •

2.

Click Reset All and OK to validate.

Double-click on Fluent Solution.1 below the Fluent case feature in the specification tree to open the Fluent Solution dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

75

Internal Flow and Temperature Calculations in a Manifold

3.

a.

Click Reset All.

b.

Set the slider position to 2.

c.

Ensure that Residuals + Fluxes&Delta option is selected as the Convergence Criterion.

d.

Ensure that Use solution steering is enabled.

e.

Ensure that Maximum CPU Time is enabled and set to 30000 s.

f.

Click OK to close the Fluent Solution dialog box.

Click

icon to open the Compute dialog box.

4.14. Postprocessing 1.

76

Click the

icon to display the scaled residuals (Figure 4.6: Scaled Residuals (p. 77)).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing Figure 4.6: Scaled Residuals

2.

Click icon to display the contours of static temperature Figure 4.7: Contours of Static Temperature (p. 77)). Figure 4.7: Contours of Static Temperature

3.

Click

icon to display the contours of velocity (Figure 4.8: Contours of Velocity (p. 78)).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

77

Internal Flow and Temperature Calculations in a Manifold Figure 4.8: Contours of Velocity

4.

Click

•

icon to display the velocity path lines (Figure 4.9: Velocity Path Lines (p. 78)).

Click

icon to change the transparency settings of the outer walls.

Figure 4.9: Velocity Path Lines

4.15. Finding Average Temperature at the Outlet In this step, find the average temperature at the outlet surface of the manifold by creating a local sensor. 1.

78

Right-click on the Sensors.1 option in the Fluent case set and select the Create Local Sensor option in the contextual menu to open the Create Sensor dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Finding Average Temperature at the Outlet 2.

Select Temperature and click OK to validate. This creates a Temperature.1 subset in the Sensors.1 set under Fluent Solution.1.

3.

Double-click Temperature.1 to open the Local Sensor dialog box. It allows you to specify the local sensor parameters and the position where you want to locate it.

a.

Click in the Supports field and select the group representing the outlet of the manifold. This sets the position of the local sensor on the outlet surface.

b.

Select Face of element (from solver) in the Position drop-down list under Values.

c.

Select Average in the Post-Treatment drop-down list. This calculates the average temperature at the outlet.

d.

Enable Create Parameters.

e.

Click OK to validate. You have created a local sensor at the outlet face. This sensor finds the average temperature at the outlet. The Sensors.1 set looks as follows:

At this point, the temperature value is not updated. 4.

Right-click on the Temperature.1 set and select Update Sensor in the contextual menu. Click OK in the Warning dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

79

Internal Flow and Temperature Calculations in a Manifold

5.

Click OK. The average temperature at the outlet face is displayed in the Temperature set.

6.

Right-click on Temperature and click on Definition... to view the temperature.

7.

Save the session. File → Save Management...

4.16. Case 2: Considering Solid Material of Walls In this case, you will take account of heat transfer through the solid walls of the manifold.

4.16.1. Opening FLUENT for CATIA V5 Workbench 1.

Open the part file. Start → manifold.CATPart Since you have already read the input file in CATIA V5, there is no need to read it again.

2.

Launch the FfC workbench. Start → Analysis & Simulation → Fluent for CATIA V5

80

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Case 2: Considering Solid Material of Walls

4.16.2. Flow Volume Same as Extracting Flow Volume (p. 67) for Case 1.

4.16.3. Meshing Parameters Same as Meshing Parameters (p. 68) for Case 1.

4.16.4. Physics Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the FLUENT for CATIA V5 specification tree in the Physical Model Definition dialog box.

1.

Enable both Accounting for Temperature Effect and Include Solid.

2.

Select Turbulent in the Flow Type drop-down list.

3.

Select k-epsilon, Realizable in the Turbulence Model drop-down list.

4.

Select Incompressible ideal gas in the Flow Property drop-down list.

5.

Click OK to validate.

4.16.5. Materials Two regions are created during the flow volume extraction (fluid region and solid region). Therefore, include one fluid material and one solid material in the case setup.

1.

Click the

icon to open the Library dialog box.

2.

Select the FLUENT for CATIA V5 fluids and mixtures materials library. To open the materials library, you have to specify the path where it is stored. For 32 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\intel_a\startup\materials\Fluids and Mixtures.CATmaterial

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

81

Internal Flow and Temperature Calculations in a Manifold For 64 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\win_b64\startup\materials\Fluids and Mixtures.CATmaterial where X-X.X.X represents the version used.

3.

Drag and drop the blue) of the flow volume.

icon (Air) in the Library (Read Only) dialog box onto the fluid region (in

This includes air as the material for your case setup. 4.

Open the solid materials library of CATIA V5. a.

Select the Metal tab.

b.

Drag and drop icon (in red) of the flow volume.

(Iron) in the Library (Read Only) dialog box onto the solid region

This assigns iron as the solid material. c.

82

Click OK to validate.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Case 2: Considering Solid Material of Walls The Materials specification tree is updated.

5.

Double-click the Thermal Material.1 option located below the Iron.1 feature in the specification tree to open the Thermal Material dialog box.

a.

Verify the values of Thermal Conductivity and Specific Heat.

b.

Close the Thermal Conductivity dialog box.

4.16.6. Boundary Conditions 1.

Specify the inlet and outlet boundary conditions as in step 1 (p. 73), step 2 (p. 73), and step 3 (p. 74) under Boundary Conditions (p. 73).

2.

Open Flow Property Definition dialog box and enable Show walls between solid/fluid zones.

3.

Specify the wall boundary conditions. a.

Click

b.

Select Wall(SolidBoundary.1.1_1).6 as support from the Groups.1 feature in the specification tree.

c. 4.

icon to open the Wall Boundary Conditions dialog box.

i.

Enable Temperature-dependent heat flux (convection).

ii.

Enter 4 W_kdeg_m2 as the Heat transfer coefficient.

iii.

Enter 298.15 kdeg as the Ambient temperature.

Click OK to close the Wall Boundary Condition dialog box.

Save the CATIA V5 analysis files in a new folder as manifold_case2.CATAnalysis. File → Save Management...

4.16.7. Solution Same as Solution (p. 75) for Case 1.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

83

Internal Flow and Temperature Calculations in a Manifold

4.16.8. Postprocessing 1.

Click

icon to display the residuals (Figure 4.10: Scaled Residuals (p. 84)).

Figure 4.10: Scaled Residuals

2.

Display the contours of static temperature (Figure 4.11: Temperature Contours (p. 84)). Figure 4.11: Temperature Contours

The temperature field fringe plot is displayed in Figure 4.12: Temperature (fringe) Contours (p. 85).

84

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Case 2: Considering Solid Material of Walls Figure 4.12: Temperature (fringe) Contours

3.

Display the contours of static temperature of the wall-fluid interface (Figure 4.13: Temperature Contours at Wall-Fluid Interface (p. 85)). a.

Right click Temperature field fringe.1 in the specification tree and select Temperature field .1 object and click Definition tab next to it.

b.

Select Wall (FluidToSolid.1.1_1).1 in the Available Groups and transfer it to the Activated Groups. The wall of the manifold is hidden and contours of the wall-fluid interface become visible. Figure 4.13: Temperature Contours at Wall-Fluid Interface

4.

Display the temperature contours on a cut plane (Figure 4.14: Setting Up the Cut Plane (p. 86)).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

85

Internal Flow and Temperature Calculations in a Manifold a.

Select the group Flow.1 and move it into the Activated Groups list in the Image Edition dialog box.

b.

Click and move the cut plane to the position shown in Figure 4.14: Setting Up the Cut Plane (p. 86). Figure 4.14: Setting Up the Cut Plane

5.

Display the contours of vector magnitude at the wall-fluid interface (Figure 4.15: Velocity Contours at Wall-Fluid Interface (p. 87)).

a.

Click

icon in the Common Images toolbar.

The contours of only the inlets and outlets appear. You have to change the settings in the Image Edition dialog box to display the walls. b.

Double-click Velocity.1 in the specification tree to open the Image Edition dialog box.

i.

86

Click the Visu tab and select Fringe in the Types list.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Case 3: Transient Analysis Without Considering Solid Material

ii.

Select the inlets, outlet and liquid-solid interface and move them to the Activated Groups list.

iii.

Click OK to validate.

Figure 4.15: Velocity Contours at Wall-Fluid Interface

6.

Save the session. File → Save Management...

4.17. Case 3: Transient Analysis Without Considering Solid Material In this case, you will make a transient analysis of the manifold.

4.17.1. Opening FLUENT for CATIA V5 Workbench 1.

Open the part file. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

87

Internal Flow and Temperature Calculations in a Manifold Start → manifold.CATPart Since you have already read the input file in CATIA V5, there is no need to read it again. 2.

Launch the FfC workbench. Start → Analysis & Simulation → Fluent for CATIA V5

3.

Setting the options. Tools → Options → Analysis & Simulation → → Fluent Options

a.

Click the Customization tab in the Options dialog box.

b.

Select Residuals from the Convergence Criterion drop-down list.

4.17.2. Flow Volume Same as Extracting Flow Volume (p. 67) for Case 1.

4.17.3. Meshing Parameters Same as Meshing Parameters (p. 68) for Case 1.

88

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Case 3: Transient Analysis Without Considering Solid Material

4.17.4. Physics Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the FLUENT for CATIA V5 specification tree in the Physical Model Definition dialog box.

1.

Enable Accounting for Temperature Effect.

2.

Select Turbulent in the Flow Type drop-down list.

3.

Select k-epsilon, Realizable in the Turbulence Model drop-down list.

4.

Select Incompressible ideal gas in the Flow Property drop-down list.

5.

Select unsteady in the Time drop-down list.

6.

Click OK to validate.

Note The Include Solid option is disabled.

4.17.5. Materials A single flow region is created during the flow volume extraction process. Therefore, include a fluid material in the case setup.

1.

Click the

icon to open the Library dialog box.

2.

Select the FLUENT for CATIA V5 fluids and mixtures materials library. To open the materials library, you have to specify the path where it is stored. For 32 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\intel_a\startup\materials\Fluids and Mixtures.CATmaterial

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

89

Internal Flow and Temperature Calculations in a Manifold For 64 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\win_b64\startup\materials\Fluids and Mixtures.CATmaterial where X-X.X.X represents the version used.

a.

Drag and drop the the FfC graphics window.

icon (Air) in the Library (Read Only) dialog box on flow volume in

This includes air as the material for your case setup. b.

Click the Apply Material.

c.

Click OK to validate. The Materials specification tree is updated.

3.

Close the Library dialog box.

4.17.6. Boundary Conditions 1.

90

Input the modulations for the various boundaries. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Case 3: Transient Analysis Without Considering Solid Material

a.

Click

icon to open the Time Modulation dialog box.

b.

Click Browse to open the File Selection dialog box.

c.

Select the file inlet-1-velo.xls from the input files folder and click Open. The specification tree is updated to show Time Modulation.1 under Modulations.1.

d.

Similarly input the files inlet-1-temp.xls, inlet-2-temp.xls, inlet-2-velo.xls, inlet-3-temp.xls, and inlet-3-velo.xls. These files create the features Time Modulation.2, Time Modulation.3, Time Modulation.4, Time Modulation.5, and Time Modulation.6 respectively in the specification tree.

e.

Rename Time Modulation.1 as inlet-1-velo. Double-click on Time Modulation.1 to edit the name.

f.

Similarly rename the other elements under Modulations.1 according to the input file they represent. This will prevent confusion when assigning the data to the respective parameters.

2.

Specify the inlet boundary conditions. a.

Click

icon to open the Inlet Boundary Condition dialog box.

b.

Click the Inlet Boundary.3 option located below the Groups.1 feature in the specification tree.

c.

Enable Velocity and set the value to 1.

d.

Select Long tube, pipe or duct as the Source of Flow.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

91

Internal Flow and Temperature Calculations in a Manifold e.

Set the value for Temperature to 300 kdeg.

f.

Enable Variant Data and select Time Modulation from the drop-down list. The time modulation data will now be applied to the parameter that you have selected using the check box (Velocity).

g.

Click

icon to open the Variation Definition dialog box.

i.

Select inlet-1-velo from the Modulations.1 group in the specification tree.

ii.

Click OK to validate.

h.

Similarly, select inlet-1-temp for Variant Temperature.

i.

Click OK to validate.

3.

Specify Velocity as 1 m_sec and Temperature as 300 kdeg for the other two inlets.

4.

Specify time modulation to the other two inlets using the following table:

5.

Variant Data

Variant Temperature

Inlet Boundary.4

inlet-2-velo

inlet-2-temp

Inlet Boundary.5

inlet-3-velo

inlet-2-temp

Specify the outlet boundary conditions.

a.

92

Boundary

Click

icon to open the Outlet Boundary Condition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Case 3: Transient Analysis Without Considering Solid Material b.

Ensure that 1 Outlet boundary is selected for Supports. Since there is a single outlet boundary in this example it is automatically selected in the Supports field in Outlet Boundary Condition dialog box.

6.

c.

Enable Gauge Pressure and specify a value of 0 N_m2.

d.

Click OK to validate.

Specify the wall boundary conditions. a.

Click

b.

Ensure that 1 Wall boundary is selected for Supports.

c. 7.

icon to open the Wall Boundary Conditions dialog box.

i.

Enable Temperature-dependent heat flux (convection).

ii.

Enter 4 W_kdeg_m2 as the Heat transfer coefficient.

iii.

Enter 298.15 kdeg as the Ambient temperature.

Click OK to close the Wall Boundary Condition dialog box.

Save the CATIA V5 analysis files as manifold_case3.CATAnalysis. File → Save Management...

4.17.7. Solution In this step, define the problem setup, define the solution settings, define the monitors, generate the mesh, and iterate the solution. Though FfC allows you to generate the mesh and start the flow computations separately, perform these steps simultaneously. 1.

Define the problem setup. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

93

Internal Flow and Temperature Calculations in a Manifold a.

Double-click the Unsteady Parameters.1 feature under Fluent Problem Setup.1 to open the Unsteady Parameters dialog box.

i.

Select automated from the Transient Controls drop-down list.

ii.

Set Time Step Size to 0.005 s.

iii.

Set Number of Time Steps to 40.

iv.

Set Data save frequency to 1 and click OK.

Note When you set Data save frequency to 1, FfC will save ANSYS Fluent data after every timestep. This helps in analyzing the solution after each time step during postprocessing.

b.

Set the initialization values.

•

2.

A.

Click Reset All.

B.

Set X Velocity to 0.0001.

Define solution settings. •

94

Double-click on Initialization Values.1.

Double-click Fluent Solution.1 to open the Fluent Solution dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Case 3: Transient Analysis Without Considering Solid Material

3.

i.

Click Reset All.

ii.

Ensure that Residuals option is selected as the Convergence Criterion.

iii.

Click Relaxation Settings to open Relaxation Settings dialog box.

iv.

Ensure that Energy is 1.

v.

Ensure that Use solution steering is disabled.

Save the analysis file in a new folder as manifold_case3.CATAnalysis. File → Save Management...

4.

Define a monitor for mass-weighted average temperature at the outlet. •

Right click on Monitors.1 and select Surface Monitor to open the Surface Monitor dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

95

Internal Flow and Temperature Calculations in a Manifold

5.

Click

i.

Select the outlet for Supports.

ii.

Select Mass Weighted Average in the Report Type drop-down list.

iii.

Select Temperature and Static Temperature under Report Of.

iv.

Select Time Step as the X-Axis Type and click OK.

icon to open the Compute dialog box.

a.

Select All and Default Solution Options in the two drop-down lists available.

b.

Click OK in the Compute dialog box to launch the computations.

4.17.8. Postprocessing 1.

96

Click

icon to display the residuals (Figure 4.16: Scaled Residuals (p. 97)).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Case 3: Transient Analysis Without Considering Solid Material Figure 4.16: Scaled Residuals

Figure 4.17: Surface Monitor Plot

2.

Display the contours of static temperature on the wall boundary for different time steps (Figure 4.18: Contours of Static Temperature at 0.08 s (p. 99)). a.

Click

icon. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

97

Internal Flow and Temperature Calculations in a Manifold FLUENT for CATIA V5 displays the contours at time step zero by default. b.

Double-click Temperature field iso.1 to open the Image Edition dialog box.

• c.

Select the 0.08 Time Step in the Occurrences tab.

Double-click on the color map to open the Color Map Edition dialog box.

i.

Set Imposed max to 350.

ii.

Set Imposed min to 300.

iii.

Click on

button and enable Smooth in the Color Edition dialog box.

The temperature distribution is as shown in Figure 4.18: Contours of Static Temperature at 0.08 s (p. 99).

98

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Case 3: Transient Analysis Without Considering Solid Material Figure 4.18: Contours of Static Temperature at 0.08 s

3.

Similarly display temperature contours for 0.15 s, 0.175 s, and the final time step (Figure 4.19: Contours of Static Temperature at 0.15 s (p. 99), Figure 4.20: Contours of Static Temperature at 0.175 s (p. 100), and Figure 4.21: Contours of Static Temperature at the Final Time Step (p. 100)). Figure 4.19: Contours of Static Temperature at 0.15 s

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

99

Internal Flow and Temperature Calculations in a Manifold Figure 4.20: Contours of Static Temperature at 0.175 s

Figure 4.21: Contours of Static Temperature at the Final Time Step

4.

Display the contours of velocity distribution on wall boundary and inlets (Figure 4.22: Velocity (fringe) Distribution at the Final Step (p. 101)).

a.

Click

b.

Double-click on the color map and click on the Color Edition dialog box. •

100

icon button in the Color Map Edition dialog box to open

Select Smooth in the Color Edition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Case 3: Transient Analysis Without Considering Solid Material Figure 4.22: Velocity (fringe) Distribution at the Final Step

5.

Display the velocity vectors on a cut plane Figure 4.23: Velocity Vectors in a Cut Plane Passing Through Two Inlets (p. 101)). a.

b.

Double-click on Velocity.1 to open the Image Edition dialog box. i.

Select Symbol under Types in the Visu tab.

ii.

Click OK.

Click

icon to view the velocity vectors in a section.

Figure 4.23: Velocity Vectors in a Cut Plane Passing Through Two Inlets

6.

Save the session. File → Save Management...

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

101

Internal Flow and Temperature Calculations in a Manifold

4.18. Summary In this tutorial you learned how to solve a problem with and without heat conduction in solid walls. You also learned how to solve a problem with unsteady solution and vary the boundary conditions using the time modulation feature. You then included two different materials in your case setup and assigned them to appropriate mesh regions in the domain. You may want to generate the report of your simulation. For details about generating reports, refer to Volatile Gas Emission Modeling Using Species Transport Model (p. 173).

102

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 5: External Flow Calculations Over a Blimp 5.1. Introduction This tutorial illustrates the setup and solution of a 3D, external turbulent fluid flow over an advertising blimp. In order to properly place wires for the anchoring system, it is important to predict the forces around the blimp. In this tutorial, you will learn how to: • Define flow volume, physics, meshing parameters, and boundary conditions for a given problem. • Solve the case for external fluid flow. • Initialize the calculations for meshing and analyze the mesh quality using a cut plane. • Initialize the calculations for flow and perform postprocessing

5.2. Prerequisites This tutorial assumes that you are familiar with the menu structure in FfC. It also assumes that you have read the Getting Started (p. 1) portion of the Tutorial Guide and completed Internal Flow Calculation (p. 9). Some of the steps in setup and solution procedure will not be shown explicitly.

Note It is assumed that you have the FMS and FMD licenses available. If you do not have FMD and FMS (CATIA V5) licenses then you will not be able to generate mesh as explained in the tutorial.

5.3. Problem Description The problem to be considered is shown in Figure 5.1: Blimp Geometry (p. 104). The blimp is at the center of the external ow domain. Air flows parallel to the walls of the external ow domain towards the blimp at 10 m/s. This allows you to simulate the effects of inclined velocity ow on the blimp. The flow is assumed to be turbulent.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

103

External Flow Calculations Over a Blimp Figure 5.1: Blimp Geometry

5.4. Preparation 1.

Copy the CATIA V5 part file, blimp_with_box.CATPart and blimp_without_box.CATPart to your working directory. The file blimp_without_box.CATPart includes only the blimp geometry, without an external flow boundary around the blimp geometry. You will have to create the external flow boundaries manually. The file blimp_with_box.CATPart includes blimp geometry as well as the external flow boundary around the blimp geometry. If you choose to read the file blimp_with_box.CATPart, skip the step 3.

2.

Start the FfC environment.

5.5. Setting the Options Tools → Options → Analysis & Simulation → Fluent Options 1.

104

Click the General tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 5.2: Options Dialog Box — General

a.

Enter the path for the ANSYS Fluent solver in the text entry box next to Folder for solver.

Note The ANSYS Fluent solver is provided with the installed FfC package. You can use the Browse button to specify the path for the solver: For 32 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/ntx86 For 64 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/win64 Similarly, specify the path for the external postprocessor, CFD-Post (or FloWizard) executable.

b.

Set the remaining parameters as shown in Figure 5.2: Options Dialog Box — General (p. 105).

Note You can specify the Maximum number of iterations. For this tutorial the recommended value is 5000 iterations. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

105

External Flow Calculations Over a Blimp 2.

Click the Data Management tab in the Options dialog box. a.

Enter the path for Temporary files, FLUAnalysisComputations file and FLUAnalysisResults file in the External Storage folder group box. You can use the Browse button to specify the path. The analysis files will be saved in the temporary folders while FfC is computing the solution. The analysis will be saved to its permanent location when the computation is complete.

b.

Set the remaining parameters as shown in Figure 5.3: Options Dialog Box — Data Management (p. 106). Figure 5.3: Options Dialog Box — Data Management

3.

106

Click the Advanced Parameters tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 5.4: Options Dialog Box — Advanced Parameters

• 4.

Set the parameters as shown in Figure 5.4: Options Dialog Box — Advanced Parameters (p. 107).

Click the Customization tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

107

External Flow Calculations Over a Blimp Figure 5.5: Options Dialog Box — Customization

a.

Enable Advanced Turbulence Models.

Note If the Advanced Turbulence Models option is disabled, then the default turbulence model (k-epsilon, Realizable) for turbulent flows and Reynolds Stress Model for turbulence with strong swirl will be selected without any further access to more turbulence models.

b.

Enable Advanced Boundary Condition Parameters.

Note The Advanced Boundary Condition Parameters option allows specification of heat generation rate for wall boundary.

c.

Enable Use solution steering by default.

Note The Use solution steering by default option enables solution steering mechanism to control the solution convergence automatically.

108

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Creating the External Flow Domain d.

Enable Control "Solver Accuracy Settings" based on slider position of "Mesh Definition". The Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" option uses second order solutions after 75% accuracy settings during mesh definition. If this option is disabled, then first order solution is computed for all slider positions.

5.

Click OK to close the Options dialog box.

5.6. Reading the File 1.

Read the CATIA V5 file (blimp_without_box.CATPart) in FLUENT for CATIA V5. File → Open... This opens the File Selection dialog box, using which you can select the file to be read.

2.

Select the file, blimp_without_box.CATPart. By default, the file is opened in the Part or Product workbench of CATIA V5.

Tip To use the entire screen space, remove the specification tree on the left-hand side by selecting the View → Specifications menu item or pressing the F3 key on your keyboard.

5.7. Creating the External Flow Domain The geometry that you have read in CATIA V5 is the blimp geometry. In this step, you will create an external flow domain around the blimp geometry. The boundaries of this domain will consist of a rectangular duct of thin walls open from the inlet and outlet sides of the blimp. 1.

Launch Part workbench of CATIA V5. Start → Mechanical Design → Part Design

Note Use sketcher tool to create the box around the blimp (see Figure 5.7: External Flow Domain Extents (Rear View) (p. 110)).

2.

Using various geometry features in CATIA V5 create a hollow rectangular shaped domain around the blimp geometry (see Figure 5.8: Blimp and External Flow Domain (p. 111)). The following guidelines will help you understand the dimensions of the flow domain surrounding the blimp. a.

The extents of the external flow domain on all sides (except the outlet side) of the blimp should be three times the length of the blimp.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

109

External Flow Calculations Over a Blimp b.

The extents of the external ow domain on the outlet side should be around six times the length of the blimp. See Figure 5.6: External Flow Domain Extents (Blimp Length is 143 Units) (p. 110) and Figure 5.7: External Flow Domain Extents (Rear View) (p. 110) for details. Figure 5.6: External Flow Domain Extents (Blimp Length is 143 Units)

Figure 5.7: External Flow Domain Extents (Rear View)

3.

110

Click the

icon to open the Pad Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Starting FLUENT for CATIA V5

4.

Specify the parameters as shown in the Pad Definition dialog box and click OK to validate. The geometry is as shown in Figure 5.8: Blimp and External Flow Domain (p. 111).

Note If you want to use the blimp with box directly, the file blimp_with_box.CATPart is also provided with the input files. Figure 5.8: Blimp and External Flow Domain

5.8. Starting FLUENT for CATIA V5 1.

Launch the FfC workbench. Start → Analysis & Simulation → FLUENT for CATIA V5

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

111

External Flow Calculations Over a Blimp This updates the graphics display. The specification tree on the left-hand side also gets updated and displays the analysis-related parameters. 2.

In the Options dialog box, specify the location of the directory where you want to store the solver files.

5.9. Extracting Flow Volume In this step, you will define the inlet and outlet faces, and extract the flow volume. 1.

Click the icon or double-click the Geometry Definition.1 option located below the Environment.1 feature in the specification tree to open the Geometry Definition dialog box.

2.

Click in the text entry field next to Inlet, zoom in the inlet side of the geometry and select the square face (i.e., the hollow square frame) at the inlet side of the blimp as inlet. When you move the pointer near the inlet, faces around the pointer will get highlighted.

3.

Click in the text entry field next to Outlet, zoom in the outlet side of the geometry and select the square face (i.e., the hollow square frame) at the outlet side of the blimp as outlet.

4.

Click OK to validate. This creates a flow volume for the geometry. The flow volume is displayed in the graphics window. The specification tree on the left-hand side also gets updated to show relevant parameters.

5.10. Physics 1.

112

Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the FLUENT for CATIA V5 specification tree in the Physical Model Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Meshing Parameters 2.

Select Turbulent in the Flow Type drop-down list.

3.

Disable Accounting for Temperature Effect.

4.

Select k-epsilon, Realizable in the Turbulence Model drop-down list.

5.

Select steady in the Time drop-down list.

6.

Click OK to validate.

5.11. Meshing Parameters 1.

Click the icon or double-click the Mesh Definition.1 option located below the Environment.1 feature in the specification tree to open the Mesh Definition dialog box.

a.

Click Reset All.

b.

Move the slide bar towards Accuracy till it shows a value of 75. When you move the slide bar, the other parameters will change accordingly.

c.

Make sure that the Optimized Surface mesher (proximity detection) is selected.

d.

Set Critical length to 2 mm.

e.

Enable Min Mesh size and set it to 3 mm. This helps in capturing the finer details of the blimp like the fins and also in better convergence of the solution.

f.

Select Geometry tab and make sure you make the settings as shown in Figure 5.9: The Geometry and Surface mesh Tab Settings (p. 114) (A).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

113

External Flow Calculations Over a Blimp Figure 5.9: The Geometry and Surface mesh Tab Settings

g.

Select Surface Mesh tab and specify a value of 35 and 1.1 for Automatic mesh capture and Growth rate, respectively (see Figure 5.9: The Geometry and Surface mesh Tab Settings (p. 114) (B).). This parameter defines the coarsest settings for all surface mesh, and you use it to define the surface mesh size at the external flow boundaries.

h.

Select Volume Mesh tab and ensure that Size progression is set to 1.1. This parameter controls the growth rate of mesh size.

i.

Click OK to validate. You have defined a coarse mesh for the external domain, but it is very important to have a fine mesh on the blimp surface. Therefore, in the next step you will identify the blimp surface and specify different parameters for it.

2.

Identify the blimp surface. a.

Make the external faces of the domain transparent.

b.

Expand the Nodes and Elements set in the specification tree.

c.

Bring the cursor on each of subgroup listed in the Nodes and Elements set. This highlights the corresponding face of the domain in the graphics display. In this tutorial, FluidToSolid1.1_1 is the blimp surface. It can be different for your case.

114

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Meshing Parameters d.

3.

Perform the following to see the mesh: i.

Click the

icon.

ii.

Right-click FluidToSolid.1.1_1 under Nodes and Elements in the specification tree and select Activate/Deactivate to activate the mesh visualization.

Double-click the FluidToSolid1.1_1 option located below the Nodes and Elements feature in the specification tree to open the Global Parameters dialog box.

a.

Set the value of Mesh Size to 3.5 mm.

b.

Disable Absolute sag.

c.

Set Relative sag to 0.054542.

d.

Set Min Size to 0.4 mm.

e.

Enable Automatic mesh capture.

f.

Set Tolerance to 35 mm.

g.

Select Geometry tab and set the following values: Table 5.1: Parameter Values Parameter

Value

Constraint Sag

0.175

Angle between faces

10 deg

Angle between curves

10 deg

Min holes size

4.291 mm

Min size

2 mm

Tolerance

0 mm

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

115

External Flow Calculations Over a Blimp

h. 4.

Disable Constraint ref size independent from mesh size.

Constrain the geometry to get an accurate mesh. a.

Right-click Links Manager.1 and select Hide/Show to hide the total geometry.

b.

Click the •

icon to open the Add/Remove Constraints dialog box.

Select the edges of the blimp as shown in Figure 5.10: Selection of Blimp Edges as Mesh Constraints (p. 116) and click OK. Figure 5.10: Selection of Blimp Edges as Mesh Constraints

c.

116

Click the

icon to mesh the part globally.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Meshing Parameters Figure 5.11: Mesh at Blimp Extremities after Constraining Geometry

The resultant mesh will be accurate at the sharp corners of the geometry as show in Figure 5.11: Mesh at Blimp Extremities after Constraining Geometry (p. 117). Without constraining you may encounter empty unmeshed spaces at the sharp edges of the geometry as shown in Figure 5.12: Mesh at Blimp Extremities Without Constraining Geometry (p. 117). Figure 5.12: Mesh at Blimp Extremities Without Constraining Geometry

Note You can obtain an accurate mesh also by specifying 0 as the Angle between faces and Angle between curves in the Geometry tab of the Global Parameters dialog box. If you do this, then there is no need to specify geometry constraints.

5.

Click the

icon to exit the meshing workbench.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

117

External Flow Calculations Over a Blimp

5.12. Materials 1.

Click the

icon to open the Library dialog box.

2.

Select the FLUENT for CATIA V5 fluids and mixtures materials library. To open the materials library, you have to specify the path where it is stored. For 32 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\intel_a\startup\materials\Fluids and Mixtures.CATmaterial For 64 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\win_b64\startup\materials\Fluids and Mixtures.CATmaterial where X-X.X.X represents the version used.

3.

In the Fluid tab, click the

icon (Air).

4.

Hold the mouse button, and drag and drop the material on to the flow volume in the graphics window. This includes the selected material (Air) in your case setup.

5.

118

Close the Library dialog box. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Boundary Conditions

5.13. Boundary Conditions 1.

Specify the inlet boundary conditions. a.

Click the

icon to open the Inlet Boundary Condition dialog box.

Note There is a single inlet and outlet boundary in this example, hence they are automatically selected in the Supports field in Boundary Condition dialog boxes.

2.

b.

Ensure that 1 Inlet boundary is selected for Supports

c.

Enable Velocity and set the value to 10 m_s.

d.

In the Inlet Direction drop-down list, select Normal to Support.

e.

Select Long tube, pipe or duct from the Source of Flow drop-down list.

f.

Click OK to validate.

Specify the outlet boundary conditions. a.

Click the

icon to open the Outlet Boundary Condition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

119

External Flow Calculations Over a Blimp

3.

b.

Ensure that 1 Outlet boundary is selected for Supports

c.

Enable Gauge Pressure (static) and retain the value of 0 N_m2.

d.

Click OK to validate.

Save the CATIA V5 analysis files. File → Save Management...

5.14. Mesh Generation In this step, you will compute the mesh first and then iterate the solution. 1.

Click the

icon to open the Compute dialog box.

a.

Select the Mesh only in the Compute drop-down list.

b.

Click OK in the Compute dialog box to launch the computations. In this step, only the mesh is computed, therefore calculations will not take much time.

2.

120

Observe the mesh quality to ensure that the mesh is suitable for the simulation. a.

Right-click on the Nodes and Elements set and select Mesh Visualization in the contextual menu.

b.

Click the

icon to open the Quality Analysis dialog box. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Mesh Generation

c.

Click the

icon to open the Quality Report dialog box.

The Quality Report gives you details on items such as average skewness, maximum skewness of the cells in the domain, and cell count of the domain.

d.

Click

the icon to activate the mesh visualization mode.

e.

Click the box.

f.

Select Y and disable Exact mesh cut.

g.

Move the plane using mouse so that the new mesh at the blimp surface is visible (Figure 5.13: Cutting Plane Through Mesh (p. 122) and Figure 5.14: Zoomed-in View of Mesh Near Blimp Surface (p. 122)).

icon in the Mesh Analysis Tools toolbar to open the Cutting Plane Definition dialog

This step is required just to make sure that you have created a fine mesh at the blimp surface.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

121

External Flow Calculations Over a Blimp Figure 5.13: Cutting Plane Through Mesh

Figure 5.14: Zoomed-in View of Mesh Near Blimp Surface

h.

Display the cells based on the skewness (Figure 5.15: Cells Display Based on Skewness Criteria (p. 123)). i.

Keep the plane cut.

ii.

Open the Quality Analysis dialog box.

iii.

Select Skewness criteria and click Apply. This displays cells on the plane cut in different colors. Blue color indicates good quality cells, yellow color indicates bad quality cells, and red color indicates the cell of worst quality.

iv.

122

Close the Cutting Plane Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Solution v.

Right-click the blimp_without_box_FluentPart option located below the Link Manager.1 variable and select the Hide/Show option in the contextual menu that appears.

Figure 5.15: Cells Display Based on Skewness Criteria

5.15. Solution 1.

Double-click on Initialization Values.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Initialization Values dialog box. •

2.

Double-click on Fluent Solution.1 below the Fluent case feature in the specification tree to open the Fluent Solution dialog box. •

3.

Click Reset All and OK to validate.

Click Reset All and OK to validate.

Define a force monitor to measure the drag. a.

Right-click on Monitors.1 option below the Fluent case feature in the FfC specification tree.

b.

Select Force Monitor option in the contextual menu that appears to open the Force Monitor dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

123

External Flow Calculations Over a Blimp

c.

Click the Wall (FluidToSolid.1.1_1).4 option located below Groups.1 feature in the specification tree. This updates the Supports text entry field in the Force Monitor dialog box.

Note The wall selected should represent the blimp body.

4.

124

d.

Select Drag in the Moment or Force Type drop-down list.

e.

Set X to 1 and other coordinates to 0 in the Force Vector group-box.

f.

Click OK to validate.

Start the computations.

a.

Click the

icon again to open the Compute dialog box.

b.

Select Analysis Case Solution Selection in the drop-down list.

c.

Click the Fluent Solution.1 variable located below Fluent case in the specification tree.

d.

Click OK in the Compute dialog box to launch the computations. The solution converges in approximately 150 iterations. The residuals and the drag monitor are as shown in the Figure 5.16: Residuals (p. 125) and Figure 5.17: Drag Monitor (p. 125).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Solution Figure 5.16: Residuals

Figure 5.17: Drag Monitor

5.

Save the session. File → Save Management...

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

125

External Flow Calculations Over a Blimp

5.16. Postprocessing 1.

Click the

icon to display the contours of total pressure. (Figure 5.18: Contours of Total Pressure (p. 126))

FfC displays contours of the entire model. You have to make settings to display the total pressure contours of the only blimp surface. •

Double-click on the color map to open the Color Map Edition dialog box. •

Click

and enable Smooth in the Color Edition dialog box.

Figure 5.18: Contours of Total Pressure

2.

Display the contours of velocity vectors on a cut plane (Figure 5.19: Setting the Cut Plane Position (p. 127)).

a.

Click the

b.

Double-click Velocity.1 to open the Image Edition dialog box. •

126

icon

Select Symbol in the Visu tab and click OK.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing Figure 5.19: Setting the Cut Plane Position

3.

c.

Click

and set the cut plane position as shown in Figure 5.19: Setting the Cut Plane Position (p. 127).

d.

Right-click Links Manager.1 in the specification tree and select Hide/Show to show the blimp geometry.

Double-click the color map to open the Edit Color Map dialog box. •

Enable Impose max and Impose min and set them to 11 and 6.5, respectively. This will show the stagnation points at the nose and the tail of the blimp (Figure 5.20: Contours of Velocity Vectors on a Cut Plane (p. 127)). Figure 5.20: Contours of Velocity Vectors on a Cut Plane

4.

Display the velocity path lines (Figure 5.21: Velocity Path Lines (p. 128)).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

127

External Flow Calculations Over a Blimp

•

Click the

icon to display the velocity path lines.

See Appendix B: Displaying Velocity Path Lines (p. 129) for details on displaying path lines.

Note You have to choose the Shading with Material ( so that the path lines are displayed in color.

) icon from the View toolbar

Figure 5.21: Velocity Path Lines

5.17. Summary In this tutorial you learned how to setup the case for external ow volume cases, specify local mesh parameters to get the finer mesh at the required regions in the geometry, and observe the mesh quality using a cut plane. You also learned how to initialize the calculations only for the mesh generation and then continue for the ow calculations. You may want to generate the report of your simulation. For details on report generation, refer to Volatile Gas Emission Modeling Using Species Transport Model (p. 173).

5.18. Appendix A: Displaying Contours of only the Blimp Surface 1.

128

Right-click on Total Pressure (fringe).1 in the Fluent Solution.1 set and select Properties in the contextual menu to open the Image Edition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Appendix B: Displaying Velocity Path Lines

2.

Select Wall (FluidToSolid.1.1 1).4, representing the blimp surface, from Available Groups using the button.

5.19. Appendix B: Displaying Velocity Path Lines 1.

Define a limited cut plane group from which the particles should be released.

•

Click

to open the Limited Cut Plane Group dialog box and create the cut.

Enter values for the plane so that it is positioned as shown. The path lines generated from it should pass through the immediate space around the blimp. 2.

Disable On boundary in the Color Map Edition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

129

External Flow Calculations Over a Blimp

To open the Color Map Edition dialog box, double-click on the color band of the contours. 3.

Double-click the Velocity path lines (norm).1 option created in the Fluent Solution.1 set of the specification tree to open the Image Edition dialog box. a.

Select Path Lines under Types.

b.

Under Release from Surfaces, select Limited Cut Plane Group.1 as the Inlet. Decrease the density of path lines for better viewing.

c.

Click Options... to open the Visualization Options dialog box. •

d.

130

Set Path skip to 5.

Click OK to close the Image Edition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 6: Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model 6.1. Introduction Many engineering problems involve rotating flow domains. One example is mixing tank that is typically used in chemical industry. For problems, where all the moving parts (fan/rotor blades, hub and shaft surfaces, etc.) are rotating at a prescribed angular velocity, and the stationary walls (e.g., tank outer wall, duct walls) are surfaces of revolution with respect to the axis of rotation, the entire domain can be referred to as a single rotating frame of reference. However, when each of several parts is rotating about a different axis of rotation or about the same axis at different speeds, or when the stationary walls are not surfaces of revolution (such as the volute around a centrifugal blower wheel), a single rotating coordinate system is not sufficient to immobilize the computational domain so as to predict a steady-state flow field. This scenario can be taken care of using Multiple Rotating Reference Frame (MRF) model available in FfC. This tutorial illustrates the procedure for setting up and solving a problem using the MRF capability. This tutorial demonstrates how to do the following: • Identify and separate fluid zone around the rotating part. • Change group types. • Specify rotation to the fluid zone around the rotating part. • Set rotation to rotating parts (wall zones). • Using force monitor to determine momentum force.

6.2. Prerequisites This tutorial assumes that you are familiar with the menu structure in FfC. It also assumes that you have read the Getting Started (p. 1) portion of the Tutorial Guide and completed Internal Flow Calculation (p. 9). Some of the steps in setup and solution procedure will not be shown explicitly.

Note It is assumed that you have the FMS and FMD licenses available. If you do not have FMD and FMS (CATIA V5) licenses then you will not be able to generate mesh as explained in the tutorial. Initialize the calculations for flow and perform postprocessing

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

131

Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model

6.3. Problem Description This problem considers a generic mixing tank with only one rotor. The rotor is fitted at the bottom end of a shaft entering the tank from the top. A domain is shown in Figure 6.1: Mixing Tank Schematic (p. 132). The rotor consists of 4 blades and is rotating with an angular velocity of 500 rpm. The flow is assumed to be turbulent. Figure 6.1: Mixing Tank Schematic

6.4. Preparation 1.

Copy the CATIA V5 file, mixer_inclined_shaft-new.CATPart to your working directory.

2.

Start the FfC environment.

6.5. Setting the Options Tools → Options → Analysis & Simulation → Fluent Options 1.

132

Click the General tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 6.2: Options Dialog Box — General

a.

Enter the path for the ANSYS Fluent solver in the text entry box next to Folder for solver.

Note The ANSYS Fluent solver is provided with the installed FfC package. You can use the Browse button to specify the path for the solver: For 32 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/ntx86 For 64 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/win64 Similarly, specify the path for the external postprocessor, CFD-Post (or FloWizard) executable.

b.

Set the remaining parameters as shown in Figure 6.2: Options Dialog Box — General (p. 133).

Note You can specify the Maximum number of iterations. For this tutorial the recommended value is 2500 iterations. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

133

Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model 2.

Click the Data Management tab in the Options dialog box. a.

Enter the path for Temporary files, FLUAnalysisComputations file and FLUAnalysisResults file in the External Storage folder group box. You can use the Browse button to specify the path. The analysis files will be saved in the temporary folders while FfC is computing the solution. The analysis will be saved to its permanent location when the computation is complete.

b.

Set the remaining parameters as shown in Figure 6.3: Options Dialog Box — Data Management (p. 134). Figure 6.3: Options Dialog Box — Data Management

3.

134

Click the Advanced Parameters tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 6.4: Options Dialog Box — Advanced Parameters

• 4.

Set the parameters as shown in Figure 6.4: Options Dialog Box — Advanced Parameters (p. 135).

Click the Customization tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

135

Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model Figure 6.5: Options Dialog Box — Customization

a.

Enable Advanced Turbulence Models.

Note If the Advanced Turbulence Models option is disabled, then the default turbulence model (k-epsilon, Realizable) for turbulent flows and Reynolds Stress Model for turbulence with strong swirl will be selected without any further access to more turbulence models.

b.

Enable Advanced Boundary Condition Parameters.

Note The Advanced Boundary Condition Parameters option allows specification of heat generation rate for wall boundary.

c.

Enable Use solution steering by default.

Note The Use solution steering by default option enables solution steering mechanism to control the solution convergence automatically.

136

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Extracting Flow Volume d.

Enable Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" . The Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" option uses second order solutions after 75% accuracy settings during mesh definition. If this option is disabled, then first order solution is computed for all slider positions.

e. 5.

Select Residuals from the Convergence Criterion drop-down list.

Click OK to close the Options dialog box.

6.6. Reading the File 1.

Read the CATIA V5 file (mixer_inclined_shaft-new.CATPart) in FLUENT for CATIA V5. File → Open... This opens the File Selection dialog box, using which you can select the file to be read.

2.

Select the file, mixer_inclined_shaft-new.CATPart. By default, the file is opened in the Part or Product workbench of CATIA V5.

Tip To use the entire screen space, remove the specification tree on the left-hand side by selecting the View → Specifications menu item or pressing the F3 key on your keyboard.

6.7. Starting FLUENT for CATIA V5 1.

Launch the FfC workbench. Start → Analysis & Simulation → FLUENT for CATIA V5 This updates the graphics display. The specification tree on the left-hand side also gets updated and displays the analysis-related parameters.

2.

In the Options dialog box, specify the location of the directory where you want to store the solver files.

6.8. Extracting Flow Volume Click the icon or double-click the Geometry Definition.1 option located below the Environment.1 feature in the specification tree to open the Geometry Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

137

Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model

1.

Select flow volume from the Geometry definition drop-down list.

2.

Retain No selection for Inlet.

3.

Click in the text entry field next to Outlet, zoom in the top side of the tank and select the tank top surface as the outlet.

4.

Make sure that Merge all Fluids is deactivated.

5.

Click OK to validate and close the Geometry Definition dialog box. This extracts the flow volume and the graphics window gets updated to show the extracted flow volume. Figure 6.6: Flow Volume

6.

138

Once the flow volume is extracted as shown above, FfC will create group of publications located below Groups.1.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Physics Figure 6.7: Groups

a.

Double click on Outlet Boundary.1 to open the Group of Boundaries dialog box.

b.

Select Symmetry from the Type drop-down list.

c.

When the Type is changed to Symmetry the name of the boundary group will be modified and the color of the group will also be changed.

6.9. Physics Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the FLUENT for CATIA V5 specification tree to open the Physical Model Definition dialog box.

1.

Disable Accounting for Temperature Effect. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

139

Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model 2.

Select Turbulent in the Flow Type drop-down list.

3.

Select k-epsilon, Realizable in the Turbulence Model drop-down list.

4.

Select steady in the Time drop-down list.

5.

Click OK to validate.

6.10. Meshing Parameters Click the icon or double-click the Mesh Definition.1 option located below the Environment.1 feature in the specification tree to open the Mesh Definition dialog box.

1.

Click

icon to select the optimized surface mesh.

2.

Move the slide bar towards Fine till the number above it shows a value of 75. As you move the slide bar, other parameters will change accordingly. Use the Reset All button to set all the field values to their default values. Note that, if you don't use the Reset All button, the values from the previous session will be taken by FfC for meshing.

3.

Click the Global tab and enter 4.4 mm for Critical Length.

4.

Retain the default values for other parameters.

140

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Materials

5.

Click OK to close the Mesh Definition dialog box.

6.11. Materials In this step, apply material to the outer fluid zone using the drag and drop method.

1.

Click the

icon to open the Library dialog box.

2.

Select the FLUENT for CATIA V5 fluids and mixtures materials library. To open the materials library, you have to specify the path where it is stored. For 32 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\intel_a\startup\materials\Fluids and Mixtures.CATmaterial For 64 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\win_b64\startup\materials\Fluids and Mixtures.CATmaterial where X-X.X.X represents the version used.

3.

Click and hold the mouse button on water-liquid material icon.

4.

Drag and drop the material on to the outer fluid zone displayed in the graphics window.

5.

Close the Library dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

141

Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model

6.12. Naming the Fluid Zones 1.

Click the

icon.

2.

Select any zone in the specification tree under Properties.1. Make the outer tank wall transparent. The selected zone gets highlighted. Identify the fluid zone around the rotor blades.

3.

Rename the smaller zone around the rotor-blades as rotating-zone and rename the other fluid zone representing tank volume as outer-fluid-zone.

4.

Create a separate group for faces of the shaft. a.

Set the view from rendering style to perspective. View → Render Style → Perspective

b.

142

Click the

icon to open the Group of Boundaries dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Naming the Fluid Zones Figure 6.8: Shaft-Rotating-Zone

c.

Now zoom in the model around the impeller to select the faces of the shaft lying in the rotating zone in the Support text entry (Figure 6.8: Shaft-Rotating-Zone (p. 143)).

d.

Select wall as the Type.

e.

Specify shaft-rotating-zone as the Name.

f.

Select Wall (FluidtoSolid.3.0 1).3 under Groups.1 in the specification tree as shown in Figure 6.9: Rotor-Blades (p. 143) and rename it as rotor-blades. Figure 6.9: Rotor-Blades

g.

Similarly, rename a group for the tank-outer-wall as shown in Figure 6.10: Tank-Outer-Wall (p. 144).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

143

Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model Figure 6.10: Tank-Outer-Wall

h.

Similarly, rename a group for shaft-not-rotating-zone as shown in Figure 6.11: Shaft-Not-RotatingZone (p. 144). Figure 6.11: Shaft-Not-Rotating-Zone

6.13. Specify the MRF Zone Note The mixing tank is divided into two fluid zones, due to which the MRF model is applied here. A rotation speed is specified for the impeller blades, which is bounded by surfaces of revolution. The other fluid zone is specified as stationary. The flow volume is divided into two fluid zones as mixing tanks typically have baffles on the outside walls, which are not surfaces of revolution. 1.

144

Under Properties.1 in the specification tree, double click on the Property corresponding to the inner fluid zone Flow Property Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Specify the MRF Zone

2.

Select Moving Reference Frame in the Motion Type drop-down list.

3.

Click the

icon to open the Motion of Rotating Machinery dialog box.

a.

Select one vertical face of the shaft as Support for direction calculation.

b.

Enter 500 turn_mn for Rotational Speed.

c.

Select Clockwise for rotation direction and click OK. The direction of rotation should be clockwise with reference to the top of the tank. Use Clockwise or Counter Clockwise options to get the desired rotational direction.

4.

Click OK in the Flow Property Definition dialog box.

5.

Click the

icon.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

145

Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model

6.

7.

146

a.

Click the text entry next to the Supports and select rotor-blades in specification tree under Groups.1.

b.

Change the Name to rotor-blades.

c.

Select Rotating in the Motion Type scrolling list.

d.

Select Relative to adjacent fluid region in the Reference Frame scrolling list.

e.

Enable Clockwise and click OK.

Similarly, define new wall boundary conditions using the same parameters as mentioned above. a.

Select the group shaft-rotating-zone as support.

b.

Rename this wall boundary as shaft-rotating-zone.

Click the

icon.

a.

Click the text entry next to Supports and select shaft-not-rotating-zone in specification tree under Groups.1.

b.

Change the Name to shaft-not-rotating-zone.

c.

Select Rotating in the Motion Type scrolling list. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Solution d.

Select Absolute in the Reference frame scrolling list.

e.

Enter 500 turn_mn for Rotational Speed.

f.

Select the shaft outer wall for Support for direction calculation.

g.

Enable Clockwise and click OK.

6.14. Solution 1.

Double-click on Initialization Values.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Initialization Values dialog box. •

2.

3.

Click Reset All and OK to validate.

Double-click on Fluent Solution.1 in the specification tree to open the Fluent Solution dialog box.

a.

Click Reset All.

b.

Ensure that Use solution steering is enabled.

c.

Ensure that Max number of iterations is enabled and set to 2500.

d.

Click OK to validate.

Click the a.

icon to open the Compute dialog box.

Select All and Default Solution Option in the two drop-down lists.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

147

Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model b.

Click OK to validate and start the computations.

Note Solution converges after around 2000 iterations. It will take a few hours to complete the solution. You can postprocess the results by interrupting the computations. Use Stop Computation button to stop the calculations.

4.

Save the analysis files as mix_tank_Analysis1.CATAnalysis file and propagate directory. File → Save Management...

6.15. Postprocessing 1.

Click the

icon to open the Residual Images dialog box.

Figure 6.12: Residual Plot

2.

Show velocity vectors on a cut plane.

a.

Click

icon.

Velocity contours are displayed and this is listed under Fluent Solution.1 as Velocity.1.

148

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing

b.

Double click on Velocity.1 to open the Image Edition dialog box.

c.

In the Image Edition box under Visu tab, select Symbol as Type.

Note Velocity vectors will be displayed on boundaries. Click the Options... tab to manipulate arrows.

d.

Click OK to verify. To include parts of the mixing tank in this image right click on the Link Manager.1 and in the contextual menu, click Hide/Show. For a better view you may have to make some parts transparent or hide them.

e.

Click the

icon to open the Cut Plane Analysis dialog box

Keep the settings as shown in Figure 6.13: Cut Plane Analysis Dialog Box (p. 150).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

149

Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model Figure 6.13: Cut Plane Analysis Dialog Box

f.

Adjust the position of the plane using the compass, so that the plane cuts the tank vertically into two equal parts.

Note You can also double-click on the compass to adjust the cutting plane. This opens the Parameters for Compass Manipulation dialog box.

g.

150

Similarly, we can show velocity vectors on a horizontal cutting plane passing from the blades. See Figure 6.14: Velocity Vectors (p. 151).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing Figure 6.14: Velocity Vectors

3.

Show static pressure contours on a cut plane. a.

Click the

icon.

Static pressure contours are displayed and it is listed under Fluent Solution.1 as Pressure( nodal values).1. You can include parts of the mixing tank in this image. b.

4.

The procedure to show the pressure contour on a cut plane is same as you performed in the previous step.

Show turbulence kinetic energy contours on the blades. a.

Click the

icon.

Contour of turbulent kinetic energy will be displayed and this will be listed under Fluent Solution.1 as Turbulence Kinetic Energy (average iso).1. b.

Double click Turbulence Kinetic Energy (average iso).1 to open the Image Edition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

151

Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model

c.

Click the Selection tab and select rotor-blades under Available Groups and click the down arrow. rotor-blades is available under Activated Groups and the contours are shown on the rotorblades.

6.16. Summary In this tutorial you learned how to setup the case for rotating impellers, blowers using Multiple Reference Frame (MRF) approach embedded in FfC. This approach can also be used for turbomachinery applications in which rotor-stator interaction is relatively weak, and the flow is relatively uncomplicated at the interface between the moving and stationary zones. You may want to generate the report of your simulation. For details on report generation, refer to Volatile Gas Emission Modeling Using Species Transport Model (p. 173).

152

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 7: Compressible Flow Nozzle 7.1. Introduction The purpose of this tutorial is to compute the flow through a compressible nozzle. In this tutorial you will learn how to: • Model compressible flow. • Set boundary conditions for the compressible nozzle geometry. • Use Full Multigrid (FMG) initialization to obtain faster convergence. • Compute the solution for a quadrant of the symmetric geometry to increase the speed of the calculations. • Perform postprocessing to analyze the results.

7.2. Prerequisites This tutorial assumes that you are familiar with the menu structure in FfC. It also assumes that you have read the Getting Started (p. 1) portion of the Tutorial Guide and completed Internal Flow Calculation (p. 9). Some of the steps in setup and solution procedure will not be shown explicitly.

Note It is assumed that you have the FMS and FMD licenses available. If you do not have FMD and FMS (CATIA V5) licenses then you will not be able to generate mesh as explained in the tutorial. Initialize the calculations for flow and perform postprocessing

7.3. Problem Description The problem considers the flow through a compressible nozzle. The geometry of the nozzle is shown in Figure 7.1: Problem Schematic (p. 154).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

153

Compressible Flow Nozzle Figure 7.1: Problem Schematic

7.4. Preparation 1.

Copy the CATIA V5 file, compressible_nozzle.CATPart and the journal file, nozzle.jou to your working directory.

2.

Start the FfC environment.

7.5. Setting the Options Tools → Options → Analysis & Simulation → Fluent Options 1.

154

Click the General tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 7.2: Options Dialog Box — General

a.

Enter the path for the ANSYS Fluent solver in the text entry box next to Folder for solver.

Note The ANSYS Fluent solver is provided with the installed FfC package. You can use the Browse button to specify the path for the solver: For 32 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/ntx86 For 64 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/win64 Similarly, specify the path for the external postprocessor, CFD-Post (or FloWizard) executable.

2.

b.

Enable Use double precision solver.

c.

Set the remaining parameters as shown in Figure 7.2: Options Dialog Box — General (p. 155).

Click the Data Management tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

155

Compressible Flow Nozzle a.

Enter the path for Temporary files, FLUAnalysisComputations file and FLUAnalysisResults file in the External Storage folder group box. You can use the Browse button to specify the path. The analysis files will be saved in the temporary folders while FfC is computing the solution. The analysis will be saved to its permanent location when the computation is complete.

b.

Set the remaining parameters as shown in Figure 7.3: Options Dialog Box — Data Management (p. 156). Figure 7.3: Options Dialog Box — Data Management

3.

156

Click the Advanced Parameters tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 7.4: Options Dialog Box — Advanced Parameters

• 4.

Set the parameters as shown in Figure 7.4: Options Dialog Box — Advanced Parameters (p. 157).

Click the Customization tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

157

Compressible Flow Nozzle Figure 7.5: Options Dialog Box — Customization

a.

Enable Advanced Turbulence Models.

Note If the Advanced Turbulence Models option is disabled, then the default turbulence model (k-epsilon, Realizable) for turbulent flows and Reynolds Stress Model for turbulence with strong swirl will be selected without any further access to more turbulence models.

b.

Enable Advanced Boundary Condition Parameters.

Note The Advanced Boundary Condition Parameters option allows specification of heat generation rate for wall boundary.

c.

Disable Use solution steering by default.

d.

Disable Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" . For more information on the Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" control, refer to the FLUENT for CATIA V5 User's Guide.

158

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Extracting Flow Volume e. 5.

Select Residuals from the Convergence Criterion drop-down list.

Click OK to close the Options dialog box.

7.6. Reading the File 1.

Read the CATIA V5 file (compressible_nozzle.CATPart) in FLUENT for CATIA V5. File → Open... This opens the File Selection dialog box, using which you can select the file to be read.

2.

Select the file, compressible_nozzle.CATPart. By default, the file is opened in the Part or Product workbench of CATIA V5.

Tip To use the entire screen space, remove the specification tree on the left-hand side by selecting the View → Specifications menu item or pressing the F3 key on your keyboard.

7.7. Starting FLUENT for CATIA V5 1.

Launch the FfC workbench. Start → Analysis & Simulation → FLUENT for CATIA V5 This updates the graphics display. The specification tree on the left-hand side also gets updated and displays the analysis-related parameters.

2.

In the Options dialog box, specify the location of the directory where you want to store the solver files.

7.8. Extracting Flow Volume In this step, you will define the inlet and outlet edges and extract the flow volume. Refer Figure 7.1: Problem Schematic (p. 154) to select the correct edges for the inlet and outlet edges. 1.

Click the icon or double-click the Geometry Definition.1 option located below the Environment.1 feature in the specification tree to open the Geometry Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

159

Compressible Flow Nozzle

a.

Enable Geometry is Symmetric.

b.

Click the

c.

Click on the field next to Plane of Symmetry and select the XY and ZX planes from the graphics window.

d.

Select solid model from the Geometry definition drop-down list.

e.

Select Edges from the Selection mode drop-down list.

f.

Click on the field next to Dry reference Surface, zoom-in on the geometry, and select the outer surface of the nozzle.

g.

Retain the default selection of No propagation from the Propagation Type drop-down list.

h.

Click on the field next to Inlet, zoom-in on the geometry, and select the inner edges of the smaller diameter opening of the nozzle.

icon to orient the geometry to isometric view.

When you move the pointer near the inlet, the edges around the pointer get highlighted. Select the appropriate face as shown in Figure 7.6: Selected Inlet Edges (p. 161).

160

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Extracting Flow Volume Figure 7.6: Selected Inlet Edges

i.

Click on the field next to Outlet, zoom-in on the geometry, and select the inner edges of the larger diameter opening of the nozzle, as shown in Figure 6.7. Figure 7.7: Selected Outlet Edges

j.

Click OK to validate. This creates a flow volume for the geometry. The flow volume is displayed in the graphics window. The specification tree on the left-hand side also gets updated to show the relevant parameters. The graphics window also gets updated to display the quadrant of symmetry as shown in Figure 7.8: Figure showing a Quadrant of Symmetry (p. 162).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

161

Compressible Flow Nozzle Figure 7.8: Figure showing a Quadrant of Symmetry

k.

2.

Select a quadrant of symmetry so that the symmetry plane is clearly visible and click OK in the Symmetry dialog box (Figure 7.8: Figure showing a Quadrant of Symmetry (p. 162)).

Click OK to validate and close the Geometry Definition dialog box.

7.9. Meshing Parameters Note If FMS and FMD licenses are not available, you can generate the surface mesh using Octree 2D mesher.

1.

162

Click the icon or double-click the Mesh Definition.1 option located below the Environment.1 feature in the specification tree to open the Mesh Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Meshing Parameters

2.

Click the Reset All button.

3.

Move the slide bar towards Fine till the number above it shows a value of 75. Some of the parameters in the Mesh Definition dialog box are linked to the position of the slider bar. Therefore, depending on the mesh type, moving the slider changes the values of these parameters.

4.

Use the default Optimized Surface mesher as the Mesh Type.

5.

Click the Global tab. a.

Enter 0.101 mm for Critical Length.

b.

Enable Min Mesh size and enter a value of 0.8 mm.

c.

Enable Mesh size and enter a value of 8 mm.

6.

Retain the default values in the Geometry and Surface mesh tabs.

7.

Click the Volume Mesh tab, enable Size progression, and enter a value of 1.15. a.

Enable Use TGrid for Fluids.

b.

Ensure that fluid walls only is selected from the Grow boundary layers from drop-down list.

c.

Select Uniform Growth from the Boundary Layer Method drop-down list.

d.

Enter 1 mm for First Height, 4 for Number of layers, 1.1 for Growth rate, and 60 deg for Max angle change.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

163

Compressible Flow Nozzle 8.

Click OK to validate and close the Mesh Definition dialog box.

7.10. Physics Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the FLUENT for CATIA V5 specification tree to open the Physical Model Definition dialog box.

1.

Enable Accounting for Temperature Effect.

2.

Select Compressible in the Flow Property drop-down list.

3.

Retain the default settings for the remaining parameters and click OK to validate.

7.11. Materials In this step, apply material to the outer fluid zone using the drag and drop method.

1.

Click the

icon to open the Library dialog box.

2.

Select the FLUENT for CATIA V5 fluids and mixtures materials library. To open the materials library, you have to specify the path where it is stored. For 32 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\intel_a\startup\materials\Fluids and Mixtures.CATmaterial For 64 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\win_b64\startup\materials\Fluids and Mixtures.CATmaterial where X-X.X.X represents the version used.

3.

In the Fluid tab, select Air.

4.

Hold the mouse button, and drag and drop the material on to the flow volume in the graphics window.

164

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Boundary Conditions This includes Air in your case setup.

5.

Close the Library dialog box. The list below the Materials.1 feature in the specification tree is automatically updated to show Air.1.

7.12. Boundary Conditions 1.

Set the boundary conditions at the inlet opening.

a.

Click the

icon to open the Inlet Boundary Condition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

165

Compressible Flow Nozzle There is a single inlet and outlet boundary in this example, hence they are automatically selected in the Supports field in Boundary Condition dialog boxes.

2.

b.

Ensure that 1 Inlet boundary is selected for Supports.

c.

Enter 101325 N_m2 for Gauge Pressure (Total).

d.

Enter 310.92 K for Temperature.

e.

Click OK in the Inlet Boundary Condition dialog box to validate.

Set the boundary conditions at the outlet opening.

a.

Click the

icon to open the Outlet Boundary Condition dialog box.

b.

Ensure that 1 Outlet boundary is selected for Supports.

c.

Enter 91192.5 N_m2 for Gauge Pressure (Static).

d.

Enter 293.17 K for Temperature.

e.

Click OK to validate.

7.13. Operating Conditions 1.

Double-click Operating Conditions.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Operating Conditions dialog box.

2.

Enter 0 N_m2 for Operating Pressure.

166

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

ANSYS Fluent Solution Settings 3.

Click OK to close the Operating Conditions dialog box.

7.14. Journal Customization 1.

Double-click Journal customization.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Journal Customization dialog box.

2.

Enable Pre-Iteration journal file:.

3.

Click the button below Pre-Iteration journal file: to open the Select File dialog box and select the nozzle.jou file from your working directory.

4.

Click OK to close the Journal Customization dialog box. Full Multigrid (FMG) Initialization is performed in the journal customization. In the FMG iteration, the inviscid Euler equations are solved to obtain an approximate solution. This solution is generally better than constant initial values and thus helps in faster convergence. FMG Initialization is especially useful for compressible flows.

7.15. ANSYS Fluent Solution Settings 1.

Save the CATIA V5 analysis files. File → Save Management...

a.

Select the Analysis1.CATAnalysis file and click the Save As... button.

b.

Rename the Analysis1.CATAnalysis file to compressible-nozzle_Analysis1.CATanalysis.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

167

Compressible Flow Nozzle c.

Click the Propagate directory button and click OK to close the Save Management dialog box.

Note You specify the path where all the analysis files must be saved. Using Save Management... saves the analysis file along with other solution files written by FfC.

2.

3.

168

Double-click Initialization Values.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Initialization Values dialog box.

a.

Click Reset All.

b.

Enable X Velocity and enter a value of 20 m_s.

c.

Disable Temperature and click OK to close the Initialization Values dialog box.

Double-click Fluent Solution.1 below the Fluent Case feature in the specification tree to open the Fluent Solution dialog box.

a.

Click Reset All.

b.

Move the slider bar till it shows a value of 1.

c.

Click the Relaxation Settings... button to open the Relaxation Settings dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Solution

i.

Set the parameters as shown in the dialog box.

ii.

Click OK to close the Relaxation Settings dialog box.

d.

Enter 2000 for Max number of iterations.

e.

Click OK to close the Fluent Solution dialog box.

7.16. Solution In this step, you will generate the mesh and iterate the solution. Though FfC allows you to generate the mesh and start the flow computations separately, here you will perform these steps simultaneously. 1.

Click the

icon to open the Compute dialog box.

2.

Select All and Default Solution Option in the two drop-down lists.

3.

Click OK to validate and start the computations.

Note FLUENT for CATIA V5 will start the computation process and the progress will be displayed in the Fluent Calculations Progression dialog box. Click the Stop Computation button if you want to interrupt the calculations. The solution will converge in approximately 225 iterations. 4.

Click the

icon to display the scaled residuals.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

169

Compressible Flow Nozzle

7.17. Postprocessing 1.

Click the

icon to display the contours of static pressure.

Figure 7.9: Contours of Static Pressure

2.

170

Click the

icon to display the contours of Mach number.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Summary Figure 7.10: Contours of Mach number

The Mach number contours show that the flow is subsonic (Mach number is approximately 0.9) near the throat of the nozzle.

7.18. Summary This tutorial demonstrated how to compute the flow through a compressible nozzle. It showed how to define symmetry planes for a geometry and compute for a quadrant of the geometry to increase the speed of the calculations. It also demonstrated the use of FMG initialization in compressible flows to achieve faster convergence. In order to achieve better convergence, it is always advisable to avoid backflow (reversed flow) from the exit of the domain, especially if the flow is supersonic. In this case, there was some backflow in a small number of faces, but there was no problem in convergence, since the flow was subsonic. If you face convergence issues due to backflow, you may want to extend the domain downstream to avoid reversed flow. You may want to generate the report of your simulation. For details on report generation, refer to Volatile Gas Emission Modeling Using Species Transport Model (p. 173).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

171

172

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 8:Volatile Gas Emission Modeling Using Species Transport Model 8.1. Introduction This tutorial demonstrates how to model fluid exhaust streams emitted from an office photo-copy machine. In this tutorial you will learn how to: • Understand the use of edge propagation to extract flow volume. • Use of reference surface to define edge propagation. • Use species transport model in FLUENT for CATIA V5. • Modify the pre-defined species mixture material to suit your application. • Rename and change group types. • Model the dispersion of gaseous species throughout a room. • Postprocess the species transport quantities.

8.2. Prerequisites This tutorial assumes that you are familiar with the menu structure in FfC. It also assumes that you have read the Getting Started (p. 1) portion of the Tutorial Guide and completed Internal Flow Calculation (p. 9). Some of the steps in setup and solution procedure will not be shown explicitly.

Note It is assumed that you have the FMS and FMD licenses available. If you do not have FMD and FMS (CATIA V5) licenses then you will not be able to generate mesh as explained in the tutorial. Initialize the calculations for flow and perform postprocessing

8.3. Problem Description A room, shown in Figure 8.1: Problem Schematic (p. 174), contains a photo-copier machine with rear sources that emit waste gases. Other objects in the room include a person, a trash can, a file cabinet, closets, and exhaust vents. The goal of the simulation is to report the concentration of total volatile organic compounds (VOCs). VOCs, which are normally gaseous hydrocarbons, are criteria pollutants that can be found in all non-industrial environments. These chemicals are produced by a wide range of sources, and are of particular interest in addressing indoor air quality (IAQ) concerns. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

173

Volatile Gas Emission Modeling Using Species Transport Model Figure 8.1: Problem Schematic

8.4. Preparation 1.

Copy the CATIA V5 file, photo-copy-machine.CATPart to your working directory.

2.

Start the FfC environment.

8.5. Setting the Options Tools → Options → Analysis & Simulation → Fluent Options 1.

174

Click the General tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 8.2: Options Dialog Box — General

a.

Enter the path for the ANSYS Fluent solver in the text entry box next to Folder for solver.

Note The ANSYS Fluent solver is provided with the installed FfC package. You can use the Browse button to specify the path for the solver: For 32 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/ntx86 For 64 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/win64 Similarly, specify the path for the external postprocessor, CFD-Post (or FloWizard) executable.

b. 2.

Set the remaining parameters as shown in Figure 8.2: Options Dialog Box — General (p. 175).

Click the Data Management tab in the Options dialog box. a.

Enter the path for Temporary files, FLUAnalysisComputations file and FLUAnalysisResults file in the External Storage folder group box. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

175

Volatile Gas Emission Modeling Using Species Transport Model You can use the Browse button to specify the path. The analysis files will be saved in the temporary folders while FfC is computing the solution. The analysis will be saved to its permanent location when the computation is complete. b.

Set the remaining parameters as shown in Figure 8.3: Options Dialog Box — Data Management (p. 176). Figure 8.3: Options Dialog Box — Data Management

3.

176

Click the Advanced Parameters tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 8.4: Options Dialog Box — Advanced Parameters

• 4.

Set the parameters as shown in Figure 8.4: Options Dialog Box — Advanced Parameters (p. 177).

Click the Customization tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

177

Volatile Gas Emission Modeling Using Species Transport Model Figure 8.5: Options Dialog Box — Customization

a.

Enable Advanced Turbulence Models.

Note If the Advanced Turbulence Models option is disabled, then the default turbulence model (k-epsilon, Realizable) for turbulent flows and Reynolds Stress Model for turbulence with strong swirl will be selected without any further access to more turbulence models.

b.

Enable Advanced Boundary Condition Parameters.

Note The Advanced Boundary Condition Parameters option allows specification of heat generation rate for wall boundary.

c.

Disable Use solution steering by default.

d.

Enable Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" . For more information on the Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" control, refer to the FLUENT for CATIA V5 User's Guide.

178

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Extracting Flow Volume e. 5.

Select Residuals from the Convergence Criterion drop-down list.

Click OK to close the Options dialog box.

8.6. Reading the File 1.

Read the CATIA V5 file (photo-copy-machine.CATPart) in FLUENT for CATIA V5. File → Open... This opens the File Selection dialog box, using which you can select the file to be read.

2.

Select the file, photo-copy-machine.CATPart. By default, the file is opened in the Part or Product workbench of CATIA V5.

Tip To use the entire screen space, remove the specification tree on the left-hand side by selecting the View → Specifications menu item or pressing the F3 key on your keyboard.

8.7. Starting FLUENT for CATIA V5 1.

Launch the FfC workbench. Start → Analysis & Simulation → FLUENT for CATIA V5 This updates the graphics display. The specification tree on the left-hand side also gets updated and displays the analysis-related parameters.

2.

In the Options dialog box, specify the location of the directory where you want to store the solver files.

8.8. Extracting Flow Volume In this step, you will define the inlet and outlet edges and extract the flow volume. Refer Figure 8.1: Problem Schematic (p. 174) to select the correct edges for the inlet and outlet edges. 1.

Click the icon or double-click the Geometry Definition.1 option located below the Environment.1 feature in the specification tree to open the Geometry Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

179

Volatile Gas Emission Modeling Using Species Transport Model

2.

Select solid model from the Geometry definition drop-down list.

3.

Select Edges from the Selection mode drop-down list.

4.

Click on the field next to Dry reference Surface, zoom-in on the geometry, and select the outer surface of the ceiling.

5.

Select Point continuity from the Propagation Type drop-down list.

6.

Click on the field next to Propagation support surface, zoom-in on the geometry, and select the inner surface of the ceiling, as shown in Figure 8.6: Selected Inner Surface of Ceiling (p. 180). Figure 8.6: Selected Inner Surface of Ceiling

180

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Extracting Flow Volume 7.

Click on the field next to Inlet, zoom-in on the geometry, and select the inner edges of the three inlet vents. When you move the pointer near the inlet, the edges around the pointer get highlighted. When you select one edge, the remaining three adjoining edges will be selected automatically, since you are using edge propagation. Select the appropriate edge as shown in Figure 8.7: Selected Inlet Edges (p. 181). Figure 8.7: Selected Inlet Edges

8.

Select No propagation from the Propagation Type drop-down list.

9.

Click on the field next to Outlet, zoom-in on the geometry, and select the inner edges of the door and the inner edges of the outlet opening on the ceiling, as shown in Figure 8.8: Selected Outlet Edges (p. 182).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

181

Volatile Gas Emission Modeling Using Species Transport Model Figure 8.8: Selected Outlet Edges

10. Click OK to validate and close the Geometry Definition dialog box. This creates a flow volume for the geometry. The flow volume is displayed in the graphics window. The specification tree on the left-hand side also gets updated to show the relevant parameters.

8.9. Meshing Parameters Note If FMS and FMD licenses are not available, you can generate the surface mesh using Octree 2D mesher.

1.

182

Click the icon or double-click the Mesh Definition.1 option located below the Environment.1 feature in the specification tree to open the Mesh Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Physics

2.

Click the Reset All button.

3.

Retain the default position of the slider bar at 50. Some of the parameters in the Mesh Definition dialog box are linked to the position of the slider bar. Therefore, depending on the mesh type, moving the slider changes the values of these parameters.

4.

Use the default Optimized Surface mesher as the Mesh Type.

5.

Click the Global tab and enter 1.643 mm for Critical Length.

6.

Retain the default values in the Geometry tab.

7.

Click the Surface Mesh tab, enable Min face number, and enter 4. A Min face number of 4 signifies that at least four cells will be created on any face. By defining this parameter, the region between the room wall and the back side of the photocopy machine will be resolved properly (which is important from the analysis point of view).

8.

Click the Volume Mesh tab, enable Size progression, and enter a value of 1.1.

9.

Click OK to validate and close the Mesh Definition dialog box.

8.10. Physics Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the FLUENT for CATIA V5 specification tree to open the Physical Model Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

183

Volatile Gas Emission Modeling Using Species Transport Model

1.

Enable Accounting for Temperature Effect.

2.

Select Turbulent in the Flow Property drop-down list.

3.

Select k-epsilon, Realizable as the Turbulence Model.

4.

Select Incompressible ideal gas from the Flow Property drop-down list.

Note FLUENT for CATIA V5 will open a Warning dialog box, asking you to set the operating pressure in the Operating Conditions dialog box. Click OK in the Warning dialog box. You will set the operating pressure at a later stage of the tutorial.

5.

Select steady from the Time drop-down list.

6.

Select Species Transport from the Model Definition drop-down list.

7.

Click OK to validate.

8.11. Materials 1.

Click the a.

icon to open the Library dialog box.

Select the FLUENT for CATIA V5 fluids and mixtures materials library. To open the materials library, you have to specify the path where it is stored. For 32 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\intel_a\startup\materials\Fluids and Mixtures.CATmaterial For 64 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\win_b64\startup\materials\Fluids and Mixtures.CATmaterial

184

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Materials where X-X.X.X represents the version used. b.

Click the Mixture Material tab and select Benzene-air.

c.

Hold the mouse button, and drag and drop the material on to the flow volume in the graphics window. This includes the selected material in your case setup.

d.

Close the Library dialog box. The list below the Materials.1 feature in the specification tree is automatically updated to show Benzene-air.1 and its constituent species materials.

2.

Delete all other materials from the Benzene-air.1 mixture material except Benzene-vapor. a.

To delete Oxygen, right-click on Oxygen from the Benzene-air.1 list and select the Delete (Del) option.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

185

Volatile Gas Emission Modeling Using Species Transport Model

b. 3.

Similarly, delete Carbon-dioxide, Water-vapor, and Nitrogen from the Benzene-air.1 list.

Add Air to the Benzene-air.1 materials list. a.

Right-click on Benzene-air.1 and select the Add Specie(s) option to open the Add Species dialog box.

b.

Select Air from the Species selection list and click Add.

c.

Close the Add Species dialog box. The specification tree for Benzene-air.1 will be updated as shown in Figure 8.9: Specification Tree Updated for Benzene-air.1 (p. 187).

186

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Modifying Boundary Groups Figure 8.9: Specification Tree Updated for Benzene-air.1

8.12. Modifying Boundary Groups 1.

2.

Rename Inlet Boundary (FluidInlet.1 1).1 to vent1. a.

Double-click Inlet Boundary (FluidInlet.1 1).1 below the Groups.1 feature in the specification tree to open the Group of Boundaries dialog box.

b.

Delete the entry for Name and enter vent1.

c.

Click OK to close the Group of Boundaries dialog box.

Similarly, rename other boundary groups as shown in the table: Table 8.1: Boundary Group Names Boundary Group

New Name

Inlet Boundary (FluidInlet.1 1).1

vent1

Inlet Boundary (FluidInlet.1 1).2

vent2

Inlet Boundary (FluidInlet.1 1).3

vent3

Outlet Boundary (FluidInlet.1 1).4

door

Outlet Boundary (FluidInlet.1 1).5

opening

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

187

Volatile Gas Emission Modeling Using Species Transport Model

3.

4.

188

Change the boundary type for the three benzene inlets from wall to inlet. a.

Double-click Wall (FluidToSolid.1.7 1).11 below the Groups.1 feature in the specification tree to open the Group of Boundaries dialog box.

b.

Delete the entry for Name and enter benz1.

c.

Select Inlet Boundary from the Type drop-down list.

d.

Click OK to close the Group of Boundaries dialog box.

Similarly, change the boundary type for the remaining two benzene inlets to Inlet Boundary and rename them to benz2 and benz3 respectively.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Boundary Conditions

8.13. Boundary Conditions 1.

Set the boundary conditions at the ceiling inlet vents (vent1, vent2, and vent3).

a.

Click

icon to open the Inlet Boundary Condition dialog box.

b.

Select vent1, vent2, and vent3 located below the Groups.1 feature in the specification tree. This automatically updates the Supports field.

c.

Enter 0 for Gauge Pressure (Total).

d.

Enter 293.17 Kdeg for Temperature.

e.

Click the Species Mass Fractions button to open the Species Mass Fractions dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

189

Volatile Gas Emission Modeling Using Species Transport Model

f. 2.

i.

Retain the default value of 0 for the mass fraction of Benzene-vapor.

ii.

Click OK to close the Species Mass Fractions dialog box.

Click OK in the Inlet Boundary Condition dialog box to validate.

Set the boundary conditions at the benzene inlets (benz1, benz2, and benz3).

a.

Click

icon to open the Inlet Boundary Condition dialog box.

b.

Select benz1, benz2, and benz3 located below the Groups.1 feature in the specification tree. This automatically updates the Supports field.

3.

190

c.

Enable Velocity and enter 0.833 m/s.

d.

Enter 310.92 Kdeg for Temperature.

e.

Enter 1 for the mass fraction of Benzene-vapor in the Species Mass Fractions dialog box.

f.

Click OK to validate.

Set the boundary conditions at the outlet door (door).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Boundary Conditions

a.

Click

icon to open the Outlet Boundary Condition dialog box.

b.

Select door located below the Groups.1 feature in the specification tree. This automatically updates the Supports field.

4.

c.

Retain the default value of 0 N_m2 for Gauge Pressure (Static).

d.

Enter 293 Kdeg for Temperature.

e.

Enter 0 for the mass fraction of Benzene-vapor in the Species Mass Fractions dialog box.

f.

Click OK to validate.

Set the boundary conditions at the outlet opening (opening).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

191

Volatile Gas Emission Modeling Using Species Transport Model a.

Click

icon to open the Outlet Boundary Condition dialog box.

b.

Select opening located below the Groups.1 feature in the specification tree. This automatically updates the Supports field.

c.

Enable Velocity and enter 5 m_s.

d.

Enter 310.92 Kdeg for Temperature.

e.

Enter 1 for the mass fraction of Benzene-vapor in the Species Mass Fractions dialog box.

f.

Click OK to validate.

8.14. Operating Conditions 1.

Double-click Operating Conditions.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Operating Conditions dialog box.

2.

Enter 101325 N_m2 for Operating Pressure.

3.

Click OK to close the Operating Conditions dialog box.

8.15. ANSYS Fluent Solution Settings 1.

Double-click Initialization Values.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Initialization Values dialog box. •

2.

192

Click Reset All and OK to validate.

Double-click Fluent Solution.1 below the Fluent Case feature in the specification tree to open the Fluent Solution dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

ANSYS Fluent Solution Settings

3.

a.

Click Reset All.

b.

Ensure that Residuals + Fluxes&Delta is selected from Convergence Criterion drop-down list.

c.

Enter 1000 for Max number of iterations.

d.

Click OK to close the Fluent Solution dialog box.

Save the CATIA V5 analysis files. File → Save Management...

a.

Select the Analysis1.CATAnalysis file and click the Save As... button.

b.

Rename the Analysis1.CATAnalysis file to compressible-photo-copy-machine_Analysis1.CATanalysis.

c.

Click the Propagate directory button and click OK to close the Save Management dialog box.

Note You specify the path where all the analysis files must be saved. Using Save Management... saves the analysis file along with other solution files written by FfC.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

193

Volatile Gas Emission Modeling Using Species Transport Model

8.16. Solution In this step, you will generate the mesh and iterate the solution. Though FfC allows you to generate the mesh and start the flow computations separately, here you will perform these steps simultaneously. 1.

Click the

icon to open the Compute dialog box.

2.

Select All and Default Solution Option in the two drop-down lists.

3.

Click OK to validate and start the computations.

Note FLUENT for CATIA V5 will start the computation process and the progress will be displayed in the Fluent Calculations Progression dialog box. Click the Stop Computation button if you want to interrupt the calculations. The solution will converge in approximately 600 iterations.

8.17. Postprocessing 1.

Generate the report of the simulation. a.

Click the

icon to open the Report Generation dialog box.

b.

Specify the appropriate path to the Output Directory where you want FLUENT for CATIA V5 to save the simulation report.

c.

Enter an appropriate Title for the report and click OK. This opens the web browser and displays the report page. A report is a summary of the simulation you have performed. It reports information about the mesh details, flow physics, boundary conditions, and results.

194

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing Figure 8.10: Report Showing the Solver Status

Figure 8.11: Report Showing the Mass Flow Rate at All Boundaries

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

195

Volatile Gas Emission Modeling Using Species Transport Model Figure 8.12: Report Showing Image of Residuals

2.

196

Display the path lines of Benzene-vapor mass fraction. a.

Click

icon to open the Species dialog box.

b.

Select Benzene-vapor Solution and click OK to close the Species dialog box.

c.

Double-click on Mass Fraction (path lines).1 from the Benzene-vapor Solution list below the Fluent Solution.1 feature in the specification tree to open the Image Edition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing

d.

Click on the field next to Inlet and select vent1, vent2, and vent3 from the specification tree below the Groups.1 feature. This will remove vent1, vent2, and vent3 from the Release from Surfaces list for the Inlet.

e.

Click OK to close the Image Edition dialog box. Figure 8.13: Pathlines of Mass Fraction of Benzene-vapor

3.

Display the velocity vectors on various cut planes.

a.

Click

icon to display the contours of velocity of Benzene-vapor.

b.

Double-click on Velocity.1 from the Benzene-vapor Solution list below the Fluent Solution.1 feature in the specification tree to open the Image Edition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

197

Volatile Gas Emission Modeling Using Species Transport Model

198

c.

In the Visu tab, select Symbol from the Types selection list to display the velocity vectors.

d.

Click OK to close the Image Editiondialog box.

e.

Display the velocity vectors on a plane cutting through the door, middle vent (vent2), and the opening on the ceiling (Figure 8.14: Velocity Vectors on a Cutting Plane through the Door, Middle Vent, and the Opening (p. 199)). i.

Click

to open the Cut Plane Analysis dialog box.

ii.

Disable Clipping.

iii.

Double-click on the compass ( ) in the graphics window to open the Parameters for Compass Manipulation dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing

iv.

Enter 0, 0, and 90 for Angle in the Coordinates group box and click Apply.

v.

Close the Parameters for Compass Manipulation dialog box.

vi.

In the Cut Plane Analysis dialog box, enable View section only and Project vectors on plane. You can also change the orientation of the cut plane by manipulating the position of the axes in the compass in the graphics window.

Figure 8.14: Velocity Vectors on a Cutting Plane through the Door, Middle Vent, and the Opening

f.

Similarly, display the velocity vectors on a cut plane through the human body (Figure 8.15: Velocity Vectors on a Cutting Plane through the Human Body (p. 200)).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

199

Volatile Gas Emission Modeling Using Species Transport Model Figure 8.15: Velocity Vectors on a Cutting Plane through the Human Body

4.

200

Display the contours of mass fraction of benzene-vapor. a.

Click

icon to open the Species dialog box.

b.

Select Benzene-vapor Solution and click OK to close the Species dialog box.

c.

Double-click on Mass Fraction (Iso).1 from the Benzene-vapor Solution list below the Fluent Solution.1 feature in the specification tree to open the Image Edition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing

d.

Click the Selections tab.

e.

Keep only Wall(FluidToSolid.1.2 1).6, Wall(FluidToSolid.1.2 1).7, Wall(FluidToSolid.1.2 1).8, and Wall(FluidToSolid.1.2 1).9 in the Available Groups list and move all the other groups to the Activated Groups list, using

button.

f.

Move Flow.1 from the Activated Groups list to the Available Groups list using

button.

g.

Click OK to close the Image Edition dialog box (Figure 8.16: Contours of Mass Fraction of Benzene (p. 201)).

Figure 8.16: Contours of Mass Fraction of Benzene

5.

Display the cut plane view of the benzene mass fraction through one of the benzene inlets (Figure 8.17: Contours of Mass Fraction of Benzene Vapor on a Cutting Plane Through a Benzene Inlet (p. 202)). Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

201

Volatile Gas Emission Modeling Using Species Transport Model Figure 8.17: Contours of Mass Fraction of Benzene Vapor on a Cutting Plane Through a Benzene Inlet

6.

Display the contours of static temperature (Figure 8.18: Contours of Static Temperature (p. 202)). a.

Click

to display the contours of static temperature.

b.

Perform similar steps as in Step 13.3 to display the contours of static temperature as shown in Figure 8.18: Contours of Static Temperature (p. 202) Figure 8.18: Contours of Static Temperature

8.18. Summary This tutorial demonstrated how to setup and solve a species transport case in FLUENT for CATIA V5. It showed how to use edge propagation to extract the flow volume and use a reference surface to define 202

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Summary edge propagation. It also demonstrated postprocessing of the species transport quantities using various cut planes.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

203

204

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 9: Cavitation Model 9.1. Introduction This tutorial examines cavitating flow of water over a hydrofoil. This is a typical hydrofoil for propellers and brings a challenge to the physics and numerics of cavitation models, because of the high pressure differentials involved and the high ratio of liquid to vapor density. Using FfC's modeling capability, you will be able to predict the strong cavitation near the trailing edge on the upper surface of the hydrofoil. In this tutorial you will learn how to: • Perform advanced meshing operations to generate trailing edge mesh. • Use the cavitation model in FLUENT for CATIA V5. • Set boundary conditions for external flow. • Change boundary group types. • Perform postprocessing to analyze the cavitation quantities.

9.2. Prerequisites This tutorial assumes that you are familiar with the menu structure in FfC. It also assumes that you have read the Getting Started (p. 1) portion of the Tutorial Guide and completed Internal Flow Calculation (p. 9). Some of the steps in setup and solution procedure will not be shown explicitly.

Note It is assumed that you have the FMS and FMD licenses available. If you do not have FMD and FMS (CATIA V5) licenses then you will not be able to generate mesh as explained in the tutorial. In this tutorial, you will start with the hydrofoil-3d_Analysis.CATAnalysis file which contains the mesh related settings. If you wish to perform the meshing on your own, you may refer to the appendix provided at the end of this tutorial.

9.3. Problem Description A hydrofoil is used to create lift by creating low pressure on the upper surface and higher pressure on the lower surface. The pressure on the upper surface of hydrofoil can become so low that the liquid water is transformed into gaseous phase (water vapor). This tutorial demonstrates this problem. A 3 dimensional hydrofoil is modeled. The hydrofoil is moving at 16.91 m/sec (about 60.8 km/hr) in liquid water. The hydrofoil motion is modeled by holding the hydrofoil stationary, but specifying velocity to the flow of liquid water over the stationary hydrofoil.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

205

Cavitation Model In order to determine whether cavitation is going to occur or not, it is necessary to have accurate pressure distribution. The problem of cavitation is thus solved in two parts. In first part, the flow solution (single phase) is obtained. In second part, the cavitation model (based on mixture multiphase model) available in FfC is activated. The flow and pressure distribution obtained in the first part is used to determine the location of cavitation. Figure 9.1: Problem Schematic

9.4. Preparation 1.

Copy the input file, cavitation.zip to your working directory and unzip it. It will extract files (hydrofoil-3d_Analysis.CATAnalysis, hydrofoil_3d.CATPart, hydrofoil_3d_FluentPart.CATPart, and hydrofoil_3d_FluentProduct.CATProduct).

2.

Start the FfC environment.

9.5. Setting the Options Tools → Options → Analysis & Simulation → Fluent Options 1.

206

Click the General tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 9.2: Options Dialog Box — General

a.

Enter the path for the ANSYS Fluent solver in the text entry box next to Folder for solver.

Note The ANSYS Fluent solver is provided with the installed FfC package. You can use the Browse button to specify the path for the solver: For 32 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/ntx86 For 64 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/win64 Similarly, specify the path for the external postprocessor, CFD-Post (or FloWizard) executable.

2.

b.

Select Maximum number of iterations from the Default criterion to stop steady state solver drop-down list and enter a value of 1000.

c.

Set the remaining parameters as shown in Figure 9.2: Options Dialog Box — General (p. 207).

Click the Data Management tab in the Options dialog box. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

207

Cavitation Model a.

Enter the path for Temporary files, FLUAnalysisComputations file and FLUAnalysisResults file in the External Storage folder group box. You can use the Browse button to specify the path. The analysis files will be saved in the temporary folders while FfC is computing the solution. The analysis will be saved to its permanent location when the computation is complete.

b.

Set the remaining parameters as shown in Figure 9.3: Options Dialog Box — Data Management (p. 208). Figure 9.3: Options Dialog Box — Data Management

3.

208

Click the Advanced Parameters tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 9.4: Options Dialog Box — Advanced Parameters

• 4.

Set the parameters as shown in Figure 9.4: Options Dialog Box — Advanced Parameters (p. 209).

Click the Customization tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

209

Cavitation Model Figure 9.5: Options Dialog Box — Customization

a.

Enable Advanced Turbulence Models.

Note If the Advanced Turbulence Models option is disabled, then the default turbulence model (k-epsilon, Realizable) for turbulent flows and Reynolds Stress Model for turbulence with strong swirl will be selected without any further access to more turbulence models.

b.

Enable Advanced Boundary Condition Parameters.

Note The Advanced Boundary Condition Parameters option allows specification of heat generation rate for wall boundary.

c.

Disable Use solution steering by default.

d.

Disable Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" . For more information on the Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" control, refer to the FLUENT for CATIA V5 User's Guide.

210

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Materials e. 5.

Select Residuals from the Convergence Criterion drop-down list.

Click OK to close the Options dialog box.

9.6. Reading the File 1.

Read the CATIA V5 file (hydrofoil-3d_Analysis.CATAnalysis) in FLUENT for CATIA V5. File → Open... This opens the File Selection dialog box, using which you can select the file to be read.

2.

Select the file, hydrofoil-3d_Analysis.CATAnalysis. By default, the file is opened in the Part or Product workbench of CATIA V5.

3.

Click

the icon to orient the geometry to isometric view.

Tip To use the entire screen space, remove the specification tree on the left-hand side by selecting the View → Specifications menu item or pressing the F3 key on your keyboard.

9.7. Physics Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the FLUENT for CATIA V5 specification tree to open the Physical Model Definition dialog box.

1.

Retain the default selection of Single Phase from the Model Definition drop-down list

2.

Click OK to validate.

9.8. Materials •

Click the a.

icon to open the Library dialog box.

Select the FLUENT for CATIA V5 fluids and mixtures materials library. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

211

Cavitation Model To open the materials library, you have to specify the path where it is stored. For 32 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\intel_a\startup\materials\Fluids and Mixtures.CATmaterial For 64 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\win_b64\startup\materials\Fluids and Mixtures.CATmaterial where X-X.X.X represents the version used. b.

Select Water-liquid in the Fluid tab.

c.

Hold the mouse button, and drag and drop the material on to the flow volume in the graphics window. This includes the selected material in your case setup.

d.

Close the Library dialog box. The list below the Materials.1 feature in the specification tree is automatically updated to show Water–liquid. It will be used as the primary phase material when we switch to the cavitation model at a later stage in the tutorial.

9.9. Boundary Conditions 1.

212

Set the inlet boundary conditions.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Boundary Conditions

a.

Click

icon to open the Inlet Boundary Condition dialog box.

b.

Select the two inlet boundaries, Inlet Boundary (FluidInlet.1_1).1 and Inlet Boundary (FluidInlet.3 _1).5 located below the Groups.1 feature in the specification tree. This automatically updates the Supports field.

2.

c.

Enable Velocity and enter a value of 16.91 m_s.

d.

Click OK in the Inlet Boundary Condition dialog box to validate.

Set the outlet boundary conditions. a.

Click

icon to open the Outlet Boundary Condition dialog box.

b.

Select the two outlet boundaries, Outlet Boundary (FluidOutlet.1_1).2 and Outlet Boundary (FluidOutlet.3_1).6 located below the Groups.1 feature in the specification tree.

c.

Enable Gauge Pressure (Static) and enter a value of -35000 N_m2.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

213

Cavitation Model d.

Click OK to validate.

9.10. Meshing Parameters •

Click

icon to open the Compute dialog box.

a.

Select Mesh Only from the drop-down list.

b.

Click OK.

After the meshing is done, confirm that the boundary layers are present on the outlet side of the hydrofoil, while there will be none on the inlet side. If the boundary layers are present on both the sides then check that you have set the Max. angle between adjacent face and prism direction to 90 deg as shown in Figure 9.4: Options Dialog Box — Advanced Parameters (p. 209). Observe the mesh (Figure 8.16). Figure 9.6: Mesh With Boundary Layers on Outlet Side

9.11. Cavitation Model Solution 1.

Select the cavitation model. a.

214

Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the specification tree to open the Physical Model Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Cavitation Model Solution

b.

Select Multiphase from the Model Definition drop-down list. Select Cavitation from the Multiphase Model drop-down list.

c. 2.

Click OK to validate.

Add the secondary phase material (Water-vapor). The primary phase material, Water-liquid, has already been applied in the single phase setup in Materials (p. 211).

a.

Click the

icon to open the Library dialog box.

b.

In the Library dialog box, select Water-vapor and click OK. This automatically updates the list below the Materials.1 feature in the specification tree to show Water-vapor.1.

c.

Double-click Cavitation.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Cavitation dialog box.

d.

Click on the text field next to Material in the Secondary Phase Definition group box and select Water-vapor.01 from the tree below the Materials.1 feature.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

215

Cavitation Model

3.

e.

Enter 3574 N_m2 for Vaporization Pressure.

f.

Ensure that the values for Surface Tension Coefficient and Non-Condensable Gas Mass Fraction are defined as shown in the dialog box.

g.

Click OK to close the Cavitation dialog box.

Set the Fluent solution parameters. a.

Double-click Fluent Solution below the Fluent Case feature in the specification tree to open the Fluent Solution dialog box.

b.

Enter 10 for Number of parallel processes.

c.

Click the Residual Convergence Criteria button to open the Residual Convergence Criteria dialog box.

i.

216

Retain the default settings and click the Phases Input button to open the Phases Input dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Cavitation Model Solution

d.

4.

ii.

Ensure that the Volume Fraction for Secondary Phase 1 is set to 0.001.

iii.

Click OK to close the Phases Input dialog box.

iv.

Click OK to close the Residual Convergence Criteria dialog box.

Click the Relaxation Settings button to open the Relaxation Settings dialog box.

i.

Set the parameters as shown in the dialog box.

ii.

Click OK to close the Relaxation Settings dialog box.

e.

Enter 2000 for Max number of iterations.

f.

Click OK to close the Fluent Solution dialog box.

Save the CATIA V5 analysis files. File → Save Management...

a.

Select the hydrofoil-3d_Analysis.CATAnalysis file and click the Save As... button.

b.

Click the Propagate directory button and click OK to close the Save Management dialog box.

Note You specify the path where all the analysis files must be saved. Using Save Management... saves the analysis file along with other solution files written by FfC.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

217

Cavitation Model 5.

Compute the solution. a.

Click the

icon to open the Compute dialog box.

b.

Select All and Default Solution Options from the two drop-down lists available.

c.

Click OK in the Compute dialog box to launch the computation.

FLUENT for CATIA V5 will continue the computation process and the progress will be displayed in the Fluent Calculations Progression dialog box. Solution converges in approximately 1000 iterations but it may vary slightly depending on the number of parallel processors the solution is run on. Click the Stop Computation button if you want to interrupt the calculations. For residuals see Figure 9.7: Scaled Residuals for Cavitation Model (p. 218) Figure 9.7: Scaled Residuals for Cavitation Model

9.12. Postprocessing 1.

218

Display the contours of static pressure on the hydrofoil (Figure 9.8: Contours of Static Pressure on the Hydrofoil (p. 219)).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing

a.

Click the

icon to display the contours of static pressure on the entire domain.

b.

Double-click on Pressure (nodal values).1 from the Cavitation list below the Fluent Solution.1 feature in the specification tree to open the Image Edition dialog box.

c.

Click the Selections tab.

d.

Keep only Wall(FluidToSolid.1.3_2).4 and Wall(FluidToSolid.3.7_1).10 in the Activated Groups list and move all the other groups to the Available Groups list, using the

e.

button.

Click OK to close the Image Edition dialog box . Figure 9.8: Contours of Static Pressure on the Hydrofoil

2.

Display a cut plane view of the contours of static pressure (Figure 9.9: Cut Plane view of Contours of Static Pressure (p. 221)). a.

Click the

icon to open the Cut Plane Analysis dialog box. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

219

Cavitation Model b.

Disable Clipping.

c.

Double-click on the compass ( Manipulation dialog box.

) in the graphics window to open the Parameters for Compass

i.

Enter 0, 0, and 90 for Angle in the Coordinates group box and click Apply.

ii.

Close the Parameters for Compass Manipulation dialog box. You can also change the orientation of the cut plane by manipulating the position of the axes in the compass in the graphics window.

d.

220

Disable Show cutting plane and enable Clipping in the Cut Plane Analysis dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing Figure 9.9: Cut Plane view of Contours of Static Pressure

e. 3.

Close the Cut Plane Analysis dialog box.

Display the contours of volume fraction of primary phase (Figure 9.10: Contours of Volume Fraction of Primary Phase (Liquid Water) (p. 222)). a.

Click the

icon to open the Phases dialog box.

b.

Select Primary Phase Solution from the available list and click OK to display the primary phase contours of volume fraction (Figure 9.10: Contours of Volume Fraction of Primary Phase (Liquid Water) (p. 222)).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

221

Cavitation Model Figure 9.10: Contours of Volume Fraction of Primary Phase (Liquid Water)

4.

Similarly, display the contours of volume fraction of secondary phase (Figure 9.11: Contours of Volume Fraction on Secondary Phase (Water Vapor) (p. 222)). Figure 9.11: Contours of Volume Fraction on Secondary Phase (Water Vapor)

5.

222

Zoom in to the hydrofoil to view the region where cavitation has occurred (Figure 9.12: Contours of Volume Fraction of Secondary Phase (region where cavitation has occurred) (p. 223)).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Appendix Figure 9.12: Contours of Volume Fraction of Secondary Phase (region where cavitation has occurred)

9.13. Summary This tutorial demonstrated how to setup and solve a cavitation case in FLUENT for CATIA V5. It showed how to perform advanced meshing operations to generate the trailing edge mesh. It also demonstrated postprocessing of the cavitation quantities using a cut plane. You may want to generate the report of your simulation. For details on report generation, refer to Volatile Gas Emission Modeling Using Species Transport Model (p. 173).

9.14. Appendix This section describes the advanced mesh settings to generate the mesh for the given geometry. You can perform the steps enlisted in this section to create the mesh and then continue to compute the solution.

Note Ensure to set the values in the Options dialog box as shown in Figure 9.2: Options Dialog Box — General (p. 207) in the beginning of this tutorial.

9.14.1. Reading the File 1.

Read the CATIA V5 file (hydrofoil-3d.CATPart) in FLUENT for CATIA V5. File → Open... This opens the File Selection dialog box, using which you can select the file to be read.

2.

Select the file, hydrofoil-3d.CATPart. By default, the file is opened in the Part or Product workbench of CATIA V5.

Tip To use the entire screen space, remove the specification tree on the left-hand side by selecting the View → Specifications menu item or pressing the F3 key on your keyboard. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

223

Cavitation Model

9.14.2. Starting FLUENT for CATIA V5 1.

Launch the FfC workbench. Start → Analysis & Simulation → FLUENT for CATIA V5 This updates the graphics display. The specification tree on the left-hand side also gets updated and displays the analysis-related parameters.

2.

In the Options dialog box, specify the location of the directory where you want to store the solver files.

9.14.3. Extracting Flow Volume 1.

2.

Define the inlet and outlet faces. a.

Click the

b.

Select faces from the Selection mode drop-down list.

c.

Click on the field next to Inlet, zoom-in on the geometry, and select the appropriate face.

d.

Click on the field next to Outlet, zoom-in on the geometry, and select the appropriate face.

e.

Click OK to validate.

Split the flow volume. a.

224

icon to open the Geometry Definition dialog box.

Right-click on Geometry Definition.1 below the Environment.1 feature in the specification tree and select the Split flow volumes option to open the Split Flow Volumes dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Appendix

b.

Click on the field next to Geometry and select Extrude.2 from the volume.2 list below the hydrofoil3d feature in the specification tree. This automatically updates the Geometry field.

c.

Click OK to validate.

When the flow volume extraction is done, the different mesh parts will be available in the tree below the Nodes and Elements.1 feature. Apart from defining the mesh settings globally in the Mesh Definition dialog box, you will also define the meshing parameters for some of the mesh parts separately.

9.14.4. Modifying Boundary Groups 1.

2.

Double-click on Wall (FluidToSolid.1.2_2).3 below the Groups.1 feature in the specification tree to open the Group Of Boundaries dialog box.

a.

Select Symmetry from the Type drop-down list.

b.

Click OK to close the Group Of Boundaries dialog box.

Similarly, change the group type of the other groups as shown in the table: Table 9.1: Boundary Group Types Boundary Group

New Type

Interior Boundary (FluidToFluid.1.3_2).8

Wall

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

225

Cavitation Model Wall (FluidToSolid.3.6_1).9

Symmetry

This updates the specification tree below the Groups.1 feature.

9.14.5. Mesh Settings 1.

Click the

to open the Mesh Definition dialog box.

a.

Click the Reset All button.

b.

Move the sliding pointer towards Fine until it shows a value of 100. Some of the parameters in the Mesh Definition dialog box are linked to the position of the slider bar. Therefore, depending on the mesh type, moving the slider changes the values of such parameters.

226

c.

Enter 2 mm for Critical length.

d.

Enable Mesh size and enter a value of 30 mm.

e.

Click the Geometry tab and enter 2 mm for Merge simplification.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Appendix

f.

g.

Click the Surface mesh tab.

i.

Enable Relative sag and enter a value of 0.02.

ii.

Enable Automatic mesh capture and enter a value of 0.3 mm.

iii.

Enable Growth rate and enter a value of 1.15.

iv.

Enable Min face number and enter a value of 2.

Click the Volume mesh tab. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

227

Cavitation Model

i.

Enable Size progression and enter a value of 1.2.

ii.

Enable Use TGrid for Fluids.

iii.

Select Uniform Growth from the Boundary Layer Method drop-down list.

iv.

Enter 0.5 mm for First height.

v.

Enter 6 for Number of layers.

vi.

Enter 1.2 for Growth rate.

vii. Enter 60 deg for Max angle change. h. 2.

Click OK to validate.

Define the advanced mesher settings for the trailing edge of hydrofoil. a.

Double-click on FluidToSolid.1.3_2 below the Nodes and Elements feature in the specification tree to open the Global Parameters dialog box. Figure 9.13: Figure Showing Mesh Parts for Advanced Meshing

228

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Appendix

3.

b.

Enter 5 mm for Mesh size and 0.02 for Relative Sag.

c.

Enter 0.3 mm for Min Size and 0.3 mm for Tolerance.

d.

Click the Geometry tab and enter 0.5 mm for Constraint Sag.

e.

Disable Constraint ref size independent from mesh size.

f.

Disable Merge during simplification.

g.

Click OK to close the Global Parameters dialog box.

Apply imposed nodes on the trailing edge of the hydrofoil. a.

Hide the upper portion of the geometry so that the trailing edge of the hydrofoil becomes visible.

b.

Click the

icon to open the Imposed Elements dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

229

Cavitation Model

c.

Select the trailing edge of the hydrofoil as shown in Figure 9.14: Selection of Trailing Edge of Hydrofoil (p. 230). Figure 9.14: Selection of Trailing Edge of Hydrofoil

This opens the Edit Elements Distribution dialog box.

d.

Enable Size and enter a value of 3 mm.

e.

Click OK in the Edit Elements Distribution dialog box to validate.

4.

Set the advanced meshing parameters for the upper surface of the hydrofoil, FluidToSolid.3.7_1 (similar to Step 2 (p. 228)).

5.

Update the surface mesh of the boundary zones near to the hydrofoil trailing edge.

230

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Appendix

a.

Click the

icon.

b.

Right-click on FluidToSolid.1.3_2 below the Nodes and Elements.1 feature in the specification tree and select the Update Mesh item.

c.

Similarly, update the mesh for FluidToSolid.3.7_1, FluidToFluid.1.3_1, and FluidToFluid.1.3_2.

Note We have imposed nodes in order to capture the trailing edge geometry of the hydrofoil. By updating the mesh of the nearby surfaces locally, a gradual growth in the mesh of these surfaces is achieved, resulting in creation of the expected cavitation zone. Therefore, it is important to follow the correct sequence while updating the mesh locally for the mesh parts mentioned in the steps above.

6.

Reconvert the changed groups to their original type. a.

Double-click on Wall (FluidToFluid.1.3_2).8 to open the Group of Boundaries dialog box.

b.

Select Interior Boundary from the Type drop-down list.

c.

Click OK to close the Group of Boundaries dialog box. This updates the specification tree below the Groups.1 feature.

9.14.6. Generating the Mesh 1.

Click the to

icon open the Compute dialog box.

a.

Select Mesh Only from the drop-down list.

b.

Click OK to start the mesh generation

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

231

Cavitation Model Figure 9.15: Figure Showing Entire Mesh

Figure 9.16: Figure Showing Hydrofoil Mesh

Figure 9.17: Zoomed View of the Hydrofoil Mesh

2.

Save the CATIA V5 analysis files. File → Save Management...

232

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Appendix

a.

Select the Analysis1.CATAnalysis file and click the Save As... button.

b.

Rename the Analysis1.CATAnalysis file to hydrofoil-3d_Analysis.CATanalysis.

c.

Click the Propagate directory button and click OK to close the Save Management dialog box.

Note You specify the path where all the analysis files must be saved. Using Save Management... saves the analysis file along with other solution files written by FfC.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

233

234

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 10: Using Periodic Boundary Conditions 10.1. Introduction For cases where physical geometry of interest and expected pattern of the flow/thermal solution have a periodically repeating nature, you can use periodic boundary condition feature available in FfC. Two types of periodic conditions are available in FfC, rotational periodic and translational periodic. The first type does not allow a pressure drop across the periodic planes. Second type allows a pressure drop to occur across translationally periodic boundaries, enabling you to model "fully-developed" periodic flow. This tutorial is an extension of Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model (p. 131) and explains the steps needed for creating rotational periodic boundary condition. This tutorial demonstrates how to do the following: • Identify and separate fluid zone around the rotating part. • Change group types. • Specify rotation to the fluid zone around the rotating part. • Set rotation to rotating parts (wall zones). • Define periodic boundaries.

10.2. Prerequisites This tutorial assumes that you are familiar with the menu structure in FfC. It also assumes that you have read the Getting Started (p. 1) portion of the Tutorial Guide and completed Internal Flow Calculation (p. 9). Some of the steps in setup and solution procedure will not be shown explicitly.

Note It is assumed that you have the FMS and FMD licenses available. If you do not have FMD and FMS (CATIA V5) licenses then you will not be able to generate mesh as explained in the tutorial.

10.3. Problem Description This problem considers a generic mixing tank with only one rotor. The flow is assumed to be turbulent. The rotor is fitted at the bottom end of a shaft entering the tank from the top. A domain is shown in Figure 10.1: Mixing Tank Schematic (p. 236). The rotor consists of 4 blades and is rotating with an angular velocity of 500 rpm. This is different from the domain used in Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model (p. 131) in terms of inclination of rotor shaft with respect to the tank's axis. In Modeling Mixing Tanks Using Multiple Rotating Reference Frame (MRF) Model (p. 131) it is inclined whereas in present case it is parallel to the tank's axis. As geometry is periodically repeating with an angle of 90°, periodic boundary condition is used to simplify the problem. While implementing

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

235

Using Periodic Boundary Conditions periodic boundary condition for the present problem make sure that computational domain has one complete blade of rotor. For the present geometry this condition is achieved by dividing the flow domain by YZ and XZ plane. Figure 10.1: Mixing Tank Schematic

10.4. Preparation 1.

Copy the CATIA V5 file, mix-test.CATPart to your working directory.

2.

Start the FfC environment.

10.5. Setting the Options Tools → Options → Analysis & Simulation → Fluent Options 1.

236

Click the General tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 10.2: Options Dialog Box — General

a.

Enter the path for the ANSYS Fluent solver in the text entry box next to Folder for solver.

Note The ANSYS Fluent solver is provided with the installed FfC package. You can use the Browse button to specify the path for the solver: For 32 bit the path is: FfC Installation/FfC-RX-X.X.XX/solver/Fluent.Inc/ntbin/ntx86 For 64 bit the path is: FfC Installation/FfC-RX-X.X.XX/solver/Fluent.Inc/ntbin/win64 Similarly, specify the path for the external postprocessor, CFD-Post (or FloWizard) executable.

b.

Set the remaining parameters as shown in Figure 10.2: Options Dialog Box — General (p. 237).

Note You can specify the Maximum number of iterations. For this tutorial the recommended value is 2000 iterations. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

237

Using Periodic Boundary Conditions 2.

Click the Data Management tab in the Options dialog box. a.

Enter the path for Temporary files, FLUAnalysisComputations file and FLUAnalysisResults file in the External Storage folder group box. You can use the Browse button to specify the path. The analysis files will be saved in the temporary folders while FfC is computing the solution. The analysis will be saved to its permanent location when the computation is complete.

b.

Set the remaining parameters as shown in Figure 10.3: Options Dialog Box — Data Management (p. 238). Figure 10.3: Options Dialog Box — Data Management

3.

238

Click the Advanced Parameters tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 10.4: Options Dialog Box — Advanced Parameters

• 4.

Set the parameters as shown in Figure 10.4: Options Dialog Box — Advanced Parameters (p. 239).

Click the Customization tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

239

Using Periodic Boundary Conditions Figure 10.5: Options Dialog Box — Customization

a.

Enable Advanced Turbulence Models.

Note If the Advanced Turbulence Models option is disabled, then the default turbulence model (k-epsilon, Realizable) for turbulent flows and Reynolds Stress Model for turbulence with strong swirl will be selected without any further access to more turbulence models.

b.

Enable Advanced Boundary Condition Parameters.

Note The Advanced Boundary Condition Parameters option allows specification of heat generation rate for wall boundary.

c.

Disable Use solution steering by default.

Note The Use solution steering by default option enables solution steering mechanism to control the solution convergence automatically.

240

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Extracting Flow Volume d.

Enable Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" . The Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" option uses second order solutions after 75% accuracy settings during mesh definition. If this option is disabled, then first order solution is computed for all slider positions.

e. 5.

Select Residuals from the Convergence Criterion drop-down list.

Click OK to close the Options dialog box.

10.6. Reading the File 1.

Read the CATIA V5 file (mix-test.CATPart) in FLUENT for CATIA V5. File → Open... This opens the File Selection dialog box, using which you can select the file to be read.

2.

Select the file, mix-test.CATPart. By default, the file is opened in the Part or Product workbench of CATIA V5.

Tip To use the entire screen space, remove the specification tree on the left-hand side by selecting the View → Specifications menu item or pressing the F3 key on your keyboard.

10.7. Starting FLUENT for CATIA V5 1.

Launch the FfC workbench. Start → Analysis & Simulation → FLUENT for CATIA V5 This updates the graphics display. The specification tree on the left-hand side also gets updated and displays the analysis-related parameters.

2.

In the Options dialog box, specify the location of the directory where you want to store the solver files.

10.8. Extracting Flow Volume Click the icon or double-click the Geometry Definition.1 option located below the Environment.1 feature in the specification tree to open the Geometry Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

241

Using Periodic Boundary Conditions

1.

Enable Geometry is Symmetric.

2.

Click on the field next to Plane of Symmetry and select the XZ and YZ planes from the graphics window.

3.

Select flow volume from the Geometry definition drop-down list.

4.

Retain No selection for Inlet.

5.

Click in the text entry field next to Outlet, zoom in the top side of the tank and select the tank top surface as the outlet.

6.

Make sure that Merge all Fluids is deactivated.

7.

Click OK to validate and close the Geometry Definition dialog box. This extracts the flow volume and the graphics window gets updated to show the extracted flow volume. Figure 10.6: Flow Volume

8.

242

Once the flow volume is extracted as shown above, FfC will create group of publications located below Groups.1.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Physics

a.

Double click on Outlet Boundary.1 to open the Group of Boundaries dialog box.

b.

Select Symmetry from the Type drop-down list.

c.

When the Type is changed to Symmetry the name of the boundary group will be modified and the color of the group will also be changed.

10.9. Physics Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the FLUENT for CATIA V5 specification tree to open the Physical Model Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

243

Using Periodic Boundary Conditions 1.

Disable Accounting for Temperature Effect.

2.

Select Turbulent in the Flow Type drop-down list.

3.

Select k-epsilon, Realizable in the Turbulence Model drop-down list.

4.

Select steady in the Time drop-down list.

5.

Click OK to validate.

10.10. Meshing Parameters Click the icon or double-click the Mesh Definition.1 option located below the Environment.1 feature in the specification tree to open the Mesh Definition dialog box.

1.

Click Reset All.

2.

Click the

3.

Move the slide bar towards Fine till the number above it shows a value of 75.

icon to select the optimized surface mesh.

As you move the slide bar, other parameters will change accordingly. Use the Reset All button to set all the field values to their default values. Note that, if you don't use the Reset All button, the values from the previous session will be taken by FfC for meshing. 4.

Click the Global tab and enter 4.4 mm for Critical Length.

5.

Retain the default values for other parameters.

6.

Click OK to close the Mesh Definition dialog box.

244

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Create a Separate Group for Faces of the Shaft

10.11. Materials In this step, apply material to the outer fluid zone using the drag and drop method.

1.

Click the

icon to open the Library dialog box.

2.

Select the FLUENT for CATIA V5 fluids and mixtures materials library. To open the materials library, you have to specify the path where it is stored. For 32 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\intel_a\startup\materials\Fluids and Mixtures.CATmaterial For 64 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\win_b64\startup\materials\Fluids and Mixtures.CATmaterial where X-X.X.X represents the version used.

3.

Click and hold the mouse button on water-liquid material icon.

4.

Drag and drop the material on to the outer fluid zone displayed in the graphics window.

5.

Close the Library dialog box.

10.12. Create a Separate Group for Faces of the Shaft 1.

Set the view from rendering style to perspective.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

245

Using Periodic Boundary Conditions View → Render Style → Perspective 2.

Click the

con to open the Group of Boundaries dialog box.

Figure 10.7: Shaft-Rotating-Zone

3.

Zoom into the model around the impeller to select the faces of the shaft lying in the rotating zone in the Support text entry (Figure 10.7: Shaft-Rotating-Zone (p. 246)).

4.

Select Wall as the Type.

5.

Specify shaft-rotating-zone as the Name.

6.

Select Wall (FluidtoSolid.2.0_1).1 under Groups.1 in the specification tree as shown in Figure 10.8: RotorBlades (p. 246) and rename it as rotor-blades. Figure 10.8: Rotor-Blades

246

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Naming the Fluid Zones 7.

Similarly, rename a group for shaft-not-rotating-zone as shown in Figure 10.9: Shaft-Not-RotatingZone (p. 247). Figure 10.9: Shaft-Not-Rotating-Zone

8.

Similarly, rename a group for tank-outer-wall as shown in Figure 10.10: Tank-Outer-Wall (p. 247). Figure 10.10: Tank-Outer-Wall

10.13. Naming the Fluid Zones 1.

Click the

icon.

2.

Select any zone in the specification tree under Properties.1.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

247

Using Periodic Boundary Conditions Make the outer tank wall transparent. The selected zone gets highlighted. Identify the fluid zone around the rotor blades.

3.

Rename the smaller zone around the rotor-blades as rotating-zone and rename the other fluid zone representing tank volume as outer-fluid-zone.

10.14. Specify MRF Zone The mixing tank is divided into two fluid zones, due to which the MRF model is applied here. A rotation speed is specified for the impeller blades, which is bounded by surfaces of revolution. The other fluid zone is specified as stationary. The flow volume is divided into two fluid zones as mixing tanks typically have baffles on the outside walls, which are not surfaces of revolution. 1.

248

Under Properties.1 in the specification tree, double click on the Property corresponding to the inner fluid zone Flow Property Definition dialog box.

a.

Select the Moving Reference Frame from the Motion Type drop-down list.

b.

Click the

icon to open the Rotational Inputs dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Specify MRF Zone

i.

Enter 500 turn_mn for Rotational Speed.

ii.

Select one vertical face of the shaft as Surface for direction calculation.

iii.

Select Clockwise for rotation direction and click OK. The direction of rotation should be clockwise with reference to the top of the tank. Use Clockwise or Counter Clockwise options to get the required rotational direction.

c. 2.

Click OK in the Flow Property Definition dialog box.

Under Properties.1 in the specification tree, double click on the Property corresponding to the outer fluid zone Flow Property Definition dialog box. Figure 10.11: Motion Direction

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

249

Using Periodic Boundary Conditions

a.

Select Stationary from the Motion Type drop-down list.

b.

Click the

c.

3.

250

icon to open the Rotational Inputs dialog box.

i.

Enable Direction and enter -1 for Z.

ii.

Click OK to close Rotational Inputs dialog box.

Click OK in the Flow Property Definition dialog box.

Click the

icon.

a.

Click the text entry next to the Supports and select rotor-blades in specification tree under Groups.1.

b.

Change the Name to rotor-blades.

c.

Enable Moving Wall.

d.

Select Rotating in the Motion Type scrolling list.

e.

Select Relative to adjacent fluid region in the Reference Frame scrolling list. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Specify Periodic Zone f.

Enter 0 turn_mn for Rotational Speed.

g.

Enable Clockwise and click OK.

10.15. Specify Periodic Zone

1.

Right-click on Geometry Definition.1 and select Periodic Specification to open the Periodic Specification dialog box.

2.

Select two faces for both Periodic Faces and Shadow Faces.

3.

Click in the text entry field next to Periodic Faces and select two faces from the geometry.

4.

Similarly, select two faces on the other side for Shadow Faces.

5.

Select Rotational from the Periodic Type drop-down list.

6.

Click OK to close the Periodic Specification dialog box. When you define periodic boundary conditions, periodic and periodic-shadow will be updated under Groups.1 specification tree. Similarly Periodic Specification.1 feature is also created under the Geometry Definition.1 specification tree.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

251

Using Periodic Boundary Conditions Figure 10.12: Periodic Zone

7.

252

(Optional) Manual modification of Periodic Point and Matching Point. a.

Click the

to change the view to Shading with Material.

b.

Double-click Periodic (Flow.2).12 to open Group Of Boundaries dialog box.

i.

Click in the text entry field next to Periodic Point and select the point as shown in Figure 10.13: Periodic Point — Shading with Material (p. 253).

ii.

Similarly select the Matching Point.

iii.

Change the view to Shading with Edges as shown in Figure 10.14: Periodic Point — Shading with Edges (p. 253).

iv.

Click OK in the Group Of Boundaries dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Solver Settings Figure 10.13: Periodic Point — Shading with Material

Figure 10.14: Periodic Point — Shading with Edges

As FfC calculates periodic angle based on the position of Periodic Point and Matching Point. This step is important for cases where periodic planes have non-uniform height variation normal to their surface.

10.16. Solver Settings 1.

Double-click on Initialization Values.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Initialization Values dialog box. •

2.

Click Reset All and OK to validate.

Double-click on Fluent Solution.1 in the specification tree to open the Fluent Solution dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

253

Using Periodic Boundary Conditions

a.

Click Reset All.

b.

Move the Solver Accuracy Settings slide bar to 4.

c.

Ensure that Residuals is selected from the Convergence Criterion drop-down list.

d.

Click the Relaxation Settings to open Relaxation Settings dialog box. i.

Enter 0.3 for Momentum and 0.5 for Pressure.

ii.

Click OK to close the Relaxation Settings dialog box.

e.

Specify a value of 2000 iterations for Max number of iterations.

f.

Click OK to validate and close the Fluent Solution dialog box.

10.17. Perform Computation 1.

Click the

icon to open the Compute dialog box.

2.

Select All and Default Solution Option in the two drop-down lists.

3.

Click OK to validate and start the computations.

Note Solution converges after around 1100 iterations. It will take a few hours to complete the solution. You can postprocess the results by interrupting the computations. Use Stop Computation button to stop the calculations.

10.18. Save Management Save the analysis files as periodic_flow_Analysis1.CATAnalysis file and propagate directory. File → Save Management...

254

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing

10.19. Postprocessing 1.

Display residuals and monitor plots. •

Click the

icon to open the Residual Images dialog box.

Figure 10.15: Residual Plot

2.

Display velocity vectors on a cut plane.

a.

Click the

icon.

Velocity contours are displayed and this is listed under Fluent Solution.1 as Velocity.1.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

255

Using Periodic Boundary Conditions

b.

Double click on Velocity.1 to open the Image Edition dialog box.

c.

In the Image Edition box under Visu tab select Symbol as Type.

Note Velocity vectors will be displayed on boundaries. Click the Options... tab to manipulate arrows.

d.

Click OK to verify. To include parts of the mixing tank in this image right click on the Link Manager.1 and in the contextual menu, click Hide/Show. For a better view you may have to make some parts transparent or hide them.

e.

Click the

icon to open the Cut Plane Analysis dialog box

Keep the settings as shown in Figure 10.16: Cut Plane Analysis Dialog Box (p. 257).

256

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing Figure 10.16: Cut Plane Analysis Dialog Box

f.

Adjust the position of the plane using the compass, so that the plane cuts the tank vertically into two equal parts.

Note You can also double-click on the compass to adjust the cutting plane. This opens the Parameters for Compass Manipulation dialog box.

g.

Similarly you can display velocity vectors on a horizontal cutting plane passing from the blades. See Figure 10.17: Velocity Vectors (p. 258).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

257

Using Periodic Boundary Conditions Figure 10.17: Velocity Vectors

3.

Display static pressure contours on a cut plane. a.

Click the

icon.

Static pressure contours are displayed and it is listed under Fluent Solution.1 as Pressure( nodal values).1. You can include parts of the mixing tank in this image . b.

4.

Display turbulence kinetic energy contours on the blades. a.

258

The procedure to show the pressure contour on a cut plane is same as you performed in the previous step.

Click the

icon. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing Contour of turbulent kinetic energy will be displayed and this will be listed under Fluent Solution.1 as Turbulence Kinetic Energy (average iso).1. b.

Double click Turbulence Kinetic Energy (average iso).1 to open the Image Edition dialog box.

c.

Click the Selection tab and select rotor-blades under Available Groups and click the down arrow. rotor-blades is available under Activated Groups and the contours are shown on the rotorblades.

5.

Display velocity vectors and static pressure with periodic repeats.

a.

Click

icon.

Velocity contours are displayed and this is listed under Fluent Solution.1 as Velocity. 1. b.

Double click on Velocity.1 to open the Image Edition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

259

Using Periodic Boundary Conditions

i.

Select Symbol as Type under the Visu tab.

ii.

Click the Selections tab and change the settings as shown. Click More to view all the options in the Image Edition dialog box.

iii.

Click OK to close the Image Edition dialog box. Figure 10.18: Velocity Vectors without Periodic Repeats

c.

260

Click the

icon to open Image transformation dialog box.

i.

Click in the text entry field next to Image and select a face from the geometry.

ii.

Click OK in the Image transformation dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing When you click OK, the geometry gets updated with the remaining periodic repeats. Right click on the Link Manager.1 and in the contextual menu, click Hide/Show to view the image as shown in Figure 10.19: Velocity Vectors with Periodic Repeats (p. 261). Figure 10.19: Velocity Vectors with Periodic Repeats

d.

Display the static pressure on rotor blades. i.

Click the

icon.

Static Pressure contours are displayed and is listed under Fluent Solution.1 as Pressure(nodal values).1. ii.

Double click on Pressure(nodal values).1 to open the Image Edition dialog box. A.

Move rotor-blades to Activated Groups selection list.

B.

Move Flow.2 and Flow.3 to Available Groups selection list.

C.

Click OK to close the Image Edition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

261

Using Periodic Boundary Conditions Figure 10.20: Static Pressure on Rotor Blade

e.

Click the

icon to open Image transformation dialog box.

i.

Click in the text entry field next to Image and select a face from the geometry.

ii.

Click OK in the Image transformation dialog box.

10.20. Summary In this tutorial you learned how to setup the case for rotational periodic domains by using rotational periodic boundary condition available in FfC. This approach can also be used for turbo machinery applications in which rotor-stator interaction is relatively weak, and the flow is relatively uncomplicated at the interface between the moving and stationary zones. To generate the report of your simulation, refer to Volatile Gas Emission Modeling Using Species Transport Model (p. 173).

262

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 11: Using Moving Mesh Model 11.1. Introduction Analysis of turbomachinery often involves the examination of unsteady effects due to flow interaction between the stationary components and the rotating blades. In this tutorial, sliding mesh capability of FfC is used to analyze the unsteady flow through a fan. The fan-stator interaction is modeled by allowing mesh associated with the fan blade to rotate relative to the stationary mesh associated with the stator blade. This tutorial demonstrates how to do the following: • Identify and separate fluid zone around the rotating part. • Specify rotation to the fluid zone around the rotating part. • Set rotation to rotating parts (wall zones). • Set up unsteady solver and its parameter. • Create moving mesh zone. • Use monitors to determine mass flow rate at inlet, mass-weighted total pressure at the outlet.

11.2. Prerequisites This tutorial assumes that you are familiar with the menu structure in FfC. It also assumes that you have read the Getting Started (p. 1) portion of the Tutorial Guide and completed Internal Flow Calculation (p. 9). Some of the steps in setup and solution procedure will not be shown explicitly.

Note It is assumed that you have the FMS and FMD licenses available. If you do not have FMD and FMS (CATIA V5) licenses then you will not be able to generate mesh as explained in the tutorial.

11.3. Problem Description This problem considers flow through fan in a duct (Figure 11.1: Problem Schematic (p. 264)). Fan has four blades and is operating at a rotational speed of 1500 rpm. For stator a simplied geometry of blades is taken and is modeled as a part of the walls, it comprises four blades.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

263

Using Moving Mesh Model Figure 11.1: Problem Schematic

11.4. Preparation 1.

Copy the CATIA V5 file, fan_duct.CATPart to your working directory.

2.

Start the FfC environment.

11.5. Setting the Options Tools → Options → Analysis & Simulation → Fluent Options 1.

264

Click the General tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 11.2: Options Dialog Box — General

a.

Enter the path for the ANSYS Fluent solver in the text entry box next to Folder for solver.

Note The ANSYS Fluent solver is provided with the installed FfC package. You can use the Browse button to specify the path for the solver: For 32 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/ntx86 For 64 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/win64 Similarly, specify the path for the external postprocessor, CFD-Post (or FloWizard) executable.

b.

Set the remaining parameters as shown in Figure 11.2: Options Dialog Box — General (p. 265).

Note You can specify the Maximum number of iterations. For this tutorial the recommended value is 2000 iterations. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

265

Using Moving Mesh Model 2.

Click the Data Management tab in the Options dialog box. a.

Enter the path for Temporary files, FLUAnalysisComputations file and FLUAnalysisResults file in the External Storage folder group box. You can use the Browse button to specify the path. The analysis files will be saved in the temporary folders while FfC is computing the solution. The analysis will be saved to its permanent location when the computation is complete.

b.

Set the remaining parameters as shown in Figure 11.3: Options Dialog Box — Data Management (p. 266). Figure 11.3: Options Dialog Box — Data Management

3.

266

Click the Advanced Parameters tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 11.4: Options Dialog Box — Advanced Parameters

• 4.

Set the parameters as shown in Figure 11.4: Options Dialog Box — Advanced Parameters (p. 267).

Click the Customization tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

267

Using Moving Mesh Model Figure 11.5: Options Dialog Box — Customization

a.

Enable Advanced Turbulence Models.

Note If the Advanced Turbulence Models option is disabled, then the default turbulence model (k-epsilon, Realizable) for turbulent flows and Reynolds Stress Model for turbulence with strong swirl will be selected without any further access to more turbulence models.

b.

Enable Advanced Boundary Condition Parameters.

Note The Advanced Boundary Condition Parameters option allows specification of heat generation rate for wall boundary.

c.

Disable Use solution steering by default.

Note The Use solution steering by default option enables solution steering mechanism to control the solution convergence automatically.

268

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Extracting Flow Volume d.

Enable Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" . The Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" option uses second order solutions after 75% accuracy settings during mesh definition. If this option is disabled, then first order solution is computed for all slider positions.

e. 5.

Select Residuals from the Convergence Criterion drop-down list.

Click OK to close the Options dialog box.

11.6. Reading the File 1.

Read the CATIA V5 file (fan_duct.CATPart) in FLUENT for CATIA V5. File → Open... This opens the File Selection dialog box, using which you can select the file to be read.

2.

Select the file, fan_duct.CATPart. By default, the file is opened in the Part or Product workbench of CATIA V5.

Tip To use the entire screen space, remove the specification tree on the left-hand side by selecting the View → Specifications menu item or pressing the F3 key on your keyboard.

11.7. Starting FLUENT for CATIA V5 1.

Launch the FfC workbench. Start → Analysis & Simulation → FLUENT for CATIA V5 This updates the graphics display. The specification tree on the left-hand side also gets updated and displays the analysis-related parameters.

2.

In the Options dialog box, specify the location of the directory where you want to store the solver files.

11.8. Extracting Flow Volume First, you will model the system using MRF zone and after its convergence you will use moving mesh zone feature available in FfC to capture the unsteady effects of interaction between rotating and stationary components of the system. In this step, you will define the inlet and outlet faces, and extract the flow volume. 1.

Click the icon or double-click the Geometry Definition.1 option located below the Environment.1 feature in the specification tree to open the Geometry Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

269

Using Moving Mesh Model

2.

Select flow volume from the Geometry definition drop-down list.

3.

Click on the field next to Inlet and select the bottom surface of the geometry.

Note To select the bottom surface of the geometry, do the following:

1. Click

icon to open the Named Views dialog box.

2. Select *bottom and click OK to close the Named Views dialog box.

4.

Similarly, define the outlet face by selecting the top surface, as shown in Figure 11.6: Flow Volume (p. 270). Figure 11.6: Flow Volume

5.

Click OK to validate and close the Geometry Definition dialog box. This creates a flow volume for the geometry. The flow volume is displayed in the graphics window. The specification tree on the left-hand side also gets updated to show relevant parameters.

270

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Materials

11.9. Materials 1.

Click the

icon to open the Library dialog box.

2.

Select the FLUENT for CATIA V5 fluids and mixtures materials library. To open the materials library, you have to specify the path where it is stored. For 32 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\intel_a\startup\materials\Fluids and Mixtures.CATmaterial For 64 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\win_b64\startup\materials\Fluids and Mixtures.CATmaterial where X-X.X.X represents the version used.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

271

Using Moving Mesh Model

3.

Drag and drop the in the graphics window.

4.

Close the Library dialog box.

icon (Air) in the Library (Read Only) dialog box on to the flow volumes

11.10. Meshing Parameters Click the icon or double-click the Mesh Definition.1 option located below the Environment.1 feature in the specification tree to open the Mesh Definition dialog box.

1.

Click Reset All. Click Reset All to revert back to default values corresponding to the slider position.

2.

Move the slide bar towards Fine till the number above it shows a value of 75. As you move the slide bar, other parameters will change accordingly. Use the Reset All button to set all the field values to their default values. Note that, if you don't use the Reset All button, the values from the previous session will be taken by FfC for meshing.

3.

In the Global tab and enter 0.4 for Critical Length.

4.

Enable Min Mesh size and set it to 0.2 mm.

5.

Click OK to close the Mesh Definition dialog box.

272

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Renaming Groups

11.11. Physics Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the FLUENT for CATIA V5 specification tree to open the Physical Model Definition dialog box.

1.

Disable Accounting for Temperature Effect.

2.

Select Turbulent in the Flow Type drop-down list.

3.

Select k-epsilon,Realizable in the Turbulence Model drop-down list.

4.

Select steady in the Time drop-down list.

5.

Click OK to validate.

11.12. Naming the Fluid Zones 1.

Click the

icon.

2.

Select any zone in the specification tree under Properties.1.

3.

Rename the smaller zone as inner-fluid-zone and rename the other fluid zone as outer-fluidzone.

11.13. Renaming Groups 1.

Select Wall (FluidtoSolid.3.0_1).2 under Groups.1 in the specification tree (Figure 11.7: Fan-Blades (p. 274)) and rename it as fan-blades.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

273

Using Moving Mesh Model Figure 11.7: Fan-Blades

2.

Similarly, rename the wall under Groups.1 as outer-wall (see Figure 11.8: Outer Wall (p. 274)). Figure 11.8: Outer Wall

3.

Similarly, rename the inlet under Groups.1 as inlet (Figure 11.9: Inlet (p. 274)). Figure 11.9: Inlet

274

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Specify MRF Zone 4.

Similarly, rename the outlet under Groups.1 as outlet (Figure 11.10: Outlet (p. 275)). Figure 11.10: Outlet

11.14. Specify MRF Zone Note The duct volume is divided into two fluid zones. You will specify rotation speed to the inner fluid zone that surrounds impeller blade and is bounded by surface of revolution. Specify the other fluid zone as stationary. •

Under Properties.1 in the specification tree, double click on the Property corresponding to the inner fluid zone Flow Property Definition dialog box.

a.

Select the Moving Reference Frame from the Motion Type drop-down list.

b.

Click the

icon to open the Rotational Inputs dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

275

Using Moving Mesh Model

c.

i.

Enable Direction.

ii.

Enter 0, 0, 1 for X, Y, Z.

iii.

Enter 1500 turn_mn for Rotational Speed.

iv.

Enable Counter Clockwise.

v.

Click OK to close the Rotational Inputs dialog box.

Click OK in the Flow Property Definition dialog box.

11.15. Specify Boundary Conditions 1.

Specify the inlet boundary conditions.

•

Click

icon to open the Inlet Boundary Condition dialog box.

There is a single inlet and outlet boundary in this example, hence they are automatically selected in the Supports field in Boundary Condition dialog boxes.

2.

276

i.

Enable Gauge Pressure (Total) and set the value to 0 N_m2.

ii.

Select External environment from the Source of Flow drop-down list.

iii.

Click OK to validate.

Specify the outlet boundary conditions.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Specify Boundary Conditions

•

3.

Click icon

to open the Outlet Boundary Condition dialog box.

i.

Ensure that 1 Outlet boundary is selected for Supports.

ii.

Enable Mass Flow Rate and set enter the value of 0.035 kg_s.

iii.

Select External Environment from the Downstream conditions drop-down

iv.

Click OK to validate.

Click the

icon.

a.

Click the text entry next to the Supports and select fan-blades in specification tree under Groups.1.

b.

Change the Name to fan-blades.

c.

Enable Moving Wall.

d.

Select Rotating in the Motion Type scrolling list.

e.

Select Relative to adjacent fluid region in the Reference Frame scrolling list.

f.

Enter 0 turn_mn for Rotational Speed. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

277

Using Moving Mesh Model g.

4.

Enable Counter Clockwise and click OK.

Click the

icon.

a.

Ensure that outer-wall is selected for Supports from the specification tree.

b.

Click the text entry next to the Supports and select outer-wall in specification tree under the Groups.1.

c.

Change the Name to outer-wall.

11.16. Operating Conditions •

Double-click Operating Conditions.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Operating Conditions dialog box. a.

Ensure that Operating Pressure is 101325.

b.

Click OK to close the Operating Conditions dialog box.

11.17. Solver Settings 1.

Double-click on Initialization Values.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Initialization Values dialog box. •

2.

Double-click on Fluent Solution.1 in the specification tree to open the Fluent Solution dialog box.

a.

278

Click Reset All and OK to validate.

Click Reset All. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Perform Computation b.

Move the Solver Accuracy Settings slide bar to 4.

c.

Ensure that Residuals is selected from the Convergence Criterion drop-down list.

d.

Click the Relaxation Settings to open Relaxation Settings dialog box. i.

Enter 0.3 for Momentum and 0.5 for Pressure.

ii.

Click OK to close the Relaxation Settings dialog box.

e.

Specify a value of 2000 iterations for Max number of iterations.

f.

Click OK to validate and close the Fluent Solution dialog box.

11.18. Perform Computation 1.

Click the

icon to open the Compute dialog box.

2.

Select All and Default Solution Option in the two drop-down lists.

3.

Click OK to validate and start the computations.

Note Solution converges after around 650 iterations. It will take a few hours to complete the solution. You can postprocess the results by interrupting the computations. Use Stop Computation button to stop the calculations.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

279

Using Moving Mesh Model Figure 11.11: Residual Plot

Note Solution converges after around 650 iterations Figure 11.11: Residual Plot (p. 280). It will take a few hours to complete the solution. You can postprocess the results by interrupting the computations. Use Stop Computation button to stop the calculations.

11.19. Save Management Save the analysis files as fan_duct_steady.CATAnalysis file and propagate directory. File → Save Management...

11.20. Applying Moving Mesh 1.

Defining physics for unsteady case. •

280

Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the FLUENT for CATIA V5 specification tree to open the Physical Model Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Applying Moving Mesh

2.

Select unsteady from the Time drop-down list.

ii.

Click OK to validate and close the Physical Model Definitions dialog box.

Create the moving mesh zone. •

3.

i.

Under Properties.1 in the specification tree, double click on the Property corresponding to the inner fluid zone Flow Property Definition dialog box.

i.

Select the Moving Mesh from the Motion Type drop-down list.

ii.

Click OK to close the Flow Property Definition dialog box.

Set the solution parameters for unsteady calculation. •

Double-click on Unsteady Parameters.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Unsteady Parameters dialog box.

i.

Select user controlled from the Transient Controls drop-down list.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

281

Using Moving Mesh Model ii.

Enter 3e-004s for Time Step Size.

iii.

Enter 400 for Number of Time Steps.

iv.

Enter 20 for Max iterations per time step.

v.

Enter 33 for Data save frequency.

vi.

Click OK to close the Unsteady Parameters dialog box.

In general, the time step size and the number of iterations per time step are determined based on the minimum mesh size on the periphery of the sliding region and rotational speed of the rotor/moving mesh. Using rotational speed, we can determine the tangential velocity of the rotor at the interface. The time step size can be determined by dividing the minimum mesh size (say in m) by tangential velocity (m/sec). The time step size specified in the FfC simulation is slightly smaller (approximately 80%) of the value obtained by the above expression. Therefore, in any given time step, the mesh advances by about 80% of the minimum mesh size on the periphery.

11.21. Solution In this step, you will define monitors and iterate the solution. 1.

2.

282

Define a surface monitor for mass flow rate at inlet. a.

Right-click on Monitors.1 in the Fluent Solution.1 set in the specification tree.

b.

Select Surface Monitor from the contextual menu to open the Surface Monitor dialog box.

i.

Enter mass-flow-rate-inlet for Name.

ii.

Click the text entry next to the Supports and select inlet in the specification tree under the Groups.1.

iii.

Select Mass Flow Rate in the Report Type drop-down list.

iv.

Select Time Step in the X-Axis Type drop-down list.

v.

Click OK to close the Surface Monitor dialog box.

Similarly, define mass-weighted total pressure monitors at the outlet.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing

The monitors will appear in the Monitors.1 list under Fluent Case feature in the specification tree. 3.

Save the analysis files as fan_duct_unsteady.CATAnalysis file and propagate directory. File → Save Management...

Note Computations of unsteady case takes more than a day. If you want to skip this step, you can use the analysis files (fan_duct_unsteady.CATAnalysis) provided with this tutorial.

4.

5.

Click the

icon to open the Compute dialog box.

a.

Select All and Continue Computation in the two drop-down lists.

b.

Click OK to validate and start the computations.

Save the analysis file once the solution is converged. File → Save Management...

11.22. Postprocessing 1.

Display the residual plot and surface monitor plots.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

283

Using Moving Mesh Model Figure 11.12: Residuals — Unsteady

Figure 11.13: Mass Flow Rate at Inlet

284

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing Figure 11.14: Mass Weighted Total Pressure at Outlet

2.

Display the contours of static and total pressures. a.

Click the

icon.

The FfC display gets updated and shows the static pressure plot. b.

Click

icon.

c.

Double-click on Pressure to open the Image Edition dialog box. i.

In the Image Edition box under Visu tab select Average-iso as Type.

ii.

Click the Selections tab and remove Flow.2 and Flow.3 from the Activated Groups.

iii.

Move fan-blade to Activated Groups.

iv.

Click OK to validate.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

285

Using Moving Mesh Model Figure 11.15: Static Pressure — Fan Blade

3.

Click

icon and repeat the same procedure described above to display contours of total pressure.

Figure 11.16: Total Pressure — Fan Blade

4.

Display the contours of static pressure along with total pressure. Ensure that both the postprocessing images are active and are displayed in the graphics window. •

Place both the images at an appropriate distance. i.

Click

icon to open the Images Layout dialog box.

ii.

Specify the parameters as shown in the dialog box and click OK to validate. This will place both the postprocessing images at some distance from each other and you can view each image individually. You may have to move the color-bands to appropriate positions manually. To move the color-map, click the color-map with the left mouse button and drag it to a suitable position.

286

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing Figure 11.17: Total Pressure and Static Pressure

5.

Display the velocity vectors.

a.

Click

icon.

Velocity contours are displayed and this is listed under Fluent Solution.1 as Velocity.1. b.

c.

Double-click on Velocity.1 to open the Image Edition dialog box. i.

In the Image Edition box under Visu tab select Symbol as Type.

ii.

Click the Selections tab and remove Flow.2 and Flow.3 from the Activated Groups.

iii.

Move fan-blade to Activated Groups.

iv.

Click

v.

Select Element (from solver) from Position drop-down list.

vi.

Click OK to validate.

to expand the Image Edition dialog box.

Repeat the procedure to display velocity vectors in Flow.2 and Flow.3 region.

Figure 11.18: Velocity Vectors on fan-blade

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

287

Using Moving Mesh Model 6.

Display the contours of turbulent kinetic energy. a.

Click the

icon.

Contour of turbulent kinetic energy will be displayed and this will be listed under Fluent Solution.1 as Turbulence Kinetic Energy (average iso).1. b.

Double-click Turbulence Kinetic Energy (average iso).1 to open the Image Edition dialog box. i.

In the Image Edition box under Visu tab select Average-iso as Type.

ii.

Click the Selections tab and remove Flow.2 and Flow.3 from the Activated Groups.

iii.

Move fan-blade to Activated Groups.

iv.

Click OK to validate.

Figure 11.19: Turbulent Kinetic Energy Over Blades

7.

Create animation of velocity vectors for inner-fluid. a.

b.

288

Double-click on Velocity.1 to open the Image Edition dialog box. i.

Click the Selections tab and select Flow.3 under activated groups.

ii.

Click OK to validate.

Click

icon to open Animation dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing

c.

i.

Click More>> (

) to show additional controls.

ii.

Enable All occurrences and Memorize frames under Animate On.

iii.

Click

to see the motion of the frames.

Save the animation. Tools → Image → Video...

Click

button to open the Video Properties dialog box.

i.

Use

to select the location and name of the video file (movie000.avi).

ii.

Click Capture tab and enable Document Window.

iii.

Click OK to close the Video Properties dialog box.

iv.

Click the record button (

v.

Click

vi.

Click the stop button (

) to start recording the animation.

in the Animation dialog box to play the animation. ) to stop the recording.

FfC will automatically save the video file in the selected directory with the specified name. Select preview to see the movie. d.

Display moving mesh at different intervals. i.

Right-click the Fluent Solution.1 option in the specification tree and select Generate Image option in the contextual menu to open the Image Generation dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

289

Using Moving Mesh Model

ii.

290

A.

Select Deformed mesh in the Available Images list.

B.

Click OK to close the Image Generation dialog box.

Double-click on Deformed mesh.1 to open the Image Edition dialog box.

A.

Click the Selections tab and remove Flow.2 and Flow.3 from the Activated Groups.

B.

Move fan-blade and outer-wall to Activated Groups.

C.

Click Occurrences tab and select 396 Step Number.

D.

Click OK to validate.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Summary Figure 11.20: Moving Mesh at Different Intervals

iii. e.

Similarly, display the moving mesh at final time step.

Creating animation of moving mesh. i.

Repeat the procedure described in previous steps.

ii.

Save the animation file as movie001.avi.

11.23. Summary In this tutorial you have learned how to setup the case using moving mesh zone feature available in FfC which is very useful in analyzing the unsteady flow through turbomachineries. This approach can also be used for turbo machinery applications in which rotor-stator interaction is of great importance. You also learned to define monitors to determine mass flow rate at inlet, and mass weighted total pressures at the outlet. To generate the report of your simulation, refer to Volatile Gas Emission Modeling Using Species Transport Model (p. 173).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

291

292

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Chapter 12: Simulation of Water Flow in a Bath Tub Using VOF Model 12.1. Introduction This tutorial examines the flow of water in a small bath tub. You will be able to predict the shape of the water free surface and its movement by using the volume of fluid (VOF) multiphase modeling capability of ANSYS Fluent. This tutorial demonstrates how to do the following: • Set up and solve a transient problem using the VOF model available in FfC. • Patch initial conditions (water levels) as desired. • Automatically save data files at defined points during the solution. • Examine the flow and water surface level interface of the two fluids using volume fraction contours.

12.2. Prerequisites This tutorial assumes that you are familiar with the menu structure in FfC. It also assumes that you have read the Getting Started (p. 1) portion of the Tutorial Guide and completed Internal Flow Calculation (p. 9). Some of the steps in setup and solution procedure will not be shown explicitly.

Note It is assumed that you have the FMS and FMD licenses available. If you do not have FMD and FMS (CATIA V5) licenses then you will not be able to generate mesh as explained in the tutorial.

12.3. Problem Description The problem considers the transient tracking of a water free surface level in the bath tub as shown in Figure 12.1: Problem Schematic (p. 294).

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

293

Simulation of Water Flow in a Bath Tub Using VOF Model Figure 12.1: Problem Schematic

The following is the chronology of events modeled in this simulation: • At time zero, some portion of the tank and the water inlet pipe is filled with water, while the rest of the domain is filled with air. To initiate the flow, the water velocity at the inlet boundary is set as 3.2 m/s. • The simulation is run for 20 milliseconds to determine the free surface level of water in the bath tub. Air will be designated as the primary phase, and water(i.e. liquid water) will be designated as the secondary phase. Patching will be required to fill the bath tub with the secondary phase in the region of the inlet pipe, and at some height from the bottom of the tank. Gravity will be included in the simulation.

12.4. Preparation 1.

Copy the CATIA V5 file, vof_tub-n.CATPart to your working directory.

2.

Start the FfC environment.

12.5. Setting the Options Tools → Options → Analysis & Simulation → Fluent Options 1.

294

Click the General tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 12.2: Options Dialog Box — General

a.

Enter the path for the ANSYS Fluent solver in the text entry box next to Folder for solver.

Note The ANSYS Fluent solver is provided with the installed FfC package. You can use the Browse button to specify the path for the solver: For 32 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/ntx86 For 64 bit the path is: FfC Installation/FfC-RX-X.X.X/solver/Fluent.Inc/ntbin/win64 Similarly, specify the path for the external postprocessor, CFD-Post (or FloWizard) executable.

b.

Set the remaining parameters as shown in Figure 12.2: Options Dialog Box — General (p. 295).

Note You can specify the Maximum number of iterations. For this tutorial the recommended value is 2000 iterations. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

295

Simulation of Water Flow in a Bath Tub Using VOF Model 2.

Click the Data Management tab in the Options dialog box. a.

Enter the path for Temporary files, FLUAnalysisComputations file and FLUAnalysisResults file in the External Storage folder group box. You can use the Browse button to specify the path. The analysis files will be saved in the temporary folders while FfC is computing the solution. The analysis will be saved to its permanent location when the computation is complete.

b.

Set the remaining parameters as shown in Figure 12.3: Options Dialog Box — Data Management (p. 296). Figure 12.3: Options Dialog Box — Data Management

3.

296

Click the Advanced Parameters tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Setting the Options Figure 12.4: Options Dialog Box — Advanced Parameters

• 4.

Set the parameters as shown in Figure 12.4: Options Dialog Box — Advanced Parameters (p. 297).

Click the Customization tab in the Options dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

297

Simulation of Water Flow in a Bath Tub Using VOF Model Figure 12.5: Options Dialog Box — Customization

a.

Enable Advanced Turbulence Models.

Note If the Advanced Turbulence Models option is disabled, then the default turbulence model (k-epsilon, Realizable) for turbulent flows and Reynolds Stress Model for turbulence with strong swirl will be selected without any further access to more turbulence models.

b.

Enable Advanced Boundary Condition Parameters.

Note The Advanced Boundary Condition Parameters option allows specification of heat generation rate for wall boundary.

c.

Enable Use solution steering by default.

Note The Use solution steering by default option enables solution steering mechanism to control the solution convergence automatically.

298

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Extracting Flow Volume d.

Enable Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" . The Control "Solver Accuracy Settings" based on slider position of "Mesh Definition" option uses second order solutions after 75% accuracy settings during mesh definition. If this option is disabled, then first order solution is computed for all slider positions.

5.

Click OK to close the Options dialog box.

12.6. Reading the File 1.

Read the CATIA V5 file (vof_tub-n.CATPart) in FLUENT for CATIA V5. File → Open... This opens the File Selection dialog box, using which you can select the file to be read.

2.

Select the file, vof_tub-n.CATPart. By default, the file is opened in the Part or Product workbench of CATIA V5.

Tip To use the entire screen space, remove the specification tree on the left-hand side by selecting the View → Specifications menu item or pressing the F3 key on your keyboard.

12.7. Starting FLUENT for CATIA V5 1.

Launch the FfC workbench. Start → Analysis & Simulation → FLUENT for CATIA V5 This updates the graphics display. The specification tree on the left-hand side also gets updated and displays the analysis-related parameters.

2.

In the Options dialog box, specify the location of the directory where you want to store the solver files.

12.8. Extracting Flow Volume In this step, you will define the inlet and outlet faces, and extract the flow volume. 1.

Click the icon or double-click the Geometry Definition.1 option located below the Environment.1 feature in the specification tree to open the Geometry Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

299

Simulation of Water Flow in a Bath Tub Using VOF Model

2.

Select solid model from the Geometry definition drop-down list.

3.

Select Edges from the Selection Mode drop-down list.

4.

Click on the field next to Dry reference Surface and select the surface of the geometry as shown in Figure 12.6: Dry reference Surface Face Selection (p. 300). Figure 12.6: Dry reference Surface Face Selection

5.

Select Tangent continuity from the Propagation type drop-down list.

6.

Click on the field next to Inlet and select the inner edge of the inlet pipe and the edge of the tub, as shown in Figure 12.7: Inlet Edges Selection (p. 301).

300

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Extracting Flow Volume Figure 12.7: Inlet Edges Selection

When you select one outer edge of the tub, the remaining eight edges are also selected. 7.

Similarly, define the outlet edge by selecting the edge of the tub and the edge of the drain as shown in Figure 12.8: Outlet Edge Selection (p. 301). Figure 12.8: Outlet Edge Selection

8.

Click OK to validate and close the Geometry Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

301

Simulation of Water Flow in a Bath Tub Using VOF Model Figure 12.9: Extracted Flow Volume

This creates a flow volume for the geometry. The flow volume is displayed in the graphics window, see Figure 12.9: Extracted Flow Volume (p. 302). The specification tree on the left-hand side also gets updated to show relevant parameters.

12.9. Split Flow Volume 1.

Set the view from rendering style to perspective. View → Render Style → Perspective

2.

Right-click on Geometry Definition from the specification tree and click on Split flow volumes.

3.

Zoom in on the inlet pipe from the inside of the tub. You may have to hide the surface to see it.

4.

Enable Edge selection by propagation.

5.

Select Point continuity from the Propagation type drop-down list.

302

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Meshing Parameters Figure 12.10: Split Flow Volumes

6.

Select the face of the inlet pipe for Propagation support surface.

7.

Click on the text field next to Geometry. a.

Select the inside edge of the inlet pipe. See Figure 12.10: Split Flow Volumes (p. 303).

b.

Select Plane.2 from the specification tree under Links Manager.1 for Geometry. Expand Links Manager.1 and tub(tub.1) to locate Plane.2

8.

Click OK. The flow volume is now split into three parts.

12.10. Meshing Parameters Click the icon or double-click the Mesh Definition.1 option located below the Environment.1 feature in the specification tree to open the Mesh Definition dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

303

Simulation of Water Flow in a Bath Tub Using VOF Model

1.

Click Reset All. Click Reset All to revert back to default values corresponding to the slider position.

2.

Use the default Optimized Surface mesher (proximity detection) as the Mesh Type.

3.

Move the slide bar towards Fine till the number above it shows a value of 75. As you move the slide bar, other parameters will change accordingly. Use the Reset All button to set all the field values to their default values. Note that, if you don't use the Reset All button, the values from the previous session will be taken by FfC for meshing.

4.

In the Global tab and enter 2mm for Critical Length.

5.

Click on the Geometry tab and retain the default settings as shown.

304

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Physics

6.

Click on the Surface mesh tab and retain the default settings as shown.

7.

Click OK to close the Mesh Definition dialog box.

12.11. Physics Click the icon or double-click the Physics Definition.1 option located below the Environment.1 feature in the FLUENT for CATIA V5 specification tree to open the Physical Model Definition dialog box.

1.

Disable Accounting for Temperature Effect.

2.

Select Laminar in the Flow Type drop-down list.

3.

Select unsteady from the Time drop-down list.

4.

Select Multiphase in the Model Definition drop-down list.

5.

Select VOF as the Multiphase Model.

6.

Click OK to validate and close the Physical Model Definition dialog box. . Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

305

Simulation of Water Flow in a Bath Tub Using VOF Model

12.12. Materials 1.

Click the

icon to open the Library dialog box.

2.

Select the FLUENT for CATIA V5 fluids and mixtures materials library. To open the materials library, you have to specify the path where it is stored. For 32 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\intel_a\startup\materials\Fluids and Mixtures.CATmaterial For 64 bit the path is: C:\Program Files\FfC\FfC-RX-X.X.X\win_b64\startup\materials\Fluids and Mixtures.CATmaterial where X-X.X.X represents the version used.

3.

Drag and drop the in the graphics window.

4.

Click the

306

icon (Air) in the Library (Read Only) dialog box on to the flow volumes

User Material icon.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Operating Conditions 5.

Select Water-liquid in the Library (Read Only) dialog box and click on Apply Material.

6.

Close the Library dialog box. The materials are updated in the tree.

12.13. VOF Specifications 1.

Double-click on VOF.1 under Fluent Problem Setup.1 in the tree to open the Multiphase Definition dialog box.

You can see that Air is selected as the Primary Phase Material. 2.

Click on the text field next to Material to select the secondary phase.

3.

Click on Water-liquid.01 from the tree under Materials.1.

4.

Select Implicit from the VOF Scheme drop-down list.

5.

Enable Implicit Body Force.

6.

Click on Phases Interaction and enter 0.07 N_m for Surface Tension Coefficients.

12.14. Operating Conditions Double-click Operating Conditions.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Operating Conditions dialog box.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

307

Simulation of Water Flow in a Bath Tub Using VOF Model

1.

Ensure that Operating Pressure is 101325 N_m2.

2.

Enter 300 mm for Z Coordinate in Reference Pressure Location group.

3.

Ensure that the X and Y Coordinates are 0mm.

4.

Enable Gravity.

5.

Enter -9.81 m_s2 for the Z Component in the Gravitational Acceleration group.

6.

Ensure that the X and Y Components are 0 m_s2.

7.

Ensure that Operating Temperature is set to 288.16Kdeg.

8.

Click OK to validate and close the Operating Conditions dialog box.

12.15. Specify Boundary Conditions 1.

Specify the inlet boundary conditions.

•

Click i.

icon to open the Inlet Boundary Condition dialog box. Select the inlet boundary which corresponds to the surface of the inlet pipe. This automatically updates the Supports field.

308

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Specify Boundary Conditions ii.

Select Velocity Inlet from the Inlet Type drop-down list.

iii.

Click on Phases Input.

iv.

2.

3.

A.

Enter 3.2 m_s for Velocity Magnitude, for both primary and secondary phase.

B.

Enter 1 for Volume Fraction.

C.

Click OK.

Click OK to validate.

Similarly specify the second inlet boundary conditions.

a.

Ensure that the upper surface of the tub is selected for Supports.

b.

Select Pressure Inlet as the Inlet Type.

c.

Ensure that Gauge Pressure (Total) is 0 N_m2.

d.

Ensure that Volume Fraction is 0 by clicking on Phases Input.

Specify the outlet boundary conditions.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

309

Simulation of Water Flow in a Bath Tub Using VOF Model a.

Click icon

to open the Outlet Boundary Condition dialog box.

b.

Ensure that the boundary which corresponds to the drain hole at the bottom of the tub is selected.

c.

Enable Gauge Pressure (static) and set the value to 0 N_m2.

d.

Click on Phases Input and enter 1 for Volume Fraction.

e.

Click OK to validate.

12.16. Patch the Secondary Phase 1.

Click on

from the Boundary Conditions toolbar.

2.

Select the flow properties corresponding to the inlet pipe, and the lower two split levels from the specification tree under Properties.1. This automatically updates the Supports field.

3.

Select Secondary Phase 1 from the Patch Quantity drop-down list.

4.

Ensure that Volume fraction is set to 1.

12.17. Unsteady Settings 1.

Double-click on Unsteady Parameters.1 from the tree under Fluent Problem Setup.1 to open the Unsteady Parameters dialog box.

2.

Select user controlled from the Transient Controls drop-down list.

3.

Enter 0.001 s for the Time Step Size.

4.

Ensure that Number of Time Steps is 20.

5.

Enter 50 for Max. iterations per time Step.

310

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Solver Settings 6.

Enter 4 for Data save frequency. You can enter a different value for Data save frequency depending upon your requirement.

7.

Click OK to validate and close the dialog box.

12.18. Solver Settings 1.

2.

Double-click on Initialization Values.1 below the Fluent Problem Setup.1 feature in the specification tree to open the Initialization Values dialog box.

a.

Click Reset All.

b.

Click on Phases Input, enable and set Volume Fraction to 0.

c.

Click OK to validate.

Double-click on Fluent Solution.1 in the specification tree to open the Fluent Solution dialog box.

a.

Click Reset All.

b.

Move the Solver Accuracy Settings slide bar to 4.

c.

Ensure that Residuals is selected from the Convergence Criterion drop-down list.

d.

Click on Residual Convergence Criteria.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

311

Simulation of Water Flow in a Bath Tub Using VOF Model

e.

i.

Ensure that none are enabled.

ii.

Click on Phases Input and enter 0.001 for Volume Fraction.

Click OK to close the Fluent Solution dialog box.

12.19. Save Management Save the analysis files as vof.CATAnalysis file and propagate directory. File → Save Management...

12.20. Perform Computation 1.

Click the

icon to open the Compute dialog box.

2.

Select All and Default Solution Option in the two drop-down lists.

3.

Click OK to validate and start the computations. Figure 12.11: Residual Plot

12.21. Postprocessing 1.

Display the contours of volume fraction. a.

312

Click the

icon. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Postprocessing

b.

Select Secondary Phase.1 Solution from the Phases dialog box. In the Occurrences tab of the Image Edition dialog box, you can select the Time Step at which you want to display the contours.

Figure 12.12: Volume fraction at time step 4

Figure 12.13: Volume fraction at time step 12

Figure 12.14: Volume fraction at time step 20

2.

Display velocity contours on a cut plane.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

313

Simulation of Water Flow in a Bath Tub Using VOF Model

a.

Click the

icon.

Velocity contours are displayed and this is listed under Fluent Solution.1 as Velocity.1. b.

Click the

icon to open the Cut Plane Analysis dialog box.

i.

Enable View section only.

ii.

Disable Show cutting plane.

iii.

Enable Clipping.

iv.

Adjust the position of the plane using the compass, so that the plane cuts the tank vertically into two equal parts. See Figure 12.15: Cut Plane Image of Velocity Contours at Time Step 20 (p. 314).

Figure 12.15: Cut Plane Image of Velocity Contours at Time Step 20

3.

Click the a.

Open the Image Edition dialog box.

b.

Click on Options... button in the Visu tab to open the Visualization Options dialog box.

c.

314

icon.

i.

Disable Variable.

ii.

Increase Maximum length to 8 so that the vectors are clearly visible.

iii.

Click OK to validate and close the Visualization Options dialog box.

Click the

icon to open the Cut Plane Analysis dialog box.

i.

Enable View section only.

ii.

Disable Show cutting plane. Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

Summary iii.

Enable Clipping.

iv.

Enable Project vectors on plane.

v.

Adjust the position of the plane using the compass, so that the plane cuts the tank vertically into two equal parts. See Figure 12.16: Cut Plane Image of Velocity Vectors (p. 315).

Figure 12.16: Cut Plane Image of Velocity Vectors

Note You can create an animation for velocity. Refer to Using Moving Mesh Model (p. 263) for more information on creating animation.

12.22. Summary This tutorial demonstrated the application of the volume of fluid method with surface tension effects. The problem involved the free surface level determination of water and postprocessing showed how the position and shape of the surface between the two immiscible fluids changed over time.

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.

315

316

Release 19.2 - © ANSYS, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.