ANSYS ICEM CFD Help Manual - Portal de Documentacion de

ANSYS ICEM CFD Help Manual - Portal de Documentacion de
ANSYS ICEM CFD Help Manual
ANSYS, Inc.
Southpointe
275 Technology Drive
Canonsburg, PA 15317
[email protected]
http://www.ansys.com
(T) 724-746-3304
(F) 724-514-9494
ANSYS ICEM CFD 15.0
November 2013
ANSYS, Inc. is
certified to ISO
9001:2008.
Copyright and Trademark Information
© 2013 SAS IP, Inc. All rights reserved. Unauthorized use, distribution or duplication is prohibited.
ANSYS, ANSYS Workbench, Ansoft, AUTODYN, EKM, Engineering Knowledge Manager, CFX, FLUENT, HFSS and any
and all ANSYS, Inc. brand, product, service and feature names, logos and slogans are registered trademarks or
trademarks of ANSYS, Inc. or its subsidiaries in the United States or other countries. ICEM CFD is a trademark used
by ANSYS, Inc. under license. CFX is a trademark of Sony Corporation in Japan. All other brand, product, service
and feature names or trademarks are the property of their respective owners.
Disclaimer Notice
THIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION INCLUDE TRADE SECRETS AND ARE CONFIDENTIAL AND PROPRIETARY PRODUCTS OF ANSYS, INC., ITS SUBSIDIARIES, OR LICENSORS. The software products
and documentation are furnished by ANSYS, Inc., its subsidiaries, or affiliates under a software license agreement
that contains provisions concerning non-disclosure, copying, length and nature of use, compliance with exporting
laws, warranties, disclaimers, limitations of liability, and remedies, and other provisions. The software products
and documentation may be used, disclosed, transferred, or copied only in accordance with the terms and conditions
of that software license agreement.
ANSYS, Inc. is certified to ISO 9001:2008.
U.S. Government Rights
For U.S. Government users, except as specifically granted by the ANSYS, Inc. software license agreement, the use,
duplication, or disclosure by the United States Government is subject to restrictions stated in the ANSYS, Inc.
software license agreement and FAR 12.212 (for non-DOD licenses).
Third-Party Software
See the legal information in the product help files for the complete Legal Notice for ANSYS proprietary software
and third-party software. If you are unable to access the Legal Notice, please contact ANSYS, Inc.
Published in the U.S.A.
Table of Contents
Main Menu Area ......................................................................................................................................... 1
File Menu ............................................................................................................................................... 1
Project Management Options ........................................................................................................... 2
Entity Management Options ............................................................................................................. 4
Geometry ................................................................................................................................... 5
Mesh .......................................................................................................................................... 7
Blocking ..................................................................................................................................... 9
Attributes ................................................................................................................................. 11
Parameters ............................................................................................................................... 12
Cartesian .................................................................................................................................. 13
Import/Export Options ................................................................................................................... 13
Import Model ........................................................................................................................... 14
Import Geometry ..................................................................................................................... 22
Faceted .............................................................................................................................. 23
ICEM CFD Mesh ............................................................................................................ 23
Nastran ........................................................................................................................ 23
Patran .......................................................................................................................... 23
STL ............................................................................................................................... 24
VRML ........................................................................................................................... 24
Legacy ............................................................................................................................... 24
Acis ............................................................................................................................. 26
CATIA V4 ....................................................................................................................... 27
DWG ............................................................................................................................ 29
GEMS ........................................................................................................................... 30
IDI ................................................................................................................................ 30
ParaSolid ...................................................................................................................... 31
Rhino 3DM ................................................................................................................... 32
Plot3d .......................................................................................................................... 33
STEP / IGES .................................................................................................................. 34
Formatted Point Data ......................................................................................................... 35
Reference Geometry ........................................................................................................... 36
Import Mesh ............................................................................................................................. 37
From ANSYS ....................................................................................................................... 37
From Abaqus ...................................................................................................................... 37
From CFX ........................................................................................................................... 37
From CGNS ......................................................................................................................... 39
From Fluent ........................................................................................................................ 39
From LS-DYNA .................................................................................................................... 39
From Nastran ...................................................................................................................... 39
From Patran ........................................................................................................................ 40
From Plot3d ........................................................................................................................ 40
From Starcd ........................................................................................................................ 40
From STL ............................................................................................................................ 40
From TecPlot ....................................................................................................................... 41
From Vectis ......................................................................................................................... 41
Export Geometry ...................................................................................................................... 41
To IGES ............................................................................................................................... 42
To Parasolid ........................................................................................................................ 42
To Rhino 3DM ..................................................................................................................... 43
To STL ................................................................................................................................ 44
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
iii
Help Manual
Export Mesh ............................................................................................................................. 44
To Abaqus .......................................................................................................................... 45
To ANSYS ............................................................................................................................ 45
To Autodyn ......................................................................................................................... 46
To Exodus ........................................................................................................................... 46
To Ideas .............................................................................................................................. 47
To LS-DYNA ........................................................................................................................ 47
To Nastran .......................................................................................................................... 47
To Patran ............................................................................................................................ 48
To Radioss .......................................................................................................................... 48
To FE Modeler ..................................................................................................................... 48
Write STL file ....................................................................................................................... 49
Spectral Elements ............................................................................................................... 49
Replay Scripts ................................................................................................................................. 49
Exit ................................................................................................................................................. 53
Edit Menu ............................................................................................................................................. 53
Undo .............................................................................................................................................. 53
Redo .............................................................................................................................................. 54
Clear Undo ..................................................................................................................................... 54
Shell ............................................................................................................................................... 54
Facets > Mesh ................................................................................................................................. 54
Mesh > Facets ................................................................................................................................. 54
Struct Mesh > CAD Surfaces ............................................................................................................ 54
Struct Mesh > Unstruct Mesh .......................................................................................................... 54
Struct Mesh > Super Domain .......................................................................................................... 54
Shrink Tetin File .............................................................................................................................. 55
View Menu ........................................................................................................................................... 55
Fit .................................................................................................................................................. 55
Box Zoom ....................................................................................................................................... 56
Top ................................................................................................................................................ 56
Bottom ........................................................................................................................................... 56
Left ................................................................................................................................................ 56
Right .............................................................................................................................................. 56
Front .............................................................................................................................................. 56
Back ............................................................................................................................................... 56
Isometric ........................................................................................................................................ 56
View Control ................................................................................................................................... 56
Save Picture .................................................................................................................................... 57
Mirror and Replicates ...................................................................................................................... 59
Annotation ..................................................................................................................................... 60
Add in the current window ....................................................................................................... 60
Modify by selecting .................................................................................................................. 61
Pick and move .......................................................................................................................... 61
Pick and remove ....................................................................................................................... 61
Reset mouse ............................................................................................................................. 61
Add Marker .................................................................................................................................... 62
Clear Markers ................................................................................................................................. 62
Mesh Cut Plane ............................................................................................................................... 62
Info Menu ............................................................................................................................................. 64
Geometry Info ................................................................................................................................ 65
Surface Area ................................................................................................................................... 65
Frontal Area .................................................................................................................................... 65
iv
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Help Manual
Curve Length .................................................................................................................................. 65
Curve Direction .............................................................................................................................. 65
Mesh Info ....................................................................................................................................... 65
Mesh Area/Volume ......................................................................................................................... 66
Element Info ................................................................................................................................... 66
Node Info ....................................................................................................................................... 67
Element Type/ Property Info ............................................................................................................ 67
Toolbox .......................................................................................................................................... 67
Project File ..................................................................................................................................... 67
Domain File .................................................................................................................................... 67
Mesh Report ................................................................................................................................... 67
Settings Menu ...................................................................................................................................... 69
General .......................................................................................................................................... 70
Product .......................................................................................................................................... 71
Display ........................................................................................................................................... 73
Speed ............................................................................................................................................. 78
Memory ......................................................................................................................................... 78
Lighting ......................................................................................................................................... 79
Background Style ........................................................................................................................... 80
Mouse Bindings/Spaceball .............................................................................................................. 81
Selection ........................................................................................................................................ 83
Remote .......................................................................................................................................... 85
Model/Units ................................................................................................................................... 85
Geometry Options .......................................................................................................................... 88
Meshing ......................................................................................................................................... 90
Hexa Meshing .......................................................................................................................... 90
Quality/Histogram Info ............................................................................................................. 94
Edge Info .................................................................................................................................. 96
Solver ............................................................................................................................................. 96
Reset .............................................................................................................................................. 97
Help Menu ........................................................................................................................................... 98
Help Topics ..................................................................................................................................... 98
Tutorial Manual .............................................................................................................................. 98
User’s Manual ................................................................................................................................. 98
Programmer’s Guide ....................................................................................................................... 98
Output Interfaces ........................................................................................................................... 99
Installation & Licensing Guide ......................................................................................................... 99
What's New .................................................................................................................................... 99
Show Customer Number ................................................................................................................. 99
About ANSYS ICEM CFD .................................................................................................................. 99
Graphical Main Menu, Utilities and Display Options ............................................................................... 99
Main Menu Icons .......................................................................................................................... 100
Utilities Icons ................................................................................................................................ 102
Display Management Icons ........................................................................................................... 104
Selecting Entities, Keyboard and Mouse Functions ............................................................................... 107
Selection Options ............................................................................................................................... 107
Selection Mode Keymap ............................................................................................................... 107
Location Selection Toolbar ............................................................................................................ 111
Geometry Selection Toolbar .......................................................................................................... 112
Mesh Selection Toolbar ................................................................................................................. 114
Blocking Selection Toolbars ........................................................................................................... 116
Density Selection Toolbar .............................................................................................................. 119
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
v
Help Manual
Hotkeys .............................................................................................................................................. 120
Geometry ..................................................................................................................................... 121
Blocking ....................................................................................................................................... 123
Edit Mesh ..................................................................................................................................... 124
Spaceball and Mouse Binding ............................................................................................................. 125
Display Tree ............................................................................................................................................. 127
Model ................................................................................................................................................. 128
Geometry ........................................................................................................................................... 128
Geometry Subsets Options ........................................................................................................... 129
Modify Geometry Subset Options ................................................................................................. 131
Geometry Points Options .............................................................................................................. 133
Geometry Curves Options ............................................................................................................. 134
Geometry Surfaces Options .......................................................................................................... 136
Geometry Bodies Options ............................................................................................................. 138
Geometry Densities Options ......................................................................................................... 139
Mesh .................................................................................................................................................. 140
Mesh Display Options ................................................................................................................... 141
Mesh Subsets ............................................................................................................................... 145
Modify Mesh Subsets .................................................................................................................... 148
Mesh Points .................................................................................................................................. 154
Mesh Lines ................................................................................................................................... 154
Mesh Shells .................................................................................................................................. 154
Mesh Volumes .............................................................................................................................. 158
Blocking ............................................................................................................................................. 158
Blocking Options .......................................................................................................................... 159
Blocking Subset Options ............................................................................................................... 160
Modify Subsets Options ................................................................................................................ 161
Vertices ........................................................................................................................................ 162
Edges ........................................................................................................................................... 163
Faces ............................................................................................................................................ 164
Blocks ........................................................................................................................................... 164
Pre-Mesh ...................................................................................................................................... 166
Topology ...................................................................................................................................... 171
Local Coordinate Systems ................................................................................................................... 171
Element Properties ............................................................................................................................. 172
Connectors ........................................................................................................................................ 173
Constrained Nodes ............................................................................................................................. 173
Contacts ............................................................................................................................................. 174
Displacements .................................................................................................................................... 175
Loads ................................................................................................................................................. 176
Material Properties ............................................................................................................................. 177
Rigid Walls .......................................................................................................................................... 177
Single Surface Contacts ...................................................................................................................... 178
Temperatures ..................................................................................................................................... 178
Velocities ............................................................................................................................................ 179
Parts ................................................................................................................................................... 180
Parts Display Options .................................................................................................................... 180
Create Part ............................................................................................................................. 180
Create Assembly ..................................................................................................................... 182
More Part Display Options ....................................................................................................... 185
Parameters ......................................................................................................................................... 190
Subcases ............................................................................................................................................ 191
vi
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Help Manual
Geometry ................................................................................................................................................ 193
Create Point ........................................................................................................................................ 193
Screen Select ................................................................................................................................ 194
Explicit Coordinates ...................................................................................................................... 194
Base Point and Delta ..................................................................................................................... 195
Center of 3 Points/Arc ................................................................................................................... 195
Based on 2 Locations .................................................................................................................... 195
Curve Ends ................................................................................................................................... 196
Curve-Curve Intersection .............................................................................................................. 196
Parameter along a Curve ............................................................................................................... 197
Project Point to Curve ................................................................................................................... 197
Project Point to Surface ................................................................................................................. 197
Create/Modify Curve ........................................................................................................................... 197
From Points .................................................................................................................................. 198
Arc from 3 Points .......................................................................................................................... 198
Circle from Center and 2 Points ..................................................................................................... 198
Surface Parameters ....................................................................................................................... 199
Surface-Surface Intersection ......................................................................................................... 200
Project Curve on Surface ............................................................................................................... 200
Segment Curve ............................................................................................................................. 201
Concatenate/Reapproximate Curves ............................................................................................. 201
Extract Curves from Surfaces ......................................................................................................... 202
Modify Curves .............................................................................................................................. 202
Create Midline .............................................................................................................................. 206
Create Section Curves ................................................................................................................... 206
Create/Modify Surface ........................................................................................................................ 207
From Curves ................................................................................................................................. 207
Curve Driven ................................................................................................................................ 208
Sweep Surface .............................................................................................................................. 208
Surface of Revolution .................................................................................................................... 209
Loft Surface over Several Curves .................................................................................................... 209
Offset Surface ............................................................................................................................... 209
Midsurface ................................................................................................................................... 210
Segment/Trim Surface .................................................................................................................. 213
Merge/Reapproximate Surfaces .................................................................................................... 213
Untrim Surface ............................................................................................................................. 214
Create Curtain Surface .................................................................................................................. 214
Extend Surface ............................................................................................................................. 215
Geometry Simplification ............................................................................................................... 217
Standard Shapes ........................................................................................................................... 221
Create Body ........................................................................................................................................ 224
By Topology .................................................................................................................................. 225
By Material Point ........................................................................................................................... 226
Create/Modify Faceted ........................................................................................................................ 227
Create/Edit Faceted Curves ........................................................................................................... 227
Convert from Bspline .............................................................................................................. 228
Create Curve ........................................................................................................................... 228
Move Nodes ........................................................................................................................... 228
Merge Nodes .......................................................................................................................... 229
Create Segments .................................................................................................................... 229
Delete Segments .................................................................................................................... 229
Split Segment ......................................................................................................................... 229
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
vii
Help Manual
Restrict Segment .................................................................................................................... 229
Move to New Curve ................................................................................................................ 229
Move to Existing Curve ........................................................................................................... 229
Surfaces ....................................................................................................................................... 229
Convert from Bspline .............................................................................................................. 230
Coarsen Surface ...................................................................................................................... 231
Create New Surface ................................................................................................................ 231
Merge Edges .......................................................................................................................... 231
Split Edge ............................................................................................................................... 232
Swap Edge ............................................................................................................................. 232
Move Nodes ........................................................................................................................... 233
Merge Nodes .......................................................................................................................... 233
Create Triangles ...................................................................................................................... 234
Delete Triangles ...................................................................................................................... 234
Split Triangles ......................................................................................................................... 235
Delete Non-Selected Triangles ................................................................................................ 236
Move to New Surface .............................................................................................................. 236
Move to Existing Surface ......................................................................................................... 236
Merge Surfaces ....................................................................................................................... 236
Faceted Cleanup ........................................................................................................................... 236
Align Edge to Curve ................................................................................................................ 237
Close Faceted Holes ................................................................................................................ 237
Trim By Screen ........................................................................................................................ 238
Trim By Surface Selection ........................................................................................................ 238
Repair Surface ........................................................................................................................ 238
Create Character Curve ........................................................................................................... 239
Repair Geometry ................................................................................................................................ 241
Build Topology .............................................................................................................................. 242
Check Geometry ........................................................................................................................... 245
Close Holes ................................................................................................................................... 246
Remove Holes ............................................................................................................................... 246
Stitch/Match Edges ....................................................................................................................... 247
Using Stitch/Match Edges for Y-Junctions ................................................................................ 249
Split Folded Surfaces ..................................................................................................................... 250
Adjust Varying Thickness ............................................................................................................... 250
From Solid Method ................................................................................................................. 250
Specify Corners Method .......................................................................................................... 251
Find Surfaces Without Thickness Assigned ............................................................................... 251
Make Normals Consistent .............................................................................................................. 251
Feature Detect Bolt Holes .............................................................................................................. 252
Feature Detect Buttons ................................................................................................................. 254
Feature Detect Fillets .................................................................................................................... 255
Transform Geometry ........................................................................................................................... 256
Translation ................................................................................................................................... 257
Rotation ....................................................................................................................................... 257
Mirror Geometry ........................................................................................................................... 258
Scale Geometry ............................................................................................................................ 258
Translate and Rotate ..................................................................................................................... 258
Restore Dormant Entities .................................................................................................................... 259
Delete Point ........................................................................................................................................ 259
Delete Curve ....................................................................................................................................... 260
Delete Surface .................................................................................................................................... 260
viii
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Help Manual
Delete Body ........................................................................................................................................ 260
Delete Any Entity ................................................................................................................................ 260
Mesh ........................................................................................................................................................ 261
Global Mesh Setup .............................................................................................................................. 261
Global Mesh Size .......................................................................................................................... 267
Shell Meshing Parameters ............................................................................................................. 270
Autoblock Options .................................................................................................................. 272
Patch Dependent Options ....................................................................................................... 273
Patch Independent Options .................................................................................................... 280
Shrinkwrap Options ................................................................................................................ 280
Volume Meshing Parameters ......................................................................................................... 281
Tetra/Mixed ............................................................................................................................ 281
Robust (Octree) ................................................................................................................ 281
Quick (Delaunay) .............................................................................................................. 286
Smooth (Advancing Front) ................................................................................................ 287
Hexa-Dominant ...................................................................................................................... 288
Cartesian ................................................................................................................................ 288
Body-Fitted ....................................................................................................................... 289
Hexa-Core ........................................................................................................................ 293
Prism Meshing Parameters ............................................................................................................ 294
Global Prism Settings .............................................................................................................. 294
Prism Element Part Controls .................................................................................................... 305
Smoothing Options ................................................................................................................ 306
Advanced Prism Meshing Parameters ...................................................................................... 307
Periodicity Set Up ......................................................................................................................... 312
Part Mesh Setup ................................................................................................................................. 315
Surface Mesh Setup ............................................................................................................................ 318
Curve Mesh Setup ............................................................................................................................... 320
Create Mesh Density ........................................................................................................................... 327
Define Connectors .............................................................................................................................. 329
Arbitrary Connectors .................................................................................................................... 329
Bolt Weld Connectors .................................................................................................................... 330
Seam Weld Connectors ................................................................................................................. 330
Spot Weld Connectors .................................................................................................................. 333
Spot Weld From File ...................................................................................................................... 335
Mesh Curve ........................................................................................................................................ 336
Compute Mesh ................................................................................................................................... 336
Compute Surface Mesh ................................................................................................................. 336
Compute Volume Mesh ................................................................................................................. 337
Tetra/Mixed Mesh Type ........................................................................................................... 337
Hexa-Dominant Mesh Type ..................................................................................................... 341
Cartesian Mesh Type ............................................................................................................... 341
Body-Fitted Mesh Method ................................................................................................. 341
Compute Prism Mesh .................................................................................................................... 346
Blocking .................................................................................................................................................. 349
Create Block ....................................................................................................................................... 349
Initialize Block ............................................................................................................................... 350
From Vertices/Faces ...................................................................................................................... 357
3D Blocks ................................................................................................................................ 357
2D Blocks ................................................................................................................................ 362
Extrude Face ................................................................................................................................. 363
Interactive .............................................................................................................................. 363
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
ix
Help Manual
Fixed Distance ........................................................................................................................ 363
Extrude Along Curve ............................................................................................................... 364
2D to 3D Blocks ............................................................................................................................ 365
3D to 2D ....................................................................................................................................... 371
Split Block .......................................................................................................................................... 371
Split Block .................................................................................................................................... 372
Ogrid Block ................................................................................................................................... 373
Extend Split .................................................................................................................................. 376
Split Face ...................................................................................................................................... 377
Split Vertices ................................................................................................................................. 378
Split Free Face ............................................................................................................................... 379
Imprint Free Face .......................................................................................................................... 379
Split Free Block ............................................................................................................................. 381
Merge Vertices .................................................................................................................................... 382
Merge Vertices .............................................................................................................................. 382
Merge Vertices by Tolerance .......................................................................................................... 385
Collapse Block .............................................................................................................................. 385
Merge Vertex to Edge .................................................................................................................... 385
Edit Block ........................................................................................................................................... 388
Merge Blocks ................................................................................................................................ 388
Merge Faces ................................................................................................................................. 389
Modify Ogrid ................................................................................................................................ 389
Periodic Vertices ........................................................................................................................... 389
Convert Block Type ....................................................................................................................... 390
Change Block IJK .......................................................................................................................... 395
Renumber Blocks .......................................................................................................................... 395
Associate ............................................................................................................................................ 395
Associate Vertex ........................................................................................................................... 396
Associate Edge to Curve ................................................................................................................ 396
Associate Edge to Surface ............................................................................................................. 397
Associate Face to Surface .............................................................................................................. 398
Disassociate from Geometry ......................................................................................................... 401
Update Associations ..................................................................................................................... 401
Reset Associations ........................................................................................................................ 403
Snap Project Vertices .................................................................................................................... 404
Group/Ungroup Curves ................................................................................................................ 405
Auto Associate .............................................................................................................................. 405
Move Vertex ....................................................................................................................................... 405
Move Vertex ................................................................................................................................. 406
Set Location ................................................................................................................................. 407
Align Vertices ................................................................................................................................ 408
Align Vertices In-line ..................................................................................................................... 408
Set Edge Length ........................................................................................................................... 408
Move Face Vertices ........................................................................................................................ 409
Transform Blocks ................................................................................................................................ 409
Translate Blocks ............................................................................................................................ 410
Rotate Blocks ................................................................................................................................ 410
Mirror Blocks ................................................................................................................................ 410
Scale Blocks .................................................................................................................................. 411
Copy Periodic Blocking ................................................................................................................. 411
Translate and Rotate ..................................................................................................................... 411
Edit Edge ............................................................................................................................................ 412
x
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Help Manual
Split Edge ..................................................................................................................................... 412
Unsplit Edge ................................................................................................................................. 414
Link Edge ..................................................................................................................................... 414
Unlink Edge .................................................................................................................................. 414
Change Edge Split Type ................................................................................................................ 415
Pre-Mesh Params ................................................................................................................................ 415
Update Sizes ................................................................................................................................. 415
Scale Sizes .................................................................................................................................... 418
Edge Params ................................................................................................................................. 419
Bunching Laws ....................................................................................................................... 422
Match Edges ................................................................................................................................. 425
Refinement ................................................................................................................................... 426
Pre-Mesh Quality ................................................................................................................................ 427
Pre Mesh Quality Options .............................................................................................................. 428
Angle ..................................................................................................................................... 429
Aspect Ratio ........................................................................................................................... 429
Constant Radius ...................................................................................................................... 429
Custom Quality ....................................................................................................................... 429
Determinant (2x2x2 stencil) .................................................................................................... 430
Determinant (3x3x3 stencil) .................................................................................................... 430
Distortion ............................................................................................................................... 430
Equiangle Skewness ............................................................................................................... 430
Eriksson Skewness .................................................................................................................. 431
Ford ....................................................................................................................................... 431
Hex. Face Aspect Ratio ............................................................................................................ 431
Hex. Face Distortion ................................................................................................................ 431
Max Angle .............................................................................................................................. 431
Max Dihedral Angle ................................................................................................................ 431
Max Length ............................................................................................................................ 431
Max Ortho .............................................................................................................................. 432
Max Ortho 4.3v ....................................................................................................................... 432
Max Ratio ............................................................................................................................... 432
Max Sector Volume ................................................................................................................. 432
Max Side ................................................................................................................................. 432
Max Warp ............................................................................................................................... 432
Max Warp 4.3v ........................................................................................................................ 432
Mid Node ............................................................................................................................... 433
Mid Node Angle ..................................................................................................................... 433
Min Angle ............................................................................................................................... 433
Min Ortho ............................................................................................................................... 433
Min Sector Volume .................................................................................................................. 433
Min Side ................................................................................................................................. 433
Opp Face Area Ratio ................................................................................................................ 433
Opp. Face Parallelism .............................................................................................................. 434
Orientation ............................................................................................................................. 434
Quality ................................................................................................................................... 434
Taper ...................................................................................................................................... 435
Volume ................................................................................................................................... 435
Volume Change ...................................................................................................................... 435
Warpage ................................................................................................................................. 435
X Size ..................................................................................................................................... 435
Y Size ..................................................................................................................................... 435
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
xi
Help Manual
Z Size ..................................................................................................................................... 435
Pre-Mesh Quality Histogram ......................................................................................................... 436
Pre-Mesh Smooth ............................................................................................................................... 437
Quality Method ............................................................................................................................ 437
Orthogonality Method .................................................................................................................. 439
Multiblock Method ....................................................................................................................... 444
Block Checks ...................................................................................................................................... 449
Delete Block ....................................................................................................................................... 449
Edit Mesh ................................................................................................................................................ 451
Create Elements .................................................................................................................................. 451
Node (Point Element) .................................................................................................................... 452
Bar (Line Element) ......................................................................................................................... 453
Triangle ........................................................................................................................................ 453
Quad ............................................................................................................................................ 454
Tetra ............................................................................................................................................. 455
Prism ............................................................................................................................................ 455
Pyramid ........................................................................................................................................ 456
Hexa ............................................................................................................................................. 456
Auto Element Type ........................................................................................................................ 457
Extrude Mesh ..................................................................................................................................... 458
Extrude by Element Normal .......................................................................................................... 458
Extrude Along Curve ..................................................................................................................... 459
Extrude by Vector ......................................................................................................................... 460
Extrude by Rotation ...................................................................................................................... 461
Check Mesh ........................................................................................................................................ 462
Errors ........................................................................................................................................... 462
Possible Problems ......................................................................................................................... 463
Display Mesh Quality .......................................................................................................................... 465
Quality ......................................................................................................................................... 466
Aspect Ratio ................................................................................................................................. 467
Aspect Ratio (Fluent) ..................................................................................................................... 469
Custom Quality ............................................................................................................................. 470
Determinant ................................................................................................................................ 470
Distortion ..................................................................................................................................... 471
Element Stretch ............................................................................................................................ 471
Equiangle Skewness ..................................................................................................................... 471
Ford ............................................................................................................................................. 471
Hex. Face Aspect Ratio .................................................................................................................. 471
Hex. Face Distortion ...................................................................................................................... 472
Max Angle .................................................................................................................................... 472
Min Angle ..................................................................................................................................... 472
Max Dihedral Angle ...................................................................................................................... 472
Max Length .................................................................................................................................. 472
Max Ortho .................................................................................................................................... 472
Min Ortho ..................................................................................................................................... 472
Max Orthogls ................................................................................................................................ 472
Max Ratio ..................................................................................................................................... 472
Max Sector Volume ....................................................................................................................... 472
Min Sector Volume ........................................................................................................................ 473
Max Side ....................................................................................................................................... 473
Min Side ....................................................................................................................................... 473
Min Side (Quad Optimized) ........................................................................................................... 473
xii
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Help Manual
Max Warp ..................................................................................................................................... 473
Max Warpgls ................................................................................................................................. 473
Mesh Distribution ......................................................................................................................... 473
Mesh Expansion Factor ................................................................................................................. 475
Mid Node ..................................................................................................................................... 475
Mid Node Angle ........................................................................................................................... 475
Opp Face Area Ratio ...................................................................................................................... 475
Opp Face Parallelism ..................................................................................................................... 476
Orientation ................................................................................................................................... 476
Orthogonal Quality ....................................................................................................................... 476
Prism Thickness ............................................................................................................................ 478
Quadratic Dev .............................................................................................................................. 478
Skew ............................................................................................................................................ 478
TGrid Skew ................................................................................................................................... 479
Surface Area ................................................................................................................................. 480
Surface Dev .................................................................................................................................. 480
Taper ............................................................................................................................................ 480
Tetra Special ................................................................................................................................. 480
Volume ......................................................................................................................................... 481
Volume Change ............................................................................................................................ 481
Volume/Area/Length .................................................................................................................... 481
Workbench Shape ........................................................................................................................ 481
X Size ........................................................................................................................................... 481
Y Size ........................................................................................................................................... 482
Z Size ........................................................................................................................................... 482
Quality Metric Histogram ............................................................................................................. 482
Smooth Mesh Globally ........................................................................................................................ 483
Smooth Multiblock Domains Globally ................................................................................................. 488
Smooth Hexahedral Mesh Orthogonal ................................................................................................ 494
Repair Mesh ....................................................................................................................................... 502
Build Mesh Topology .................................................................................................................... 502
Remesh Elements ......................................................................................................................... 503
Remesh Bad Elements ................................................................................................................... 505
Find/Close Holes in Mesh .............................................................................................................. 506
Mesh From Edges ......................................................................................................................... 506
Stitch Edges .................................................................................................................................. 507
Smooth Surface Mesh ................................................................................................................... 507
Flood Fill / Make Consistent ........................................................................................................... 507
Associate Mesh With Geometry ..................................................................................................... 510
Enforce Node, Remesh .................................................................................................................. 510
Make/Remove Periodic ................................................................................................................. 511
Mark Enclosed Elements ............................................................................................................... 511
Merge Nodes ...................................................................................................................................... 513
Merge Interactive ......................................................................................................................... 514
Merge Tolerance ........................................................................................................................... 516
Merge Meshes .............................................................................................................................. 516
Split Mesh .......................................................................................................................................... 519
Split Nodes ................................................................................................................................... 520
Split Edges .................................................................................................................................... 521
Swap Edges .................................................................................................................................. 523
Split Tri Elements .......................................................................................................................... 525
Split Internal Wall .......................................................................................................................... 525
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
xiii
Help Manual
Y-Split Hexas at Vertex .................................................................................................................. 525
Split Prisms ................................................................................................................................... 526
Move Nodes ....................................................................................................................................... 527
Interactive .................................................................................................................................... 527
Exact ............................................................................................................................................ 528
Offset Mesh .................................................................................................................................. 528
Align Nodes .................................................................................................................................. 529
Redistribute Prism Edge ................................................................................................................ 529
Project Node to Surface ................................................................................................................ 532
Project Node to Curve ................................................................................................................... 533
Project Node to Point .................................................................................................................... 533
Un-Project Nodes .......................................................................................................................... 534
Lock/Unlock Elements .................................................................................................................. 534
Snap Project Nodes ....................................................................................................................... 534
Update Projection ......................................................................................................................... 535
Project Nodes to Plane .................................................................................................................. 535
Transform Mesh .................................................................................................................................. 535
Translate ....................................................................................................................................... 536
Rotate .......................................................................................................................................... 537
Mirror ........................................................................................................................................... 538
Scale ............................................................................................................................................ 539
Translate and Rotate ..................................................................................................................... 539
Convert Mesh Type ............................................................................................................................. 540
Tri to Quad ................................................................................................................................... 541
Quad to Tri .................................................................................................................................... 541
Tetra to Hexa ................................................................................................................................ 542
All Types to Tetra ........................................................................................................................... 544
Shell to Solid ................................................................................................................................. 545
Create Mid Side Nodes .................................................................................................................. 546
Delete Mid Side Nodes .................................................................................................................. 549
Adjust Mesh Density ........................................................................................................................... 549
Refine All Mesh ............................................................................................................................. 550
Refine Selected Mesh .................................................................................................................... 552
Coarsen All Mesh .......................................................................................................................... 552
Coarsen Selected Mesh ................................................................................................................. 553
Renumber Mesh ................................................................................................................................. 554
User Defined ................................................................................................................................. 554
Optimize Bandwidth ..................................................................................................................... 555
Assign Mesh Thickness ........................................................................................................................ 555
Reorient Mesh .................................................................................................................................... 557
Reorient Volume ........................................................................................................................... 557
Reorient Consistent ...................................................................................................................... 557
Reverse Direction .......................................................................................................................... 558
Reorient Direction ........................................................................................................................ 558
Reverse Line Element Direction ..................................................................................................... 558
Change Element IJK ...................................................................................................................... 558
Delete Nodes ...................................................................................................................................... 558
Delete Elements ................................................................................................................................. 559
Edit Distributed Attribute .................................................................................................................... 559
Properties ............................................................................................................................................... 561
Load Material From File ....................................................................................................................... 562
Load Material From Library ................................................................................................................. 562
xiv
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Help Manual
Write Material File ............................................................................................................................... 563
Create Material Property ..................................................................................................................... 563
Isotropic ....................................................................................................................................... 564
Shell Element Anisotropic ............................................................................................................. 565
Solid Element Anisotropic ............................................................................................................. 565
Shell Element Orthotropic ............................................................................................................. 565
Isotropic Thermal Material ............................................................................................................. 566
Anisotropic Thermal Material ........................................................................................................ 566
Create Material Property Table ............................................................................................................ 566
Define Point Element Properties .......................................................................................................... 568
Define 1D Element Properties ............................................................................................................. 570
Bar Element Properties ................................................................................................................. 570
Rigid Elements Properties ............................................................................................................. 571
Rod Connection Properties ........................................................................................................... 572
Mass Connection Properties .......................................................................................................... 572
Damper Connection Properties ..................................................................................................... 572
Spring Properties .......................................................................................................................... 573
Viscous Damper Element Properties .............................................................................................. 573
Beam Element Properties .............................................................................................................. 573
Gap Element Properties ................................................................................................................ 574
Beam With Cross Section ............................................................................................................... 575
Define 2D Element Properties ............................................................................................................. 575
Shell Elements .............................................................................................................................. 576
Shear Elements ............................................................................................................................. 577
Layered Composite Elements ........................................................................................................ 577
Define 3D Element Properties ............................................................................................................. 578
Constraints .............................................................................................................................................. 579
Create Constraint / Displacement ........................................................................................................ 579
Create Constraint / Displacement on Point .................................................................................... 581
Create Constraint / Displacement on Curve ................................................................................... 581
Create Constraint / Displacement on Surface ................................................................................. 582
Create Constraint / Displacement on Subset .................................................................................. 583
Create Constraint / Displacement on Part ...................................................................................... 583
Create Constraint Equation ................................................................................................................. 583
Define Constrained Node Sets ............................................................................................................. 583
Define Contact ................................................................................................................................... 584
Automatic Detection .................................................................................................................... 584
Manual Definition ......................................................................................................................... 586
Define Single Surface Contact ............................................................................................................. 586
Define Initial Velocity .......................................................................................................................... 587
Define Planar Rigid Wall ...................................................................................................................... 587
Loads ....................................................................................................................................................... 589
Create Force ....................................................................................................................................... 589
Create Force on Point .................................................................................................................... 591
Create Force on Curve ................................................................................................................... 591
Create Force on Surface ................................................................................................................ 592
Create Force on Subset ................................................................................................................. 592
Create Force on Part ...................................................................................................................... 592
Place Pressure ..................................................................................................................................... 592
Place Pressure on Surface .............................................................................................................. 593
Place Pressure on Subset ............................................................................................................... 594
Place Pressure on Part ................................................................................................................... 594
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
xv
Help Manual
Create Temperature Boundary Condition ............................................................................................. 594
Temperature on Point ................................................................................................................... 595
Temperature on Curve .................................................................................................................. 595
Temperature on Surface ................................................................................................................ 596
Temperature on Body ................................................................................................................... 596
Temperature on Subset ................................................................................................................. 597
Temperature on Part ..................................................................................................................... 597
Solve Options .......................................................................................................................................... 599
Setup Solver Parameters ..................................................................................................................... 601
NASTRAN Setup Solver Parameters ............................................................................................... 602
ANSYS Setup Solver Parameters .................................................................................................... 607
LS-DYNA Setup Solver Parameters ................................................................................................. 608
Setup Analysis Type ............................................................................................................................ 609
NASTRAN Setup Analysis Type ....................................................................................................... 610
Linear Static Analysis (Sol 101) ................................................................................................. 611
Modal (Sol 103) ....................................................................................................................... 612
Buckling Analysis (Sol 105) ...................................................................................................... 612
Nonlinear Static (Sol 106) ........................................................................................................ 612
Direct Frequency Response (Sol 109) ....................................................................................... 612
Direct Transient Response (Sol 109) ......................................................................................... 613
Modal Frequency Response (Sol 111) ...................................................................................... 613
ANSYS Setup Analysis Type ........................................................................................................... 614
Structural Analysis .................................................................................................................. 614
Thermal .................................................................................................................................. 615
LS-DYNA Setup Analysis Type ........................................................................................................ 616
Abaqus Setup Analysis Type .......................................................................................................... 617
Autodyn Setup Analysis Type ........................................................................................................ 618
Setup a Subcase ................................................................................................................................. 618
NASTRAN Setup a Subcase ............................................................................................................ 619
ANSYS Setup a Subcase ................................................................................................................ 620
Abaqus Setup a Subcase ............................................................................................................... 621
Write/View Input File .......................................................................................................................... 622
NASTRAN Write/View Input File ..................................................................................................... 622
ANSYS Write/View Input File .......................................................................................................... 623
LS-DYNA Write/View Input File ...................................................................................................... 625
Abaqus Write/View Input File ........................................................................................................ 626
Autodyn Write/View Input File ...................................................................................................... 627
Submit Solver Run .............................................................................................................................. 628
NASTRAN Submit Solver Run ......................................................................................................... 628
ANSYS Submit Solver Run ............................................................................................................. 629
LS-DYNA Submit Solver Run .......................................................................................................... 630
Output ..................................................................................................................................................... 631
Select Solver ....................................................................................................................................... 631
ANSYS .......................................................................................................................................... 633
ANSYS CFX ................................................................................................................................... 646
ANSYS Fluent ................................................................................................................................ 647
CGNS ............................................................................................................................................ 649
Polyflow ....................................................................................................................................... 651
Boundary Conditions .......................................................................................................................... 653
Edit Parameters .................................................................................................................................. 655
Write Input ......................................................................................................................................... 655
ANSYS Input Files .......................................................................................................................... 655
xvi
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Main Menu Area
The Main Menu area contains drop down menus for managing projects, files, and settings. It also includes
Utility icons for common tasks and display options.
Figure 1: Main Menu Area
File Menu
Figure 2: File menu
The File menu commands for managing your project, for managing the entities that comprise a project,
for importing and exporting data, for managing Replay Scripts, and to quit the program.
Project Management Options
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
1
Main Menu Area
Entity Management Options
Import/Export Options
Replay Scripts
Exit
Project Management Options
Your ANSYS ICEM CFD work is organized into Project files (*.prj). A project file contains the information
necessary to manage several data files associated with your project. The data files in a project are a
Geometry file (*.tin), Mesh file (*.uns), Blocking file (*.blk), Attributes files (*.fbc and *.atr),
and Parameters file (*.par).
Options for managing your project file include the following:
New Project
To initiate a project file, select the New Project option.
Figure 3: New Project Window
• Browse to the desired folder. This location becomes the working folder for all files associated with
your project.
• You must specify a File name.
• The only available Save as type option is .prj for project files.
2
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
• Click Save.
Note
• Existing project files in the current folder will be displayed.
• You may choose a File name from the existing files displayed or from a list of the most
recently opened project files using the drop down list, although a new project name is
advised to prevent overwriting an existing project.
• If you already have a project open, this option will close the current project.
Open Project
To work on an existing project, select the Open Project option.
Navigate to the working folder and select the desired project from the Open Project window; or
select an existing project from the drop down list in the File name field.
Note
ANSYS ICEM CFD supports native projects (.prj extension) or ANSYS Workbench projects
(.wbpj extension).
Save Project
To update the project file (*.prj) on your disk, select the Save Project option.
If you are working in an existing project, this option will overwrite that project. If not, you will be
prompted for a File name and location.
This option also updates and saves the data files associated with the project. The files saved are
the Geometry file (*.tin), Mesh file (*.uns), Blocking file (*.blk), Parameters file (*.par) and
Attributes files (*.fbc and *.atr).
Save Project As
To create a new project file with existing work, select the Save Project As option.
The Save Project As dialog box opens, prompting you for a File name and location for your project.
Close Project
To unload all project data and leave your ICEM CFD session open, select the Close Project option.
If the project has changed, you will be prompted to save your changes.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
3
Main Menu Area
Figure 4: Save Confirmation Window
Change Working Directory
To specify a default directory where the project and data files will be saved, select the Change Working
Directory option.
You can directly enter the path name or browse to the desired working directory for the project.
Figure 5: Change Working Directory Window
Entity Management Options
Your ANSYS ICEM CFD project consists of several entities, each with its own data which may be managed
independently. Each option in this section opens a submenu to manage that entity’s data.
Geometry
Mesh
Blocking
Attributes
Parameters
Cartesian
4
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Geometry
The geometry file (*.tin) includes details of the shapes, names, material properties, and so on of all
component parts in the project. Options for managing the geometry file are shown in Figure 6: Geometry
Options (p. 5).
Figure 6: Geometry Options
Open Geometry
To load a geometry file into memory and display its graphical image, select the Geometry > Open
Geometry option.
Select the required geometry file (*.tin) in the Open window. You may have to browse to a different working directory.
If a geometry is already loaded, the Geometry Exists window will open, prompting you to either
merge the new geometry with the existing geometry or replace the existing geometry.
Figure 7: Geometry Exists Window
Save Geometry
To update the .tin file with all your recent geometry work, select the Geometry > Save Geometry
option.
This option will overwrite an existing, open geometry file. If no geometry file is open, a Save all
geometry window will prompt you for a File name and location.
Save Geometry As
To create a new .tin file with existing geometry data, select the Geometry > Save Geometry As option.
The Save all geometry window opens where you are prompted for a File name and location.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
5
Main Menu Area
Save Visible Geometry As
To create a new .tin file containing only those geometry entities currently displayed, select the Geometry > Save Visible Geometry As option. This is typically done when you need to work with a subset
of all geometry in your project.
The Save only visible geometry window opens where you are prompted for a File name and location.
Save Only Some Geometry Parts As
To create a new .tin file containing a subset of all geometry in your project, select the Geometry >
Save Only Some Geometry Parts As option.
The Save only some parts window opens where you are prompted for a File name and location,
followed by the Select parts dialog box for you to choose which parts are saved in the new file.
Save Geometry As Version ...
To save the geometry in an earlier ANSYS ICEM CFD format, select the Geometry > Save Geometry As
Version option. Options available are Version 4.3, Version 10.0, or Version 13.0.
Note
• Options related to Mesh Type and Mesh Method introduced in ANSYS ICEM CFD 11.0 will
be ignored when saving a geometry file in the ANSYS ICEM CFD 10.0 or earlier format.
• The parameter related to curves and surfaces introduced in ANSYS ICEM CFD 14.0 will be
ignored when saving the geometry file in the ANSYS ICEM CFD 13.0 or earlier format.
Note
This parameter is introduced because of changes to AutoVT in ANSYS
Workbench and can be introduced when the model comes through ANSYS
Workbench, including with the Workbench CAD interfaces.
Close Geometry
To remove the geometry information from the graphical display and close the loaded geometry file,
select the Geometry > Close Geometry option.
If the geometry has been modified, the Save Geometry window will open, asking if you want to
save the modified geometry.
Figure 8: Save Geometry Window
6
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Mesh
The mesh file (*.uns) includes details of the line, shell, and volume mesh elements of the project.
Options for managing the mesh file are shown in Figure 9: Mesh Options (p. 7).
Figure 9: Mesh Options
Open Mesh
To load a mesh file into your project and display its image, select the Mesh > Open Mesh option.
Select the required mesh file (*.uns) in the Open dialog box. You may have to browse to a different
working directory.
If a mesh file is already loaded in the project, the Mesh Exists window will open, prompting you
to either merge the new mesh with the existing mesh or replace the existing mesh (similar to Figure 7: Geometry Exists Window (p. 5)).
Open Mesh Shells Only
To load only a shell (surface) mesh, select the Mesh > Open Mesh Shells Only option.
Select the required mesh file in the Open window. If a mesh file is already loaded in the project,
the Mesh Exists window will open, prompting you to either merge with, or replace, the existing
mesh.
Load from Blocking
To load the mesh from the currently loaded blocking file, select the Mesh > Load from Blocking option.
The existing mesh will be converted from structured to unstructured mesh; and the meshing entities
in the display tree will be updated.
Save Mesh
To update your .uns file with all your recent mesh work, select the Mesh > Save Mesh option.
This option will overwrite an existing, open mesh file. If no mesh file is open, a Save all mesh window
will prompt you for a File name and location.
Save Mesh As
To create a new .uns file with existing mesh data, select the Mesh > Save Mesh As option,
The Save all mesh window opens where you will be prompted for a File name and location.
Save Visible Mesh As
To create a new .uns file containing only those mesh entities currently displayed, select the Mesh >
Save Visible Mesh As option. This is typically done when you need to work with a subset of all mesh
in your project.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
7
Main Menu Area
The Save only visible mesh window opens where you will be prompted for a File name and location.
Save Only Some Mesh As
To create a new .uns file containing a subset of your mesh data, select the Mesh > Save Only Some
Mesh As option.
The Save Some Mesh As dialog box opens where you select the mesh types and/or mesh parts to
be saved in the new file. See Figure 10: Save Some Mesh As Dialog (p. 8).
Figure 10: Save Some Mesh As Dialog
Mesh file
The currently loaded Mesh file name will appear here. You may use the existing file name, type a
new Mesh file name, or browse for a file by clicking on the box to the right of the field.
Types
Select All to include all mesh types, or Select to choose the mesh elements to be saved. The selected
types will be highlighted.
Parts
Select All to include the mesh associated with all the existing parts, or Select to choose the mesh
parts to be saved. The selected parts will be highlighted.
Close Mesh
To remove the mesh information from the graphical display and close the loaded domain file or mesh
file, select the Mesh > Close Mesh option.
If the mesh has been modified, the Save Mesh window will open, asking if you want to save the
modified mesh (similar to Figure 8: Save Geometry Window (p. 6)).
8
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Blocking
The blocking file (*.blk) includes details of the underlying framework used to create a structured
hexahedral mesh in your project. Blocking files may also be loaded from or saved to unstructured mesh.
The options for managing the blocking file are shown in Figure 11: Blocking Options (p. 9).
Figure 11: Blocking Options
Open Blocking
To load a blocking file into your project and display its image, use the Blocking > Open Blocking option.
Select the desired blocking file from the Open dialog box. You may have to browse to different
working directory.
If a blocking file is already loaded in the project, the Blocking Exists window will open, prompting
you to either merge the new blocking with the existing blocking or replace the existing blocking
(similar to Figure 7: Geometry Exists Window (p. 5)).
Load from Unstruct mesh
To create a hexa blocking file from an unstructured mesh composed entirely of hexa elements, select
the Blocking > Load from Unstruct mesh option. This option is useful to regenerate a blocking file
from a hexa mesh that was originally created from a blocking file, and is most robust when used in this
fashion. This option can also be used on unstructured meshes originally written from external Multiblock
formats such as Plot3D.
It is also useful to create complicated 2D blocking by first creating 2D elements. Each quad element
becomes a 2D hexa block. Complicated block structures can be made this way, which may not be
possible to do in a top-down method.
Save Blocking
To update your .blk file with all your recent blocking work, select the Blocking > Save Blocking option.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
9
Main Menu Area
If an existing blocking file, filename.blk is already open, then this option will rename the existing
blocking file to filename.blk0 (and then sequentially filename.blk1, filename.blk2,
etc.) and save the current file to filename.blk.
Note
The automatic indexing of blocking file names makes it easy to jump back to an
earlier step if you wish.
Note
A key strength of ANSYS ICEM CFD Hexa is the separate blocking layer file. This blocking
file sit on top of the geometry (*.tin file) and is associated with it, but can be loaded
with other topologically similar models and associated with them. In this way a blocking
structure can be used with a family of geometries to rapidly create a series of high
quality meshes or shared between colleagues working on similar tasks.
Save Blocking As
To create a new .blk file with existing blocking data, select the Blocking > Save Blocking As option.
The Save as window opens where you will be prompted for a File name and location.
Save Blocking as 4.0 Format
To save the blocking file in the legacy ANSYS ICEM CFD 4.0 format, select the Blocking > Save Blocking
– 4.0 format option.
Save Unstruct Mesh
To save the existing blocking pre-mesh in an unstructured hexa mesh format (*.uns file), select the
Blocking > Save Unstruct Mesh option.
The Save Mesh as dialog box opens where you will be prompted for a File name and location. The
unstructured mesh is not loaded.
Save Multiblock Mesh
To save the current blocking data in the Multiblock structured format, select the Blocking > Save
Multiblock Mesh option.
A dialog box will open prompting you to choose which type of domains to convert.
Figure 12: Convert Multiblock
10
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Write Super Domain
To save the current blocking data in a merged, one-domain Multiblock mesh, select the Blocking >
Write Super Domain option. The intended solver must be compatible with the Super Domain format.
Write Cartesian Grid
To save the current blocking data in a Cartesian grid format, select the Blocking > Write Cartesian Grid
option. This is useful as a starting point for the Body-Fitted Cartesian (BFCart) meshing module (see the
Cartesian file information on the Body-Fitted Mesh Method page).
To use this option, start by creating a block from the geometry extents. You can modify the vertex
locations, but ensure the block remains aligned with a Cartesian coordinate system (right angled
corners). Control the Cartesian grid distribution and biasing with splits and edge parameters. Also,
edge distributions should be “copied to parallel” to maintain a consistent Cartesian distribution
throughout the grid.
Close Blocking
To remove the blocking information from the graphical display and close the loaded blocking file, select
the Blocking > Close Blocking option.
If the blocking has been modified, the Save Blocking window will open, asking if you want to save
the modified blocking (similar to Figure 8: Save Geometry Window (p. 6)).
Attributes
The attributes files (extension *.fbc or *.atr) maintain the association of user-specified data for
parts, element properties, loads and constraints with nodes/elements of the mesh for a project. The
files are updated automatically to preserve consistency with the mesh, every time the project is saved.
You can perform the following operations on an existing attributes file as shown in Figure 13: Attributes
Options (p. 11).
Figure 13: Attributes Options
Open Attributes
To load an attributes file (*.atr or *.fbc), select the Attributes > Open Attributes option.
Select the desired attributes file from the Open dialog box, or select an existing file from the drop
down list in the File name field. You may have to browse to the working folder.
Save Attributes
To update your .fbc and .atr files with all your recent boundary conditions and attributes work, select
the Attributes > Save Attributes option.
This option will overwrite existing, open attributes files. If no attribute file is open, a Save as window
will prompt you for a File name and location.
Save Attributes As
To create new .fbc and .atr files with existing attributes data, select the Attributes > Save Attributes
As option.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
11
Main Menu Area
The Save as window opens where you will be prompted for a File name and location.
Close Attributes
To close the attributes files, select the Attributes > Close Attributes option.
Parameters
The parameters file (extension *.par) contains mesh-independent data such as material properties,
local coordinate systems, solver analysis set up and run parameters. The data in the parameters file is
cross-referred in the attributes file when a set of parameters is associated to the nodes/elements of the
mesh. The parameters file is also updated automatically along with the attributes files whenever a
project is saved.
You can perform the following operations on an existing parameters file as shown in Figure 14: Parameters
Options (p. 12).
Figure 14: Parameters Options
Open Parameters
To load a parameters file (*.par), select the Parameters > Open Parameters option.
Select the desired file from the Open dialog box; or select an existing file from the drop down list
in the File name field. You may have to browse to the working folder.
Save Parameters
To update your .par file with all your recent parameters work, select the Parameters > Save Parameters
option.
This option will overwrite an existing, open parameters file. If no parameter file is open, a Save as
window will prompt you for a File name and location.
Save Parameters As
To create new .par file with existing parameters data, select the Parameters > Save Parameters As
option.
The Save as window opens where you will be prompted for a File name and location.
Close Parameters
To close the parameters file, select the Parameters > Close Parameters option.
Note
The data format for both the attributes and parameters files is unique for a solver. The default
format is Nastran. The conversion of Nastran files to ANSYS & LS-DYNA files is done automatically depending on the selected solver. The other solver-specific attributes and parameters
can be specified through the Edit Parameters and/or Edit Attributes options available under
Advanced Edit Options in the Write/View Input File DEZ. After selecting this option, the
Solver Parameters window will open and you can set the required parameters.
12
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Cartesian
The Cartesian file (extension *.crt) contains information regarding the Cartesian grid for your project,
if one has been created. See Write Cartesian Grid under Blocking (p. 9).
You can perform the following operations on an existing Cartesian file as shown in Figure 15: Cartesian
Options (p. 13).
Figure 15: Cartesian Options
Load Cartesian
To load a Cartesian grid file (*.crt), select the Cartesian > Load Cartesian option.
Select the desired file from the Open dialog box, or select an existing file from the drop down list
in the File name field. You may have to browse to the working folder.
Save Cartesian
To update your .crt file with all your recent Cartesian grid work, select the Cartesian > Save Cartesian
option.
This option will overwrite an existing, open Cartesian file. If no Cartesian file is open, a Save as
window will prompt you for a File name and location.
Save Cartesian As
To create a new .crt file with existing Cartesian grid data, select the Cartesian > Save Cartesian As
option.
The Save as window opens where you will be prompted for a File name and location.
Close Cartesian
To close the Cartesian file, select the Cartesian > Close Cartesian option.
Import/Export Options
ANSYS ICEM CFD is capable of importing or exporting Geometry and parts data from/to many popular
CAD software programs, as well as importing or exporting Mesh data from/to many third party Solvers.
The Import Model option uses available Workbench Readers to extend the options for interfacing
with third party software.
Import Model
Import Geometry
Import Mesh
Export Geometry
Export Mesh
Note
The special characters Ä, ä, Ç, Ö, ö, Ü, and ü are not supported in file names on Linux.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
13
Main Menu Area
Import Model
The Import Model option allows you to use the Workbench Readers to import many kinds of files into
ANSYS ICEM CFD.
The following table lists the ANSYS product file types that may be imported using this option.
ANSYS licensed product file types that may be imported using Workbench Readers.
ANSYS
*.agdb, *.anf, *.cmdb, *.dsdb, *.mechdat, *.meshdat,
*.meshdb, *.mshdat, *.mshdb, *.wbpj
BladeGen
*.bgd
DesignModeler
*.agdb
GAMBIT
*.dbs
SpaceClaim
*.scdoc
Table 1: Geometry Interface Support using Workbench Readers (p. 14) lists the third party CAD software
formats supported by the Import Model option (√ = supported).
Table 1: Geometry Interface Support using Workbench Readers
Windows 32 (Intel IA32)
Windows x64 (EM64T,
AMD64)
Linux x64 (Intel
Xeon EM64T,
AMD64)
CAD
Product
(file
types)
Version of
CAD Package
MS MS WinWin- dows 7
dows
XP
MS
MS WinWin- dows 7
dows
XP
MS Windows 8
(Pro &
Enterprise)
Red Red
Hat Hat 5
6
SuSE
ES
11
Reader
for ACIS
(*.sat,
*.sab)
24
√
√
√
√
√
√
√
Reader
for AutoCAD
(*.dwg,
*.dxf )
2013
√
√
√
√
√
√
√
√
2014
Reader
for
CATIA V4
(*.model,
*.dlv)
4.2.4
√
√
√
√
√
Reader
for
CATIA V5
(*.CATPart,
*.CATProduct)
V5-6R2013
√
√
√
√
√
14
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
√
File Menu
Windows 32 (Intel IA32)
Windows x64 (EM64T,
AMD64)
Linux x64 (Intel
Xeon EM64T,
AMD64)
Red Red
Hat Hat 5
6
CAD
Product
(file
types)
Version of
CAD Package
MS MS WinWin- dows 7
dows
XP
MS
MS WinWin- dows 7
dows
XP
Reader
for
CATIA V5
- CADNexus
CAPRI
CAE
Gateway
V3.16.1
(*.CATPart,
*.CATProduct)
V5R21,
V5–6R2012,
V5–6R2013
√
√
√
√
Reader
for
CATIA V6
(*.CATPart,
*.CATProduct)
R2013
√
√
√
√
Creo Ele- 17.0
ments/Dir- 18.0
ect Mod18.1
eling
(*.pkg,
*.bdl,
*.ses,
*.sda,
*.sdp,
*.sdac,
*.sdpc)
√
√
√
√
√
√
√
√
√
√
√
√
Reader/Plugin for
Creo Elements/Pro
(Pro/ENGINEER)
(*.prt,
*.asm,
*.prt*,
*.asm*)
Wildfire 5
√
√ (requires
Pro/E Wildfire 5
M020)
√
√ (requires
Pro/E Wildfire 5
M020)
Creo Parametric 1.0
√
√
√
√
Creo Parametric 2.0
√
√
√
√
MS Windows 8
(Pro &
Enterprise)
SuSE
ES
11
√
√ (requires
Creo Elements/Direct Modeling M030
or later)
√ (requires
Creo Para-
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
15
Main Menu Area
CAD
Product
(file
types)
Version of
CAD Package
Windows 32 (Intel IA32)
Windows x64 (EM64T,
AMD64)
Linux x64 (Intel
Xeon EM64T,
AMD64)
MS MS WinWin- dows 7
dows
XP
MS
MS WinWin- dows 7
dows
XP
Red Red
Hat Hat 5
6
SuSE
ES
11
√
√
MS Windows 8
(Pro &
Enterprise)
metric 2.0
M030)
Reader
Creo Parafor Creo
metric 2.0
Elements/Pro
(Pro/ENGINEER)
(*.prt,
*.asm,
*.prt*,
*.asm*)
√
√
√
√
√
Reader/Plugin
for
Autodesk
Inventor
(*.iam,
*.ipt)
√
√
√
√
√ (requires
Autodesk
Inventor
2013 SP2)
√
√
2013
√
2014
Reader
for
Autodesk
Inventor
(*.iam,
*.ipt)
2013
√
√
√
√
√
Reader
for JT
(*.jt)
9.5
√
√
√
√
√
√
√
√
√
√
Reader
26.0
for Parasolid
(*.x_t,
*x_b,
*.x_txt,
*.xmt_b,
*.xmt_bin)
Reader
for Solid
Edge
(*.asm,
*.par,
16
ST5
√
√
ST6
√
√
√
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
√
File Menu
Windows 32 (Intel IA32)
Windows x64 (EM64T,
AMD64)
Linux x64 (Intel
Xeon EM64T,
AMD64)
Version of
CAD Package
MS MS WinWin- dows 7
dows
XP
MS
MS WinWin- dows 7
dows
XP
MS Windows 8
(Pro &
Enterprise)
Red Red
Hat Hat 5
6
SuSE
ES
11
Reader
for SolidWorks
(*.sldasm,
*.sldprt)
2013
√
√
√
√
√
Reader/Plugin
for SolidWorks
(*.sldasm,
*.sldprt)
2012
√
√
√
√
CAD
Product
(file
types)
*.psm,
*.pwd)
Reader
for STEP
(*.stp,
*.step)
√
2013
AP203,
AP214
Reader
for STL
(*.stl)
Reader
for NX
(*.prt)
8.5
Reader/Plugin
for NX
(*.prt)
8.5
Plugin
for TeamCenter
Engineering
√
√
√
√
√
√
√
√
√
√
√
√
√
√
√
√
√
√
√
√
√
√
√
√
√
√
8.0
√
√
√
√
7.5
√
√
√
√
Unified Architecture
8.1.0.4 (2tier only)
with NX7.5
√
√
Unified Architecture
8.3 (2- and
4-tier) with
NX7.5.4
MP2 or
higher,
NX8.0
(8.3.3.4 or
√
√
√
√
√
√
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
√
17
Main Menu Area
CAD
Product
(file
types)
Version of
CAD Package
Windows 32 (Intel IA32)
Windows x64 (EM64T,
AMD64)
Linux x64 (Intel
Xeon EM64T,
AMD64)
MS MS WinWin- dows 7
dows
XP
MS
MS WinWin- dows 7
dows
XP
MS Windows 8
(Pro &
Enterprise)
Red Red
Hat Hat 5
6
√
√
√ (requires
patch
9.1.2.3)
higher) &
NX8.5
(8.3.3.5 or
higher)
Unified Architecture
9.1 (2- & 4tier) with
NX7.5,
NX8.0 &
NX8.5
Note
This option only appears if ANSYS Workbench is installed along side ANSYS ICEM CFD.
18
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
SuSE
ES
11
File Menu
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
19
Main Menu Area
Model Files from Workbench project
When the Workbench project (*.wbpj) file is read using the Import Model option, the existing geometry
and/or mesh files will be located. You can then select the specific data file to be imported.
Selecting at the project level is more convenient than locating the particular Workbench geometry
or mesh files within the directory structure. However, the Model Files from Workbench project
option is particularly important if there are multiple files located.
Parts, Sizes
allows you to replace the default Workbench parameters with the parameters defined in an existing
tetin file to the imported geometry. The selected tetin file would transfer its global, part, and entity
based settings to the newly imported geometry. This results in rapid meshing parameter setup for a
modified geometry.
Import Geometry
allows you to import geometry. In general, the geometry import options available follow the options
available in ANSYS Workbench Meshing. All the options under Geometry Preferences will be active
only when Import Geometry is enabled.
Use Associativity
Default is OFF. If checked ON, ICEM CFD will use a default part manager database to store persistency
data.
Note
• Valid extensions are .prt .asm .prt* .asm* .par .psm .pwd .CATPart .CATProduct .sldasm
.sldprt .ipt and .iam. Otherwise you will get an error message about an invalid file format.
• It is required that your ICEM CFD project exist to store the associated geometry file.
Import Mesh
allows you to import meshes from *.meshdat. or *.mechdat files. Legacy formats such as *.cmdb and
*.dsdb are also supported. When only Import Mesh is enabled, all the Geometry Preferences options
will be deactivated.
Geometry Preferences
allows you to set the following geometry preferences:
Create Subset(s) from Named Selection
enables the creation of geometry subsets instead of parts, thereby allowing you to decide which
part the geometry entity (point/curve/surface) should be associated to. When this option is disabled
each geometry entity (point/curve/surface) will be assigned to only one part, thereby losing association
with other Named Selections (which are mapped to parts). This option is available only when the
Import Mesh option is disabled.
Create Entity and Part Names
uses attribute/entity names assigned in the CAD file to create entity and part names in ICEM
CFD.
Create Material Points
enables the automatic creation of material points during import.
20
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Import Solid Bodies
enables the import of solid bodies.
Import Surface Bodies
enables the import of surface bodies.
Import Line Bodies
enables the import of line bodies.
Import Work Points
enables the import of work points.
CAD Attribute Transfer
allows import of CAD system attributes into ANSYS ICEM CFD.
CAD Attribute Prefixes
allows you to set the CAD attribute prefix when CAD Attribute Transfer is enabled. By default
the filter is set to SDFEA;DDM. If the filter is set to an empty string, all applicable entities will
be imported as CAD system attributes. You may enter multiple prefixes with each prefix delimited
by a semicolon.
Named Selection Processing
creates a named selection based on data generated in the CAD system.
Named Selection Prefixes
allows you to set the named selection processing prefix key when Named Selection Processing
is enabled. If the filter is set to an empty string, all applicable entities will be imported as named
selections. You may enter multiple prefixes with each prefix delimited by a semicolon.
Enclosure and Symmetry Processing
enables the processing of enclosure and symmetry named selections. This option is enabled by default.
Mixed Import Resolution
allows parts of mixed dimension to be imported as components of assemblies which have parts of different dimension. By default, no bodies from a multibody part will be transferred to ANSYS ICEM CFD.
You can select the appropriate combination of bodies to be transferred to ANSYS ICEM CFD using the
following options:
Solid
solid(s) from the selected geometry's multibody part(s) are imported into ANSYS ICEM CFD.
Surface
surface(s) from the selected geometry's multibody part(s) are imported into ANSYS ICEM CFD.
Line
line(s) from the selected geometry's multibody part(s) are imported into ANSYS ICEM CFD.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
21
Main Menu Area
Point
point(s) from the selected geometry's multibody part(s) are imported into ANSYS ICEM CFD.
Note
The Mixed Import Resolution options are valid only for “real” CAD files (Parasolid,
UniGraphics, CATIA, etc.). For ANSYS Workbench (*.agdb) files, only the primary options
(Import Solid Bodies, Import Surface Bodies, Import Line Bodies) are valid.
Convert Units
allows you to scale the imported geometry/mesh based on the units specified.
Default
retains the original units from the imported file.
Inch
scales the imported geometry/mesh to inches (in).
Feet
scales the imported geometry/mesh to feet (ft).
Meter
scales the imported geometry/mesh to meters (m).
Centimeter
scales the imported geometry/mesh to centimeters (cm).
Millimeter
scales the imported geometry/mesh to millimeters (mm).
Import Geometry
Figure 16: Import Geometry Options
The Import Geometry option allows you to import geometry from various sources, including several
faceted geometry formats (Nastran, Patran, STL, or VRML) or CAD drawing packages (CATIA, DWG,
Parasolid, Rhino 3DM, STEP/IGES, etc.). When you select the CAD software format of the geometry file
you want to import; a corresponding window will pop up with further options.
Options for importing geometry are shown in Figure 16: Import Geometry Options (p. 22).
For detailed CAD-related information specific to ANSYS Workbench, see the CAD Integration section of
the product help. Within the Help Viewer, expand the CAD Integration section in the hierarchical tree.
Faceted
Legacy
Formatted Point Data
Reference Geometry
22
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Faceted
The Faceted submenu gives several options for importing faceted geometry.
Figure 17: Import Faceted Geometry
Options for importing faceted geometry are shown in Figure 17: Import Faceted Geometry (p. 23).
ICEM CFD Mesh
Nastran
Patran
STL
VRML
ICEM CFD Mesh
The ICEM CFD Mesh option allows you to import unstructured mesh file as triangulated surface data.
The volume elements in the mesh file will be ignored. Surfaces and curves are segmented by part.
Note
You can convert loaded mesh to facets using the Mesh>Facets option (Edit > Mesh>Facets).
Nastran
The Nastran option allows you to import a Nastran surface mesh file (*.dat, *.bdf ) as triangulated surface
data.
Patran
The Patran option allows you to import Patran files (*.pat).
Transfer family information
Multiple
converts each Patran group (PID) into an ICEM CFD part.
Single
brings the Patran groups all in as one part.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
23
Main Menu Area
STL
The STL option allows you to import a Stereolithography Part file (*.stl) as triangulated surface data.
Note that the parts defined in the STL file will also be imported. Select the format for the part names
and click Done to finish the operation.
Part names
Generate
generates part names of the format Filename.PartName, where PartName is the part name
defined in the STL file.
From file
retains the part names as defined in the STL file.
Note
This option is valid only for STL files in ASCII format. For STL files in binary format,
part names of the format Filename.PartName will be generated as described.
VRML
The VRML option allows you to import a VRML file as triangulated surface data (*.wrl).
Note
You can only import VRML files in ASCII format. The import of binary VRML files in not
supported in ANSYS ICEM CFD.
Legacy
The Legacy option allows you to import geometry from various CAD formats such as CATIA V4, Rhino
3D, IGES, and Parasolid, etc. Select the format of the geometry file you want to import; a corresponding
window will pop up with further options.
Note
Some higher formats are supported in the Import Model option using Workbench Readers.
If your model fails to read with the ANSYS ICEM CFD Legacy option, try the Import Model
option instead.
24
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
The supported legacy geometry interfaces are listed in Table 2: Legacy Geometry Interface Support (p. 25)
(√ = supported).
Table 2: Legacy Geometry Interface Support
Windows 32 (Intel IA32)
Windows x64 (EM64T, AMD64)
Linux x64 (Intel
Xeon EM64T,
AMD64)
CAD
Product
Version of
CAD Package
MS
MS WinWin- dows 7
dows
XP
MS
MS WinWin- dows 7
dows
XP
MS Windows 8
Red Red
Hat Hat 5
6
SuSE
ES
11
Reader
for ACIS
18.0.1
√
√
√
√
√
√
√
√
Reader
for CATIA
V4
4.2.4
√
√
√
√
√
√
√
√
Reader
for DWG
√
√
√
√
√
√
√
√
Reader
for GEMS
√
√
√
√
√
√
√
√
√
√
√
Reader
for IDI
MS 8/9
√
√
√
√
√
Reader
for Parasolid
24.0
√
√
√
√
√
Reader
for Rhino
3DM
√
√
√
√
√
Reader
for Plot3d
√
√
√
√
√
Reader
for IGES
4.0, 5.2, 5.3
√
√
√
√
√
√
√
√
Reader
for STEP
AP203,
AP214
√
√
√
√
√
√
√
√
Figure 18: Import Legacy Geometry
Options for importing geometry are shown in Figure 18: Import Legacy Geometry (p. 25).
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
25
Main Menu Area
Acis
CATIA V4
DWG
GEMS
IDI
ParaSolid
Rhino 3DM
Plot3d
STEP / IGES
Acis
The Acis option converts an Acis file (*.sat) to a Geometry file (*.tin) and loads it. Select an Acis file in
the file browser window, and click Open. The Import Sizes From Tetin File window will open where
you can select a previously setup version of the model and transfer parts and mesh parameters to the
newly imported geometry. This saves time that would have been spent setting up the new model.
Figure 19: Import Acis Geometry window
Model mesh params
are the global mesh settings.
Surface families, mesh params
will put the imported surface entities into parts (same as the original) and assign surface based mesh
parameters.
Curve families, mesh params
will put the imported curve entities into parts (same as the original) and assign curve based mesh
parameters.
Point families
will put the imported point entities into parts (same as the original). Point entities do not support mesh
parameters.
Note
These surface/curve/point entity options are based on the entity names matching between
the source file and the imported file.
26
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
CATIA V4
The CATIA V4 option converts a CATIA file (*.model) to a Geometry file (*.tin) and loads it. Select a
CATIA file in the file browser window, and click Open. This will open the Import Geometry from Catia
window.
Figure 20: Import Geometry From Catia Window
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
27
Main Menu Area
Tetin file
Select the required path to store the Geometry file (*.tin) by clicking on the file browser icon.
In/Out Filters
Catia Input
Four CATIA input filters are provided here. By default the SHOW area is converted and the entities
located in the NOSHOW area are ignored. Both PICK and NOPICK are usually enabled.
File Output
Suppresses specific entity classes, which are of no further importance for ANSYS ICEM CFD.
Often CATIA models contain a lot of points and curves, which slow down the GUI and may even
have to be deleted before meshing. Therefore, NO POINTS and NO CURVES are enabled by default
while NO SURFACES is disabled by default.
Use CATIA Layer Filter
allows you to enter specific layer numbers to import. For instance specifying “17, 18” for Filter args
would only import entities in these two layers and leave out other layers which may only contain
construction geometry or the 2D drawing.
Other Options
The Preview option results in a roughly approximated conversion of the CATIA model with a large
Triangulation Tolerance. Although approximation slows down the conversion, the resulting Tetin
file is usually smaller and can be processed faster.
Sometimes trimming 2D boundary curves of CATIA faces exceeds the boundary of the underlying
surface a little. These faces are suppressed by default. These suppressions are reported in the
message window and if you want to force those faces to be contained in the Tetin file then
you need to enable the Ignore Range Errors option.
To extract all boundary curves into the Tetin file you should enable With Boundary Curves.
Note
This option conflicts with the No Curves option so the latter should be disabled.
Note
This option may require a longer time to complete.
If Loops instead of Faces is enabled, planar faces are written as loops instead of Bspline surfaces
in the Tetin file. Loops are easily meshed using the Shell Mesher.
Create Bounding Box will create a box around the converted model. The bounding box is
automatically assigned a special part name.
Note
This option may require a longer time to complete.
If the faces of polyhedral solids in their original state are too complex to be represented by an
unstructured domain, then by default they are represented by planer Bspline surfaces. If the
28
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Mesh polyhedral solids option is enabled, the surface mesher is invoked to convert complex
shaped faces of polyhedral solids into an unstructured domain entity.
Estimate Maximum Size estimates the maximum size from the model dimension instead of
using an infinite large value.
Take Layer from Shell/Skin/Solid only imports entities from layers containing these entity
types. When enabled, it will not import entities from layers containing only curves or points.
Transform to active Axis System transforms geometry to the active local coordinate system.
Part Naming
You can select from the given four options:
Default
will directly transfer all the information of the CATIA model to the Tetin file. It will make the
whole model into one part.
Part by Layer
will write a Tetin file by the layers defined in the CATIA. Entities kept in the same layers will be
transferred into the same part.
Part by Color
will work the same way as layers. But it will translate the entities into part by color type instead
of layer.
CATIAMIF-Parts
is chosen if the CATIAMIF interface was used on the CATIA model. It will give the name of the
parts and mesh parameters set to the part defined by the CATIAMIF interface.
Entity Naming
This option is useful for giving names to the entities and parts.
Default
will write names as set in default.
CATIA-Names
will translate entities into Tetin files with the same names as defined in the CATIA files.
CATIAMIF-Names
is applicable if the CATIAMIF interface was used on the CATIA model. It will give the name of
the parts as defined in the CATIAMIF interface.
Triangulation tolerance
sets up the global triangulation tolerance in ANSYS ICEM CFD (Settings > Model). This affects how
the nurbs are rendered. It also affects mesh projection. Finer tri tolerance means slower rendering
but more accurate projection. (Refer to Figure 76: Examples of Triangulation Tolerance (p. 87) for
more information.)
DWG
The DWG option converts a DWG (AutoCAD Drawing) file to a Tetin file and loads it (Only 2D geometries).
Selecting the DWG option pulls up a file browser. Select the DWG file (*.dwg, *.dxf ) to be imported and
click Open to start translator.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
29
Main Menu Area
Another window will appear, where you have to specify path and name of the Tetin file which is converted from DWG file. After supplying the name and path, click Open to end the process.
GEMS
The GEMS option converts a GEMS file to a Tetin file and loads it.
Select the GEMS file to be imported and click Open to open the window shown below.
Figure 21: Import Geometry from GEMS window
Tetin File
select the required path to store the Tetin file by clicking on the icon.
Tri Tolerance
takes a default value of 0.001 if not otherwise specified.
Unitless
if enabled, the exact unit of Gems geometry is not transferred to the Tetin file.
IDI
The IDI option allows you to import IDI files. Select the IDI geometry file to import. The following options
are available for importing IDI geometry files.
30
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Figure 22: Import Geometry From IDI window
Single Tetin File
creates one Tetin file for the IDI file. If this IDI file is an assembly file, then the Tetin file will contain all
the parts.
Tetin File Per Part
creates one Tetin file for each part. If the IDI file is an assembly file, and Create/Load assembly tetin is
enabled, then the Tetin file is also created for the entire assembly and is loaded into the GUI.
Part Naming
specifies whether part names or numbers are used.
Create/Load assembly tetin
if enabled, the assembly Tetin file will be created and loaded.
Merges multiple instances
if enabled, multiple instances of a part will be merged in one part file.
Import as faceted geometry
The IDEAS CAD data is actually high quality Bspline data. This is usually preferable, but this can add up
to a large amount of data for large models. If this option is enabled, it will convert it to faceted data on
import. This option is not recommended for use with patch based methods.
Disable group to part mapping
disables group to part mapping in the Tetin file.
ParaSolid
The ParaSolid option converts a Parasolid model to a Geometry file (*.tin) and loads it.
The following options are available:
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
31
Main Menu Area
Figure 23: Import Geometry from Parasolid window
Parsolid File
specifies the Parasolid file.
Tetin File
specifies the output Tetin file.
Units
specifies the appropriate units of the geometry.
Rhino 3DM
The Rhino 3DM option converts a Rhino file (*.3dm) to a Geometry file (*.tin) and loads it. The following
options for this conversion are available:
32
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Geometry
By default all the entities in the Rhino file will be imported. If Selected Geometry is clicked, then entities
of different types can be specified for import:
• Points
• Curves
• Surfaces
• Solids
This refers to manifold Boundary Representation (B-rep) solids.
• Meshes
This refers to tessellated (STL-type) data.
Use Object Names for Parts
In Rhino, each object (point, curve, surface, etc.) may have a name associated with it. Enabling this option
will use the Rhino object name as the Part Name. By default the name of the layer on which the object
resides is used.
Include Hidden Layers
Enabling this option will import objects on hidden layers. By default, objects on hidden layers will not
be imported.
Split Composite Curves
If enabled, composite curves will be split into their component curves and imported, instead of as a
single curve.
Include B-rep Surface Trim Curves
If enabled, the 3D spatial curves associated with the 2D parametric trim curves or a surface will be generated and imported, otherwise only the trimmed surface is imported.
Plot3d
The Plot3d option converts a Plot3d file to a Geometry file (*.tin) and loads it.
Figure 24: Import Geometry from Plot3d window
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
33
Main Menu Area
Describe Plot3D File Content
User Input allows you to specify file parameters.
Input type
Specify the input type. Windows_unformatted type refers to unformatted Plot3d meshes created on
Windows. This option allows Unix platforms to read these files as well.
Number of blocks
Specify whether there is a single block or multiple blocks.
Precision
Specify either single or double precision.
Data layout
Specify whether data layout is in planes or not.
Include IBLANK array
Specify whether to include or omit IBLANK array.
Swap byte order
To toggle compatibility between platforms with little-endian or big-endian data storage.
STEP / IGES
The STEP/IGES option converts a STEP/IGES file to a Geometry file (*.tin) and loads it.
The following options are available for importing STEP/IGES geometry.
Figure 25: Import Geometry from Step or IGES window
Tetin File
specifies the required path to save the Tetin file by clicking on the icon.
Use Version 5.1 Step Translator
allows you to translate the file using ANSYS ICEM CFD 5.1 parameters.
Create part name from STEP/IGES file
If multiple STEP/IGES files are opened at once, this option will create the part names in the converted
geometry file from the STEP/IGES files.
34
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Merge geometry files after conversion
If multiple STEP/IGES files are opened at once, this option will merge the multiple geometry files
after conversion.
Ignore units
if enabled, the units specified in the import file will be disregarded and meters are assumed to be
the length unit.
Use healing
if enabled, the Parasolid Kernel attempts healing on the IGES geometry (bodies, surfaces, and loops)
before sending it to the IGES translator.
Formatted Point Data
The Formatted point data option converts formatted point data into the ANSYS ICEM CFD format. The
data is read in as Bspline data.
In this format, each surface's data is represented in the following way: The first line contains two numbers,
the number points for each curve, and the number of curves for each surfaces. The remaining lines
represent the points of the surface. An example is shown below:
24
0.0682618 9.731237 0.5112982
-0.2821764 19.30035 0.5278823
-1.046131 9.840971 1.598944
-1.646277 19.23213 1.157967
-1.866522 9.97312 2.660025
-2.986559 19.06998 1.786853
-2.552526 10.16115 3.688797
-4.276251 18.82248 2.374612
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
35
Main Menu Area
Figure 26: Import Geometry from Formatted Point Data window
Reference Geometry
The Reference Geometry option allows you to use an existing Tetin file as a reference to map the mesh
setup and other parameters to the currently loaded geometry file. This is important in parametric
modeling, as the setup that is done for one Tetin file can be reused for subsequent design changes.
The parameters that will be read from the reference geometry file include:
• Global Meshing parameters
• Entity meshing parameters
• Prism meshing parameters
• Part names of entities
• Dormant curves and points
• Density regions
• Connector definitions
• Geometry subsets
• Periodicity
36
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Import Mesh
Figure 27: Import Mesh options
The Import Mesh menu allows you to import mesh from the following formats:
From ANSYS
From Abaqus
From CFX
From CGNS
From Fluent
From LS-DYNA
From Nastran
From Patran
From Plot3d
From Starcd
From STL
From TecPlot
From Vectis
From ANSYS
The From ANSYS option allows you to import an ANSYS mesh file into ANSYS ICEM CFD. Select a *.cdb
file to import.
From Abaqus
The From Abaqus option allows you to import an Abaqus mesh file into ANSYS ICEM CFD.
From CFX
The From CFX option allows you to import a CFX5 mesh file into ANSYS ICEM CFD.
After selecting the CFX5 *.def file, you need to choose the translation option shown below.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
37
Main Menu Area
Figure 28: Import CFX Options
Set Face Parts from
BC Patches
creates a Part for each different boundary condition (inlet, outlet, wall, Domain-Interface-1-side-1,
etc.) as shown in Figure 29: Set Face Parts from BC Patches Option (p. 38).
Figure 29: Set Face Parts from BC Patches Option
Surfaces
creates a part from each surface (surface 1, surface 2, etc.) as shown in Figure 30: Set Face Parts from
Surfaces Option (p. 38).
Figure 30: Set Face Parts from Surfaces Option
38
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Click Done to complete the process.
Note
CFX5 mesh import disallows duplicate nodes and faces. Internal walls should not be split,
because this introduces duplicate nodes and faces and the connectivity between the faces
may be incorrect. Use Reorient Mesh > Reorient Consistent on all thin surfaces prior to export
to avoid inconsistencies in the orientation of face elements.
From CGNS
The From CGNS option allows you to import a CGNS mesh file into ANSYS ICEM CFD. You need to
specify whether the input mesh file is structured or unstructured mesh.
From Fluent
The From Fluent option allows you to import a Fluent mesh file into ANSYS ICEM CFD. Select a *.cas
file to import.
From LS-DYNA
The From LS-DYNA option allows you to import an LS-DYNA mesh file into ANSYS ICEM CFD.
Figure 31: Import LS-DYNA Options
Import include files as
INCLUDE files can be read in as links or as actual data.
Note
If the INCLUDE files are read in as data, they will be written to the assembly file and the
original file structure will not be preserved.
Note
Any unsupported LS-DYNA cards will be written to a temp file named “unsupported.k”
in the working directory, and will be appended to the input file of this project if it is
written out.
From Nastran
The From Nastran option allows you to import a Nastran mesh file into ANSYS ICEM CFD.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
39
Main Menu Area
Figure 32: Import Mesh from Nastran Options
From Patran
The From Patran option allows you to import a Patran mesh file into ANSYS ICEM CFD.
Figure 33: Import Mesh from Patran Options
Transfer family information
Multiple
converts each Patran group (PID) into an ICEM CFD part.
Single
brings the Patran groups all in as one part.
From Plot3d
The From Plot3d option allows you to import a Plot3d mesh file into ANSYS ICEM CFD.
Plot3d files do not provide a topology, so ANSYS ICEM CFD will recompute a topology. Mesh will be
converted to an unstructured mesh by default. The subfaces, edges, and vertices belonging to the recomputed topology will added to separate parts.
From Starcd
The From Starcd option allows you to import a STAR-CD mesh file into ANSYS ICEM CFD. Select any
one of the *.cel, *.vrt, or *.inp files with the same file name.
From STL
The From STL option allows you to import an STL mesh file into ANSYS ICEM CFD. Note that the parts
defined in the STL file will also be imported. Select the format for the part names and click Done to
finish the operation.
40
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Part names
Generate
generates part names of the format Filename.PartName, where PartName is the part name
defined in the STL file.
From file
retains the part names as defined in the STL file.
Note
This option is valid only for STL files in ASCII format. For STL files in binary format,
the part names of the format Filename.PartName will be generated as described.
From TecPlot
The From TecPlot import filter allows you to read CFX files and convert the mesh data to ANSYS ICEM
CFD unstructured mesh.
From Vectis
The From Vectis option allows you to import a Vectis mesh file (*.sdf ) into ANSYS ICEM CFD.
Note
This option is available only on Linux systems.
Export Geometry
Figure 34: Export Geometry Options
The Export Geometry option allows you to export geometry in the following formats.
To IGES
To Parasolid
To Rhino 3DM
To STL
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
41
Main Menu Area
To IGES
The To IGES option allows you to export geometry in IGES format. After selecting To IGES, select the
geometry file (*.tin) that you want to import in the Select tetin file window.
Figure 35: Export to IGES File
After selecting the geometry file, supply the name and the path of for the IGES file and click Save in
the Select iges file window to complete the export process.
Note
Faceted data cannot be exported to an IGES file. If faceted data is found in the geometry
file, it will not be translated.
To Parasolid
The To Parasolid option converts geometry in ANSYS ICEM CFD to a Parasolid file.
Select To Parasolid and then select the tetin file to export in the Select tetin file window. After selecting
the geometry file, supply the name and the path of for the IGES file and click Save in the Select ps file
window to complete the export process.
Files with an asterisk (*) indicates these files are OK to select.
Note
Faceted data cannot be exported to a Parasolid file. If faceted data is found in the geometry
file, it will not be translated.
42
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
To Rhino 3DM
The To Rhino 3DM option converts geometry in ANSYS ICEM CFD to a Rhino 3DM file format (*.3dm).
Select the geometry file (*.tin) to be exported. The following options are available.
Geometry
By default all the entities in the geometry file will be exported. If Selected Geometry is clicked, then
entities of different types can be specified for export:
• Points
• Curves
• Surfaces
• Meshes
Units
Specify the units of measurement of the file.
Tolerance
This is the absolute tolerance value passed to the Rhino file. It is used in Rhino for operations such as
trimming and intersecting.
Include Dormant Entities
By default, any dormant entities (typically points and curves) created will not be exported to Rhino. If
this option is enabled, the dormant entities will also be exported.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
43
Main Menu Area
Do Not Trim Surfaces
If this option is enabled, any trim curves are removed, so that trimmed surfaces will be exported to Rhino
as untrimmed.
Rebuild Coedges
If enabled, the coedges (3D spatial curves) will be rebuilt from the 2D parametric curves (pcurves) by
projection prior to exporting. This sometimes improves the quality of the exported 3DM file, particularly
when the Tetin file has relatively large tolerances.
Version 2 Compatibility
The default will export the data to a Version 3 3DM (Rhino) file, which cannot be read by Rhino Version
2.xx. If this option is enabled, then the 3DM file will be version 2 compatible.
To STL
The To STL option converts geometry in ANSYS ICEM CFD to the STL format. Select the appropriate file
format and click Done to finish the operation.
File format
specifies the format for the STL file.
Ascii
exports the STL file in ASCII format.
Binary
exports the STL file in binary format.
Export Mesh
Figure 36: Export Mesh Options
Mesh generated in ANSYS ICEM CFD can be exported to the following formats:
To Abaqus
To ANSYS
44
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
To Autodyn
To Exodus
To Ideas
To LS-DYNA
To Nastran
To Patran
To Radioss
To FE Modeler
Write STL file
Spectral Elements
To Abaqus
The To Abaqus option allows you to export the mesh in Abaqus format. For information about the
Abaqus interface, select the Output Interfaces option in the Help menu to open the ANSYS ICEM CFD
CFD Output Interfaces information, and click ABAQUS in the Table of Supported Solvers.
Figure 37: Abaqus Export Options
To ANSYS
The To ANSYS option allows you to export the mesh in ANSYS format. For information about the ANSYS
interface, select the Output Interfaces option in the Help menu to open the ANSYS ICEM CFD Output
Interfaces information, and click ANSYS in the Table of Supported Solvers.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
45
Main Menu Area
Figure 38: ANSYS Export Options
To Autodyn
The To Autodyn option allows you to export the mesh in Autodyn format. Information for this option
can be found in the Solve Options > Autodyn Options > Write/View Input File section.
Note
This solver format supports multiblock structured or unstructured mesh. If a multiblock domain
is loaded, the multiblock.info interpreter will be used. For unstructured mesh, the LS-DYNA
interpreter will be used to create the unstructured mesh.
To Exodus
For information about the Exodus interface, select the Output Interfaces option in the Help menu to
open the ANSYS ICEM CFD Output Interfaces information, and click EXODUS in the Table of Supported
Solvers.
The options available are:
Figure 39: Exodus Options
46
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
To Ideas
The To Ideas option allows you to export the mesh in Ideas format. For information about the Ideas
interface, select the Output Interfaces option in the Help menu to open the ANSYS ICEM CFD Output
Interfaces information, and click IDEAS in the Table of Supported Solvers.
Figure 40: Ideas Options
To LS-DYNA
The To LS-DYNA option allows you to export the mesh in LS-DYNA format. For information about the
LS-DYNA interface, select the Output Interfaces option in the Help menu to open the ANSYS ICEM
CFD Output Interfaces information, and click LS-DYNA in the Table of Supported Solvers.
Figure 41: LS–Dyna Export Options
To Nastran
The To Nastran option allows you to export the mesh in Nastran format. For information about the
Nastran interface, select the Output Interfaces option in the Help menu to open the ANSYS ICEM CFD
Output Interfaces information, and click NASTRAN in the Table of Supported Solvers.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
47
Main Menu Area
Figure 42: Nastran Export Options
To Patran
The To Patran option allows you to export the mesh in Patran format. For information about the Patran
interface, select the Output Interfaces option in the Help menu to open the ANSYS ICEM CFD Output
Interfaces information, and click PATRAN in the Table of Supported Solvers.
Figure 43: Patran options window
To Radioss
The To Radioss option allows you to export the mesh in Radioss format. For information about the
Radioss interface, select the Output Interfaces option in the Help menu to open the ANSYS ICEM CFD
Output Interfaces information, and click RADIOSS in the Table of Supported Solvers.
Figure 44: Radioss options window
To FE Modeler
The To FE Modeler option allows you to export the mesh to a *.dat file (similar to the Nastran format)
which can be imported into FE Modeler. For v15.0, you can also save the *.uns file and read it in FE
Modeler.
48
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
Write STL file
The Write STL File option allows you to write mesh data as faceted data in STL format which can be
read by any other solver/software. Specify the parameters as appropriate and click Done to finish the
operation.
Ascii STL file?
allows you to write the STL file in ASCII or binary format.
Perform shift?
checks if a vertex extends into negative space. When enabled, the whole mesh will be shifted by the
amount the vertex extends into negative space.
Surface Mesh domain
specifies the surface mesh domain file.
STL output file
specifies the output STL file.
Spectral Elements
The Spectral Elements option allows you to create spectral elements. Select the elements to be created
into spectral elements. Select the Order and the Bunching law to be used. The following Bunching
laws are available:
• Gauss-Lobatto-Legendre
• Chebyshev-Lobatto
• Legendre
Replay Scripts
ANSYS ICEM CFD makes it possible for users to write their own specialized scripts to customize ANSYS
ICEM CFD or run complex operations in batch mode. A script is basically a program written in the Tcl/Tk
language. There are a number of standard references for this language, and more information that can
be found at http://www.scriptics.com/.
The Replay Scripts menu item opens a submenu of options as shown in Figure 45: Replay Options (p. 50).
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
49
Main Menu Area
Figure 45: Replay Options
Replay Control
This option helps you create script files by performing operations in ANSYS ICEM CFD and recording
the equivalent Tcl/Tk commands in a Replay file. The user can modify or run this Replay file as a script
file. This gives opportunity for users unacquainted with Tcl/Tk to also use scripting.
Note
If you are using ANSYS ICEM CFD in Workbench and want to step through Workbench
Input Parameters you have created, you must open the Workbench Replay Control from
the One-click menu. For more information, See Workbench Integration in the ANSYS ICEM
CFD User’s Manual.
The example shown in Figure 46: Replay Control window (p. 50) contains the script commands recorded while the following operations were performed in ANSYS ICEM CFD :
Geometry > Create Point > Screen Select.
New part name is POINTS.
Screen select a location on the loaded Geometry file.
Figure 46: Replay Control window
The Replay control window can be minimized at any time.
Record (after current)
To record commands in the Replay file, toggle this option ON. Commands will be appended.
50
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
File Menu
All commands
To record all the commands that you or ANSYS ICEM CFD performs, toggle this option ON.
Do one
While running the script, clicking this button will perform only one step, or one line of the Replay
file.
Do all
ANSYS ICEM CFD will run the whole Replay file when this option is selected.
Do Range
To run a specific subset of the commands in the Replay file, select this option. The Replay Range
window opens where you select the Start line and End line numbers, as shown in Figure 47: Replay
Range window (p. 51).
Figure 47: Replay Range window
Skip
To ignore the command line where the cursor lies, select this option. The cursor will move to the
next line.
Load
To open a previously stored Replay file (*.rpl) in the Replay Control window, select this option.
The File Selection window opens where you choose the Replay file to be loaded.
Save
Saves the Replay file in a location specified in the File selection window.
Edit
Opens the Replay script in your text editor (e.g. Notepad) where you to modify the script. You will
be prompted to save your work when you close the editor.
Insert
Inserts one line in the script so that you can enter comments or commands.
Delete one
Removes the selected line of command from the Replay file.
Delete all
Clears all the commands from the Replay Control window.
Delete range
Deletes a specific range of commands from the Replay file.
Renumber
If you have added or deleted commands manually, this button re-sequences the command line
numbers.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
51
Main Menu Area
Always update
Updates the model after each step. When this is disabled, the replay script will be run in batch mode
and the model will be updated at the end. You can enable this option to see the step by step updates,
however, you can disable it to more rapidly generate the model.
Ignore errors
When disabled (default), the replay control will stop executing the replay script when an erroneous
command is reached. When enabled, the replay control will skip the erroneous command and continue to execute the subsequent commands in the replay script.
Stop
Halts an ongoing Replay of your script file.
Clean
Filters through the Replay file and removes unnecessary lines. You can adjust this clean filter by right
clicking on the Replay window and choosing Edit Filter. Simply enter the ic_commands that you
want removed. There is also the right click option to Undo Clean, which will undo the actions of
the clean filter.
Note
If an Undo action was performed while recording the Replay file, then the user needs
to manually remove the appropriate lines from the script (starting with undo_begin
and ending with the undo_end command). The Clean filter does not take care of
this.
Done
Closes the Replay Control window. You will be prompted to save the Replay file before closing the
window if it is not saved.
Load script file
The Load script file option opens a dialog box where you select a replay script file (*.rpl) to display
in the Replay Control window.
Run from script file
The Run from script file option opens a dialog box where you select a previously written script and
initiate automatic replay.
Note
In order to know what commands are available to you to do useful things like load
meshes and run applications, a set of functions that begin with the letters ic_ that can
be called from scripts are documented in the Programmer’s Guide. The user is discouraged
from reading through the tcl files in $ICEM_ACN/bin/med and using undocumented
functions because they might change at any time.
Recording scripts
The Recording scripts option starts/stops the recording of commands.
52
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Edit Menu
Exit
The Exit option closes the ANSYS ICEM CFD application. You will be prompted to save any new work
in your project.
Edit Menu
Figure 48: Edit menu
The Edit menu has the following options:
Undo
Redo
Clear Undo
Shell
Facets > Mesh
Mesh > Facets
Struct Mesh > CAD Surfaces
Struct Mesh > Unstruct Mesh
Struct Mesh > Super Domain
Shrink Tetin File
Undo
The Undo option undoes the last operation. For a few operations like smoothing, refinement, coarsening,
conversion, etc., where the whole mesh is changing, only one Undo operation is possible.
Note
Operations related to display cannot typically be undone.
Note
When using Undo for blocking operations, the index control may be affected because the
active state of the index control may be modified by the Undo operation.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
53
Main Menu Area
Redo
The Redo option redoes the previous Undo operation. You can only redo operations that have been
undone.
Note
Once a new command is performed; all operations undone are lost from the undo/redo
history.
Clear Undo
The Clear Undo option clears up the memory used by the Undo history. This option is most useful
after performing an operation (such as “Add to Part” , “Change Type”, or “Split/Redistribute Prisms”) on
a large number of elements because the Undo needs to store the state both before and after the operation in memory.
Note
The Clear Undo option frees up the memory for further operations, but you will not be
able to undo the particular operation any more.
Shell
The Shell option opens a new terminal in the current working directory.
Facets > Mesh
The Facets > Mesh option will convert the faceted geometry data into unstructured mesh format.
Mesh > Facets
The Mesh > Facets option will convert unstructured mesh format into faceted geometry data.
Struct Mesh > CAD Surfaces
The Struct Mesh > CAD Surfaces option will convert structured mesh format into CAD surfaces.
Struct Mesh > Unstruct Mesh
The Struct Mesh > Unstruct Mesh option will convert structured mesh format into unstructured mesh
format.
Struct Mesh > Super Domain
The Struct Mesh > Super Domain option will convert structured mesh format into a superdomain file.
In the popup window that appears, highlight the domains with the specified project prefix that are to
be converted to a superdomain.
54
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
View Menu
Shrink Tetin File
The Shrink tetin file option removes header lines, comment lines, and unnecessary definitions in the
Tetin files, which can reduce the size of the Tetin file significantly. The comment lines include the date
and software version of the last modification.
Selecting this option will automatically open a browser window. Select the desired Tetin file. The
number of lines removed will appear in the Message window. From the browser window, you can either
save the file with a new name or overwrite the original file.
View Menu
The View menu contains options for choosing different orientations of the model in the graphics display.
Figure 49: View Options
The different options are shown in Figure 49: View Options (p. 55).
Fit
Box Zoom
Top
Bottom
Left
Right
Front
Back
Isometric
View Control
Save Picture
Mirror and Replicates
Annotation
Add Marker
Clear Markers
Mesh Cut Plane
Fit
The Fit option scales the model so that it fits in the graphics window.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
55
Main Menu Area
Box Zoom
The Box Zoom option will prompt you to click and drag a rectangular region which is then zoomed in
to fill the graphics window.
Top
The Top option orients the model so that you see it parallel to the XZ-plane, looking from the positive
Y-axis.
Bottom
The Bottom option orients the model so that you see it parallel to the XZ-plane, looking from the
negative Y-axis.
Left
The Left option orients the model so that you see it parallel to the YZ-plane, looking from the negative
X-axis.
Right
The Right option orients the model so that you see it parallel to the yZ-plane, looking from the positive
X-axis.
Front
The Front option orients the model so that you see it parallel to the XY-plane, looking from the positive
Z-axis.
Back
The Back option orients the model so that you see it parallel to the XY-plane, looking from the negative
Z-axis.
Isometric
The Isometric option orients the model so that you see a 3D pictorial representation of the model is
shown.
Note
One of the six orthographic views or the isometric view may be easily selected by clicking
on one of the points of the Display Triad in the graphics window.
View Control
The View Control options allow you to save or edit the current view.
56
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
View Menu
Figure 50: View Control Options
Save Current View
allows you to save the current view.
Edit/Load/Save Views
allows you to edit and save different views. You can save the views to an external file for use with any
project. The views can also be saved with the current project file when the Automatically Save Views
to Project option in the Settings - General DEZ is enabled (see the General (p. 70) section). The View
Control appears in the bottom-right corner of the screen.
Save Picture
The Save Picture option allows you to save different views of the model in different picture formats.
The format can be selected from the Save Picture DEZ shown in Figure 51: Save Picture DEZ (p. 57).
Figure 51: Save Picture DEZ
Output Prefix
specifies the name of the picture file you want to save in the current directory (where project file exists).
Alternatively, you can browse to any other directory by clicking on the icon.
Generate new file names
toggles the generation of output files with new names each time the function is used.
Format
specifies the picture format. You can select any of the following picture formats: PostScript, PS from
screen, PPM, X11, TIFF, GIF, JPEG, and VRML.
The following options are available for the PS from screen, PPM, X11, TIFF, GIF, and VRML formats:
Invert black and white
controls the foreground/background color. When enabled, the background color in the saved image
will be changed from black to white.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
57
Main Menu Area
Landscape mode
controls the orientation of the saved image. When enabled, the image will be saved in landscape
mode; else the image will be saved in portrait mode.
Scale Factor
scales the image taken with respect to the actual size appearing in the graphics window. Example:
A Scale Factor of 2 doubles the size of the picture taken.
Quality (for JPEG format only)
specifies the quality level, which will determine the file size.
Figure 52: PostScript Format Options
The following options are available for the PostScript format:
PS Type
specifies the PS type. The PS format is suitable for operating systems other than Windows, like UNIX.
The EPS format is suitable for the Windows operating system.
PS Mode
specifies the color mode for the image saved. Color maintains the actual colors of the picture. Gray
converts all the colors to gray scale. Mono converts the picture to black and white.
Include Frame
shows the border of the picture in a different color than the background.
Title (top)
specifies the title for the image. This can be viewed at the top of the postscript file.
Label (bottom)
specifies the label which will appear at the bottom of the postscript file.
58
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
View Menu
Send to printer
allows you to print the picture after saving.
Mirror and Replicates
The Mirrors and Replicates DEZ contains options that allow you to create a mirror image of a model.
Note
Mirrors and replicates are not real objects. They are only for display purposes and therefore
cannot be selected or have operations performed on them.
Figure 53: Mirror and Replicates DEZ
X, Y, Z Mirror
contains options for defining the mirror plane. You can use the standard defined mirror planes (normal
or outward in the X, Y, or Z directions) or define a specific plane in the required direction using the
Modify specific mirror dialog (seeFigure 54:Modify specific mirror Dialog (p. 59)).
Figure 54: Modify specific mirror Dialog
Replicate by rotating with
enables the creation of replicates by rotation. Specify the Center, Axis, and Angle of rotation to create
the replicates.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
59
Main Menu Area
Replicate by translating
enables the creation of replicates by translation. Specify the distances in the X, Y, and Z directions for
the translation.
Times
indicates the number of replicates.
Annotation
Annotations are graphical objects (such as thumbnail pictures or some explanatory text) that are defined
independently of the data being displayed, and are generally fixed in position in the window.
Figure 55: Annotations Options
The available annotation options are as follows:
Add in the current window
Modify by selecting
Pick and move
Pick and remove
Reset mouse
Add in the current window
The Add in the current window option allows you to add annotations to the currently displayed data.
Figure 56: Create/Modify Annotation window
Create
allows you to create the following types of annotations:
• Text
• Utf Text
60
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
View Menu
• Lines
• Box
• Circle
• Polygon
• Marks
• Image
• Colormap Bar
The options available are:
Text font
specifies the font size to use for text annotations.
Line width
specifies the line width, in pixels, used for drawing line, circle, box, and polygon annotations.
Arrow type
determines whether an arrow will be drawn at the start and/or end points of the line.
Symbol type
specifies the type of symbols used in mark annotation.
Symbol size
specifies the size of marker annotations.
Color
specifies the color of the annotation.
Fill
enables the filling of box, circle, polygon, and mark annotations.
Modify by selecting
The Modify by selecting option allows you to modify features of specific annotations, such as size,
text, color, and font.
Pick and move
The Pick and move option allows you to pick and move specific annotations.
Pick and remove
The Pick and remove option allows you to pick and remove specific annotations.
Reset mouse
The Reset mouse option allows you to reset the mouse.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
61
Main Menu Area
Add Marker
The Add Marker option allows you to display text in the GUI using the Add marker dialog (see Figure 57: Add Marker Dialog (p. 62)).
Figure 57: Add Marker Dialog
Position
specifies the coordinates for the position of the marker.
Select
allows you to select the position of the marker from the existing geometric information.
Text
specifies the text to be displayed as a marker.
Accept
creates given text at a given location as a marker.
Reset
resets the position and text to the previously created marker.
Cancel
cancels the command and closes the Add Marker dialog.
Help
launches the Help manual.
Clear Markers
The Clear Marker option allows you to clear all the created markers from the GUI.
Mesh Cut Plane
A cut plane is used to visualize results on a plane cut through the three dimensional model. Results are
viewed on the cut plane as well as on the 2D Dynamic window. The cut plane may be defined in several
ways depending on the application. These options are described here in detail.
62
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
View Menu
Figure 58: Manage Cut Planes DEZ
Show Cut Plane
enables the display of the cut plane.
Show whole elements
enables the display of the elements at the borders of the cut plane.
Method
contains options for defining the cut plane.
By Coefficients
defines the cut plane by the equation of the normal vector. The equation is of the form: Ax + By +
Cz + D = 0. Specify the coefficients A, B, C, and D in the fields Ax , By, Bz, and D.
By Point and Normal
defines the cut plane by a point and the normal. Specify the Global Cartesian coordinates in the X,
Y, and Z direction for the point (Pn ) and the X, Y, and Z components of a unit vector normal to the
desired cut plane (NX, NY, and NZ).
By Corner Points
creates a cut plane passing through the three specified points. You can enter the Cartesian coordinates
for Pt1, Pt2, and Pt3.
By 3 Points
creates a cut plane passing through the three locations selected.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
63
Main Menu Area
Move or Rotate
allows you to interactively move and/or rotate a previously defined cut plane. Use the left mouse
button to rotate the cut plane about the normal axis and the middle mouse button to move the cut
plane. Click the right mouse button to end the interactive movement of the cut plane.
Middle X plane
positions the cut plane at the middle of the geometry in the X-direction.
Middle Y plane
positions the cut plane at the middle of the geometry in the Y-direction.
Middle Z plane
positions the cut plane at the middle of the geometry in the Z-direction.
Fraction Value
specifies the location of the plane.
Display back plane
enables the display of the back plane.
Draw plane normal
enables the display of the normal direction of the plane.
Draw plane border
enables the display of the border of the back plane.
Color
specifies the color of the back plane. To select a different color, click on the color bar and select a color
from the menu that appears.
Create mesh subset
creates a mesh subset of cut plane elements.
Info Menu
The Info menu provides useful information related to the model like curve length, node information,
distance between two points, etc.
Figure 59: Info Options
The options available are as follows:
64
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Info Menu
Geometry Info
Surface Area
Frontal Area
Curve Length
Curve Direction
Mesh Info
Mesh Area/Volume
Element Info
Node Info
Element Type/ Property Info
Toolbox
Project File
Domain File
Mesh Report
Geometry Info
The Geometry Info option prints the number of surfaces, curves, material points and parts existing in
the model in the message window.
Surface Area
The Surface Area option prints information (like surface names, total area, etc.) for the selected surfaces
in the message window.
Frontal Area
The Frontal Area option prints information about the area of the model in front of the screen in the
message window.
Curve Length
The Curve Length option prints information (like curve name, curve length, etc.) for the selected curves
in the message window.
Curve Direction
The Curve Direction option will prompt you to select curves. The curve direction will be displayed for
each selected curve. The curve direction is the direction of increasing curve parameter, from 0 to 1.
Note
The curve direction can be reversed using the Reverse Direction option in the Modify
Curve(s) DEZ. Curve direction may affect some meshing and geometry functions that
utilize curve end locations.
Mesh Info
The Mesh Info option prints the following information about the mesh in the message window:
• Total number of elements
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
65
Main Menu Area
• Total number of nodes
• The minimum (Min) and maximum (Max) coordinates of the bounding box.
• Number of elements by type
• Number of elements by parts
• Maximum edge sides
This is the maximum edge distance between nodes of the mesh. The nodes will be placed in the
subset that is listed.
• Minimum edge sides
This is the minimum edge distance between nodes of the mesh. The nodes will be placed in the
subset that is listed.
Mesh Area/Volume
The Mesh Area/Volume option prints the area and volume of the mesh elements by type, and the
total area and volume in the message window. For example:
Area of 5534 TRI_3 is 6
Total Area is 6.0
Volume of 10442 TETRA_4 is 0.358048
Volume of 4040 PENTA_6 is 0.590489
Volume of 314 PYRA_5 is 0.051463
Total Volume is 1.0
Note
ANSYS ICEM CFD is essentially unitless. The area and volume values reported in the message
window are the square and cube, respectively of the length units in ANSYS ICEM CFD. For
example, if the length units are in meters, the values represent square meters for area and
cubic meters for volume.
The length units can be set in the Model/Units DEZ.
Element Info
The Element Info option prints the following information for the selected elements in the message
window:
• Number of elements selected
• Element type
• Element part
• Node numbers
• Element Thickness (for surface elements)
• Mesh Quality (for mesh elements, if Quality metrics are selected under Settings > Meshing > Quality Info)
66
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Info Menu
If more than one element is selected, the information for each element is printed out in the message
window.
Node Info
The Node Info option prints the following information for the selected nodes in the message window:
• Number of nodes selected
• Node number
• Node dimension
• Node coordinates
• Thickness at node (for surface elements)
• Mesh Quality (for mesh elements, if Quality metrics are selected under Settings > Meshing > Quality Info)
If more than one node is selected, the information for each node is printed out in the message window.
Element Type/ Property Info
The Element Type / Property Info option prints information about element types and defined material
properties in the message window.
Toolbox
The Toolbox option will open a window in the lower right hand corner of the GUI that includes a calculator, notepad, unit conversion tables, and a variables/parameters window.
Note
Variables may be used instead of numerical values in scripts and geometry creation
functions.
Project File
The Project File option prints information regarding the project file in the message window.
Domain File
The Domain File option prints information about the domain file in the message window.
Mesh Report
The Mesh Report option allows you to generate a mesh quality report using the options in the Mesh
Quality Report DEZ.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
67
Main Menu Area
Figure 60: Mesh Quality Report DEZ
Mesh report file name
specifies the name of the mesh report file.
Title
specifies title of the mesh report project.
Author
specifies the author of the project.
Write summary
enables the writing of the summary for the mesh.
Mesh types
contains options to report available mesh statistics for all or selected element types.
All
reports available mesh statistics for all available element types.
Select
limits the mesh statistics report to only check the selected element types.
68
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
Quality
Write quality
enables the writing of the quality for the mesh.
All existing quality types
enables the writing of the quality report for all existing quality types for the mesh. The list of quality
measures reported is dependent on the loaded mesh. This option is disabled by default. When disabled
(default), the mesh report will include the quality report for only the Quality, Determinant, Aspect
Ratio, Min angle, Max ortho, Max warp, Max warpgls, and Skew measures.
Write diagnostics
enables the writing of the diagnostics for the mesh.
Settings Menu
The Settings menu contains different setting options that allow you to change the default settings of
display, memory, speed, etc.
Figure 61: Settings Options
The options available are as follows:
General
Product
Display
Speed
Memory
Lighting
Background Style
Mouse Bindings/Spaceball
Selection
Remote
Model/Units
Geometry Options
Meshing
Solver
Reset
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
69
Main Menu Area
General
The General setting options allow you to change the default settings regarding files, number of processors, text editor, etc., for ANSYS ICEM CFD in the Settings-General DEZ.
Figure 62: Settings-General DEZ
Number of Processors
specifies the number of processors. Some operations such as tetra meshing, hexa meshing, and
smoothing can use multiple processors if they are available. Specifying multiple processors will enhance
the performance of these operations. You can specify a value from 0 to 256. The default is 1. If the
Number of Processors is set to 0, the number of processors will be set automatically to the maximum
number of processors available.
Text Editor
defines the default text editor that will be used by ANSYS ICEM CFD. For example: Notepad for Windows
and vi for UNIX systems.
Temporary Directory
defines a temporary directory where ICEM CFD data files are written. To define the location, list the path
of an existing directory using UNIX notation (for example, c:/users/temp instead of c:\users\temp).
If the directory does not exist, ICEM CFD will not create it.
Save Emergency Mesh on Crash
enables the saving of the mesh file in the event of a program crash.
Save Emergency Tetin on Crash
enables the saving of the Tetin file in the event of a program crash.
Save Emergency Blocking on Crash
enables the saving of the blocking file in the event of a program crash.
70
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
Clean up Temporary Files
enables the cleaning up of temporary files, if any, inside the project directory.
Record Journal File
creates a journal file (*.jrf ) of the Tcl/Tk commands representing all the operations in an entire session.
This is similar to replay scripts, except that the journal file is saved in the working directory. The journal
files can be accessed using the same options used for Replay Scripts.
Note
Journal files are useful for debugging purposes. Technical Support may utilize these files
when diagnosing a problem.
Keep existing file names
enables the use of the existing mesh, geometry, and other file names when saving a project instead of
creating new file names to match the project name. These file names are stored with the project and
loading the project file will automatically load these files too. This feature is useful when working with
large files. If this option is disabled (default), saving the project with a new name will create new files
with matching names for geometry, mesh, attributes, etc.
Clear undo after saving project or geometry
enables the clearing of the Undo history after saving the project or geometry. If this option is disabled,
you will be able to undo operations even after the project has been saved.
Automatically Save Views to Project
enables the saved views to be saved with the project file. This option is enabled by default.
Note
You can use the View > View Control > Edit/Load/Save Views option (see the View
Control (p. 56) section) to edit the views saved with the project file. The View Control
appears in the bottom-right corner of the screen.
Use JAVA Help
allows you to open the Java file version of the Help Manual when selecting Help > Help Topics.
Product
The Product settings include options for running ANSYS ICEM CFD. The settings control which tabs are
visible in the ANSYS ICEM CFD environment.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
71
Main Menu Area
Figure 63: Product-Selection DEZ
Product Setup
allows you to set the flavor of ANSYS ICEM CFD. This directly affects which tabs are visible in the interface.
The tabs for Geometry, Mesh, and Edit Mesh are visible in all cases.
Note
Changes made to this DEZ do not take effect until the next time the software is started.
Default
determines the default capabilities of ANSYS ICEM CFD available for a user based on the license key.
If the aienv and aioutcfd key are available, the default is FEA + CFD Utilities. If only the aienv
key is available (without aioutcfd) then the FEA Version is the default. If an aimed key (comes
with Tetra or Hexa) is drawn along with aioutcfd, the default will be the CFD Version. If the
aimed key is not accompanied by an aioutcfd key, then ANSYS solvers – CFD Version is the
default. If you have the aiaddon key, then ANSYS Solvers – FEA Version is the default.
Note
If a user has all of these keys, the default will use the order above. The user can
override this by specifically choosing one of the other radio buttons. If a tab is chosen
without access to the required keys, the message window will display a license error
when the user tries to access that tab.
FEA + CFD Utilities
displays all tabs. This includes access to all CFD solvers, CFD utilities, and advanced setup options
for FEA solvers like ANSYS, LS-DYNA, and Nastran.
FEA Version
shows the Properties, Loads, Constraints and Solve Options tabs, but not the Output (CFD) tab.
You can set advanced boundary conditions for FEA solvers like ANSYS, LS-DYNA, and Nastran.
72
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
CFD Version
shows the Output tab, but not the Properties, Loads, Constraints or Solve Options tabs. Separate
license keys for Quad, Tetra, and Hexa meshers are required.
ANSYS Solvers - CFD Version
similar to the CFD Version, except that the Output tab shows buttons for ANSYS solvers instead of
the larger list of solvers.
ANSYS Solvers - FEA Version
similar to the FEA Version, except license limited to only export to ANSYS, Autodyn and LS-DYNA.
Blocking
enables the Blocking tab. The ANSYS ICEM CFD Hexa license (aihexa) is required.
GUI Style
specifies the style for the GUI. You can select either the Workbench style or the traditional ICEM CFD
style. The Workbench style has the display tree on the upper-left and the DEZ on the lower-left of the
interface. The background colors are set up to match those in ANSYS Workbench and the ANSYS logo
is displayed in the upper-right corner of the graphics window. The message window is wider and spans
the entire window when there is no histogram, scan, index, or interrupt window present. This is the
default setting for ANSYS ICEM CFD. The ICEM CFD style has the positions of the display tree and the
DEZ swapped, with a solid background color.
Note
This is not the same as the option to use the old GUI.
Beta Options
enables beta options within ANSYS ICEM CFD to be made available. These options are new features that
are pending more extensive testing and documentation before being added to the standard release.
Note
After enabling any option, you must quit and restart the software to see the changes.
Display
The Display options allow you to change the display settings for ANSYS ICEM CFD using the options
in the Settings-Display DEZ. Some changes in settings will be effective only after restarting ANSYS
ICEM CFD.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
73
Main Menu Area
Figure 64: Display Settings window
74
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
Use Native Display List
enables the use of OpenGL or another accelerated graphics library when possible. The final color including
the lighting effects are fixed until the surfaces are refreshed. This option is recommended, because the
color and lighting effects are updated for every redraw. Depending on the system and machine, this
option may result in slower display redraws. Some nVidia graphics cards may show slower performance
when this option is enabled.
Note
If you encounter graphics performance problems, disable the Use Native Display List
option and click Apply. You do not need to restart ANSYS ICEM CFD for this change to
take effect.
Use OpenGL Feedback
enables the use of OpenGL's feedback mechanism to detect the 3D coordinates of the location on the
model that the mouse is pointing to. This option is recommended when the option Use Native Display
List is enabled, since it allows the program to release the memory holding the model's geometry data
once it has been used to create the display list.
Disable Overlays
disables the use of overlays in drawing a selection box since some graphical cards perform slower with
this option.
Enable Smooth Movement
Enable Smooth Movement improves display performance, allowing you to rotate very large models
smoothly. With this option enabled, you will need to double click to change the model’s center of rotation,
in Dynamic Mode. See The ANSYS ICEM CFD GUI in the User’s Manual and Mouse Bindings/Spaceball (p. 81) in the Help manual.
Simplify Geometries
contains options for simplifying the geometry rendering.
Auto Simplify
simplifies geometry rendering as the model is zoomed out. This option can speed up rendering of
large assemblies or models containing a large number of surfaces. The Simplification level (pixels)
option sets the threshold for simplification.
Simplification level (pixels)
sets the threshold for simplifying geometry rendering. As the model is zoomed out, surfaces of less
than the specified number of pixels across are displayed in a more simplified way in order to speed
up graphics performance. The default is 10 pixels, meaning that as the model is zoomed out and
each surface becomes less than 10 pixels across, its display is simplified.
Figure 65: Simplifying Geometry Rendering (p. 76) shows a jet with surfaces shown as Wireframe
with Show Full enabled, and Simplification level set to 50 pixels. As the model is zoomed out,
the smaller surfaces fall below the 50 pixel threshold, and the display is simplified.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
75
Main Menu Area
Figure 65: Simplifying Geometry Rendering
Select Icon Size
specifies the icon size. You can select Normal, Large, or Huge, as required. The software needs to be
restarted before any change will take effect. If your screen resolution is very high, you may prefer the
Huge setting.
ICON SIZES
Tab
DEZ (Data Entry
Zone)
Normal
24
35
Large
35
35
Huge
35
48
The font size will also change depending on the icon size set and the screen resolution.
76
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
View Fit Percentage
determines the percentage of the screen on which the model will be displayed when the Fit to Screen
option is used. For example, if set to 90, when Fit to Screen is selected, the model will displayed on 90
percent of the total height and width of the screen display. The default of 95% is usually sufficient to
prevent the on-screen prompts from obscuring a portion of the model.
Warn if Elements Displayed
sets the threshold number of elements that will be displayed without a warning. These elements are
displayed according to the Tree Mesh Display settings after the mesh is loaded. The default value is
1000000, and the value 0 will disable the warning completely.
In the case of Tetra Octree mesh, this warning is displayed before the in-process smoothing. If the
specified number is exceeded, a popup window will tell you the number of elements about to be
displayed and ask if you want them to be displayed.
Figure 66: Example of Display Elements Window
Note
If you are generating large numbers of shell elements and do not want to display
them, disable them under Tree Mesh Display.
Float Display Precision
sets the number of decimal places displayed.
Quadratic Accuracy
makes the Bspline display a smoother curve.
Show External Node/Element Numbers
displays the external Node or Element information. Internally, these numbers may be different in order
to optimize the meshing routines, but most users prefer to interact with the external numbers as they
were before being imported into ANSYS ICEM CFD or as they will appear after export. This affects the
behavior of node and element number display, as well as features such as creating a subset from node
numbers.
Show Origin Marker
displays the origin marker on the screen.
Show XYZ Axes
displays the XYZ axes in the bottom right corner. This triad is interactive and clicking on it will orient
the display.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
77
Main Menu Area
Fast Box Selection
enables the “-overlay” option for the selection box. This can increase performance when there are millions
of selected items. Since the memory or accuracy penalty is small, it is recommended that it is enabled
for all models.
Tree Mesh Display
allows you to select the default elements which are displayed when a geometry or mesh is loaded. You
can enable the display of points, lines, shell elements (triangles and quads), and volume elements
(hexahedra, tetrahedra, prisms, and pyramids) as required. On a large model, displaying all the Shells
by default may take too long, so you may want to disable the shell elements. When computing a large
tetra mesh, disabling Show Triangles would prevent the time consuming display of these elements
before and during the in-process smoothing steps.
Speed
The Speed options allow you to modify display modes related to geometry and mesh.
Figure 67: Speed Options window
Fast Dynamics - Geometry
enables a point display mode for the geometry to improve rotational performance.
Fast Dynamics - Mesh
enables a point display mode for the mesh to improve rotational performance.
Threshold (ms)
specifies the length of time between the last input and the time when the display refreshes.
Memory
The Memory options contain features related to the program’s maximum memory parameters.
78
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
Figure 68: Memory Related Features
Max Display List Size (MB)
specifies how much memory is dedicated to making redraws faster.
Max Binary Tetin Size (MB)
specifies the maximum amount of memory that a binary Tetin file can take up. A value of 0 means no
limit.
Max Geometry Memory (MB)
specifies the amount of memory for use by the geometry. A value of 0 is the recommended value since
if this space is exceeded it will not load anything.
Max Mesh Memory (MB)
specifies the amount of memory for use by the mesh. 0 is the recommended value since if this space is
exceeded it will not load anything.
Max Memory for Undo (MB)
specifies the maximum amount of memory that the undo option will take up. A value of 0 means no
limit.
Enable Undo/Redo logging
specifies whether or not to reserve memory for the availability of undo for log messages.
Enable Undo/Redo for Large Operations
specifies whether or not to reserve memory for the availability of undo for larger operations.
Note
Disabling this option also allows a more efficient algorithm (reduced memory usage) for
Linear to Quadratic conversion.
Lighting
The Lighting options allow you to interactively set the direction and different components of the
lighting on entities displayed in solid view.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
79
Main Menu Area
Figure 69: Settings-Lighting DEZ
Ambient
specifies the ambient light setting. The Ambient setting has a range of 0 to 1.
Diffuse
specifies the diffuse light setting. The Diffuse setting has a range of 0 to 1.
Specular
specifies the specular setting. The Specular setting has a range of 0 to 1. For more uniform shading,
lower the specular component.
Shininess
specifies the shininess setting. The Shininess setting has a range of 1 to 10.
Direction
specifies the direction of the lighting as a vector.
Use Two Opposite Lights
enables the use of two opposite lights. For faceted data, the default lighting settings may not be
ideal due to the differing orientations of the surface facets. In such a case, utilizing the Use Two
Opposite Lights option, and lowering the specular component to zero will remove the contrast
and provide more uniform shading.
Restore defaults
restores all lighting settings to their default values.
Background Style
The Background Style options allow you to select the background style and colors.
80
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
Figure 70: Settings-Background DEZ
Background Style
allows you to select a solid background, or one of the following gradients: Top-Bottom, Left-Right, or
Diagonal.
Background Color
specifies the background color selected from the menu of colors. Click the palette icon to open a separate
window with a color map. To select a color from the colormap, move the cross-hairs to the desired color,
and use the sliding arrow on the right to select the desired shade. Click on a blank square under User
colors to make the specified color an option. Click on the desired color square and click Apply to select
it as the background color.
Background Color2
specifies the second background color selected to form gradients along with the first Background Color.
Show ANSYS Logo
enables the use of the ANSYS logo in the graphics window.
Mouse Bindings/Spaceball
The default functions for the mouse buttons and space ball are shown in Figure 71: Default Spaceball
and Mouse Bindings (p. 82). and Table 3: Default Mouse Bindings (p. 82)
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
81
Main Menu Area
Figure 71: Default Spaceball and Mouse Bindings
Table 3: Default Mouse Bindings
Button
Dynamic Mode function
Selection Mode function
Left Button
3D Rotate
Select / DESELECT (with Shift
Key)
Middle Button
Pan
Done selection
Right Button
Zoom / Rotate
Backup / Cancel
Scroll Wheel
Zoom
The Settings>Mouse Bindings/Spaceball DEZ allows you to redefine the dynamic and selection operations of the mouse buttons.
82
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
Figure 72: Settings-Mouse Bindings/Spaceball DEZ
The left, middle, and right mouse buttons all must have different settings.
Wheel Sensitivity
controls the mouse wheel sensitivity.
Mouse wheel for cutplane
enables the manipulation of the cut plane slider with the mouse wheel when a mesh cut plane is enabled.
You may disable this option when working with large meshes, so that accidental scrolling does not cause
the entire volume mesh to be re-rendered.
Zoom in as Moving
allows you to zoom in as you scroll up or down.
The Spaceball option allows you to control the Spaceball check during the ANSYS ICEM CFD startup.
A Spaceball (http://www.3dconnexion.com/) is a 3D mouse that lets you Pan, Zoom and Rotate as if
you are holding the model in your hand, while you use your traditional mouse with your other hand
to Select, Edit, etc. ANSYS ICEM CFD allows simultaneous Dynamic and Selection Mode which can lead
to productivity gains, particularly for new users who will find the Spaceball movement to be more intuitive and consistent across tools.
Start Spaceball at startup
enables the check for a Spaceball during startup. This option is enabled by default. If you do not have
a Spaceball, disable this option for a quicker startup.
Selection
The Selection options allow you to change the default settings related to selection of geometry, mesh,
and blocking.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
83
Main Menu Area
Figure 73: Settings – Selection DEZ
Auto Pick Mode
• initiates the selection process automatically when it is logical to do so.
• activates continuation mode for the middle mouse button (behaves like Apply plus reiterates the
command or proceeds to the next logical selection step.)
Allow Plane Selection
allows the selection tool to snap to planes. When selecting a location on the screen, there is an entity
type-based selection hierarchy within a certain proximity of the cursor. The select location tool will snap
to a point first, then curve, then surface. If no entity types are within a few pixels of the cursor, and Allow
Plane Selection is enabled, it will also snap to the X, Y or Z = 0 planes. This option can also be activated
during selection using the Select location toolbar and enabling Allow any plane selection.
Allow Preview Name
enables the displaying of the entity name while previewing selection in geometry selection operations.
For example, if in curve select mode, preview selection will highlight the curve as well as the curve name.
Minimum Aspect Ratio
sets the lowest quality that elements are allowed to reach during interactive node movement operations.
Wait for Edit Confirmation
requires the confirmation of selected entities using the middle mouse button after all selections have
been made for operations that require a fixed number of selections. If this option is disabled, then the
operations will be carried out and finished once all selections are available.
Cut Delay Threshold
specifies the threshold value for updating the cut plane. If the redraw speed takes longer than the specified
number of milliseconds, the unstructured cut plane will update only when the mouse is released and
not at every stage along its movement.
84
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
Flood Select Angle
controls the selection of elements. You can change the angle if you want to select neighboring elements
with the selection.
Remote
The Remote option allows you to run the program on a remote machine. For this, you need to map
the remote machine with the proper settings in the Settings-Remote DEZ.
Figure 74: Settings—Remote DEZ
Remote Host
specifies the hostname of the remote machine.
Remote User
specifies the user name on the remote machine.
Remote Directory
specifies the directory on the remote machine in which the operation is to be run.
Remote ICEM_ACN
specifies the directory on the remote machine where ANSYS ICEM CFD is installed.
Remote Shell
specifies the type of shell on the remote machine from which the operation will be run.
Model/Units
The Model/Units option allows you to set model preferences.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
85
Main Menu Area
Figure 75: Model/Units Setting Options
Topo Tolerance
specifies the topology tolerance used in operations where topology is automatically calculated.
Restore
resets the topology tolerance to the default value. The default topology tolerance will be set to the
smaller of:
• 0.05% of the bounding box diagonal.
• The value so that no more than 5% of the curves in the model are a length less than 2 * the Topo
Tolerance value.
Triangulation Tolerance
is the distance allowed between the triangle edge and the actual surface edges. ANSYS ICEM CFD triangulates Bspline surfaces and curves when it reads Tetin files. A very low tolerance will give a good representation of the geometry but will require more memory and longer processing time. A higher tolerance
will give good performance and less memory usage but a coarser representation of the geometry.
A coarser geometry representation may be a better choice for a large model that will be coarsely
meshed. For example, a bigger triangulation tolerance would be reasonable for a full engine assembly
model that is going to be shrinkwrapped. If fine precision is required, you may choose a finer triangulation tolerance. For example, some geometry operations, such as trimming a curve with a curved
surface will be affected. Also, users who generate very thin boundary layers on curved surfaces may
have issues if their surface curvature is not being adequately represented.
86
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
An optimal value for most models is 0.001. This setting is independent of the mesh element size.
Note
Triangulation tolerance does not affect faceted geometry.
In the examples below, note that for every 1/10th reduction in the Tri Tolerance, each square of the
surface representation is further divided into 12-16 squares.
Figure 76: Examples of Triangulation Tolerance
Tri Tolerance = 0.1
Tri Tolerance = 0.01
Tri Tolerance = 0.001 (default)
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
87
Main Menu Area
Unitless tolerance
is a factor of the minimum edge length of a given surface or curve. If enabled, the triangulation tolerance
is calculated using this factor for each surface. If disabled, the triangulation tolerance is in actual units.
Length Units
allows you to set the length units in ANSYS ICEM CFD. You can select the appropriate unit from the list.
The default selection is Unitless, where you need to ensure that the intended units are reasonable. In
this case, you can use the Measure Distance (
right scale.
) tool to make sure the model appears to be of the
Note
The units information will be saved to the Tetin file.
Geometry Options
The Geometry Options allow you to set geometry preferences.
Figure 77: Geometry Options
Name new geometry
enables the display of entity names and modification of entity names when creating geometry entities.
If disabled, the entity names will not be visible and the default naming convention will be followed.
Default Naming Convention
If the last two characters of an entity name are digits, then the numbers will be incremented for
each new entity created. If the last two characters are not digits, then new entity names will be
generated by adding “00” to the name and successively incrementing the number. Examples are
shown below.
88
Entity
name
Next Entity Name (Automatically Generated)
abc00
abc01
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
abc.53
abc.54
abc.1
abc.00
abc0.1
abc000
Note
Part names and entity names should be less than 64 alphanumeric characters. Names
should start with a letter, not a digit. Evaluators (i.e., “+”, “-”, “/”, and “*”) should not
be used in names because they can be misinterpreted as expressions or as denoting
an assembly. Part names are written with all upper-case characters. Entity names
are case sensitive.
Replace same name item
enables replacing the previously existing entity when an existing name is used for an entity. If disabled,
then the new entity will automatically be named according to the default naming convention and the
next incremented name will appear in the Name field.
Inherit part name
controls the default behavior of new geometry entities that are created.
• Inherited
specifies that all applicable geometry operations will take the part name from the first object selected. This inherited part name will be used for the new objects that are created.
• Create New
specifies that new geometry objects will be created in the working part name (the part name
defined in the Point, Curve, Surface, Faceted Data, or Repair forms). Some operations, such as
Create Point From Screen, requires a specified working part, so it will take on the working part
name even if the Inherited option is used.
Default Part Name
specifies the default working part for any new geometry created in Point, Curve, Surface, Faceted Data,
or Repair forms. The working part name for a particular project can be changed independent of this
default name.
Create auxiliary points
retains the points used in the creation of geometry.
Create surface topology
creates and maintains the topological connections when geometry is created.
Note
This is currently only used for Create/Modify Surface functions.
Part Table Data
These options apply to the Part Mesh Setup and Edit Attributes tables, with are accessed by rightclicking on the Parts Display Tree.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
89
Main Menu Area
Mesh Setup
opens the Mesh Setup Data dialog with the various options available for the Part Mesh Setup table.
All options are enabled by default.
Attributes
opens the Attributes Data dialog with the various options available for the Edit Attributes table. All
options are enabled by default.
Meshing
The Meshing option allows you to set the preferences for mesh generation. The different meshing
setting options are described in the following sections.
Hexa Meshing
Quality/Histogram Info
Edge Info
Hexa Meshing
The Hexa Meshing option allows you to specify settings for hexa meshes.
Figure 78: Hexa Meshing Options
90
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
Multigrid level
allows you to create a linear multigrid mesh with a specified number of levels. The node count is altered
so that the number of elements on an edge is divisible by 2^M, where M is the number of multigrid
levels. Thus, the new number of nodes will be:

 −

=






+ − 

+





+
where N is the current number of nodes.
You must select Blocking > Pre-Mesh Params > Update Sizes to for the change to take effect on a
blocking with existing node distributions, or set this parameter before prescribing node counts or
element sizes.
Projection limit
controls the projection of nodes. If the Projection limit is set to a non-zero value, P, the nodes along an
edge within distance P of the end of the edge will not be projected. Instead, they will be linearly interpolated between the first point farther than P and the end. Nodes on the interior of a face within distance
P of the edge of the face will not be projected. Instead, they will be linearly interpolated from the interior
of the face. If the Projection limit is set to 0, all nodes will be projected.
The Projection limit is set to a non-zero value in cases where you want to keep the nodes on the
edges and avoid projection to the underlying surfaces. This option is typically used for Navier-Stokes
grids where the grid spacing is small relative to the geometry tolerance. Allowing nodes within a
gap in the geometry to project would skew the elements. With a value P set to slightly larger than
the gap, the nodes would instead be interpolated. The value may have to be set by trial and error
depending on skewness or negative determinants being reported by pre-mesh quality checks.
Default meshing law
specifies the default meshing law used for node distributions for edges. Edges which have a meshing
law set will retain their current law unless Blocking > Pre-Mesh Params > Update Sizes is applied.
Default bunching ratio
specifies the default node expansion ratio along an edge from either end of the edge.
Note
Though the settings are saved in the .aienv_options file, some settings such as the
bunching ratio and the meshing law may also be saved in the blocking file. If a blocking
file is loaded, it will override the settings saved in the settings file.
Find Worst Blocks (range)
specifies the range of Worst Blocks displayed by the Find Worst blocks option.
Ogrid Smooth Transition
provides a smooth transition from the offset layer to interior layers. This option uses transfinite interpolation to prevent intermediate unprojected Ogrid splits from adversely affecting the smoothness of the
mesh.
In the following figure, the cyan-colored Ogrid edge split, between the outer perimeter and the
inner square, is not shaped for optimal mesh quality.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
91
Main Menu Area
Figure 79: Ogrid Not Interpolated
This second figure shows the central Hgrid portion and the Ogrid split has been interpolated (shaped)
to more smoothly transition the mesh across the model.
Figure 80: Ogrid, interpolated
Floating grid
is used when grid distribution on faces is independent of the sub-edge structure. It also helps to turn
on this option if a series of block splits have been made where the splits do not extend through the
whole topology. With this option, subsequent splits would not "connect" to previous non-extended
splits.
Project to Bsplines
projects the mesh to the true Bspline geometry rather than the faceted representation, which is the internal triangulated representation of surface data as defined by Settings > Model > Triangulation Tolerance.
This can be used instead of decreasing the tri-tolerance or using projection limit, where small gaps in
the faceted representation create skewed elements on a Navier-Stokes grid. This, however, takes longer
and more memory to compute the pre-mesh.
Check/Fix Blocks
checks the internal block data structures for inconsistencies and fixes them if possible.
Check/Fix Inverted Blocks
checks for all the inverted (left-handed) blocks and redefines the block by reordering the vertices to
make it right-handed.
Write 7-node-hexas as pyramids
when enabled (by default this option is disabled), converts degenerate 7-noded-hexas (2 nodes merged
along an edge) into two pyramids when you select the Convert to Unstruct Mesh option under
Blocking > Pre-Mesh in the Model tree or when using the File > Blocking > Save Unstructured Mesh
option.
92
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
Verbose mode
displays additional minor warning messages that are intended to aid development or support in diagnosing possible problems that may occur. This option is disabled by default, but warnings intended to help
the user with errors or problems are always displayed.
Update options from current blocking
when enabled, this option allows the previously saved hexa settings to be overwritten by the settings
from the currently loaded blocking file. When disabled, the previously saved hexa settings will be retained
and the settings in the currently loaded file will be ignored. This option is enabled by default.
Transfinite degree
Transfinite interpolation is used for face interpolation when computing a mesh. The default is linear but
quadratic is better for maintaining initial element heights. The drawback is that it can produce inverted
elements in bowtie-shaped blocks where linear would work fine.
Reference topology
specifies the name of another blocking (the basis for the smoothed mesh) that you have loaded in
the same session. If you generate an Euler mesh and the run the mesh smoother on it you can read
that mesh back into hexa and create a different blocking that, for instance has Navier Stokes spacing.
If the NS blocking references the Euler blocking then it will follow the shape of the smoothed Euler
elements to give you a smooth mesh but with the NS spacing.
Unstruct face mesh type
specifies the default mesh type that will be used for meshing unstructured 2D surface blocking. The
following options are available:
• Quad w/one Tri
• Tri (STL like)
• All Tri
• All Quad
• Quad Dominant
What to Mesh
specifies the entities or blocks to mesh for Blocking Tree > Pre-Mesh. Used typically for blocks with
a mixture of mapped (structured), swept, and free (fully unstructured) 3D blocks as encountered
using Multizone techniques.
All Blocks
will mesh all blocks. This is the default. Any unstructured (free) blocks will be filled with tetras
using the Delaunay algorithm which could take some time for large volumes such as in external
flow models.
Vertices
not used.
Edges
will mesh only edges to create line elements.
Faces
will mesh only faces and edges to create surface mesh.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
93
Main Menu Area
Struct & Swept Blocks
will mesh mapped (structured) and swept blocks, but not free (unstructured) blocks.
Note
This option can be used with multizone blocking to more efficiently iterate and
improve the surface mesh and boundary layers. The All Blocks option can then
be used to mesh the unstructured regions also.
Number of Tetra Smoothing steps
specifies the number of Tetra smoothing steps for Multizone unstructured blocks. You may want to
lower this during early iterations of Multizone blocks in order to save time.
Restore Hexa Defaults
restores the hexa meshing settings to the defaults.
Quality/Histogram Info
The Quality/Histogram Info option allows you to specify settings for displaying information regarding
quality criteria that will be reported for Element Info under the Info menu. You can also set the default
settings for the histogram display that will be used by the Pre-Mesh Quality histogram and the Quality
Metric histogram.
94
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
Figure 81: Settings-Quality
Check Quality
allows you to select the quality metrics that will be reported for Element Info under the Info menu. The
default is set to report the Quality metric only. For the descriptions of the quality metrics, see Edit Mesh
> Display Mesh Quality.
Histogram Defaults
allows you to select the settings for the histogram display.
Note
You can also change the histogram display settings (and ranges) by right-clicking in the
histogram window.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
95
Main Menu Area
Show
displays the elements within the selected (highlighted) histogram bars.
Solid
displays all selected elements in solid view.
Note
This option may slow down the display speed.
Color by Quality
displays the histogram by colors that corresponds to the quality range. The color contour bar will
display the range of quality by color.
Evaluation at
specifies the nodes for which the determinants and distortion will be evaluated for hexa and quad elements. This is used for linear as well as quadratic elements.
• Corner Nodes
The Jacobian determinants of a volume element will be calculated at r = -1, 0, 1; s = -1, 0, 1; t =
-1, 0, 1 (natural coordinate system).
• Gauss Points
The determinants will be calculated at the Gauss points of the selected order.
Edge Info
The Edge Info option allows you to specify settings for displaying information regarding edges.
Figure 82: Settings-Edge Info
Calculate min / max mesh edge sides
enables the calculation and display of maximum and minimum distances between nodes of a mesh in
the information given for Info > Mesh Info.
Solver
The Solver option opens a DEZ to select an Output Solver (CFD) or Common Structural Solver (FEA).
96
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Settings Menu
Figure 83: Select Solver DEZ
Output Solver
Select an Output Solver from the drop-down list.
More information about the ANSYS ICEM CFD Output Interfaces is available from the Help menu.
Select the Output Interfaces option to open a browser window containing the ANSYS ICEM CFD
Output Interfaces information. Select the name of an interface in the Table of Supported Solvers
for more detail about that specific interface.
Common Structural Solver
select a Common Structural Solver from the drop-down list. The following options are available:
• Nastran
• ANSYS
• LS-DYNA
• Abaqus
• Autodyn
Additional setup for your specific model is done from the Solve Options tab.
Set As Default
sets the current selection as the default solver.
Reset
The Reset option allows you to reset the project settings to the defaults. Click Yes in the Settings
dialog to reset Project settings to the default. This will overwrite the user settings done in the project.
Figure 84: Reset Options Dialog
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
97
Main Menu Area
Help Menu
The Help menu provides access to different sections of the ANSYS ICEM CFD Documentation via the
ANSYS Help Viewer. On selecting the desired option, the Help Viewer will open at the first page of the
selected document.
Help Topics
Tutorial Manual
User’s Manual
Programmer’s Guide
Output Interfaces
Installation & Licensing Guide
What's New
Show Customer Number
About ANSYS ICEM CFD
Figure 85: Help Options
Help Topics
The Help Topics option opens the ANSYS ICEM CFD Help Manual, which contains descriptions of all
the features available in ANSYS ICEM CFD.
Tutorial Manual
The Tutorial Manual option opens the ANSYS ICEM CFD Tutorial Manual, which contains several textbased tutorial examples.
Additional tutorials and other supporting documents are available on the ANSYS Customer Portal. To
access tutorials and their input files on the ANSYS Customer Portal, go to http://support.ansys.com/
training. You will require a Show Customer Number (p. 99) to access the Customer Portal
User’s Manual
The User’s Manual option opens the ANSYS ICEM CFD User's Manual, which offers a more technical
description of many of the features available in ANSYS ICEM CFD.
Programmer’s Guide
The Programmer's Guide option takes you to the ANSYS ICEM CFD Programmer's Guide Table of
Contents.
98
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Graphical Main Menu, Utilities and Display Options
ANSYS ICEM CFD is fully scriptable (in Tcl/Tk) and taking advantage of this is an excellent way to compress
your process and use the tools more efficiently. The Programmer's Guide includes:
• ANSYS ICEM CFD scripting basics
• Form creation functions for manipulating the GUI
• External commands for running external programs or performing operations at the OS level
• Scripting commands for use in ANSYS ICEM CFD
• Blocking commands for use in ANSYS ICEM CFD Hexa blocking
• Meshing Directives providing additional scripting commands for use with ANSYS ICEM CFD Meshing,
Editing, etc.
Output Interfaces
The Output Interfaces option opens the ANSYS ICEM CFD Output Interfaces information in a browser.
For information about a specific interface, refer to the Table of Supported Solvers and click the name
of the interface.
Installation & Licensing Guide
The Installation & Licensing Guide option describes Installation processes and Licensing requirements
for ANSYS ICEM CFD.
What's New
The What's New option opens the list of additions and improvements to the current release of ANSYS
ICEM CFD.
Show Customer Number
The Show Customer Number option shows your Customer Number that is included in the license file.
The Customer Number is needed to access the Customer Portal.
Note
Reference the Customer Number when contacting ANSYS ICEM CFD Technical Support
by phone (1-800-937-3321) or by email ([email protected]).
About ANSYS ICEM CFD
The About ANSYS ICEM CFD option gives information about the version and release date of ANSYS
ICEM CFD.
Graphical Main Menu, Utilities and Display Options
Some of the most frequently used functions are made available for quick access in the Figure 86: Graphical Main Menu (p. 100).
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
99
Main Menu Area
Figure 86: Graphical Main Menu
The Main Menu icons include options to manage your Project, Geometry, Mesh or Blocking files.
They function exactly as the equivalent text based menus.
Utilities for taking measurements of your project’s features or defining a Local Coordinate system are
available along with Undo and Redo.
Display management options include sizing, zooming, and drawing style.
Main Menu Icons
Utilities Icons
Display Management Icons
Main Menu Icons
The Main Menu icons include options to manage your Project, Geometry, Mesh or Blocking files.
They function exactly as the equivalent text based menus.
Figure 87: Main Menu Icons
Open Project
To work on an existing project, select the Open Project option.
Navigate to the working folder and select the desired project from the Open Project window; or
select an existing project from the drop down list in the File name field.
Save Project
To update the project file (*.prj) on your disk, select the Save Project option.
This option also updates and saves the data files associated with the project. The files saved are
the Geometry file (*.tin), Mesh file (*.uns), Blocking file (*.blk), Parameters file (*.par) and
Attributes files (*.fbc and *.atr).
Geometry Menu
The Geometry drop-down menu contains options to Open, Save, and Close your Geometry file:
100
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Graphical Main Menu, Utilities and Display Options
Open Geometry
To load a geometry file into memory and display its graphical image, select the Open Geometry
icon.
Save Geometry
To update the geometry file with all your recent work, select the Save Geometry icon.
Close Geometry
To remove the geometry information from the graphical display and close the loaded geometry
file, select the Close Geometry icon. If the file has been modified, you will be asked whether you
want to save the file.
Mesh Menu
The Mesh drop-down menu contains options to Open, Save, and Close your Mesh file:
Open Mesh
To load a mesh file into memory and display its graphical image, select the Open Mesh icon.
Save Mesh
To update the mesh file with all your recent work, select the Save Mesh icon.
Close Mesh
To remove the mesh information from the graphical display and close the loaded mesh file, select
the Close Mesh icon. If the file has been modified, you will be asked whether you want to save the
file.
Blocking Menu
The Blocking drop-down menu contains options to Open, Save, and Close your Blocking file:
Open Blocking
To load a blocking file into memory and display its graphical image, select the Open Blocking
icon.
Save Blocking
To update the blocking file with all your recent work, select the Save Blocking icon.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
101
Main Menu Area
Close Blocking
To remove the blocking information from the graphical display and close the loaded blocking
file, select the Close Blocking icon. If the file has been modified, you will be asked whether you
want to save the file.
Utilities Icons
Utilities for taking measurements of your project’s features or defining a Local Coordinate system are
available along with Undo and Redo.
Measurement Menu
The Measurement drop-down menu contains options to measure distance or angle, or to find the
xyz coordinates of a location in the graphical display:
Measure Distance
To measure the distance between two points in the graphical display, use the Measure Distance
option. Select the locations with the left mouse button. The distance between the two points will
be displayed in the message window.
Measure Angle
To measure the angle between two intersecting vectors, use the Measure Angle option. Select
three points in the graphical display. The first location is at the point of intersection, and the second
and third locations define the two different vectors as shown in Figure 88: Pixel Sequence to Measure
Angle (p. 102). The angle between these two vectors will be reported in the message window.
Figure 88: Pixel Sequence to Measure Angle
Find Location
To find the xyz coordinates of a point in the graphical display, use the Find Location option.
Select a pixel with the left mouse button. The location of the point in space will be displayed in the
message window and in the GUI.
102
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Graphical Main Menu, Utilities and Display Options
Local Coordinate Systems
You can define local coordinate systems (LCS) for use in geometry, mesh, blocking or boundary
condition manipulation. The default coordinate system located at the origin is called Global.
Note
LCS information is saved in both geometry (.tin) and parameter (.par) files. If the
geometry is closed, the LCS data will also be closed if only the geometry was loaded.
However, if mesh, blocking, boundary conditions, or loads are also loaded, the LCS data
will not be removed when the geometry is closed and/or replaced. This will ensure that
the LCS info remains in the case that other entities such as mesh, blocking, boundary
conditions, or loads are defined in relation to the LCS.
Figure 89: Define Local Coordinate System DEZ
Name
specifies the name for the local coordinate system (LCS). You can define as many systems as you
wish.
Number
is used by output interfaces to signify a solver's LCS number.
Reference
specifies the reference coordinate system which is the basis for the new coordinate system.
Type
specifies the coordinate system type. The LCS Type can be Rectangular (Cartesian), Cylindrical, or
Spherical. A Rectangular LCS has X, Y, and Z axes. A Cylindrical LCS has R, θ, and Z coordinates. A
Spherical LCS has R, θ, and Φ coordinates.
Defined by
specifies the method used to define the LCS. The following methods are available:
Defined by 3 points
In this method, the first point defines the origin of the LCS. The second point defines the positive
Z axis relative to the origin for rectangular and cylindrical coordinate systems, and the θ axis (Φ
= 0) for spherical coordinate systems. The third point defines positive X for Cartesian coordinate
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
103
Main Menu Area
systems, and θ = 0 for cylindrical and spherical coordinate systems. This vector is ortho-normalized
if the selected third point is not 90 degrees relative to the first two. Points can be selected by
clicking on a graphic location, or by clicking on a prescribed (pre-existing) point.
Defined by 1 point
The current screen view plane defines the orientation. The selected point defines the origin. The
vector normal out of the screen defines the positive Z axis (Cartesian and cylindrical) or Φ = 0
(spherical). The horizontal direction to the right defines the positive X axis (Cartesian) or θ = 0
(cylindrical and spherical). The vertical direction upward describes the positive Y axis (Cartesian)
or θ = 90 (cylindrical and spherical). Points can be selected by clicking on a graphic location, or
by clicking on a prescribed (pre-existing) point.
Click Apply to create and activate the LCS. A triad showing the coordinate system axes will be displayed in the screen at the point of origin. The Global coordinate system is always displayed in the
lower right hand corner (not at the origin). The defined LCS will also appear in the Display Tree.
For more information on options to modify Local Coordinate Systems using the Display Tree, see
Display Tree > Local Coordinate Systems.
Refresh / Recompute
The Refresh/Recompute drop-down menu contains two options:
Refresh
The Refresh option allows you to refresh the screen.
Recompute Premesh
The Recompute Premesh option allows you to recompute the mesh.
Undo
The Undo option reverses (undoes) the most recently performed operation.
Redo
The Redo option repeats the previously reversed operation.
Display Management Icons
Display management options include sizing, zooming, and drawing style.
WireFrame Display Options
104
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Graphical Main Menu, Utilities and Display Options
The WireFrame Display Options drop-down menu contains the following options:
WireFrame Simple Display
The WireFrame Simple Display option allows you to display wireframe representation of CAD
data or a "Hard Feature" representation of triangulated surface data, including surface boundaries
as hard features.
WireFrame Full Display
The WireFrame Full Display option allows you to display a more detailed representation of the
CAD data, showing more isobars than in the simple representation. For triangulated surface data, a
detailed representation will show all the surface triangles.
SolidFrame Display Options
The SolidFrame Display Options drop-down menu contains the following options:
Solid Simple Display
The Solid Simple Display option allows you to display a smooth or flat shaded representation
of surfaces, which is simplified for parametric surfaces.
Solid Full Display
The Solid Full Display option allows you to display a smooth shaded representation of surfaces
which are triangulated in details.
Solid Full Flat Display
The Solid Full Flat Display option allows you to display a flat shaded representation of surfaces
which are triangulated in details.
Solid/Wire Full Display
The Solid/Wire Full Display option allows you to display a wireframe over a smooth or flat
shaded representation of surfaces which are triangulated in details.
Fit Window
The Fit Window option scales the model so that it fits in the GUI.
Box Zoom
The Box Zoom option prompts you to select a region on GUI to zoom in to.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
105
106
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Selecting Entities, Keyboard and Mouse Functions
ANSYS ICEM CFD offers several ways of interacting with your model, including context-sensitive hotkeys
and mouse functions.
Selection options, hotkeys, and mouse functions that are appropriate for a given mode (Selection or
Dynamic) and Function tab are presented in this chapter.
Selection Options
Hotkeys
Spaceball and Mouse Binding
Selection Options
In ICEM CFD, you may select locations or graphical entities (geometry, mesh, blocking, nodes, and so
on) in multiple ways. Common methods are point/click, drawing a surrounding figure, or selecting from
a list (name or other identifier). Most selection options are shown in the Selection Mode Keymap
graphic and supporting table.
Not all selection options are available in all contexts. Available Selection options for each context are
presented in a pop-up toolbar in that context. Some selection options appear on the toolbar for only
one specific context, although many appear in multiple contexts. Descriptions of the various Selection
toolbars follow.
Selection Mode Keymap
Location Selection Toolbar
Geometry Selection Toolbar
Mesh Selection Toolbar
Blocking Selection Toolbars
Density Selection Toolbar
Selection Mode Keymap
Figure 90: Selection Mode Hotkeys (p. 108) and its associated table lists most of the Selection mode
functions in ICEM CFD. In any given context, a subset of these will be available, and will be indicated
in a pop-up Selection toolbar.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
107
Selecting Entities, Keyboard and Mouse Functions
Figure 90: Selection Mode Hotkeys
Hotkey function
SHIFT + Hotkey function
Select all appropriate objects
a
Objects may be visible or blanked
Useful for selecting a large number
of objects
b
Select all appropriate blanked objects
Select items in a circular region
c
Click (center point) and drag (radius) to define the selection region.
Toggle select diagonal corner vertices
d
In certain Blocking selection contexts, this allows you to select
multiple, contiguous blocks by
clicking two diagonally opposite
vertices.
Select elements by numbers
e
In certain Mesh selection contexts,
this opens a dialog box to specify
a range of ID numbers.
Set feature angle for flood fill
g
108
Opens a dialog box to set the
maximum angle at which attached
items are selected. This applies to
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Selection Options
Hotkey function
SHIFT + Hotkey function
certain selection functions that allow you to start with one item, and
quickly select all attached.
If feature angle is set to zero, all
attached, appropriate items will be
selected.
Toggle between all edges and highlighted edges
h
Highlighting of Specific edges may
be determined in many ways. For
example, selecting Show Single in
the Curves Display tree.
Select a path in between two selected
nodes
Preselect two or more, non-contiguous, faceted edges on a faceted
surface, and then use this option
to select all the edges between
them.
i
or
k
l
Split two edges and flood fill in
between them
This is useful if the edge section
you want to select is not clearly
delineated into facets.
Select one attached layer
Selects items immediately adjacent
to the current selection, within the
feature angle limit.
or
Select all items attached to current selection
Selects all attached items, within
the feature angle limit.
Select items by Material
Toggle between full and partial enclosure
m
Used in mesh selection contexts,
Materials must be defined and associated with parts.
Determines whether objects must
be fully or partially within the selection area to be included.
n
OR
Select the next item picked
Select by numbers
Cyclically steps through all appropriate objects. Accept with middle
mouse button.
In certain Blocking selection contexts, a dialog box is opened to
accept a numeric identifier.
OR
Select by name
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
109
Selecting Entities, Keyboard and Mouse Functions
Hotkey function
Select next edge segment
In certain Blocking edge selection
contexts, this helps to select a
piecewise continuous edge, rather
than clicking on individual segments.
SHIFT + Hotkey function
In Geometry and Density selection
contexts, a dialog box is opened to
accept an alphanumeric identifier.
Toggle boundary type
o
p
Active only in (Geometry) Surface
or (Blocking) Face selection contexts.
Toggles between ON: selecting all
surfaces, or faces, regardless of the
boundary (inner and outer), and
OFF: only the outer boundary surfaces, or faces, will be selected.
ON/OFF status is applicable to any
surface, or face, selection tool.
Select items in a polygonal region
Select items in a part
Use the left mouse button to select
multiple points until the polygon
is created.
Middle button completes the selection and closes the polygon.
Right button cancels points.
After selection, entities may be individually de-selected from the list.
A dialog box is opened listing all
appropriate parts
Check the box to select a part.
Select all items attached to current selection, up to a curve
r
In surface mesh selection context,
all attached elements within the
feature angle limit and constrained
by the nearest curve are selected.
Select elements by Property
Used in mesh selection contexts,
Properties must be defined and
associated with parts.
Select items in a subset
s
A dialog box opens listing all appropriate subsets from which to
choose.
Select mesh attached to geometry
t
110
Selects the mesh associated with
the selected geometry.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Selection Options
Hotkey function
Select all appropriate visible objects
v
SHIFT + Hotkey function
Select block by vertex
Enter vertex numbers in the popup dialog box.
x
Cancel selection mode.
0
Select all node elements
1
Select all line elements
Select all surface elements
2
A drop down list offers the opportunity to choose which surface element types.
Select all volume elements
A drop down list offers the opportunity to choose which volume element types.
3
[
Undo selection. This is the same as clicking the right mouse button.
]
Accept selection. This is the same as clicking the middle mouse button.
Toggle Dynamics
F9
Switch to Dynamic mode to reorient the model in the Graphics window, back to
Selection mode to complete your selection.
The same response is achieved by holding down the Ctrl key.
?
Print hotkey list (message window)
Location Selection Toolbar
When in Select Location mode the toolbar shown in Figure 91: Select Location Toolbar (p. 111) pops
up showing the Select location options.
Figure 91: Select Location Toolbar
The first two icons are selection mode functions as described in Selection Mode Keymap (p. 107):
•
Toggle Dynamics
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
111
Selecting Entities, Keyboard and Mouse Functions
•
Cancel selection
In addition to the common functions, there are several functions specific to the Select location context:
•
Toggle allow any plane selection (key = 1)
If toggled ON, a location on any plane can be selected.
•
Toggle allow on XY plane selection (key = 2)
If toggled ON, it allows you to select a location on the XY plane.
•
Toggle allow on XZ plane selection (key = 3)
If toggled ON, it allows you to select a location on the XZ plane.
•
Toggle allow on YZ plane selection (key = 4)
If toggled ON, it allows you to select a location on the YZ plane.
•
Toggle allow on Mesh/Block selection (key = 5)
Toggles between allowing you to select a location on Mesh elements or a location on Blocking.
Note
It may be easier to select mesh nodes if you disable Toggle allow any plane selection.
•
Toggle show location (key = 6)
Toggles the display of the selection location coordinates.
•
Toggle show entity name (key = 7)
Toggles the display of the selected entity's name.
•
Toggle highlight entity (key = 8)
Toggles the highlighting of the selected entity.
Geometry Selection Toolbar
When in Select geometry mode the toolbar shown in Figure 92: Select Geometry Toolbar (p. 112) pops
up showing the Select geometry options.
Figure 92: Select Geometry Toolbar
112
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Selection Options
Many of these icons invoke selection mode functions as described in Selection Mode Keymap (p. 107):
•
Toggle Dynamics
•
Select items in a polygonal region
•
Select all appropriate objects
•
Select all appropriate visible objects
•
Select all appropriate blanked objects
•
Cancel selection
•
Toggle between full and partial enclosure
•
Select the next item picked
•
Toggle between all edges and highlighted edges
•
Select all items attached to current selection
•
Select one attached layer
•
Set feature angle for flood fill
•
Toggle boundary type
•
Select items in a subset
•
Select items in a part
•
Select by name
In addition to the common functions, there are several functions specific to the Select geometry context:
•
Toggle preselect highlight and name
Allows geometry entities to be highlighted and their names to display before you select them. Enable
Preview Name must be enabled in the Selection menu to see the name.
•
Toggle selection of points
If toggled ON, points can be selected.
•
Toggle selection of curves
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
113
Selecting Entities, Keyboard and Mouse Functions
If toggled ON, curves can be selected.
•
Toggle selection of surfaces
If toggled ON, surfaces can be selected.
•
Toggle selection of bodies
If toggled ON, bodies can be selected.
•
Toggle selection of mesh
If toggled ON, the mesh selection toolbar will appear and mesh elements can be selected.
Segment Selection Toolbar
The Select segments toolbar appears when the context requires selection of faceted edges. The Select
segments options are described below.
Figure 93: Select Segments Toolbar
All of the icons invoke selection mode functions as described in Selection Mode Keymap (p. 107):
•
Toggle Dynamics
•
Select items in a polygonal region
•
Cancel selection
•
Toggle between full and partial enclosure
•
Select all items attached to current selection
•
Select one attached layer
•
Select a path in between two selected nodes
•
Split two edges and flood fill in between them
•
Set feature angle for flood fill
Mesh Selection Toolbar
When in Select mesh elements mode the toolbar shown in Figure 94: Select Mesh Toolbar (p. 115) pops
up showing the Select mesh elements options.
114
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Selection Options
Figure 94: Select Mesh Toolbar
All except the last of these icons invoke selection mode functions as described in Selection Mode
Keymap (p. 107):
•
Toggle Dynamics
•
Select items in a polygonal region
•
Select items in a circular region
•
Select all appropriate objects
•
Select all appropriate visible objects
•
Select all appropriate blanked objects
•
Cancel selection
•
Toggle between full and partial enclosure
•
Select all items attached to current selection
•
Select all items attached to current selection, up to a curve
•
Select one attached layer
•
Set feature angle for flood fill
•
Select items in a subset
•
Select items in a part
•
Select elements by numbers
•
Select items by Material
•
Select items by Property
•
Select mesh attached to geometry
•
Select all node elements
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
115
Selecting Entities, Keyboard and Mouse Functions
•
Select all line elements
•
Select all surface elements
•
Select all volume elements
In addition to the common functions, the last icon invokes a function specific to the Select mesh elements context:
•
Toggle selection of geometry
If toggled ON, the geometry selection toolbar will appear and geometry entities can be selected. This
option is available when geometry or mesh selection would be applicable.
Blocking Selection Toolbars
When selecting blocking, you may be required to select Blocks, Faces, Edges, Compcurves, or Vertices.
Each of these has its own toolbar with its specific selection options.
Select Blocking - block
Figure 95: Select Blocking Block Toolbar
All of these icons invoke selection mode functions as described in Selection Mode Keymap (p. 107):
•
Toggle Dynamics
•
Select items in a polygonal region
•
Select items in a circular region
•
Select all appropriate visible objects
•
Select all appropriate blanked objects
•
Cancel selection
•
Toggle between full and partial enclosure
•
Select block by vertex
•
Select items in a subset
•
Select items in a part
116
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Selection Options
•
Select by numbers
•
Toggle select diagonal corner vertices
Select Blocking - face
Figure 96: Select Blocking Face Toolbar
All of these icons invoke selection mode functions as described in Selection Mode Keymap (p. 107):
•
Toggle Dynamics
•
Select items in a polygonal region
•
Select items in a circular region
•
Select all appropriate visible objects
•
Cancel selection
•
Toggle between full and partial enclosure
•
Toggle between all faces and boundary faces
•
Select items in a subset
•
Select items in a part
•
Toggle select diagonal corner vertices
Select Blocking - edge
Figure 97: Select Blocking Edge Toolbar
All of these icons invoke selection mode functions as described in Selection Mode Keymap (p. 107):
•
Toggle Dynamics
•
Select items in a polygonal region
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
117
Selecting Entities, Keyboard and Mouse Functions
•
Select items in a circular region
•
Select all appropriate visible objects
•
Cancel selection
•
Toggle between full and partial enclosure
•
Select next edge segment
•
Select items in a subset
•
Select items in a part
Select Blocking - compcurve
Figure 98: Select Blocking Compcurve Toolbar
All of these icons invoke selection mode functions as described in Selection Mode Keymap (p. 107):
•
Toggle Dynamics
•
Select items in a polygonal region
•
Select items in a circular region
•
Select all appropriate visible objects
•
Cancel selection
•
Toggle between full and partial enclosure
•
Select items in a subset
•
Select items in a part
•
Select by numbers
118
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Selection Options
Select Blocking - vertex
Figure 99: Select Blocking Vertex Toolbar
All of these icons invoke selection mode functions as described in Selection Mode Keymap (p. 107):
•
Toggle Dynamics
•
Select items in a polygonal region
•
Select items in a circular region
•
Select all appropriate visible objects
•
Cancel selection
•
Toggle between full and partial enclosure
•
Select items in a subset
•
Select items in a part
•
Select by numbers
Density Selection Toolbar
When working with Density regions, the toolbar shown in Figure 100: Select Densities Toolbar (p. 119)
pops up showing the Select densities options.
Figure 100: Select Densities Toolbar
Note
The Select densities toolbar has fewer options than other entity selections. For example,
the Enclosure toggle (
) is not available because only the partial enclosure mode is available.
All of these icons invoke selection mode functions as described in Selection Mode Keymap (p. 107):
•
Toggle Dynamics
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
119
Selecting Entities, Keyboard and Mouse Functions
•
Select items in a polygonal region
•
Select all appropriate objects
•
Select all appropriate visible objects
•
Select all appropriate blanked objects
•
Cancel selection
•
Select the next item picked
•
Select by name
Hotkeys
Many of the most frequently used commands in ANSYS ICEM CFD are accessible via single or combination
keystrokes. Many of these hotkeys are common across all contexts while others are specific to the active
function group – Geometry, Blocking, or Edit Mesh. To access any hotkeys related to geometry, mesh,
blocking operations, you must first go to the respective tab.
Note
Make sure that the Caps Lock is not toggled ON when using hotkeys.
Hotkeys work only when the cursor is in the graphics display area.
Hotkeys which are available in any context are shown in the following image and table.
Figure 101: Common Hotkeys
F1
Open online help
F4
Emergency Reset
Note
Emergency Reset is useful if a series of random keystrokes accidentally locks the
keyboard. If a user clicks too fast or bumps multiple keys at a time the keyboard
may lock up. The Emergency reset attempts to fix this problem and unlock the
keyboard.
F5
Set wireframe offset
F6
Set wireframe offset to 0
120
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Hotkeys
F7
Increment wireframe offset
F8
Decrement wireframe offset
Note
The Wireframe Offset Display controls allow you to optimize the wireframe display
for solid and wireframe modes. This can be useful when the wireframe display is
difficult to see in contrast to the solid display. For example, if the wireframe offset
is set too high you can see overlapping lines, if it is set too low, the wireframe
lines look dim. This can happen when adjusting the zoom, or if the model dimensions make the wireframe offset difficult to compute automatically. When generating images of the mesh it is recommended to increase the wireframe offset
slightly to ensure better crispness of solid/wireframe mesh display. Increasing the
wireframe display makes the wireframe lines larger and clearer, but it can also
bring lines in the background to the foreground. The default Wireframe offset (Zoffset) tries to automatically set the wireframe value based on the model dimensions.
F10
Save Project
F11
Emergency Reset
F12
Save hardcopy
Apply
Note
Enter
Pressing the Enter key after typing in a field in the GUI is the same as
clicking on the Apply button.
Geometry
In addition to the common hotkeys listed above, the hotkeys shown in the following image and table
are available only when working with the Geometry tab functions.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
121
Selecting Entities, Keyboard and Mouse Functions
Figure 102: Geometry Hotkeys
Hotkey function
Ctrl + Hotkey function
a
Concatenate curves
Merge surfaces
b
Build diagnostic topology
c
Create curve
d
Delete geometry entities
Delete geometry permanently
e
Extend surface
Create curtain surface
f
Faceted tools
Move facets to new
g
Concatenate curves
Split curve
h
Home position
i
Toggle solid display
m
Move geometry
o
Offset surface
p
Project point to curve
Project curve to surface
?
122
Project point to surface
Reverse view
Split curve
Extend split
Scale to fit
y
z
Stitch/match edges
Copy geometry
r
x
Create surface
Isometric view
j
s
SHIFT + Hotkey function
Zoom in
View in x-direction (right
side)
Redo last undone operation
View in y-direction (top
view)
Undo last operation
View in z-direction (front
view)
Print hotkey list (message
window)
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Hotkeys
Blocking
In addition to the common hotkeys listed above, the hotkeys shown in the following image and table
are available only when working with the Blocking tab functions.
Figure 103: Blocking Hotkeys
a
Hotkey function
Ctrl + Hotkey function
SHIFT + Hotkey function
Merge vertices
Merge vertices with propogation
Merge blocks
Initialize blocks
Create blocks from vertices
c
d
Delete blocks
Delete blocks permanently
e
Split edge
Unsplit edge
f
Associate face to surface
Fix inverted blocks
g
Group curves
Ungroup curves
h
Home position
i
Index control
j
Toggle solid display
Restrict blocks – corners
k
Isometric view
Change block IJK
l
Align vertices
Set vertex location
m
Move vertex
Move multiple vertices
Set edge mesh parameters
Match edges for node distribu- Scale sizes
tion
o
Create O-grid
Rescale O-grid
p
Project edge to curve
Project edge to surface
q
Check Quality – determinant Check Quality – aspect ratio
Check Quality – angle
r
Recompute pre-mesh
Reset index control
Reverse view
s
Split block
Extend split
n
Set edge length
Project vertex to point
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
123
Selecting Entities, Keyboard and Mouse Functions
Hotkey function
u
Update Mesh sizes
v
Snap selected vertices
x
SHIFT + Hotkey function
Snap visible vertices
Scale to fit
View in x-direction (right
side)
y
z
Ctrl + Hotkey function
Zoom in
Redo last undone operation
View in y-direction (top
view)
Undo last operation
View in z-direction (front
view)
Print hotkey list (message
window)
?
Edit Mesh
In addition to the common hotkeys listed above, the hotkeys shown in the following image and table
are available only when working with the Edit Mesh tab functions.
Figure 104: Edit Mesh Hotkeys
Hotkey function
Ctrl + Hotkey function
a
Merge nodes without propogation
Merge nodes with propogation
b
Build mesh topology
c
Create element
d
Delete mesh elements
e
Mesh from edges
h
Home position
i
j
124
SHIFT + Hotkey function
Mesh diagnostics
Isometric view
Toggle solid display
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Spaceball and Mouse Binding
Hotkey function
Ctrl + Hotkey function
m
Move node
Move multiple nodes
p
Project node to curve
Project node to surface
q
Quality metrics, custom
quality
Smooth mesh globally
r
Remesh elements
Remesh bad elements
s
Split edges without propog- Split edges with propogation
ation
t
Convert Tri to Quad, quadriz- Convert Quad to Tri
ation OFF
v
Snap by current projection
w
Swap edges
x
Scale to fit
y
z
Zoom in
SHIFT + Hotkey function
Project node to point
Reverse view
Convert Tri to Quad,
quadrization on (refine)
View in x-direction (right
side)
Redo last undone operation
View in y-direction (top
view)
Undo last operation
View in z-direction (front
view)
Print hotkey list (message
window)
?
Spaceball and Mouse Binding
ANSYS ICEM CFD allows simultaneous connection of both a Spaceball and a 3-button mouse. The default
actions for these is shown in Figure 105: Default Spaceball and Mouse Bindings (p. 125). For additional
information on managing your spaceball and mouse, see Mouse Bindings/Spaceball.
Figure 105: Default Spaceball and Mouse Bindings
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
125
126
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Display Tree
Use the Display Tree, which is located on the left of the GUI window, to manage what is displayed,
and how it is displayed, in the graphics window. ANSYS ICEM CFD offers a great deal of control in the
mesh generation process. The ability to manage the mesh generation is enhanced if you become familiar with the functions within the Display Tree.
The Display Tree has branches for the four most common types of entities that exist in most projects:
Geometry, Mesh, Blocking, and Parts/Subsets. Other branches will appear as various properties, loads,
constraints, etc. are applied to the model.
Figure 106: Display Tree
Mouse Usage
Mouse Operation
Description
Right button
Displays Options menu of the selected Display Tree item.
Shift + Left button
To automatically select all the items listed in between two
selected (highlighted) items.
Control + Left button
To select items in addition to, or deselect items from, a
set of previously selected (highlighted) items.
Left button on check box
Toggles entity visibility.
Double click on Display Tree item with
check box
Toggles entity visibility.
Double click on Display Tree item
without check box
Opens the Modify options of the selected item.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
127
Display Tree
Model
Right-click on Model in the Display tree to see the Model display options available, as shown below.
Create All Nodes
Displays all branches available in the Display tree. The default behavior is to display a branch only if
entities of that type exist in the model.
Geometry Units
Opens a DEZ in which you can specify a global unit of length to be used in your model.
Choose the appropriate units, and then click Apply (DEZ is preserved) or OK (DEZ is closed).
Geometry
Click the right mouse button on Geometry in the Display tree to see the Geometry display options
available, as shown below. The geometry options work only if a Geometry file is loaded.
Figure 107: Geometry Tree Display Options
Show All
Displays the whole geometry.
Hide All
Hides the whole geometry.
Blank Entities
Makes selected entities invisible.
Unblank All Entities
Restores blanked entities.
Rename Entity
Opens a Rename Geometry DEZ where you assign a new name to the selected entity.
New Name
Enter the desired name.
Type
Choose the type of geometry from the drop-down list to constrain the selection options.
POINT/CURVE/SURFACE/DENSITY/ENTITY
Click the Select ... icon, and then choose an appropriate geometry from the GUI window.
The following sections describe the subparts of the Geometry Tree.
Geometry Subsets Options
128
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Geometry
Modify Geometry Subset Options
Geometry Points Options
Geometry Curves Options
Geometry Surfaces Options
Geometry Bodies Options
Geometry Densities Options
Geometry Subsets Options
Elements can be grouped into Subsets, which have display options that can be controlled independently.
Right click on Subsets under Geometry to view the display options as shown below.
Figure 108: Subsets Display Options
Create
Creates subsets by the following methods.
Figure 109: Create Subset by Selection Window
Create Subset by Selection
Select geometry or mesh entities to add to the subset, then click Apply. If there are no valid
selections and Apply is clicked, then an empty subset will be created.
Note
When entities are selected, the type of entity followed by the entity name appears
in the field. For example, the selection of a surface of the entity “box.00” will
appear as “surface box.00”. When manually entering an entity, the same format
must be used.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
129
Display Tree
Break Part into Subsets by Surface Connectivity
Creates subsets of connected surfaces filtered by the angle of connectivity or surface curvature.
Note
Build Topology must be completed before using this feature.
This feature starts with one of the selected surfaces and returns the connected surfaces that are
connected at an angle less than the defined value, or has a curvature less than the defined
value. Then it moves on to the next surface. If none of the attached surfaces meet the defined
criteria it is placed in its own group.
Surfaces
Select the surfaces to be broken into subsets.
Angle
If the angle between the connected surfaces is less than the defined angle, then it will be
added to the same group. An angle of 180 would mean that all connected surfaces would
be in the same group. An angle of 0 would mean that all angles would stop surface grouping,
so each surface would be in its own group. Parallel surfaces meet at an angle of 0.
Curvature
If the curvature of a surface is less than the defined curvature value, than it will be added
to the group. A curvature value of 360 means that no surfaces would be excluded based
on curvature, and a value of 0 means that all surfaces would become their own group.
If the default values of angle = 180 and curvature = 360 are used, the selected surfaces will be
broken into groups by connectivity. After the groups are created, the subsets are ordered by
surface area, where the largest groups are listed first.
Create Subset by Attributes
Create subsets of geometry or mesh entities filtered by specified attributes. Toggle ON the desired
type of attribute, and enter the criteria in the field. More than one criteria can be used, for example,
entities with mesh maximum sizes between 50 and 100 can be defined by entering “< 100 > 50”.
Mesh Maximum Size
To create a subset of surfaces and curves filtered by the Maximum element size set for the surfaces
or curves.
Curve Length
To create a subset of curves filtered by curve length.
Surface Area
To create a subset of surfaces filtered by surface area.
Preview Subset
Click to highlight the entities that have the defined attributes. To create the subset of these entities, click Apply.
Show All
Displays all created subsets.
130
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Geometry
Hide All
Hides all created subsets.
Create Part
Creates parts from selected subsets.
Note
Subsets should not overlap since parts are “exclusive groups”.
Modify Geometry Subset Options
Right click on an existing subset name and the following options will be shown.
Figure 110: Modify Subset Options
Info
Gives information about the subset.
Modify
You can modify Subsets with the following options.
Figure 111: Add to Subset by Selection Window
Add to Subset by Selection
Select the geometric entities to add to the subset.
Remove from Subset by Selection
Select the geometric entities to remove from the subset.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
131
Display Tree
Add Layer(s) to Subset
You can add layers to a subset using different methods of the Flood Fill option as shown below.
Figure 112: Modify Subset – Add Layer Method
• Add Layer Method
Enter the number of layers attached to the selected entity to be added to the subset.
• All Attached Method
This will make a subset of all the attached items of the selected item.
• To Angle
The items that are attached to the selected entity at this angle or less will be added to the
subset. Enter the required angle (degrees) as shown below.
Figure 113: Modify Subset – To Angle Method
• At one side
If an entity is selected, all the surfaces attached to that entity will be highlighted. Select any
of the highlighted surfaces with the left mouse button and click the middle mouse button
or press Apply to add that surface to the subset.
132
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Geometry
Delete
Deletes the subset
Rename
To rename the subset.
Copy
Makes a copy of the subset.
Clear
Clears the subset contents.
Add
To add elements to the subset.
Remove
To remove elements from the subset.
Geometry Points Options
The display options for Points are shown below.
Figure 114: Points Display Options
Show Large
Shows the visible points as large points.
Show Dormant
Shows all the dormant points which are not permanently deleted.
Show Protected
This option will show a yellow sphere around protected points, a red sphere around hard-protected
points.
Show Point Names
Displays the point names of the visible points.
Show Point Info
Gives information about a selected point, including the point name, part name, and geometric location.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
133
Display Tree
To employ this option, select Points > Show Point Info. Proceed to select a point with the left
mouse button and accept the selection with the middle mouse button. Information on the point(s)
will be listed in the Messages window.
Blank Points
Blanks selected points.
Unblank All Points
Restores blanked points.
Show Only Points
Displays only the selected points and makes everything else invisible.
Show Attached Curves
Displays the curves which are attached to the selected point.
Show Attached Surfaces
Displays the surfaces which are attached to the selected point.
Rename Point
To rename selected points.
Geometry Curves Options
The display options for Curves are shown below.
Figure 115: Curves Display Options
Show Unattached
Shows the curves that are not attached to any of the geometry.
Show Single
Shows all the curves that are attached to only one surface.
Show Double
Shows all the curves that are shared by two surfaces.
134
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Geometry
Show Multiple
Shows all the curves that are shared by more than two surfaces.
Show Wide
Displays line data with thicker lines, to help distinguish between geometry and mesh.
Show Dormant
Shows all the dormant curves which are not permanently deleted.
Color by Count
Colors curves by the number of surfaces the curve is associated with. This option works only after CAD
repair. See Repair Geometry (p. 241).
• Green
Not associated with any surfaces
• Yellow
Associated with only one surface edge
• Red
Associated with two surface edges
• Blue
Associated with more than two surface edges
Show Composite
Displays the existing composite curves with different colors. Blocking must be loaded for this option.
Composite curves are curves that are grouped together for the purpose of edge association. See Blocking
> Associate > Group/Ungroup curves.
Curve Node Spacing
Displays a preview of the node spacing on curves.
Curve Element Count
Displays the number of elements prescribed on each curve.
Curve Tetra Sizes
Displays a tetra icon sized to indicate the tetra sizes that are set (if any) on each visible curve.
Curve Hexa Sizes
Displays a hexa icon sized to indicate the hexa sizes that are set (if any) on each visible curve.
Show Curves Names
Displays the names of the visible curves
Show Curve Info
Gives information about a selected curve, including the curve and part names.
To employ this option, select Curves > Show Curve Info. Proceed to select a curve with the left
mouse button and accept the selection with the middle mouse button. Information on the curve(s)
will be listed in the Messages window.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
135
Display Tree
Blank Curves
Blanks all the selected curves.
Unblank All Curves
Restores blanked curves.
Show Only Curves
Shows only selected curves on the screen and keeps others invisible.
Show Attached Points
Shows all the points which are attached to the selected curve.
Show Attached Surfaces
Shows the surfaces which are attached to the selected curve.
Rename Curve
You can rename the selected curves.
Geometry Surfaces Options
The display options for Surfaces are shown below.
Figure 116: Surfaces Display Options
Show Full
A more detailed representation of the CAD data, showing more isobars than in the Simple representation.
For triangulated surface data, a detailed representation will show all the surface triangles.
Show Simple
A wireframe representation of CAD data or a "Hard Feature" representation of triangulated surface data,
including surface boundaries as hard features.
136
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Geometry
Show Simpler
This wireframe representation requires less memory than the Simple option. This option is beneficial for
simplifying more complicated models, and making them easier to translate or rotate.
Show Simplest
This representation uses the least memory. This option is recommended for simplifying models that are
extremely complicated.
Wire Frame
The surfaces are drawn using lines, in either simple or detailed formats.
Solid
A solid or shaded representation of the surface data, which can be either simple or detailed.
Solid & Wire
A combination of the Solid and Wireframe representations of the surface data.
Grey Scale
This will convert the color geometry into grey scale.
Transparent
This will show the surface as transparent.
Show Surface Normals
When enabled, arrows indicating the positive normal direction of each visible surface will be displayed.
Color by Normal
When enabled, the part color is used to indicate the positive normal side of each visible surface. The
reverse side of each surface is colored gray.
Note
This option works only with Solid or Solid & Wire display.
Show Surface Thickness
This will show the thickness assigned for the surface.
Tetra Sizes
Selecting this option will display the reference tetra mesh sizes upon the selected visible surfaces.
Hexa Sizes
Selecting this option will display reference hexa sizes upon the selected visible surfaces.
Show Surface Names
Displays the names of the visible surfaces.
Show Surface Info
Gives information about a selected surface, including the surface and part names.
To employ this option, select Surfaces>Show Surface Info. Proceed to select a surface with the
left mouse button and accept the selection with the middle mouse button. Information on the
surface or surfaces will be listed in the Messages window.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
137
Display Tree
Blank Surfaces
Blanks the selected surfaces.
Unblank All Surfaces
Restores blanked surfaces.
Show Only Surfaces
Displays the selected surfaces only.
Show Attached Points
Displays points that are attached to the selected surface.
Show Attached Curves
Displays curves that are attached to the selected surface.
Rename Surface
To rename the selected surfaces.
Geometry Bodies Options
The display options for Bodies are shown below.
Figure 117: Bodies Display Options
Show Bounding Surfaces
Shows the boundary surfaces of the selected body.
Show Body Names
Displays the names of the visible bodies.
Show Body Info
Gives information about a selected body, including the body and part names.
To employ this option, select Bodies > Show Body Info. Proceed to select a body with the left
mouse button and accept the selection with the middle mouse button. Information on the body
will be listed in the Messages window.
Screen Move
Allows interactive movement of the material point in the plane of the screen.
138
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Geometry
Geometry Densities Options
Figure 118: Density Options Window
Create Density
Opens the Create Density Window which is explained in Create Mesh Density (p. 327).
Modify Density
Allows you to modify a previously created density region. The following options are available:
Size
Specifies the local maximum mesh size specified for the density region. This will be multiplied by
the Global Scale Factor.
Ratio
Specifies the tetra growth ratio away from the density region.
Width
For a density region, this specifies the number of layers (N) of the specified element size away from
the boundary of the density region that should have a constant expansion ratio. The layer N + 1 will
have a tetra size of the Size value multiplied by the Ratio.
For line and point densities, the Size value multiplied by the Width is the radius of the region
that the density region influences.
Density Location
Contains options for modifying the bounding nodes of the density region.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
139
Display Tree
Modify Location
Allows you to select a new location for an existing bounding node. Select the node to be moved
and its new location.
Add Location
Allows you to add new bounding node(s) to the existing density region definition. Select the
location(s) to be added to the density region extents and confirm the selection using the middlemouse button.
Delete Location
Allows you to delete existing bounding node(s) from the density region definition.
Delete Density
Allows you to select the density region(s) to be deleted.
Wide Density Lines
Displays wider density region lines.
Note
This option is often useful when taking images of the mesh setup.
Density Tetra Sizes
Shows the reference tetra size for the density region(s).
Density Color
Allows you to display the density region(s) in the color of your choice.
Show Density Names
Shows the names of the density region(s) on the screen.
Show Density Info
Reports information about the selected density region(s) in the message window.
Blank Densities
Blanks the selected density region(s).
Unblank All Densities
Restores blanked density region(s).
Rename Density
Allows you to rename the selected density region.
Mesh
The Mesh branch of the Display tree allows you to display all or part of the mesh by element type.
140
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Mesh
Figure 119: Mesh Tree
Mesh Display Options
Right click on Mesh in the Display tree to see the options available for displaying the mesh, shells or
volumes, as shown below.
Figure 120: Mesh Display Options
Cut Plane
• Manage Cut Plane
Opens the Manage Cut Plane DEZ as shown below. This option is described in Mesh Cut
Plane (p. 62) in the Main Menu chapter.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
141
Display Tree
Figure 121: Manage Cut Plane Window
• Show Cut Plane
If toggled ON, the Cut Plane will be displayed.
Element Numbers
Displays the numbers of the visible elements.
Color by Quality
Displays the elements according to the quality color setup. The color contour bar displays the range of
colors by quality.
Figure 122: Example of Color by Quality for Quality Quad Angle
Shrink 10%
Displays each element shrunk by 10% of its original size.
Shrink 50%
Displays each element shrunk by 50% of its original size.
142
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Mesh
Shrink Node Pos
Works in collaboration with the Shrink features that were previously described to redraw the nodes,
depending on whether or not the elements were shrunk.
Dot Nodes
Displays nodes as dots. If the display background color is dark, the dot nodes will be displayed as white,
and if the background color is light, the dot nodes will be displayed as black.
Node Numbers
Displays the numbers of the visible nodes.
Node Coords
Displays the coordinates of all the visible nodes.
Elem Verts
Displays the node order numbers of the visible elements. Works best if a shrink factor is also displayed.
The element vertex numbers can help you see how an element is defined, and thus see the orientation
of the element. For example, a tri element is defined by three nodes in a particular order (0, 1, 2). This
defines the orientation of the element.
Elem Triads
Displays the orientation triad of each visible element, with the I, J, and K directions.
Periodicity
Identifies the periodicity of the nodes, either translational or rotational.
Note
Periodicity applies only to Volume (Tetra and Hexa) Meshing, as well as Patch Independent
Meshing.
Quadratic Shape
Displays the correct curvature of edges with midside nodes.
Wide Lines
Displays wider lines for elements.
Couplings
Displays couplings. Couplings consists of defined hanging nodes and arbitrary interfaces.
Locked Elements
Displays any locked elements.
Distributed attribute
Makes the element with a distributed attribute visible. For example, if a model has distributed boundary
conditions, selecting this option allows you to view and edit the BC at an element or node basis. This
option is also available as an icon on the Edit Mesh toolbar.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
143
Display Tree
Diagnostics
This option allows you to utilize shell mesh diagnostics. The mesh diagnostic options can also be
accessed through Edit Mesh > Check Mesh. The difference is that the diagnostic options in the
Mesh Display Tree does not add problematic mesh to mesh subsets.
Single Edges
Displays any single edges of surface mesh elements that are visible. A single edge would represent
a hanging edge, and the element would be an internal baffle. These may or may not be legitimate.
Legitimate single edges would exist where the geometry has a zero thickness baffle with a free or
hanging edge.
Multiple Edges
Displays any edge that is shared among three or more surface elements. Legitimate multiple edges
would be found at a "T" junction, where more than two geometry surfaces meet. These elements
are a subset of the single and multiple edge checks.
Overlapping elements
Displays surface elements that occupy part of the same surface area, but do not have the same
nodes. This could be surface mesh that folds on to itself.
Non-manifold elements
Displays surface elements with non-manifold vertices. Non-manifold vertices are those where the
outer edges of their adjacent elements do not form a closed loop. Usually indicates elements that
jump from one surface to another, forming a "tent like" structure. This would usually pose no problem
for mesh quality but will represent a barrier in the mesh that probably should not be there.
Triangle boxes
Groups of four triangles that form a tetrahedron with no volume element inside.
Show
Edges
Displays only the edges of the surface mesh that are found by the selected diagnostic options.
Single edges will be displayed in yellow, and multiple edges in blue.
Edges and Faces
Displays the edges and one layer of attached faces.
144
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Mesh
Edges and 2 layers of Faces
Displays the edges and two layers of attached faces.
Show only problems
Displays only the elements found by the diagnostic options and turns off the rest of the mesh.
Mesh Subsets
Elements can be grouped into Subsets, which have display options that can be controlled independently.
Note
To view the contents of a single subset, select the subset and deselect all other subsets.
Subsets work independently of the active elements under parts and types. You can switch
between displaying entities by part, type, or by a defined grouping in a subset. Parts and
Subsets are Boolean with the geometry, but they are not Boolean with each other, meaning,
by turning a subset off, it does not turn those entities off unless they are off in the part as
well. To access specific entities of geometry or mesh, you can place the entities into a subset.
By turn off the parts, and displaying the subset, you can choose to view only the entities in
the subset.
Parts are exclusively defined, so that an entity can only be in one part. But one entity can
be part of multiple subsets.
Clicking the right mouse button on Subsets in the Mesh Tree will give the options below.
Figure 123: Mesh Subsets Display Options
Create
To create a new subset of currently active parts and types. There are different options for creating subsets
as shown below.
Figure 124: Create Subset Window
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
145
Display Tree
Create Subset by Selection
Create a subset by entering a name and selecting either geometric or mesh entities.
Create Subset near Position
Create a subset near a certain position by entering the XYZ coordinates as shown below.
Figure 125: Create Subset Near Position Window
• Nodes
Toggle this ON if nodes are to be selected.
• 1d elems
Toggle this ON if 1d elements (lines and curves) are to be selected.
• 2d elems
Toggle this ON if 2d elements (surfaces) are to be selected.
• 3d elems
Toggle this ON if 3d elements (volumes) are to be selected.
• Toggle OFF the options that you do not wish to select.
Create Subset by Element Number
Create a subset by entering the elements numbers of the elements you want to include.
Create Subset in Region
Create a subset in a specified region as shown below.
146
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Mesh
Figure 126: Create Subset in Region Window
• Min and Max Coordinates
Enter the minimum and maximum coordinates that represents the region.
• Include partially enclosed
Includes elements partially enclosed in the region specified by the coordinates.
• Nodes
Toggle this ON if nodes are to be selected.
• 1d elems
Toggle this ON if 1d elements (lines and curves) are to be selected.
• 2d elems
Toggle this ON if 2d elements (surfaces) are to be selected.
• 3d elems
Toggle this ON if 3d elements (volumes) are to be selected.
• Toggle OFF the options that you do not wish to select.
Find Worst
Creates a subset of the elements with the worst quality found using the “Quality” criterion.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
147
Display Tree
Show All
Displays all subsets.
Hide All
Hides all subsets.
Shadings
allows you to set the shading for the subset independent of the shading used for the mesh. This allows
for better visibility as the subsets can be distinguished from the surrounding mesh. By default, the
shading of the subset is Inherited from the shading used for the mesh. You can also select the Wire
Frame, Solid, or Solid & Wire rendering.
Note
Subsets created from the Quality Metric Histogram will retain their Color by Quality
based color and shading independent of this setting.
Tip
• To display other subsets with Color by Quality, combine the Solid or Solid & Wire subset
shading with the Color by Quality mesh display option.
• To display the elements of a DIAGNOSTIC subset without the Color by Quality shading,
you can copy it to a new subset and disable the DIAGNOSTIC subset (Mesh > Subsets >
DIAGNOSTIC).
Modify Mesh Subsets
Right clicking on an existing mesh subset displays the options shown below.
Figure 127: Modify Mesh Subset Options
Info
Gives information about the subset.
Modify
Subsets can be modified by the options in the window shown below.
148
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Mesh
Figure 128: Modify Subset Window
The following options are common to all of the Modify Subset options.
• Clear
Clears all the entities in the subset.
• Reset to Active Parts and Types
Resets the subset to contain all active (visible) parts and types.
• Remove Inactive Parts and Types
Removes the inactive (not visible) parts and types from the subset.
The different Modify Subset options are described below.
Add to Subset by Selection
Select mesh entities to add to a subset.
Add to Subset near Position
Enter the node numbers or XYZ coordinates of entities to add to a subset.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
149
Display Tree
Add by Element Number
Enter element numbers to add to a subset.
Add Contents of Subset
Add contents of an existing subset to the current subset.
Add to Subset in Region
Choose a subset with a specified region to modify.
Figure 129: Add to Subset in Region Window
• Min and Max Coordinates
Enter the minimum and maximum coordinates that represent the region.
• Include partially enclosed
Includes elements partially enclosed in the region specified by the coordinates.
Restrict to subset by selection
Allows you to restrict a subset to the entities that are selected.
150
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Mesh
Remove from subset by selection
Removes the selected entities from the subset.
Add Layer(s) to Subset
You can add layers to a subset using different methods of the Flood Fill option as described
below.
Figure 130: Add Layer(s) to Subset Window
• Add Layer Method
Enter the number of layers attached to the selected entity to be added to the subset.
• All Attached Method
This will add all the attached items of the selected entity to the subset.
• Same Part
Adds all entities in the same part.
• To Curve
Adds all entities up to the nearest boundary curve.
• To Angle
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
151
Display Tree
The items that are attached to the selected entity at this angle or less will be added to the
subset. Enter the required angle (degrees).
Figure 131: Modify Subset – By Angle Method
– Only visible elements
Toggle ON to add visible entities only.
– Also volume elements
Toggle ON to add volume elements.
Remove Layer(s) from Subset
You can remove layers from a subset using different methods as described below.
• Num Layers
Enter the number of layers to be removed.
• Only visible
To remove visible entities only.
Make scan plane
Creates a subset of scan plane elements. This option is for advanced users.
152
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Mesh
Figure 132: Make Scan Plane Window
Delete
Deletes an existing subset.
Rename
To rename a subset.
Copy
Copies a subset.
Clear
Clears the contents of a subset.
Add 1 layer
Adds the adjacent layer of entities to the subset.
Add
To select entities to be added to the subset.
Remove
To select entities to be removed from the subset.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
153
Display Tree
Make Element set
To define a subset as an element set.
Make Node set
To define a subset as a node set.
Mesh Points
Click on Points in the Mesh Tree to turn nodes ON or OFF from the display.
Mesh Lines
Click on Lines in the Mesh Tree to turn bar elements ON or OFF from the display.
Right clicking on Lines in the Mesh Tree gives the display option Direction. Toggling ON this option
displays an arrow showing the relationship between the first and second nodes along the line element.
This can be useful to display the dependency for 1D line element properties. The direction of the line
element can be changed using Edit Mesh > Reorient Mesh > Reverse Line Element Direction.
Mesh Shells
The display options for Shells are shown below.
Figure 133: Shells Display Options
Wire Frame
Displays the mesh with a wire frame outline, colored part by part.
Solid
Displays the mesh as a solid mesh.
Solid & Wire
Displays the mesh as a solid mesh with a wire frame outline. The wire frame is drawn in the color of the
background.
By dimension
Displays shell elements only as solid mesh.
Hidden Line
Displays a wire frame mesh with the backside of the model hidden.
154
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Mesh
Color by Quality
Displays the shell elements according to the quality color setup. The color contour bar displays the range
of colors by quality.
Figure 134: Examples of Color by Quality—Aspect Ratio
Tri elements
Tetra elements
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
155
Display Tree
Dual Mesh
Allows you to view the mesh dual. When enabled, it draws the wire-frame between the centroid of each
cell to better show the node centered volumes. An example of the mesh dual for a tetra-prism mesh is
shown in Figure 135: Mesh Dual for a Tetra-Prism Mesh (p. 156).
Figure 135: Mesh Dual for a Tetra-Prism Mesh
This option is just a visual aid and can be used only for surface meshes.
Note
The mesh dual of a hexa mesh is still a hexa mesh.
156
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Mesh
Shell Thickness
Displays the surface mesh thickness.
Normals Using Arrow
When enabled, arrows indicating the positive normal direction of each visible unstructured surface element
will be displayed.
Normals Using Color
When enabled, the part color is used to indicate the positive normal side of each visible unstructured
surface element. The reverse side of each element is a darker color.
Note
This option works only with Solid or Solid & Wire display.
Face Icons
Adds part colored face icons to the wireframe display. The icons appear similar to Shrink 75%.
Diagnostics
This option allows you to utilize shell mesh diagnostics. The mesh diagnostic options can also be accessed
through Edit Mesh > Check Mesh. The difference is that the diagnostic options in the Mesh Display
Tree does not add problematic mesh to mesh subsets.
Single Edges
Displays any single edges of surface mesh elements that are visible. A single edge would represent
a hanging edge, and the element would be an internal baffle. These may or may not be legitimate.
Legitimate single edges would exist where the geometry has a zero thickness baffle with a free or
hanging edge.
Multiple Edges
Displays any edge that is shared among three or more surface elements. Legitimate multiple edges
would be found at a "T" junction, where more than two geometry surfaces meet. These elements
are a subset of the single and multiple edge checks.
Overlapping elements
Displays surface elements that occupy part of the same surface area, but do not have the same
nodes. This could be surface mesh that folds on to itself.
Non-manifold elements
Displays surface elements with non-manifold vertices. Non-manifold vertices are those where the
outer edges of their adjacent elements do not form a closed loop. Usually indicates elements that
jump from one surface to another, forming a "tent like" structure. This would usually pose no problem
for mesh quality but will represent a barrier in the mesh that probably should not be there.
Triangle boxes
Groups of four triangles that form a tetrahedron with no volume element inside.
Show
Edges
Displays only the edges of the surface mesh that are found by the selected diagnostic options.
Single edges will be displayed in yellow, and multiple edges in blue.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
157
Display Tree
Edges and Faces
Displays the edges and one layer of attached faces.
Edges and 2 layers of Faces
Displays the edges and two layers of attached faces.
Show only problems
Displays only the elements found by the diagnostic options and turns off the rest of the mesh.
Surface Bounds
Displays the surface boundary region and all elements attached to that region. Useful in visualizing curve
boundary regions.
Mesh Volumes
Volume display options are shown below.
Figure 136: Volume display options
Wire Frame
Displays the elements with a wire frame mesh on it.
Solid
Displays the elements as a solid mesh.
Solid & Wire
Displays the mesh as a solid mesh with a wire frame outline. The wire frame is drawn in the color of the
background.
Hidden Line
Displays a wire frame mesh with the backside of the model hidden.
Volume Bounds
Displays the volumetric boundary region and all elements attached to that region. Useful in visualizing
the surface boundary regions.
Blocking
Click the right mouse button on Blocking in the Display tree to see the options available.
158
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Blocking
Blocking Options
Right-click on the Blocking branch in the Display tree to view the Blocking display options. When the
blocking tab is active, the hot key “i” will initialize the index control. The Blocking display options are
as follows:
Figure 137: Blocking Display Options
Index Control
Figure 138: Index Control Window
Select corners
Allows you to select boundary node vertices and adjusts the index range accordingly.
Reset
Resets the values to the minimum and maximum values, so that the entire blocking is displayed.
Query Edge
Allows you to select an edge. The system will then center the Index control on the dimension corresponding to the edge selected
When an O-grid is created, a new index direction will be added to the Index control and a
message will be printed with the corresponding dimension. O-grid dimensions are named On
where n begins with a value of 3. The reason for this is that dimensions 0, 1, and 2 already
correspond to the I, J, and K indices.
The index range is not taken into account when the mesh is saved.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
159
Display Tree
Index Sets
Contains options for saving and managing index sets based on the index control values.
Show
shows the list of the currently saved index sets in the Saved Index Sets dialog.
You can select the index set to restore from the list and the blocking display will be reset
corresponding to the saved index values.
Add
saves the current set of index values. The saved index sets are numbered sequentially (1, 2, etc.).
Clear
clears all the currently saved index sets from the Saved Index Sets list.
Load
allows you to load previously saved index sets from an index control (*.ictrl) file.
Save
allows you to write the currently saved index sets to an index control (*.ictrl) file.
Done
Closes the window
Set Line Width
Sets the width of Block edge lines.
Init output blocks
Initializes the number of output blocks to be equal to the number of regular topology blocks.
Blocking info
Provides information in the message window about the blocking (number/type of blocks, topology info,
index info) and pre-mesh (number of nodes, elements). Information about shared walls (if defined) will
also be reported.
Blocking Subset Options
Right click on Subsets in the Blocking tree to view the Display options are shown below.
Figure 139: Blocking Subset Display Options
Create
Select entities to add to a new Blocking Subset.
160
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Blocking
Figure 140: Create Subset Window
After the subset is created, it will be displayed in the Display Tree under Blocking>Subsets as
shown below.
Figure 141: Blocking Subset Tree
Modify Subsets Options
Right click on a created subset to view the options shown below.
Figure 142: Modify Subset Options
Modify
Blocking subsets can be modified with the options shown below.
Figure 143: Modify Subset window
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
161
Display Tree
Add to Subset by Selection
Select the blocking entities to add to the subset.
Remove from Subset by Selection
Select the blocking entities to remove from the subset.
Delete
Deletes the subset.
Rename
Renames the subset.
Vertices
The display options for Vertices are shown below.
Figure 144: Vertices Display Options
On surfaces
To turn the display of vertices on surfaces ON or OFF.
Periodic
To turn the display of vertices that are marked as periodic ON or OFF.
Names
Displays the names of the vertices.
Proj type
Vertices will be tagged according to type:
• p: Associated to a prescribed point (red).
• c: Associated to a curve (green).
• s: Associated to a surface (white).
• v: Associated to an interior, volume, or vertex (blue).
Indices
Displays the block indices.
Numbers
Vertices will be displayed with unique numbers assigned to them during creation of the blocks.
162
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Blocking
Show Vertex Info
Gives information about a selected vertex.
Edges
The display options for Edges are shown below.
Figure 145: Edges Display Options
Internal edges
To turn the display of internal edges in a volume ON or OFF.
Show associations
Shows the associations of different edges to curves.
Bunching
Displays the node distribution on edges.
Counts
Displays the number of elements of the edges.
Projected Edge Shape
Displays the edges after mesh calculation with the current node distribution.
Projected Mesh Shape
Displays the mesh after calculation with the current edge distribution.
Meshing set
Displays the special meshing sets.
Shape source
Turns the linked edges ON or OFF. All the arrows will point from the source edge to the target edge.
Simple
Shows edges in simple form.
Color by Count
Only for 2D blocking.
Show Edge Info
Gives information about the selected edge. The edge vertices, spacing, ratio, constraints, edge dimension,
index, number of nodes, mesh law, and number of edge segments (if any) will be reported in the message
window.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
163
Display Tree
Faces
The display options for Faces are shown below.
Figure 146: Faces Display Options
Periodic Faces
Allows you to turn the display of periodic faces ON or OFF. Periodic faces are established when all associated vertices have been set to periodic using the Periodic Vertices option in the Blocking tab. Vertex
periodicity can also be displayed by enabling Periodic for Vertices in the tree. Further splits across
periodic faces create new edges and vertices which are automatically set to periodic.
Face Projection
Toggles ON or OFF the display of faces associated with surfaces (see Associate Face to Surface (p. 398)).
The projected faces will be displayed depending on their association as follows:
Face Association
Display
Face→Part
Part Color along with Part Name
Face→Link Shapes
White or Black (depending on the background color)
Face→Selected Surface
Purple
Face→Interpolate
Green
Face→Reference Mesh
Yellow
Boundary
Displays only the faces that lie on the outer surfaces.
Shared Wall Info
Reports information about the currently defined shared wall configurations in the message window. The
volumes having a shared wall between them and the shared surface will be reported.
Show Face Info
Gives information about the faces. The face vertices, face elements, and the projection type will be reported in the message window.
Blocks
The display options for Blocks are shown below.
164
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Blocking
Figure 147: Blocks Display Options
Solid
Displays blocks in solid color.
Whole blocks
Shows each block as a black icon.
No shrink
If toggled ON , the actual size of the block is displayed.
Find Worst
This option calculates the determinant value for each block and highlights the elements with the worst
value or values. A bad determinant block usually results in a bad determinant grid. Moving the vertices
can help improve the determinant values. You can set the number of worst blocks to display by clicking
on Settings and choosing Meshing Options>Hexa Meshing, then setting a numerical value for Find
Worst. The default range is 1–3, but you can set the range to any desired level (for example, 3–5 or 2–8).
The worst blocks are listed by their determinant values and shown in red in the model.
IJK
Displays the IJK grid orientation for each block.
Refinement
This option will blank all the black icons and will display the blocks that are affected by the Refinement
command, which is in the Meshing Menu.
Classes
Displays the blocks along with their respective axis and index numbers. For each block the three axial
directions are indicated by 1, 2, and 3, and O-grids are represented by 0.
Show structured
Shows the structured blocks.
Show unstructured
Show the unstructured blocks.
Show swept
Shows swept blocks in the geometry.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
165
Display Tree
Blanking
Restores blanked blocks.
Blank Blocks
Blanks the selected blocks.
Show Block Info
Gives information about the selected block.
Pre-Mesh
The display options for Pre-Mesh are shown below.
Figure 148: Pre-Mesh Display Options
Wireframe
Displays the model in the wireframe mode.
Solid
Displays the model in the solid mode.
No projection
When the mesh is generated, it will conform to the blocking without being projected to the actual CAD
geometry.
Project vertices
When the mesh is generated, the vertices/points on the edges of the blocks will be projected to the
curves or surfaces to which they are associated. No other projection will take place.
Project edges
When the mesh is generated, the nodes on the edges of the blocks will be projected to the curves or
surfaces to which they are associated. The face nodes will not be projected to the surfaces, but rather
interpolated between the edges. This option is generally used for two-dimensional models. Project
edges may be used for three-dimensional models as well, as a method to quickly confirm a correct mesh
before employing the Project faces operation.
Project faces
When the mesh is generated, all face nodes and edge nodes will be projected to their associated curves
and surfaces. This option is generally used for three-dimensional models.
166
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Blocking
Active Parts
Allows you to select surface parts to be considered for projection when the mesh is generated. All surface
parts highlighted in the selection list will be projected to during the mesh generation.
When you compute the pre-mesh, a message will appear indicating the part(s) to which projection
has been disabled.
Recompute
Recomputes the mesh.
Show size info
Reports the number of nodes and elements in the message window.
Convert to Unstruct Mesh
Converts the blocking to an unstructured mesh.
Convert to MultiBlock Mesh
Writes out the multiblock mesh for the current blocking.
Reference MultiBlock Mesh
Automatically references the multiblock mesh in the current directory for meshing the current blocking.
Note
Only one multiblock mesh file should exist in the current directory.
Scan planes
Scan planes are used to view the volume grid. The following Scan plane control window will be displayed.
Figure 149: Scan Planes Window
• There are a number of selection fields for displaying scan planes across each of the principal directions
(i, j, k, o3, o4, etc.). #0 corresponds to the first scan plane across i, #1 corresponds to the second, across
j, etc. Higher scan planes, such as #3 or #4, scan across the first and second O-Grid indices, respectively.
• There is a Block and a Grid index for each scan plane. The Block index is the block number in which
the scan plane is displayed. The lowest and highest block are typically in the VORFN region and may
not be displayed. The Grid index is the node number within the block.
• The up/down arrow buttons allow you to increase/decrease the Block or Grid index by one, respectively.
If you click and hold down the up/down arrow button, you will be able to scroll through the Block/Grid
index (you need not click the button repeatedly).
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
167
Display Tree
• By default, the scan plane is in the color of the volume parts it passes through. However, the Color
buttons allow you to specify a color for each scan plane (see Figure 150: Selecting the Scan Plane
Color (p. 168)).
Figure 150: Selecting the Scan Plane Color
• The Select button allows you to select an edge in the model. The scan plane perpendicular to this
edge is then displayed. This is the easiest way to place a scan plane in the model.
• The Solid check box controls whether the mesh will be displayed in solid or wire-frame form.
Tip
Scan planes are very useful for diagnosing blocking issues. Running a scan plane through
the problem area is often the best way to gain understanding of what is happening in
the volume. Typically the scan plane will reveal issues with projection or edge distribution.
Fixing these will improve the quality. Enabling the display of edge association and edge
bunching can also help identify the problem.
Cut Planes
A cut plane is used to visualize results on a plane cut through the three dimensional model. Results are
viewed on the cut plane as well as on the 2D Dynamic window. The cut plane may be defined in several
ways depending on the application.
168
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Blocking
Figure 151: Pre-Mesh Cut Plane
Method
• By Coefficients
Defines the cut plane by the equation of the normal vector. The equation is of the form: Ax
+ By + Cz + D = 0. Enter the coefficients A, B, C, D of the equation.
• By Point and Normal
pt
Enter the Global Cartesian coordinates in the X, Y, and Z direction.
NX
Enter the X component of a unit vector normal to the desired cut plane.
NY
Enter the Y component of a unit vector normal to the desired cut plane.
NZ
Enter the Z component of a unit vector normal to the desired cut plane.
• By Corner Points
Creates a cut plane passing through the given three points. You can enter the Cartesian coordinates of Pt1, Pt2, and Pt3 points.
• By 3 Points
You can select any three points in the GUI using the left mouse button to define a cut plane.
• Move or Rotate
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
169
Display Tree
You can interactively move a previously defined cut plane while holding the left mouse button
down. Once you get to the desired location, release the mouse button. Use the middle mouse
button to rotate the cut plane about the normal axis. When you get the desired orientation,
release the mouse button. To end the interactive movement of the cut plane, click on the
right mouse.
• Middle X plane
This will put the cut plane at the middle of the geometry in the X-direction.
• Middle Y plane
This will put the cut plane at the middle of the geometry in the Y-direction.
• Middle Z plane
This will put the cut plane at the middle of the geometry in the Z-direction.
Fraction value
Select the location of the plane by changing the fraction value either by moving the sliding bar or
entering a value.
Solid Mode
To display the cut plane in solid mode.
Shrink elements
To shrink elements in the display.
Note
Cut planes show the grid lines relative to planes in 3D space. Scan planes show grid lines
relative to grid planes. Either method may be used. For unstructured blocking, it is recommended to use cut planes.
Note
The cut planes for Pre-Mesh can be viewed before writing out the mesh. This allows for
mesh quality inspection and block editing before writing out the final mesh.
Output Blocks
Controls the number of block files written out for multi-block structured grids.
Hexa supports two levels of block decomposition. The first level is what you see by default, and
what is used to mesh the model. However, it is sometimes desirable to mesh with one set of blocks
and group blocks together for a smaller number of blocks for the solver. The output blocks option
can be used to achieve this. First, click on Init output blocks. This makes your output blocks the
same as your regular blocks.
Then select Output Blocks under the Blocking > Pre-Mesh Display Tree. Now, operations such as
Merge Blocks, Extend Split, Merge Face, and Renumber Blocks can be performed on the output
blocks. By merging blocks you can reduce the number of blocks that are written to the solver. The
170
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Local Coordinate Systems
blocks that are used to mesh the model are unchanged. You can switch between the regular blocks
and the output blocks at any time.
Note
Face selection operations for Output Blocks are not fully supported.
Topology
The display option for Topology is shown below.
Figure 152: Topology Display Options
Create sub-topo
A portion of the current (root) block topology may be extracted to create a new topology. Each sub-topology has the following display options.
Figure 153: Sub-topo Display Options
• Copy
Makes a copy of a sub-topology.
• Merge
Merges selected sub-topologies.
• Rename
To rename the sub-topology.
• Delete
Deletes the sub-topology.
• Save
Saves the sub-topology.
Local Coordinate Systems
You can define local coordinate systems (LCS) for use in geometry, mesh, blocking or boundary condition
manipulation using the LCS icon in the main menu. The default coordinate system located at the origin
is called Global.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
171
Display Tree
When a LCS is defined, its name will appear in the display tree as shown below. Deactivating all Local
Coordinate Systems in the Display tree will activate the Global coordinate system. You can view only
one LCS at a time.
Figure 154: Local Coordinate Systems Tree
Right click on a defined coordinate system in the Display Tree for the following options.
Delete
Removes the LCS from the display tree and its data from the geometry and parameter files.
Modify
Opens the Define Local Coordinate System DEZ to allow you to modify the coordinate system.
See Local Coordinate Systems in the Main Menu chapter for the description of all the options.
Rename
Opens a dialog box where you may give the LCS a new name.
Flip Axis
Cycles the LCS axes through the sequence X-Y-Z, to Z-X-Y, to Y-Z-X, back to X-Y-Z relative to the original
LCS. For non-rectangular coordinate systems the transformation is the same, except using the R, θ, and
Z axes, or the R, θ, and Φ axes.
This approach is useful to transform a Z-dominant coordinate system to an X-dominant or Y-dominant coordinate system. For example, if you want to change the orientation for the 1-point definition
method or have the first two points of the 3-point method define something other than Z-direction,
it might be best to define the LCS in the easiest method possible and Flip Axis to get the appropriate
LCS.
Element Properties
If the model contains different defined Elements, such as 0D, 1D, 2D (TRI/QUAD) or 3D elements
(TETRA/HEXA), they will be under Points, Lines, Surfaces and Volumes respectively. The Element Properties
Tree will appear as shown below.
172
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Constrained Nodes
Figure 155: Element Properties Tree
Points contain all the 0D element properties and Lines contains 1D element properties, etc. When element
properties are defined, they will appear in both the Element Properties tree as well as the part display
tree to which they belong. To edit any of these definitions, double click the defined properties.
Right clicking on Element Properties in the Display tree will give you the options to Delete Empty
Properties. This option removes empty element properties from the display tree and refreshes the
Element Properties branch. This option can be run whenever needed after modifications are made to
Element Properties
Connectors
If connectors are defined for a model, they will be listed under the Connectors Tree.
Right clicking on the Connectors Tree will give you the following options.
Figure 156: Modify Connectors Options
Create
Opens the Define Connectors window. See Mesh > Define Connectors for more information.
Make All Active
Makes all connectors active.
Make All Inactive
Makes all connectors inactive.
Delete All
Deletes all connectors defined in the model.
Constrained Nodes
Node constraints may be set using the Define Constrained Node sets option on the Constraints tab,
or by right-clicking Constrained nodes in the display tree. See the Define Constrained Node Sets page
for information on the node constraint options.
If constrained node sets are defined, they will be listed under Constrained nodes in the display tree.
Right-clicking on the name of a Constrained Node set, will give you the following options
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
173
Display Tree
Delete
Removes the selected constrained node set.
Rename
Opens a dialog box to specify a new name for the constrained node set.
Modify
Opens the Modify Constrained Nodes DEZ where you can change the parameters of the node set. For
more information regarding the options available, see the Define Constrained Node Sets page.
Contacts
Contact boundary conditions may be set using the Define Contact option on the Constraints tab, or
by right-clicking Contacts in the display tree. See the Define Contact page for information on the contact
constraint options.
When you turn on the display for a contact set, the contact area will be drawn as white and the target
set as red. This display is useful for Automatic Contact Setup to see the elements that are marked depending on the defined contact proximity factor.
Figure 157: Contacts Tree
To edit a contact boundary condition, right click on the defined contact boundary condition set to
choose from the following options.
174
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Displacements
Figure 158: Modify Contacts Options
Modify
Opens the Modify Surface-to-Surface Contact Parameters DEZ. For more information on the options
available, see the Define Contact page.
Switch contact/target
To switch the target set and the contact set for the given contact region.
Delete
Deletes the selected contact.
Rename
To rename the selected contact.
Displacements
Multipoint Constraint Equations may be set using the Create Constraint Equation option on the
Constraints tab. See the Create Constraint Equation page for information on multipoint constraint options.
Multipoint Constraint Equations that are defined on points, curves and surfaces will appear in the Display
tree as shown below.
Figure 159: Displacements Tree
To edit any constraints, right-click on the constraint name in the display tree and choose from the following options.
Figure 160: Modify Displacement Options
Delete
Removes the selected displacement.
Rename
Opens a dialog box to specify a new name for the displacement.
Modify
Opens the Modify Constraint Equation DEZ where you can change the parameters of the multipoint
constraint equation (displacement). For more information regarding the options available, see the Create
Constraint Equation page.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
175
Display Tree
Right click on Displacements in the Display Tree to choose from the following options.
Figure 161: Displacement Display Options
Show All
Displays all the defined displacement.
Hide All
Hides all the displacement.
Loads
Loads that are defined on points, curves and surfaces will appear in the Display tree as shown below.
In this context, ‘Loads’ may be of force or pressure type.
Figure 162: Loads Display Tree
Right click on a defined load to choose from the following options.
Delete
Deletes the selected load.
Rename
Opens a dialog box to specify a new name for the selected load.
Modify
Opens a Modify Force (or Modify Pressure, as appropriate) DEZ which allows you to adjust the parameters of the load.
For full information on the options available, see Create Force (or Place Pressure) in the Help viewer.
Right click on Loads in the Display Tree to choose from the following options.
Show All
Displays all the defined loads.
Hide All
Hides all the loads.
176
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Rigid Walls
Material Properties
Material Properties that are defined are located in the Display tree as shown below.
Figure 163: Material Properties Display Tree
To edit the material properties of an element, you can double click the left mouse button on the defined
material name in the Display Tree to open the Define Material Property DEZ.
Right clicking on a defined material name in the Display Tree will give you the following options.
Figure 164: Modify Material Properties Options
Delete
Removes the Material Property definition.
Rename
Opens a dialog box to assign a new name to the selected material property.
Modify
Opens the Define Material Property DEZ to allow to modify the material properties.
For more information on the options available, see Create Material Property in the Help viewer.
Copy
Opens a dialog box to assign a distinct name to the new material being defined. The new material
properties may then be modified as necessary.
Rigid Walls
Rigid Wall boundary conditions may be set using the Define Planar Rigid Wall option on the Constraints
tab, or by right-clicking Rigid walls in the Display tree. See the Define Planar Rigid Wall page for information on the Rigid Wall boundary condition options.
When set, Rigid Wall boundary conditions will appear in the Display Tree as shown below.
Figure 165: Rigid Walls Tree
Right-clicking on the name of a Rigid wall, will give you the following options.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
177
Display Tree
Delete
Removes the selected rigid wall boundary condition.
Rename
Opens a dialog box to specify a new name for the rigid wall boundary condition.
Modify
Opens the Modify Planar Rigid Wall DEZ where you can change the parameters. For more information
regarding the options available, see the Define Planar Rigid Wall page.
Single Surface Contacts
Single Surface Contact constraints are available only for the LS-DYNA solver.
You may set Single Surface Contact constraints using the Define Single Surface Contact option on
the Constraints tab, or by right-clicking Single Surface Contacts in the Display tree. See the Define
Single Surface Contact page for information on the Single Surface Contact options.
Right-clicking on the name of a Single Surface Contact in the Display tree, will give you the following
options.
Delete
Removes the selected single surface contact.
Rename
Opens a dialog box to specify a new name for the single surface contact.
Modify
Opens the Modify Single Surface Contact DEZ where you can change the parameters. For more information regarding the options available, see the Define Single Surface Contact page.
Temperatures
Temperature boundary conditions defined on points, curves or surfaces will appear in the Display Tree
as shown below.
Figure 166: Temperatures Tree
Right click on a defined temperature to choose from the following options.
Delete
Deletes the selected temperature boundary condition.
178
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Velocities
Rename
Opens a dialog box to specify a new name for the selected temperature boundary condition.
Modify
Opens a Modify Temperature Boundary Condition DEZ which allows you to adjust the parameters of
the boundary condition.
For full information on the options available, see Create Temperature Boundary Condition in the
Help viewer.
Right click on Temperatures in the Display Tree to choose from the following options.
Show All
Displays all the defined temperature boundary conditions.
Hide All
Hides all the defined temperature boundary conditions.
Velocities
You may set Velocity Boundary Conditions using the Define Initial Velocity option on the Constraints
tab, or by right-clicking Velocities in the Display tree. See the Define Initial Velocity page for information
on the Single Surface Contact options.
When set, velocity boundary conditions will appear in the Display Tree as shown below.
Figure 167: Velocities Tree
Right click on a defined velocity boundary condition set to choose from the following options.
Delete
Deletes the selected velocity boundary condition.
Rename
Opens a dialog box to specify a new name for the selected velocity boundary condition.
Modify
Opens a Modify Initial Velocity Parameters DEZ which allows you to adjust the initial translational and
rotational velocities.
For full information on the options available, see Define Initial Velocity in the Help viewer.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
179
Display Tree
Parts
Figure 168: Parts Tree
The Parts Display tree contains a list of all the parts in the currently loaded Geometry and Mesh files.
If a part is active, then all the mesh and active geometry elements that are associated it will be displayed.
The exception to this rule is if a certain subset is enabled, the entities of that subset are displayed independently of the active parts in the Parts Tree.
Parts Display Options
Right click on Parts to view the following display options.
Figure 169: Parts Display Options
The options are described in the following sections:
Create Part
Create Assembly
More Part Display Options
Create Part
Parts can be created by four methods.
180
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Parts
Figure 170: Create Part Window
Create Part by Selection
Select geometrical or mesh entities to create a part.
Create Part near Position
Select a position using x, y, and z coordinates to create a part.
Figure 171: Create Part by Near Position window
• Locations
Enter x, y, z coordinates of a specific position.
• Nodes
Toggle this ON if nodes are to be selected.
• 1d elems
Toggle this ON if 1d elements (lines and curves) are to be selected.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
181
Display Tree
• 2d elems
Toggle this ON if 2d elements (surfaces) are to be selected.
• 3d elems
Toggle this ON if 3d elements (volumes) are to be selected.
• Toggle OFF the options that you do not wish to select.
Create Part in Region
Define a region by specifying the range of x, y, and z coordinates that bound the region.
• Min and Max Coordinates
Enter the minimum and maximum coordinates that represent the region.
• Include partially enclosed
Includes elements partially enclosed in the region specified by the coordinates.
• Nodes
Toggle this ON if nodes are to be selected.
• 1d elems
Toggle this ON if 1d elements (lines and curves) are to be selected.
• 2d elems
Toggle this ON if 2d elements (surfaces) are to be selected.
• 3d elems
Toggle this ON if 3d elements (volumes) are to be selected.
• Toggle OFF the options that you do not wish to select.
Create Part with Blocks
Select blocks to create a part.
Create Assembly
Assemblies can be used in ANSYS ICEM CFD to help organize data. An assembly is a collection of parts.
Note
It is important to note that an assembly is treated as a part with the syntax of ASSEMBLY /
PART. The “/” character denotes an assembly. In as such, the base level assembly can contain
entities, but this is not a recommended practice. Assemblies can contain other assemblies,
denoted by the syntax ASSEMBLY1 / ASSEMBLY2 / PART, but it is recommended to keep assembly, sub-assembly, and part names unique.
182
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Parts
Assemblies with their constituent parts will appear in the Display tree as shown below.
Figure 172: Parts Tree with Parts and Assemblies
Note
Assembly names appear in black font, and part names appear in non-black colors. If a part
color is set to white, a contrast background color will automatically appear in the Display
Tree window to make the part names readable.
Assemblies can be created through the following ways:
• Using the Create Part option and entering the syntax ASSEMBLY1 / PART1 as the Part name. Then
entities can be selected to be added to PART1 in ASSEMBLY1.
• Parts can also be dragged and dropped into assemblies through the Display Tree. Parts in an assembly
can be moved into other assemblies, and entire assemblies can also be added to other assemblies.
• Selecting Create Assembly in the Parts Display Options menu will open the Create Assembly DEZ.
Figure 173: Create Assembly DEZ
Assembly name
Base level assembly that parts will be added to. If this assembly exists, the selected parts will be
added to it. If the assembly does not exist, it will be created.
Create Assembly by Part Selection
This option allows you to select a set of parts to add to an assembly. Parts that are in existing
assemblies can also be selected. These parts will be moved to the new base assembly. For example,
if the Assembly name is defined as ASSEM2 and a part ASSEM1/PART is selected, the new part
will be moved directly under ASSEM2 (named ASSEM2/PART).
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
183
Display Tree
Create Assembly by Wildcard
This option allows you to select a set of existing parts to add to an assembly. The Wildcard
text to search will be used to compare part names and used to define which parts should be
moved to the defined Assembly name. For example, if the parts BOX_FRONT, BOX_BACK, BOX_SIDE,
INLET, OUTLET exist in a model, then entering the assembly name BOX_ASSEM and entering the
Wildcard text BOX will create an assembly BOX_ASSEM containing the three parts BOX_FRONT,
BOX_BACK, and BOX_SIDE.
Assembly Display Options
Right-click on any assembly in the Display tree to view the Assembly Display options.
Rename
allows you to rename the selected assembly.
Blank
makes the selected assembly invisible.
Show
displays the selected assembly.
Merge to part
merges the constituent parts with the selected assembly.
Create Sub-Assembly
allows you to create a sub-assembly within an existing assembly from a list of selected parts. Selecting
the Create Sub-Assembly option will open the Create Sub-Assembly DEZ.
Figure 174: Create Sub-Assembly DEZ
Sub-Assembly name
specifies the sub-assembly name. The name also indicates the base assembly within which the
sub-assembly is created. For example, the sub-assembly name ASM.1/ASM.2 indicates that ASM.2
is a sub-assembly within ASM.1.
184
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Parts
Create Sub-Assembly by Part Selection
This field allows you to select a set of parts to be added to the sub-assembly. Parts in existing assemblies can also be selected, and will be moved to the new sub-assembly.
Note
Parts can also be moved between assemblies and sub-assemblies by dragging
and dropping within the tree.
Delete
allows you to delete the geometry within the selected assembly.
More Part Display Options
Show All
Shows all parts in the display.
Hide All
Hides all parts in the display.
Reverse Blank All
Reverses which parts are blanked so that blanked parts become visible and visible parts are blanked.
Tip
If you have a large number of parts and want to blank most of them, it may be faster to
select the parts you want visible, then use Blank Select followed by a Reverse Blank
All.
Expand All
Expands the entire Part Tree.
Collapse All
Collapses the Part Tree.
Blank Selected
Blanks all selected parts.
Restrict Selected
Blanks all parts except selected ones.
Delete Empty Parts
Deletes empty parts.
Expose Component Parts
Exposes the hidden component parts created in ANSYS ICEM CFD and makes them available in the Parts
branch of the model tree.
Boundary conditions in ANSYS ICEM CFD are assigned on a per part basis. When loads, constraints,
pressures, forces, displacements, etc. are applied on individual entities, the user usually does not
want to see them as separate parts. So a hidden component part is created and the necessary
boundary condition will be applied to the hidden part. This is usually preferable since it cuts down
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
185
Display Tree
on clutter and these entities can be viewed or adjusted through the Loads or Displacements
branches of the tree. Such hidden parts will be reported when you display the part information
(right-click on a part and select Info from the part display options).
For example:
-----------------------------------------------------------------------------------Info for part GEOM
-----------------------------------------------------------------------------------Geometry Info ---Part contains 6 surfaces; Total surface area is 6.0
Part contains 12 curves
Part contains 8 points
Bounding box around part is {0 0 0} {1 1 1}
Part contains 2 hidden component part(s):
GEOM:FORCE0 contains 1 surfaces
GEOM:TEMP0 contains 1 surfaces
The ':' in the part name GEOM:FORCE0 indicates that the part is a hidden component of the part
GEOM.
However, for various reasons, some users may occasionally want to expose these hidden component
parts as separate parts in the Parts branch of the model tree. This can be done with the Expose
Component Parts option.
When the Expose Component Parts option is used, such parts will be renamed with a '#' replacing
the ':' and they will be available in the Parts Tree.
Part GEOM:FORCE0 renamed to GEOM#FORCE0
Part GEOM:TEMP0 renamed to GEOM#TEMP0
2 part(s) renamed
Figure 175: Using the Expose Component Parts Option
Note
This operation cannot be undone.
Tip
CATIA V5 and other CAD tools use Component Parts for colors, etc. The hidden component
parts are included in the ANSYS ICEM CFD geometry file during conversion. You may
find the Expose Component Parts option useful to expose the hidden color ID as a part
name.
186
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Parts
Move Component Parts
This operation moves the component part into its parent. Unlike Expose Component Parts where
component parts are renamed, the number of parts in the tree is not increased, resulting in reduced
clutter. Following this operation, BCs on the hidden part are ignored. The operation is not reversible.
Edit Attributes
Opens a table of the attributes of all the parts, as shown in the figure below. The part name, color, material, and thickness can be edited directly in the table.
The columns that are grayed out are not applicable for the type of geometry found in that part.
Clicking on the column heading will sort the data in ascending or descending order. Columns can
be toggled on and off by right-clicking on the headings and selecting the desired options. The
column widths can be re-sized by moving the mouse over the column border and dragging it to
the desired width. The vertical grab bar at the right of the table can be dragged aside to reveal the
Display Window.
Figure 176: Edit Attributes
Part Mesh Setup
Opens a table of the Part Mesh Setup options. This form is more efficient for large numbers of parts
than the Mesh > Part Mesh Setup table.
Figure 177: Part Mesh Setup
The columns that are grayed out are not applicable for the type of geometry found in that part.
Clicking on the column heading will sort the data in ascending or descending order. Columns can
be toggled on and off by right-clicking on the headings and selecting the desired options. The
column widths can be resized by moving the mouse over the column border and dragging it to
the desired width. The vertical grab bar at the right of the table can be dragged aside to reveal the
Display Window.
“Good” Colors
Automatically selects new colors for all Parts, trying to pick ones that are easy to distinguish from the
others in use. Normally, the colors are assigned by an algorithm that employs the parts name, thus, the
same family in two different projects will have identical colors. It is not, however, always possible to
make all colors distinguishable from the others that are currently in use and the Good Colors option
provides an alternative.
Color By Material
Assigns colors according to material instead of parts.
Individual Part Display Options
Right-click on any part in the Display tree to view the following display options:
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
187
Display Tree
Info
Reports information about the selected part in the message window. The geometry information reported
includes the number of surfaces, curves, and points contained in the part, the surface area, and the
bounding box extents. The mesh information reported includes the number and the types of elements,
the mesh area, and the bounding box extents. The boundary condition information and information
about hidden component parts (see Expose Component Parts (p. 185)) will also be reported. For example:
-----------------------------------------------------------------------------------Info for part GEOM
-----------------------------------------------------------------------------------Geometry Info ---Part contains 6 surfaces; Total surface area is 6.0
Part contains 12 curves
Part contains 8 points
Bounding box around part is {0 0 0} {1 1 1}
Part contains 2 hidden component part(s):
GEOM:FORCE0 contains 1 surfaces
GEOM:TEMP0 contains 1 surfaces
Mesh Info ---Part contains 1548 element(s)
Part contains types LINE_2 (0) NODE (0) TRI_3 (0)
Mesh area of part is 6
Bounding box around part is {0 0 0} {1 1 1}
Part GEOM contains 2 hidden component parts:
GEOM:FORCE0 contains 232 elements of type(s) TRI_3
GEOM:TEMP0 contains 229 elements of type(s) TRI_3
Boundary Condition Info ---Part GEOM:FORCE0 contains bc type(s) FORCE MOMENT
Part GEOM:TEMP0 contains bc type(s) TEMP
------------------------------------------------------------------------------------
Blank
Blanks the selected part in the display.
Show
Shows the selected part in the display.
Add to Part
Allows you to add entities to an existing part.
Add to Part by Selection
Allows you to add geometry entities to the selected part. Click
entities to be added to the part.
188
(Select entities) and select the
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Parts
Adjust Geometry Names
Adjusts the name(s) of the entities added to the part based on the original part selected. This
option is disabled by default, implying that the original entity names will be retained.
Add to Part by Region
Allows you to add mesh entities within the defined region to the selected part.
Min X, Min Y, Min Z, Max X, Max Y, Max Z
Define the extents of the region.
Include partially enclosed
Allows you to include elements that are partially enclosed by the defined region.
Nodes
Allows you to add nodes within the defined region to the selected part.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
189
Display Tree
1d elems
Allows you to add 1D elements within the defined region to the selected part.
2d elems
Allows you to add 2D elements within the defined region to the selected part.
Blocking Material, Add Blocks to Part
Allows you to add blocks to the selected part. Click
added to the part.
(Select block(s)) and select the blocks to be
Break by connectivity
Creates a sub-part comprising all the surfaces from the selected part. This option is valid only for parts
containing surfaces. The following additional options will be made available for the original part:
Merge to part
Merges the sub-part comprising the surfaces with the original part.
Create Sub-Assembly
Allows you to create a sub-assembly within the part from a list of selected parts. Selecting the Create
Sub-Assembly option will open the Create Sub-Assembly DEZ (see Create Sub-Assembly (p. 184)
for details).
Change Color
Allows you to change the part color to one of your choice.
Rename
Allows you to rename the part.
Delete
Deletes the part.
Parameters
Different solver parameters can be defined to perform different types of analysis. To define a parameter,
go to Solve Options –> Setup Solver Parameters. See Setup Solver Parameters (p. 601) for details. To
edit a parameter, double left-click on its branch in the tree.
190
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Subcases
Figure 178: Parameters Tree
If gravity is defined, either within the boundary conditions in ANSYS ICEM CFD or in an imported file,
it will appear in the Display Tree for editing.
Subcases
Different subcases can be defined to allow you to solve a model for two separate load settings. To
define a subcase, go to the Solve Options tab, and click on Set up a Subcase
shown below.
to open the window
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
191
Display Tree
Figure 179: Create or Modify Subcase Window
ID
Enter the Subcase ID number.
To define Subcase 2, change ID to 2, LOAD to 2 and leave SPC as 1 and also select ALL for DISP, STRESS
and ESE as shown in Figure and then click Apply. Now you can see the Subcases tree by expanding it
in Display Tree which looks as shown in
Figure 180: Display Tree with Two Subcases
192
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Geometry
Figure 181: Geometry Menu
The Geometry tab contains the following options:
Create Point
Create/Modify Curve
Create/Modify Surface
Create Body
Create/Modify Faceted
Repair Geometry
Transform Geometry
Restore Dormant Entities
Delete Point
Delete Curve
Delete Surface
Delete Body
Delete Any Entity
Note
General Naming Convention
Part names and entity names should be less than 64 alphanumeric characters. Names should
start with a letter, not a digit. Evaluators (i.e., “+”, “-”, “/”, and “*”) should not be used in
names because they can be misinterpreted as expressions or as denoting an assembly. Part
names are written with all upper-case characters. Entity names are case sensitive.
Create Point
The different options for creating points are shown below.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
193
Geometry
• Part
The part name for the newly created point. The default naming behavior can be set in Settings >
Geometry Options.
• Name
Enter a name for the point. If no entity name is given, the name of the point will be the part name
with a numeric extension. The default naming convention is described under Settings > Geometry
Options.
Note
This name field is very useful when you want to write a script. You can define a specific
name for a newly created entity through the Name field while writing the script itself
rather than the automatically generated name (which could be different in every session
depending on the order of creation of the entity).
Screen Select
The Screen Select option allows you to select the location of the point by clicking directly on the
display window. A temporary bright yellow point will be generated until you press the middle mouse
button to complete the selection.
• Allow work plane selection
This option allows you to select locations on any entity as well as in space.
Explicit Coordinates
The Explicit Coordinates option allows you to create a point by specifying the XYZ coordinates,
or create multiple points as a function of an equation.
Create 1 point
Enter the X, Y, and Z coordinates of the point to be created.
194
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Point
Create multiple points
Allows you to create multiple points defined by functions of one variable (m). Expressions may include:
+, –, /, *, ^, ( ), sin( ), cos( ), tan( ), asin( ), acos( ), atan( ), log( ), log10( ), exp( ), sqrt( ), abs( ), distance(pt1,
pt2), angle(pt1, pt2, pt3), X(pt1), Y(pt1), Z(pt1). All angles are written in degrees.
m1 m2 ... mn OR m1, mn, incr
There are two possible formats to define the variable m. List format (m1 m2 m3 ... mn) is a simple
list of the variable values, without commas. Loop format (m1, mn, incr) is the first value, last value,
and increment value, delimited by commas. For example, if the variable m has values 0.1, 0.3, 0.5,
and 0.7, this can be represented in both the following ways:
List format: 0.1 0.3 0.5 0.7
Loop format: 0.1, 0.8, 0.2
F(m) –> X
The coordinate X of the points to be created will be calculated as the expression of the specified
function of variable m.
F(m)–> Y
The coordinate Y of the points to be created will be calculated as the expression of the specified
function of variable m.
F(m)–> Z
The coordinate Z of the points to be created will be calculated as the expression of the specified
function of variable m.
Base Point and Delta
The Base Point and Delta option allows you to create a point with reference to an existing point.
Select the base point and enter in the offset along each axis to describe the location of the new point.
Center of 3 Points/Arc
The Center of 3 Points option allows you to select 3 points or locations to define an arc. The
center point, or the point that is equidistant from all 3 points, will be created.
Based on 2 Locations
The Based on 2 Locations option allows you to create a point based on two locations. Select one
of the following two methods:
• N Points
Enter a number (N) of points that you want to create equally spaced between 2 selected locations.
• Parameters
To create a parametric point along a 2-point vector, define the parameter value between 0 and 1,
and select the two points that represent the vector.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
195
Geometry
Curve Ends
The Curve Ends option allows you to select a curve to create points at the 2 ends of the curve.
Specify whether the selected curve is Bspline or Faceted.
For Bspline curves the following options are available.
Curve(s)
Click on the icon and select the curve(s).
How
• Both
This option creates two points at the ends of the curve. The point at the start of the curve
(parameter = 0) will be named by default “pnt.01” and the end point (parameter = 1) will be
named “pnt.02”.
• Min or Max coordinates
These options will create a point at the location along the curve at the specified minimum or
maximum coordinate. For example, if the xmin option is selected, the point along the curve with
the minimum X coordinate will be created.
Note
If xmin = xmax for a curve, xmin will be created at the starting point of the curve and
xmax at the end point. This command creates end points and not the peak points of
the entire curve.
For Faceted curves, the following options are available.
Curve(s)
Click on the icon and select the curve(s).
Angle for curves
Allows you to extract points only for curves with angles greater than the specified angle.
Curve-Curve Intersection
The Curve-Curve Intersection option allows you to create a point at the intersection of two curves.
Select the intersecting curves.
Gap Tolerance
The distance between the two curves should be less than this value to create an intersection point.
196
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Curve
Parameter along a Curve
The Parameter along a Curve option allows you to create a parametric point along a curve, select
from the following two methods.
• N Points
Enter a number (N) of parametric points that you want to create along a curve.
• Parameters
Define the parameter value between 0 and 1, and select the curve.
Project Point to Curve
The Project Point to Curve option allows you to create a point by projecting an existing point
on to curve, select the point and curve. The projection will be normal to the curve.
Project Point to Surface
The Project Point to Surface option allows you to create point by projecting an existing point
on to surface, select the point and surface. The projection will be normal to the surface.
Surface
Select the surface that the point will be projected to.
Points
Select the point(s).
Embed point
If enabled, the projected point will become attached to the surface data and a node will be created at
the projected point when mesh is generated.
Create/Modify Curve
The different options for creating and modifying curves are shown in Figure 182: Create/Modify
Curve Options (p. 197).
Figure 182: Create/Modify Curve Options
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
197
Geometry
• Part
The part name for the newly created curve. The default naming behavior can be set in Settings >
Geometry Options.
• Name
Enter a name for the curve. If no entity name is given, the default naming convention will be followed
as described under Settings > Geometry Options.
From Points
The From Points option allows you to create a Bspline curve by interpolating through n number
of points.
From Points
Click on the icon and select any location on the screen to create points that define a curve.
Arc from 3 Points
The Arc option allows you to create an arc from three points.
From 3 Points
Creates a Bspline arc through three points.
Center and 2 Points
• Radius
If enabled, the radius will be set as the specified value. If disabled, the radius will be set at the
distance between the first two points selected.
• Keep Center or Start/End
The Keep Center option will take the first point selected as the center, the second point as the
first arc beginning, and calculate the arc end from the vector defined by the first point and third
point. The radius used will be determined by the Radius parameter.
The Keep Start/End option will use the first and second points selected as the arc ends and calculate the center using the Radius parameter if specified, or else the average distance between
the first and second points, and the first and third points. The plane will be defined by the three
selected points.
• Points
Select 3 points.
Circle from Center and 2 Points
The Circle from Center and 2 Points option allows you to create a circle of known radius and
center point in a plane.
198
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Curve
• Radius
If toggled ON, the radius will be set as the specified value. If toggled OFF, the radius will be set at
the distance between the first two points selected.
• Start angle
For a full circle, the start angle is 0. Otherwise, specify the desired start angle.
• End angle
The end angle for a full circle is 360, and for a semi-circle is 180.
• Points
The first point selected is the center point of the circle. The next 2 points selected will be used to
define the plane of the circle.
Surface Parameters
The Surface Parameters option creates a curve that follows the parametric path of a selected
spline surface.
• Isocurve Methods
Select from three methods to create the curve.
– Direction on Surface
Select two points to indicate the isoparametric curve used to define the new curve.
– Point on Edges
Select a location on the surface edge to create a curve passing through that location, normal to
the edge. You can select any UV parameters, that is, any surface location, but it will automatically
use the nearest edge (minimum parametrical distance) from the selected location. A green line will
be displayed to indicate the normal direction from the selected edge.
– By Parameter
Select either the U or V direction and the parameter value between 0 and 1 to create an isoparametric curve.
Note
If the UV boundary curve data is corrupted, then the following error message may appear:
“No active isocurve segments found for this parameter.” Use the Geometry > Repair Geometry
> Build Topology function to resolve any gaps in the boundary curves.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
199
Geometry
Surface-Surface Intersection
The Surface-Surface Intersection option allows you to create an isoparametric curve from two
intersecting surfaces. You can choose the option to create a faceted curve, or a Bspline curve.
Surfaces
Isoparametric curves will be created for the intersections of the selected surfaces. If Only Different Parts
is enabled, then curves will be created at the intersections of the selected surfaces from different parts
only. If it is disabled, then curves will be created at the intersections of all the selected surfaces. If no
surfaces are selected, and Apply is pressed, then the operation will be applied to all surfaces.
Parts
This option will apply the function to the selected parts. If Only Different Parts is enabled, then curves
will be created at the intersections of surfaces from different parts only. If it is disabled, then curves will
be created at the intersections of all surfaces within the selected parts. If no parts are selected, and Apply
is pressed, then the operation will be applied to all parts.
2 sets
This option will apply the function to two sets of selected surfaces. Specify the Curve Type, either Bspline
or Faceted. Select the sets of surfaces.
Project Curve on Surface
The Project Curve on Surface option allows you to create a curve by projecting an existing curve
onto a surface. This curve can be used to force nodes and line elements to follow a certain path or to
trim the surface as part of geometry creation or repair.
The following methods are available.
Normal to Surface
The selected curves are projected in a normal direction to each selected surface. Multiple curves and
surfaces may be selected.
Specify Direction
Select one or more curves and one surface. Specify the direction using the drop-down list. The curves
are projected in the specified direction when you click Apply.
• X, Y or Z Direction
Projects the curve onto the surface along the specified vector: X direction (1 0 0), Y direction (0
1 0), or Z direction (0 0 1).
• Screen Normal
Projects the curve based on the screen orientation of the model. The curve is projected in a normal
direction to the screen.
• Along a Vector
Projects the curve to the surface along a vector. Define the vector by selecting two screen locations.
• Keep original
200
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Curve
When enabled, the original curve is kept. When disabled, the original curve is deleted.
• Trim surfaces
When enabled, the projected curve will trim the surface.
Segment Curve
The Segment Curve option allows you to segment an existing curve into new curves. Select from
the following four methods to segment a curve.
• Segment by point
Select the point at which the curve is to be segmented.
• Segment by curve
Select the curve and the location on the curve. The curve will be split at the nearest point of intersection with another curve.
• Segment by plane
Define a plane to segment the curve by selecting an axis normal to the plane and a point on the
plane, or a vector normal to the plane and two points on the plane.
• Segment faceted by connectivity
To split two faceted curves that are merged together.
• Segment faceted by angle
To split a faceted curve by a specified angle value.
Concatenate/Reapproximate Curves
The Concatenate/Reapproximate Curves option merges two or more existing curves into one
new curve. The original curve is deleted. Curves can be merged with the following options:
• Reapproximate Curve
Redefines the curve based on a locally set triangulation tolerance instead of the global tolerance.
Used to create a smoother curve definition.
• Concatenate Curve
Joins the curves selected that are separated by a gap less than the given tolerance limit.
• 2D Hull
Creates a convex 2D hull around the selected curves. The curves are connected into a faceted curve
that does not follow any concave shapes.
– Tolerance
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
201
Geometry
The curve approximation tolerance.
– Max shrink
The relative shrink wrap tolerance. The value entered should be between 0 and 1. A typical value
is 0.2.
– Four curves
This option splits the concatenated faceted curve into four edges so that a surface can be created
from them.
Extract Curves from Surfaces
The Extract Curves from Surfaces option allows you to extract the boundary curves from a surface.
Specify whether the selected surface is Bspline or Faceted.
For Bspline surfaces the following options are available.
Check Topology
If enabled, curves will be created only on surfaces edges that do not have curves attached to them.
Create New
If enabled, a new curve will be created for each surface edge.
For Faceted surfaces the following options are available.
Angle for surfaces
Curves will be extracted only from surfaces with angles greater than the specified angle.
Min number of segments
Only curves with the specified minimum number of segments will be extracted.
Which curve segments
Specify whether curves will be extracted from the interior, exterior, or both sides of the surface.
Modify Curves
Curves can be modified with the following options.
• Reverse direction
switches the direction of curves so that the curve start and end points are reversed. Left click on a
curve and an arrow will indicate its current direction. To reverse the curve direction, confirm by
pressing the middle mouse button.
Note
This function is valid only for parametric (Bspline) curves. Faceted curves must first
be re-approximated in order to change the direction of the curve.
202
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Curve
• Extend
Extends a curve to the specified point or curve, or extends the curve by a designated length.
Extend to Pnt
Extends the curve to a designated point. When the user selects the edge, the end closest to the selected
location is extended. An arrow will indicate which curve end will be extended.
Figure 183: Example of Extend Curve to Pnt
Original Curves
Curve Extended to
Point
Extend to Crv
Extends the curve to another selected curve. The extension is a straight line tangential with the end
of the original curve.
Figure 184: Example of Extend Curve to Crv
Original Curves
Curve Extended to
Curve
Extend to Length
Extends the curve by the specified length. If the curve is not a straight line, it can be extended as an
arc or as a line. You can determine which end is extended during the curve selection.
Figure 185: Examples of Extend Curve to Length as Arc and Line
Extend Curve to Length as an
Arc
Extend Curve to Length as a
Line
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
203
Geometry
During extension, a curve will be created in the direction of the extension. The original and extension curves will then be concatenated and the concatenated curve will be re-approximated
(using an automatically determined tolerance) and replaced.
Note
The re-approximation will use the default topology tolerance if it is smaller than
the automatically determined tolerance value.
• Match curves
Extends curve(s) to match at a point, tangency and/or radius of curvature.
Accuracy
Select the method used to determine the best matching curve. The Geom method performs geometric
matching with internally set factors. The Exact method matches the end point, tangency, and/or radius
of curvature as closely as possible.
Figure 186: Example of Match Curves, Geom and Exact Methods
Original Curves
Geom Method
Exact Method
Curves to Modify
The Both Curves option will adjust both curves to match. The First Curve option only modifies the
first curve selected.
Method
This determines the method of matching the curves. The following methods are available:
204
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Curve
Common end point
Common end point and tangency
Common end point, tangency and radius of curvature
Common end point and radius of curvature
Figure 187: More Examples of Match Curve Methods
Match Curves with Both Curves Option, and
Common End Point Method
Match Curves with Both Curves Option, and
Common End Point, Tangency, and Radius of
Curvature Method
Keep Original
Keeps the original curves and creates new ones to match.
• Bridge curves
Creates a new curve that connects two existing curves keeping tangency of first two curves. The end
that is closer to the location of the cursor when selecting the curves will be the end that is bridged.
The curve magnitude defines how far to keep the tangency as a fraction of curve length from the
start and end point (First and Second Curve, respectively). The magnitude can range from 0 to 1,
where 0 means no tangency is kept for 0 distance, and 1.0 attempts to maintain tangency for the
full curve length.
After selecting the curves to be bridged, you can adjust the curve magnitude by text entry or by
moving the sliders until the desired shape is achieved.
Figure 188: Examples of Bridge Curves
First Curve Magnitude = 0.30, Second Curve Magnitude = 0.30
First Curve Magnitude = 0.50, Second Curve
Magnitude = 0.50
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
205
Geometry
First Curve Magnitude = 0.70, Second Curve Magnitude = 0.70
First Curve Magnitude = 1.00, Second Curve
Magnitude = 0.0
Notice that for the Curve Magnitudes of 0.70, tangency to both curves cannot be maintained for 70%
of the curve lengths, so a compromise is made. For the last example with the First Curve Magnitude
of 1.00, tangency to the first curve is attempted for the full length of the bridge, but it does not
maintain tangency to the second curve.
Create Midline
The Create Midline option creates the midline between two curves or sets of curves.
From 2 Curves
Select two curves and the midline of these curves will be created.
By Pairs
Select two sets of connected curves to create a single midline between them. Each set can contain more
than one curve.
Create Section Curves
The Create Section Curves option creates new curves at the intersection of selected surfaces with
single or multiple planes.
Surfaces
Select the surfaces.
Plane Setup
Specify the planes that intersect with the selected surfaces to create the new curves.
Normal to XYZ Plane
Select the plane normal to the X, Y, or Z axis. The plane will pass through the origin (0, 0, 0).
Start Point / Multiple
This option allows you to define a Start Point through which the plane must pass, and allows
for multiple planes defined by an offset value.
Delta Offset
To define multiple planes, a Start Point and End Point must be defined. The offset value is defined
as a fraction of the distance between the Start and End points. Planes will pass through each
offset point, as well as the Start and End points, resulting in multiple section curves. For example,
if a Delta Offset value of 0.5 is entered, a plane will pass through the Start Point, the End Point,
and the point halfway between the Start and End points.
206
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Surface
Normal to Three Points
Select 3 points to define a plane. The plane normal to this will be used in the creation of the new
curves.
Normal to Existing Curve
Select a curve. The number of sections that is entered will result in equally distributed planes normal
to the selected curve at the local parameter. For example, if a curve that is a circle is selected, and
10 sections are specified, then 10 planes normal to the circle, at every 36 degrees, will be used to
create the new curves.
Create/Modify Surface
The different options for creating and modifying surfaces are shown in Figure 189: Create/Modify
Surface Options (p. 207).
Figure 189: Create/Modify Surface Options
• Part
The part name for the newly created surface. The default naming behavior can be set in Settings >
Geometry Options.
• Name
Enter a name for the surface. If no entity name is given, the default naming convention will be followed
as described under Settings > Geometry Options.
From Curves
The From Curves option allows you to create surfaces from curves. The following options are
available for creating surfaces from curves.
From 2-4 Curves
Select two to four curves to form the boundaries of a surface.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
207
Geometry
Tolerance
Adjacent curve ends must be within this tolerance distance in order for boundaries of the surface
to be created.
Note
This function automatically closes gaps between boundary curves, using a best fit approximation. For the best results, manually connect curves to form a closed loop that can be
specified as the surface boundary.
From Curves
Select any number of curves to form a surface. The curves may be overlapping and unconnected.
From 4 Points
Select four points to define the new surface.
Curve Driven
The Curve Driven option creates a surface by sweeping one or more curves along a Driving curve.
The direction of the Driven curves changes with the curvature of the Driving curve.
Note
This function provides predictable results for relatively simple driven curves that are either
a plane curve or that have a constant curvature. The results may be of lower quality for 3D
curves with variable curvature.
Figure 190: Example of Curve Driven Surface
Sweep Surface
The Sweep Surface option creates a surface by sweeping a reference curve along a vector (Driving
curve). The orientation of the swept curve(s) remain constant, and are swept in the same direction of
the vector or Driving curve.
Screen Vector Method
Define the vector by selecting two points, and select the curve(s) to be swept. The vector will determine the size of the resulting surface. For example, for if the two vectors {0 0 0} and {5 3 2} are
208
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Surface
entered, the curve will be swept such that a surface of 5 units in the X direction, 3 units in the Y
direction, and 2 units in the Z direction will be created.
Driving Curve Method
Select the Driving curve and the curve(s) to be swept. The curve will be swept in the same direction
of the Driving curve, from parameter 0 to 1.
Figure 191: Example of Sweep Surface
Surface of Revolution
The Surface of Revolution option creates a surface of revolution by revolving a reference curve
around an axis with a specified start and end angle. The default start angle is 0, and the default end
angle is 360. More than one curve can be chosen to be revolved around the axis.
Loft Surface over Several Curves
The Loft Surface over Several Curves option creates a surface by interpolating across two or
more curves. The tolerance value determines the degree of approximation. The smaller the tolerance
value, the closer the final surface to the input curves.
Offset Surface
The Offset Surface option creates a new surface by offsetting an existing surface. Enter the distance
to offset the surface normal to the base surface.
Distance
Distance to offset the surface normal to the base surface.
Surfaces
Select the surfaces to be offset.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
209
Geometry
Midsurface
The Midsurface option creates a new surface midway between two existing surfaces or parts.
Midsurfaces can be created with the following options.
Note
After midsurfacing complicated models, gaps may sometimes exist between surfaces. To
close these gaps, the following operations can be used:
Create/Modify Surface > Extend Surface> Extend Curve to Surface(s)
Create/Modify Surface > Extend Surface> Close Gaps Between Midsurfaced Parts
Repair Geometry > Stitch/Match Edges.
By Parts Method
Select the parts for which midsurfaces are to be created for all paired surfaces. Each part should be a
solid part (consisting of surfaces making up a thin solid). The resulting surfaces would represent the
midsurfaces for that part.
• Search Distance
The distance within which candidate pairs of surfaces are searched for. For example, if the Search
Distance is 10, then all pairs of surfaces within 10 units of distance are selected as candidates for
midsurfacing. This value should be slightly higher than the maximum thickness of the entire
model. When this parameter is zero, selecting two surfaces will result in finding the midsurface.
A nonzero value for the search parameter helps the code to find the midsurface automatically
for a large group of surfaces.
• How
This parameter sets the degree by which the operation is interactive.
– Quiet
This is the default setting, in which the operation is automated.
– Confirm
After midsurfacing, any surfaces that have not been successfully paired and midsurfaced will
be presented. You have the option to delete these surfaces (as they may be side surfaces that
should not get midsurfaced), put these surfaces into a subset for further evaluation, or choose
Cancel to ignore them.
– Present/Confirm
Will give you the following options for the pair of surfaces for which you want to generate the
midsurface. Allows you to view the new midsurface before creating it.
→ y = compress
This option will create the midsurface option that is displayed.
→ n = no
210
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Surface
This cancels the midsurface operation.
→ p = partial
This will present the different options available for non-matching surfaces. The partial
option will create a midsurface by projecting the smaller surface in between the two
surfaces. The double partial option will create the midsurface to represent the smallest
common surface area of the two selected surfaces. The non-partial option will create
a midsurface between the entire selected surfaces, not just the overlapping portions.
→ a = surface 1
This option will display alternate midsurface options. For example, if one of the original
surfaces has a hole, the alternate midsurface options allows you to select the midsurface
with or without the hole.
→ d = delete
This option deletes the original surfaces.
• Parts
Clicking on the Parts selection icon will open a pop-up window where the parts for midsurfacing
can be selected.
• Keep original
Keeps the original surfaces after the midsurface creation.
• Delete unattached curves and points
Deletes unattached curves and points.
• Create assemblies
Creates assemblies of the selected parts for the midsurface creation.
• Partial
For non-matching surfaces, if this option is toggled ON, the midsurface will be created only
between the portions that overlap.
Note
For the Confirm and Present/Confirm methods, the partial options are presented
in the display.
• Similar pairs only
Identifies the matching surfaces from the selected surfaces and generates the midsurface accordingly.
• Prefer connected pairs
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
211
Geometry
Is disabled by default. If enabled, connectivity of surfaces over proximity will be used to determine
the best surface pairs for creating the midsurface. Also, if there are no connected surfaces, then
no midsurfaces will be created. If disabled, then the pairs of surfaces used for midsurfaces will
be determined by distance and surface normals.
Note
It is recommended to build topology before using this function.
Note
If Settings > Geometry Options > Inherit part name is set to Create New, and Keep
Original and Create assemblies are both disabled, the newly created midsurface will
be placed in new part. If both options are enabled, the created midsurface will be placed
in the same part, as part of the subset MIDS, and original geometry will be moved to the
subset ORIG in the same part.
By Surfaces Method
Any surfaces can be selected to create a midsurface, independent of which part the individual surfaces
belong to. All possible midsurfaces will be created for the selected surfaces.
See description of options above.
By Pairs Method
Identifies pairs of connected surfaces via flood fill, re-approximates sides with more than one surface,
and then creates a single midsurface between the two sides.
• Side 1 and 2
Specify the different sides of the surface pairs.
• Keep original
Keeps the original surfaces after the midsurface creation.
• Delete unattached curves and points
Deletes unattached curves and points.
• Partial
For non-matching surfaces, if this option is enabled, the midsurface will be created only between the
portions that overlap.
Note
For the Confirm and Present/Confirm methods, the partial options are presented in
the display.
212
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Surface
Segment/Trim Surface
The Segment/Trim Surface option allows you to segment a selected CAD surface by a Bspline
curve. The selected curve must lie on the surface, and must form an enclosed loop if it is fully contained
within the surface boundaries. Surfaces can be segmented by the following four options.
• By Curves
Select the curve(s) to segment the selected surface.
• By Plane
Specify a plane by defining three points on the plane, or by a vector normal to the plane and a point
that the plane passes through. The surface will be segmented by this plane.
• By Connectivity
Segments surfaces that are merged by definition but not physically connected.
Note
This option applies only to faceted data.
• By Angle
Splits the surface by the value of the angle prescribed.
Note
This option applies only to faceted data.
Merge/Reapproximate Surfaces
The Merge/Reapproximate Surfaces option allows you to merge two surfaces at their seam. If
you select NURBS data surfaces, you will be given the option to convert them into faceted data before
merging.
The options for re-approximating surfaces will create one surface from a set of selected surfaces while
re-approximating the surface boundaries to a given tolerance. This is useful for several operations, including the following:
1. To clean up surface data by creating a re-approximated surface from multiple segmented surfaces.
2. To clean up more complicated geometric formats into a more simple surface data structure that is easier
to manipulate. For example, some CAD systems will represent a four sided surface as a trimmed plane.
Re-approximation will create a ruled surface to replace this.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
213
Geometry
3. To convert a faceted surface representation to a Bspline representation if the boundaries of the faceted
surface is well defined.
Note
To perform this operation, Build Topology is necessary.
There are four options to merge surfaces:
• Merge Surfaces
Merges two surfaces that are separated by a gap within the specified tolerance.
• Reapproximate selected surface(s)
Re-approximates the selected surfaces into one surface.
• Reapproximate selected surface(s) bounded by curve(s)
Re-approximates two adjacent surfaces that are joined by a common curve.
• Reapproximate selected surface(s) bounded by hull
Re-approximates surfaces that are bounded by a hull.
– Faceted only
Allows you to select faceted surfaces only.
• Reapproximate each surface
Allows you to choose the automated Quiet option, or the Confirm option that will display the merged
surface before creating it.
– Faceted only
Allows you to select faceted surfaces only.
Untrim Surface
The Untrim Surface option is for spline surfaces only. This option untrims or removes any previous
segmentation of the selected surface(s).
Create Curtain Surface
The Create Curtain Surface option creates a surface extruded from a selected curve and projected
onto a target surface, normal to the target surface.
Select the initial curve and surface, as shown in the example below. The Trim surface option will attempt
to trim the set of surfaces selected to form a T-connection.
214
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Surface
Figure 192: Select Curve and Surface for Curtain Surface Function
The final surface obtained is shown in Figure 193: Curtain Surface (p. 215).
Figure 193: Curtain Surface
Extend Surface
The following options are available for extending surfaces.
Extend Curve to Surface Method
Extends selected curves to selected surfaces. The following methods and options are available.
• Closest
Projects the selected curve(s) to the selected surface(s), and creates new surface(s) normal to the
selected surface(s).
• Tangential from edge
Extends a surface edge to the selected surfaces in a direction normal to the selected edge. The
extension follows the curvature of the original surface.
• Tangential along U/V
Extends a surface edge to the selected surfaces in the u or v direction of the original surface.
• Trim surfaces
Attempts to trim the selected surface(s) to form a T-connection.
• Tolerance
This value is the build topology tolerance.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
215
Geometry
Extend Surface at Edge Method
Extends a surface at the selected edge.
• Surface
Select the surface to be extended.
• Curve
Select the edge at which the surface is to be extended.
• Extension
The relative length of the extension. A value of 0.2 defines an extension of 20% of the original
surface.
• Absolute distance
If this is toggled ON, then the Extension value is taken as an absolute distance instead of a relative
factor.
• Trim surfaces
Attempts to trim the selected surface(s) to form a T-connection.
Close gaps between midsurfaced parts
This function requires connected regions of surfaces to be in separate parts. For each part selected, the
single edges are checked for their proximity to the surfaces of the other parts. If the proximity is within
the specified distance, it will attempt to extend the surfaces in the same way as the Extend Curve to
Surface Method.
• Parts
Select the parts that the surfaces belong to.
• Dist.
Enter the maximum gap distance to be closed.
• Method
– Closest
Projects the selected curve(s) to the selected surface(s), and creates new surface(s) normal to
the selected surface(s).
– Tangential from edge
Extends a surface edge to the selected surfaces in a direction normal to the selected edge. The
extension follows the curvature of the original surface.
– Tangential along U/V
Extends a surface edge to the selected surfaces in the u or v direction of the original surface.
• Preview Vectors
216
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Surface
Displays the possible vectors of the surface extension. You can select individual vectors to Exclude
or Include.
• Extension Arrow Size
Select the vector arrow size.
• Trim surfaces
Attempts to trim the selected surface(s) to form a T-connection.
• Tolerance
This value is the build topology tolerance.
Geometry Simplification
The Geometry Simplification option creates a set of faceted surfaces wrapped around the selected
geometry, including surfaces, curves, or points. The original geometry is retained.
Convex Hull Method
There are 3 methods to choose from, single hull, interactive split and regular split.
For faceted data, it may be helpful to first merge all surfaces, and then merge all nodes of the concatenated surface within a tolerance. This will reduce the computation time.
There are three different options for the Convex Hull Method.
• Single Hull
Creates a crude wrapped surface around the actual selected surfaces as shown in Figure 195: Single
Hull Option (p. 218).
Figure 194: Example Geometry
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
217
Geometry
Figure 195: Single Hull Option
• Interactive Splits
In this method, you will be prompted to draw lines representing split planes. These planes do not
need to be aligned with the global axis.
Figure 196: Split Planes
218
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Surface
Figure 197: Interactive Splits Method
• Uniform Splits
In this method, a uniformly spaced grid of planes is used to segment the actual selected surfaces
and a hull is then created around each segment. You must define the number of planes in the X, Y
and Z directions. The planes (X, Y, Z axes) are either aligned to the global coordinate system (the
Model option) or to that of the current Screen orientation, with the X-axis horizontal, Y-axis vertical,
and Z-axis normal to the screen. A large number of planes will create a three-fold large number of
segmented components, which may take a long time to process for complicated geometry. For example, a 10 x 10 x 10 grid will create 1000 components.
Coarsen before Creating Hull
Faceted entities will be coarsened to reduce the triangulation and the processing time.
Tolerance
Edges of the faceted triangles will be merged within the tolerance setting during the coarsening process.
The value is an absolute setting.
Remove Interior Faces
If enabled, the interior hull surfaces of segments created by the Interactive Splits or Uniform Splits
methods will be removed. Only the outer shell formed around the selected surfaces will be retained.
Hull for Each Part
Each segment created after a hull is built around a component will be put into a new part.
Cartesian Shrinkwrap
Wraps a complicated geometry using a Cartesian staircase mesh. The mesh is then locally projected
and smoothed to get a simplified representation of the geometry.
Note
For the resulting mesh, if surfaces mesh sizes are set, then this will override the global max
size value.
The following options are available:
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
219
Geometry
Max. cell size
The size of the facets of the shrinkwrap. This should be set to just a little larger than the largest hole
you want to ignore.
Num. of smooth iterations
Number of smoothing iterations to be performed.
Surface projection factor
Factor from 0 to 1 that determines how well the shrinkwrap will project to the geometry after the staircase
mesh is created.
Part for envelope
Determines the Part that the Shrinkwrap will be created in. You can select an existing part, use the screen
select to select a part on the screen, or type in a new part name in the field. The inherited option will
place the shrink wrapped mesh in the same part as the geometry that it lays on, this is determined by
a normal vector ray calculated from each facet.
Wrap part by part
Creates an individual shrinkwrap per part.
Active parts only
If enabled, then shrinkwrap will only be applied to the active parts.
Create Geometry
If disabled, the wrap produced is mesh. If enabled, the wrap is automatically converted into a faceted
geometry. When used in conjunction with the inherited option for Part for envelope, the Part names
for the new geometry entities will be the inherited names followed by “_WRAP” to differentiate them
from the original geometry.
Figure 198: Engine Geometry (p. 220) shows an engine geometry. Such engine geometries may have
much more detail than is needed for an under hood analysis and can be simplified. The geometry
can be wrapped to close holes, combine parts, and generally simplify the data as shown in Figure 199: Wrapped Engine (p. 221).
Figure 198: Engine Geometry
220
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Surface
Figure 199: Wrapped Engine
The wrapped surface mesh can then be used with a bottom-up tetra method to generate a volume
mesh or converted to faceted geometry as described.
Figure 200: Mesh with Volume Mesh Cut Plane
Standard Shapes
The Standard Shapes option creates standard geometrical shapes. The following options are
available.
Figure 201: Create Standard Shapes Options
Box
There are two methods to creating a box.
• Specify
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
221
Geometry
Define the lengths of the box sides in the X, Y, and Z directions and select the point for the box
origin. For example, an X Y Z size of “1 1 1” and Box Origin “0 0 0” will result in a box with sides
of length one, with its origin at the coordinates (0,0,0).
• Entity bounds
Creates a bounding box around the selected entities. The X, Y, and Z lengths of the box can be
scaled by the specified factor.
– Adjust min/max values
If this is enabled, the minimum and maximum coordinate values of the box will be displayed. To create a new box, you can change any of these values and click Apply.
Sphere from 2 points
• Radius
If enabled, then the radius length can be defined.
• Start/End angles
The angles (in degrees) are measured from the normal of the center plane of a sphere (the pole).
An arc from the Start angle to the End angle will be rotated 360 degrees. For example, a Start
angle of 0 and an End angle of 90 will result in the top half of a sphere.
• Locations
You will be prompted to select two locations on the screen. The first is the center of the spherical
surface, and the second defines the normal of the center plane (pole). If Radius is toggled OFF,
then the second point will determine the length of the radius as well.
Cylinder
• Radius1 and 2
Specify the Radius1 and Radius2 of the respective base circles of the cylinder.
• Base1 and Base2
If enabled, the respective bases circles will be created.
• Two axis Points
Select two points to define the axis of the cylinder.
Drill a Hole
• Surface
Select the surface in which the hole is to be drilled.
• Remove Hole
222
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Surface
Enable if you wish to replace a current hole. This will allow you to select a curve (hole) which will
be deleted and replaced with the new specified hole. If no curve is selected, the last hole created
will be removed.
Note
If Remove Hole is enabled, and the selected curve is a feature and not a hole,
that curve will still be removed.
• Radius
Enter the radius length.
• Location
Select the point of the center of the hole.
Plane normal to curve
• Side
Enter the length of the side for the uniform surface.
• Location on curve
Select the location on the curve at which the normal plane is to be created.
• Curve parameter
Instead of selecting the location on the curve, the distance along the curve can be specified.
Disc normal to curve
• Radius
Enter the radius length for the disc.
• Location on curve
Select the location on the curve at which the disc is to be created.
• Curve parameter
Instead of selecting the location on the curve, the distance along the curve can be specified.
Trim normal to curve
Creates a plane normal to the selected curve and trims this plane with the selected surface(s). The plane
will only be created if the intersection curve of the plane to be created and the selected surfaces is a
closed loop.
Surfaces
Select the surface that will be used to trim the newly created plane.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
223
Geometry
Location on curve
Click on the selection icon and select the location on the curve where the plane will be created. Click
on Apply to create the plane.
Curve parameter
To specify the location on curve using the curve parameter (between 0 to 1), select any location on
the curve, enter the curve parameter, and click Apply.
In the example in Figure 202: Surfaces and Curve Selection (p. 224), the top and bottom surfaces of
the hemisphere are selected. And the point on the curve is selected for the creation of the plane.
In the second figure, note that the created plane's intersection with the selected surfaces creates a
closed loop.
Figure 202: Surfaces and Curve Selection
Figure 203: Trim Normal to Curve – Plane Creation
Create Body
Bodies can be created from surfaces that make up a volume. The different options for creating
bodies are as follows:
By Topology
By Material Point
• Part
224
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Body
The part name for the newly created body. The default naming behavior can be set in Settings >
Geometry Options.
• Name
Enter a name for the body. If no entity name is given, the default naming convention will be followed
as described under Settings > Geometry Options.
By Topology
Bodies can be created by topology either from the Entire Model or from Selected surfaces. There
must not be any gaps in order for a body to be created.
The default part name will be BODY, unless you enter another part name. If no entity name is given,
the name of the body to be created will be the part name plus a numeric extension.
Note
In order to import Tetin files from ANSYS ICEM CFD into the Mechanical application or the
DesignModeler application, use the Entire Model option to build bodies from the topology
first.
Note
A body will be created for each closed volume. In the example geometry shown below, if
the Entire Model method is chosen, or if all the surfaces are selected with the Selected
surfaces method, two bodies will created from the two closed volumes. Each body can then
have separate volume meshes.
Figure 204: Create Body by Topology
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
225
Geometry
Figure 205: Volume Mesh of Separate Bodies
By Material Point
Bodies can also be defined by specifying a Material Point within a closed volume. Material Points
can be created at a specified point or at the centroid of two points.
Note
If a material point is specified at the centroid of the cube in the example geometry below,
then the body will be defined as inner cube. A volume mesh can be generated for the body
as shown below.
Figure 206: Creating Material Point
226
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Faceted
Figure 207: Volume Mesh of Defined Body
Create/Modify Faceted
The Create/Modify Faceted option allows you to create/modify faceted curves and surfaces. Faceted
curves and surfaces can be created and modified with the following options.
Create/Edit Faceted Curves
Surfaces
Faceted Cleanup
Figure 208: Creat/Modify Faceted DEZ
• Part
The part name for the newly created entity. The default naming behavior can be set in Settings >
Geometry Options.
• Name
Enter a name for the faceted curve or surface. If no entity name is given, the default naming convention
will be followed as described under Settings > Geometry Options.
Create/Edit Faceted Curves
Faceted curves can be created and edited with the following options.
Convert from Bspline
Create Curve
Move Nodes
Merge Nodes
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
227
Geometry
Create Segments
Delete Segments
Split Segment
Restrict Segment
Move to New Curve
Move to Existing Curve
Figure 209: Create/Edit Facted Curves Options
Convert from Bspline
The Convert from Bspline option converts Bspline curves to faceted curves.
Create Curve
The Create Curve option creates a faceted curve from specified locations.
Move Nodes
You can move nodes with any of the following options. After choosing the option, click Apply.
Screen
Select the curve, and then click and drag the node to the desired location.
Location
Specify the node and its new location.
Plane
A node can be moved along a plane normal to a specified axis or vector. Define the plane by choosing
the normal axis or vector, and click Apply. Select the curve, then click and drag the node.
Surface
The node of a curve can be moved along a constraint surface. Select the curve and the surface, then
click and drag the node of the curve along the surface.
Line
A node can be moved along a certain line. Specify the line by choosing two points and clicking Apply.
Select the curve, then click and drag the node along the line.
Offset
Specify the offset in the X, Y, and Z directions to move the node.
228
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Faceted
Merge Nodes
A node can be merged to a selected point on another curve. First select the faceted curve, followed
by the reference curve. Then the fixed point on the reference curve has to be selected. After that the
node selected on the first faceted curve merges with the point selected on the reference curve.
Create Segments
The Create Segments option allows you to add segments to an existing curve. First select a curve
to which the new segments will be added. Then select points on the screen to create the segments.
The selection is in continuation mode: each point selected adds to the segment, until the middle mouse
button is pressed. The points are not constrained to existing nodes; rather they are constrained to any
location on the visibly displayed geometry.
Delete Segments
The Delete Segments option allows you to delete segments from an existing curve. First select
the curve to edit, then select the segments to be deleted from that curve.
Split Segment
The Split Segment option splits selected segments of the selected curve into two. Split location
is at the middle of the element.
Restrict Segment
Select the curve and then select the segment on the curve to be displayed, while the display of
all the other segments of the curve will be restricted.
Move to New Curve
The Move to New Curve option moves the selected segments to a new curve. Select the curve
and then select the segment to move
Move to Existing Curve
The Move to Existing Curve option moves the selected segments to a n existing curve. Select
the initial and destination curves, then click and drag the curve to the new location.
Surfaces
Faceted surfaces can be created and modified with the following options:
Convert from Bspline
Coarsen Surface
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
229
Geometry
Create New Surface
Merge Edges
Split Edge
Swap Edge
Move Nodes
Merge Nodes
Create Triangles
Delete Triangles
Split Triangles
Delete Non-Selected Triangles
Move to New Surface
Move to Existing Surface
Merge Surfaces
Figure 210: Create/Modify Faceted Options
• Part
The part name for the newly created surface. The default naming behavior can be set in Settings >
Geometry Options.
• Name
Enter a name for the surface. If no entity name is given, the default naming convention will be followed
as described under Settings > Geometry Options.
Convert from Bspline
The Convert from Bspline option converts a CAD (Bspline) surface into triangulated surface data.
You have the option to delete the old CAD surfaces.
230
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Faceted
To reconvert the faceted surface into a Bspline surface, see Geometry > Create/Modify Surface >
Merge/Reapproximate Surfaces.
Note
Converting a faceted surface to a Bspline surface is a difficult operation and requires
the boundaries of the faceted surface to be well defined.
Coarsen Surface
The Coarsen Surface option reduces the number of triangles on a faceted surface. This option is
useful for reducing the amount of data. After the surface is selected, you will be prompted to select
curves and then points in order to maintain the sharp features of the surface. Otherwise, the original
surface integrity may not be maintained. The curves and points that have been extracted from the selected surface by one of the following methods should be selected:
Create curve > Extract from surface
Create curve > Build topology
Repair Geometry > Create topology
Create point > Extract from curve
Tolerance
Distance within which to merge nodes of the surface. Default is 1/10th of the Min edge length. The
Min edge value is the length of the shortest edge on the selected surface. The tolerance value is a
maximum deviation from the original surface triangulation.
Create New Surface
The Create New Surface option allows you to create a new faceted surface from three selected
points, three locations selected on the screen, or from edges.
The following options are available when creating faceted surfaces using the From edges method:
Allow internal edge selection
If enabled, this allows the selection of non-single (internal) edges to create a new surface. Internal edges
have more than one adjoining triangle.
Complete edges
If enabled, this allows selection of edges that are not connected.
Merge Edges
The Merge Edges option merges one set of edges to another set of edges in faceted surfaces by
aligning and merging the edge nodes.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
231
Geometry
Allow internal edge selection
If enabled, this allows the selection of non-single (internal) edges to be merged. Internal edges have
more than one adjoining triangle.
Merge tolerance
Merges edges that lie within the specified tolerance of each other.
Merge ends
If enabled, the starting and end nodes of the edges will be merged. If disabled, the starting and end
nodes will not be affected.
Split Edge
First select the surface, then the edge to be split. The selected edge and the adjacent elements
will be split into two, as shown in the example.
Figure 211: Edge Selected to Split
Figure 212: Split Edge
Swap Edge
The Swap Edge option swaps edge of two adjacent triangles. The original edge will be replaced
by an edge that connects the other two corners of the triangles, as shown in the example.
232
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Faceted
Figure 213: Edge Selected to Swap
Figure 214: Swapped Edge
Move Nodes
You can move nodes of faceted surfaces with any of the following options. After choosing the
option, click Apply.
Location
Moves nodes to a selected location on the geometry. First select any location on the geometry, then
select the nodes to be moved and press the middle mouse button.
On screen
Moves nodes anywhere on the plane defined by the screen. Select the surface, then click and drag the
surface node.
On plane
Moves nodes on a plane intersecting the node and normal to a specified axis or vector. First, select the
surface, describe the plane within the menu, and then move the click and drag the node on that plane.
Normal
Define the plane to move the node by typing in the i j k values of the normal of the plane within the
box.
Offset XYZ
Specify the offset in the X, Y, and Z directions to move the node.
Line
A node can be moved along a certain line. Specify the line by choosing two points and clicking Apply.
Select the surface, then click and drag the node along the line.
Merge Nodes
The Merge Nodes option merges nodes from one surface with nodes on another surface.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
233
Geometry
Screen
Merges two or more nodes together. First select the surface with the nodes that are to be merged. Then
select the reference surface(s). Select a point on the reference surface to merge the nodes with. Then
select the nodes to be merged, and click the middle mouse button to accept. Pressing the middle mouse
button twice will exit from the function.
Tolerance
Merges nodes that lie within the specified tolerance of each other. This is useful for reducing data.
Other faceted editing functions and repair methods will also be more robust if duplicate nodes within
a surface are removed.
Create Triangles
First select a surface to which the new triangles will be added. Then select three points on the
screen to create the triangles. The points are not constrained to existing nodes, but can be at any location
on the displayed geometry.
Note
Selecting nodes for creating faceted triangles requires solid or solid/wire display mode for
surfaces.
Delete Triangles
Select the surface to edit (the surface facets will be displayed in white), then select the triangles
to be deleted from that surface.
Figure 215: Triangle Selected to be Deleted
There are two options for deleting triangles:
Delete Selection
Deletes only the selected triangle.
234
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Faceted
Figure 216: Delete Selection
Keep Selection
Retains the selected triangle and deletes the rest of the surface.
Figure 217: Keep Selection
Split Triangles
The Split Triangles option splits selected triangles into three triangles. The split location is at the
centroid of the element.
Figure 218: Triangle Selected to be Split
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
235
Geometry
Figure 219: Triangle Split
Delete Non-Selected Triangles
The Delete Non-Selected Triangles option deletes the triangles that are not selected.
Move to New Surface
The Move to New Surface option creates a new surface from the selected triangle(s).
Move to Existing Surface
The Move to Existing Surface option moves the elected triangle(s) to an existing surface.
Merge Surfaces
The Merge Surfaces option merges two faceted surfaces.
Faceted Cleanup
Faceted surfaces can be cleaned up with the following options:
Align Edge to Curve
Close Faceted Holes
Trim By Screen
Trim By Surface Selection
Repair Surface
Create Character Curve
236
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Faceted
Figure 220: Faceted Cleanup Options
Align Edge to Curve
There are three different alignment methods.
Align to Curve
Projects the nodes of the selected surface edge to the nearest location on the selected curve. You will
be prompted to select the surface, the curve, and the boundary edge(s) of the selected surface to align
to the curve. The nodes attached to the edges will be projected to the nearest location on the curves.
Project Node to Curve
Projects the selected nodes of the selected surface to the nearest location on the selected curve. You
will be prompted to select the surface, the curve, and the nodes of the selected surface to align to the
curve. This option allows you to select any nodes on the surface in comparison to the Align to Curve
method, where only boundary edges/nodes can be moved. The nodes selected will be projected to the
nearest location on the curves.
Smooth Edges
This option will take a set of boundary edges and smooth out the transition along the edge. You will
be prompted to select a surface, and a set of boundary edges of the surface. The software will internally
create a temporary Bspline curve through the nodes of the edges using the tolerance value entered for
Smooth Tol, and project the nodes to this smoothed Bspline. By adjusting the Smooth Tol value you
can adjust the transition of the boundary edges.
Close Faceted Holes
The Close Faceted Holes option creates new triangles to fill in the gap between a selected set of
curves or edges. Select the boundary edges of the hole. The selected curves or edges do not necessarily
have to form a closed loop.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
237
Geometry
Trim By Screen
The Trim by Screen option cuts a hole through surfaces using points selected from the screen.
Select points on the screen to draw the hole on a surface and to cut the hole through all the surfaces
below it.
Trim By Surface Selection
The Trim by Surface Selection option cuts a hole through surfaces using points on a surface.
Select points on the surface to create the hole.
Repair Surface
The Repair Surface option creates a Bspline patch to replace an area of the faceted surface. You
can define the perimeter of the patch by selecting locations. The patch is projected to the faceted surface.
The faceted surface is then cut out and replaced with a Bspline patch. Figure 221: Using the Repair
Surface Option (p. 238) shows the use of this option to patch holes in the surface mesh.
Figure 221: Using the Repair Surface Option
238
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create/Modify Faceted
Surf Locations
allows you to select the faceted surface and then select locations on that faceted surface to define the
patch to be replaced.
Curve Shape
determines how the surface locations are used to define the patch (see Figure 222: Options for Curve
Shape (p. 239)).
• Lines: Locations are connected by straight lines.
• Smooth : Locations are connected by a smooth curve.
• Circle : First three locations are used as three points on a circle. The circular shape is then projected
to the faceted surface to determine the final patch.
Figure 222: Options for Curve Shape
Keep original
allows you to keep the original faceted surface patch under the Bspline surface patch.
Create Character Curve
The Create Character Curve option creates a Bspline patch to replace an area of the faceted
surface where two features join. This can be a sharp, smoothed or arc (fillet) connection. You can define
the rough character line and how far on either side of this line should be used to make the patch. An
array of faceted surface locations on either side of the character line are determined and smoothed out
to create a smoother surface. These are then used to extract an intersection curve to define the theoretical intersection of the character curve. Finally, the faceted surface within the character curve area is
replaced with the Bspline surface.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
239
Geometry
Figure 223: The Create Character Curve Option
Figure 224: Replacing a Faceted Fillet Using the Create Character Curve Option (p. 240) shows the use
of this option to replace a faceted fillet with a smoother Bspline fillet.
Figure 224: Replacing a Faceted Fillet Using the Create Character Curve Option
PreCurve
allows you to select locations along the character line you want to capture.
PreSides
allows you to select two locations, one in each plane on either side of the character curve. This determines
how far from the character curve the Bspline patch extends in each direction.
Curve Shape
determines how the surface locations are used to define the PreCurve.
• Lines: Locations are connected by straight lines.
• Smooth : Locations are connected by a smooth curve.
240
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Repair Geometry
• Arc : First three locations are used as three points on a circle. The arc is then projected to the faceted
surface to determine the curve.
Show Presurface
shows a preview of the Bspline surface before applying the function.
Note
This was part of the Mesh Prototyper product functionality and the algorithm includes
other options which can be scripted for.
Repair Geometry
The main objective in CAD repair is to detect and close gaps between neighboring surfaces (faces).
Typically, the procedure for geometry repair is as follows:
1.
Build Topology builds curves and points, which will help to diagnose the model for geometrical problems.
The curves will automatically take on colors to show their association to adjacent surfaces.
2.
Repair any gaps or holes in the topology.
The options for repairing geometry are outlined in subsequent sections.:
Build Topology
Check Geometry
Close Holes
Remove Holes
Stitch/Match Edges
Split Folded Surfaces
Adjust Varying Thickness
Make Normals Consistent
Feature Detect Bolt Holes
Feature Detect Buttons
Feature Detect Fillets
• Part
The part name for newly created curves and points. The default naming behavior can be set in Settings
> Geometry Options.
Note
Existing entities will keep their names and parameters.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
241
Geometry
Build Topology
The Build Topology option creates a series of curves and points from surface edges and corners
depending on the proximity of the surface edges to each other. If the curves are within a geometric
tolerance, they are merged together as one. The curves are then displayed in a specific color to illustrate
their connectivity in the surface data, which can be used to determine any gaps or holes in the geometry.
Note
Dormant Entities
Curves and points can be made dormant either by deleting them with the Delete permanently option disabled, through building topology with feature angle and filter
points/curves enabled, or through feature detection tools. If a curve or point is dormant,
it will not be recreated when building topology, but build topology may make it active.
If a curve or point is permanently deleted, it is removed from the database. If the topology is rebuilt, the curve will be recreated. Flood fill, and patch based meshing will also
fail across a boundary (curve or point) that has been permanently deleted. Curves and
points that are unattached to surfaces or curves will always be permanently deleted, as
the sole purpose of dormant curves and points is to maintain connectivity between attached geometry.
Note
Embedded Entities
Points that are within the build topology tolerance from a surface, and curves that are
parallel to a surface within the build topology tolerance and not on the boundary of
the surface will be embedded into the surface. If a point or curve is embedded or linked
to the surface it means that the surface has connectivity to these curves and points. The
patch dependent mesher requires this connectivity to include the curve/point as a
boundary to the mesher. An embedded curve or point is different than a boundary
curve or point in that it is doubly connected to the surface instead of having a single
connection like a boundary entity. An embedded curve is connected to the surface twice
(on positive and negative sides of the surface), whereas the boundary curves are only
attached to the surface on one side.
If the embedded curve is attached to a second surface, the embedded curve becomes
a multiple edge, and defines a T-connection. Typical T-connections connect 3 surfaces,
but since in the case of an embedded curve the underlying surface is not fully trimmed,
the doubly connected edge helps represent the geometry in a more accurate fashion.
That is, the connection is defined to the positive and negative side of the base surface
and to the boundary of the second surface.
Table 4: Build Topology Colors
Yellow
Single or free edge curves (those adjacent to only one
surface)
Red
Double edge curves (curves adjacent to two surface)
242
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Repair Geometry
Blue
Multiple edge curves (curves adjacent to three or more
surfaces)
Green Unattached curves (not attached to any surface)
Topology can be built with the following options.
Tolerance
The tolerance is defined in units of the model, and controls how accurately you want to treat surfaceto-surface proximity. The tolerance between two surfaces is shown in Figure 225: Tolerance (p. 243).
Figure 225: Tolerance
For any two faces (surfaces) that meet at a common edge (curve), there is typically a finite distance
between the two edges. By default, a curve is associated with all the edges of each face. In the figure
above, a curve would be associated to edge 1, and a second curve would be associated to edge 2.
This topology of the two surfaces would indicate a gap in the model.
Typically, ANSYS ICEM CFD meshers can handle this if the gap is smaller than the proposed element
size on the surfaces or curves. Therefore, you would set a tolerance larger than the gap if you are
using a large element size. A tolerance smaller than the gap would create yellow curves which could
be fixed.
The recommended tolerance is approximately 1/10th the size of the average mesh size.
Filter by angle
Filtered curves are made dormant if the surfaces on either side meet at less than the specified angle.
Filtered points are made dormant if the curves on either side meet at less than the specified angle.
Feature curves and points that meet at greater than the specified angle remain. Since Octree Tetra forces
the mesh to respect curves and points, removing unnecessary ones increases the patch independence
and mesh quality. Points or curves (even double yellow curves) can also be deleted manually for the
same purpose.
Filter points
Enabling this option will filter points by the angle between their respective curves, as long as the angle
is not zero.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
243
Geometry
Filter curves
Enabling this option will filter curves by the angle between their respective surfaces, as long as the angle
is not zero.
Method
Topology can be built for All parts, Only visible parts, or by Selection of specific entities.
Note
The All parts option is different from choosing the Selection Method and then Select
all appropriate objects (key = a), and will yield a different result. The All parts option
includes dormant entities, but the Selection Method > Select all appropriate objects
does not include dormant entities.
Part by part
The topology is built part by part.
Single curve cleanup
Enter a value for the Single Edge Tolerance. This option will merge single curves only that are within
the Single Edge Tolerance distance of each other.
Note
This is useful for certain models with small features, where the Build Topology Tolerance
must be kept smaller than those features. In such cases, larger gaps with single edges
can be cleaned up with this option.
Split surface at T-connections
Surfaces that form a T-connection will be split and trimmed at the common edge. When meshed, the
mesh will conform to the common edge.
Split facets at interior curves
Faceted surfaces are trimmed along interior curves that do not span the surface or form a closed loop.
When meshed, the mesh will conform to the interior curve.
Join edge curves
Combines edges with the defined angle to concatenate smaller curves into a single curve. This option
applies to both Bspline and faceted data.
Delete unattached curves and points
Deletes any green curves and unattached points. Sometimes you may keep these since they could be
used as construction curves.
Keep dormant as dormant
Entities that were made dormant by the user will be kept dormant when the topology is built.
Use Local Tolerance
This option enables Build Topology to use a local tolerance, relative to edge length, that prevents merging
away small features that are smaller than the global Build Topology tolerance.
This option is useful if a model has a range of scales and the tolerance required for most of the
model causes important small features to be corrupted. The model shown in Figure 226: Model with
Small Feature (p. 245) has an important feature which is highlighted.
244
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Repair Geometry
Figure 226: Model with Small Feature
If the Build Topology tolerance is set to a value larger than the local feature edges, the defined
tolerance may be ignored locally by disabling this option.
Figure 227: Use Local Tolerance Option
(A) Use Local Tolerance enabled
(B) Use Local Tolerance disabled
Check Geometry
The geometry can be checked by all parts, only visible parts, selected parts, or selected surfaces.
The following methods and options can be used to check the geometry.
Results Placement
specifies how the results will be placed. The surfaces that are found can be shown, placed in a specified
part, or in a specified subset.
Check Surfaces
• Edges
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
245
Geometry
Specify whether the geometry should be checked for Single edges or Multiple edges.
• Curvature/Area
If Curvature is selected, specify a High or Low curvature and a Ref. Angle. Surfaces with curvatures
higher or lower than the reference angle will be found. For example, if a Low curvature of 5 degrees
is specified, all surfaces with curvature less than 5 degrees will be found.
If Area is selected, specify Large or Small, and the Ref. Area. If Large is selected, then surfaces
that have an area larger than the Ref. Area will be found, and if Small is selected, then surfaces
that have an area smaller than the Ref. Area will be found.
• Normal
This will find all surfaces with a normal within the tolerance angle from the specified axis.
Close Holes
The Close Holes option closes holes in the surface by creating a new surface. The necessary condition for closing the hole is that the curve must form a closed loop.
Figure 228: Example of Closed Hole
Curves
Select the curves representing the edges of the hole. After clicking Apply, confirm by pressing Y.
Multiple Holes
If there is more than one hole, you can select the curves for all the holes at one time. But the holes will
be closed individually.
Remove Holes
The Remove Holes option removes the hole composed of curves that form a continuous loop. A
new surface is not created, as with the Close Holes operation. Instead, the trim features adjacent to
the selected curves are deleted.
246
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Repair Geometry
Figure 229: Example of Removed Hole
Stitch/Match Edges
The Stitch/Match Edges option stitches or matches edges separated by a gap. Select a pair of
curves or multiple pairs of curves to fix. The curve pair will be highlighted in white and will automatically
fit to the screen. If multiple pairs have been selected, after each pair is fixed, the next pair will then be
highlighted and fit to the screen. The following methods can be used to stitch or match edges:
User Select
After selecting curves, enter the appropriate key to select from any of the methods of stitching or
matching edges: (n)o change, (f )ill, (b)lend, (t)rim, (m)atch, (a)uto, or (x) for cancel. Each method is explained below. The User Select method is useful when employing a series of different options.
Match
Adjacent surfaces are modified so that one edge matches the other.
Extend/Trim
Recalculates the intersection of the two adjacent surfaces of a gap. Recommended if one or both of the
edges appear jagged.
Figure 230: Surfaces Before Extend/Trim
Figure 231: Trimmed Surfaces
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
247
Geometry
Fill
Creates surfaces to fill in a gap. The surfaces are created between a calculated center point and the selected curves. This is recommended for curve pairs that are more or less coplanar. Any overlap using
this method can usually be ignored.
Blend
Creates a ruled spline surface between the curves. Recommended for curve pairs that are not co-planar
and that have a high degree of curvature.
Figure 232: Blend method
n = no change
No repair is attempted. If fixing multiple pairs of curves, the next pair will be presented. If only one pair
of curves was initially selected, you can select a new set of curves.
a= auto
Automatically determines the best method, fill, blend, trim or match, to fix the gap or hole.
x= cancel
No repair is attempted and the operation is ended.
p = set/unset partial
Enable or disable for whole or partial fixing of the gap. If this is enabled (prompt will read Unset
partial), matching will project the ends of the shorter edge normal to the larger edge instead of
stretching it to match the entire larger edge; fill or blend will create a surface between the smaller
edge and normal projection to the larger edge.
The different parameters for the Stitch/Match Edges operations are described below.
Max Gap Distance
This should be slightly more than the maximum gap between any two surfaces of the entire model. This
option is available for the User Select method.
Single curves only
allows you to restrict to single curves only. This option is available for the User Select method.
Partial
Enable or disable for whole or partial fixing of the gap. If this is enabled, (prompt will read Unset partial),
matching will project the ends of the shorter edge normal to the larger edge instead of stretching it to
match the entire larger edge; fill or blend will create a surface between the smaller edge and normal
projection to the larger edge. This option is available for the Match, Fill, and Blend methods.
Confirmation
After the repair option is selected, the result will be made visible. You need to give confirmation after
viewing the result.
248
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Repair Geometry
y = yes
Saves the change.
n = no
The change is not saved.
r = retry
To retry repair by selecting a different repair method.
Using Stitch/Match Edges for Y-Junctions
The following example shows how to use Stitch/Match Edges to close gaps in T- or Y-junctions, as
shown in the figure below.
Figure 233: Example of Y-Junction with Gaps
First, select the three curves that need to be stitched to close the gap. Select the Extend/Trim method.
This will trim and stitch two edges together and then automatically connect the third surface. The result
is shown below.
Figure 234: Y-Junction with Stitched Edges
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
249
Geometry
Split Folded Surfaces
Folded surfaces are segmented and new curves created where the surface is folded at an angle
greater than the specified Max angle. It will help the surface Mesher (Shell) as additional curves are
placed on the surface. The Max angle option measures from each end of the surface. The first point,
from one edge, whose tangent deviates more than specified angle (default is 90 degrees) splits the
surface. For a cylinder, this will generate more than one curve.
Adjust Varying Thickness
The Adjust Varying Thickness option allows you to assign a thickness to the selected surface
using the following methods:
From Solid Method
Specify Corners Method
Find Surfaces Without Thickness Assigned
From Solid Method
This option assigns thickness values to a surface based on the midsurface/solid model.
Midsurface(s)
Select the set of midsurfaces.
Solid surface(s)
Select the set of surfaces on both sides of the midsurface(s).
Max thickness
Limits the thickness assigned to a surface. The thickness values get assigned at certain control points
along a surface. Each control point thickness is found by projection normal to the surface in either direction. The sum of these projections (positive or negative) define the thickness. An empty (default) Max
thickness value means that there is no thickness limit.
Note
Thickness computations could be inaccurate if the surface data is not very good and a
control point projection is not projected correctly. If you see this it would be recommended to try one of the following:
• Improve the surface data.
• Limit the selection of midsurface/solid surfaces to just the local region.
• Reduce the order of the surface to reduce the number of control points.
• Use a maximum thickness to limit the thickness computed.
• Use the Specify corners method to define the assigned thicknesses manually.
Order
Defines the number of control points along a surface. For example, Order 4 means 4 x 4 control points
along the surface or 16 total control points. For a 4-sided surface, along each edge there would be 4
250
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Repair Geometry
interpolation points creating a thickness interpolation surface between the 16 total points along the
edges.
Specify Corners Method
This option can be used to assign thickness values to a surface as well as to display the assigned
thickness values of a surface.
Surface
Select a surface or set of surfaces. If the thickness values are assigned, they will be displayed. If multiple
surfaces are selected, the only value that will be displayed is the value of the first surface selected.
Order
Defines the number of control points along a surface. For example, an order of 4 x 4 control points
means that there are 16 total control points along the surface. For a 4-sided surface, along each edge
there would be 4 interpolation points creating a thickness interpolation surface between the 16 total
points along the edges.
Corner/Middle Points
The thickness values for each specific control point.
Note
There is currently no convenient way to visualize specific control points, so the best way to
see the results is by right-clicking Geometry > Surfaces > Show Surface Thickness in the
Display Tree. The thickness values can then be assigned in an iterative method.
Find Surfaces Without Thickness Assigned
This option will evaluate a set of selected surfaces and find surfaces that do not have thickness information assigned. If Settings > Geometry Options > Inherit Part Name > Create New is enabled, the surfaces
without thickness information will be moved to a new part. If the Inherit Part Name option is disabled,
then the names of the surfaces found will only be listed in the Message Window.
Note
The Display should be set to Solid mode so that the surfaces which do not have thicknesses assigned will be highlighted in gray, and can be easily recognized.
Part
Enter the name of the new part (or select the default name) or choose an existing part.
Surface
Select the surface or set of surfaces.
Make Normals Consistent
There are two methods available.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
251
Geometry
Make Consistent
Aligns the normals of all the surfaces in the direction of the selected Reference surface normal. The
check box Reverse normals will align the normal of all the surfaces in the opposite direction of the
reference surface normal.
Reverse Normal
Reverses the normal of the selected surface.
Feature Detect Bolt Holes
The Feature Delect Bolt Holes option detects single edged connected regions in a part whose
diameter is between the defined min and max values. When a bolt hole is detected, the following occurs:
• The bolt hole curves are either placed in a subset (if Settings > Geometry Options > Inherited part name
is set to Inherited), or placed in the defined part name (if Settings > Geometry Options > Inherited part
name is set to Create New).
• The curves that are marked as bolt holes have the mesh parameter settings modified to the defined
Number of quad layers and height ratio (Ring offset ratio). If smart sizing is used, the mesh size will also
be adjusted as defined in the note below.
Curves to check
The bolt hole detection will be run on the selected curves. If no curves are selected, the bolt hole detection
will be run on the entire model.
Num quad layers
The number of quad layers of uniform height to be grown from the hole. This is equivalent to the Tetra
Width mesh curve parameter.
Ring offset ratio
An expansion ratio from the first layer of elements on the curve. This ratio will be multiplied by the
element height of the previous layer to define the next layer. You can enter any positive real number.
This is equivalent to the Height Ratio mesh parameter.
Min / Max diameter
Bolt holes with diameters within this specified range will be found.
Remove holes below min
If the min diameter is set larger than holes you want to remove, then this option will remove all holes
smaller than the Min diameter.
Note
It is recommended to set mesh sizes before using this feature, as the offset layers require
the mesh size of the curves to be set properly.
If the mesh size and Num quad layers are defined, the smart sizing will try to decrease the mesh size
so that the defined mesh size is obtained at the top of the quad layers rather than at the bolt hole. The
smart sizing function calculates the ratio of the original mesh size at the outer ring of the quad layers
to the new mesh size and reduces the original mesh size by this ratio.
252
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Repair Geometry
In the example below, bolt holes without smart sizing are shown. Uniform mesh spacing was set on all
curves prior to bolt hole detection.
Figure 235: Bolt Hole Without Smart Sizing
An example of bolt holes with smart sizing is shown below, with the same original uniform mesh spacing.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
253
Geometry
Figure 236: Bolt Hole With Smart Sizing
Note
It is important to note that if you run bolt hole detection multiple times with smart sizing,
the mesh size will be reduced further each time, as it uses the currently defines mesh parameters to compute what the new size should be. This could lead to excessive refinement,
so it is recommended to only run this feature once, or redefine the nominal mesh size on
the curves before running bolt holes a second time.
Feature Detect Buttons
The Feature Detect Buttons option detects button features and puts them into geometry subsets.
Figure 237: Example of Button Features
All curves within the button are made dormant so that the meshing of the button is handled in a special
way.
254
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Repair Geometry
There are three types of buttons that can be detected: Standard buttons, Fillet buttons and Split buttons.
By default the software will look for standard buttons, but there also options to also check for fillet and
split buttons.
A fillet button is enclosed by a set of fillets, while a split button is enclosed by two surfaces. See the
examples below.
Figure 238: Example of Fillet and Split Buttons
Fillet Button
Split Button
Surfaces to check
Select the surfaces that will be checked for buttons.
Fillet buttons
If enabled, the selected surfaces will also be checked for fillet buttons.
Rel. Tolerance
This option is applied to detection of fillet buttons only. If this is disabled, the default tolerance that will
be used is 0.001. If this is enabled, a relative tolerance can be specified for button detection.
Fillets are detected if its boundaries are created from arcs. To check whether a curve is an arc, the
curve deviation from an arc will be checked using this tolerance.
Split buttons
A split button is a button enclosed by 2 surfaces. If enabled, the selected surfaces will be checked for
split buttons as well.
Feature Detect Fillets
The Feature Detect Fillets option detects fillet regions and puts them into subsets.
Surfaces to check
Select the surfaces in which to check for fillets.
Min fillet length
Specify the minimum fillet length.
Max fillet length
Specify the maximum fillet length.
Min fillet curvature
Note
The fillet length can be found using the equation:
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
255
Geometry
L = (180 * R * θ) / π
where R = radius of the fillet and θ = fillet angle in radians.
All the fillets with lengths between the specified max and min lengths will be placed in
the subset.
Specify the fillet curvature in degrees. All the fillets whose curvature is greater than the specified
curvature will be placed in the subset.
Relative Tolerance
If this is enabled, the default tolerance that will be used is 0.001. If this is enabled, a relative tolerance
can be specified for fillet detection.
Fillets are detected if its boundaries are created from arcs. To check whether a curve is an arc, the
curve deviation from an arc will be checked using this tolerance.
Transform Geometry
Use transformation tools to change selected entity or entities.
Figure 239: Transformation Tools
The following transformation tools are available:
Translation
Rotation
Mirror Geometry
Scale Geometry
Translate and Rotate
In complex geometry, if only one entity type needs to be transformed, you must display only that entity
type and hide others with the display tree options. Clicking the Copy option causes the transformation
functions to apply to a copy of the selected entities.
By default, all newly created copies will be placed in the same part as the parent entity. To place copies
in a new part, use IncrementParts, as explained below.
Note
The Settings > Geometry Options > Inherit part name toggle does not apply to
Transform Geometry options.
Select
Click on the selection icon and select the entities to be transformed.
256
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Transform Geometry
Translation
There are two methods of defining a translation vector.
Copy
If enabled, a copy of the selected entities will be translated.
Number of copies
Specify the number of copies.
IncrementParts
To add the newly created copies of entities to a new part, click the IncrementParts icon. A window will
open with the list of the parts of the selected entities. If a part is selected, the new entities will be placed
in a new part named [old_part_name]_0. For multiple copies, each copy will be placed in a separate
part, for example, GEOM_1, GEOM_2, GEOM_3, etc.
Explicit method
Type the offset distances of the translation for all three directions.
Vector method
• Through 2 points
Select two existing points. Out of these two points the first point selected will represent the tail
of the vector while the other will represent the head of the vector.
• Distance
Specify the distance of the translation.
Rotation
The Rotation option rotates the selected geometry about an axis.
Copy
If enabled, a copy of the selected entities will be rotated.
Number of copies
Specify the number of copies of the selected entities to be created.
IncrementParts
To add the newly created copies of entities to a new part, click the IncrementParts icon. A window will
open with the list of the parts of the selected entities. If a part is selected, the new entities will be placed
in a new part named [old_part_name]_0. For multiple copies, each copy will be placed in a separate
part, for example, GEOM_1, GEOM_2, GEOM_3, etc.
Angle
If this is enabled, you can manually specify the angle of rotation. If disabled, the angle of rotation is
automatically set based on the number of copies. For n copies, the angle of rotation is set to 360/(n +
1). For example, for 1 copy, the angle of rotation is 180 degrees, and for 2 copies, it is 120 degrees.
Axis
The axis of rotation can be defined as one of the global axes, or by a vector through two specified points.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
257
Geometry
Center of Rotation
The center of rotation may be chosen as the Origin, Centroid (of the geometry) or another specified
point.
Mirror Geometry
The Mirror Geometry option mirrors selected geometry about a plane.
Copy
If enabled, a copy of the selected entities will be mirrored.
IncrementParts
To add the newly created copies of entities to a new part, click the IncrementParts icon. A window will
open with the list of the parts of the selected entities. If a part is selected, the new entities will be placed
in a new part named [old_part_name]_0. For multiple copies, each copy will be placed in a separate
part, for example, GEOM_1, GEOM_2, GEOM_3, etc.
Plane Axis (Normal)
Define the normal of the mirroring plane, either as one of the global axes, or by a vector through two
specified points.
Point of Reflection
The point of reflection may be chosen as the Origin, Centroid (of the geometry) or another specified
point.
Scale Geometry
The Scale Geometry option allows you to scale the selected geometry in all three directions or
in any particular direction.
Copy
If enabled, a copy of the selected entities will be scaled.
IncrementParts
To add the newly created copies of entities to a new part, click the IncrementParts icon. A window will
open with the list of the parts of the selected entities. If a part is selected, the new entities will be placed
in a new part named [old_part_name]_0. For multiple copies, each copy will be placed in a separate
part, for example, GEOM_1, GEOM_2, GEOM_3, etc.
X, Y, Z factor
Enter the scale factor for each direction.
Center of Transformation
The center of the scaling transformation may be chosen as the Origin, Centroid of the geometry, or
another Selected point.
Translate and Rotate
The Translate and Rotate option allows you to translate and rotate the geometry at the same
time.
258
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Delete Point
Copy
If enabled, a copy of the selected entities will be created in the new location.
IncrementParts
To add the newly created copies of entities to a new part, click the IncrementParts icon. A window will
open with the list of the parts of the selected entities. If a part is selected, the new entities will be placed
in a new part named [old_part_name]_0. For multiple copies, each copy will be placed in a separate
part, for example, GEOM_1, GEOM_2, GEOM_3, etc.
3 points –> 3 points
Select six points in all. The first three points will be used as the reference for the entity to be transformed.
The second set of three points is used to define the transformation. The result will match the first points
of both sets, and the direction from the first to the second point, and the plane defined by the third
point.
Curve –> Curve
Select two curves. The first curve is used as a reference for the entity to be transformed. The second
curve is used to define the transformation. The result will match the beginning (parameter = 0) of both
curves, the direction from parameter 0 to 0.5, and the plane defined by the end (parameter 1) of the
curves. A curve used to define the transformation can be included in the entities selected to be transformed.
LCS –> LCS
Click Show LCS to view any defined coordinate systems. Select two local coordinate systems.
The result will match the origin and the axes of the first to the second LCS.
Restore Dormant Entities
This Restore Dormant Entities option restores dormant curves and points.
Dormant curves and points are a fundamental part of ANSYS ICEM CFD feature build topology. When
build topology is performed, the software builds connectivity information between surfaces. For example,
a surface is attached to a set of curves that is attached to a set of points. This information is needed
for flood fill operations, patch based meshing, and many geometry operations that require connectivity
information. When a curve is made dormant, the curve is still in the database and can be restored
through this feature. Thus the connectivity between the surfaces still exists. Dormant curves and points
can also be displayed by right clicking on Curves and Points Display Trees and selecting Show Dormant.
Curves and points can be made dormant either by deleting them with Delete permanently option disabled, through building topology with feature angle and filter points/curves enabled, or through feature
detection tools. If a curve or point is dormant, it will not be recreated when building topology, but
build topology may make it active. If a curve or point is permanently deleted, it is removed from the
database. If the topology is rebuilt, the curve will be recreated. Flood fill, and patch based meshing will
also fail across a boundary (curve or point) that has been permanently deleted. Curves and points that
are unattached to surfaces or curves will always be permanently deleted, as the sole purpose of dormant
curves and points is to maintain connectivity between attached geometry.
Delete Point
The Delete Point option deletes selected points.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
259
Geometry
Delete unattached
automatically deletes unattached points.
Delete permanently
permanently deletes the selected points and removes them from the database.
Join incident curves
If two curves are attached at a point, and they do not form a sharp angle, then if the point is deleted,
this option will concatenate the curve.
Delete All Dormant Points
deletes all dormant points.
Delete Curve
The Delete Curve option deletes selected curves.
Delete unattached
automatically deletes unattached curves.
Delete permanently
permanently deletes the selected curves and removes them from the database.
Delete All Dormant Curves
deletes all dormant curves.
Delete Surface
The Delete Surface option permanently deletes the selected surfaces and removes them from the
database.
Delete Body
The Delete Body option permanently deletes the selected bodies and removes them from the
database.
Delete Any Entity
The Delete Any Entity option deletes selected entities.
Delete unattached
automatically deletes unattached entities.
Delete permanently
permanently deletes the selected entities and removes them from the database.
260
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Mesh
Figure 240: Mesh Menu
The Mesh tab contains the following options:
Global Mesh Setup
Part Mesh Setup
Surface Mesh Setup
Curve Mesh Setup
Create Mesh Density
Define Connectors
Mesh Curve
Compute Mesh
Global Mesh Setup
The Global Mesh Setup options provide the general and specific meshing algorithm parameters
used for the various meshers. The global mesh parameters are stored in the geometry file and help
define global controls for the following:
Global Mesh Size
Shell Meshing Parameters
Volume Meshing Parameters
Prism Meshing Parameters
Periodicity Set Up
Figure 241: Global Mesh Setup Parameters
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
261
Mesh
For a comprehensive list of the different meshing parameters and which methods they apply to, see
Table 5: Parameters for Surface Meshing Methods (p. 262), Table 6: Parameters for Volume Meshing
Methods (p. 263), and Table 7: Parameters for Other Meshing Methods (p. 265).
Table 5: Parameters for Surface Meshing Methods
Surface Meshing Methods
Mesh Parameters
Autoblock
Patch Dep.
Patch Indep.
Shrinkwrap
Max Element*
Y
Y
Y
Y
Min Size Limit*
N
Y
Y
N
Elements in
gap
N
N
Y
N
Refinement
N
N
Y
N
Periodicity
N
N
Y
N
Global Parameters
Part Meshing Parameters
Internal Wall
N/A
N/A
N/A
N/A
Thin Wall
N/A
N/A
N/A
N/A
Hexa-core
N/A
N/A
N/A
N/A
Prism setting
N/A
N/A
N/A
N/A
Surface Meshing Parameters
Ignore Size
Y
Y
N
N
Surface mesh
type
N/A
N/A
N/A
N/A
Prism Meshing Parameters
Growth law
N/A
N/A
N/A
N/A
Initial height
N/A
N/A
N/A
N/A
Height ratio
N/A
N/A
N/A
N/A
Number of
layers
N/A
N/A
N/A
N/A
Max size*
Y
Y
Y
Y
Height
N/A
N/A
N/A
N/A
Height ratio
N/A
Y
N/A
N/A
No. of layers
N/A
N/A
N/A
N/A
Tetra width
N/A
N/A
Y
N/A
Tetra size ratio
N/A
N/A
Y
N/A
Min Size Limit*
N
N
Y
N
Surface Parameters
262
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Surface Meshing Methods
Mesh Parameters
Autoblock
Patch Dep.
Patch Indep.
Shrinkwrap
Max deviation*
Y
Y
Y
N
Surface mesh
type
Y
Y
Y
N/A
Max size*
Y
Y
Y
N
No. of nodes
Y
Y
Y
N
Height
N
Y
N
N
Height ratio
N
Y
N
N
No. of layers
N
Y
N
N
Tetra width
N/A
N/A
Y
N/A
Min Size Limit*
Y
N
Y
N
Max deviation*
Y
N
Y
N
Bunching
N
Y
N
N
Densities*
N
N
Y
N
Connectors
N
Y
Y
N
Curve Parameters
*Scale Factor is applied
Table 6: Parameters for Volume Meshing Methods
Volume Meshing Methods
Mesh
Parameters
Octree
Delaunay
Adv.
Front
Hexa
Dom.
Cartesian
Global Parameters
Max Element*
Y
Y
Y
Y
N
Min Size
Limit*
Y
N/A
N/A
N/A
N
Elements
in gap
Y
N
N
N
N
Refinement
Y
N/A
N/A
N/A
N
Periodicity
Y
N/A
N/A
N/A
N
Part Meshing Parameters
Internal
Wall
Y
N/A
N/A
N/A
N
Thin Wall
Y
N/A
N/A
N/A
N
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
263
Mesh
Volume Meshing Methods
Mesh
Parameters
Octree
Delaunay
Adv.
Front
Hexa
Dom.
Cartesian
Hexa-core
Y
Y
N
N/A
N/A
Prism setting
Y
Y
Y
N/A
N
Surface Meshing Parameters
Ignore
Size
N
N/A
N/A
N/A
N
Surface
mesh type
N
Y
Y
Y
N/A
Prism Meshing Parameters
Growth
law
N/A
N/A
N/A
N/A
N/A
Initial
height
N/A
N/A
N/A
N/A
N/A
Height ratio
N/A
N/A
N/A
N/A
N/A
Number
of layers
N/A
N/A
N/A
N/A
N/A
Surface Parameters
Max size*
Y
N/A
N/A
N/A
Y
Height
N/A
N/A
N/A
N/A
N
Height ratio
N/A
N/A
N/A
N/A
N
No. of layers
N/A
N/A
N/A
N/A
N
Tetra
width
Y
N
N
N
N/A
Tetra size
ratio
Y
N
N
N
N/A
Min Size
Limit*
Y
N/A
N/A
N/A
Y
Max deviation*
Y
N/A
N/A
N/A
N
Surface
mesh type
N
Y
Y
Y
N/A
Curve Parameters
Max size*
Y
N/A
N/A
N/A
N
No. of
nodes
N
N/A
N/A
N/A
N
Height
N/A
N/A
N/A
N/A
N
264
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Volume Meshing Methods
Mesh
Parameters
Octree
Delaunay
Adv.
Front
Hexa
Dom.
Cartesian
Height ratio
N/A
N/A
N/A
N/A
N
No. of layers
N/A
N/A
N/A
N/A
N
Tetra
width
Y
N
N
N
N/A
Min Size
Limit*
Y
N/A
N/A
N/A
N
Max deviation*
Y
N/A
N/A
N/A
N
Bunching
N
N/A
N/A
N/A
N
Densities*
Y
Y
N
N
Y
Connectors
Y
Y
Y
Y
N
*Scale Factor is applied
Table 7: Parameters for Other Meshing Methods
Other Methods
Mesh Parameters
Prism
Blocking
Global Parameters
Max Element*
Y
Y
Min Size
Limit*
N/A
N
Elements in
gap
N
N
Refinement
N/A
N
Periodicity
Y
Y
Part Meshing Parameters
Internal
Wall
N/A
N/A
Thin Wall
N/A
N/A
Hexa-core
N/A
N/A
Prism setting
N/A
Y
Surface Meshing Parameters
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
265
Mesh
Other Methods
Mesh Parameters
Prism
Blocking
Ignore Size
N/A
N
Surface
mesh type
N/A
N
Prism Meshing Parameters
Growth law
Y
N
Initial
height
Y
Y
Height ratio
Y
Y
Number of
layers
Y
Y
Surface Parameters
Max size*
N/A
Y
Height
Y
Y
Height ratio
Y
Y
No. of layers
Y
Y
Tetra width
N/A
N/A
Tetra size
ratio
N/A
N/A
Min Size
Limit*
N/A
N
Max deviation*
N/A
N
Surface
mesh type
N/A
N
Max size*
N/A
Y
No. of
nodes
N/A
Y
Height
Y
Y
Height ratio
Y
Y
No. of layers
Y
Y
Tetra width
N/A
N/A
Min Size
Limit*
N/A
N
Max deviation*
N/A
N
Bunching
N/A
N
Curve Parameters
266
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Other Methods
Mesh Parameters
Prism
Blocking
Densities*
N/A
N
Connectors
N/A
N
*Scale Factor is applied
Global Mesh Size
The Global Mesh Size parameters affect meshers at the surface, volume, and inflation (prism) layer
levels.
Global Element Scale Factor
multiplies other mesh parameters to globally scale the model. For a list of parameters affected by this
scale factor, see the tables in Global Mesh Setup.
For example, if the Max Element Size of a given entity is 4 units, and the Global Element Scale
Factor is 3.5, then the actual maximum element size used for meshing of that entity will be 4 * 3.5
= 14.0 units. The Global Element Scale Factor can be any positive real number, and it allows you
to globally control the mesh size instead of changing the mesh parameters for different entities.
Display
when enabled, a reference mesh element will be displayed that corresponds to the specified element
size.
Global Element Seed Size
Max Element
controls the size of the largest element. The largest element size in the model will not exceed the
Max Element size multiplied by the Global Element Scale Factor. It is recommended that the Max
Element value is a power of 2. Even if you specify a value other than a power of two, some meshers
(Octree/Patch Independent) approximate the Max Element size to the nearest power of two while
meshing.
Note
If the Max Element size is set to 0, the Automatic Sizing feature will be implemented.
Autosizing temporarily sets a Global Max Element size, which produces a uniform
mesh, if no surface or curve sizes are smaller. If most surface sizes are not set (< 22%),
the autosizing will set the Global Max Element size to 0.025 * the bounding box diagonal of the geometry. If most surface sizes are set (> 22%), the autosizing will set
the Global Max Element size to be the largest surface size that is specified.
If the Global Max Element size is too large (>= 0.1* the bounding box diagonal), and
either no surface sizes are set or are also greater than this value, a message will appear
informing you that the mesh size may be inadequate to represent the geometry and
asking if you want to run with autosizing instead.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
267
Mesh
Curvature/Proximity Based Refinement
when enabled, the mesh is automatically refined based on geometry curvature and proximity. This will
result in larger elements on flat planar surfaces and smaller elements in areas of high curvature or
within small gaps. The algorithm attempts to satisfy the Refinement and Elements in Gap settings, but
is limited by the Min size limit. The effective Min size limit is scaled by the Global Element Scale Factor
along with the Max Element Size. Entity Min size limits may be smaller than the global setting and will
cause further local refinement.
Note
This option currently applies only to Octree and Patch Independent meshing.
All other mesh sizes will be rounded to the nearest power of 2 of the Min Size Limit value.
The following options are applicable when Curvature/Proximity Based Refinement is enabled:
Min size limit
specifies the size limit for the smallest element. Mesh elements will be limited from being subdivided
smaller than this value. To see a mesh element of this size displayed on the screen, enable the Display
option and click Apply.
Elements in Gap
is used to force the Octree/Patch Independent mesher to create a defined number of elements in a
gap (proximity based refinement). The specified value may not be possible if the Min size limit is
too large, as the mesh can not be refined smaller than the Min size limit. Any positive integer can
be entered for this option.
Refinement
defines the number of edges that would fit along a radius of curvature if that radius were extended
out to 360 degrees. This is generally used to avoid having too many elements along a given curve
or surface, if the Min size limit is too small for that particular curve. Any positive integer can be
entered for this option. See the example in Figure 242: Refinement (p. 268).
Figure 242: Refinement
Ignore Wall Thickness
prevents the Curvature / Proximity Based sizing function from refining for closely spaced parallel
surfaces, though it will still resolve other forms of proximity. The Elements in Gap function may
cause the model to over-refine within or around thin walled sections of a model. In these cases, the
refinement results in relatively uniform elements and high mesh density in those areas. This can
dramatically increase the element count. Enabling the Ignore Wall Thickness option will result in
a mesh that uses larger elements in the thin walled area. There will still be refinement near the edges
of the thin wall, but it will not refine most of the area. These larger elements will not be uniform
and are likely to have lower quality. These higher aspect ratio tetra elements are also more likely to
result in holes or non-manifold vertices in the thin wall, which can be addressed using the Define
Thin Cuts option for Octree Tetra meshing.
268
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
In the following examples, all refinement was controlled automatically by the Curvature /
Proximity Based Refinement sizing function.
Figure 243: FEA Model with Ignore Wall Thickness Option Disabled
Figure 244: FEA Model with Ignore Wall Thickness Option Enabled
In the CFD example shown, there is a thin wall separating larger volumes. There is no need to
refine the mesh for the wall thickness because meshing is not required within the wall. In this
example, the quality is better when using Ignore Wall Thickness because of fewer size transitions.
Figure 245: CFD Model with Ignore Wall Thickness Option Disabled
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
269
Mesh
Another view of the same CFD model
Figure 246: CFD Model with Ignore Wall Thickness Enabled
Shell Meshing Parameters
The Shell Meshing Parameters control the various surface meshing algorithms. These parameters
also control the surface mesh that is used for various volume meshers.
Mesh type
specifies the type of surface mesh. If an individual surface is assigned a different type of surface mesh,
then the local control will override the global setting.
All Tri
meshes the geometry with a pure triangular mesh.
Quad w/one Tri
allows for a Quad Dominant mesh with one tri element per surface. The tri element allows for better
transition between uneven mesh distribution on the loop edges. Automatic tri-reduction steps may
even remove the tri element.
Quad Dominant
creates a quad mesh that allows for several transitional triangles. This mesh type is very useful in
meshing complicated surfaces where a pure quad mesh may have poor quality.
270
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
All Quad
meshes the geometry with a pure quadrilateral surface mesh.
Note
This mesh type requires uniform sizes otherwise it will create some tri elements to
maintain connectivity.
Mesh method
specifies the meshing method or algorithm to be used. If an individual surface is assigned a different
type of mesh method, then the local control will override the global setting.
Autoblock
This method uses the mapped or block-based meshing algorithm. It automatically determines the
best fit to obtain the defined minimum edge and orthogonality. For surface patches that cannot be
mapped (having more or less than 4 corners), the Patch Dependent method is called through this
block-based algorithm.
Patch Dependent
This is a free surface mesh generator that meshes closed regions called loops. Loops are created
from surfaces or curves, and holes and internal curves are taken into account. The mesh is seeded
according to the node spacing defined on the curves. Mesh from adjacent loops sharing a single
curve is automatically joined together. This meshing method gives the best quad dominant quality
while capturing surface details.
Note
For Patch Dependent meshing using Mesh Type of All Tri, the Curve Mesh Setup
parameters of Height, Height Ratio, and Num Layers are respected, but quad
elements will be used for the offset layers.
If only Height Ratio is used in conjunction with the Global Shell Meshing Parameter Adapt Mesh interior, it can control the rate of transition for the All Tri
or Quad Dominant mesh types.
Patch Independent
Patch independent meshing is best for low quality geometry or surfaces with poor connectivity. It
uses the Octree method to create a robust patch independent surface mesh. See The Octree Mesh
Method in the ANSYS ICEM CFD User's Manual.
The geometry does not need to be a closed volume. If the Mesh Type is set to Quad mesh, the
Patch Independent mesher will first generate a tri mesh, which can be automatically converted
to a pure quad or quad dominant mesh.
Note
Patch independent meshing does not respect surface meshing parameters that have
been set. However, it can take advantage of Octree parameters such as
Curvature/Proximity Based Refinement, and Density Regions. Refer to the Table
of Meshing Parameters.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
271
Mesh
Figure 247: Example of Patch Independent Meshing
Shrinkwrap
Shrinkwrap meshing is best for geometry with gaps in STL representation. It uses the Cartesian
method to initially generate all Quad mesh, with Quad dominant / All Tri options for better capturing
of features. This generates watertight shell mesh with feature suppression. If the capture of greater
detail is desired, then the Patch Independent Octree Tetra mesh would produce a better result, given
that the model is of sufficient quality.
Note
The shrinkwrap mesher requires a closed volume input.
Figure 248: Example of Shrinkwrap Meshing
Autoblock Options
The Autoblock mesh method creates a 2D surface blocking in the background to generate 2D shell
mesh. Since blocking is used in the background, you will essentially define the controls for the intermediate blocking file that will be generated. For more information on blocking and mesh generation, see
Blocking > Create Block > 2D Surface Blocking.
272
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
General Parameters
Ignore size
ignores sliver surfaces smaller than the specified value by merging the smaller loop with the adjacent
loop.
Surface Blocking Options
The meshing algorithm on a surface to surface basis can be varied among the following options:
Free
All surfaces will be meshed similar to Patch Dependent Meshing.
Some mapped
Some surfaces will be meshed as orthogonally meshed surfaces, and the remainder will be meshed
similar to Patch Dependent Meshing. Surfaces with primarily 4 corners and 4 sides are likely to be
mapped (orthogonally meshed), even if they also have other shallow corners or multiple edges.
Surfaces with more or less than 4 clear corners will be meshed as free blocks.
Mostly mapped
Most surfaces will be meshed as orthogonally meshed surfaces, and the remainder will be meshed
similar to Patch Dependent Meshing. This is achieved by blocking subsurfaces, for example, a triangular surface may be blocked in a 3 block Y pattern (quarter O-grid), and a half circle may be blocked
with a C-grid (half O-grid). In other cases, a surface with 5 or 6 corners may be split to create 2
mapped regions.
Merge mapped blocks
attempts to group mapped surfaces to form larger mesh regions.
Note
Blocks can be converted between free and mapped blocks using Edit Block > Convert
Block Type.
Note
For more descriptions of the different block types, see User’s Manual > Hexa > Hexa
Block Types.
Patch Dependent Options
General Parameters
Ignore size
ignores sliver surfaces with an edge that is smaller than the defined value by merging the smaller
loop with the adjacent loop.
Respect line elements
forces the surface mesher to respect nodes from given line elements on curves instead of creating
new nodes. This is useful to connect a mesh to an existing mesh.
In Figure 249: Line Element Generated (p. 274), a curve of element count 14 was meshed and a
line element was generated.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
273
Mesh
Figure 249: Line Element Generated
In Figure 250: Line Element Count Changed (p. 274), the element count was changed from 14 to
10.
Figure 250: Line Element Count Changed
If the four curves are chosen for Patch based surface meshing, and Respect line elements is
enabled, line element mesh will remain intact. The resulting mesh is shown in Figure 251: Respect
Line Elements Enabled (p. 275).
274
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Figure 251: Respect Line Elements Enabled
When Respect line elements is disabled, the surface mesh created has ignored the line element
mesh and readjusted the mesh on the curves based on the element count, as shown in Figure 252: Respect Line Elements Disabled (p. 275).
Figure 252: Respect Line Elements Disabled
Respect line elements is useful to make sure that new mesh matches and connects with an
existing mesh. This is particularly useful if the existing mesh came from another mesher, such
as ANSYS ICEM CFD Hexa mesher, or from an outside product. This option is also helpful if there
is a complex edge distribution that would be hard to match with the curve parameter controls.
In the example in Figure 253: Example of Respect Line Elements Option (p. 276), the inner fan
was meshed using the ANSYS ICEM CFD Hexa mesher and the outer shroud was meshed with
Respect line elements to create a node for node conformal mesh.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
275
Mesh
Figure 253: Example of Respect Line Elements Option
Quadratic elements
when enabled, generates the patch dependent surface mesh with mid side nodes (quadratic elements),
such that triangles have 6 nodes (3 corners and 3 mid side nodes) and quads have 8 nodes (4 corners
and 4 mid side nodes). The mid side nodes are projected to the surface and the resulting edge shape
is quadratic (rather than linear). When this option is disabled, the patch dependent surface mesh
consists of linear triangles and quads, each with 3 or 4 corner nodes, respectively.
Note
Typically FEA solvers prefer quadratic elements. Most CFD solvers do not support
quadratic elements at all.
Tip
You can also use the Create Mid Side Nodes (p. 546) option to convert linear elements
to quadratic.
Boundary Parameters
Protect given line elements
is available when Ignore size is set and Respect line elements is enabled in the General section
of the Shell Meshing Parameters list. If enabled, it will protect existing line elements that are
smaller than the Ignore size value from being removed.
Smooth boundaries
smooths the surface mesh boundaries after meshing. This will typically give better quality mesh, but
it may not respect the initial node spacing.
Allow free bunching
if enabled, it allows free bunching for patch independent (Octree, with or without Tetra) surfaces. If
disabled, curve bunching is done by the Patch Dependent mesher and respected by Patch Independent
functions.
276
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Offset type
Standard
Offsets will be created normal to the edges without special solutions for sections with small or
large angles, such as corners. The number of nodes on the offset front may not be identical as
the number of nodes on the initial boundary.
Figure 254: Standard Offset Example
Simple
Offsets will be created normal to the edges without special solutions for sections with small or
large angles, such as corners. The number of nodes on the offset front is identical to the number
of nodes on the initial boundary.
Figure 255: Simple Offset Example
Forced Simple
This option is the same as simple offset, but without collision checking.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
277
Mesh
Figure 256: Forced Simple Offset Example
Interior Parameters
Force Mapping
If the boundary is nearly quadrilateral, the mesher forces the generation of structured mesh instead
of unstructured mesh up to this specified block quality. Default value is 0. For hybrid meshes a value
of 0.2 is preferred.
Max nodes adjustment
For opposite boundaries with differing node counts, this function will calculate the ratio of the node
counts as a percentage. For all ratio percentage values less than this specified value, mapping will
be applied to the mesh. For all ratio percentage values greater than this specified value, mapping
will not be applied.
Project to surfaces
If enabled, it will allow the mesher to project the mesh to the surface.
Note
Disable this if the geometry does not have surfaces.
Adapt mesh interior
Uses the surface sizes to coarsen the mesh internally. For example, if curve size is set to 1, and surface
size to 10, then the mesh will start with a mesh size of 1 on the curves, but transition to 10 in the
middle of the surface. This is more effective on larger surfaces where the element reduction is more
dramatic.
The default growth rate for the transition to the surface max size is 1.5. This growth rate can
be adjusted by setting the surface Height Ratio to between 1.0 and 3. Sizes below 1.0 are inverted (i.e., 0.667 = 1.5). Sizes above 3 are ignored and the default is used. If this option is enabled, Force Mapping is disabled on surfaces whose maximum size setting exceeds its perimeter
curve sizes by a factor of 2 or more.
The difference in the transition rate is shown in Figure 257: Example of Adapt Mesh Interior
option (p. 278):
Figure 257: Example of Adapt Mesh Interior option
Adapt Mesh Interior option disabled
278
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Adapt Mesh Interior option enabled
Default Surface Height Ratio =
1.5
Surface Height Ratio = 3
Note
The Max Element size specified in the General Parameters takes precedence over
this value.
Note
For All Quad, Quad Dominant, and Quad with one Tri mesh, the Force Mapping
option has priority over this option. To apply the Adapt mesh interior option to
these types of mesh, set the Force Mapping value to 0.
Orient to surface normals
orients the shell normals in the same direction as the surface normals. This option is enabled by
default.
Repair Parameters
Try harder
• Level 0
If the mesher fails, no further meshing step is tried. The problem(s) will be reported.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
279
Mesh
• Level 1
If the mesher fails, simple triangulation is attempted to fix the problems (for “All Tri” and
“Quad Dominant” mesh types only).
• Level 2
All Level 1 steps will be completed. If necessary, all Level 1 steps will be retried without
merging at dormant curves.
• Level 3
All Level 2 steps will be completed. If necessary, surface meshing will be retried with the Tetra
mesher.
Improvement level
• Level 0 does pure Laplacian smoothing. Nodes are moved while keeping the mesh topology unchanged.
• Level 1 will mesh any failed loop with an STL method if element types Quad Dominant or All
Tri has been selected. This makes the mesher more robust. Very bad quadrangles will be split into
triangles.
• Level 2 will operate as Level 1, and also will combine triangles to quadrangles and will split more
bad quadrangles into triangles. This option is most used.
• Level 3 will operate as Level 2, and also will move nodes off curves to improve the quality.
Respect dormant boundaries
If enabled, all dormant curves and points are included in the mesh boundary definitions. The default
is off.
Relax dormant boundaries for smoothing
If Mesh dormant is enabled, then this option allows nodes on dormant curves and points to be
moved in order to improve smoothing.
Patch Independent Options
This method uses the Octree Tetra process to create a robust patch independent surface mesh. See The
Octree Mesh Method in the ANSYS ICEM CFD User's Manual.
Shrinkwrap Options
Num. of smooth iterations
is the number of smoothing iterations that will be performed to improve mesh quality.
Surface projection factor
controls the tightness of the shrinkwrap to the geometry. Values can range from 0 to 1.0, where a value
of 0 indicates shrinkwrap totally free from the geometry, and a value of 1.0 indicates shrinkwrap that is
strictly on the geometry. The example in Figure 258: Surface Projection Factor (p. 281) illustrates the results
of using different values for the Surface projection factor.
280
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Figure 258: Surface Projection Factor
Surface Projection
Factor = 0.2
Surface Projection
Factor = 0.9
Volume Meshing Parameters
The Volume Meshing Parameters control the various volume meshing algorithms. Each mesh
type has different options, as described in the following sections.
Tetra/Mixed
Hexa-Dominant
Cartesian
Tetra/Mixed
The following Mesh Methods are available for Tetra meshing:
Robust (Octree)
Quick (Delaunay)
Smooth (Advancing Front)
Robust (Octree)
The Robust (Octree) option will generate a tetra mesh using a top-down meshing approach. An Octree
mesher does not require an existing surface mesh because one is created by the Octree process. It will
accept a variety of parameters in a more general way. For instance, curve sizes are respected, but specific curve node spacing distributions are not. For a better understanding of the Octree meshing
methodology, see The Octree Mesh Method in the ANSYS ICEM CFD User's Manual.
Run as batch process
allows you to run the meshing operation in batch mode.
Fast transition
enables a faster transition from the more refined elements to coarser elements instead of a more
gradual transition when computing the mesh. This will reduce the number of elements in the overall
mesh. This option is particularly useful if you plan to delete the Octree volume mesh anyway since it
saves time and memory during mesh generation.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
281
Mesh
Edge criterion
determines to what extent a tetra is cut to represent geometry. The entered value is a factor of the tetra
edge. After subdivision, if a tetra edge intersects an entity (surface), the tetra will be cut if the subdivision
of the edge from the intersection is less than the prescribed value.
The values can range from 0 to 1. A larger value (e.g., 0.5) may be prescribed if you want to ignore
inexact duplicates, however geometry may not be properly captured if the value is too large. Increasing the value will increase the nodes moving to fit to the geometry. Reducing the value will increase
refinement near entities, and will also reduce non-manifold vertices in trailing edges. The default
of 0.2 is adequate for most cases. This value is useful in cases where thin cuts fail or are difficult to
setup.
Figure 259: Edge Criterion
Edge criterion = 0.2
Edge criterion = 0.01
Define thin cuts
allows you to resolve gaps based on pairs of surface or curve parts which are close to each other. The
thin cut definition prevents surface elements from spanning between nodes on the two parts specified.
This helps prevent non-manifold nodes in areas where the mesh size may be larger than the gap.
Figure 260: Thin Cuts (p. 283) shows an example of thin cuts. If the face of a tetra element has a
surface/line/node on part A, then it cannot have a surface/line/node in part B.
282
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Figure 260: Thin Cuts
Note
If the surfaces of the two parts, A and B, meet (see Figure 261: Thin Cuts for Intersecting
Parts (p. 283)), then the contact curve must be in a third part, C, or the thin cut will fail.
Figure 261: Thin Cuts for Intersecting Parts
Clicking the Define thin cuts button will bring up the Thin cuts window where pairs of parts can
be selected or entered to define a thin cut “pair”. A part can belong to more than one thin cut pair.
The following limitations apply to the definition of thin cuts:
• If two surfaces approach asymptotically, the thin cut definition may eventually fail.
• If the separation rule of thin cuts is violated at any point, all thin cuts will fail and be deactivated.
Due to the existing limitations with defining thin cuts, in some cases, it may be more effective to
adjust the edge criterion.
Edit entry
allows you to enter or edit the names of the parts in a pair.
Select
allows you to select parts from a window displaying all the part names. The pair of parts selected
should not be touching. If two surface parts meet along an edge (such as a sharp cusp) the curves
and points between the parts must be in a third part name.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
283
Mesh
Add
adds the thin cut pair selected or entered.
Modify
allows you to modify a thin cut pair.
Delete
allows you to delete a thin cut pair definition.
Done
saves the thin cut pair definitions and closes the window.
Cancel
cancels the thin cut pair definitions.
Smooth mesh
when enabled, the mesh is smoothed after finishing subdivision down to the specified mesh sizes.
Iterations
number of iterations to be performed for the smoothing to match the supplied Min quality.
Min Quality
all elements with quality less than the specified value will be smoothed. The default is 0.4.
Coarsen mesh
is a useful option if the geometry to be captured is difficult to mesh with the desired coarse mesh size.
This allows the Octree process to fit to the geometry and flood fill with a finer mesh and then automatically coarsen it. For instance, it could mesh to capture features with approximately 150k elements and
then automatically coarsen down to 15k elements while still maintaining the features. This may be
needed in some situations, but it is recommended that you mesh without this option and coarsen the
mesh with the Edit Mesh tools where there are more controls available.
Iterations
number of iterations to be performed for the coarsening to meet the specified Worst Aspect Ratio.
Worst Aspect Ratio
a limiting factor for mesh coarsening (any elements below this quality will be excluded from the
next iteration of coarsening).
Fix Non-manifold
if enabled, the mesher will do additional work to try to fix non-manifold elements. These are only a
possible problem, depending on your model and solver. See here for a description of non-manifold
elements. It is strongly recommended to leave this option on and that you check for non-manifold elements after the mesh is computed.
Note
You may still have non-manifold elements for several reasons. They may be representative
of the true geometry, and acceptable to the solver and therefore not a problem. It is also
possible that the meshing parameters may be too coarse to cope with the geometry; in
which case you could reduce the mesh size and/or apply thin cuts and/or reduce the
edge criterion to allow for subdivision within the thin space. If only a few non-manifold
284
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
elements exist, you can repair them with mesh editing. Try splitting nodes or delete the
non-manifold elements and remesh locally.
Close Gaps
is used to close gaps in the surface mesh between different materials. If enabled, triangles will be created
to fill these gaps.
Fix Holes
if disabled, the mesher will not perform extra steps to try to close holes to form a watertight volume. If
enabled, the mesher will perform extra steps to close holes with a clear solution. If the mesher detects
leakage with an unclear solution, it will interactively prompt the user for the solution.
Use active local coordinate system
allows you to orient the Octree mesh along the active local coordinate system instead of along the
global coordinate system. If the LCS is not Cartesian, the equivalent Cartesian LCS is used.
Figure 262: Orienting Octree Tetra Mesh Along LCS
Note
This option is helpful when converting oriented Octree tetra mesh to oriented hexa hybrid
mesh (Convert Tetra to Hexa method – 12 tetra to 1 hexa).
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
285
Mesh
Figure 263: LCS Oriented Octree Tetra Mesh Converted to LCS Oriented Hexa
Mesh
In such cases, make sure the Use active coordinate system option is enabled for the
12 tetra to 1 hexa method in the Convert Tetra to Hexa DEZ (see the Convert Tetra
to Hexa section).
Quick (Delaunay)
The Quick (Delaunay) option will generate a tetra mesh using a bottom-up meshing approach (Delaunay
Tetra algorithm). This algorithm requires an existing, closed surface mesh. If this has not yet been created,
it will automatically create the surface mesh from the geometry as defined by the Global Mesh Setup
settings (or the Surface Mesh option). The volume mesh will then be generated from this surface mesh.
You can also run this in two steps by creating/importing a surface mesh first and then running this
mesher. If a surface mesh exists, you can also specify the Input as Existing Mesh when Compute Mesh
is applied.
Note
A closed surface mesh is needed to contain the volume mesh. You can run a mesh check
for single edges, overlapping elements or duplicate elements (Edit Mesh > Check Mesh).
Single edges may appear on the edges of internal baffles, but should not be found on the
outer perimeter of the model or the Delaunay fill will fail.
Delaunay Scheme
allows you to select the Delaunay scheme to be used.
Standard
uses the standard Delaunay scheme with a skewness-based refinement.
TGlib
uses the latest TGrid Delaunay volume grid generation algorithm that utilizes a more gradual transition
rate near the surface, and a faster transition rate towards the interior. Like the standard Delaunay
scheme, it uses a skewness-based refinement.
286
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Use AF
uses the latest TGrid Advancing Front Delaunay algorithm which has smoother transitions than
the pure Delaunay algorithm.
Note
The TGlib options will be ignored when the Create Hexa-Core option is enabled for the
Quick (Delaunay) method.
Memory scaling factor
The initial memory requirements will be multiplied by this factor. If no value is supplied, the default is
taken as 1. The initial memory requirement is calculated from the surface mesh (or from volume mesh
if it is supplied). If the initial memory calculation falls short, it will double it and try again. It will restart
3 times before failing due to insufficient memory allocation.
Spacing Scaling Factor
The rate at which the tetra grow from the surface mesh. It is similar, but not mathematically identical,
to the expansion factor used by other algorithms. This value directly affects the number of tetra elements
generated.
Fill holes in volume mesh
This is for use on an existing tetra mesh with internal voids (cavity re-meshing). This will fill the voids
without regenerating the full tetra domain. You could delete the tetra mesh in a region, insert a new
surface mesh component and then cavity re-mesh to the existing tetra mesh. Alternatively, this could
be used simply to remesh a region of poor tetra mesh.
Mesh internal domains
If this option is enabled, the Delaunay tetra mesher will also attempt to fill internal volume regions. With
this option disabled, only those volumes adjacent to external shell elements will be meshed.
Flood fill after completion
This option only pertains to models with multiple material points. If this option is enabled, the volume
mesh will be assigned to different volume parts based on material point containment.
Verbose output
When enabled, the mesher outputs more detailed messages to help in debugging any potential problem.
In general, you should not need to have this option enabled, but it may help to enable this for debugging.
Smooth mesh
When enabled, the mesh is smoothed after finishing subdivision down to the specified mesh sizes.
Iterations
Specifies the number of iterations to be performed for the smoothing to match the supplied Min
quality.
Min Quality
All elements with quality less than the specified value will be smoothed. The default is 0.4.
Smooth (Advancing Front)
The Smooth (Advancing Front) option will generate a tetra mesh using a bottom-up meshing approach
using the Advancing Front Tetra mesher. The surface mesh will be created as defined by the Global
Mesh Setup settings (or Surface Mesh option). The volume mesh will then be generated from this surface
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
287
Mesh
mesh. If a surface mesh exists, you can also specify the Input as Existing Mesh when Compute Mesh
is applied.
This meshing method results in a more gradual change in element size. The initial surface mesh should
be of fairly high quality.
Note
The surface mesh should be one enclosed volume with no single edges, multiple edges, nonmanifold vertices, overlapping elements or duplicate elements. Sudden changes in element
size, either adjacent to one another or across a narrow volume gap, can cause quality issues
or even failure.
The surface mesh must be either tri or quad elements for the Advancing Front mesh method.
Expansion Factor
The ratio at which to grow the tetra from the surface mesh. The default is 1. This value directly affects
the number of tetra elements generated.
Do Proximity Checking
This option will check the proximity between nodes to prevent clustering or stretching so that small
gaps are filled properly. Enabling this option will result in a longer meshing time.
Flood fill after completion
This option only pertains to models with multiple material points. If this option is enabled, the created
mesh will be assigned to their different volume parts.
Verbose output
When enabled, this option writes more messages to help in debugging any potential problem. In general
you should not need to have this option enabled, but if the mesher has a problem meshing, it may help
to enable this for debugging.
Hexa-Dominant
The Hexa-Dominant option will generate a hexa-dominant mesh using a bottom-up meshing approach.
The Hexa-Dominant mesher starts with surface quad dominant mesh and uses an Advancing Front
scheme to fill as much of the volume as possible. For simple volumes, it can fill it completely. For more
complicated volumes, it usually fills several layers in from the surface with hexa elements and then fills
the middle with tetras and pyramids. Then a diagnostic is run, and if those central elements are poor,
the inner volume will be meshed again with the Delaunay mesher. The surface mesh will be created
with the parameters defined under Global Mesh Setup or Surface Mesh Setup. The volume mesh will
then be generated from this surface mesh. If a surface mesh exists, you can also choose to specify Existing Mesh for the Input.
Remesh Center
deletes tetra elements from the center region of the mesh, and remeshes it using the Delaunay mesher.
This will result in better quality mesh at the center region.
Cartesian
The Cartesian option will generate a Cartesian mesh using a top-down meshing approach. This creates
pure Cartesian and unstructured Cartesian meshes with H-Grid refinement. The mesher works by continuously refining the initial grid in a binary fashion in each dimension, and eliminating the non-volume
288
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
cells, up to the specified maximum refinement. The Cartesian mesher does not require an existing surface
mesh and will ignore meshing parameters defined to control local surfaces.
The following mesh methods are available.
Body-Fitted
Hexa-Core
Body-Fitted
The Body-Fitted option creates unstructured hexa mesh of uniform size based on Cartesian mesh and
fits it to the geometry. This works for both CAD and STL geometries. The mesher can handle “dirty”
geometries as long as the cell size is larger than the gap size.
Note
The cell size should be smaller than the thickness of the model.
Projection Factor
controls the tightness of the body-fitted Cartesian mesh to the geometry. Values can range from 0 to
1.0, where a value of 0 indicates Cartesian mesh totally free from the geometry, and a value of 1.0 indicates
mesh that is strictly on the geometry.
Split Degenerate
splits boundary quad and hexa elements with flat corners (triangular shaped), and propagates this split
to produce higher quality elements. This option does not introduce pyramids or tetra elements.
Note
The shorter edge length introduced by this option may pose a problem for some users
such as reducing the time step for explicit solvers. Also, the quality improvement is
usually not as good as the improvement produced by the Create Pyramids option. It is
recommended that you try different options to determine which produces the best result
for a particular topology and for a particular solver/physics.
Figure 264: Body-Fitted Cartesian Mesh with Boundary Hexa Elements (p. 290) shows the BFC mesh
having boundary hexa elements with flat corners.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
289
Mesh
Figure 264: Body-Fitted Cartesian Mesh with Boundary Hexa Elements
Figure 265: Split Degenerate Option (p. 290) shows the results of using the Split Degenerate option.
The boundary hexa element has been split and the split is propagated through the neighboring
elements.
Figure 265: Split Degenerate Option
For this model, the use of an inflation layer proves to provide the best quality, as shown in Figure 266: BFC Mesh with Inflation Layer (p. 291).
290
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Figure 266: BFC Mesh with Inflation Layer
Create Pyramids
remeshes bad quality hexa elements (with determinant quality less than 0.05) using a Delaunay algorithm.
This effectively replaces the poorest hexa elements with higher quality tetra and pyramid elements.
Refinement Type
Uniform
creates hexa elements of uniform size.
2-to-1
creates hexa elements of varying size with 2-to-1 size transition. This will introduce hanging nodes
in the mesh.
3-to-1
creates hexa elements of varying size with 3-to-1 size transition. This mesh can be made conformal
using the Edit Mesh > Resolve refinements option for limited configurations.
Aspect Ratio
allows you to control the aspect ratio of the otherwise uniform Cartesian mesh. This can be used to fill
the volume more efficiently in cases where there is a strong gradient aligned with the coordinate system.
The default setting is 1 1 1. Changing the aspect ratio allows you to stretch the Cartesian grid. For
example, setting the aspect ratio to 1 2 0.75 will result in a Cartesian mesh that is twice as long in
the Y direction as the X direction and 0.75 times the size in the Z direction. This is applied to the entire
model.
You can also create a Cartesian file with varying aspect ratio. Use the Hexa blocking tools to create
a block with splits and edge parameters to control the distribution. Then, use the File > Blocking
> Write Cartesian Grid option to convert the blocking to a Cartesian grid file. You can then refer
to this file when computing the grid (see the Cartesian file (p. 344) option for details).
Figure 267: Hexa Mesh With Varying Aspect Ratio (p. 292) shows the Cartesian mesh for a Femur,
with the aspect ratio varying along the shaft.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
291
Mesh
Figure 267: Hexa Mesh With Varying Aspect Ratio
Project Inflated Faces
allows full projection to the surface for inflated faces rather than limiting the projection with the projection
factor.
Outer Bounding Box
allows you to specify the outer mesh region for external flow meshes by setting the min-max coordinates
of the flow region. This can be used instead of explicitly creating the tunnel geometry.
min-max Coordinates
specify the explicit coordinates or click the selection icon to pick diagonal min and max coordinates to
specify the outer bounding box size.
Use active local coordinate system
allows you to orient the mesh along the active local coordinate system instead of along the global coordinate system. LCS are translated to equivalent Cartesian coordinates.
Boundary Layers
The Body-Fitted Cartesian mesher can create a layer of hexa elements parallel to the wall. These are
necessary for properly capturing curvature and can be subdivided to get boundary layers. For some
geometry parts, such as inlets, outlets and “flat” sides, you may not want to have this offset. However,
you may want to apply inflation to flat parts if they are not in the Cartesian planes (X Y Z) to prevent
stair-stepping. To determine if a part will have a single offset layer (with uniform aspect ratio), enable
prism for the appropriate parts in the Part Mesh Setup dialog. For ANSYS ICEM CFD, standard prism
controls do not apply for Body-Fitted Cartesian meshing. Instead, if the prism option is enabled for a
specific part, and then meshed using the Cartesian Body-Fitted method, the boundary layer will be
offset. The boundary layer is determined on a part by part basis, so parts must be created and surfaces
assigned appropriately.
Figure 268: Example of Boundary Layers in Body-Fitted Cartesian Mesh
292
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
In Figure 268: Example of Boundary Layers in Body-Fitted Cartesian Mesh (p. 292), the prism option is
enabled for the SURFS part containing the walls of the corner pipe but disabled for the INLET and
OUTLET parts. When the Body-Fitted Cartesian mesh is computed, the boundary layer is grown along
the SURFS part to better capture curvature, but terminates at the INLET and OUTLET. This single
boundary layer can then be split to increase near wall resolution if needed.
Define Thin Cuts
The Define thin cuts option allows you to prevent elements stretching across a gap. You can define
the thin cut pair using the Define thin cuts button in the Tetra/Mixed Meshing parameters for the
Robust (Octree) mesh method (see the Define thin cuts (p. 282) option).
Note
The thin cuts option works best for regions of the mesh which will be cut away, rather than
thin solid regions where the mesh is to be retained.
Hexa-Core
The Hexa-Core option will generate a hexa-core mesh using a bottom-up meshing approach. It will
retain the tri surface or prism mesh, delete the existing tetra mesh, and remesh the volume interior
with Cartesian meshing. The tetra elements will be mapped to the tri or prism faces with the Delaunay
algorithm.
Note
Hexa-Core is implemented as part of Tetra meshing. Under Compute Mesh > Volume
Mesh, the Create Hexa-Core option can be selected when using Tetra/Mixed Mesh
Type, and Robust (Octree) or Quick (Delaunay) Mesh Methods.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
293
Mesh
Figure 269: Example of Hexa-Core Mesh
Fill holes in volume mesh
will remesh only the missing tetra portions. This option is required only for multiple tetra fill volume
regions. It is disabled by default, as it is not necessary for single volume fill (internal meshes).
Refinement Type
Uniform
creates hexa elements of uniform size.
2-to-1
creates hexa elements of varying size with 2-to-1 size transition. This will introduce hanging
nodes in the mesh.
3-to-1
creates hexa elements of varying size with 3-to-1 size transition. This mesh can be made conformal using the Edit Mesh > Resolve refinements option for limited configurations.
Outer Bounding Box
allows you to specify outer mesh region for external flow meshes.
min-max Coordinates
specify the explicit coordinates or click the selection icon to pick diagonal min and max coordinates
to specify the outer bounding box size.
Use active local coordinate system
allows you to orient the mesh along the active local coordinate system instead of along the global
coordinate system.
Prism Meshing Parameters
The Prism Meshing Parameters include global prism settings as well as more advanced options.
You can create prisms from existing volume or surface mesh.
See the Prism Mesh section in the User's Guide for more general information on Prism Meshing.
Global Prism Settings
Growth Law
determines the height of the layers given the initial height and height ratio.
• Linear
294
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
The prism height of a particular layer is defined by h(1+(n-1)(r-1)), where h=initial height, r=height
ratio, and n=layer number. The total height at layer n is:
nh((n-1)(r-1) + 2)/2.
• Exponential
The prism height of a particular layer is defined by h*r(n-1), where h=initial height, r=height ratio,
and n=layer number. The total height at layer n is:
h(1-rn)/(1-r).
• WB-Exponential
This is the exponential growth law as defined in ANSYS Workbench. The prism height of a particular layer is defined by h*exp((r-1)(n-1)), where h = initial height, r = height ratio, and n = layer
number.
Figure 270: Prism Growth Law (p. 295) shows a box with edge length = 1, h = 0.05, r = 1.5, and n =
5, with different growth laws applied.
Figure 270: Prism Growth Law
Initial height
is the height of the first layer of elements.
Note
If the initial height is set to 0, it will be automatically determined by the local triangle
size, where the height of the last layer will be the minimum attached triangle edge length
times the Prism height limit factor.
Height ratio
is the expansion ratio from the first layer of elements on the surface. This ratio will be multiplied by the
element height of the previous layer to define the height of the next layer.
Number of layers
is the number of layers to be grown from the surface or curve.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
295
Mesh
Total height
is the total height of all the prism layers.
Note
If neither the initial height nor the total height is set, the prism layer heights will be
“floating” in order to produce a smooth volume transition to the tetrahedra (see Figure 271: All Prism Heights Floating (p. 296)). In order to smooth the volume transition, the
last prism layer height must not exceed a certain height-to-base ratio. This value is 0.5
by default, but can be adjusted using the Prism height limit factor.
The Prism height limit factor combined with the shortest edge of the base triangle for
each column are used to calculate the last prism height for each column. This is combined
with the growth ratio, number of layers and the growth law to back calculate the initial
height required for each column in order to produce a smooth growth ratio. If you would
rather have a fixed initial height, you can redistribute the prism layers later.
You can use a combination of floating prism layer height and prescribed initial/total
height on selected entities/parts (see Figure 272: Combination of Prescribed and Floating
Prism Heights (p. 297)). In this case, the initial height has been set on only the valve part.
The prism heights on the valve part are now calculated using the specified initial height
along with the growth law, ratio, and number of layers. All other prism heights remain
floating.
Figure 271: All Prism Heights Floating
296
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Figure 272: Combination of Prescribed and Floating Prism Heights
Interpolate Heights
if set to On, determines the prism layer heights of prism nodes without given heights by constructing
new data points from prism nodes with fixed heights. If there are no fixed heights, the size of the triangle
is used. By default, Interpolate Heights is off.
Compute params
will compute the missing parameter based on the given parameters if one of the parameter values is
blank.
Fix marching direction
if enabled, prisms are grown in a direction normal to the base triangles on the surface. However, the
quality of mesh is still controlled by Min prism quality.
When Fix marching direction is enabled, directional smoothing applies only to the first layer. The
initial direction is evaluated from the face normals attached to the vertex to be extruded. This is
done by interpolation. For further layers, the direction is “fixed” and directional smoothing is disabled.
Figure 273: Use of the Fix Marching Direction Option
Fix Marching Direction Disabled
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
297
Mesh
Fix Marching Direction Enabled
In the first example in Figure 273: Use of the Fix Marching Direction Option (p. 297), Fix Marching
Direction is disabled and the prism direction is controlled by the directional smoothing steps and
the Ortho weight value. In the second example, Fix Marching Direction is enabled. The prisms
grow normal to the surface, except in cases of extremely poor quality first layer elements.
In the next set of examples in Figure 274: Fix Marching Direction Option (p. 298), prisms were grown
largely orthogonal to the base triangles up to the 3rd layer, beyond which the Min prism quality
caused a change in direction. This method may be more appropriate when growing prism in the
VORFN region.
Figure 274: Fix Marching Direction Option
Fix Marching Direction Enabled
Fix Marching Direction Disabled
Note
If you do not use any directional smoothing, the prism marching direction is already
fixed.
Min prism quality
locally prevents or adjusts prism growth in problem areas in order to maintain quality. Complex geometry
combined with aggressive prism parameters may result in poor quality elements. If the quality does not
meet the minimum value, the prism elements are re-smoothed directionally, or pyramids are used to
replace some prism elements. Setting a value that is too high will result in local prism interruptions and
more pyramids.
Table 8: Effect of Min Prism Quality and Initial Height (p. 298) demonstrates the effect of Min prism
quality on prism mesh of two different initial heights.
Table 8: Effect of Min Prism Quality and Initial Height
Initial Height = 0.15, Growth Ratio = 1.2, Number of Layers =
5
298
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Min prism quality value
Actual Prism Quality
0.0
0.003
0.01
0.065
0.075
0.1
0.1
0.13
Initial Height = 0.1, Growth Ratio = 1.2, Number of Layers =
5
Min prism quality value
Actual Prism Quality
0.0
0.146
0.01
0.146
0.075
0.146
0.1
0.146
In contrast, for the mesh with an Initial Height of 0.1, the prism quality is already higher than the
Min prism quality value.
Ortho weight
is the weighting factor for the directional smoothing steps. The range is from 0 (to improve triangle
quality), to 1 (to improve prism orthogonality).
In the example in Figure 275: Ortho Weight = 0.1 (p. 299), the Ortho weight is set to 0.1. The
smoother focuses on improving the aspect ration of the triangle caps, which also results in improved
tetra quality.
Figure 275: Ortho Weight = 0.1
Figure 276: Ortho Weight = 0.5 (p. 300) illustrates the same mesh with Ortho weight = 0.5.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
299
Mesh
Figure 276: Ortho Weight = 0.5
Figure 277: Ortho Weight = 0.9 (p. 300) illustrates the mesh with Ortho weight = 0.9. The smoother
focuses on maintaining orthogonality with the wall, except when quality will be too poor.
Figure 277: Ortho Weight = 0.9
Ortho weight is applied during directional smoothing. If no directional smoothing is applied, the
mesh is grown orthogonal to the wall in a fixed marching direction and poor elements are simply
removed, as shown in Figure 278: No Directional Smoothing or Ortho Weight Applied (p. 300).
Figure 278: No Directional Smoothing or Ortho Weight Applied
300
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Fillet ratio
tries to create a fillet proportional to the total height of the prism. When prisms are grown in the corner
zone of a tet mesh, it is possible to control the smoothness of prism layer along a fillet using this parameter. A value of 0 means no fillets.
Note
For meshing corners with angles less than 60 degrees, there may not be space for a fillet.
Figure 279: Examples of Fillet Ratio
Fillet Ratio = 0.0
Fillet Ratio = 0.5
Here, the radius of the inner prism fillet is 0.5 times the height of the total prism
thickness.
Fillet Ratio = 1.0
Max prism angle
controls prism layer growth around angles and when adhering to adjacent surfaces. This is the maximum
internal angle between the base and the extruded direction. This parameter can range from 140 to 180
degrees. If extruding from one surface and not its neighbor, and the angle between the two surfaces is
less than the specified value, the prisms will adhere to the adjacent wall.
For instance 135 is the theoretical minimum needed to go around a 90 degree corner (90+45
meeting up with the 90+45 coming from the other surface); to account for tolerances, the minimum
setting is 140 degrees. A max prism angle of 180 allows the mesh to fold back on to its self, like at
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
301
Mesh
the trailing edge of a wing or a cusp between pipes in a manifold (90+90 meeting up with the
90+90 from the other side).
Figure 280: Max Prism Angle – Example 1
Max Prism Angle = 140 degrees
Here, the angle between the planes is 158.2
(21.8) degrees. Since the Max prism angle
is less than the angle between the walls, the
prism layers are capped with pyramids.
Max Prism Angle = 180 degrees
Here, the Max prism angle exceeds the
separation angle between the surfaces, so
the prism remains attached to the adjacent
surface.
Figure 281: Max Prism Angle – Example 2
Max Prism Angle = 140 degrees
Here, the Max prism angle is set to 140, which is not
enough to meet the prisms from the under side of the
cusp.
Max Prism Angle = 180 degrees
Here, the Max prism angle is set to 180 and the Min
prism quality is set to 0.0001 so that the prisms from
the top surface can meet the prisms from the lower
surface. The prisms where the two surfaces meet have
large internal angles and poor quality.
Note
Pyramids are usually not favorable. However in “cusp” situations such that exist on
the trailing edge of a wing or within a manifold where two pipes meet at a slight
angle, it is better to have the prism layer terminate with pyramids than try to wrap
302
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
around the cusp. It is recommended to set Max prism angle to 160 degrees, particularly for applications with cusp geometry.
Max height over base
When the prism aspect ratio (ratio of height over base of the base triangle) reaches this value, the prism
stops growing.
The examples in Figure 282: Max Height Over Base (p. 303) illustrate the use of this option for a 6
layer prism mesh.
Figure 282: Max Height Over Base
No Value Set for Max Height Over Base
In this case, the prisms with a smaller base have the same height as the prisms with wider
bases. The resulting tall prisms have much greater volume than their adjacent tetra elements
and are not considered ideal.
Max Height Over Base = 1.0
If the Max height over base is set to 1.0, then the prism height can not exceed the average
base length. Prisms that would have exceeded this are not grown. Other prisms may not
grow due to related quality issues.
Max Height Over Base = 0.5
In this case, even the initial height would exceed this ratio for the elements in the corner,
so no prisms are grown there. Generally, the initial height at the wall would be less than
half the smallest element size.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
303
Mesh
Prism height limit factor
restricts the prism aspect ratio (height of each prism element over base size for each column) to the
specified value by limiting the prism growth ratio, but maintains the number of layers.
If the initial height is set globally or on a part or entity, and the growing prism layers reach the
specified aspect ratio, the growth ratio is reduced so that the height for additional layers will remain
constant at that height limit factor (aspect ratio).
If the initial height is not set globally and not set on the part or entity, it will “float” (see the Total
height section) to improve the transition to the tetrahedra. You can then use the prism height
limit factor to control the transition by adjusting the maximum height-over-base ratio of the prisms.
This will be used to calculate the initial heights on a column by column basis and so that a single
growth ratio will be used and produce a smoother transition to the maximum prism height for each
column. If the initial height is left to “float” and the prism height limit is not set, a value of 0.5 will
be used to obtain smooth volume transition from the prisms to the attached tetra.
Figure 283: Prism Height Limit Factor
No Value Set for Prism Height Limit Factor
Prism Height Limit Factor = 0.5
Prism Height Limit Factor = 1.0
304
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Ratio multiplier
only applies to the Exponential Growth Law. This value is multiplied to the height ratio for each successive layer. For example, if the Height Ratio is set to 1.2, and the Ratio multiplier set to 1.1, then the
ratio between the first two layers will be 1.2, the ratio between the second and third layer will be (1.2
* 1.1), the ratio between the third and fourth layer will be (1.2 * 1.1 * 1.1), etc. The default value is 1.
The Ratio max option under Advanced Prism Meshing sets the maximum ratio value.
Prism Element Part Controls
These settings are required when growing prism mesh without an existing tetra mesh. A part name is
required to assign the prism elements correctly. This can be done by typing a new name or selecting
from the list of parts.
You may assign a different volume part to the prism, or add a side or top part in order to better differentiate it from the tetra region. In this case, be sure to add the prisms to the main volume part before
generating output to the solver so it will be seen as one volume.
You may want to grow prisms away from the flow domain (towards the outside region). In this case,
the top triangles (Top Part), as well as side quads (Side Part) must also be assigned to named parts.
New volume part
allows you to specify a new part for prism elements, either from an existing surface or volume mesh.
Side part
allows you to specify a part for the quad faces on the side boundaries of the prism elements.
Top part
allows you to specify a part for the tri faces capping off the top of the last prism layer.
Extrude into orphan region
allows you to extrude prisms away from the existing volume, instead of into it.
In Figure 284: Prisms Extruded into the Orphan Region (p. 306), prism mesh was extruded from the pipe
mesh region. The part STEEL_SIDE represents the metal's thickness.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
305
Mesh
Figure 284: Prisms Extruded into the Orphan Region
Smoothing Options
Number of surface smoothing steps
is the number of iterations that the surface mesh is smoothed before prism layer generation. The quality
of the final prism mesh mostly depends on triangle quality. It is recommended to start with quality above
0.3.
Note
Set smoothing steps to 0 while extruding only one layer. Otherwise the default value is
usually adequate.
Triangle quality type
specifies various quality criteria for improving the triangular surface mesh by smoothing. This operation
is performed at the beginning as well as before extruding a new layer.
When Laplace is selected, the mesh is improved using the Laplace elliptic solver. Separate
weighting is given for orthogonality and triangle quality.
Note
Laplace smoothing is typically best for final prism quality.
306
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Number of volume smoothing steps
is the specified number of smoothing steps on the existing Tetra mesh before prism layer generation.
A smooth Tetra mesh is essential for a high quality prism mesh. Smooth the Tetra mesh and perform all
diagnostics before running this smoother, in which case you may reduce the number of iterations.
Note
The smoother is much more effective before prism mesh is grown.
Note
If extruding only one layer, set smoothing steps to 0. Otherwise the default value is
usually adequate.
Max directional smoothing steps
is the number of smoothing steps for the face normal vectors before the next prism layer is created. The
default value is appropriate for most problems.
First layer smoothing steps
smooths the first layer with the given number of steps.
Advanced Prism Meshing Parameters
Auto Reduction
In some cases, the prism mesher is unable to create the specified number and size of layers due to
geometry constraints. If this option is enabled, the prism mesher will automatically reduce the layer size
to meet the required number of layers without creating pyramids or other problems in the mesh.
This is useful for solvers that require complete prism layers with no pyramids. In Figure 285: Example
of Auto Reduction (p. 307), the prism parameters were set for 6 layers. Without Auto Reduction,
there will be stair stepping down to 4 layers in the gap. With Auto Reduction enabled, the mesher
created 6 layers as specified by automatically reducing the layer size to fit and redistributing the
prism layer as appropriate to improve quality.
Figure 285: Example of Auto Reduction
Auto Reduction disabled
Auto Reduction enabled
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
307
Mesh
Blayer 2d
This option is used to create a boundary layer in a 2D mesh using prism meshing. This surface mesh can
be used with a 2D solver or swept to create the volume mesh.
Note
Using Prism BLayer 2D is more advanced than applying an Offset with the Patch Independent meshers. Offset is controlled by setting the Height, Ratio and Number of layers
parameters on the curves. 2D prism controls are the same as regular prism controls, except
you must select the surface part as well as the curve part. 2D Prism can also be applied
on an existing shell mesh in the same way that 3D prism is applied to an existing tetra
mesh.
Note
Since 2D prisms are really just quads, the split prism and redistribute prism commands
do not work.
2D prism works with quad or tri mesh and can be controlled with the 3D prism controls to adjust
number of layers, initial height, orthogonality, etc.
Figure 286: BLayer 2D Applied to a 2D Surface with Quad Mesh
Figure 286: BLayer 2D Applied to a 2D Surface with Quad Mesh (p. 308) shows a 2D surface with
quad mesh, with prism applied to the top and left curves.
308
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Figure 287: BLayer 2D Applied to a 2D Surface with Tri Mesh
Figure 287: BLayer 2D Applied to a 2D Surface with Tri Mesh (p. 309) shows a 2D surface with tri
mesh, with prism applied to the top and left curves. Note that the initial height is “floating” in this
case.
Figure 288: BLayer 2D and Additional Prism Parameters Applied to a 2D Surface with Tri Mesh
Figure 288: BLayer 2D and Additional Prism Parameters Applied to a 2D Surface with Tri Mesh (p. 309)
shows the same 2D surface with tri mesh, with prism initial height set to 1, ortho weight set to 0.5,
and number of layers set to 7.
Delete Base Triangles
If enabled, the triangles at the interface with the existing tetra elements will be deleted when growing
into ORFN regions.
Delete Standalone
If enabled, triangles that are not attached to anything will be deleted.
Do Checks
If enabled, additional checks are done on the mesh. These include checking interfaces between materials
and checking for pockets within the mesh. Results are reported in the message window and the prism
log file.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
309
Mesh
Do Not Allow Sticking
If enabled, “pointy” tetrahedra are not allowed to be stuck between layers.
Intermediate Write
If enabled, the prism file will be written out after each layer is created. This is a fail safe measure. If the
Prism mesher is not able to complete all the layers or is interrupted for some reason, you can load the
saved mesh file and continue. The mesh file will be located in your working directory and named
“prism.uns”.
Refine Prism Boundary
If enabled, this allows the Prism mesher to refine the boundary between the prisms and tetras, if this
will improve the mesh quality.
Stair Step
This option affects the behavior of the Stop Columns option, and is only effective if Stop Columns is
enabled.
If Stair Step is enabled, the difference in adjacent prism columns is limited to 1 layer. When disabled,
adjacent columns can have different numbers of layers that differ by more than 1.
Figure 289: Using the Stair Step Option (p. 310) shows the prism layers grown on a ship sail. Note
that when the Stair Step option is disabled, the prism layers are fully extruded on the sail.
Figure 289: Using the Stair Step Option
Stair Step option enabled
Stair Step option disabled
310
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Stop Columns
If enabled, a column of prisms is stopped if the marching direction cannot be determined or a collision
is detected. If disabled, and a collision is detected at any point, the entire next layer is stopped unless
Auto Reduction is also enabled. In many cases, disabling this option may cause the Prism mesher to
terminate prematurely.
Figure 290: Example of Stop Columns and Stair Step Options
Stair Step option enabled:
Stair Step option disabled:
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
311
Mesh
Use Existing Quad Layers
This option deals with cases where a prism layer meets a wall. If enabled, the software will attempt to
align the boundary of the prism layers to the existing quad surface mesh. If the existing mesh has a
different structure or the prism mesh has trouble mapping to the structure, then the prism faces will be
used for the surface mesh. If disabled, this option will adjust the existing mesh to follow the faces of
the uncovered prisms.
Use Prism V10
uses the ANSYS ICEM CFD Version 10 prism executable (prism_v10.exe) instead of the default executable.
Max Jump Factor
The maximum allowable jump in height between neighboring vertices (default is 5.0). If adjacent prism
columns exceed this ratio, the Prism mesher will terminate prematurely and an error message will note
that Max Jump Factor was exceeded.
Max Size Ratio
The maximum allowable size ratio when growing larger prisms into smaller tetra elements (default is
0.0).
Min Smoothing Steps
The minimum number of marching direction smoothing steps (default is 6). This does not override Max
directional smoothing steps, but acts as a lower limit.
Min Smoothing Val
The marching directions will be smoothed until the quality is above this value (default is 0.1) or the Max
directional smoothing steps is reached. If Min Smoothing Val is met, but the Max directional
smoothing steps has not been yet reached, smoothing will continue until the number of Min
Smoothing Steps have been completed.
Ratio Max
The maximum height ratio between prisms from one layer to the next.
Tetra Smooth Limit
The tetra elements will be smoothed until they are above this value (default is 0.3).
Read a Prism Parameters File
allows you to select an existing prism parameters file. This will be used to set all the prism parameters,
including Advanced Prism Meshing Parameters. These prism parameters files can be shared between
projects for consistency and easy setup.
Periodicity Set Up
The Periodicity Set Up option allows you to define periodicity.
Define Periodicity
ensures that the nodes line up from one periodic face to another.
Note
Behind the interface, periodicity is always defined in the global coordinate system.
However, it can be setup with an active local coordinate system (LCS). When you click
312
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Global Mesh Setup
Apply, the axis vector will be normalized and the LCS parameters will be converted to
global coordinates.
Note
Periodicity can be set for both Tetra and Hexa meshes.
Rotational periodic
This option ensures that the nodes will line up along an axis symmetric model, and also force the nodes
to be rotationally periodic with one another. An example of rotational periodicity is that a node and its
periodic counterpart on an opposing periodic face share the same R and Z coordinates of a cylindrical
coordinate system. ANSYS ICEM CFD has the ability to mesh all the way to the axis of rotation.
Figure 291: Rotational Periodic Geometry
There are three methods to defining the Rotational axis.
The User defined methods require the following parameters:
• Base
The base point of rotation (x y z).
• Axis
A vector defining the direction of the axis of rotation (i j k).
• Angle
The angle that makes up the computational domain within the axis symmetric model. An angle
of 360 degrees would mesh the entire rotational domain.
OR
Sectors
The number of sectors in 360 degrees that make up the entire rotational computational domain.
The Vector method requires 2 points to define the vector for the axis of rotation, and the angle to
define the rotational domain.
An example of a rotational periodic mesh is shown in Figure 292: Rotational Periodic Mesh (p. 314).
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
313
Mesh
Figure 292: Rotational Periodic Mesh
Translational Periodicity
This option ensures that the nodes line up along a translational symmetric model, as illustrated in Figure 293: Translational Periodic Geometry (p. 314) and Figure 294: Translational Periodic Mesh (p. 315). Enter
the Offset vector value that defines one periodic face from the other (Dx Dy Dz).
Figure 293: Translational Periodic Geometry
314
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Part Mesh Setup
Figure 294: Translational Periodic Mesh
Part Mesh Setup
The Part Mesh Setup option opens a dialog where you can specify the mesh parameters for different
parts, as shown in Figure 295: Part Mesh Setup Window (p. 315). Values defined here at the Part level
will override Global settings. If a value of 0 is entered for a parameter, the global parameter value will
be used.
Note
Entity level controls will override Part level parameter settings.
Note
Clicking the header cell for a parameter (e.g.,max size) will open up a window, which allows
you to specify the same parameter value for all available parts.
Figure 295: Part Mesh Setup Window
Prism
Select the parts that prism layers will be applied to. For each part, the Height, Height Ratio and the
Num Layers can be specified. Volume, Surface and/or Curve parts can be selected. When using the
Prism mesher in ANSYS ICEM CFD, the default prism parameters are set under Mesh > Global Mesh
Setup > Global Prism Settings. However, parameters that are entered here at the Part level will
override the Global settings. In addition, the entity settings of Height, Height Ratio, and Number of
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
315
Mesh
Layers will override the Part level settings. Entering zero for any of the settings will default back to
the Global Settings.
If there are multiple volume materials, and none have the prism option enabled, then prism
mesh will grow from the selected surface parts into the adjacent volumes. If only certain volume
parts have prism enabled, then prism mesh will be grown only into those volume parts. After
you enter the parameters, click Apply, and then Dismiss to close the window.
For 3D, the prisms are grown (inflated) from the shell (tri or quad) elements of each part. This
can be done with or without a volume mesh, but having a tetra volume mesh during inflation
helps with collision avoidance and ensures that you will have a volume mesh after prism generation is complete. For 2D, the prisms are grown (inflated) from the curve parts into the selected
surface parts (must be selected). The 2D prism only works if Advanced Prism Meshing Parameters
> Blayer 2D is enabled.
Note
At least one surface entity must be selected or the prism mesher will not run. Different prism heights can be specified on adjacent parts, though a transition region
with unspecified height is required in between these parts. If a surface part separates
two or more volume parts, select the volume parts on the side of the surface you
want to grow the prisms. If you select both sides, prisms will grow in both directions
from the surface part. If you want different prism properties on either side of a surface
grown into 2 volumes, do one at a time (run prism iteratively). If adjacent tri element
parts have heights that differ by more than a factor of 2, the prism mesher may fail
(this limit is controlled in the Advanced Prism Meshing Parameters). Not setting
a height for Prism, (here or in the Global Prism Parameters DEZ) will allow the
height to float. You can also allow the height to float globally and set specific initial
heights per part or on an entity by entity basis.
Hexa-Core
Enable this option to use Hexa-Core meshing for the volume part, and to set the desired parameters.
The global parameters for Hexa-Core meshing can be set under Mesh > Global Mesh Setup > Volume
Meshing Parameters > Cartesian Mesh Type > Hexa-Core Mesh Method. The default Max Size is
based on a weighted average of the perimeter surface elements.
If all or none are selected, Hexa-Core will fill all volumes (similar to Prism).
To enable Hexa-Core meshing for all available parts, click the hexa-core header and all available
parts will be selected.
Max Size
specifies the maximum element size. The actual maximum element size will be this value multiplied
by the Global Element Scale Factor.
Note
Local maximum element sizes defined on bodies/materials can be used to limit the
maximum size for the Hexa-Core method. For other methods, such as BFCart, Octree
Tetra or Delaunay Tetra, you will need to set the local maximum size using a density
region (refer to Create Mesh Density (p. 327) for details). This is because the material
is applied (via flood-fill from the material point) after subdivision is complete.
316
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Part Mesh Setup
Height
specifies the height of the first layer of elements normal to the surface or curve. For volume meshing,
this parameter affects the Hexa and Prism initial mesh layer height. For Patch Dependent Surface
meshing, when applied to a curve, this value can affect the initial height of the layer of quads along
that curve. For example, this could be used to specify the initial height of a quad ring around a bolt
hole.
Height Ratio
is the expansion ratio from the first layer of elements on the surface. This ratio will be multiplied
by the element height of the previous layer to define the next layer.
The default growth rate for the transition to the surface Max Size is 1.5. This growth rate can
be adjusted by setting the surface Height ratio to between 1.0 and 3. Sizes below 1.0 are inverted
(i.e., 0.667 = 1.5). Sizes above 3 are ignored and the default is used.
When applied to curves, the Height Ratio can have several effects on Patch Dependent meshing.
When used with an initial Height and Number of Layers, it determines the growth rate of one
layer of quads over the previous layer. When used with the Adapt Mesh Interior setting, it
affects how quickly the mesh transitions from the curve sizes to the surface sizes.
Num Layers
is the number of layers to be grown from the surface or curve.
Tetra Size Ratio
controls the growth (edge length) of tetra mesh as it moves away from the surface.
For Octree Tetra mesh, size transitions are 2 to 1 locally, but you can still affect the transition
rate over a larger number of transitions. For example, if the surface size is 2 and the volume
size is 64, you may see something size transitions like the following:
Delaunay
2
3
4.5
6.75
10.13
15.19
22.78
34.17
51.26
76.89
Octree
2
2
4
4
8
8
16
32
32
64
If the ratio was 1.5, the big picture would show both the Octree and Delaunay sizes growing
at a rate of 1.5, but the Octree method has to fit it to powers of 2 times the smallest size in
the model. Also, you can imagine that changing this to 1.4 or 1.6 might not make that much
difference to the Octree mesher, at least not for the first few layers, but would directly change
the Delaunay progression.
Tetra Width
creates the specified number of tetra layers with element size as specified by the Max Size.
Min size limit
Mesh elements will be limited from being subdivided smaller than this value. For Tetra meshing,
this value overrides the value calculated by the Curvature/Proximity Based Refinement option.
The actual minimum size will be the value multiplied by the Global Element Scale Factor.
This parameter works only with the Curvature/Proximity Based Refinement option. You can
override the global setting on particular entities or parts if this is set smaller than the global
setting. Min size limit functions to limit the amount of Curvature/Proximity Based Refinement,
however, if the sizing function is satisfied without refining down to this minimum size, it will
stop on its own and may never refine down to this Min size limit value.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
317
Mesh
Max Deviation
is a method of subdivision based on the proximity of the centroid of a tri or quad surface element
to the actual geometry. If the distance is greater than this value, the element will automatically split
and the new nodes will be projected onto the geometry. The actual distance is the value multiplied
by the Global Element Scale Factor.
Int Wall
if enabled, the part will be meshed as an internal wall. This applies to Octree Tetra Meshing only.
This is necessary if you wish to mesh the surface of an internal wall within a volume.
Split Wall
if enabled, the part will be meshed as a split wall with overlapping pairs of elements and nodes, so
that both sides of the wall are effectively treated as having surface elements. This applies to Octree
Tetra Meshing only.
Show size params using scale factor
adjusts the reference element display to show the actual Max Size on each entity after multiplying
the set maximum size by the Global Element Scale Factor. To display this size for each entity, use
the display options in the Display Tree, such as the Tetra Sizes or Hexa Sizes options under Surfaces.
Apply inflation parameters to curves
allows you to apply the inflation parameters (Height, Height ratio, and Num. layers) to curves. By
default, these parameters are applied only to surfaces because these options can produce a different
result with the Patch Dependent Surface mesher when applied to curves. For instance, if you intend
for these parameters to affect only Prism generation (volume mesh), they should not be applied to
the curves if you also intend to use the Patch dependent surface mesher and do not want the surface
mesh to be affected.
Remove inflation parameters from curves
allows you to remove any parameters related to inflation layers from curves.
Surface Mesh Setup
The Surface Mesh Setup option allows you to set mesh parameters for selected surfaces. For
models with blocking, this applies only to 3D blocking.
318
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Surface Mesh Setup
Figure 296: Surface Mesh Setup
Surface(s)
specifies the surfaces for which meshing parameters are to be defined.
Maximum size
specifies the maximum element size. The actual size is this value multiplied by the Global Element Scale
Factor. You may end up with small elements on the selected entities if you are using Curvature/Proximity Based Refinement or Maximum Deviation.
Height
is the height of the first element, normal to the entity. This value applies to Hexa mesh only, and can
be any positive real number.
Height ratio
is the expansion ratio from the first layer of elements on the surface. This ratio will be multiplied by the
element height of the previous layer to define the next layer. This value is used for Prism and Hexa mesh,
and can be any positive real number.
The default growth rate for the transition to the surface Max Size is 1.5. This growth rate can be
adjusted by setting the surface Height ratio to between 1.0 and 3. Sizes below 1.0 are inverted (i.e.,
0.667 = 1.5). Sizes above 3 are ignored and the default is used.
Number of layers
is the number of layers to be grown from the surface or curve.
Tetra width
creates the specified number of tetra layers with element size as specified by the Max size.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
319
Mesh
Tetra size ratio
controls the growth of tetra as it move away from the surface. It is used for Tetra mesh.
Min size limit
Mesh elements will be limited from being subdivided smaller than this value. This option is the same as
Curvature/Proximity Based Refinement, but is applied locally to the selected part or entities. This is
a factor that is multiplied by the Global Element Scale Factor.
This parameter works only with the Curvature/Proximity Based Refinement option. You can
override the global setting on particular entities or parts if this is set smaller than the global setting.
Min size limit functions to limit the amount of Curvature/Proximity Based Refinement, however,
if the sizing function is satisfied without refining down to this minimum size, it will stop on its own
and may never refine down to this Min size limit value.
Maximum deviation
is a method of subdivision based on the proximity of the centroid of a tri or quad surface element to
the actual geometry. If the distance is greater than this value, the element will automatically split and
the new nodes will be projected onto the geometry. The actual distance is the value multiplied by the
Global Element Scale Factor.
Note
This only applies to the interior of surface mesh, not to the boundary. Node bunching
settings for the boundary curves will still be respected.
Mesh type
specifies the mesh type for the selected surface. If a mesh type is selected for a specific surface, then
this will override the global mesh settings. See Global Mesh Setup > Shell Meshing Parameters for a
description of mesh types.
Mesh method
specifies the mesh method for the selected surface. If a mesh method is selected for a specific surface,
then this will override the global mesh settings. See Global Mesh Setup > Shell Meshing Parameters for
a description of Mesh methods.
Remesh selected surfaces
allows you to remesh selected surfaces after changing surface mesh parameters. The new surface mesh
will automatically be generated.
Blank surfaces with params
when toggled, the surfaces with parameters applied to them will be make invisible or visible.
Curve Mesh Setup
The Curve Mesh Setup option allows you to set mesh parameters for curves. This feature is useful
for both surface and tetra meshing in controlling mesh size or distribution on surface boundaries. There
are several parameters, but in most cases setting the element size is sufficient for meshing.
There are the following methods for setting the Curve Mesh Size:
• Figure 297: Curve Mesh Setup – General (p. 321): This method involves entering the parameter values
in the provided fields.
320
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Curve Mesh Setup
• Figure 298: Curve Mesh Setup – Dynamic (p. 325): This method allows you to select a curve and adjust
the values using the mouse buttons.
• Figure 299: Curve Mesh Setup – Copy Parameters (p. 326): This method allows you to copy curve mesh
parameters to the selected curve(s).
Figure 297: Curve Mesh Setup – General
General
allows you to enter the following parameter values in the respective fields:
Select Curve(s)
specifies the curves for which mesh parameters are to be defined.
Maximum size
is the maximum element size for the selected curves. The actual element size will be this value
multiplied by the Global Element Scale Factor. The element size can be displayed by right clicking
on Curves in the Model tree and selecting Curve Tetra Sizes or Curve Hexa Sizes.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
321
Mesh
Number of nodes
is the number of elements for the selected curves. This is an alternative option to setting the element
size. The number of elements entered should be more than 2. The node spacing can be displayed
by right clicking on Curves in the Model tree and selecting Curve Node Spacing.
Height
is the height of the first elements, normal to the curve. This value applies to Hexa mesh and Patch
Dependent Surface mesh, and can be any positive real number.
Height Ratio
is an expansion ratio from the first layer of elements on the curve. This ratio will be multiplied by
the element height of the previous layer to define the next layer. You can enter any positive real
number. This parameter applies to Hexa, Prism mesh, and Patch Dependent Surface mesh.
Number of layers
is the number of layers to be grown from the surface or curve.
Tetra width
creates the specified number of tetra layers with element size as specified by the Max size.
Min size limit
Mesh elements will be limited from being subdivided smaller than this value. For Tetra meshing, this
value overrides the value calculated by the Curvature/Proximity Based Refinement option. The
actual minimum size will be the value multiplied by the Global Element Scale Factor.
This parameter works only with the Curvature/Proximity Based Refinement option. You can
override the global setting on particular entities or parts if this is set smaller than the global
setting. Min size limit functions to limit the amount of Curvature/Proximity Based Refinement,
however, if the sizing function is satisfied without refining down to this minimum size, it will
stop on its own and may never refine down to this Min size limit value.
Maximum deviation
is a method of subdivision based on the proximity of the centroid of a tri or quad surface element
to the actual geometry. If the distance is greater than this value, the element will automatically split
and the new nodes will be projected onto the geometry. The actual distance is the value multiplied
by the Global Element Scale Factor.
Advanced Bunching
contains options providing more control over the mesh parameters. Refer to Blocking > Pre-Mesh
Params > Edge Params > Bunching Laws for more detailed explanation.
Bunching law
BiGeometric
This is the default bunching law. The two initial heights and ratios define parabolas in a coordinate system where the number of node points is the X-axis and the cumulative distance
along the edge is the Y-axis. The parabolas are truncated where their tangent lines are
identical; the spacing is linear between these points. If there are not enough nodal points to
form this linear segment, a hyperbolic law is used and the ratios are ignored.
Biexponential
The spacing of the node intervals is calculated according to the law specified for Exponential
1 and 2. However, Spacing 1, Ratio 1, Spacing 2 , and Ratio 2 are used to define the distribution. The Spacing 1 and Ratio 1 parameters define the distribution from the beginning of the
322
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Curve Mesh Setup
edge to the midpoint of the edge, and Spacing 2 and Ratio 2 define the distribution from
the terminating end of the edge to the midpoint of the edge.
Curvature
The spacing of the node intervals is calculated according to the curvature of the function
defining the distribution.
Exponential 1
The spacing of the i'th interval is defined as a function of the Spacing 1 and Ratio parameters.
Exponential 2
The same as Exponential 1, except that the Spacing 2 and Ratio 2 parameters are used and
the distribution starting point is the terminating end of the edge.
FullCosinus
The spacing of node intervals is calculated using the cosine function. The ends of the edge
have the same constraint values for spacing and ratio.
Geometric 1
Spacing 1 is used to set the first distance from the starting end of the edge, with the remaining
nodes are spaced with a constant growth ratio. Only Spacing 1 is specified.
Geometric 2
The same as Geometric 1, except that Spacing 2 is used to define the distribution starting
from the terminating end of the edge.
HalfCosinus1
The spacing pattern follows a half cycle of a Cosine function. The parameters for spacing and
ratio differ on either end.
HalfCosinus2
The spacing pattern follows a half cycle of a Cosine function. The parameters for spacing and
ratio are similar to HalfCosinus 1, but distribution starts from the opposite end.
Hyperbolic
The spacing at each end are used to define a hyperbolic distribution of the nodes along the
edge. You can set Spacing 1 and Spacing 2, and the growth ratios are determined internally.
Linear
The spacing of the node intervals is calculated using a linear function.
Poisson
The spacing of the node intervals is calculated according to a Poisson distribution. Requested
values of Spacing 1 and Spacing 2 are used. Requested values of Ratio 1 and Ratio 2 are not
used directly, but are used to determine if the requested spacing is appropriate. If not, the
spacing will be adjusted automatically.
Uniform
The nodes along the edge are uniformly distributed.
Spacing
The spacing of the first node from the beginning of the edge (first cell height). When an edge
is selected, an arrow appears along the edge. Spacing 1 refers to the parameters at the beginning
end of the arrow, and Spacing 2 refers to the edge end where the arrow is pointing.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
323
Mesh
Ratio
specifies the growth rate from one cell height to the next. Ratio 1 refers to the parameters at
the beginning end of the arrow, and Ratio 2 refers to the edge end where the arrow is pointing,
as shown in the figure below.
Max Space
specifies the maximum element spacing of the curve.
Curve direction
displays the curve direction with a yellow arrow along the curve at the midpoint. The arrow
points from side1 (spacing 1 and ratio 1) toward side2 (spacing 2 and ratio 2). This is enabled
by default.
Reverse direction
reverses the curve direction.
Note
The Reverse direction button just flips side 1 and 2, it does not reverse the
spacing, the bunching law, etc.
Adjust attached curves
adjusts the mesh sizes on attached curves with the specified parameters. This applies to curves that
are attached at an angle between 60 and 120 degrees only. In order to select this option, the Max
size parameter and the bunching law of the reference curve must be specified. The attached curves
will automatically be assigned one of the following bunching laws, depending on the curve direction:
Geometric 1, Geometric 2, or BiGeometric. The curve bunching of the attached curves will correspond
to the values of Height and Height Ratio for the reference curve.
Remesh attached surfaces
allows you to change the mesh by changing the element size or number of elements on the curve.
This option should be used when meshing has been completed, but you want to change the curve
mesh sizes. The new surface mesh will automatically be generated.
324
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Curve Mesh Setup
Figure 298: Curve Mesh Setup – Dynamic
Dynamic
Select the curve parameter to be modified by clicking the increment/decrement icon ( ) next to it.
This will display the values for that parameter for each curve. You can then select the value for a specific
curve and use the left mouse button to increase the value or the right mouse button to decrease the
value in increments set in the Value field.
Curve Properties (Dynamic)
allows you to specify the increment for specific curve mesh parameters in dynamic mode. Select the
curve mesh parameter in the Incr/Decr for field, enter the value by which to increment/decrement
the parameter in the Value field, and click Apply in the Curve Properties (Dynamic) group box.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
325
Mesh
Figure 299: Curve Mesh Setup – Copy Parameters
Copy Parameters
allows you to copy curve mesh parameters to the selected curve(s).
From Curve
allows you to select the curve to copy the parameters from.
To Selected Curve(s)
specifies the curve(s) to which the parameters will be copied.
Copy
Relative
allows you to copy the parameters from the source curve relative to the curve length of the
specified curve(s).
Absolute
allows you to copy the exact parameters from the source curve to the specified curve(s), regardless
of curve length.
326
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Mesh Density
Blank curves with params
blanks curves with prescribed parameters. Curves without parameters will remain visible.
Note
The number of nodes and the meshing laws specified take precedence in determining the
number of nodes. Then spacings 1 and 2 are equally balanced, followed by ratios 1 and 2,
which are also equally balanced, and finally Max space is considered.
Create Mesh Density
The Create Mesh Density option allows you to create or manipulate a density region. This is a
polyhedral (or polygonal for 2D) zone in which one can prescribe a local maximum element size. This
is useful for refining the mesh in a volumetric zone that is not adjacent to any geometry, for example,
in the wake region of a vehicle. You can have density regions within one another, or partially intersecting
one another.
Figure 300: Create Density DEZ
Figure 301: Example of Mesh Density
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
327
Mesh
A smaller mesh size within one density region will supersede that of a greater mesh size if they overlap
or intersect. The density region does not have to be totally within the volumetric domain, but can intersect geometry and partially be within the dead zone.
Note
The density region is not part of the geometry, and mesh nodes are not constrained to the
density region.
Note
This affects only Tetra, Cartesian, and Patch Independent surface mesh methods.
Name
specifies the name for the density region. Enter an appropriate name or accept the default.
Size
specifies the local maximum mesh size that can occur within the density region. This will be multiplied
by the Global Scale Factor.
Ratio
specifies the tetra growth ratio away from the density region.
Width
For a density region, this specifies the number of layers (N) of the specified element size away from the
boundary of the density region that should have a constant expansion ratio. The layer N + 1 will have
a tetra size of the Size value multiplied by the Ratio.
For line and point densities, the Size value multiplied by the Width is the radius of the region that
the density region influences.
Density Location
The location of the density region can be defined in the following ways:
• From Points
Select one or more points to define the boundaries of the density region.
• From Entity Bounds
Select an entity to define a density region within its boundaries.
328
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Define Connectors
Define Connectors
The Define Connectors option allows you to define connectors. Connectors are meshing directives
assigned to geometry so that when the geometry is meshed, mesh links are created between different
parts. Line or shell elements are created to link parts with node to node connections. In general, mesh
connectors are defined with the geometry so that if a geometry is updated parametrically, the connectors
can be updated from one tetin file to a second tetin file. See Main Menu > File Menu > Import Geometry > Reference Geometry for more information.
Figure 302: Define Connectors Options
The various types of connectors are shown in Figure 302: Define Connectors Options (p. 329).
Arbitrary Connectors
Bolt Weld Connectors
Seam Weld Connectors
Spot Weld Connectors
Spot Weld From File
Arbitrary Connectors
The Arbitrary Connectors option allows you to create arbitrary connectors between any two entities. Each node of the start entity will have a connector to the end entity, but the end entity does not
have to have all of its nodes connected. Arbitrary connectors are always created from the nearest point
of the first entity to the nearest point of the second entity. The following options are available:
Arbitrary connector name
You can enter a name for the arbitrary connector, or use the default name.
Source
You can either select entities (generally curves) or existing parts as the source.
Target
Target entities are surfaces or parts containing surfaces. If only one or some of the surfaces of the part
are to be selected for the target, then use the Entities method. If all the surfaces in the part are required
to be selected, then use the Existing Part method.
Note
Ensure that the source and the target entities are selected in the correct order, select
the source entity first and then the target entity.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
329
Mesh
Connector Part Name
The part name for the connectors is automatically generated, starting with ARB_WELD0.
Max projection
A value slightly more than the distance between the source and the farthest target surface.
Active
If disabled, the connector will not be created when remeshing.
Bolt Weld Connectors
The Bolt Weld Connectors option allows you to create bar elements inside a hole which all connect
to one node at the center. These are also named bolt spiders because of their appearance. It is important
to put the bar elements which circle the hole into a part of their own, because connectors will be created
from all the bars in the specified part. If hole curves are put into a separate part before surface meshing,
hole bars will automatically be in a separate part from the rest. This is because when the surface
mesher runs, bar elements are put in the same part as the curves they lie on. If the part is changed
after surface meshing, the bar elements must also be changed in order for the bolt weld connectors to
be created. The following options are available:
Bolt hole name
A new part name for the bolt curves is automatically generated, starting with BOLT_CURVES0.
Bolt curves
specifies the curves representing the bolt hole.
Connector Part Name
specifies the part name for the connectors which is automatically generated, starting with BOLT_WELD0.
Num quad rings
is the number of quad layers to mesh around the bolt curves. This is subject to the space available
around the curves.
Washer
Washers are represented by line (bar) elements and the thickness of the washer is represented by the
quad layer(s) generated. The line elements will go from the inner and outer rings of the quad layer(s)
to the center of the bolt hole to allow the load to get transferred from the bolt to both sides of the
washer.
Note
To generate a washer at least one quad layer must be specified.
Active
if disabled, the connector will not be created when remeshing.
Seam Weld Connectors
The Seam Weld Connectors option allows you to create bar elements from all nodes that lie on
the specified curve to a specified surface. The created connectors will be normal to the surface, so the
330
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Define Connectors
surface elements may be automatically split in order to create nodes at the proper locations to connect
the bars. If nodes are aligned around the seam within a tolerance, then the elements will not be split.
Seam connector name
The part name is generated automatically, starting with SEAM_CURVES0
Weld type
• Point to point
creates a row of bar elements between the nodes of the source curves and the nearest nodes of
the target surface mesh.
• Curtain tris/quads
creates quad elements with some tri elements in between the nodes of the source curves and
the nodes of the target surface mesh. Curtain welds are generally intended to be defined on
single edges to close a gap between two parts.
Note
In many cases, extending surfaces by using Geometry > Create/Modify Surface
> Extend Surface > Close gaps Between Midsurfaced Parts is a more robust
way of ensuring the creation of shell elements to represent the connection between
parts.
• Tent
is a specialized method that creates curtain elements with additional tent elements and defines
particular meshing parameters on the source curves. The geometry is modified by surface extension
or curtain surface functions. The Tent welds extend the surfaces to intersection and then diagonal
quads represent the fillet welds.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
331
Mesh
Tent Weld type
select either T welds or Lap welds.
Diagonals
For T welds, diagonals can be added to the Positive or Negative directions, or both. For Lap
welds, diagonals can be added only to either the Positive or Negative directions.
No. layers
number of quad rows along the welds.
Tent weld spacing
– Distance to Weld Toe
The weld spacing can be determined by specifying the Distance to weld toe, the Number
of layers to toe, and the Growth ratio after weld parameters.
– Weld fillet radius
The weld spacing can also be determined by specifying the fillet radius of the weld.
Source curves
specifies the curves representing the edge of surface to be seam welded to the target surface.
Note
The source curves information may not be retained when you try to modify an existing
seam weld connector.
Target part
specifies the surface part to which the connectors will attach. The connectors will be normal to the surface.
Since new nodes are projected, the surface elements must lie on top of a surface, and they must be in
the same part as the surface.
Max projection
is a value slightly more than the distance between the source entity and the farthest target surface.
Part name
The connector part name is automatically generated, starting with SEAM_WELD0.
Element splitting
• Remesh area (Tri/Quad)
remeshes the area of the seam weld after creating the mesh and connector.
• Terminate
terminates the split to keep the mesh count down. It doesn’t give as many high aspect ratio
quads, but it creates many tri elements.
• Propagate
332
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Define Connectors
propagates the split through the mesh until the propagation is stopped by a tri element or it
exits to the ORFN region.
Note
This may result in new quad elements with poor aspect ratios.
Spot Weld Connectors
The Spot Weld Connectors option allows you to create bar elements from all nodes that lie on
the specified part to a specified surface. The created connectors will be normal to the surface, so the
surface elements may be automatically split in order to create nodes at the proper locations to connect
the bars. If the nodes are aligned within a tolerance, the surface elements will not be split.
Spot welds support 3T welds, which are 3 plates being welded together. For a 3T spot weld, pick 2
parts as Target parts.
A spot weld is intended to be used in the middle of a surface. It can also be defined on a surface
boundary, with the condition that the source points should split the curve at the surface boundary.
The following options are available for Spot Weld connectors:
Spot Weld name
The part name is automatically generated, starting with SPOT_POINTS0.
Source points
specify points which represent one end of the connectors.
Note
The source point must be embedded in the source surface and both must belong to the
same part.
Target parts
specifies the two parts that are to be connected.
Connector Part name
The part name for the connectors is automatically generated, starting with SPOT_WELD0.
Max projection
is a value is slightly greater than the maximum distance between two target parts.
Weld options
• Point to Point
creates a line element attached to the nodes of both surfaces, and normal to both surfaces.
– Element Splitting
→ Remesh area (Tri/Quad)
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
333
Mesh
remeshes the area of the spot weld after the mesh is created.
→ Terminate
terminates the split to keep the mesh count down and doesn’t give as many high aspect
ratio quads, but it creates many more tri elements
→ Propagate
propagates the split through the mesh until the propagation is stopped by a tri element or
it exits to the ORFN region.
• Mesh independent line
This is like the point weld, but the nodes on the two sides do not have to be forced into the
mesh. Instead, any nodes in the nuggets area are connected to the line element through a second
set of line elements for both sets of surface mesh. Typically, the first line element is defined as
an RBE2 element in Nastran, and the second set of line elements on each side are defined as
RBE3 elements, which have a weighting factor based on how close it sits to the node of the line
element. If the leg of the RBE3 is approximately zero, it gets a weighting value of one, and if it
is large the weighting value is approximately zero.
– RBE3 Part Name
For a mesh independent weld, there is a weld element (that does not connect to the mesh),
and connector elements that connect the weld element to the mesh. The connector elements
to into the RBE3 Part. Typically, this weld is used for Nastran, where the line elements in this
part should get an RBE3 Element Property.
• Mesh independent hexa
This is like the line independent weld, but the base line element (RBE2) is replaced by a Hexa
element with a thickness defined by the diameter. Each of the four nodes at each surface has a
RBE3 connection from its node to all nodes of the nearest element. The Hexa elements typically
get a rigid material property, and the line element connectors are weighted as in a line mesh independent weld.
– Weld Radius
defines the weld diameter. The weld diameter (Radius * 2) would be equal to the diagonal of
the Hex element for each face that is near the shells.
– RBE3 Part Name
Contains the line elements that connect the Hexa element to the mesh. These line elements
should get an RBE3 element property.
• Area weld
An hourglass type of weld, where there is a nugget area or diameter, and a node in the center
between the two surfaces meshes, where the center node is attached to any nodes within the
diameter on either side. This is mesh independent, and the weld/line elements adapt to where
the mesh is.
– Weld Radius
334
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Define Connectors
The weld connects all the nodes on the defined parts within the specified radius to the central
node.
Active
if disabled, the connector will not be created when remeshing.
Spot Weld From File
The Spot Weld from File option allows you to create bar elements from the weld data file.
Spot Weld data file
enter or browse for the path to the Weld data file. See below for sample lines of a Weld data file.
Description
No.
X
Y
Z
PID1 PID2 PID3 Diameter
MASTIC
1
3046.278 531.872 1520.413 54325 54525
5
MASTIC
2
3095.952 528.354 1526.115 54325 54525
5
MASTIC
3
3145.952 525.258 1531.003 54325 54525
5
WSPOT
44 3340.525 695.365 537.187 54325 54525
WSPOT
45 3370.485 695.982 524.562 54325 54525 54625
MASTIC
46 3456.33 520.374 1543.035 54325 54525 54625 10
MASTIC
47 3260.055 525.304 1537.365 54325 54525 54625 10
MASTIC
48 3491.99 519.932 1543.285 54325 54525
10
Note
The first column must define the connection type. The X, Y, and Z columns define the
coordinates of the connection location. The PID1, PID2, and PID3 columns define the
parts connected. The Diameter column is important for MASTIC connections. For WSPOT
connections, the Diameter column should be left blank.
Spot Weld report file
After welding, a Weld report file of this name will be generated and placed in the working directory.
This will list all the welds, which ones failed and why. Common reasons for failure include missing or
misnamed parts or badly placed welds.
Element splitting
• Remesh area (Tri/Quad)
remeshes the area of the weld after the mesh is created.
• Terminate
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
335
Mesh
terminates the split to keep the mesh count down and doesn’t give as many high aspect ratio
quads, but it creates many more tri elements.
• Propagate
propagates the split through the mesh until the propagation is stopped by a tri element or it
exits to the ORFN region.
Connector Part name
The part name for the connectors is automatically generated, starting with SPOTWELDFILE0.
Max projection
is the value slightly more than the maximum distance between two target parts.
Mesh Curve
The Mesh Curve feature extracts 1D line elements from the selected curves. If the curve mesh size
has been defined, it will be respected.
Figure 303: Mesh Curve DEZ
Compute Mesh
The Compute Mesh option allows you to generate the mesh specified by the mesher and various
parameters.
Figure 304: Compute Mesh Options
The settings in the Global Mesh Setup options will be applied unless otherwise specified.
Compute Surface Mesh
Compute Volume Mesh
Compute Prism Mesh
Compute Surface Mesh
The Compute Surface Mesh option generates a surface mesh. By default the software tries to
apply good meshing parameters for use in surface meshing, but you can apply additional controls by
336
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Compute Mesh
changing the meshing parameters. The parameters that control the surface meshing are defined under
Global Mesh Setup, Part Mesh Setup, and Surface Mesh Setup or Curve Mesh Setup
Overwrite Surface Preset/Default Mesh Type
if enabled, the specified mesh type will be used instead of the mesh type set in Global Mesh Setup >
Shell Meshing Parameters.
Overwrite Surface Preset/Default Mesh Method
if enabled, the specified mesh method will be used instead of the mesh method set in Global Mesh
Setup > Shell Meshing Parameters.
Input
specifies the geometry that will be used as input for the surface mesh.
All
meshes the entire geometry.
Visible
meshes the visible geometry.
Part by Part
meshes the selected parts one by one. This provides non-conformal mesh between part interfaces.
From Screen
allows you to select the entities to be meshed from the display.
Note
For Patch Dependent meshing, if curves that form a closed loop are selected and meshed
with one element type, and then remeshed using another element type, the original
elements will not be deleted.
Compute Volume Mesh
The Compute Volume Mesh option generates a volume mesh using the selected volume mesh
type and method. The descriptions of the different options and their parameters are described in
Global Mesh Setup > Volume Meshing Parameters. The volume mesh will be applied using the parameters
that are set there.
Load mesh after completion
This option applies to all the Compute Volume Mesh options. If disabled, the surface mesh will not be
loaded into the GUI. This may be useful for big models.
The available volume mesh types are as follows.
Tetra/Mixed Mesh Type
Hexa-Dominant Mesh Type
Cartesian Mesh Type
Tetra/Mixed Mesh Type
There are three different Mesh Methods available for Tetra/Mixed Meshing: Robust (Octree), Quick
(Delaunay), and Smooth (Advancing Front). The different options for each mesh method are:
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
337
Mesh
Robust (Octree) Mesh Method
This algorithm ensures refinement of the mesh where necessary (based on entity sizes and the curvature
and proximity based refinement settings), but maintains larger elements where possible, according to
the ICEM CFD octree algorithm and applied settings (such as tetra ratio). For additional information see
The Octree Mesh Method.
Create Prism Layers
generates prism inflation layers into the tetra volume mesh that is created, according to the prism
meshing parameters that are specified under Global Mesh Setup > Prism Meshing Parameters, Part
Mesh Setup, Surface Mesh Setup, and/or Curve Mesh Setup.
Create Hexa-Core
generates a hexa-core mesh using a bottom-up meshing approach. It will retain the tri surface or
prism mesh, delete the existing tetra mesh, and remesh the volume interior with Cartesian meshing.
The tetra elements will be mapped to the tri or prism faces with the Delaunay algorithm.
Input
specifies the geometry that will be used as input for the Volume Mesh.
All
meshes the entire geometry.
Visible
meshes the visible geometry.
Part by Part
meshes the selected parts one by one. This provides non-conformal mesh between part interfaces.
From File
runs the mesher in batch mode from an existing tetin file. Enter the name of the Tetin file or
browse the file manager.
Use Existing Mesh Parts
forces the Octree Tetra mesher to align to the surface mesh of the selected existing mesh parts
when the All or Visible option is selected for the input geometry. The Octree tetra mesh will be
generated in its normal top down (volume first) method and then be “made conformal” with the
existing surface mesh.
Quick (Delaunay) Mesh Method
uses the Delaunay Tetra mesher and a bottom-up meshing approach to generate a mesh. The surface
mesh can be an existing mesh or will be created with the parameters defined under Global Mesh Setup
> Shell Meshing Parameters or Surface Mesh Setup. The volume mesh will then be generated from this
surface mesh. The Delaunay method is robust and fast.
Note
This method works with quads or tris or a combination of both. Quads will use pyramids
to transition to the Tetras. The surface mesh can have multiple volumes and have multiple
edge elements. However, the Delaunay mesh method requires a closed surface mesh,
and cannot tolerate single edges, overlapping elements or duplicate elements. You can
run a mesh check (Edit Mesh > Check Mesh) before generating the volume mesh. Also,
sudden changes in element size, either adjacent or across a narrow volume gap, can
cause quality issues or failure.
338
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Compute Mesh
Create Prism Layers
generates prism inflation layers into the tetra volume mesh that is created, according to the prism
meshing parameters that are specified under Global Mesh Setup > Prism Meshing Parameters, Part
Mesh Setup, Surface Mesh Setup, and/or Curve Mesh Setup.
Create Hexa-Core
generates a hexa-core mesh using a bottom-up meshing approach. It will retain the tri surface or
prism mesh, delete the existing tetra mesh, and remesh the volume interior with Cartesian meshing.
The tetra elements will be mapped to the tri or prism faces with the Delaunay algorithm.
The Hexa-Core mesh parameters are specified under Global Mesh Setup > Volume Meshing
Parameters > Cartesian Mesh Type > Hexa-Core Mesh Method.
Volume Part Name
allows you to select from the list of existing volume parts, select a part from the screen, or supply a
new name. The created mesh will be assigned to this part name.
If you select inherited, the mesher will place the volume element into the same part as an existing material point. For the Delaunay method, the existing material point name will be used,
but without its specific location. This option works well for models with only one material point.
For more advanced models, such as conjugate heat transfer models or models with sections of
porous media, it is recommended that you enable the Flood fill after completion option
(available in the Quick (Delaunay) mesh method options) to use each material point with its
location to determine the volume mesh part names for each region.
Note
When the inherited option is selected, the mesher will run the flood fill operation,
even if Flood fill after completion is disabled under Volume Meshing Parameters
in the Global Mesh Setup.
Input
specifies the geometry that will be used as input for the Volume Mesh.
All Geometry
meshes the entire geometry.
Existing Mesh
allows the mesher to align to the existing mesh.
Part by Part
meshes the selected parts one by one. This provides non-conformal mesh between part interfaces.
From File
runs the mesher in batch mode from an existing tetin file. Enter the name of the Tetin file or
browse the file manager.
Smooth (Advancing Front) Mesh Method
This option will use the Advancing Front Tetra mesher to generate a mesh using a bottom-up meshing
approach. The surface mesh will be created with the parameters defined under Global Mesh Setup >
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
339
Mesh
Shell Meshing Parameters or Surface Mesh Setup. The volume mesh will then be generated from this
surface mesh.
Note
The surface mesh should be one enclosed volume with no single edges, multiple edges,
non-manifold vertices, overlapping elements or duplicate elements. Sudden changes in
element size, either adjacent to one another or across a narrow volume gap, can cause
quality issues or even failure.
The surface mesh must be either tri or quad elements for the Advancing Front mesh
method.
The primary advantage of the Advancing Front Method is the ability to generate a smoothly transitioning Tetra mesh, with a volume growth ratio controlled by the Expansion Factor under the
Global Mesh Parameters.
Create Prism Layers
generates prism inflation layers into the tetra volume mesh that is created, according to the prism
meshing parameters that are specified under Global Mesh Setup > Prism Meshing Parameters, Part
Mesh Setup, Surface Mesh Setup, and/or Curve Mesh Setup.
Volume Part Name
allows you to select from the list of existing volume parts, select a part from the screen, or supply a
new name. The created mesh will be assigned to this part name.
If you select inherited, the mesher will place the volume element into the same part as an existing material point. For this method, the existing material point name will be used, but without
its specific location. This option works well for models with only one material point. For more
advanced models, such as conjugate heat transfer models or models with sections of porous
media, it is recommended that you enable the Flood fill after completion option (available in
the Smooth (Advancing Front) mesh method options) to use each material point with its location
to determine the volume mesh part names for each region.
Input
specifies the geometry that will be used as input for the Volume Mesh.
All Geometry
meshes the entire geometry.
Existing Mesh
allows the mesher to align to the existing mesh.
Part by Part
meshes the selected parts one by one. This provides non-conformal mesh between part interfaces.
From File
runs the mesher in batch mode from an existing tetin file. Enter the name of the Tetin file or
browse the file manager.
340
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Compute Mesh
Hexa-Dominant Mesh Type
This option will generate a Hexa-Dominant mesh using a bottom-up meshing approach. The HexaDominant mesher starts with surface quad dominant mesh and uses an Advancing Front scheme to fill
as much of the volume as possible. For simple volumes, it can fill it completely. For more complicated
volumes, it usually fills several layers in from the surface with hexa elements and then fills the middle
with tetras and pyramids. Then a diagnostic is run, and if those central elements are poor, the inner
volume will be meshed again with the Delaunay mesher. The surface mesh will be created with the
parameters defined under Global Mesh Setup > Shell Meshing Parameters or Surface Mesh Setup. The
volume mesh will then be generated from this surface mesh or the specified input.
Input
allows you to select from the following types of input to generate the mesh.
All Geometry
meshes the entire geometry.
Existing Mesh
allows the mesher to align to the existing mesh parts.
Volume Part Name
allows you to select from the list of existing volume parts, select a part from the screen, or supply a new
name. The created mesh will be assigned to this part name.
Cartesian Mesh Type
This option will generate a Cartesian mesh using a top-down meshing approach. The mesher works by
continuously refining the initial grid in a binary fashion in each dimension, and eliminating the nonvolume cells, up to the specified maximum refinement. The Cartesian mesher does not require an existing
surface mesh and will ignore meshing parameters defined to control local surfaces. The mesh will be
refined until the finest cell size does not exceed the Max element size specified in Global Mesh Setup
or the Surface Mesh setup.
Body-Fitted Mesh Method
Body-Fitted Mesh Method
This option creates unstructured hexa mesh based on Cartesian mesh and fits it to the geometry. This
works for both CAD and STL geometries. The mesher can handle “dirty” geometries as long as the Max
element size is larger than the gap size.
Note
The max element size should be smaller than the thickness of the model.
Figure 305: Handling of Gaps in the Geometry (p. 342) shows an example where the gap in the geometry
is ignored by the body-fitted mesh method.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
341
Mesh
Figure 305: Handling of Gaps in the Geometry
Volume Part Name
allows you to select from the list of existing volume parts, select a part from the screen, or supply a new
name. The inherited option will use the material points in the geometry to determine the part name for
each region. The created mesh will be assigned to this part name.
Enforce Split
These options allow you to use a pre-existing Cartesian mesh as the basis for the body-fitted Cartesian
algorithm. This Cartesian mesh can be created elsewhere or can be created from ANSYS ICEM CFD Hexa
Blocking. It can include biasing and various aspect ratios. It can also be aligned with various features of
the geometry.
None
does not enforce a pre-existing Cartesian mesh, but rather creates a Cartesian mesh within the BFCart
algorithm. This background mesh may have a given aspect ratio and may be aligned with the LCS.
These options are controlled by the Global Mesh Parameters for BFCart.
Figure 306: BFCart Mesh Generated Using the None Option (p. 343) shows an example where
this option has been used.
342
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Compute Mesh
Figure 306: BFCart Mesh Generated Using the None Option
Initial
In order to body fit, the BFCart algorithm must take the inverse of the Cartesian mesh. The end result
of the process is that the nodes of the original Cartesian mesh become the centers of the resulting
mesh. The split lines of the original mesh end up between the split lines of the final mesh.
Figure 307: BFCart Mesh Generated Using the Initial Option (p. 343) shows an example where
this option has been used.
Figure 307: BFCart Mesh Generated Using the Initial Option
Final
With the Final option, the supplied Cartesian mesh is inverted before the rest of the process begins
so that the later body fitting inversion changes it back and the final grid can line up with the original.
Due to internal complexities, this only works if the “uniform” Cartesian mesh is used. It does not
work for 2 to 1 hanging node Cartesian mesh.
Figure 308: BFCart Mesh Generated Using the Final Option (p. 344) shows an example where this
option has been used.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
343
Mesh
Figure 308: BFCart Mesh Generated Using the Final Option
Cartesian file
specifies the Cartesian grid file to be used when starting from an existing Cartesian grid file rather
than generating one based on the mesh parameters of the current model. When used in conjunction with the File > Blocking > Write Cartesian Grid option to export a block file as a Cartesian
grid, you will be able to use block splits and edge parameters to control Cartesian bunching,
distribution and aspect ratio. The imported mesh is used as the starting point before body fitting
takes place.
Key-Points
The Key-Points option can be used to align the body-fitted Cartesian mesh with corner points. Behind
the scenes, this uses Key-Point blocking to create a Cartesian file aligned with the points and then
uses the Final option with that file to align the Cartesian splits with the points. This option is useful
for models having features aligned in Cartesian directions. An example of a circuit board is shown
in Figure 309: BFCart Mesh Generated Using Key-Points (p. 344) with several features aligned in the
Cartesian directions.
Figure 309: BFCart Mesh Generated Using Key-Points
344
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Compute Mesh
Tolerance
specifies the minimum distance between adjacent grid lines. The default value is 0.0. If the default
value is used, the tolerance will be computed internally based on the minimum entity dimension.
Inflation
contains options for growing the body fitting inflation layer.
Defined
grows the inflation layer on the parts for which the prism option is enabled in the Part Mesh Setup
dialog. The setting works as an on/off toggle. The other Part Mesh Setup options for prisms, including
initial “height”, “ratio” and number of layers (“width”), are not yet used for BFCart inflation.
All
grows the inflation layer on all parts.
None
does not grow the inflation layer regardless of the settings in the Part Mesh Setup dialog.
Figure 310: Selective Inflation for the Body-Fitted Cartesian Mesh (p. 345) shows the inflation options
available for the Body-Fitted Cartesian mesh generated for a sphere with a gap.
Figure 310: Selective Inflation for the Body-Fitted Cartesian Mesh
(A) Inflate Parts set to None — The mesh quality is poor as the stair step mesh is projected to the
round surfaces of the sphere.
(B) Inflate Parts set to All — All parts are inflated, including the flat surface in the gap. The mesh
quality is not as good as it could be due to miter elements generated in some corners.
(C) Inflate Parts set to Defined — Only the sphere surfaces are inflated, while the gap surface part
is not inflated. The inflation from the curved walls runs into the gap and gives the best resulting
quality. On the left of the gap, the inflated hexas are split propagated to give better boundary resolution.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
345
Mesh
Compute Prism Mesh
Generates prism inflation layers into the volume mesh to resolve boundary layer effects efficiently.
Existing tetra mesh is restructured to maintain proper connectivity and quality. The prism layers are
typically orthonormal to the viscous wall boundaries. The prism meshing parameters can be specified
under Global Mesh Setup > Prism Meshing Parameters, Part Mesh Setup, Surface Mesh Setup, and/or
Curve Mesh Setup.
Input
allows you to select the mesh in which the prism inflation layers will be generated.
• Existing Mesh
creates prism mesh in the existing mesh.
• From File
runs the Prism Mesher in batch mode from an existing mesh (*.uns) file. Enter the name of the
file or browse the file manager.
Select Parts for Prism Layers
allows you to define the parameters of prism layers for different parts.
Figure 311: Select Parts for Prism Layer
346
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Compute Mesh
Select the parts that prism layers will be applied to. For each part, the Height, Height Ratio and the
Num Layers can be specified. Volume, Surface and/or Curve parts can be selected. When using the
Prism mesher in ANSYS ICEM CFD, the default prism parameters are set under Mesh > Global Mesh
Setup > Global Prism Settings. However, parameters that are entered here at the Part level will
override the Global settings. In addition, the entity settings of Height, Height Ratio, and Number of
Layers will override the Part level settings. Entering zero for any of the settings will default back to
the Global Settings.
If there are multiple volume materials, and none have the prism option enabled, then prism mesh
will grow from the selected surface parts into the adjacent volumes. If only certain volume parts
have prism enabled, then prism mesh will be grown only into those volume parts. After you enter
the parameters, click Apply, and then Dismiss to close the window.
For 3D, the prisms are grown (inflated) from the shell (tri or quad) elements of each part. This can
be done with or without a volume mesh, but having a tetra volume mesh during inflation helps
with collision avoidance and ensures that you will have a volume mesh after prism generation is
complete. For 2D, the prisms are grown (inflated) from the curve parts into the selected surface
parts (must be selected). The 2D prism only works if Advanced Prism Meshing Parameters > Blayer
2D is enabled.
Note
• You can compute a prism mesh without an input surface model loaded. Prism will generate
a temporary faceted surface model from the input mesh.
• Different prism heights can be specified on adjacent parts, though a transition region with
unspecified height is required in between these parts.
• If a surface part separates two or more volume parts, select the volume parts on the side
of the surface you want to grow the prisms. If you select both sides, prisms will grow in
both directions from the surface part. If you want different prism properties on either side
of a surface grown into 2 volumes, do one at a time (run prism iteratively).
• If adjacent tri-element parts have heights that differ by more than a factor of 2, the prism
mesher may fail (this limit is controlled in the Advanced Prism Meshing Parameters). Not
setting a height for Prism, (here or in the Global Prism Parameters DEZ) will allow the
height to float. You can also allow the height to float globally and set specific initial heights
per part or on an entity by entity basis.
Load mesh after completion
if disabled, the mesh file will not be loaded into the GUI. This may be useful for big models.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
347
348
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Blocking
Figure 312: Blocking Menu
The Blocking tab contains the following options to create blocking over any geometry.
Create Block
Split Block
Merge Vertices
Edit Block
Associate
Move Vertex
Transform Blocks
Edit Edge
Pre-Mesh Params
Pre-Mesh Quality
Pre-Mesh Smooth
Block Checks
Delete Block
Create Block
The Create Block option establishes new blocking.
Figure 313: Create Block Options
The following options are available for creating blocks:
Initialize Block
From Vertices/Faces
Extrude Face
2D to 3D Blocks
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
349
Blocking
3D to 2D
Note
If a blocking file is not loaded, then only the first option, Initialize Blocks, will be active. If
a blocking file is already loaded, then all the options will be active.
Inherit Part Name
when enabled, the created blocks will inherit their part name from the entities they were created from.
When initializing 2D surface blocking, the part name can be inherited from underlying surface parts. For
other blocking operations, such as Extrude Face or 2D to 3D), which start from an existing blocking, the
part name of the new blocks is inherited from the blocks they were created from. If this option is disabled,
all blocks will be in the part name specified in the drop-down list at the top of the Create Block DEZ.
Note
Mesh created within each block will belong to the same part as its block. This part name
is also used to tag the elements on export and is useful for assigning material (or zone)
properties in the solver.
Initialize Block
The Initialize Block option allows you to initialize blocks with the following options:
3D Bounding Box
allows you to create a 3D block enclosing the selected entities. If no entities are selected, the block will
encompass the entire geometry.
ANSYS ICEM CFD Hexa blocking is typically done in a top down method that starts from a single
large block which is subdivided down to create the topology. Initializing this 3D bounding box is
the first step.
350
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Block
Note
Not selecting any entities is more efficient, particularly for scripting, if you intend to block
the geometry extents.
Project vertices
when enabled, the initial block vertices will be moved to the nearest locations on the geometry.
Orient with geometry
attempts to find the best fit of the geometry in any orientation, and to create the smallest block
possible around the geometry selected.
2D Blocking
enables the creation of a surface blocking composed of six 2D face blocks forming a box around the
geometry.
Initialize with settings
allows you to use the user-defined settings set in the Hexa/Mixed Meshing Options DEZ (Settings
> Meshing Options > Hexa/Mixed) and saved under .aienv_options for block initialization. For
example, you can set the default bunching ratio to 1.2 and the multigrid level to 3 and save the
settings. Future block initialization with the Initialize with settings option enabled will use these
settings as default.
This option is enabled by default.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
351
Blocking
2D Surface Blocking
allows you to create automatic surface blocking for surface-only mesh. It creates a 2D block for each
surface. When Inherit Part Name is enabled, the part name will be inherited from the underlying surface
parts.
Note
This can be a precursor for the 2D to 3D Fill, i.e., Multi-zone method.
Note
If surface mesh sizes (max size, height, and height ratio) have been previously set, they
will be used to calculate the distributions for the blocking edges.
Note
Geometry topology information is required to establish connectivity between the blocks.
You can check topology by right-clicking on Curves in the model tree and enabling the
Color by Count option. Make sure that you have double edges (red curves) between
surfaces that you want connected. Single edges (yellow curves) may indicate a gap
between surfaces. Build diagnostic topology if necessary.
2D blocking can be created with the following options:
352
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Block
Surfaces
allows you to select specific surfaces for initializing 2D surface blocking. If none are selected, all
surfaces will be initialized.
Surface Blocking
contains options for the surface blocking method, free face mesh type, and free face mesh method.
Method
specifies the surface blocking method. The following options are available:
Note
Blocks can be converted between free and mapped blocks using Edit Block >
Convert Block Type.
Free
creates all free (unstructured) 2D blocks. Unstructured blocks can have any number of sides,
and have a different number of nodes on opposite sides, with a resulting nonuniform element
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
353
Blocking
pattern. The mesh inside free blocks is paved (recursive loop algorithm) and can be all quad,
quad dominant, quad with one tri, or all tri.
Note
The default mesh type that will be used is defined under Settings > Meshing
> Hexa/Mixed > Unstruct face mesh type. You can override the default
setting by changing the mesh type in the Free Mesh Type list. After the 2D
Surface Blocking is generated, you can modify the mesh type for any particular
Free block using the Blocking > Edit Block > Convert Block Type option.
Some mapped
maps surface patches with 4 corners (possibly more sides). A mapped surface has matching
numbers of nodes on opposite sides. The mesh is “mapped” across to the opposite side of
the block and is always quad surfaced mesh. Remaining surfaces with more or less than 4
corners are blocked with “free” blocks as above.
Mostly mapped
tries to subdivide surface patches with more or less than 4 corners into mappable patches.
For instance, a 3 cornered surface is divided into a quarter O-Grid (Y-Block) pattern. A half
circle is divided into a half O-Grid (C-Block) pattern, other arbitrary shapes are simply divided.
Other surface patches with 4 corners are also mapped. Any remaining patches or sections
of patches which still cannot be mapped (more or less than 4 corners) are blocked with “free”
blocks as above.
Figure 314: Surface Blocking Methods (p. 354) shows the Free, Some mapped, and Mostly
mapped surface blocking methods.
Figure 314: Surface Blocking Methods
Swept
creates surface blocks in preparation for the 2D to 3D Fill > Swept operation. Sides of
sweepable bodies are mapped, sources are free or mapped and copied to the targets. This
method can handle multiple sources and targets.
354
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Block
Swept Surfaces
This option is available only for the Swept Method. Select all the source and target surfaces
(multiple sources and targets are supported). If it is easier, select all surfaces involved
(sources, targets, sides). If you intend to sweep everything, do not select surfaces at all
and everything will be selected.
Figure 315: Surface Blocking-Swept (p. 355) shows the swept surface blocking. In this
case, geometry topology was built between the two parts so that the sweep could pass
through both parts.
Figure 315: Surface Blocking-Swept
Note
The 2D Surface blocking is automatically imprinted to deal with multiple
source and target situations.
Note
As with all the 2D surface blocking methods, geometry connectivity translates
into blocking connectivity, so make sure to check topology.
Free Face Mesh Type
specifies the type of mesh for the free blocks. The following options are available:
• All Tri
• All Quad
• Quad Dominant
• Quad w/one Tri
Free Face Mesh Method
specifies the process for meshing free faces. The following options are available:
• ICEM CFD Quad - method is based on a recursive loop-splitting algorithm.
• Gambit Pave - method is based on the Gambit paving advancing front algorithm.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
355
Blocking
• Auto - method lets the program determine the method based on size and curvature.
Merge blocks across curves
By default, surface patches are defined by each surface. However, surfaces can be combined to improve
the blocking or prevent slivers. This is controlled or limited by dormant curves or the Ignore size
tolerance.
Behind the scenes, a “loop” is formed around the perimeter of each surface. If two blocks are
merged across a curve, the loops on either side are simply replaced by a loop that includes the
perimeters of the 2 surfaces combined. The geometry (curves and surfaces) is unaffected by the
operation.
Method
All
will merge a sliver surface with its larger neighbor if the characteristic edge length is less
than the tolerance.
Respect non-dormant
will not merge if the curve between the surfaces is not dormant. This does not mean it will
force a merge if the curve is dormant. Tolerance still determines the merge.
None
will not merge based on tolerance.
Merge dormant
will merge across dormant curves regardless of tolerance.
Note
To make a curve dormant, delete without the Delete Permanently option.
The Build Topology > Filter curves option will also make curves dormant
based on a feature angle. To restore a dormant curve, use the Geometry >
Restore dormant entities option. To view dormant curves, right-click on
Curves in the model tree and enable Show Dormant.
Note
After creating the 2D blocking, the Edit Block > Merge Blocks option can be
used to achieve a similar result.
Ignore size
specifies the tolerance that Merge blocks across curves uses to determine whether to merge
sliver blocks to the adjacent block. The sliver block's distance across the thin edge must be
smaller than this value for the block to be merged to the adjacent block.
Initialize with settings
allows you to use the user-defined settings set in the Hexa/Mixed Meshing Options DEZ (Settings
> Meshing Options > Hexa/Mixed) and saved under .aienv_options for block initialization. For
details, refer to Initialize with settings (p. 351) described above.
356
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Block
2D Planar
allows you to create a 2D Planar block in the XY plane fitting around the entire geometry. 2D planar
blocking is intended to work in the XY plane, and moving it to another orientation will make it difficult
to position internal vertices. It is better to rotate your geometry to the XY plane where Z=0.
Initialize with settings
allows you to use the user-defined settings set in the Hexa/Mixed Meshing Options DEZ (Settings
> Meshing Options > Hexa/Mixed) and saved under .aienv_options for block initialization. For
details, refer to Initialize with settings (p. 351) described above.
From Vertices/Faces
The From Vertices/Faces option allows you to create blocks from vertices or faces in either 2D
or 3D. The available options are described in the following sections:
3D Blocks
2D Blocks
3D Blocks
The following 3D block types can be created:
Hexa
allows you to create 3D Hexa blocks by specifying the corner vertices or appropriate faces of adjacent
blocks.
Corner Method
Select eight vertices (or locations) as shown in Figure 316: Selection of Vertices/Locations for the
Corner Method (p. 358) to create 3D Hexa blocks.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
357
Blocking
Figure 316: Selection of Vertices/Locations for the Corner Method
While selecting a combination of vertices and locations:
1. First select the vertices to be used, ensuring that the order of selection is appropriate.
2. Click the middle-mouse button to confirm the selection of the vertices.
3. Select the remaining locations on the geometry (not necessarily points) to complete the
selection of 8 vertices/locations.
Faces Method
Select faces of adjacent blocks as shown in Figure 317: Selection of Faces for the Faces Method (p. 358)
to create a new 3D Hexa block.
Figure 317: Selection of Faces for the Faces Method
358
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Block
Figure 318: 3D Block Created
Quarter O-Grid
allows you to create the advanced topology known as a Y-Block or Quarter O-Grid. This topology is used
to fit three Hexa Blocks into a wedge. Select six vertices/locations as shown in Figure 319: Selection of
Vertices/Locations for Quarter O-Grid (p. 359) to create the Quarter O-Grid. The three vertices of one side
of the wedge must be selected first, in clockwise or counter clockwise order. Then the remaining three
vertices can be selected. It is important that the 4th vertex selected should be connected to the 1st, 5th
to the 2nd and 6th to the 3rd respectively.
Figure 319: Selection of Vertices/Locations for Quarter O-Grid
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
359
Blocking
Figure 320: Quarter O-Grid Created
While selecting a combination of vertices and locations:
1. First select the vertices to be used, ensuring that the order of selection is appropriate.
2. Click the middle-mouse button to confirm the selection of the vertices.
3. Select the remaining locations on the geometry (not necessarily points) to complete the selection
of 6 vertices/locations.
Degenerate
allows you to create a degenerate block which is a prismatic block with 5 sides. Previously, these could
only be created by collapsing one side of a hexa block to create a wedge. The bottom up creation follows
the exact same method as the Quarter O-Grid (Y-Block) creation. However, only one block is created and
there will be a row of prism elements along one edge. Many solvers can not handle this type of blocking,
so be sure to consult your solver manual before using degenerate blocks.
Select six vertices/locations as shown in Figure 321: Selection of Vertices/Locations for Degenerate
Block (p. 360) to create the Degenerate block. The 4th vertex selected should correlate to the 1st,
the 5th to the 2nd, and the 6th to the 3rd.
Figure 321: Selection of Vertices/Locations for Degenerate Block
360
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Block
Figure 322: Degenerate Block Created
While selecting a combination of vertices and locations:
1. First select the vertices to be used, ensuring that the order of selection is appropriate.
2. Click the middle-mouse button to confirm the selection of the vertices.
3. Select the remaining locations on the geometry (not necessarily points) to complete the selection
of 6 vertices/locations.
Swept
allows you to create a swept block. Select a face of a block. All the blocks in the direction perpendicular
to this face will be made into swept blocks. A swept (free) block results in an unstructured mesh with
some tri and prism elements.
Note
This operation converts mapped blocks to swept blocks. If there is a swept or free block
included in the blocks that are to be converted, there may be an error.
Sheet
allows you to create a structured sheet block from 4 vertices. The vertices should be selected in the order
of a Z pattern (shown in Figure 323: Selecting Vertices/Locations for a Sheet Block (p. 361)). Click the
middle mouse button to confirm the selection of the vertices.
Figure 323: Selecting Vertices/Locations for a Sheet Block
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
361
Blocking
Free-Sheet
allows you to create a free sheet block from 4 vertices.
2D Blocks
Note
The 2D Blocks option allows you to create a block for a 2D blocking only. To create a 2D
(sheet) block with a 3D blocking, even if the only 3D block is unstructured, you need to use
the Sheet (p. 361) option described in the 3D Blocks (p. 357) section.
The following 2D block types can be created from vertices:
Mapped
allows you to create 2D blocks from any four specified vertices or locations.
In Figure 324: Selection of Vertices for 2D Mapped Block (p. 362), four vertices are selected to create
a mapped block.
Figure 324: Selection of Vertices for 2D Mapped Block
Figure 325: Mapped Block Created
While selecting a combination of vertices and locations:
1. First select the vertices to be used, ensuring that the order of selection is appropriate.
2. Click the middle-mouse button to confirm the selection of the vertices.
3. Select the remaining locations on the geometry (not necessarily points) to complete the selection
of 4 vertices/locations.
362
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Block
In Figure 326: Selection of Vertices and Locations for 2D Mapped Block (p. 363), a mapped block is
created from two vertices and two locations.
Figure 326: Selection of Vertices and Locations for 2D Mapped Block
Figure 327: Mapped Block Created
Free
allows you to create a free block using the selected vertices.
Extrude Face
The Extrude Face option is available only for 3D blocking. The following methods can be used to
extrude block faces.
Interactive
Fixed Distance
Extrude Along Curve
Interactive
Select the face(s) to be extruded with the left mouse button and then press the middle mouse button
and drag to interactively extrude the face(s). When Inherit Part Name is enabled, the new extruded
block inherits the part of the adjacent volume block (is in the same blocking material).
Fixed Distance
Select the face to be extruded and specify the distance for normal extrusion. When Inherit Part Name
is enabled, the new extruded block inherits the part of the adjacent volume block (is in the same
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
363
Blocking
blocking material). The face selection and extrusion of the block is shown in Figure 328: Face Selected
for Extrusion by Fixed Distance (p. 364) and Figure 329: Extrusion Completed (p. 364).
Figure 328: Face Selected for Extrusion by Fixed Distance
Figure 329: Extrusion Completed
Extrude Along Curve
Select the face to be extruded, the curve along which the extrusion is to occur, and the end point of
the curve. When Inherit Part Name is enabled, the new extruded block inherits the part of the adjacent
volume block (is in the same blocking material). The face selection and extrusion of the block is shown
in Figure 330: Face and Curve Selected for Extrusion Along Curve (p. 364) and Figure 331: Extrusion
Completed (p. 365).
Figure 330: Face and Curve Selected for Extrusion Along Curve
364
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Block
Figure 331: Extrusion Completed
2D to 3D Blocks
The 2D to 3D option allows you to convert 2D or surface blocking to 3D. The following options
are available:
MultiZone Fill
The MultiZone Fill option converts surface blocking into 3D blocking. This requires a closed volume(s)
of structured and/or unstructured surface blocks. It can produce a structured blocking if all the surface
blocks are structured 4 sided blocks, otherwise unstructured or swept blocks may result.
Figure 332: 2D Blocking – Before Fill
Figure 333: After Fill – 3D Blocking
The following options are available for the MultiZone Fill Method.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
365
Blocking
Create Ogrid around faces
allows you to add O-grid layers on the selected parts.
Note
When using this method for blocking a model with a floating internal volume, this
method has difficulty connecting the internal and external volumes and the internal
volume may merely be superimposed within the outer volume. Splitting the model
with a connecting plane will allow a topological connection and solve this problem.
Surface Parts
allows the selected parts to be marked for O-grid layer creation. These parts can be default selected
by setting prism parameters in the Part Mesh Setup parameters menu. The other prism settings
such as initial height, ratio and number of layers can also be set. You can then either accept the
default selection here or add/remove parts as desired. The number of layers will be constant
throughout a boundary layer, but varying the initial height will affect the total height above those
surfaces.
Offset distance
specifies the height of the O-grid boundary layer calculated from the Part Mesh Setup parameters
for height, ratio, and number of layers set for individual parts. If the Part Mesh Setup parameters
are not set, the offset distance will be calculated from the Global Prism Parameters. The value displayed is the average height calculated, however, the O-grid boundary layer will be created based
on the offset calculated for each individual part. For example, in Figure 334: Variable O-grid
Height (p. 367), the initial height on the highlighted surface was set to half the height of the other
surfaces.
366
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Block
Figure 334: Variable O-grid Height
If you override this calculated height, it will apply to the entire O-grid. It will prioritize the initial
height and ratio and adjust the number of layers to fit the user-specified total height.
Note
The number of layers must be constant for the entire O-grid layer, if you set varying
numbers of layers, the greatest will be used.
Note
The variable O-grid height affects the initial O-grid generation to make the process
more automatic but Multi-zone builds an editable blocking with flexible vertices. So,
any edge length, including O-grid heights, can easily be changed interactively.
Fill Type
Simple
creates a simple free block or volume region. This saves time on complex models by not attempting to decompose the volume into mapped or swept blocks. This is recommended for external
aerodynamics applications.
Swept
uses algorithms which resolve swept configurations better.
Advanced
uses algorithms which can decompose the volume into a combination of mapped, swept and
unstructured blocks. It automatically imprints free faces to aid with sweeping, etc. This will give
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
367
Blocking
a result similar to the Multi-zone Method found in ANSYS Meshing. Some work decomposing
the geometry or surface blocking beforehand can improve the results.
Note
Behind the scenes several possible algorithms are run to create the 3D blocking.
One such algorithm is similar to converting each surface block into one element,
with Mapped blocks converted into quads; then in an operation similar to the
Hex dominant mesher, the volume is filled with hexa elements. If this is successful,
then these are converted back into 3D blocking to replace the original 2D surface
blocking. Other algorithms use the mapped side mesh to guide the sweeping of
unstructured faces into swept blocks (similar to the Cooper tool). Any remaining
volumes are simply declared as unstructured blocks and can be filled with one
of the bottom up options, including Tetra, Hexa Core or Hexa Dominant mesh.
Translate
allows you to specify the X, Y and Z distance to extrude the 2D Block. When Inherit Part Name is enabled,
the 3D block inherits the blocking material (part) of the original 2D block.
Unstructured 2D blocks will be converted to Swept blocks on translation.
Rotate
allows you to extrude a 2D Block by rotation. When Inherit Part Name is enabled, the 3D block inherits
the blocking material (part) of the original 2D block.
Unstructured 2D blocks will be converted to Swept blocks on rotation. Degenerate (axis-collapsed)
swept blocks can also be handled. The degenerate 7–node hexa elements on the axis can be converted to regular elements using the Write 7–node-hexas as pyramids option in the Hexa/Mixed
Meshing Options DEZ (see Hexa Meshing (p. 90)).
368
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Block
Figure 335: 2D to 3D Rotate for a 2D Unstructured Block (p. 369) shows an example of a 2D unstructured block extruded using the 2D to 3D rotate option using an Angle of 30 degrees, Number of
copies set to 1, and Points per copy set to 7 as shown in the DEZ above.
Figure 335: 2D to 3D Rotate for a 2D Unstructured Block
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
369
Blocking
Center of Rotation
specifies the center of rotation. The Origin option allows you to rotate the block in the specified
axis direction about the origin (0,0,0). The User option allows you to rotate the block about a specified
point.
Axis of Rotation
specifies the axis or vector about which to rotate the block.
Angle
specifies the angle of rotation for each block copy.
Number of copies
specifies the number of copies of blocks.
Points per copy
specifies the number of nodes on the extruded edges.
Set Periodic Nodes
defines periodicity at both the geometry and blocking level, and will override any existing periodicity
information set under Global Mesh Setup > Set Up Periodicity.
Collapse Axis Nodes
allows you to collapse all the nodes lying on the axis of rotation.
370
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Split Block
Extrude points, Extrude curves
when enabled, the original 2D geometry gets converted to 3D as well. Points are extruded to 3D
curves and curves are extruded to 3D surfaces.
Note
The node to point association must be defined before extrusion in order for points
to be extruded to produce 3D curves. Similarly, the edge to curve association must
be defined for the curves to be extruded to 3D surfaces.
3D to 2D
The 3D to 2D option converts 3D Blocking into 2D Blocking, as shown in Figure 336: 3D Blocking (p. 371) and Figure 337: 2D Blocking (p. 371).
Figure 336: 3D Blocking
Figure 337: 2D Blocking
Split Block
The Split Block option allows you to make multiple blocks from a single block.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
371
Blocking
The following options are available for splitting blocks:
Split Block
Ogrid Block
Extend Split
Split Face
Split Vertices
Split Free Face
Imprint Free Face
Split Free Block
Split Block
The Split Block option splits the blocking at the selected edge.
Figure 338: Split Block Options
Visible
splits only blocks that are visible, where visibility is managed by blanking blocks in the graphical window
or by using the index control.
Selected
splits only the selected blocks.
372
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Split Block
Copy distribution from nearest parallel edge
copies the edge distribution (initial heights, ratios and bunching law) from the nearest parallel index to
the new edges created by the split operation. This is useful when adding splits to a blocking after already
setting up advanced distributions on existing edges. With this option disabled, the default edge distribution (Settings > Meshing Options > Hexa/Mixed) is used. Parallel node counts are always used when
splitting a block.
Project vertices
enables the automatic projection of the new vertices to the underlying geometry.
Split Method
Screen select
allows you to select the position manually where the block is to be split.
Prescribed point
allows you to split the edges through the selected point.
Relative
allows you to split the edge with the given parameter.
Absolute
allows you to split the edge in proportion to the maximum grid length in the edge direction. Edge
direction corresponds to minimum vertices number to maximum vertex number.
Curve parameter
allows you to split the edge through a selected point on a curve. Select the edge to be split first,
and then the curve at the point through which the split will be placed.
Note
The Split Block option will only propagate splits through mapped faces, and will terminate at free faces. For 2D blocking, all mapped blocks attached edge to edge will be split,
but the split will terminate at any free block. For 3D blocking, a split will propagate
through mapped blocks and swept blocks, if the split is along the sweeping direction.
A split in 3D blocking will terminate at free 3D blocks and swept blocks, if the split is
in any direction other than the sweeping direction.
Ogrid Block
The Ogrid Block option allows you to modify a single block or blocks to a 5 sub-block topology
(7 sub-blocks in 3D) as shown below. It arranges grid lines into an “O” shape to reduce skew where a
block corner lies on a continuous curve or surface. There are several variations of the basic O-grid
generation technique.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
373
Blocking
Figure 339: O-grid Demonstration
The O-grid can be created with or without face selection as shown in Figure 340: O-grid Creation With
and Without Face Selection (p. 374).
Figure 340: O-grid Creation With and Without Face Selection
a) Circular Cylinder
b) Block Inside Cylinder
c) O-grid created without face selection
374
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Split Block
d) O-grid created with face selection
O-grids can be created or removed by selecting or deselecting Blocks, Faces, Edges, and Vertices.
Figure 341: Ogrid Creation Options
The following options are also available:
Clear Selected
clears the previously selected entities.
Around block(s)
enables the creation of the O-grid around the block(s).
Offset
specifies the height of the O-grid layer.
Absolute
when enabled, the value assigned for Offset is the actual length of the radial edge of an O-grid. Assigning
a Offset of 7 would make all the radial edges of the O-grid 7 units in length.
When Absolute is disabled, Offset behaves like a relative distance: A value of 1 causes the Hexa
Mesher to place the O-grid at a location where the resulting blocks will be distorted the least. A
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
375
Blocking
higher value makes the inner blocks of the O-grid smaller, with the surrounding blocks larger, and
a smaller value makes the inner blocks larger and the surrounding blocks smaller.
Extend Split
The Extend Split option allows you to extend block splits to a selected edge or to all edges. You
can select specific blocks or all visible blocks to extend the split.
Figure 342: Extend Split Options
Edge Select
Selected Edge
when selected, allows you to select an edge to extend the split (see Figure 343: Edge Selected to
Extend Split (p. 376) and Figure 344: Block Split Extended to One Edge (p. 377)).
Figure 343: Edge Selected to Extend Split
376
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Split Block
Figure 344: Block Split Extended to One Edge
Block Select
contains options for selecting blocks when the Selected Edge option is selected.
Visible
when selected, the split will be extended through all visible blocks.
Selected
when selected, allows you to select specific blocks through which the split will be extended.
All Edges
when selected, the block split will extend to all the edges (see Figure 345: Block Split Extended to
All Edges (p. 377)).
Figure 345: Block Split Extended to All Edges
Project vertices
enables the automatic projection of the new vertices to the underlying geometry.
Split Face
The Split Face option allows you to split a face at a desired location. Select the edge where the
split will take place and hold down the left mouse button to slide the cursor on that edge to the desired
split location. Release the left mouse button and press the middle mouse button to accept the location
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
377
Blocking
and to complete the face split operation. See Figure 346: Face Selected for Face Split (p. 378) and Figure 347: Face Split (p. 378).
Figure 346: Face Selected for Face Split
Figure 347: Face Split
You can select multiple faces to split by utilizing the corner vertices tool from the selection toolbar.
Split Vertices
The Split Vertices option allows you to split a degenerate vertex. This is equivalent to uncollapsing
an edge.
The block and vertex shown in Figure 348: Vertex Selected to Split (p. 379) is the result of collapsing a
single block. Select the appropriate vertex to split, and click Apply to split the vertex as shown in Figure 349: Split Vertex (p. 379)
378
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Split Block
Figure 348: Vertex Selected to Split
Figure 349: Split Vertex
Split Free Face
The Split Free Face option allows you to split the free face of a block, which splits the block into
two free blocks.
Imprint Free Face
The Imprint Free Face option allows you to imprint edges from one face onto an unstructured
2D surface block (face).
Note
This task is automatically accomplished to sweep blocks when the Create Block > 2D to 3D
> Fill > Advanced option is used; but it may sometimes be advantageous to do it manually
before using the 2D to 3D fill or to imprint edges for other reasons, such as node for node
matching between free faces for connection, or periodicity.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
379
Blocking
Free Block
specifies the selected target block. Usually this is an unstructured 2D face across from the edges you
want to imprint.
Loop Vertices
specifies the vertices that form the loop of edges you want to imprint on the free block.
An example demonstrating the use of the Imprint Free Face option is shown in Figure 350: Use of the
Imprint Free Face Option (p. 380).
Figure 350: Use of the Imprint Free Face Option
(A) The 2D surface blocking for the geometry
The central block cannot be swept because it has different features on either side.
(B) The 2D surface blocking with the faces imprinted on either side of the central
block
(C) The imprinted face meshed
380
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Split Block
The imprinted face is a free mesh, even though the source mesh (circle) was mapped.
(D) The filled model
The 2D blocking is converted to 3D blocking using the Fill method and Fill Type
set to Swept for Blocking > Create Block > 2D to 3D.
(E) The filled model meshed
Note that the imprinting improved the sweeping.
Split Free Block
The Split Free Block option allows you to decompose a free block further into structured and
swept blocks. This operation requires that you first create sheet block(s) which will then be used to split
the free block. A free block can be split into multiple volumes in a single operation. You can then convert
the split free blocks to structured or swept blocks as required.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
381
Blocking
The sheet blocks used to split the free block are internal faces which pass through the volume. Only
structured sheets are currently supported. A structured sheet can be created from 4 vertices or points
(see the Sheet (p. 361) option in the 3D Blocks (p. 357) section). The split sheets can be either contiguous
or separated by other faces. However, the selected split sheets combined with other faces of the free
block should split the volume into manifold regions. Only those sheets which form the closed volume
need to be specified.
Note
• Currently, the sheet faces must be structured. However, other faces of the free block to be split
can be of any type (structured or free).
• Free blocks with multiple shells can be split only if the split sheets connect inner and outer
shell faces. This will result in single shell manifold volumes after the split.
• Split sheets must be connected to the boundary faces, a rectangular region fully embedded
inside the free block is not supported.
Merge Vertices
The Merge Vertices menu offers the user options for combining two or more points.
Figure 351: Merge Vertices Options
The following options are available for merging vertices:
Merge Vertices
Merge Vertices by Tolerance
Collapse Block
Merge Vertex to Edge
Merge Vertices
The Merge Vertices option allows you to merge two or more vertices.
Two vertices can be merged with the following options:
Propagate merge
propagates the merged vertices throughout the affected block(s).
Merge to average
merges at the average distance of the two vertices.
382
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Merge Vertices
Rebuild orphan
deletes the VORFN part and rebuilds it. This may be necessary in some cases to clean up the VORFN
blocks.
These options can be used in different combinations as illustrated for the example of the two vertices
to be merged in Figure 352: Selection of Vertices to be Merged (p. 383). When selecting the vertices, the
first vertex is retained and the second vertex is merged with the first.
Figure 352: Selection of Vertices to be Merged
• Propagate merge and Merge to average are disabled. Only the selected vertices will be merged (see
Figure 353: Merge Vertices Without Options (p. 383)).
Figure 353: Merge Vertices Without Options
• Propagate merge is disabled while Merge to average is enabled. Only the selected vertices will be
merged at the average distance of the two (see Figure 354: Merge to Average Option Only (p. 384)).
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
383
Blocking
Figure 354: Merge to Average Option Only
• Propagate merge is enabled and Merge to average is disabled. All the connected vertices will be merged
according to the indices value (see Figure 355: Propagate Merge Option Only (p. 384)). For example, the
Vertex to Keep has indices (x1, y, z) and Vertex to Merge has the indices (x2, y, z) so all the vertices
having indices (x1,*,*) will merge with the same family of vertex having the indices (x2,*,*) for example a
vertex with indices (x1,y1,z1) will only merge with vertex with indices (x2,y1,z1).
Figure 355: Propagate Merge Option Only
Note
After selecting the vertices, a Confirm delete station window will ask you to confirm the
direction and the index range to delete the vertices to be merged.
• Propagate merge and Merge to average are enabled. All the connected vertices will be merged similar
to the previous case, but at an average distance between the selected vertices (see Figure 356: Both
Propagate Merge and Merge to Average Options Selected (p. 385)).
384
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Merge Vertices
Figure 356: Both Propagate Merge and Merge to Average Options Selected
Merge Vertices by Tolerance
The Merge Vertices by Tolerance option allows you to merge only those nodes that come under
the specified tolerance limit. Select the vertices to be merged, and specify the tolerance value.
Collapse Block
The Collapse Block option allows you to collapse a block or an edge by shrinking one or more
edges to zero length. This modifies the topology of the remaining non-degenerate blocks. Select the
edge to define the direction that is to be collapsed to zero size. It is possible to add blocks interactively,
which will all be collapsed in the specified direction.
In Figure 357: Selection of Blocks and Edge for Collapse (p. 385), the edges and blocks selected to be
collapsed are shown in red. Figure 358: Collapsed Blocks (p. 385) shows the collapsed blocks.
Figure 357: Selection of Blocks and Edge for Collapse
Figure 358: Collapsed Blocks
Merge Vertex to Edge
The Merge Vertex to Edge option allows you to merge a selected vertex and edge. The selected
edge will be split and merged with the selected vertex.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
385
Blocking
This is most often utilized when the region between the edge and vertex contains no blocks, and the
two disconnected topologies which do not have matching vertices can be merged. Examples of this
would include connecting bottom up blocking or merging blocking topologies.
Figure 359: Connected Blocking Topologies (p. 386) shows two sub topologies which are connected at
the corners but not the middle. The resulting surface mesh is shown in Figure 360: Resulting Surface
Mesh — Unmatched (p. 387). The top of the lower part is curved to fit the upper part as the edges are
projected to the same curves. However, as the edges are not shared, the mesh across these edges is
neither connected nor matched.
Figure 359: Connected Blocking Topologies
386
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Merge Vertices
Figure 360: Resulting Surface Mesh — Unmatched
The lower block can be split to provide the matching vertices and then the Merge Vertices function
could be used, or the Merge Vertex to Edge function can be used to merge the “hanging” vertices
directly to the edge. This will split the edges for the connection, but the block will still appear as a
single block (see Figure 361: Vertex Merged to Edge (p. 387)). After merging the vertex with the edges,
the surface mesh will be properly connected (see Figure 362: Resulting Surface Mesh — Matched (p. 388)).
Figure 361: Vertex Merged to Edge
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
387
Blocking
Figure 362: Resulting Surface Mesh — Matched
Edit Block
Use the Edit Block menu to modify existing blocks.
Figure 363: Edit Block Options
The following options are available for editing blocks:
Merge Blocks
Merge Faces
Modify Ogrid
Periodic Vertices
Convert Block Type
Change Block IJK
Renumber Blocks
Merge Blocks
The Merge Blocks option allows you to merge several blocks into a single large block.
388
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Edit Block
Selected
merges all the selected blocks.
Note
When merging free blocks, you may merge only two, 2D free blocks at one time. You
may not merge 3D free blocks or mix mapped and free blocks.
Automatic
automatically merges all the blocks in the current Block part to the least number of blocks possible.
IJK Direction
merges the blocks in the direction determined by the reference edge selected.
Merge Faces
The Merge Faces option allows you to merge faces and their corresponding blocks. Select the
faces to be merged by selecting the face corners.
Modify Ogrid
The Modify Ogrid option allows you to modify the scale factor of an O-grid.
Method
specifies the method for modifying the O-grid.
Rescale Ogrid
allows you to rescale the O-grid.
Block Select
allows you to select all visible blocks or specific blocks.
Edge
is the radial O-grid edge selected.
Absolute distance, Offset
control the rescaling of the O-grid. If Absolute distance is disabled, the Offset value works as
a factor multiplied by the current O-grid size, where values less than 1 result in a smaller O-grid,
while values greater than 1 yield a larger O-grid. If Absolute distance is enabled, the Offset
value is the new length of the radial edge of the O-grid.
Reset Ogrid Orthogonality
allows you to reset the orthogonality of the selected edge. When an O-grid is created, a radial set
of edges connect the internal/outer O-grid vertices to the external/inner O-grid vertices. The vertices
are orthogonal to each other along the radial edge. This orthogonality may be modified when vertices
are moved.
Periodic Vertices
The Periodic Vertices option allows you to make selected pairs of vertices into periodic nodes.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
389
Blocking
Create
allows you to select pairs of nodes that should be periodic transforms of one another. A face is a periodic
transform of another if its four corners are periodic transforms of the other face's nodes. When a periodic
face is split, all the new vertices and faces will be periodic.
Note
An axis node should be selected twice in order to make it periodic with itself.
Remove
allows you to select a pair of vertices to remove the periodicity.
Note
To generate a periodic mesh, remember to make the initial block periodic. Further splits
will maintain this periodicity. It is much easier to make the first four pairs of vertices
periodic then to match up many vertices later to be made periodic.
Auto Create
creates periodic links between block vertices on the periodic boundaries automatically.
Note
This works on a 3D Blocking with model periodicity defined. It finds the periodic twins
through Geometry transformation and blocking edge connectivity. Periodic vertices that
are associated to points are found directly by geometry transformation. It expects that
periodic points are within a geometric tolerance of 1.0e-05. Periodic vertices that are
projected to curves are found through periodic curve pairs or blocking edge connectivity
along the periodic direction. Surface associated vertices are first found by transformation
or best closest match.
Convert Block Type
The Convert Block Type option allows you to convert blocks into the following blocking types.
See User’s Manual > Hexa > Hexa Block Types for a description of the different block types.
Mapped
converts a block to a mapped block. The block converted must have 4 corners in 2D (or 8 corners and
6 mapped faces in 3D). The Mapping algorithm forces the number of nodes on opposite sides to be
equal. If they are not equal, the larger number will be used. This number of nodes will be propagated
through all parallel edges.
Free
converts a block to a free (unstructured) block. In 2D, this will result in a paved surface which can be all
triangles, quad dominant, quad with one tri, or all quad. In 3D, the free block mesh type can be Tetra
(Delaunay, TGrid or Advancing Front), Hexa Core or Hexa Dominant mesh. In 2D, this is most often used
390
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Edit Block
to solve issues with poor internal angles after mapping to curves or to prevent node counts from
propagating across a face.
Note
An error will be reported if the selected block is in the VORFN part.
Figure 364: Conversion of a Mapped Block to a Free Block
(A) Mapped Block
(B) Free Block with All Quad Mesh
(C) Free Block with Quad with one Tri Mesh
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
391
Blocking
(D) Free Block with Quad Dominant Mesh
(E) Free Block with All Tri Mesh
Swept
converts a mapped block to a swept block. The face selected is converted to a free face and swept across
the block and any parallel blocks. While mapped blocks must have the same nodes on opposite sides
of the block in the I, J and K directions, a swept block is free to have varying nodes in two directions
(across the selected face) and is mapped in the third (perpendicular to the selected face).
392
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Edit Block
Figure 365: Conversion of a Mapped Block to a Swept Block
(A) Mapped Block
(B) Swept Block
Y-Block
converts a degenerate (wedge) block to a Y-block (quarter O-grid).
3D Free Block Mesh Type
converts a free block mesh to an unstructured mesh type of Tetra or Hexa-Core mesh. Figure 366: Changing
the 3D Free Block Mesh Type (p. 394) shows the conversion of the unstructured Delaunay tetra mesh
(with a Free Quad Dominant face) to hexa-dominant mesh using this option.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
393
Blocking
Figure 366: Changing the 3D Free Block Mesh Type
Convert free block face to free
allows you to convert the mapped external face adjacent to a free block to a free face. In Figure 367: Converting Free Block Face to Free (p. 394), the circular face adjacent to the hexa mesh is initially mapped.
The unseen volume is free (unstructured tetra in this case). This results in poor elements at the corners
(the maximum angle approaches 180 degrees as the mesh is refined). Using this option to convert the
structured face to an unstructured face (quad dominant in the example) results in improved quality.
Figure 367: Converting Free Block Face to Free
Free Face Mesh Type
converts the free face mesh type to the type selected. Figure 368: Changing the Free Face Mesh
Type (p. 394) shows the conversion of the free face mesh type from the default quad-dominant to the
all tri type which is more appropriate for the tetra mesh in the adjacent free block.
Figure 368: Changing the Free Face Mesh Type
394
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Associate
Reverse Swept Direction
reverses the sweep direction for a swept block. This can be useful in some situations where you want
to better control the seeding on the free face of the sweep, such as when using a reference mesh (see
the Reference Mesh option for the Associate Face to Surface option).
Merge Sheet with free Block
allows you to merge a 2D (sheet) block with a 3D free block. Using this option will ensure node to node
connections between the two regions. For CFD users, this option can be used to connect a wall-mounted
baffle with the rest of the mesh. For FEA users, this option can be used to combine 2D and 3D portions
of the geometry.
Figure 369: Merging 2D (Sheet) Block With a Free Block (p. 395) shows an example where a wallmounted baffle has been connected to rest of the mesh using this option.
Figure 369: Merging 2D (Sheet) Block With a Free Block
Change Block IJK
The Change Block IJK option allows you to change the IJK indices of a block.
IJK->KIJ
changes indices from IJK to KIJ.
Set Origin
sets the origin at a selected vertex.
Align Blocks
aligns all blocks with reference to a selected block.
Set IJK
sets the current IJK indices to new IJK indices.
Renumber Blocks
The Renumber Blocks option allows you to renumber blocks.
Associate
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
395
Blocking
Figure 370: Blocking Associations Options
The following options are available for blocking associations.
Associate Vertex
Associate Edge to Curve
Associate Edge to Surface
Associate Face to Surface
Disassociate from Geometry
Update Associations
Reset Associations
Snap Project Vertices
Group/Ungroup Curves
Auto Associate
Associate Vertex
The Associate Vertex option allows you to associate vertices and project the vertex onto itself,
points, curves, and surfaces. Select the vertex and the entity to project it onto.
Associate Edge to Curve
The Associate Edge to Curve option allows you to associate the edges of blocks to curves. The
vertices at the end of the edges are also associated to the same curve unless they were previously associated to another curve or point. Edge segments can be individually associated after using edge splits.
Multiple edges can be associated with multiple curves, but all the curves will be grouped into a single
composite curve.
Note
Associating edges to curves also results in the creation of line elements along those
curves. For 2D planar blocking, it is essential that all the perimeter edges be associated
with perimeter curves because many solvers use the perimeter line elements as
boundaries.
Project vertices
If enabled, the vertices will automatically be projected to the corresponding curves.
Project to surface intersection
If enabled, the surface-surface intersection will be captured correctly. This is for poor geometry situations
where the intersection curve may not match with the intersection of the surfaces. If you associate an
edge with a curve using this option, the edge will be colored purple. The edge is associated with the
396
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Associate
curve, but when the mesh is generated, the nodes will first project to the curve, and then they will
project to the surface (the true surface/surface intersection).
In the examples in Figure 371: Examples of Project to Surface Intersection (p. 397), the intersection
curve is slightly above the surface. The green edge on the left is associated with the curve without
enabling this option and therefore its nodes are off the true surface intersection. The purple edge
on the right is associated to the curve with this option. The edge is therefore associated with the
curve, but the nodes ultimately project to the surface intersection. This is better than simply projecting
the edge to the curve because the nodes are guided by the curvature of the curve.
Figure 371: Examples of Project to Surface Intersection
Project ends to curve intersection
If enabled, the vertices will be enforced at the ends of the curve.
Associate Edge to Surface
The Associate Edge to Surface option allows you to associate the edges of blocks to surfaces.
The color of the selected edges will turn white/black, indicating that the nodes on that edge will be
projected to the nearest active surface. By default, edges and faces between two blocking materials
(boundary faces) will automatically associate with the nearest active surface. Related vertices and edge
splits will also be associated with the nearest active surface. When moving vertices or edge splits, there
will be no movement until the cursor passes over an active surface. Ensure that the vertices or edge
splits are moving on the correct surface.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
397
Blocking
Associate Face to Surface
The Associate Face to Surface option allows you to adjust how faces relate to the geometry. By
default, edges and faces between two blocking materials (boundary faces) will automatically associate
with the nearest active surface.
Click the selection icons to select the face(s) and the surface part.
The following options are available for associating faces to surfaces:
Closest
finds the closest surface for projection. For boundary faces, this returns face association to the default.
It can also be used to force internal faces to follow a surface.
Interpolate
interpolates the shape of the meshed face from the shape of the bounding edges, rather than projecting
the nodes to the surface. The surface mesh will still inherit the family name of the closest surface part.
Use this feature if a face crosses a missing or poor quality surface.
Part
projects the face to the surface that is in the specified part. This is useful for closely spaced curved surfaces,
such as turbine blades, to ensure that each face projects to the correct surface, and not merely the
closest surface.
Note
If you associate the face to a part which contains no surfaces, it will instead interpolate
the mesh and place the elements in the specified part. This can be used to control the
part name of the interpolated mesh.
Shared Wall
allows you to set a general projection rule regarding faces between two specific volume parts.
Create
sets the rule that the faces between the specified volume parts should always be projected to surfaces
of the specified surface part.
Remove Shared Wall
removes the above rule for a given pair of volume parts.
None
removes the default behavior so that edges/faces between specified volumes do not automatically
associate with surfaces. This is useful when there is no boundary between volumes or if you are using
volume parts to break up a model for display or selection purposes, but the regions don’t actually
represent physical differences which would require a boundary.
Link Shapes
allows the internal face to have the same shape as the linked boundary face. The faces can be unlinked
by disassociating them. Select the boundary face and the associated internal face.
A model with two different materials is shown in Figure 372: Example of Link Shapes (p. 399). The
Shared Wall option is set to None, so there is no projection between the parts. In figure (A), the
398
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Associate
internal face is not linked to the top face. The top block projects to the curved surface (not shown),
but the inner block is interpolated straight across the volume. After linking the internal face with
the top face (figure (B)), the change in the mesh curvature transitions more gradually across both
blocks instead of just the top one.
Figure 372: Example of Link Shapes
(A) Internal Face not Linked to the Boundary Face
(B) Internal Face Linked to the Boundary Face
Reference Mesh
allows you to use an existing surface mesh to seed an unstructured or swept face. This option can be
used to obtain a better quality mesh or to set up node for node contact with a preexisting unstructured
mesh.
An example demonstrating the use of the Reference Mesh option is shown in Figure 373: Using
the Reference Mesh Option (p. 400). The Multi-zone blocking on the geometry was generated automatically and one half mapped by default. The other half is an unstructured swept block with “all
tri” free faces. To use a reference mesh, load an unstructured surface mesh and make sure the mesh
perimeter matches the edge perimeter, including associations to surrounding curves. Verify the
sweep direction (see the Reverse Swept Direction option) for the swept block. Select the Reference
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
399
Blocking
Mesh option, select the appropriate unstructured face and click Apply. The swept mesh will be
seeded with the reference mesh.
Figure 373: Using the Reference Mesh Option
(A) The automatically generated Multi-zone blocking/mesh on the geometry.
(B) The unstructured quad dominant surface mesh used as the reference mesh.
400
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Associate
(C) The resulting swept mesh seeded with the reference mesh.
Selected Surface
allows you to associate the selected face(s) with the specified surface.
Disassociate from Geometry
The Disassociate from Geometry option allows you to disassociate the selected edge, surface or
face that is associated to the geometry.
The selection of different entities to be disassociated can be done individually or together.
Note
Any association can be removed (associated to nothing), however, you can easily overwrite
associations without disassociating first. For instance, if an edge is associated with a curve,
you can directly associate it with a surface, you do not need to first disassociate it.
Update Associations
The Update Associations option allows you to set associations to the nearest entities of the assigned type.
Vertices
updates associations of all vertices.
Edges
updates associations of all edges.
Faces
updates associations of all faces.
Only Dormant entities
when enabled, will update associations for blocking that was associated with entities that are now
dormant to the closest entities instead.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
401
Blocking
Update Blocking
allows you to update blocking to a new geometry file. This option is used when there are geometric
changes while the topology remains the same. Update Blocking uses the entity names. If blocking is
created for one geometry file and saved, and then a second geometry file with consistent entity names
is opened, the Update Blocking option will attempt to update the blocks to the new geometry file.
• Parametric
When there is a parametric change in geometry, then Parametric method will update the blocking
associations. When the initial blocking file is saved in relation to the first geometry file, the vertices
contain links to the geometry in terms of the curve T parameter space and surface UV parameter
space. Using the Parametric method will move the vertices to the same parametric space of the
new geometry file.
• Morphing
For some changes in geometry, such as geometric entities moved a large distance, or a Trim
Surface operation, the Morphing Method should be used. This approach uses the Parametric
method for curves, but for surfaces it will evaluate whether the surfaces are trimmed and adjust
the vertices linked to the UV parameter space to a more accurate position based on attached
curves. Instead of moving the surface vertices based on the UV parameter space, the surface
vertices will be moved in reference to neighbor vertices.
The original geometry and blocking is shown in Figure 374: Original Geometry and Blocking (p. 402).
The geometry is then scaled in the Z direction as shown in Figure 375: Geometry Scaled in Z Direction (p. 403). Finally, the result of updating the blocking associations is shown in Figure 376: Blocking
Associations Updated (p. 403).
Figure 374: Original Geometry and Blocking
402
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Associate
Figure 375: Geometry Scaled in Z Direction
Figure 376: Blocking Associations Updated
Reset Associations
The Reset Associations option resets the associations of exterior blocking entities back to association with the nearest entity.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
403
Blocking
Vertices
allows you to reset the vertex-point associations.
All
resets associations for all vertices.
Only visible
resets associations for visible vertices.
Edges
allows you to reset the edge-curve associations.
All
resets associations for all edges.
Only visible
resets associations for visible edges.
Faces
allows you to reset the face-surface associations.
All
resets associations for all faces.
Only visible
resets associations for visible faces.
Snap Project Vertices
The Snap Project Vertices option allows you to project all the vertices that are associated to respective points, curves or surfaces. The following options are available for projecting vertices:
All Visible
projects all visible vertices to their respective entity.
Selected
projects selected vertices to their respective entity.
Move O-Grid nodes
moves internal nodes (that are not projecting) which are attached via an O-grid edge to external nodes
(nodes that are projecting) relative to the projection.
Note
Projection only applies to active parts. Projection will not be affected by entities that are
blanked but are included in visible parts. If you do not want nodes to be moved to certain
entities, the entities must be placed in a separate part that is disabled.
404
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Move Vertex
Group/Ungroup Curves
The Group/Ungroup Curves option allows you to group curves into a composite curve, or ungroup
composite curves into separate curves. This is needed for associating an edge to a set of curves. The
curves should first be grouped into a composite curve, and then the edge can be associated to that
composite curve.
Composite curves can be displayed by right clicking on Curves in the Display Tree and selecting the
option Show Composite.
Group Curves
groups the selected curves into one composite curve. The selected curves can include existing composite
curves.
Selected
groups only the selected curves.
All tangential
groups all curves that are tangential to the selected curves.
Part by Part
groups all the curves in each part into composite curves.
Ungroup Curves
allows you to select the composite curve to ungroup.
Auto Associate
The Auto Associate option allows you to associate edges to curves. Auto Association looks at the
topology of the surfaces and the topology of the blocking and attempts to link the edge projections
of the blocking in relation to the topology of the geometry.
Move Vertex
Figure 377: Move Vertices Options
The following options are available for moving vertices:
Move Vertex
Set Location
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
405
Blocking
Align Vertices
Align Vertices In-line
Set Edge Length
Move Face Vertices
Move Vertex
The Move Vertex option allows you to modify the location of a vertex. Select a vertex using the
left mouse button, accept the selection by pressing the middle mouse button, and use the right mouse
button to cancel the selection. After fixing the constraints, select the vertex to move.
Single Method
allows you to select a single vertex to be moved.
Multiple Method
allows you to select multiple vertices for movement.
Movement Constraints
allows you to constrain a vertex to moving in any direction.
Normal to Surf
allows you to move the vertex normal to the surface.
Move dependent
allows you to move dependent vertices.
There are different types of vertices/edges, and their movement is governed by their projection as
shown in Figure 378: Different Types of Vertices and Edges (p. 406).
Figure 378: Different Types of Vertices and Edges
White Edges/Vertices
These are between two material volumes. The edge and the associated vertices will be projected to the
closest CAD surface between these material volumes. Vertices can only move on the surfaces.
Blue Edges/Vertices
These are in the volume. The blue vertices can be moved by selecting the edge just before it and can
be dragged onto that edge.
Green Edges/Vertices
These edges and the associated vertices are being projected to curves. The vertices can only be moved
on the curves that they are projected to.
406
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Move Vertex
Red Vertices
These cannot be moved, they are projected to fixed points. They can only be moved by first changing
their projection to one of the other projection types.
Set Location
The Set Location option allows you to move vertices by setting their location with the following
options:
Set Position
allows you to modify the coordinates of selected vertices. The vertices may be selected individually. You
can also select a Reference Point and based on its position, modify the X, Y, and Z (or R, θ, and Z) directions of the selected vertices.
Multiple vertices can be selected and modified at the same time. Typically, this function is used to
modify a number of vertices to one specific coordinate, for example Y=0, to ensure a true symmetry
plane.
Reference From
allows you to select the reference point of the vertices to be moved. The reference point can either
be an existing vertex, or a position on the screen.
Set Coordinate System
sets the appropriate coordinate system.
• Cartesian Coordinate System
Select which direction to move the vertices: X, Y, Z, or the Normal direction. Enter the number
of units of distance.
• Cylindrical Coordinate System
Select which direction to move the vertices: R, θ, or Z direction. Enter the number of units of
distance.
Vertices to Set
specifies the vertices to be moved. Select the vertices to be moved and click Apply.
Increment Position
allows you to move vertices by the specified increment in any direction. For example, vertices can be
moved 10 units in the X-direction by entering “10” in the Modify X option.
Set Coordinate System
sets the appropriate coordinate system.
• Cartesian Coordinate System
Select which direction to move the vertices: X, Y, Z, or the Normal directions. Enter the number
of units of distance.
• Cylindrical Coordinate System
Select which direction to move the vertices: R, θ, or Z directions. Enter the number of units
of distance.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
407
Blocking
Vertices to Set
specifies the vertices to be moved. Select the vertices to be moved and click Apply.
Align Vertices
The Align Vertices option allows you to align vertices along an edge to a selected reference vertex
using planes. You can specify the plane in which the vertices will move.
Along edge direction
allows you to align all vertices along the selected edge to the reference vertex.
Reference vertex
specifies the vertex that the vertices along the selected edge will be aligned to. The vertex must be at
a location along the edge.
Coordinate system
specifies the current active coordinate system, either Cartesian or Cylindrical.
• Cartesian Coordinate System
Move in plane
allows you to select the plane in which the vertices are to be moved. For the User Defined option,
specify the vector normal to the desired plane.
• Cylindrical Coordinate System
Parameter
allows you to select the specified parameter of the vertices will be aligned to the reference vertex.
Align Vertices In-line
The Align Vertices In-line option allows you to align vertices to a defined line. Select two points
to define the reference direction of the line, and then select the vertices to align to that line.
Set Edge Length
The Set Edge Length option allows you to modify the length of edges explicitly. Select the edge(s)
to be modified and specify the length.
Freeze Vert(s)
allows you to override the default vertex adjustment and select which end vertex remains “frozen”
in the same position when the edge length is modified. This option is disabled by default.
The default node movement is determined based on the association of the end vertices. If the
association is the same, both vertices are moved equally. In other cases, the more restrictive
vertex association is frozen automatically, and the other vertex is moved as per the length
specified. Vertices associated to an entity will be restricted as opposed to non-associated vertices.
408
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Transform Blocks
The order of restrictive association is association to point > association to curve > association
to surface.
Note
When selecting multiple vertices to be frozen, ensure that only one of the end vertices
of the edge being modified is selected.
Move Face Vertices
The Move Face Vertices option allows you to move or rotated face vertices.
Move Face Vertices
allows you to move the face vertices. Select the face whose vertices are to be moved. Specify the direction
by entering an offset vector, or by selecting the start and end points for moving the face vertices.
Rotate Vertices
allows you to rotate the vertices. Select the vertices to be rotated, the center point, and the angle of
rotation. Specify the rotation axis by entering a vector, or by selecting the start and end points.
Transform Blocks
Figure 379: Transform Block Window
The following options are available for transforming blocks.
Translate Blocks
Rotate Blocks
Mirror Blocks
Scale Blocks
Copy Periodic Blocking
Translate and Rotate
For the Translate, Rotate, Mirror, Scale and Translate and Rotate options, select the block(s) to be
transformed. When no specific blocks are selected, it implies that the whole blocking will be transformed.
You can specify whether to make copies of the blocks using the Copy option.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
409
Blocking
You can use the Transform geometry also option to transform the geometry only when transforming
all the blocks. To use this option, do not explicitly select any blocks, which is functionally equivalent to
selecting all blocks.
Translate Blocks
The Translate Blocks option allows you to move the original block topology laterally without rotation.
Select
Opens the Select Blocking-block menu to choose which blocks will be moved/copied.
Copy
If checked, the original block will remain, duplicate(s) will be created.
Transform geometry also
If checked, the geometry will be moved/copied with the selected block(s).
There are two methods to specify the distance of translation:
Explicit
allows you to specify the direction to move the block in X, Y, and Z directions.
Two Point Vector
allows you to specify the magnitude and direction to move the block by selecting two points to define
a vector.
Rotate Blocks
The Rotate Blocks option allows you to rotate the original block topology.
Axis
specifies the axis of rotation. Select the X, Y, Z axes, or another user-defined vector.
Angle
specifies the value of the angle the block is to move.
Center of Rotation
specifies the center of rotation. Select the origin, centroid, or a user-defined point.
Mirror Blocks
The Mirror Blocks option allows you to mirror the topology about a specified plane.
The Plane Axis defines the plane orientation by its normal vector: X-axis, Y-axis, Z-axis, or a vector
defined by two points.
Specify the Point of Reflection as the origin, centroid, or a user-defined point.
410
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Transform Blocks
Scale Blocks
The Scale Blocks option allows you to change the size of the topology.
Scale Blocks by setting a factor for each direction of the coordinate system.
Specify the Center of Transformation as the origin, centroid, or a user-defined point.
Copy Periodic Blocking
The Copy Periodic Blocking option allows you to copy the blocking for periodic models. This
feature is useful when the model is periodic but the geometry is available only for one sector. The
blocking is first done on the sector geometry, and then both the geometry and blocking are copied
and rotated to form the full model.
Note
The periodicity settings defined in Mesh > Set Up Periodicity will be applied.
Num. copies
specifies the number of copies of the geometry to be made.
Increment parts
allows you to select Parts that will remain the same and the copies will be placed in Parts with the
same name plus an increment. By default, the copies of entities will be placed in the same Part as
the original. For example, two copies of the Part “Blade” can be created and placed in Parts named
“Blade_2”, and “Blade_3”.
Translate and Rotate
The Translate and Rotate option allows you to translate and rotate the blocking simultaneously.
The reference location and target locations can be defined by 3 points, a curve or LCS and the blocking
is translated and rotated to match.
Copy
If enabled, a copy of the selected entities will be created in the new location.
Translate and Rotate Method
The three options for method are as follows:
3 points –> 3 points
Select six points in all. The first three points will be used as the reference for the entity to be transformed. The second set of three points is used to define the transformation. The result will match
the first points of both sets, and the direction from the first to the second point, and the plane
defined by the third point.
Curve –> Curve
Select two curves. The first curve is used as a reference for the entity to be transformed. The second
curve is used to define the transformation. The result will match the beginning (parameter = 0) of
both curves, the direction from parameter 0 to 0.5, and the plane defined by the end (parameter 1)
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
411
Blocking
of the curves. A curve used to define the transformation can be included in the entities selected to
be transformed.
LCS –> LCS
Click Show LCS to view any defined coordinate systems. Select two local coordinate systems.
The result will match the origins and align the axes of the first LCS to the second LCS.
Edit Edge
Figure 380: Edit Edge Options
The following options are available for editing unstructured surface block edges:
Split Edge
Unsplit Edge
Link Edge
Unlink Edge
Change Edge Split Type
Split Edge
The Split Edge option allows you to edit block edges using the following Split types.
Spline
allows you to select the edge to be split and converted to a spline. Click on the edge and drag to specify
the desired shape of the spline. The change will be applied when the mouse button is released. In Figure 381: Spline Type Edge Split (p. 412), the first picture shows the initial edge, and the second picture
shows the edge after a spline split.
Figure 381: Spline Type Edge Split
Linear
allows you to split the selected edge into linear edges. Figure 382: Linear Type Edge Split (p. 413) shows
linear splits of a straight edge.
412
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Edit Edge
Figure 382: Linear Type Edge Split
Control Point
is shown in Figure 383: Control Point Type Edge Split (p. 413).
Figure 383: Control Point Type Edge Split
Automatic Linear
allows you to automatically make the selected edge into a linear edge.
All Edges
allows you to convert all the edges into linear edges.
Note
This option corresponds to using the command ic_hex_auto_split_edge all in the replay script.
Tangents
uses the tangencies of the attached edges at a vertex to a selected edge to split the selected edge. Each
edge will be split twice, once for each vertex. For example, for a simple O-grid inside of a block, if the
internal block's edges were split with this option, the internal block would take on a spherical shape.
Method
For each vertex, the edge can be split by one of the following methods:
Orthogonal
The length of the tangent edge will be based on the specified Factor. Enter a value or use the
sliding bar.
Enter Tangent
Specify a Tangency point in relation to the vertex. The length of the tangent edge will be based
on the specified Factor. Enter a value or use the sliding bar.
None
This option ignores the tangency of the vertex.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
413
Blocking
All at Vertex (Smooth)
allows you to split all the edges connected to the selected vertex to improve the angles between the
edges at that vertex. If there are four edges, they will be split so that they meet at 90 degree angles at
the vertex.
Tip
When using replay scripts, the command ic_hex_split_edge allows you to split the edge at
the specified location.
For example, ic_hex_split_edge 21 25 0 1.7 8.5 0 implies that edge 21–25 will
be split at the location (1.7, 8.5, 0). The value 0 in this example indicates that this is the first
split between the vertices 21 (start vertex) and 25 (end vertex). Alternatively, a value of 1
would indicate that the split is the second between the specified vertices, and so on.
To use an existing point to indicate the location to be used, you can use the following in
the replay script:
set name pnt.00 ;# point must exist
set loc [ic_geo_get_point_location $name]
set x [lindex $loc 0]
set y [lindex $loc 1]
set z [lindex $loc 2]
ic_hex_split_edge 21 25 0 $x $y $z
Unsplit Edge
The Unsplit Edge option allows you to remove splits from edges. For the Single method, select
the vertex of the split edge to remove. For the All method, select the edge to remove all the splits.
Link Edge
The Link Edge option allows you to set the shape of edges. Select the target edges and then the
edge for the source of the shape.
Selected
sets the shape of only the selected edge.
Interactive
allows you to set the shape of the targeted edge(s) interactively.
In dimension
sets the shape automatically for all connected edges. Select the source edge for the Link Edge Dimension,
the Source index or vertex, and the Target index or vertex.
Unlink Edge
The Unlink Edge option allows you to unset the shapes of edges linked by the Link Edge option.
414
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Params
Change Edge Split Type
The Change Edge Split Type option allows you to change the edge split type (e.g., change spline
to linear). The options available are Spline, Linear, and Control Point.
Pre-Mesh Params
Figure 384: Pre-Mesh Parameters Options
The following options are available for Pre-Mesh parameters:
Update Sizes
Scale Sizes
Edge Params
Match Edges
Refinement
Update Sizes
The Update Sizes option allows you to update sizes in the pre-mesh. The following options are
available for updating sizes in the pre-mesh:
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
415
Blocking
Update All
computes the edge node spacing based on constraint equations with the default (BiGeometric) meshing
law. You can adjust the number of nodes on each edge based on the Global Surface or Curve Mesh
Size and by default each edge will follow the BiGeometric geometry law.
Note
The default meshing law and bunching ratio are specified under Settings > Meshing >
Hexa/Mixed.
Note
You can check the distribution by clicking Blocking > Edge > Show Edge Info to verify
that each edge follows the default (BiGeometric) geometry law.
Note
For 3D blocking, the Curve Mesh Size parameters are only applied to edges that are
associated with curves. For 2D blocking, the Curve Mesh Size parameters are applied
to all curves.
Keep Distributions
adjusts the number of nodes on each edge based on the Global Surface or Curve Mesh Size. It differs
from the Update All method in that the edges follows the geometric law assigned to it, and not the
default geometric law.
Note
For 3D blocking, the Curve Mesh Size parameters are only applied to edges that are
associated with curves. For 2D blocking, the Curve Mesh Size parameters are applied
to all curves.
Keep Counts
allows you to change the geometry law of the edges to the default (BiGeometric) geometry law. This
option differs from Update All and Keep Distribution in that the distribution of nodes is not altered
according to the Global Surface or Curve Mesh Size.
Curve->Edge bunching
transfers the Advanced Bunching Parameters specified for curves to their associated edges.
You can apply Advanced Bunching to curves using the options available for Curve Mesh Setup in
the Mesh tab. You can apply various bunching laws including Uniform, BiGeometric, and Hyperbolic,
(described in the Bunching Laws (p. 422) section) along with end spacing, ratios and maximum
spacing. This is primarily for use with the patch based surface meshers. Pre-Mesh Params uses the
smallest average mesh size to calculate the initial pre-mesh distribution. The use of the Curve ->
Edge bunching option to transfer the Curve Advanced Bunching Parameters to the associated
edges is shown in Figure 385: Using the Curve->Edge Bunching Option (p. 417).
416
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Params
Figure 385: Using the Curve->Edge Bunching Option
(A) Update all does not respect Curve Advanced Bunching
(B) Curve->Edge bunching transfers Curve
Advanced Bunching to Edge Parameters
In this case, only one curve had Advanced
Parameters specified and this distribution
was copied to parallel edges.
Note
Only intentionally set Advanced Bunching is transferred. Parallel edges without explicitly
set Advanced Curve bunching will get the same distribution as their neighbors. This
means it is not necessary to setup all the curves; parallel edges will automatically inherit
the distribution from a single Curve with Advanced Bunching. To force the parallel distribution back to the default uniform bunching, you must select Uniform explicitly under
Curve Parameters or adjust it afterward with the Edge Parameters.
Note
This option is useful if you wish to store the Advanced Bunching with the Geometry file.
Generally speaking, it is recommended that you use Blocking Edge parameters instead
because there are more options and it is easier to copy or link parameters.
Multiple Curve Advance Bunching can be applied in parallel as shown in Figure 386: Multiple Curve
Advanced Bunching (p. 418). Three different edge parameters are applied on the block shown. Edge
distribution will be copied to parallel neighbors without explicit Curve Advanced Bunching. To make
the bunching return to the default uniform bunching, Curve Advanced Bunching was explicitly set
to Uniform.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
417
Blocking
Figure 386: Multiple Curve Advanced Bunching
Run Check/Fix Blocks
allows you to run the check for inconsistencies in the internal block data structures and fix them if possible.
The default setting corresponds to that set for Check/Fix Blocks in the Hexa/Mixed Meshing Options
DEZ.
Scale Sizes
The Scale Sizes option allows you to scale the mesh size globally.
Factor
specifies the factor by which the mesh size will be globally multiplied.
In Figure 388: Block Mesh Scaled by Factor of 1.5 (p. 419), the mesh size (from Figure 387: Initial Block
Mesh (p. 418)) was changed by a factor of 1.5.
Figure 387: Initial Block Mesh
418
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Params
Figure 388: Block Mesh Scaled by Factor of 1.5
Scale Initial Spacings
allows you to adjust the end spacings on each of the edges and the max space (each will be divided by
the factor) in addition to scaling the number of nodes. For example, if you entered a Factor of 1.5 and
enabled Scale Initial Spacings, the number of nodes on each edge would increase by 50% while the
end spacing on each edge would be reduced by 33%.
Note
This option only applies to the visible edges.
Edge Params
The Edge Params option allows you to modify the mesh parameters in a detailed manner by
specifying various bunching laws and the node spacing along any particular edge. Each edge has several parameters that determine the spacing of the mesh along the edge: number of nodes, the meshing
law, initial length at the beginning/end of the edge, the expansion of the mesh from the beginning/end
of the edge to the interior, and the maximum element length along the edge.
The Edge Params icon brings up a window with all the mesh parameters. Once an edge has been selected, the mesh parameters for that edge will be displayed. All parameter values may be modified,
except for the Edge ID and the Edge Length, which are pre-defined.
Note
You can also parameterize edge parameters using variables in replay scripts. Refer to Using
Variables in the Replay Script for details.
Nodes
specifies the number of nodes along the edge. The number may be modified using the up and down
arrows or by entering a number in the field.
Mesh law
Allows you to select one of several bunching laws described in detail in Bunching Laws (p. 422).
Spacing
specifies the spacing of the first node from the beginning of the edge (first cell height). When an edge
is selected, an arrow appears along the edge. Spacing 1 refers to the parameters at the beginning end
of the arrow, and Spacing 2 refers to the edge end where the arrow is pointing, as shown in Fig-
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
419
Blocking
ure 389: Edge Meshing Parameters (p. 420). You may modify the values of the parameters available for
the selected Meshing law. The actual values will differ from the requested values only if the requested
values cannot be met. For example, if the Edge length is 10 units, and you specify an initial spacing of
6 on both sides and 11 nodes along the edge, the system will simply space the nodes evenly, giving an
initial spacing of 1 and a spacing ratio of 1.
Ratio
is the growth rate from one cell height to the next. Ratio 1 refers to the parameters at the beginning
end of the arrow, and Ratio 2 refers to the edge end where the arrow is pointing, as shown in the figure
below.
Figure 389: Edge Meshing Parameters
Max Space
specifies the maximum element spacing of the curve.
Spacing Relative
if enabled, the values of Spacing 1 and Spacing 2 are displayed as fractions of the edge length.
Nodes Locked
if enabled, the number of nodes will be fixed. However, Update All will override this and apply the
global parameter values to the mesh.
Parameters locked
if enabled, the Mesh law parameters will be fixed. However, Update All will override this and apply the
global parameter values to the mesh.
Copy Parameters
allows the bunching on the currently selected edge to be copied with various options. If the To All
Parallel Edges option is selected, the distribution of the current edge will be copied to all parallel edges.
Parallel edges are edges that start and end with the same index value. If the To Visible Parallel Edges
option is highlighted, the distribution of the current edge will be copied to just the visible parallel edges.
By default, the bunching parameters of the parallel edges are based upon the relative lengths of the
selected edge and destination edges. The To Selected Edges option allows you to copy edge parameters
to selected edges. The From Edge option allows you to copy a node distribution from an edge to the
currently selected edge. You will be prompted to select the edge to copy the node distribution from.
The Reverse options will copy the node distribution and reverse it during the copy operation.
Copy Absolute
if enabled, the exact spacing from one edge will be copied to the specified edges, regardless of edge
length.
Linked bunching
allows the distribution of nodes on a single edge to be identical to the distribution of nodes on a series
of smaller parallel edges. Linked bunching allows you to define a permanent relationship, called links,
420
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Params
between these edges. For example, if the node distribution must be modified on the smaller edges, the
user does not have to specify any node distribution on the larger edge. The node distribution on the
larger edge will automatically be updated to reflect the node distribution on the smaller edges. This is
primarily used if there are splits that do not cross a block, but mesh distribution on both sides need to
match, as shown in the example below.
To use this option, first click the select icon for the Edge field (in the Pre-Mesh Params > Edge
Params DEZ and select the target edge, which is the longer edge with more nodes. Enable Linked
bunching and click the select icon to select the reference edge. It is important to select the parallel
edge with the same base index as the target edge. In the example in Figure 390: Linked Bunching
Example (p. 421), the lowest of the three edges is selected because it shares the same base index
with the target edge.
Figure 390: Linked Bunching Example
Example of parallel edges with different node distributions
Target and Reference Edge selection
Edges after Linked Bunching option is applied
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
421
Blocking
Highlight dependent edges
highlights in red the dependent edges of the edge selected.
Highlight attached faces
highlights the faces attached to the selected edge.
Highlight master edges
highlights in yellow the linked master edge of the selected edge. Linked edges depend on the master
edge for their parameters.
Reverse parameters
allows you to reverse the parameters for the ends of the currently selected edge. The parameters at the
beginning of the edge (end 1) are switched with the parameters at the end (end 2).
Note
The number of nodes and the meshing laws specified in the Edge Mesh Parameters always
take precedence in determining the number of nodes. Then spacings 1 and 2 are equally
balanced, followed by ratios 1 and 2, which are also equally balanced, and finally Max Space
is considered.
Bunching Laws
BiGeometric
The default bunching law. The two initial heights and ratios define parabolas in a coordinate system
where the number of node points is the X-axis and the cumulative distance along the edge is the Y-axis.
The parabolas are truncated where their tangent lines are identical; the spacing is linear between these
points. If there are not enough nodal points to form this linear segment, a hyperbolic law is used and
the ratios are ignored.
Uniform
The nodes along the edge are uniformly distributed.
Hyperbolic
The spacing at each end are used to define a hyperbolic distribution of the nodes along the edge. You
can set Spacing 1 and Spacing 2, and the growth ratios are determined internally.
422
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Params
The Hyperbolic Tangential Bunching law is described by the following equations:
The parameter limitations are:
Poisson
The spacing of the node intervals is calculated according to a Poisson distribution. Requested values of
Spacing 1 and Spacing 2 are used. Requested values of Ratio 1 and Ratio 2 are not used directly, but
are used to determine if the requested spacing is appropriate. If not, the spacing will be adjusted automatically.
The mapping function is obtained by solving the following differential equation:
,
with the following boundary conditions:
,
where Sp1 = Spacing 1 and Sp2 = Spacing 2.
The function P is required to satisfy the Neumann boundary condition. It is computed by an iterative
optimization process loop. Some parameter limitations are:
0.0 < Sp1 < 1.0
0.0 < Sp2 < 1.0 - Sp2
500 < Number of iterations < 9999
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
423
Blocking
Curvature
The spacing of the node intervals is calculated according to the curvature of the function defining the
distribution.
Geometric 1
Spacing 1 is used to set the first distance from the starting end of the edge, with the remaining nodes
are spaced with a constant growth ratio. Only Spacing 1 is specified.
The Geometric bunching laws are described by the following equation:
,
where is the distance from the starting end to node i, R is the ratio, and N is the total number of
nodes. The ratio R is limited by 0.25 > R > 4.0.
Geometric 2
The same as Geometric 1, except that Spacing 2 is used to define the distribution starting from the terminating end of the edge.
Exponential 1
The Exponential 1 bunching law is described by the following equation:
where
is the distance from the starting end to node i, Sp1 is Spacing 1, N is the total number of
nodes, and R is the ratio, where:
.
Exponential 2
The same as Exponential 1, except that the Spacing 2 and Ratio 2 parameters are used and the distribution
starting point is the terminating end of the edge.
Biexponential
The spacing of the node intervals is calculated according to the law specified for Exponential 1 and 2.
However, Spacing 1, Ratio 1, Spacing 2 , and Ratio 2 are used to define the distribution. The Spacing 1
and Ratio 1 parameters define the distribution from the beginning of the edge to the midpoint of the
edge, and Spacing 2 and Ratio 2 define the distribution from the terminating end of the edge to the
midpoint of the edge.
This bunching law is described by the following equation:
The parameters are computed according to the vertex constraints. If a ratio equals 0 at a vertex,
the spacing constraint at this vertex only is taken into account and the ratio constraint with the
neighbor spacing is left free by decreasing the polynomial order in the mathematical function.
Linear
The spacing of the node intervals is calculated using a linear function.
424
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Params
Match Edges
The Match Edges option allows you to match the edge spacing of a reference edge to a connecting
target edge. The node spacing on the end of the target edge that connects to the reference edge will
be modified to match the node spacing on the reference edge. The following methods are available:
Selected
allows you to match the end spacing of the selected target edge(s) to the adjacent end spacing of
the reference edge. Matching is done around a connected node, so with the interactive Selected
method, all the target edges selected must be connected to the same node as the reference edge.
Match edges is a quick way to ease edge bunching size transitions between connected edges and
adjacent blocks.
Link spacing
links the target edge end spacing with the spacing on the reference edge. Further adjustments
to the reference edge end spacing will automatically be carried to the linked target edges
making updates easier. To remove or modify linked spacing, use the Edge Parameters DEZ.
Alternatively, a match is reset when a new match is specified around the same vertex, with or
without the link spacing.
Automatic
allows you to automatically match edge spacing at selected vertices.
Vertices
specifies the selected vertices.
Spacing
Minimum
selects the edge having the minimum spacing defined at the selected vertex as the reference
edge.
Maximum
selects the edge having the maximum spacing at the selected vertex as the reference edge.
Average
averages the spacing at the selected vertex.
Match Edges Dimension
allows you to select the dimension to be matched. For example, you may want to match edges
only in the O-grid direction (o3). Or, for a turbine blade model, you may match in the I and J
directions first to match the edges in the plane, and then match in the Z direction for even
distribution perpendicular to the plane. You can use the Select option and select the reference
edges to determine the index directions for matching, or use the All option to match the edges
in all directions at once.
Copy bunching
allows you to copy the edge bunching from the selected reference edge to either selected edges
or all parallel edges. When used with scripting, this function has the advantage of listing the “from
edge” and “to edge” rather than the specific edge parameters that existed during the recording.
This is more parametric than copying bunching from the Edge Parameters DEZ.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
425
Blocking
Method
Selected Edges
allows you to copy the bunching from the reference edge to the selected target edge(s).
This copies the bunching law, end spacings, end ratios and number of nodes.
You can choose to Exclude Number of Nodes if you do not want that parameter
copied.
All Parallel Edges
allows you to copy the bunching from the reference edge to all parallel edges. If Copy absolute is enabled, the exact spacing from one edge will be copied to the specified edges,
regardless of edge length.
Refinement
The Refinement option allows you to refine blocks by a scale factor, as shown in Figure 393: Block
Refined (p. 427). A Level value greater than 1 will result in refinement, while a Level value less than 1
will result in coarsening of the pre-mesh.
Blocks
allows you to select the blocks to be refined.
Level
specifies the number of levels to refine the blocking.
Refinement Dimension
If All is selected, the blocks will be refined in every dimension. If Selected is chosen, you can enter
the dimension (edge) that specifies the direction in which to modify the block. The value 0 corresponds to the X or I direction, 1 corresponds to the Y or J direction and 2 corresponds to the Z or
K direction.
Figure 391: Initial Mesh
426
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Quality
Figure 392: Selection of Blocks and Edge for Refinement
The result is shown below, in which the block is refined in the selected region and along the selected
dimension.
Figure 393: Block Refined
Pre-Mesh Quality
The Pre-Mesh Quality option allows you to check the mesh quality. All the elements of the current
volume family will be included in the quality check.
Note
Quality for volume elements only is calculated for 3D blocking. If you use Edit Mesh > Display
Mesh Quality for the same mesh, the quality may be different if surface elements are included
for that calculation.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
427
Blocking
Criterion
specifies the quality criterion. The criteria available for selection are described in Pre Mesh Quality Options (p. 428).
Min overview
reports the minimum quality for all applicable metrics in the message window.
Histogram Options
allows you to set the minimum and maximum X-axis values, the maximum Y-height, and the number
of bars displayed in the histogram.
Note
You can also change the histogram display settings and ranges by right-clicking in the
histogram window.
Only visible index range
if the visible index range is reduced, then only the elements that are in the index range set by the Index
Control will be checked. The Index Control window is accessible from the menu that appears when right
clicking on Blocking in the Display Tree.
Active parts only
if enabled, only the elements within active parts (Display Tree) will be checked.
Pre Mesh Quality Options
The quality can be checked using many different criteria, as described in the following sections:
Angle
Aspect Ratio
Constant Radius
Custom Quality
Determinant (2x2x2 stencil)
Determinant (3x3x3 stencil)
Distortion
Equiangle Skewness
Eriksson Skewness
428
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Quality
Ford
Hex. Face Aspect Ratio
Hex. Face Distortion
Max Angle
Max Dihedral Angle
Max Length
Max Ortho
Max Ortho 4.3v
Max Ratio
Max Sector Volume
Max Side
Max Warp
Max Warp 4.3v
Mid Node
Mid Node Angle
Min Angle
Min Ortho
Min Sector Volume
Min Side
Opp Face Area Ratio
Opp. Face Parallelism
Orientation
Quality
Taper
Volume
Volume Change
Warpage
X Size
Y Size
Z Size
Angle
This option checks the minimum internal angle for each element. The default range is 0–90 degrees,
with 0 as degenerate and 90 as perfect.
Aspect Ratio
For hexahedral elements, the Aspect ratio is defined as the size of the minimum element edge divided
by the size of the maximum element edge. The values are scaled and the default range of values is
1–20, such that an Aspect ratio of 1 indicates a regular element.
Constant Radius
This option computes the distortion of a plane, based upon the nodes that compose the surface. The
less warped the plane is, the better quality of mesh the model will have. The default range is 0–20, but
if the computed range is above 20, the Min Value will be set to zero and the Max Value will be automatically adjusted to ensure the histogram includes all existing elements.
Custom Quality
This option allows you to define your own quality metric as the combination of the following quality
criteria and element types: Determinant, Warp, Min Angle, and Max Angle.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
429
Blocking
You can specify the maximum and minimum quality levels of a histogram for quad and tri elements.
All values are adjusted to a scale of 0 to 1 when Recompute is pressed.
For example, if the Min Angle Quad is 30 degrees and the maximum is 45 degrees, then 30 degrees
will correspond to the minimum value in the custom quality and 45 degrees will correspond to the
maximum value.
Determinant (2x2x2 stencil)
The Determinant, more properly defined as the relative determinant, is the ratio of the smallest determinant of the Jacobian matrix divided by the largest determinant of the Jacobian matrix. In this option,
the determinant at each corner of the hexahedron is found. The default range is 0–1 with a Determinant
value of 1 indicating a perfectly regular mesh element and 0 indicating an element degenerate in one
or more edges. Negative values indicate inverted elements.
Note
This determinant is appropriate for 3D linear hexas and calculates more quickly than the
3x3x3 matrix because it does not include the unnecessary mid side nodes.
Determinant (3x3x3 stencil)
This is for hexahedral elements. This option is the same as the 2x2x2 stencil, but edge midpoints of
blocks are added to the Jacobian computation.
The Jacobian determinants for hexahedras will be calculated at r,s,t = -1,0,1 of the natural coordinate
system of the element (27 node positions). Next it calculates the maximum absolute determinant of
the 27 determinants (3x3x3). If this is at position i with absolute determinant value max0, then for each
of the 27 positions (j) (except i) the absolute distance of determinant j to determinant i will be calculated.
The final result will then be 1 minus the maximum of the absolute distances divided by max0, so that
the range of this quality criterion value will be between -1 and 1. The Jacobian determinant is the determinant of the Jacobian operator which connects the derivatives of the natural coordinates (r,s,t) with
the derivatives of the local coordinates (x,y,z). J = ((dx/dr dy/dr dz/dr) (dx/ds dy/ds dz/ds) (dx/dt dy/dt
dz/dt)).
Note
A good book to understand the determinant calculation is: Finite Element Procedures,
by K.J. Bathe, Prentice Hall, New Jersey 07632, 1996.
Distortion
This is available only for hexa elements and is the measurement of the twisting of the element from
the ideal shape. For this the Jacobian determinants will be calculated at r,s,t=-1,0,1 of the natural coordinate system of the element (27 node positions). The distortion is 27 times the minimum of all absolute
determinants divided by the sum of all 27 absolute determinants (0 if all Jacobian determinants are 0).
Equiangle Skewness
This quality parameter applies to tetra, hexa, quad, and tri elements.
430
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Quality
Element equiangle skew = 1.0 – max ((Qmax – Qe) / (180 – Qe), (Qe – Qmin) / Qe),
where
Qmax = largest angle in the face or element
Qmin = smallest angle in the face or element
Qe = angle of an equiangular face or element (e.g., 60 degrees for a triangle, and 90 degrees for a
square).
Eriksson Skewness
This is an empirical criterion, obtained for a hexahedral element by dividing the volume of the closest
parallelepiped by the product of its edges. It measures the shear of the parallelepiped closest to the
current element using least squares approximation. The default range of values is 0–1. Generally acceptable elements have skewness ranging from 0.5 to 1.
Ford
This is a hybrid quality parameter for 3 and 4 node (tri and quad shell) element meshes based on
weighted skewness, warpage, and aspect ratio values. It was custom developed for Ford Motor Company
to fit their established processes and metrics. The possible range is from 0 to 32.
Hex. Face Aspect Ratio
This quality parameter calculates the 3 averaged face areas (average of the areas of two opposite faces)
of hexahedra elements. The maximum of the six possible divisions of the averaged face areas will be
calculated and then inverted to normalize the result.
Hex. Face Distortion
This quality parameter calculates the product of the maximum edge size in the i direction multiplied
by maximum edge size in the j direction, multiplied by the same in the k direction, and then divides
this value by the volume of the hex element. The default range is 0–20, but if the computed range is
above 20, the Min Value will be set to zero and the Max Value will be automatically adjusted to ensure
the histogram includes all existing elements.
Max Angle
This calculates the maximum internal angle of each element. The range of values is 90–180 degrees.
Max Dihedral Angle
This is the maximum angular space contained between planes which intersect. It is measured by the
angle made by any two lines at right angles to the two planes. The range of values is 90–180 degrees.
Max Length
This calculates the maximum length of the diagonals of quad faces, and the maximum side length of
tri faces. This works for all meshes and element types. The default range is 0–20, but if the computed
range is above 20, the Min Value will be set to zero and the Max Value will be automatically adjusted
to ensure the histogram includes all existing elements.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
431
Blocking
Max Ortho
This calculates the maximum deviation of the internal angles from 90 degrees for each element. The
default range is 0–90.
Max Ortho 4.3v
This calculates the maximum deviation of the internal angles of the elements from 90 degrees. For
elements other than hexas this diagnostic is equal to Max Ortho. For hexas this differs from Max Ortho
in the way that angles between 180 and 360 degrees are also considered (deviation up to 270 degrees).
Max Ratio
This calculates the maximum ratio of the lengths of any two edges that are adjacent to a vertex in an
element. The default range is 0–20, but if the computed range is above 20, the Min Value will be set
to zero and the Max Value will be automatically adjusted to ensure the histogram includes all existing
elements.
Max Sector Volume
This option is available for volume elements. For each element node the sector volume will be calculated
in the Gauss integration points of order 3 and the maximum of the calculated sector volumes will be
taken. The default range is 0–20, but if the computed range is above 20, the Min Value will be set to
zero and the Max Value will be automatically adjusted to ensure the histogram includes all existing
elements.
Max Side
This calculates the maximum side length of each element. The default range is 0–20, but if the computed
range is above 20, the Min Value will be set to zero and the Max Value will be automatically adjusted
to ensure the histogram includes all existing elements.
Max Warp
This calculates the maximum warp (in degrees) of all elements. This works only for structured volume
and surface meshes, linear hexahedral and linear quadrahedral elements. To determine warp of a
quadrilateral face, find the midpoints of all edges, which will be co-planar. Then, calculate the maximum
angle of any edge with the plane thus defined, which is the warp of the face. The maximum warp of a
volume element or hexahedron is the maximum warp of its faces. For a 2D, planar mesh of QUAD_4
elements, the warp will be zero for all elements. The default range is 0–90 degrees.
Max Warp 4.3v
This measure applies to quad, prism and hexa elements (for quadratic elements the linear part will be
checked).
To determine the warp of a quadrilateral face, the angles between the triangles connected at the 2 diagonals of the quad will be calculated and the maximum will be used.
The maximum warp of a volume element (prism or hexa) is the maximum warp of its quad faces.
For a 2D planar mesh of QUAD_4 elements, the warp will be zero for all elements.
432
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Quality
Mid Node
This calculates the maximum deviation of the mid node. The default range is 0–1.
Mid Node Angle
This calculates the angle by which the quadratic mid node is off from the linear edge. The default range
is 0–90.
Figure 394: Definition of Mid Node Angle
Min Angle
This calculates the minimum internal angle of each element. The default range is 0–90 degrees.
Min Ortho
This calculates the minimum deviation of the internal angles from 90 degrees for each element. The
default range is 0–90.
Min Sector Volume
This option is available for volume elements. For each element node the sector volume will be calculated
in the Gauss integration points of order 3 and the minimum of the calculated sector volumes will be
taken. The default range is 0–20, but if the computed range is above 20, the Min Value will be set to
zero and the Max Value will be automatically adjusted to ensure the histogram includes all existing
elements.
Min Side
This calculates the minimum side length of each element. The default range is 0–20, but if the computed
range is above 20, the Min Value will be set to zero and the Max Value will be automatically adjusted
to ensure the histogram includes all existing elements.
Note
Use this check if you are concerned about Min Side reducing the time step. There is also a
modified Laplace smoother that can help increase these min side elements.
Opp Face Area Ratio
This is applicable for hexahedral elements only. This is the measurement of the worst ratio of the areas
of the opposite faces of the hexahedral element. Ideally, this value should be 1. The default range is
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
433
Blocking
0–20, but if the computed range is above 20, the Min Value will be set to zero and the Max Value will
be automatically adjusted to ensure the histogram includes all existing elements.
Figure 395: Definition of Opposite Face Area Ratio
In the figure above, let A1 = Area of Quad Face {ABDC}, and A2 = Area of Quad Face {EFHG}. If A1>A2,
then the Opposite Face Area Ratio of this pair of faces = A1/A2. If A1<A2, then the Opposite Face Area
Ratio = A2/A1. Similarly, the Opposite Face Area Ratio is found for each opposing pair of faces, and the
maximum of all three pairs is found as the measurement for this hexahedral element.
Opp. Face Parallelism
This feature is also for hexahedral elements only. It is the measurement of the parallelism of the hexahedral elements. If the opposite faces are ideally parallel, the value is 1. The default range is 0–20, but
if the computed range is above 20, the Min Value will be set to zero and the Max Value will be automatically adjusted to ensure the histogram includes all existing elements.
Orientation
This computes the direction of the face normal determined by the orientation of the nodes based on
the right hand rule. Face orientation should be into the volumetric domain.
Quality
The criterion Quality is calculated differently for different element types.
• Tri and Tetra
The quality is calculated as the minimum ratio of height to base length of each side (normalized
to 1).
• Quad
The quality is calculated as the Determinant, as described in Determinant (2x2x2 stencil) (p. 430).
• Hexa
The quality is a weighted diagnostic between Determinant (between -1 and 1), Max Orthogls
(normalized between -1 and 1; if deviation from orthogonality is greater than 90 degrees, then
the normalized value will be smaller than 0) and Max Warpgls (normalized between 0 and 1;
434
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Quality
warpage of 0 degrees is 1, warpage of 180 degrees is 0). The minimum of the 3 normalized diagnostics will be used.
• Pyramid
The quality is calculated as the determinant.
• Prism
The quality is calculated as the minimum of the Determinant and Warpage. Warpage is normalized
to a factor between 0 and 1, where 90 degrees is 0, and 0 degrees is 1.
Taper
For hexahedral elements, the Taper is the maximum ratio of the areas of opposite faces. For quad elements, it is the maximum ratio of the lengths of opposite edges.
Volume
This computes the volume of each element based on the corner points. The default range is 0–20, but
if the computed range is above 20, the Min Value will be set to zero and the Max Value will be automatically adjusted to ensure the histogram includes all existing elements.
Volume Change
This quality metric is calculated for a specific element by finding the maximum volume of all its neighboring elements and dividing it by the volume of the element itself. The default range is 0–20, but if
the computed range is above 20, the Min Value will be set to zero and the Max Value will be automatically adjusted to ensure the histogram includes all existing elements.
Warpage
This computes the distortion of a plane, based upon the nodes that compose the surface. The default
range is 0–90, where a warpage value of 0 is flat (preferred) while 90 is degenerate.
X Size
This computes the length of the element profile in the X direction. The default range is 0–20, but if the
computed range is above 20, the Min Value will be set to zero and the Max Value will be automatically
adjusted to ensure the histogram includes all existing elements.
Y Size
This computes the length of the element profile in the Y direction. The default range is 0–20, but if the
computed range is above 20, the Min Value will be set to zero and the Max Value will be automatically
adjusted to ensure the histogram includes all existing elements.
Z Size
This computes the length of the element profile in the Z direction. The default range is 0–20, but if the
computed range is above 20, the Min Value will be set to zero and the Max Value will be automatically
adjusted to ensure the histogram includes all existing elements.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
435
Blocking
Pre-Mesh Quality Histogram
After computing the determinant values of the elements, a histogram of the values will be displayed.
The X-axis represents the quality range for the particular type, and the Y-axis represents the number
of elements within a particular histogram bar. An arrow at the top of a histogram bar indicates that
there are more elements in that bar than are displayed per the current maximum number on the Yaxis.
By clicking on any of the bars with the left mouse button, the information about the precise number
of values that fall into this interval and its boundaries are displayed in the Messages window. Bars that
are clicked on change color, and remain selected until clicked on again. To display the elements within
a selected (highlighted) histogram bar, right click on the histogram window, and select Show.
The histogram of the Angle Quality for a certain hexahedral block is shown in Figure 396: Histogram of
Angle Quality (p. 436). The histogram options menu is also shown.
Figure 396: Histogram of Angle Quality
The histogram options are as follows:
Replot
allows you to change the parameters of the histogram using the Replot window.
Figure 397: Replot Window
Min / Max X value
sets the minimum and maximum values of the particular quality type selected for the X-axis.
Max Y height
sets the maximum number of blocks for the quality ranges. A value of 0 will set the display to such
that the histogram with the largest number of elements is fully visible. A smaller number will give
increased resolution for quality ranges with fewer elements.
Num bars
sets the number of bars to use in the histogram display.
436
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Smooth
Reset
sets the maximum number on the Y-axis such that the histogram bar with the largest number of elements
is fully visible.
Show
displays the elements within the selected (highlighted) histogram bars.
Solid
redraws all selected elements using flat shading, according to the color map.
Done
closes the histogram window.
Pre-Mesh Smooth
The Pre-Mesh Smooth option allows you to smooth the pre-mesh.
Figure 398: Pre-Mesh Smooth Options
There are three options available for smoothing blocking mesh as shown in Figure 398: Pre-Mesh Smooth
Options (p. 437).
Quality Method
Orthogonality Method
Multiblock Method
Quality Method
The following options are available for the Quality method for pre-mesh smoothing:
Smoothing iterations
specifies the number of smoothing iterations to be run.
Up to quality
specifies the quality level for smoothing. The default is 0.2.
Criterion
specifies the quality criterion for smoothing.
Determinant 3x3x3
Smoothing by Determinant 3x3x3 tries to locally improve the worst determinant of all elements
hanging on a node.
Angle
Smoothing by Angle tries to locally improve the worst angle of all elements hanging on a node.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
437
Blocking
Advanced Options
contains advanced options for smoothing.
Only visible index range
If enabled, only the elements that are in the index range set by the Index Control will be checked.
The Index Control window is accessed from the menu that appears when right clicking on Blocking
in the Display Tree.
Active parts only
If enabled, only the active parts will be smoothed.
Laplace smoothing
If enabled, performs Laplace smoothing for the surface. Laplace smoothing works on the whole mesh
and tries to create uniform transition.
Figure 399: Example of Laplace Smoothing
Original Mesh
Mesh after Laplace smoothing
438
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Smooth
Orthogonality Method
The Orthogonality method relaxes unstructured hexahedral meshes in order to obtain smooth grid lines
orthogonal to the boundary as well as smooth grid angles and transitions in the inner volume. It first
smoothes the surface mesh recognizing the topological boundary edges. If the number of volume
smoothing steps is greater than 0, after each surface smoothing step the inner volume will be adjusted
by performing 1 volume smoothing step. After the surface smoothing has been finished, the inner
volume will be smoothed (according to the number of volume steps set). It can also smooth real surface
meshes.
Note
A minimum of 10 iterations of smoothing of the surface mesh must be completed for stability
reasons.
The mathematical basis is that an elliptical differential equation of the form ∇
= , where is the
“control function”, will be solved. It can be proved that by using the elliptical operator ∇ , smoothness
of the mesh will be achieved. The control function will be specified so that the smoothed mesh will
obtain certain characteristics, such as orthogonality and layer height of the first layer.
Note
The unstructured hexahedral smoother is also available under Edit Mesh >Smooth Hexahedral Mesh Orthogonal to smooth an existing mesh.
Tips to improve smoothing success:
• Create the best possible starting condition by matching edge distributions.
• Create points (geometry) at the ends of the edges, and then associate the vertices (block) to them. This
may be used to contain an area of fine mesh along a wall, preventing it from being totally smoothed out.
The following smoothing parameters are available for the Orthogonality method:
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
439
Blocking
Number of iterations on surface
specifies the number of iterations the smoother uses to relax the surface mesh (minimum is 10). The
default number of iterations on surface is also 10.
Number of iterations on volume
specifies the number of iterations the smoother uses to additionally relax the volume mesh after surface
smoothing has been finished (minimum is 0). When the number specified is greater than 0, a volume
smoothing step will be performed after each surface smoothing step to adjust the volume mesh to the
surface mesh. The default number of iterations on volume is 5.
Smooth Type
If Orthogonality is selected, then the smoother tries to retain orthogonality and the height of the first
layer (a different height can be specified for different parts using Release Orthogonality / Initial Height
Options). If Laplace is selected, the smoother tries to equalize the mesh by setting the control function
to 0 in the elliptical differential equation.
440
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Smooth
Freeze Options
freezes the specified areas of the surface boundary. You can freeze all surface boundaries, or selected
parts. To freeze Selected Parts, select the part(s), then click Selected part(s) Options. Specify the frozen
surface boundary by enabling Surface boundary. Specify the number of layers to be frozen with the
surface boundary by disabling Surface boundary and entering the number of layers n in the Layers
field. The number of layers is set to 0 by default. When Layers is greater than 0, then the surface
boundaries including the first n layers from the boundary will be frozen. For example, a value of 3 indicates
that three layers of nodes away from the surface will be frozen along with the surface boundary.
Release Orthogonality / Initial Height Options
For certain situations, it may be helpful to release the orthogonality requirement from a certain surface
part or set the first layer distance (initial height of the first element off the wall) on certain surfaces.
These are mutually exclusive since orthogonality is required to set the first layer height. Select the desired
parts, and then click Selected part(s) Options. The default is to release orthogonality for each part. You
can set the initial height by disabling Release orthogonality and then set the initial height by entering
it in the Initial Height field.
Note
You can set the Initial Height to -1 (default) in order to keep the starting initial height.
Smooth along curves
allows you to specify which edges (projected onto curves) should be smoothed. The smoothing will be
carried out when faces are smoothed. You can specify none, all, or selected curves. The default is all.
Note
If the mesh distribution has a relatively large dynamic range of mesh sizes along a curve,
then selecting this option may be counter productive.
Advanced Options
contains the following advanced smoothing options:
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
441
Blocking
Grid expansion rate
If a smoothing method other than Laplace is selected, then the grid expansion values will be used
to distribute the control function values into the inner volume. If the grid expansion rate is greater
than 0.0, the algorithm computes a pseudo structured region in which the control function values
will be interpolated by an exponential decay (the grid expansion rate will then control the negative
exponent (e power -g) of the control function values). If it is 0.0 then a Laplace interpolation of the
control function values will be done, i.e., for an inner node, the control function value will be averaged
by the control function values of its neighbor nodes.
442
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Smooth
The default values are 0.0 for the surface mesh and for the inner volume. Reasonable values
other than 0.0 should be greater than 1.0.
Note
It may be difficult to form the pseudo structured regions in some cases. If you have
such problems, set the grid expansion rate back to 0.
Note
If the grid expansion rate is set to 0.0 and the smooth type is set to Orthogonality,
the first layer height and the orthogonality at the boundary are still achieved, but
the next layers tend towards Laplace approaching the middle of the mesh. In case
of a Navier- Stokes mesh you can see the effect near the boundary where the first
layer is orthogonal to the boundary but the next layers curve as they equalize (Laplace)
the distances of the layer nodes.
Treat unstruct nodes
determines the method of treating inner unstructured nodes. An unstructured node is a node on
which no ij (surface) or ijk (volume) directions can be defined, e.g. a node which has more or less
than 4 (surface) or 6 (volume) neighbors is clearly an unstructured node.
Note
For most models, the effect of the this setting may be negligible.
Stabilization Factor
is used in the calculation of the new nodes and should be greater or equal to 1.0. A higher factor
will make the smoother more stable at the cost of orthogonality at the boundaries. If there are
problems with the smoother it is recommended to increase this value (to around 8.0). Default values
are 1.0 on surfaces and 2.0 in the volume. Increasing this parameter may be helpful on certain
model configurations if the smoother corrupts the mesh, especially if it appears due to overly orthogonal boundaries.
Use Orthogonal Distance
if enabled, then the original boundary distance of a first layer node will be calculated by projecting
it to the boundary and measuring the distance to the projected point. Otherwise, the length of the
original grid line will be used. By default this option is disabled for both the surface and volume.
In cases where there is a sharp angle between the grid lines from the first layer to the boundary,
if Use Orthogonal Distance has not been set, the calculated first layer distance may be considerably greater than the distance of the first layer nodes to the boundary (because the length
of the grid line will be used). Hence, it may be advisable to set Use Orthogonal Distance in
the same way for both Surface and Volume. This would ensure that the first layer grid line
angles in the volume near the surface boundary would be similar to the nearby surface
boundary grid line angles.
Define Edges On Part Border Options
allows you to define the border grid lines attached to the selected parts as edges, and the node
distribution on the edges will be frozen. The main purpose for defining these edges is that they
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
443
Blocking
separate the two sides of the surface mesh. If an edge is topologically internal then orthogonality
will not be established there.
Surface Fitting
constrains boundary nodes to the true geometry surfaces. When disabled, the original quad faces
are used to determine the boundary constraints. This option is enabled by default.
Keep periodic geometry
when enabled, allows you retain original dimensions on periodic faces. With this option disabled,
point projected nodes may be moved on the corresponding surfaces during smoothing with the
orthogonal smoother. This option is enabled by default.
Active parts only
if enabled, only the active parts (parts that are turned on (activated) in the Parts branch of the display
tree, see the Parts (p. 180) section) will be smoothed. The geometry or mesh of the active parts does
not need to be displayed. When this option is disabled, the whole mesh will be smoothed. This option
is disabled by default.
Multiblock Method
The Multiblock method is used to smooth multiblock mesh. This smoother works on the base of the
(structured) blocks of the pre-mesh.
The Multiblock smoother is used to obtain smooth grid lines. It is specially optimized for blade configurations. The mathematical basis is that an elliptical differential equation of the form ∇
= , where
is the “control function”, will be solved. It can be proved that by using the elliptical operator ∇ ,
smoothness of the mesh will be achieved. The control function will be specified so that the smoothed
mesh will obtain certain characteristics, such as orthogonality and layer height of the first layer.
The following parameters are available for this method.
Relaxation Block(s)
allows you to select/deselect blocks. Click on the appropriate selection icon to select or deselect blocks.
Block Display Off
if enabled, the selected blocks will not be displayed on the screen.
Smoothing Direction
3D Direction
smoothes all the blocks of the pre-mesh independently.
Select direction
allows you to select the smoothing direction.
Reference Edge
specifies the edge defining the smoothing direction. To select the smoothing direction click on
the Edge selection icon. A block will be highlighted in the display. Click on the edge that defines
the desired smoothing direction.
If I, J, or K is selected, and no Global vertices are selected, then the blocks of the pre-mesh
will be smoothed in planes starting and ending at the indices specified, and with the increment specified. The planes in between will be interpolated and smoothed, if Volume itera-
444
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Smooth
tions is set greater than 0. If directions I, J, or K is selected, and the Global Vertices option
is selected, then the pre-mesh will be smoothed globally over selected edges defined by its
end vertices, in planes starting and ending at the indices specified, and with the increment
specified. The planes in between will be interpolated and smoothed, if Volume iterations
is set greater than 0.
For example, if you select a smoothing direction I, Start Index = 1, End Index = 20, and
Increment = 5, the nodes on the planes I = 1, 6, 11, 16, and 20 would be smoothed with
the remaining nodes interpolated. It is also possible to define a list of planes by specifying
the plane numbers separated by spaces in the Planes field. In this case the plane numbers
have higher priority than the Start and End Index fields.
Note
To identify planes, use the Blocking Display Tree > Pre-Mesh > Scan Planes
function.
Auto Setup
When Auto Setup is selected, all subfaces which fulfill the following conditions will be selected as NonRelaxation Faces and Hold Cell Height Faces:
• Subfaces that belong to the selected blocks.
• Subfaces that are not perpendicular to the selected smoothing direction.
• Boundary subfaces with respect to the selected blocks. For example, they cannot be block interfaces
between two selected blocks.
• Subfaces that are not periodic.
Additionally, all vertices which are connected to the selected blocks will be defined as Global Vertices.
Layer Options
These options allow you to select layer options when smoothing.
Start Layer
is the index plane in smoothing direction at which the smoothing should start. The value should be
between 1 and less than or equal to the maximum index. If plane numbers have been set under
Planes then this field will not be used.
End Layer
is the index plane in smoothing direction at which the smoothing should end. The value should be
between 1 and less than or equal to the maximum index. If plane numbers have been set under
Planes then this field will not be used.
Increment
specifies the increment to smooth the planes between the Start and End Layers. The nodes will be
interpolated in between the layers.
Volume iterations
if set to greater than, 0 then only the nodes between the planes selected for smoothing will be
smoothed with this number of iterations after interpolation.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
445
Blocking
Planes
specifies the index planes in the smoothing direction for smoothing. The values should be between
1 and less than or equal to the maximum index, and should be separated by blanks. If specified then
it will overwrite the values for Start and End Layer, and Increment.
Face Options
allows you to choose from the following options for selected subfaces:
Non-Relaxation Faces
freezes subfaces.
Hold Cell Height Faces
orthogonality and first cell height will be obtained on all grid lines perpendicular to the selected
subfaces.
Face Display Off
if enabled, then the selected faces will not be displayed.
Face Icons
enables the display of the selected faces by icon. Otherwise the selected faces will be shown in solid
display, at 90% of their full size.
Face Filters
allows you to filter the selected faces using the Use All Selected Faces, Use Only Block Interfaces,
and Use Only Boundaries options.
Remove periodic faces
if enabled, the periodic faces will be removed from the selection.
Select or deselect faces by clicking on the appropriate selection icon.
Vertices Options
Global Vertices
If any end vertices of a block edge have been selected, and a smoothing direction is selected, then
the pre-mesh will be smoothed globally in planes. It is recommended to select all vertices as Global
Vertices and to freeze the real (not periodic) boundaries.
Layer Vertices
This option is intended to be used for O-grid vertices. For neighbor nodes, the bisector will be calculated placing the neighbor nodes on the bisector line in a distance specified as the First Layer Distance. If the First Layer Distance is smaller than 0.0, the selected vertices will not be used. Vertices
can be added or removed from the selection list, and the First Layer Distance can be changed for
the selected vertices.
Layer Vertices are only used in global edge smoothing. To access this option, a smoothing
direction must have been selected.
Vertices Display Off
if enabled, the selected global or layer vertices will not be displayed.
Select or deselect vertices by clicking on the appropriate icon.
Clear all selections
resets all selections.
446
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Pre-Mesh Smooth
Advanced Options
contains the following advanced options:
Number of Iterations / Steps
Iterations in equation solver
specifies the number of iterations for the equation solver (default is 25). An equation solver (SOR
method) is used to solve the elliptic equation method.
Steps in global edge smoothing
specifies the number of smoothing steps in the global-edge smoothing method. In each step
the Pre-Mesh will be smoothed globally and the output will be used as input in the next step
(default is 25).
Parameters
Projection limit
is useful for near-wall layers. This parameter is used for node distribution whose first spacing
from the surface is less than the geometry tolerance. A value greater than 0.0 will define a distance
normal to the surface up to which the nodes will be interpolated. A single value of projection
limit is used at all locations on the model.
Relaxation factor
is a factor to stabilize the smoothing value. Reasonable values should be between 0.0 (exclusive)
and 1.0 (inclusive). The default value is 0.5.
Residual factor
is used during global edge smoothing. Starting from the 2nd global edge step, the average
change compared to the previous step will be calculated by dividing this value by the value
calculated in the 2nd step. If this relative value gets lower than the Residual factor, a stop criterion
has been reached. The default value is 0.05.
Surface fitting
constrains boundary nodes to the true geometry surfaces. With this option disabled, the
boundary nodes will be projected to the triangulation of the geometry surfaces.
Use projection
enables smoothing steps to be performed, allowing nodes to move away from constraints (curves,
surfaces), and then the nodes are finally projected back to the curve or surface. By default, this
option is disabled.
Use orthogonal positioning
is used during global edge smoothing or plane smoothing. If Hold Cell Height has been set on
a subface, a special method will be used to calculate the control function values in a way that
the first layer nodes will be placed to hold the original or user defined (layer vertices) cell height
and to be orthogonal (bisector) to the boundary. By default, this option is enabled.
Use fractional positioning
is used during global edge smoothing or plane smoothing. If Use orthogonal positioning has
been set, the first layer nodes will not be moved in one step to the orthogonal position but in
a certain amount of steps (10). This is mainly to stabilize the orthogonal positioning algorithm
in highly clustered meshes. By default, this option is disabled.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
447
Blocking
Methods
In the structured smoother, several elliptic relaxation methods are available both for the volume and
faces (subface boundaries). The default method is Sorenson - Laplace. In the case of global edge
smoothing, this parameter is not relevant.
• Sorenson-Laplace
Sorenson methods attempt to maintain node distributions (bunching) near the surface
boundaries while improving orthogonality. This hybrid method attempts to improve orthogonality at the boundary while maintaining the first layer height from the boundary surface
and making a uniform node distribution in the interior
• Sorenson-Thomas & Middlecoff
This method improves orthogonality at the boundary while maintaining the first layer height
from the boundary surface and holding the original clustering on the interior.
• Thomas & Middlecoff
This method generally improves the orthogonality of grid lines across boundaries while
holding the original clustering in the interior.
• Laplace
This method attempts to give a uniform mesh size for all selected elements or to give a uniform
transition.
• Interpolation
This uses an algebraic transfinite interpolation method with Soni interpolants to generally
improve internal angles.
• Hilgenstock - Thomas & Middlecoff
Hilgenstock methods maintain orthogonality. This hybrid method maintains orthogonality
between block boundaries (subfaces) to give a smooth transition across subfaces, while
maintaining the first layer height from the boundary surface.
• Hilgenstock - Laplace
This attempts to improve orthogonality and uniform node distribution within the mesh.
Grid expansion rate
is the exponent for the exponential decay of Sorenson terms from the boundary to the interior of a
face. Reducing this factor will cluster the elements closer to the boundary. Default values are 3.5 for
faces and 4.6 for the volume.
Multiblock Settings
Load Settings
allows you to load previously saved Multiblock settings.
Save Settings
allows you to save the current Multiblock settings in a file.
448
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Delete Block
Run in sequence
allows you to load different Multiblock settings files and run them in sequence. Click Start sequence
to begin running the sequence of files.
Convert old settings
allows you to convert Multiblock settings which were created with the ANSYS ICEM CFD 4.3 version.
Convert file
specifies the old settings file.
Save as file
specifies the new settings file.
Convert
starts the conversion.
Block Checks
The Block Checks option allows you to check the blocks. The following methods are available for
checking/fixing blocks:
Run Check/Fix
checks the internal data structures for inconsistencies and fixes them if possible.
Fix Inverted Block
fixes all the Inverted blocks. Inverted blocks have a negative determinant.
Invert Selected Block Method
inverts the selected blocks.
Pack Block Numbers
automatically renumbers all blocks in sequential order. This is to avoid very large block numbers
that can result after repeated block editing and VORFN rebuilds.
Delete Block
The Delete Block option allows you to delete the blocks from the topology. The Delete permanently
option is disabled by default.
If Delete permanently is disabled, the block will be moved to the VORFN part. The VORFN part is essentially dormant and mesh is not computed for it, however it does help to maintain connectivity.
Blocks can be retrieved from the VORFN region using the Add Blocks to Part option.
If Delete permanently is enabled, the block will be permanently deleted. At this point connectivity
will be broken and the VORFN region will be rebuilt. This can be useful in some situations, but this will
also result in a re-indexing of the blocking. The resulting index structure is usually more complicated
and may be more difficult to work with.
Figure 400: Example of Delete Blocks Permanently
Note that there are an equal number of nodes across the hole.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
449
Blocking
Block selected to be deleted.
After the block is deleted permanently, the edges on opposite sides of the hole are no longer connected
by a VORFN block and it is possible to adjust the edge distributions separately.
450
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Edit Mesh
Figure 401: Edit Mesh Toolbar
The Edit Mesh menu contains all of the operations necessary to manipulate, check, improve the quality
of the mesh and fix any problems.
Create Elements
Extrude Mesh
Check Mesh
Display Mesh Quality
Smooth Mesh Globally
Smooth Multiblock Domains Globally
Smooth Hexahedral Mesh Orthogonal
Repair Mesh
Merge Nodes
Split Mesh
Move Nodes
Transform Mesh
Convert Mesh Type
Adjust Mesh Density
Renumber Mesh
Assign Mesh Thickness
Reorient Mesh
Delete Nodes
Delete Elements
Edit Distributed Attribute
Note
Within this menu, only the mesh elements and nodes can be checked or manipulated. You
cannot manipulate or check faceted data such as STL or Nastran that represents geometry.
Editing this type of data can be done in the Geometry menu.
Create Elements
The Create Elements option is used for manually creating different element types. Generally, to
improve some bad elements or to get rid of some problems/errors in the mesh, some elements are
deleted and good quality elements are created manually. For example, a bad quad element can be
represented by two good tri elements.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
451
Edit Mesh
Figure 402: Create Elements Options
Part
Select or enter a part name. The new elements created will go into this part.
The different options for creating elements are described in the following sections.
Node (Point Element)
Bar (Line Element)
Triangle
Quad
Tetra
Prism
Pyramid
Hexa
Auto Element Type
Node (Point Element)
The Node (Point Element) option creates a node element. You need to select a particular position
where a new node (point) should be created.
Note
This does not refer to nodes that define mesh elements, but an actual zero dimension
element that is typically at an existing mesh node location. These node elements are
commonly used for applying loads, constraints, and other boundary conditions.
Method
From nodes
allows you to select the nodes of the mesh to define new elements. A mesh must be currently loaded
so that nodes can be selected.
From points
allows you to select the points of the geometry to define new elements. A geometry file must be
loaded so that points can be selected.
From screen
allows you to select any arbitrary location by clicking on the screen.
452
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Elements
Automatic element creation
automatically creates the element after selecting the point, node, or edge, without requiring confirmation
by pressing the middle mouse button.
Bar (Line Element)
The Bar (Line Element) option allows you to select two locations to specify a bar (line) element.
It is possible to select existing nodes, points, or arbitrary locations on the screen.
Method
From nodes
allows you to select the nodes of the mesh to define new elements. A mesh must be currently loaded
so that nodes can be selected.
From points
allows you to select the points of the geometry to define new elements. A geometry file must be
loaded so that points can be selected.
From screen
allows you to select any arbitrary location by clicking on the screen.
From elements
allows you to select any element(s) and line elements will be created for each edge of the element(s).
Inherit parts
if enabled, the created line elements will be added to the same part as the original elements.
Otherwise, the line elements will be added to the part specified in the Part field.
From edges
allows you to select elements to define new line elements from their edges.
From curves
allows you to select a curve to define a new line element.
Automatic element creation
automatically creates the element after selecting the point, node, or edge, without requiring confirmation
by pressing the middle mouse button.
Triangle
The Triangle option allows you to select three locations to create a triangle. A triangular element
is a surface element. If not possible, a message will be displayed that it could not create the triangle
because the volume mesh could not be made consistent.
Method
From nodes
allows you to elect the nodes of the mesh to define new elements. A mesh must be currently loaded
so that nodes can be selected.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
453
Edit Mesh
From points
allows you to select the points of the geometry to define new elements. A geometry file must be
loaded so that points can be selected.
From screen
allows you to select any arbitrary location by clicking on the screen.
Make Volume Consistent
automatically adjusts the volumetric elements to conform with the new element(s). This only applies
when creating triangles within a tetra mesh.
Automatic element creation
automatically creates the element after selecting the point, node, or edge, without requiring confirmation
by pressing the middle mouse button.
Quad
The Quad options allows you to select four locations to specify a quad element. A quadrilateral
element is a surface element. It is possible to select existing nodes, points, or arbitrary locations on the
screen. Select in a clockwise or counterclockwise order unless Automatic vertex distribution is enabled
(see below).
Method
From nodes
allows you to select the nodes of the mesh to define new elements. A mesh must be currently loaded
so that nodes can be selected.
From points
allows you to select the points of the geometry to define new elements. A geometry file must be
loaded so that points can be selected.
From screen
allows you to select any arbitrary location by clicking on the screen.
Make Volume Consistent
automatically adjusts the volumetric elements to conform with the new element(s). This applies when
creating quads within a tetra mesh. Pyramids will be created to maintain node connectivity.
Automatic vertex distribution
For quad and hexa elements, if this option is enabled, the order of selection of nodes is disregarded,
and selected nodes will be automatically reordered to avoid creating a skewed element.
454
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Elements
Figure 403: Example of Automatic Vertex Distribution option
Automatic Vertex Distribution disabled
Automatic Vertex Distribution enabled
If the nodes were selected in the order
notated, a skewed element is created.
Although the nodes were selected in the
same order as above, a good quality quad
element is created.
Automatic element creation
automatically creates the element after selecting the point, node, or edge, without requiring confirmation
by pressing the middle mouse button.
Tetra
The Tetra option allows you to select four locations in any order to create a tetra element. A tetrahedral element has four tri faces.
Method
From nodes
allows you to select the nodes of the mesh to define new elements. A mesh must be currently loaded
so that nodes can be selected.
From points
allows you to select the points of the geometry to define new elements. A geometry file must be
loaded so that points can be selected.
From screen
allows you to select any arbitrary location by clicking on the screen.
Automatic element creation
automatically creates the element after selecting the point, node, or edge, without requiring confirmation
by pressing the middle mouse button.
Prism
The Prism option allows you to select six total locations to create a prism element. A prism element
has two tri faces and three quad faces. Select the three locations of one face, then the three locations
for the other face in the same order.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
455
Edit Mesh
Method
From nodes
allows you to select the nodes of the mesh to define new elements. A mesh must be currently loaded
so that nodes can be selected.
From points
allows you to select the points of the geometry to define new elements. A geometry file must be
loaded so that points can be selected.
From screen
allows you to select any arbitrary location by clicking on the screen.
Automatic element creation
automatically creates the element after selecting the point, node, or edge, without requiring confirmation
by pressing the middle mouse button.
Pyramid
The Pyramid option allows you to select five locations to create a pyramid element. A pyramid
element has four tri faces and one quad face. Select four locations of the base quad face first in a
clockwise or counterclockwise order, then one location for the apex.
Method
From nodes
allows you to select the nodes of the mesh to define new elements. A mesh must be currently loaded
so that nodes can be selected.
From points
allows you to select the points of the geometry to define new elements. A geometry file must be
loaded so that points can be selected.
From screen
allows you to select any arbitrary location by clicking on the screen.
Automatic element creation
automatically creates the element after selecting the point, node, or edge, without requiring confirmation
by pressing the middle mouse button.
Hexa
The Hexa option allows you to select eight locations to create a hexa element. A hexahedral element
has six quad faces. Select four vertices in a clockwise or counterclockwise order for one face, then four
more in the same order for the opposing face. You can also select the two opposing faces.
Method
From nodes
allows you to select the nodes of the mesh to define new elements. A mesh file must be loaded so
that nodes can be selected.
456
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Elements
From points
allows you to select the points of the geometry to define new elements. A geometry file must be
loaded so that points can be selected.
From screen
allows you to select any arbitrary location by clicking on the screen.
From Faces
allows you to select the two opposing faces to define the hexa element.
Automatic vertex distribution
For quad and hexa elements, if this option is enabled, the selected nodes will be automatically distributed
to create the best element.
Automatic element creation
automatically creates the element after selecting the point, node, or edge, without requiring confirmation
by pressing the middle mouse button.
Auto Element Type
The Auto Element Type option allows you to create elements based on the number of vertices
selected. Select any number of 1-8 vertices. Press the middle mouse button to create an element type.
Number of vertices selected
Element created
1
Node element
2
Bar (line) element
3
Tri element
4
Tetra element (if volume mesh is loaded), or Quad element (if pure
surface mesh is loaded)
5
Pyramid element
6
Prism element
7
(not supported)
8
Hexa element
Method
From nodes
allows you to select the nodes of the mesh to define new elements. A mesh must be currently loaded
so that nodes can be selected.
From points
allows you to select the points of the geometry to define new elements. A geometry file must be
loaded so that points can be selected.
From screen
allows you to select any arbitrary location by clicking on the screen.
Make Volume Consistent
Automatically adjusts the volumetric elements to conform with the new element(s).
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
457
Edit Mesh
Automatic vertex distribution
For quad and hexa elements, if this option is enabled, the order of selection of nodes is disregarded,
and selected nodes will be automatically reordered to avoid creating a skewed element.
Extrude Mesh
The Extrude Mesh option allows you to create elements of one type from selected elements of
a lower dimension along a defined direction. This option is generally used to create a volume mesh of
non-varying cross-section from a 2D mesh profile.
Type of original elements
Type of extruded elements
Node
Bar
Bar
Quad
Tri / Quad
Prism / Hexa
The following options are common to each available method:
Elements
allows you to select the elements to be extruded.
New volume part name
specifies the part to which the new elements created during extrusion will belong.
New side part name
specifies the part to which shell elements created at the sides of the extrusion will belong.
New top part name
specifies the part to which shell elements created at the top of the extrusion will belong.
Method
The Extrude Mesh > Method is chosen from the drop down list. The options are explained in
subsequent sections.
Delete options
If Delete original elements is enabled, the original elements selected for the extrusion will be deleted
from the mesh.
If the additional option No uncovered faces after delete is enabled, then the original elements
will only be deleted if no new uncovered faces will be created.
Extrude by Element Normal
This method of extrusion will extrude the mesh along the normal of existing mesh elements. If the
normals of all the elements are not aligned in one direction, then you need to make all element normals
consistent before extrusion (Edit Mesh > Reorient Mesh > Reorient Consistent).
Number of Layers
specifies the number of layers to be extruded. By default it extrudes one layer.
458
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Extrude Mesh
Reverse direction
when enabled, elements will be extruded in the reverse direction of the normals of existing mesh elements.
Note
The direction of the element normals will not be changed.
Spacing type
determines the height of each layer. A Fixed spacing will make each layer that same height. Spacing
can also be defined by a Function of the layer variable, using Tcl syntax. See www.scriptics.com for descriptions of Tcl syntax for different mathematical expressions.
For example, Spacing can be defined as 0.3*layer. Then the mesh will be extruded along the defined
vector, with the first layer height as 0.3, the second layer height as 0.6, etc.
Spacing can also be defined by a function of geometric growth as follows:
height1 * pow (ratio1, layer-1),
where height1 is the height of the first layer, pow is the expression for an exponent, and ratio1 is
the growth factor.
Extrude Along Curve
This method allows you to o extrude mesh along a curve which defines variable direction. By default,
the orientation of each layer will be perpendicular to the curve.
Extrude curve
specifies the existing curve along which elements should be extruded.
Show curve directions
if enabled, an arrow indicating the direction of the selected curve will be displayed.
Orient axially
The orientation of each extruded layer of elements will be the same as that of the original layer of elements.
Figure 404: Extrusion Orientation
By default, the orientation of the extruded layers will be perpendicular to the curve.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
459
Edit Mesh
If Orient Axially is enabled, the orientation of the extruded layers will be the same
as the original layer of elements.
Reverse curve direction
allows you to extrude elements in the opposite direction to the curve direction (parametric).
Project to Geometry
if enabled, then all new boundary nodes will be projected to surfaces. The last layer of new nodes will
have the same projection type as the original nodes.
Number of layers
specifies the number of layers to be extruded. By default it extrudes one layer.
Twist per layer
specifies the number of degrees for the elements to be rotated per layer. This is used for helical extrusions.
Spacing type
You can choose a Fixed spacing for each element or Curve bunching, which will use the Spacing and
Bunching law parameters that are specified for the Curve Mesh Size.
Extrude by Vector
This method allows you to extrude elements in a linear direction defined by a vector.
Direction
Choose the Method using the radio buttons.
Explicit Vector
specifies the X Y Z vector components of the vector, based on the active coordinate system. For
example, “0 0 1” will extrude in the Z direction.
Vector by points
Define a vector by selecting two points. Elements will be moved in the direction of the defined
vector.
Number of Layers
specifies the number of layers to be extruded. By default it extrudes one layer.
Spacing type
determines the height of each layer. A Fixed spacing will make each layer that same height. Spacing
can also be defined by a Function of the layer variable, using Tcl syntax. See www.scriptics.com for descriptions of Tcl syntax for different mathematical expressions.
460
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Extrude Mesh
For example, Spacing can be defined as 0.3*layer. Then the mesh will be extruded along the defined
vector, with the first layer height as 0.3, the second layer height as 0.6, etc.
Spacing can also be defined by a function of geometric growth as follows:
height1 * pow (ratio1, layer-1),
where height1 is the height of the first layer, pow is the expression for an exponent, and ratio1 is
the growth factor.
Extrude by Rotation
This method allows you to extrude elements by rotating them about an axis or vector.
Axis
specifies the axis or a vector to indicate the direction of rotation, or the axis to which the normal of the
element is aligned.
Center of Rotation
allows you to select the origin or another point as the center of rotation.
Translate
If enabled, the extruded mesh will include both translational and rotational extrusion.
Spacing
The fixed height of each extruded layer.
Direction
Choose the Method using the radio buttons.
Explicit Vector
specifies the X Y Z vector components of the vector, based on the active coordinate system. For
example, “0 0 1” will extrude in the Z direction.
Vector by points
Define a vector by selecting two points. Elements will be moved in the direction of the defined
vector.
Angle per layer
Angle of each layer of rotation.
Number of Layers
specifies the number of layers of the existing mesh for extrusion.
Merge Degenerated Elements
if enabled will merge all nodes on or near the axis of rotation within the defined Degeneration tolerance
(the default is 0.00001). For example, degenerate hexas with one degenerate face on the axis (two sets
of coincident nodes) will become prisms with one edge on the axis (two nodes).
Degeneration tolerance
If Merge Degenerated Elements is enabled, then this tolerance can be specified (default is 0.00001).
This tolerance is used to find equal nodes in degenerated elements by using it as a ratio between the
current node distance and the maximum distance of all nodes in the element.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
461
Edit Mesh
Check Mesh
The Check Mesh option allows you to locate problems with the mesh that will usually lead to
failure when translating or running the solution. Errors will most likely result in failure to write out the
mesh or read it into the solver. Possible Problems may lead to solution crashing or diversion. You can
select any combination of Errors and Possible Problems to check at one time.
The following options are available:
Set Defaults
enables the default mesh check options.
Elements to Check
You can select All to check the full mesh or select Active to check mesh from the active parts only.
Check Mode
The Create Subsets option will put all problematic elements in respective subsets, visually isolating
them for manual editing. The Check/fix each option will attempt to automatically fix those problems
that can be repaired. After each diagnostic check, you will be asked to respond to each problem found.
If the model is very large, each check could take some time.
Interrupt
On the status bar that appears when Check Mesh is running, you can choose to interrupt the operation.
The check that is currently running will be finished and the rest will be skipped.
Errors
Duplicate element
locates elements that share all of their nodes with another element of the same type. Duplicate elements
should not exist in an ideal mesh.
Note
The deleting of elements during the automatic fix will remove one of the two duplicate
elements, thus eliminating this error without creating a hole in the geometry.
Uncovered faces
For a 3D mesh, all faces on a volumetric element should either be attached to the face of another volumetric element or to a surface element. This function finds the volume elements that violate this restriction.
Usually this indicates a hole in the surface mesh. In the case of a 2D mesh, this function finds edges of
mesh elements that are not connected to another element or not capped off by a bar (line) element at
the perimeter (single or open edges).
The automatic fix will cover these uncovered faces with triangles (surface mesh). This may or may
not be the proper solution. A better method may be to first select the flawed elements and then
decide if the uncovered faces are the result of missing surface mesh or the result of a hole. If it is
due to missing surface mesh, rerun the check and choose the Fix option. If the error points out a
hole in the model, you can attempt to correct the mesh by manually creating elements or merging
nodes.
462
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Check Mesh
Missing internal faces
Between every two adjacent volume elements that are in different parts there should be a surface element.
This function finds the volume elements that violate this restriction. A mesh with only one volume part
will not have missing internal faces. For 2D meshes, this function finds two adjacent surface elements
in different parts with no line element between them. The automatic fix will create surface or line elements
between these elements.
Periodic problems
checks surface parts that have periodic faces for inconsistency in the periodicity of the nodes. Errors are
reported if periodic matches are missing. Slight offsets in node positions are often repaired automatically
during the check process. Remaining errors can be repaired manually using Edit Mesh > Repair Mesh >
Make/Remove Periodic.
Volume orientations
finds elements where the order of the nodes does not define a right-handed element.
Note
This will be automatically corrected when Check/Fix is run.
Surface orientations
checks for volume elements that share the same surface element. In doing this check, it is required to
also check for:
• uncovered faces
• missing internal faces
• duplicate elements
This check will not find elements that occupy the same volume but are attached to regions of mesh
that are not connected.
Hanging elements
checks for line elements that have one node connected to surface mesh, and the other node free (unconnected).
Penetrating elements
checks for surface elements that intersect or pass through other surface elements.
Disconnected bar elements
checks for bar elements with both nodes unconnected.
Possible Problems
Multiple edges
refers to elements with at least one edge shared among three or more elements. Legitimate multiple
edges would be found at a "T" junction, where more than two geometry surfaces meet.
Triangle boxes
refers to groups of four triangles that form a tetrahedron with no volume element inside. This is best
fixed by merging two of the nodes that would collapse the unwanted triangle box.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
463
Edit Mesh
2 single edges
refers to elements with two single edges. These are either corners of baffles or are triangles that are
protruding from a surface and are thus undesirable in the mesh.
Single-multiple edges
refers to elements that have both single and multiple edges. These elements are probably not wanted.
Stand-alone surface mesh
refers to surface elements that do not share a face with a volumetric element. This could be an area
with an extra surface element to be deleted or a missing volume element to be created.
Single edges
refers to surface elements with at least one edge that is not shared with any other surface element. This
would represent a hanging edge, and the element would be an internal baffle. These may or may not
be legitimate. Legitimate single edges would exist where the geometry has a zero thickness baffle with
a free or hanging edge.
Delaunay violation
refers to tri elements with nodes that are within the circumsphere of adjacent elements. These can often
be removed by swapping edges of these triangles.
Overlapping elements
refers to surface elements that occupy part of the same surface area, but do not have the same nodes.
This could be surface mesh that folds on to itself. This will also find elements that are at an angle of up
to 5 degrees from overlapping each other, as shown in Figure 405: Example of Overlapping Element (p. 464).
Figure 405: Example of Overlapping Element
Non-manifold vertices
refers to vertices whose adjacent elements outer edges do not form a closed loop. Usually indicates
elements that jump from one surface to another, forming a "tent like" structure. This would usually pose
no problem for mesh quality but will represent a barrier in the free domain that probably should not
be there. See the figure in Edit Mesh > Split Mesh.
Unconnected vertices
refers to vertices that are not connected to any element. These are usually eliminated automatically
upon saving the mesh.
464
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Display Mesh Quality
Display Mesh Quality
The Display Mesh Quality option runs a diagnostic check of individual element quality. Mesh
Quality can be displayed by a histogram. refer to the Quality Histogram section.
Mesh types to check
allows you to select the mesh types to check with a selected Quality criterion. For large 3D grids,
you may want to disable the check for surface elements.
Elements to check
allows you to select the mesh elements to be checked.
• All
checks all elements.
• Active parts
checks all elements in active parts.
• Visible subsets
checks elements in visible subsets only.
• Visible subsets and active parts
checks elements in visible subsets and active parts.
Quality type
specifies the Quality criterion selected from the drop-down menu.
Refresh Histogram
refreshes the histogram displayed.
The mesh quality criteria available are described in the following sections:
Quality
Aspect Ratio
Aspect Ratio (Fluent)
Custom Quality
Determinant
Distortion
Element Stretch
Equiangle Skewness
Ford
Hex. Face Aspect Ratio
Hex. Face Distortion
Max Angle
Min Angle
Max Dihedral Angle
Max Length
Max Ortho
Min Ortho
Max Orthogls
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
465
Edit Mesh
Max Ratio
Max Sector Volume
Min Sector Volume
Max Side
Min Side
Min Side (Quad Optimized)
Max Warp
Max Warpgls
Mesh Distribution
Mesh Expansion Factor
Mid Node
Mid Node Angle
Opp Face Area Ratio
Opp Face Parallelism
Orientation
Orthogonal Quality
Prism Thickness
Quadratic Dev
Skew
TGrid Skew
Surface Area
Surface Dev
Taper
Tetra Special
Volume
Volume Change
Volume/Area/Length
Workbench Shape
X Size
Y Size
Z Size
Quality Metric Histogram
Quality
The criterion Quality is calculated differently for different element types:
• Tri
The quality is calculated as the aspect ratio of the tri element as described in Aspect Ratio (p. 467).
• Tetra
The quality is calculated as the aspect ratio of the tetra element as described in Aspect Ratio (p. 467).
• Quad
The quality is calculated as the Determinant, as described in Determinant (p. 470).
• Hexa
The quality is a weighted diagnostic between Determinant (between -1 and 1), Max Orthogls
(normalized between -1 and 1; if deviation from orthogonality is greater than 90 degrees, then
466
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Display Mesh Quality
the normalized value will be smaller than 0) and Max Warpgls (normalized between 0 and 1;
warpage of 0 degrees is 1, warpage of 180 degrees is 0). The minimum of the 3 normalized diagnostics will be used.
• Pyramid
The quality is calculated as the determinant.
• Prism
The quality is calculated as the minimum of the Determinant and Warpage. Warpage is normalized
to a factor between 0 to 1, where 90 degrees is 0, and 0 degrees is 1.
Aspect Ratio
The criterion Aspect Ratio is calculated differently for different element types:
• Quad
The vectors for each of the 4 quad nodes span a parallelogram. The area of each parallelogram is
divided by the length of each component vector squared, to give 8 possible aspect ratios. The minimum ratio is taken as the aspect ratio for the quad element.
Figure 406: Aspect Ratio for Quad Elements
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
467
Edit Mesh
• Hexa
The aspect ratio is defined by the size of the minimum element edge divided by the size of the
maximum element edge. Quadratic hexahedras will also be considered.
• Tri
ANSYS ICEM CFD calculates the ratio between the area of triangle and the maximum edge length
for each element. The values are scaled, so that an aspect ratio of 1 corresponds to a perfectly regular
element, while an aspect ratio of 0 indicates that the element has zero area.
Aspect Ratio = (area/max edge length)actual / (area/max edge length)ideal
Figure 407: Aspect Ratio of Tri Elements–Examples
• Tetra
ANSYS ICEM CFD calculates the ratio between the volume of the element and the radius of its circumscribed sphere power three. The values are scaled, so that an aspect ratio of 1 corresponds to a
perfectly regular element, while an aspect ratio of 0 indicates that the element has zero volume.
Aspect Ratio = (volume/(circumscribed radius)3)actual / (volume/(circumscribed radius)3)ideal
468
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Display Mesh Quality
Figure 408: Aspect Ratio of Tetra Elements–Examples
Aspect Ratio (Fluent)
This is an alternative aspect ratio computation (as used in ANSYS Fluent). In this case, it is computed
as the ratio of the maximum value to the minimum value of any of the following distances: the normal
distances between the cell centroid and face centroids computed as a dot product of the distance
vector and the face normal, and the distances between the cell centroid and nodes. For a unit cube
(see Figure 409: Calculating the Aspect Ratio for a Unit Cube (p. 470)), the maximum distance is 0.866,
and the minimum distance is 0.5, so the aspect ratio is 1.732. This type of definition can be applied on
any type of mesh, including polyhedral.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
469
Edit Mesh
Figure 409: Calculating the Aspect Ratio for a Unit Cube
Custom Quality
This option allows you to define your own quality metric as the combination of the following quality
criteria and element types: Determinant, Warp, Min Angle, and Max Angle.
You can specify the maximum and minimum quality levels of a histogram for quad and tri elements.
All values are adjusted to a scale of 0 to 1 when Recompute is pressed.
For example, if the Min Angle Quad is 30 degrees and the maximum is 45 degrees, then 30 degrees
will correspond to the minimum value in the custom quality and 45 degrees will correspond to the
maximum value.
Figure 410: Custom Quality
Determinant
The Determinant, more properly defined as the relative determinant, is the ratio of the smallest determinant of the Jacobian matrix divided by the largest determinant of the Jacobian matrix, where each
470
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Display Mesh Quality
determinant is computed at each node of the element. The Determinant can be found for all linear
hexahedral, quadrahedral, and pyramidal elements. A Determinant value of 1 would indicate a perfectly
regular mesh element, 0 would indicate an element degenerate in one or more edges, and negative
values would indicate inverted elements.
Distortion
This is available only for hexa elements and is the measurement of the twisting of the element from
the ideal shape. For this the Jacobian determinants will be calculated at r,s,t=-1,0,1 of the natural coordinate system of the element (27 node positions). The distortion is 27 times the minimum of all absolute
determinants divided by the sum of all 27 absolute determinants (0 if all Jacobian determinants are 0).
Element Stretch
This option is available for surface and volume elements.
• For tris, this is calculated as the radius of the inscribed circle divided by the maximum edge length
and normalized by the value of an equilateral triangle with edge length 1.
• For quads and hexas, the calculated value is the minimum edge length divided by maximum edge
length normalized by the value for the idealized quad (cube) of length 1.
• For pentas and pyramids, this is calculated as the minimum of the element stretches of the quad and
triangle sides.
• For tetras, this is calculated as the radius of the inscribed sphere divided by the maximum edge
length normalized by the value of an equilateral tetra with edge length 1.
Equiangle Skewness
This quality parameter applies to tetra, hexa, quad, and tri elements.
Element equiangle skew = 1.0 – max ((Qmax – Qe) / (180 – Qe), (Qe – Qmin) / Qe),
where
Qmax = largest angle in the face or element
Qmin = smallest angle in the face or element
Qe = angle of an equiangular face or element (e.g., 60 degrees for a triangle, and 90 degrees for a
square).
Ford
A hybrid quality parameter for 3 and 4 node element meshes based on weighted skewness warp, and
aspect ratio values. The possible range is from 0 to 32.
Hex. Face Aspect Ratio
This quality parameter calculates the 3 averaged face areas of hexahedra elements, which is the average
of the areas of two opposite faces. The maximum of the six possible divisions of the averaged face areas
will be calculated and then inverted to normalize the result.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
471
Edit Mesh
Hex. Face Distortion
This quality parameter calculates the product of the maximum edge size in the i direction multiplied
by maximum edge size in the j direction, multiplied by the same in the k direction, and then divides
this value by the volume of the hex element.
Max Angle
This calculates the maximum internal angle of the quad or tri faces of elements.
Min Angle
This calculates the minimum internal angle of the quad or tri faces of elements.
Max Dihedral Angle
This is the maximum angular space contained between planes which intersect. It is measured by the
angle made by any two lines at right angles to the two planes.
Max Length
Calculate the maximum length of the diagonals of quad faces, and the maximum side length of tri faces.
This works for all meshes and element types.
Max Ortho
This calculates the maximum deviation of the internal angles of the element from 90 degrees.
Min Ortho
This calculates the minimum deviation of any interior angles of the element from 90 degrees.
Max Orthogls
This calculates the maximum deviation of the internal angles of the elements from 90 degrees. For
elements other than hexas this diagnostic is equal to Max Ortho. For hexas this differs from Max Ortho
in the way that angles between 180 and 360 degrees are also considered (deviation up to 270 degrees).
Max Ratio
This calculates the maximum ratio of the lengths of any two edges that are adjacent to a vertex in an
element.
Max Sector Volume
This option is available for volume elements. For each element node the sector volume will be calculated
in the Gauss integration points of order 3 and the maximum of the calculated sector volumes will be
taken.
472
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Display Mesh Quality
Min Sector Volume
This option is available for volume elements. For each element node the sector volume will be calculated
in the Gauss integration points of order 3 and the minimum of the calculated sector volumes will be
taken.
Max Side
This calculates the maximum length of all the edges of quad or tri faces. This works for all meshes and
element types
Min Side
This calculates the minimum length of all the edges of quad or tri faces. This works for all meshes and
element types
Min Side (Quad Optimized)
This calculates the minimum length of all the element edges. For quad elements, the opposite edge of
the minimum element edge will also be considered e.g., if the length of the opposite edge is smaller
than 1.1 times the minimum element edge length, the value will be the opposite edge length, else the
value will be 1.1 times the minimum element edge length.
Max Warp
This calculates the maximum warp (in degrees) of all elements. This works only for structured volume
and surface meshes, linear hexahedral and linear quadrahedral elements. To determine warp of a
quadrilateral face, find the midpoints of all edges, which will be co-planar. Then, calculate the maximum
angle of any edge with the plane thus defined, which is the warp of the face. The maximum warp of a
volume element or hexahedron is the maximum warp of its faces. For a 2D, planar mesh of QUAD_4
elements, the warp will be zero for all elements.
Max Warpgls
This measure applies to quad, prism and hexa elements (for quadratic elements the linear part will be
checked).
To determine the warp of a quadrilateral face, the angles between the triangles connected at the 2 diagonals of the quad will be calculated and the maximum will be used.
The maximum warp of a volume element (prism or hexa) is the maximum warp of its quad faces.
For a 2D planar mesh of QUAD_4 elements, the warp will be zero for all elements.
Mesh Distribution
The mesh distribution for all elements intersected by the line defined by the Start Point and End Point
locations will be calculated and displayed in the Mesh Distribution window. Distribution indicates
the criterion selected. You can display the distribution for element volume (Volume), average element
edge length (Avg Edgelen), minimum element edge length (Min Edgelen), or maximum element edge
length (Max Edgelen). The distribution is displayed as a graph where the abscissa (x-axis) indicates the
distance of the element centroid (projected onto the line) from the Start Point and the ordinate (y-
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
473
Edit Mesh
axis) indicates the selected criterion (Volume, Avg Edgelen, Min Edgelen, or Max Edgelen). This diagnostic is available for linear, tetra, pyramid, penta, and hexa elements.
Figure 411: Mesh Distribution
Figure 411: Mesh Distribution (p. 474) shows an example of the mesh distribution displayed. You can
use the left mouse button to zoom a portion of the plotted distribution.
Full range
resets the plot in the Mesh Distribution window to show the full range.
Load
allows you to load the mesh distribution data from a file.
Save
allows you to save the mesh distribution data to a file.
Delete
allows you to select the plots to be removed from the Mesh Distribution window.
Done
closes the Mesh Distribution window.
X log
toggles the logarithmic scaling of the x-axis.
474
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Display Mesh Quality
Y log
toggles the logarithmic scaling of the y-axis.
Symbols
allows the use of symbols to mark data.
Lines
allows the use of a line to indicate the distribution data.
X grid
toggles the display of grid lines along the x-axis.
Y grid
toggles the display of grid lines along the y-axis.
Mesh Expansion Factor
This option is available for volume elements. First, the node centered sector volume is calculated for
each node in the mesh. Then to calculate the expansion factor, the node centered volume is compared
to the volumes around the adjacent nodes to find the largest factor. For the element quality display,
for each element, the corresponding nodes will be checked and the maximum of all contributing node
mesh expansion factors will be used. If there is no node contributing to the element’s mesh expansion
factor, then the value will be 1.
Mid Node
The mid node criterion analyzes maximum deviation of mid node.
Mid Node Angle
This criterion is applicable only for Quadratic elements. It is the angle by which the quadratic mid node
is off from the linear edge.
Figure 412: Definition of Mid Node Angle
Opp Face Area Ratio
This measure is applicable to hexahedral elements only. This is the measurement of the worst ratio of
the areas of the opposite faces of the hexahedral element. Ideally, this value should be 1.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
475
Edit Mesh
Figure 413: Definition of Opposite Face Area Ratio
In the figure, let A1 = Area of Quad Face {ABDC}, and A2 = Area of Quad Face {EFHG}. If A1>A2, then
the Opposite Face Area Ratio of this pair of faces = A1/A2. If A1<A2, then the Opposite Face Area Ratio
= A2/A1. Similarly, the Opposite Face Area Ratio is found for each opposing pair of faces, and the
maximum of all three pairs is found as the measurement for this hexahedral element.
Opp Face Parallelism
This feature is also for hexahedral elements only. It is the measurement of the parallelism of the hexahedral elements. If the opposite faces are ideally parallel, the value is 1.
Orientation
Direction of the face normal determined by the orientation of the nodes based on the right hand rule.
Face orientation should be into the volumetric domain.
Orthogonal Quality
The orthogonal quality for cells is computed using the face normal vector (Ai), the vector from the cell
centroid to the centroid of each of the adjacent cells (ci), and the vector from the cell centroid to the
centroid of each of the faces (fi). See Figure 414: Vectors Used to Compute Orthogonal Quality for a
Cell (p. 477).
476
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Display Mesh Quality
Figure 414: Vectors Used to Compute Orthogonal Quality for a Cell
The following quantities are computed for each face:
• the cosine of the angle between the face normal vector (Ai) and the cell centroid to adjacent cell
centroid vector (ci).
• the cosine of the angle between the face normal vector (Ai) and the cell centroid to face center vector
(fi).
The minimum value obtained from calculating these quantities for all the faces is defined as the orthogonal quality for the cell.
The worst cells will have an orthogonal quality close to 0 while the best cells will have an orthogonal
quality close to 1.
For 2D surface mesh, a similar calculation is performed using only the edge normal vector (Ai) and the
vector from the face centroid to the centroid of each edge (ei). See Figure 415: Vectors used to Compute
Orthogonal Quality for a Face (p. 478).
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
477
Edit Mesh
Figure 415: Vectors used to Compute Orthogonal Quality for a Face
Note
The orthogonal quality measure is related to the ortho skew measure in ANSYS Fluent except
that the scale is reversed:
Ortho Skew = 1 – Orthogonal Quality
The orthogonal quality values may not correspond exactly with the ortho skew values from
ANSYS Fluent due to minor tolerance differences in how the data is handled internally.
Prism Thickness
This option is available only for linear and quadratic prism elements. This calculates the average of the
3 heights at the triangle corners.
Quadratic Dev
This computes the deviation of quadratic nodes from the corresponding linear edge. Consider a triangle
made up of 3 nodes: the deviation is the ratio of the altitude (the shortest line connecting the midside
node to the base) with the base (the two linear nodes). A value of 0 means the midside node is on the
linear edge.
Skew
This calculates the maximum skewness of an element. The skewness is defined differently for volume
and surface elements. In all cases it is normalized so that 1 is ideal and 0 is the worst possible.
• For a hexahedral element, skewness is defined as the normalized worst angle between each of the
6 face normals and the vector defined by the centroid of the hexahedron and the center of the face.
478
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Display Mesh Quality
Figure 416: Skew for Hexahedra
• For tri elements, skewness is defined as the ratio between the area of the element and the area of
an equilateral triangle having the same circumcircle.
• For quad elements, the skew is calculated by first connecting the midpoints of each side with the
midpoint of the opposite side, and finding the angle α as shown in the Figure 417: Skew for Quad
Elements (p. 479) (the smaller of the two angles will be used so that α<90 degrees). The result will be
normalized by dividing α by 90 degrees.
Figure 417: Skew for Quad Elements
TGrid Skew
The TGrid skewness measure is computed as the normalized maximum deviation from the ideal angle
at face corners (e.g., 60 degrees for a tri face, or 90 degrees for a quad face) for surface elements, or
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
479
Edit Mesh
the normalized maximum deviation from the ideal angle between face normals (e.g., 90 degrees for a
hexahedral element) for volume elements.
Note
The TGrid skewness values are inverted compared to other quality metrics in ANSYS
ICEM CFD. A value of 0 indicates the best quality element while a value of 1 indicates
a degenerate element.
Surface Area
This calculates the surface areas of all elements. This works for all meshes and element types.
Surface Dev
This measures the deviation of mesh from the actual geometry.
Taper
For hexahedral elements, the Taper is the maximum ratio of the areas of opposite faces. For quad elements, it is the maximum ratio of the lengths of opposite edges.
Tetra Special
This determines the ratio of the largest element edge to the smallest height for linear tetrahedral elements.
Figure 418: Definition of Tetra Special
In the figure, let d = height normal to surface ABC to point D. The Tetra Special value = {Max (a, b, c)}/d.
The maximum value calculated from all the nodes is the Tetra Special value for the tetrahedral element.
480
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Display Mesh Quality
Volume
This computes the volume of individual elements.
Note
This diagnostic does not consider degenerate hex elements, and will assign a negative
value for them. The Volume/Area/Length check can be used for degenerate hex elements instead.
Note
The Volume and Volume/Area/Length criteria essentially use the same calculation for
most element types and orders (linear or quadratic), but the volume check is optimized
for 8–noded (linear) hex elements. It is recommended to use Volume/Area/Length
unless you only want to check the volume mesh, or you have a linear hex mesh. In these
cases, the Volume check would be faster.
Volume Change
This quality metric is calculated for a specific element by finding the maximum volume among all of
its neighbor elements divided by the volume of the element itself.
Volume/Area/Length
This quality parameter calculates the line length of line elements, the area of surface elements, and the
volume of volume elements, with evaluation at Gauss points (4th order). It is implemented for all supported element types, including quadratic element types.
Note
The Volume and Volume/Area/Length criteria essentially use the same calculation for
most element types and orders (linear or quadratic), but the volume check is optimized
for 8–noded (linear) hex elements. It is recommended to use Volume/Area/Length
unless you only want to check the volume mesh, or you have a linear hex mesh. In these
cases, the Volume check would be faster.
Workbench Shape
This option is applicable to all shell and volume elements. It provides a composite quality metric that
ranges between -1 and 1. The metric is based on the ratio of the volume to edge length for volume
elements and the ratio of area to edge length for shell elements. A value of 1 indicates a perfect cube
or square, while a value close to 0 indicates a bad element, and a negative value indicates an inverted
element.
X Size
This computes the length of the element profile in the X direction.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
481
Edit Mesh
Y Size
This computes the length of the element profile in the Y direction.
Z Size
This computes the length of the element profile in the Z direction.
Quality Metric Histogram
Mesh quality is displayed as a histogram where the abscissa (x-axis) displays the element quality on a
scale from 0 (worst) to 1 (best) and the ordinate (y-axis) displays the number of elements in each
quality range. The default is 20 bars or divisions between 0 and 1. So the first bar would display the
number of elements whose quality is between 0 and 0.05, and the next bar between 0.05 and 0.1. The
same histogram values are also tabulated in Messages window. The Status message line will display
the min and max values of the quality criterion.
Figure 419: Mesh Quality Histogram
By clicking on any of the bars with the left mouse button, the information about the precise number
of values that fall into this interval and its boundaries are displayed in the Message window. The color
contour bar will also appear in the display. Histogram bars that have been selected become a solid
color, and remain selected until clicked on again. To display the elements within a selected (highlighted)
histogram bar, right click on the histogram window, and click Show (enabled by default). The elements
represented by that bar will be highlighted. If the Solid option is enabled, then the color of the elements
will represent the corresponding range of quality as indicated by the color contour bar.
By right clicking on the histogram, the following options are available.
Replot
allows you to change the parameters of the histogram in the Replot window.
Figure 420: Replot Window
• Min / Max X value
sets the minimum and maximum values of the particular quality type selected for the X-axis.
• Max Y height
482
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Smooth Mesh Globally
sets the maximum number of blocks for the quality ranges. A value of 0 will set the display to
such that the histogram with the largest number of elements is fully visible. A smaller number
will give increased resolution for quality ranges with fewer elements.
• Num bars
sets the number of bars to use in the histogram display.
Reset
sets the maximum number on the Y-axis such that the histogram bar with the largest number of elements
is fully visible.
Refresh
recomputes the mesh quality and refreshes the histogram display.
Show
displays the elements within the selected (highlighted) histogram bars.
Solid
displays all selected elements in solid view and by color that corresponds to the quality range. The color
contour bar will display the range of quality by color.
Note
This option slows down the display speed.
Color By Quality
when enabled (default), clicking on any histogram bar will display those elements colored according to
quality, as defined by the color bar which appear on the left side of the display window.
Highlight
applies to surface mesh only. Select one of the following options to highlight: selected elements only,
selected elements and one layer of attached surface elements, or selected elements and two layers of
attached surface elements.
Subset
puts the selected elements into a new subset.
Done
closes the histogram window.
Smooth Mesh Globally
The Smooth Mesh Globally option allows you to automatically improve the quality of the mesh
elements. Different smoothing algorithms are available depending on which mesh type is loaded. Mesh
can be smoothed with respect to a particular quality criterion and with a specified number of iterations
to achieve a given quality level. A mesh containing tetras, pyramids, prisms and triangular and quad
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
483
Edit Mesh
surface elements can be smoothed. The element quality is displayed as described in Display Mesh
Quality.
Note
It is no longer necessary to load a geometry file in order to perform mesh smoothing. Surface
nodes will be constrained to the boundary represented by the original mesh. Fixed and edge
constraints are also kept, as represented by node and bar elements.
If the desired quality is not attained, simply re-smooth until no further progress is seen. Then
consider manual editing. Place the worst elements in a subset or select them from the histogram in order to display them and make them active for editing.
If a multiblock mesh is loaded, see Smooth Multiblock Domains Globally for smoothing options.
The following options are available for smoothing the mesh:
Quality
Smoothing iterations
specifies the number of iterative steps. Each iteration will apply smoothing to a percentage of
the elements below the specified quality. The more iterations, the smaller the percentage of
elements that is selected and incremented for each step. For example, if 5 iterations are specified,
the first iteration will smooth the worse 20% of elements, the second will smooth 40%, etc. Increasing the number of iterations is more robust, but less iterations means that each iterative
step is smoothing more elements each time.
Up to value
specifies the quality level up to which the smoother will attempt to smooth the mesh.
Criterion
specifies the quality criterion. The following criteria are available:
• Quality
• Aspect ratio
• Custom quality
• Determinant
• Min angle
• Max orthogls
• Max warp
• Max warpgls
• Skew
Refer to Quality (p. 466) for details on the quality criteria.
484
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Smooth Mesh Globally
Smooth Mesh Type
Smooth
If enabled for a particular element type, then this element will be smoothed in order to produce
a higher grid quality. The quality of these element types will be represented in the quality histogram.
Freeze
If enabled for an element type, the nodes of this element type will be fixed during the
smoothing process. This element type will not be displayed in the histogram.
Float
If enabled for an element type, the smoother may move nodes of this element type freely according to their geometric constraints (points, curves, and surfaces). Nodes of floating elements
are only moved if necessary to improve the quality of the adjacent smoothed elements. In the
case that the nodes are moved, the quality of the floating elements is considered with the same
priority and with the same quality criterion/method as the smoothed elements. These floating
elements are not included in the histogram.
Note
There is a surface smoother and a volume smoother. If you smooth the surface
mesh, but float the adjacent volume mesh, you may find that the surface
smoother quality checks are not sufficient to maintain good quality in the adjacent volume mesh. However, between volume mesh types or when floating
surface mesh, the quality of the floating elements will be maintained.
Note
When smoothing a subset, the subset is actively smoothed while all other mesh
is set to float.
Smooth Parts/Subsets
All Parts
allows you to smooth elements in all parts.
Only active parts
allows you to smooth only the parts that are activated/enabled in the Display tree.
Only visible subsets
allows you to smooth only the visible subsets.
Active parts and visible subsets
allows you to smooth both the parts enabled in the Display tree and the visible subsets.
Refresh Histogram
recalculates and updates the histogram. This is useful when changing the Smooth Mesh Type options
and you want to simply check the quality of the elements prior to performing a smoothing step.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
485
Edit Mesh
Advanced Options
Laplace smoothing
Pure
solves the standard Laplace equation that calculates the average of all neighbor nodes for
any node and gives a more uniformly spaced mesh. This setting operates on mesh types
set to Smooth, smoothing surface mesh types first and then volume mesh types.
Note
Laplace smoothing surface mesh before inflating prisms results in better
prism quality. Also, using the standard Laplace equation for prisms can
sometimes lead to a lower determinant quality. Therefore, it is recommended
to run this prior to prism generation.
Edge length
uses a modified Laplacian scheme which tries to equalize the edge lengths around a node.
This option is useful in cases where the mesh size distribution is quite wide. The smoother
will try to increase the minimum edge length toward the average size to improve mesh
uniformity. Figure 421: Edge Length Based Laplace Smoothing (p. 486) shows an example
where the minimum edge length on the mesh increased after smoothing using the Edge
length criterion. The highlighted portion shows a set of elements where the smoothing
scheme was able to redistribute the edge lengths to be more equal.
Note
As this method tends to increase the minimum edge lengths in a model, it
can be very useful for explicit solvers whose time step is tied to the minimum
edge length.
Figure 421: Edge Length Based Laplace Smoothing
Residual on Surfaces
when enabled, allows you to specify the residual for surfaces.
Residual in Volume
when enabled, allows you to specify the residual for the volume.
The residual represents the smoother “convergence” rate with respect to the initial state.
It is calculated as the ratio of average node movement at the current iteration to the average
node movement at the first iteration. You can specify the residuals for surface and volume
486
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Smooth Mesh Globally
while smoothing. The residual at each iteration will be reported in the message window.
When the specified residual value is reached, the smoothing process will stop.
Note
The acceptable range for residual values specified is 0–1.
Not just worst 1%
if enabled, it will evaluate all elements while smoothing. By default the smoother only smoothes
the worst 1% of each element type.
Allow node merging
if enabled, the smoother is allowed to merge nodes to improve the mesh.
Allow refinement
allows the smoother to automatically subdivide tetras to obtain further improvement. After
smoothing with Allow refinement enabled, it may be necessary to smooth further with this
option disabled. The goal of this option is to reduce the number of cells that are attached to
one vertex by refinement in problem regions.
Group bad hex regions
is used only in unstructured hexa smoothing. If enabled, then bad hex elements are grouped
into bad regions. The smoother will run on these bad regions one at a time. If disabled, then
the smoother will smooth all the groups at once.
Ignore PrePoints
is used only for unstructured hexa smoothing. This option simply ignores the prescribed points
which hinder the quality of mesh.
Surface Fitting
is used only for unstructured hexa smoothing. It forces the smoother to follow B-spline surfaces
rather than the triangulation of the surfaces.
Prism Warpage Ratio
prisms are smoothed based on a balance between prism warpage and prism aspect ratio.
Numbers from 0.01 to 0.50 favor improving the prism aspect ratio, and from 0.50 to 0.99 favor
improving prism warpage. The farther the value is from 0.5, the greater the effect.
Violate Geometry
allows the smoothing operation to yield a higher quality mesh by violating the constraints of
the geometry. Normally when a grid is smoothed, the nodes are restricted to the geometry and
can only be moved along the geometric entities to obtain a better mesh.
Note
This option would be advantageous for situations such as a region where two
surfaces come together at an angle that makes good element quality difficult
to obtain (angles under 30 degrees). In this case, the mesh cannot both accurately
capture the geometry, and give good quality mesh. The geometry (the 30 degree
angle) can be sacrificed a small amount to improve the element quality if this
option is utilized. A large number of bad elements can be fixed in this way by
making a small sacrifice on the geometry.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
487
Edit Mesh
Tolerance
is the distance measured in units of the model that nodes can be moved off the geometry, if
Violate Geometry is enabled.
Relative Tolerance
if enabled, this will make the specified Tolerance the factor of the minimum edge length of
the mesh instead of an absolute tolerance in units of the model.
Minimum Edge
if enabled, you can specify the minimum edge length allowed in the mesh after smoothing.
Smooth Multiblock Domains Globally
The Multiblock smoother is used to obtain smooth grid lines. It is specially optimized for blade
configurations. The mathematical basis is that an elliptical differential equation of the form ∇
=,
where is the “control function”, will be solved. It can be proved that by using the elliptical operator
∇ , smoothness of the mesh will be achieved. The control function will be specified so that the
smoothed mesh will obtain certain characteristics, such as orthogonality and layer height of the first
layer.
The Multiblock smoother can also constrain nodes in one dimension and smooth nodes in the other
dimensions in order to improve mesh quality. This is useful in turbine blade analysis e.g., for the inlet
and outlet surfaces. While smoothing, the blade surfaces are frozen to maintain geometric location.
Previously, the inlet and outlet would be frozen, thereby freezing the ends of the periodic sides, and
thus, limiting the smoother. By constraining nodes in one dimension, the inlet and outlet are constrained
axially, maintaining their distance from the blade as well as their periodicity. However, the nodes can
be smoothed in the other dimensions, thereby allowing the smoother more flexibility.
For all other mesh types, the options for Smooth Mesh Globally will be displayed.
The following parameters are available when a multiblock mesh is loaded:
488
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Smooth Multiblock Domains Globally
Relaxation Domain(s)
click the appropriate icon to select or deselect domain(s) to be smoothed.
Smoothing Direction
3D
smoothes the mesh in all directions.
I, J, or K
allows you to select the smoothing direction.
Layer Options
This smoother works by smoothing planes and then interpolating the smoothing between the layers.
The model is reduced to a single block high and the layers are the mesh indices from one side to the
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
489
Edit Mesh
other along the smoothing direction. You need not smooth every plane. In models with very little twist,
selecting the first and last plane is sufficient. If a model (such as a compressor blade) has more twist, it
may be advantageous to smooth the first and last, as well as a few layers between.
Start Layer, End Layer
the first (usually 1) and last (usually the total number of layers) to be smoothed. These form the ends
of the smoothed volume and are usually setup automatically.
Increment
allows you to add smoothing planes between the first and the last planes. For instance, if you have
26 planes, you could have an increment of 5, which would mean the 6th, 11th, 16th and 21st planes
would also be smoothed. Use a smaller increment to include more planes and better capture twist
or other changes in the cross section. Setting the increment to 1 will smooth each plane individually,
and is usually not necessary.
Volume iterations
specifies the number of smoothing iterations between each actively smoothed layer. If this value is
greater than 0 then the layers between the smoothed planes will not only be interpolated but additionally smoothed.
Planes
specifies the planes which need to be smoothed directly. If set, then the Start Layer, End Layer and
Increment setting will not be used. The plane numbers are separated by blanks (e.g., “1 5 10”)
Select Options
Non-Relaxation Subfaces
freezes the selected subfaces.
Hold Cell Height Subfaces
orthogonality and first cell height will be obtained on all grid lines perpendicular to the selected
subfaces.
Fixed Edges
all edge nodes will be frozen for each selected edge.
Fixed Distribution Edges
the corresponding nodes can move but the original bunching will be retained for each selected
edge.
Global Vertices
if any end vertices of a block edge have been selected, and a smoothing direction is selected, then
the Pre-Mesh will be smoothed globally in planes. It is recommended to select all vertices as Global
Vertices and to freeze the real (not periodic) boundaries.
Layer Vertices
is intended to be used for O-grid vertices. For neighbor nodes, the bisector will be calculated placing
the neighbor nodes on the bisector line in a distance specified as the First Layer Distance. If the
First Layer Distance is smaller than 0.0, the selected vertices will not be used. Vertices can be added
or removed from the selection list, and the First Layer Distance can be changed for the selected
vertices.
Layer vertices are only used in Global edge smoothing. To access this option, a smoothing
direction must have been selected.
490
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Smooth Multiblock Domains Globally
Clear all selections
resets all selections.
Advanced Options
The following advanced options are available:
Number of Iterations/Steps
Iterations in equation solver
An equation solver (SOR method) is used to solve the elliptic equation method. This value specifies
how many iterations should be done (default is 25).
Steps in global edge smoothing
specifies the number of smoothing steps in the global-edge smoothing method. In each step,
the Pre-Mesh will be smoothed globally and the output will be used as input in the next step
(default is 25).
Parameters
Projection limit
is used for node distribution whose first spacing from the surface is less than the geometry tolerance. It is useful for near-wall layers. A value greater than 0.0 will define a distance normal to
the surface up to which the nodes will be interpolated. A single value of projection limit is used
at all locations on the model.
Relaxation factor
is a factor to stabilize the smoothing value. Reasonable values should be between 0.0 (exclusive)
and 1.0 (inclusive). Default value is 0.5.
Residual factor
is used during global edge smoothing. Starting from the 2nd global edge step, the average
change compared to the previous step will be calculated by dividing this value by the value
calculated in the 2nd step. If this relative value gets lower than the specified residual factor, a
stop criterion has been reached. Default value is 0.05.
Surface fitting
constrains boundary nodes to the true geometry surfaces. With this option off, the boundary
nodes will be projected to the triangulation of the geometry surfaces.
Use projection
smoothing steps are performed allowing nodes to move away from constraints (curves, surfaces),
and then the nodes are finally projected back to the curve or surface. This option is disabled by
default.
Use orthogonal positioning
is used during global edge smoothing or plane smoothing. If Hold Cell Height has been set on
a subface, a special method will be used to calculate the control function values in a way that
the first layer nodes will be placed to hold the original or user defined (layer vertices) cell height
and to be orthogonal (bisector) to the boundary. This option is enabled by default.
Use fractional positioning
is used during global edge smoothing or plane smoothing. If Use orthogonal positioning has
been set, the first layer nodes will not be moved in one step to the orthogonal position but in
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
491
Edit Mesh
a certain amount of steps (10). This is mainly to stabilize the orthogonal positioning algorithm
in highly clustered meshes. This option is disabled by default.
Methods
In the structured smoother, several elliptic relaxation methods are available both for the Volume
and Subfaces (subface boundaries). The default method is Sorenson - Laplace. In the case of
global edge smoothing, this parameter has no meaning.
Sorenson-Laplace
Sorenson methods attempt to maintain node distributions (bunching) near the surface boundaries
while improving orthogonality. This hybrid attempts to improve orthogonality at the boundary
while maintaining the first layer height from the boundary surface and making a uniform node
distribution in the interior
Sorenson-Thomas & Middlecoff
This method improves orthogonality at the boundary while maintaining the first layer height
from the boundary surface and holding the original clustering on the interior.
Thomas & Middlecoff
This method generally improves the orthogonality of grid lines across boundaries while holding
the original clustering in the interior.
Laplace
This method attempts to give a uniform mesh size for all selected elements.
Interpolation
This uses an algebraic transfinite interpolation method with Soni interpolants to generally improve
internal angles.
Hilgenstock - Thomas & Middlecoff
Hilgenstock methods maintains orthogonality. This hybrid maintains orthogonality between block
boundaries (subfaces) to give a smooth transition across subfaces, while maintaining the first
layer height from the boundary surface.
Hilgenstock - Laplace
This attempts to improve orthogonality and uniform node distribution within the mesh.
Grid expansion rate
is the exponent for the exponential decay of Sorenson terms from the boundary to the interior of a
subface. Reducing this factor will cluster the elements closer to the boundary. Default values are 3.5
for Subfaces and 4.6 for the Volume.
Multiblock Settings
Load Settings
allows you to load previously saved Multiblock Settings.
Save Settings
allows you to save the current Multiblock Settings in a file.
Run in sequence
allows you to load and run different Multiblock Settings files in sequence. Click Start sequence
to begin running the sequence of files.
492
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Smooth Multiblock Domains Globally
Distributed Smoothing
Distributed Smoothing
enables the use of distributed smoothing which allows you to smooth the mesh using multiple
processes executing on the same computer or different computers in a network.
Define Hosts
opens the Host Setup panel where you can specify the host settings.
You need to do the following to specify the host settings:
1.
Click New Host to open the Add Host panel where you can define the host machine. Specify
the name of the host and select the operating system type from the Type drop-down list.
Click Accept.
2.
All defined hosts will be listed in the Available Hosts list. Select the host in the Available
Hosts list and verify the relevant parameters.
3.
a.
Number Processors specifies the number of processors on the machine.
b.
The Startup Command allows you to use either the remote shell client (rsh ) or secure
shell client (ssh ). Enable Password if you require a password to access the machine.
You may click the Check button to verify that the startup command works correctly.
c.
Verify that the ICEM_ACN Path and License File path are correct and specify the
Working Directory as appropriate.
d.
Click Save Available to save the settings for the available hosts.
Select the host in the Available Hosts list and click Add -> to add the host to the Assigned
Hosts list. To remove a host from the Assigned Hosts list, select the host and click <- Re-
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
493
Edit Mesh
move. You can also permanently delete previously defined hosts using the Delete Host
button.
4.
Click Save Assigned to save the settings for the assigned hosts and close the Host Setup
panel.
Number Processes
specifies the number of processes.
Connect Timeout
specifies a timeout for connecting to the host machine.
Verbose Print
enables the printing of detailed messages in the message window.
Smooth Hexahedral Mesh Orthogonal
The unstructured hexahedral smoother relaxes unstructured hexahedral meshes in order to obtain
smooth grid lines orthogonal to the boundary as well as smooth grid angles and transitions in the inner
volume. It first smoothes the surface mesh recognizing the topological boundary edges. If the number
of volume smoothing steps is greater than 0, after each surface smoothing step the inner volume will
be adjusted by performing 1 volume smoothing step. After the surface smoothing has been finished,
the inner volume will be smoothed (according to the number of volume steps set). It can also smooth
pure surface meshes.
The mathematical basis is that an elliptical differential equation of the form ∇
= , where is the
“control function”, will be solved. It can be proved that by using the elliptical operator ∇ , smoothness
of the mesh will be achieved. The control function will be specified so that the smoothed mesh will
obtain certain characteristics, such as orthogonality and layer height of the first layer.
The unstructured hexahedral smoother is available under Edit Mesh > Smooth Hexahedral Mesh Orthogonal (to smooth an existing mesh) and under Blocking > Pre-Mesh Smooth (to smooth the Hexa
pre-mesh). If you select Blocking > Pre-Mesh Smooth, the pre-mesh will be calculated (if it does not
exist), and then you can select the Orthogonality option for the Smooth Method for the unstructured
hexahedral smoother.
Note
If you smooth the pre-mesh (Blocking), the smoother may move vertices and change edge
distributions undesirably. If you are outputting a structured mesh, it is recommended that
you save the blocking first so you can return to the previous state if necessary. If you are
outputting in an unstructured mesh format, it is recommended that you first convert to unstructured mesh and then use the Edit Mesh > Smooth Hexahedral Mesh Orthogonal
option.
Tips to improve smoothing success:
• Create the best possible starting condition by matching edge distributions.
• Create points (geometry) at the ends of the edges, and then associate the vertices (block) to them. This
may be used to contain an area of fine mesh along a wall, preventing it from being totally smoothed out.
494
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Smooth Hexahedral Mesh Orthogonal
The following smoothing parameters are available:
Number of iterations on Surface
specifies the number of iterations the smoother uses to relax the surface mesh. The minimum number
of smoothing iterations to be completed for stability reasons is 10. The default number of iterations on
surface is also 10.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
495
Edit Mesh
Number of iterations on Volume
specifies the number of iterations the smoother uses to additionally relax the volume mesh after surface
smoothing has been finished (minimum is 0). When the number specified is greater than 0, a volume
smoothing step will be performed after each surface smoothing step to adjust the volume mesh to the
surface mesh. The default number of iterations on volume is 5.
Smooth type
For both Surface and Volume, the Method drop down lists contains the following three options:
• Orthogonality
The smoother will try to retain orthogonality and the height of the first layer. For surfaces, orthogonality implies that the first layer grid lines will be orthogonal to the surface edges.
• Laplace
The smoother will try to equalize the mesh by setting the control function f to 0 in the elliptical
differential equation.
• Structured
The smoother offers two additional choices: Sorenson methods attempt to maintain node distributions (bunching) near the surface boundaries while improving orthogonality. It could be one
of two types. Hilgenstock methods maintain orthogonality and first layer height, and may be
one of two types.
Selecting Structured causes a second drop down list to appear. The following four options are
available:
– Sorenson/Laplace: This attempts to improve orthogonality at the boundary while maintaining the
first layer height from the boundary surface and making a uniform node distribution in the interior.
– Sorenson/Thomas & Middlecoff: This method improves orthogonality at the boundary while
maintaining the first layer height from the boundary surface and holding the original clustering on
the interior.
– Hilgenstock/Laplace: This attempts to improve orthogonality and uniform node distribution within
the mesh.
– The Hilgenstock/Thomas & Middlecoff method tries to maintain orthogonality at boundaries while
holding the first layer height. With Thomas & Middlecoff as the background control function, the
original clustering is intended to be maintained.
Note
During smoothing, the volume mesh will be separated into an inner (Volume) part and
boundary (Surface) part which will be smoothed independently of each other. The
boundary (surface) elements will be smoothed first, then the inner volume will be adjusted
to the smoothed surface boundary, and finally the inner (volume) elements will be
smoothed. Hence, it is advisable to set the same Smooth type for both Surface and
Volume.
496
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Smooth Hexahedral Mesh Orthogonal
Freeze Options
• All Surface Boundaries
freezes all boundary node locations.
• Selected Parts
allows you to specify freeze options for selected parts. Select the part(s), then click Selected
part(s) Options. Specify the frozen surface boundary by enabling Surface boundary. Specify the
number of layers to be frozen with the surface boundary by disabling Surface boundary and
entering the number of layers n in the Layers field. The number of layers is set to 0 by default.
When Layers is greater than 0, then the surface boundaries including the first n layers from the
boundary will be frozen. For example, a value of 3 indicates that three layers of nodes away from
the surface will be frozen along with the surface boundary.
(A) Enabling Surface
boundary
(B) Specifying number of layers
Release Orthogonality / Initial Height Options
For certain situations, it may be helpful to release the orthogonality requirement from a certain surface
part or set the first layer distance (initial height of the first element off the wall) on certain surfaces.
These are mutually exclusive since orthogonality is required to set the first layer height. Select the desired
parts, and then click Selected part(s) Options. The default is to release orthogonality for each part. You
can set the initial height by disabling Release orthogonality and then set the initial height by entering
it in the Initial Height field.
Note
You can set the Initial Height to -1 (default) in order to keep the starting initial height.
(A) Enabling Release orthogonality
(B) Specifying Initial
Height
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
497
Edit Mesh
Smooth along curves
allows you to specify which edges (projected onto curves) should be smoothed. The smoothing will be
carried out when faces are smoothed. You can specify none, all, or selected curves. The default is all.
Note
If the mesh distribution has a relatively large dynamic range of mesh sizes along a curve,
then selecting this option may be counter productive.
Advanced Options
The Choose Option drop down list contains the following advanced smoothing options:
Grid Expansion
If a smoothing method other than Laplace is selected, then the grid expansion values will be used
to distribute the control function values into the inner volume. If the grid expansion rate is greater
than 0.0, the algorithm computes a pseudo structured region in which the control function values
will be interpolated by an exponential decay (the grid expansion rate will then control the negative
exponent (e power -g) of the control function values). If it is 0.0 then a Laplace interpolation of the
control function values will be done, i.e., for an inner node, the control function value will be averaged
by the control function values of its neighbor nodes.
498
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Smooth Hexahedral Mesh Orthogonal
The default values are 0.0 for the surface mesh and for the inner volume. Reasonable values
other than 0.0 should be greater than 1.0.
Note
It may be difficult to form the pseudo structured regions in some cases. If you have
such problems, set the grid expansion rate back to 0.
Note
If the grid expansion rate is set to 0.0 and the smooth type is set to Orthogonality,
the first layer height and the orthogonality at the boundary are still achieved, but
the next layers tend towards Laplace approaching the middle of the mesh. In case
of a Navier- Stokes mesh you can see the effect near the boundary where the first
layer is orthogonal to the boundary but the next layers curve as they equalize (Laplace)
the distances of the layer nodes.
Treat unstruct nodes
determines the method of treating inner unstructured nodes. An unstructured node is a node on
which no ij (surface) or ijk (volume) directions can be defined, e.g. a node which has more or less
than 4 (surface) or 6 (volume) neighbors is clearly an unstructured node.
Figure 422: Initial Mesh (p. 499) shows the mesh before smoothing. The highlighted node is an
unstructured node, while all other nodes are structured. Figure 423: Smoothed Mesh (p. 500)
shows the mesh after smoothing.
Figure 422: Initial Mesh
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
499
Edit Mesh
Figure 423: Smoothed Mesh
• Bisector
Each structured neighbor node will be positioned in a bisector angle with respect to the unstructured node and the two other neighbors. The grid line between the node and the unstructured node will be in a bisector angle to the 2 grid lines between the unstructured node
and the corresponding neighbor node from left and right. The distance will be calculated in
a heuristic way. If the neighbor node is unstructured then it will be positioned using the
Laplace method.
• Laplace
Each neighbor node will be positioned using the Laplace method.
• Modified Laplace
Each structured neighbor node will be positioned using the Laplace method, but comparing
its distance to the unstructured node with the appropriate distances of the unstructured node
to its other neighbors (should not be greater than a certain ratio). If the neighbor node is
unstructured then it will be positioned using the Laplace method.
The hexahedral smoother works better on structured meshes because it can use structured elliptical smoother methods which are more powerful than the methods for the unstructured
parts for which it mainly uses Laplace.
Note
For most models, the effect of the this setting may be negligible.
Stabilization Factor
is used in the calculation of the new nodes and should be greater or equal to 1.0. A higher factor
will make the smoother more stable at the cost of orthogonality at the boundaries. If there are
problems with the smoother it is recommended to increase this value (to around 8.0). Default values
500
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Smooth Hexahedral Mesh Orthogonal
are 1.0 on surfaces and 2.0 in the volume. Increasing this parameter may be helpful on certain
model configurations if the smoother corrupts the mesh, especially if it appears due to overly orthogonal boundaries.
Use Orthogonal Distance
if enabled, then the original boundary distance of a first layer node will be calculated by projecting
it to the boundary and measuring the distance to the projected point. Otherwise, the length of the
original grid line will be used. By default this option is disabled for both the surface and volume.
In cases where there is a sharp angle between the grid lines from the first layer to the boundary,
if Use Orthogonal Distance has not been set, the calculated first layer distance may be considerably greater than the distance of the first layer nodes to the boundary (because the length
of the grid line will be used). Hence, it may be advisable to set Use Orthogonal Distance in
the same way for both Surface and Volume. This would ensure that the first layer grid line
angles in the volume near the surface boundary would be similar to the nearby surface
boundary grid line angles.
Define Edges on Part Border Options
The border grid lines attached to the selected parts will be defined as edges. The main purpose for
defining these edges is that they separate the two sides of the surface mesh. If an edge is topologically
internal then orthogonality will not be established there.
Fix Orientations
If Volume is enabled, then before smoothing takes place, all volume elements will be checked to
see if the node order defines a right-handed element and will be fixed if necessary.
Note
Enabling this option could result in additional calculation time.
Surface Fitting
constrains boundary nodes to the true geometry surfaces. When disabled, the original mesh faces
are used to determine the boundary constraints. This option is enabled by default.
Freeze Projected Nodes
When set, all nodes which are prescribed or projected to the geometry (curves or surfaces) will not
be allowed to move.
Keep Periodic Geometry
when enabled, ensures that the mesh will stay on the geometry on periodic sides. Otherwise the
periodic nodes can move away from the geometry. Nevertheless periodicity is still guaranteed. This
option is enabled by default.
Active Parts Only
if enabled, only the active parts (parts that are turned on (activated) in the Parts branch of the display
tree, see the Parts (p. 180) section) will be smoothed. The geometry or mesh of the active parts does
not need to be displayed. When this option is disabled, the whole mesh will be smoothed. The histogram displayed will also reflect the setting of the Active parts only option. This option is disabled
by default.
If you click Apply or OK the mesh smoothing will be started. If OK is selected, then the window will
be closed afterwards.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
501
Edit Mesh
Repair Mesh
The Repair Mesh options can be used for manually editing parts of the mesh that are not of good
quality.
Figure 424: Repair Mesh Options
The following mesh repair options are available:
Build Mesh Topology
Remesh Elements
Remesh Bad Elements
Find/Close Holes in Mesh
Mesh From Edges
Stitch Edges
Smooth Surface Mesh
Flood Fill / Make Consistent
Associate Mesh With Geometry
Enforce Node, Remesh
Make/Remove Periodic
Mark Enclosed Elements
Build Mesh Topology
Angle
Line elements (1D) will be created between shell elements (2D) attached at angles greater than the
specified angle. Node elements (0D) will be created between line elements (1D) attached at angles
greater than the specified angle.
Create bars between shell parts
automatically creates bar elements between different shell mesh parts, regardless of the angle between
them.
Selected elements
allows you to select particular elements for which to build mesh topology.
502
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Repair Mesh
Remesh Elements
Only one element type can be remeshed at a time. Select a particular surface mesh type from the
Mesh type drop-down list and then manually select particular elements. The selected elements are
first deleted, and then the vacant area is remeshed. The element sizes are determined by the size of
the surrounding edges.
Note
This option is designed for plane subsets of the surface mesh, and for selected volume
parts, but not for curved surfaces or entire volumes.
Part
The remeshed elements will be added to the selected part.
Surface projection
allows you to project new nodes onto the nearest surface.
Ignore projection
if enabled, projections to curves and points will be ignored when remeshing. If a group of elements that
are being remeshed have internal nodes that are projected to curves or points, and if Ignore projection
is disabled, the elements will not be able to be remeshed as the projections will be lost.
Note
It is recommended to enable Ignore projection when remeshing a controlled region of
mesh, and disable it when remeshing bad elements for the entire model.
Number of offset layers
specifies the total number of offset layers while remeshing the selected elements.
Offset height factor
The height of the first offset layer is this factor multiplied by the given element size. The height of any
successive layers will increase for concave edges, and decrease for convex edges.
Offset type
• Standard
Offsets will be created normal to the edges without special solutions for sections with small or
large angles, such as corners. The number of nodes on the offset front may not be identical as
the number of nodes on the initial boundary.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
503
Edit Mesh
Figure 425: Standard Offset Example
• Simple
Offsets will be created normal to the edges without special solutions for sections with small or
large angles, such as corners. The number of nodes on the offset front is identical to the number
of nodes on the initial boundary.
Figure 426: Simple Offset Example
• Forced Simple
This option is the same as Simple Offset, but without collision checking.
504
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Repair Mesh
Figure 427: Forced Simple Offset Example
Remesh Bad Elements
The Remesh Bad Elements option has similar options to Remesh Elements (p. 503), with the difference that only the bad quality elements from the selected elements will be deleted and remeshed. It
will not delete all selected elements.
Mesh type
specifies the mesh type.
Elements
specifies the elements to remesh.
Surface projection
allows you to project new nodes onto the nearest surface.
Ignore projection
if enabled, projections to curves and points will be ignored when remeshing. If a group of elements that
are being remeshed have internal nodes that are projected to curves or points, and if Ignore projection
is disabled, the elements will not be able to be remeshed as the projections will be lost.
Note
It is recommended to enable Ignore Projection when remeshing a controlled region of
mesh, and to disable it when remeshing bad elements for the entire model.
Quality metric
specifies a quality metric.
Up to quality
specifies the desired quality level.
Max iterations
is the total number of iterations to remesh in order to get the desired quality level.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
505
Edit Mesh
Find/Close Holes in Mesh
The Find/Close Holes option locates holes in the selected elements and remeshes them.
Mesh Type
specifies the appropriate surface mesh element type.
Elements
specifies the elements from which to look for holes.
Surface projection
allows you to project new nodes onto the nearest surface.
Part from geometry
when enabled, the Part for the new elements is inherited from the adjacent surface part. This is calculated
with a normal ray from the center of each new element to the nearest surface. When this option is disabled, the Part for the new elements is inherited from the surrounding elements based on the first element
selected.
Mesh From Edges
The Mesh from Edges option allows you to close holes by selecting the edges that surround it.
Mesh type
specifies the appropriate surface mesh elements available.
Edges
allows you to select the edges that surround the holes.
Surface Projection
allows you to project new nodes onto the nearest surface.
Single loop & complete edges
if enabled, it will try to complete a loop from the edges selected. If disabled, it will not mesh if the selected
edges do not form a complete loop.
Interpolation surface
interpolates the meshing area by a biquadratic approximation in order to generate a smooth surface.
Keep volume consistent
if enabled, makes sure that the surface mesh and volume mesh are consistent with each other after
remeshing.
Note
This only applies to tetra meshes.
506
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Repair Mesh
Stitch Edges
The Stitch Edges option allows you to close gaps within selected edges (usually single edges) by
merging opposing nodes, making the mesh on both sides conformal.
Edges
specifies the edges to be stitched.
Rel. Merge Tolerance
if two nodes are within this tolerance, they will be merged instead of stitched together. Specify a factor
(from 0 to 1) of the local element size. Typical values are 0.05 – 0.2. The purpose of this tolerance is to
avoid tiny element edges, not to limit the stitch area.
Merge End Nodes
when enabled, this option will merge end nodes when stitching the selected edges.
Smooth Surface Mesh
The Smooth Surface Mesh option is an automatic process for improving the quality of selected
surface mesh elements. A common mesh smoothing technique is Laplace Smoothing, which seeks to
reposition the nodes so that each internal node is at the centroid of the polygon formed by its connected
neighbors. This repositioning is usually done iteratively.
Elements
specifies the surface mesh elements to smooth.
Max Iterations
is the maximum number of iterations for smoothing the mesh.
Accuracy
is a relative tolerance for element quality (between 0 and 1) related to the local element size. The default
value is 0.025. If set to 0, then the given number of smoothing steps is done. Bigger values improve the
performance because smoothing stops when the accuracy has been reached.
Isoparametric
is an additional option for the surface smoother. The default value is 0, which is pure Laplacian
smoothing. You can increase this parameter up to 1 to produce an isoparametric mesh.
Surface projection
allows you to project new nodes onto the nearest surface.
Smooth boundaries
smoothes the boundary nodes of the surface mesh selected, not just the internal nodes. It also allows
curve nodes to be improved.
Flood Fill / Make Consistent
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
507
Edit Mesh
Flood Fill
The Flood Fill process here is the same as what happens during the Octree meshing process. Flood Fill
uses Material points to mark volume elements and group them into volume parts. See also the Octree
meshing approach in the ANSYS ICEM CFD User's Manual.
For each material point in the model, a root volume element is defined (the volume element that
this material point sits in). From each root volume element, all the neighboring volume elements
will be added, and then their neighbors are added in a flood filling manner. This process stops at
the surface elements which define the closed boundary and selects all the volume elements within
the boundary. The selected volume elements are assigned to the part of the material point within
the volume.
Note
If the flood fill process finds a second material point with a different part name within
the same process, leakage is detected. Flood fill will attempt to automatically close holes,
but if it cannot, you will be prompted to close holes interactively. A message will alert
you to which material point entities are in conflict. In the interactive process, you will be
shown a jagged line representing the connection path between the material points along
the centroids of the volume elements and through the “hole” if there is one. It will also
highlight the single edges and bring up the mesh editing option for mesh from edges
so you can more easily select the edges and close the hole. Then the flood fill will resume.
In some cases, the problem may be that both material points are in one volume or perhaps
one is in the wall between two volumes; in which case deleting or moving material points
is the solution.
Figure 428: Use of the Flood Fill Option
Note
For situations where the mesh is not surface fitted, use the Mark Enclosed Elements
option instead of Flood Fill.
508
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Repair Mesh
Make volume mesh consistent with surface mesh
makes tetra volume mesh consistent with tri surface mesh. Tetra elements near the surface are modified
to fit the surface mesh. The final volume mesh is connected node for node with the surface mesh. You
can use this command to replace a boundary or cut a surface mesh out of a volume.
Figure 429: Original Volume and Surface Meshes (p. 509) shows a manifold with an inserted baffle.
The tetra volume mesh for the manifold and the tri surface mesh for the baffle is also shown.
Figure 429: Original Volume and Surface Meshes
Figure 430: Combined Mesh (p. 509) shows the combined mesh, where the use of this option allows
you to combine the two meshes in different orientations.
Figure 430: Combined Mesh
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
509
Edit Mesh
This option may be chosen for All elements, or Selected elements.
Note
Most manual mesh editing commands, such as merge, split, etc. automatically keep the
volume consistent. Other commands, such as remesh from edges have an option to
“Keep volume consistent”.
Associate Mesh With Geometry
The Associate Mesh with Geometry option will assign the closest part to the selected surface
mesh elements.
Enforce Node, Remesh
If a node lies outside the mesh and is not the part of mesh (e.g., a Weld node) the Enforce Node,
Remesh option will remesh nearby surface nodes so that the mesh respects the node location.
Mesh type
specifies the mesh type.
Surface projection
allows you to project moved nodes onto the nearest surface.
Ignore projection
if enabled, projections to curves and points will be ignored when remeshing. If a group of elements that
are being remeshed have internal nodes that are projected to curves or points, and if Ignore projection
is disabled, the elements will not be able to be remeshed as the projections will be lost.
Note
It is recommended to enable Ignore projection when remeshing a controlled region of
mesh, and to disable it when remeshing bad elements for the entire model.
Keep volume consistent
if enabled, then the volume mesh also gets remeshed with the shell mesh, and the consistency between
the volume and surface mesh is maintained.
Note
This option only applies to tetra meshes.
Selection Method
You have the option of selecting nodes or points. If selecting points, also specify the surface mesh part
name for the new node element.
510
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Repair Mesh
Make/Remove Periodic
The Make/Remove Periodic option allows you to manipulate the periodicity of specific nodes.
You can check the existing periodicity through the mesh display options in the Model tree.
Note
In order to make nodes periodic, periodicity must be defined in Mesh > Global Mesh
Parameters.
Make Periodic
allows you to select two nodes at a time to define periodic node pairs.
Note
In order to make an axis vertex periodic with itself, select only that node, and you will
be asked to confirm that the selected node should be made periodic to itself.
Remove Periodic
removes the periodicity from the selected nodes. Select one node of each periodic node pair.
Mark Enclosed Elements
The Mark Enclosed Elements option uses Material Points within an enclosed volume of surfaces
to mark all the elements within that volume and assign them to the same Volume Part as the enclosed
Material Point. Only mesh in regions containing the selected Material Points will be affected.
Any elements within the enclosed space containing the Material Point are placed into the same Volume
Part. If the Material Point is outside of the selected surfaces, then all elements with centroids outside
of the enclosed surfaces are placed within the Volume Part. If there is an enclosed volume that does
not contain any material points, its elements are not affected.
The end result is similar to that obtained using Flood Fill, but the approach is less restricted because
the mesh does not need shells or faces aligned with the enclosing surfaces. For most situations, Flood
Fill is a more robust and faster method. For situations where the mesh is not surface fitted, this option
should be used in place Flood Fill.
In Figure 431: Example of the Mark Enclosed Elements Option (p. 512), note that the elements are marked
based on the location of the centroid of each element. Note also that the region between the cylinders
is an enclosed volume but has no Material Point, so its elements remain with the original material.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
511
Edit Mesh
Figure 431: Example of the Mark Enclosed Elements Option
Enclosed Surfaces
specifies the enclosed surfaces that form a volume.
Material Points / Bodies
specifies the Material Points.
Only volume elements
allows you to assign only volume elements within the enclosed surfaces to the part of the Material Point.
When this option is disabled, shell elements also within the enclosed surfaces will be assigned to the
part of the Material Point as well.
Note
This option is enabled by default as most solvers prefer to keep volume elements and
shell elements in different parts.
An example is shown in Figure 432: Using the Only Volume Elements Option (p. 512). When the
Only volume elements option is enabled, the volume elements within the enclosed surfaces are
included in the Material Point Part. When the Only volume elements option is disabled, the surface
elements within the enclosed surfaces are also included in the Material Point Part.
Figure 432: Using the Only Volume Elements Option
Original Mesh
512
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Merge Nodes
Only volume elements Enabled
Only volume elements Disabled
Merge Nodes
The Merge Nodes option allows you to merge two nodes together to improve mesh quality while
editing the mesh. Also, disconnected parts of mesh can be merged together.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
513
Edit Mesh
Figure 433: Merge Nodes Options
The following options are available for merging nodes:
Merge Interactive
Merge Tolerance
Merge Meshes
Merge Interactive
The Merge Interactive option allows you to merge the selected nodes.
Nodes
specifies the nodes to be merged.
Figure 434: Selection of Nodes to be Merged (p. 514) shows two nodes to be merged.
Figure 434: Selection of Nodes to be Merged
Propagate Merge
propagates the merged node through the mesh until propagation is stopped by a tri element or a mesh
boundary. Figure 435: Propagate Merge (p. 515) shows the use of the Propagate merge option.
514
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Merge Nodes
Figure 435: Propagate Merge
Merge to average
only the nodes selected will be merged. Element types will be changed if necessary to perform the
merge. Using the same example as Figure 434: Selection of Nodes to be Merged (p. 514), Figure 436: Merge
to Average (p. 515) illustrates this operation.
Figure 436: Merge to Average
If the mesh is only surface mesh, you will be given the option to terminate or propagate the merged
nodes after selecting the nodes. After making the selection, that method will be used on all following
nodes merged until the function is exited by using the middle mouse button.
Ignore projection
ignores restrictions based on node projection during merging. For instance, two point projected nodes
cannot be merged because they are each confined to their respective points. This option ignores that
restriction and allows the merge.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
515
Edit Mesh
Merge Tolerance
The Merge Tolerance option allows you to merge nodes that are within a specified tolerance.
Nodes
specifies the nodes which are checked for proximity within the tolerance.
Tolerance
specifies the tolerance value. This function will attempt to merge pairs of selected nodes whose proximity
to each other is within the tolerance.
Ignore Projection
ignores restrictions based on node projection during merging. For instance, two point projected nodes
cannot be merged because they are each confined to their respective points. This option ignores that
restriction and allows the merge.
Only on Single Edges
allows you to easily select all the mesh, but will only perform node merging on the perimeter of the
surface mesh (single edges). Interior nodes, those on double or multiple edges, are not merged with
this option, even if their proximity is within the tolerance.
Note
To color-code single edges yellow, right-click on Shells > Diagnostics in the Display tree
and enable Single edges.
Merge Meshes
The Merge Meshes option allows you to merge disconnected parts of the mesh if two or more
domains are loaded and the nodes do not match up at the interface between them. These domains
are usually created separately. The merging will match up the nodes so that one-to-one connectivity
is maintained throughout the entire merged domain. Tri elements at the interface of one domain should
be no larger than roughly 3 times the tri element size of the other domain. The larger elements will be
subdivided at the interface until they reach the size of the elements of the other domain. Tetra/tetra
and tetra/hexa merges can also be done. If a tetra mesh and hexa mesh are to be merged, pyramids
will be created at the interface.
Note
The Merge Meshes option only works well when the quad elements at the interface are
close to equilateral.
The following methods are available for merging the mesh:
Merge volume meshes
is used to merge two different volume meshes (both meshes can be tetra or one can be tetra and the
other hexa).
516
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Merge Nodes
Merge surface mesh parts
allows you to specify the surface mesh parts to be merged. Select the surface mesh parts at the interface of the two separate domains. Only one part can be selected if the surface elements of the
two separate domains are in same part at the interface.
Frozen volume mesh parts
specifies the volume parts to remain fixed. The volume mesh part that is not frozen will be modified.
If one of the volume parts is hexa mesh, then that part will be frozen whether it is selected as frozen
or not.
Resolve refinements
is used to resolve couplings, which define the connectivity between elements which are not connected
node by node (hanging nodes). In order to accommodate solvers that cannot handle couplings, this
method can be used to resolve couplings using refinement and to make the mesh more conformal.
Note
Concave regions that have a coarsened interior will be filled with fine mesh. This results
in an interior refinement area with finer mesh sizes and coarse regions around it.
Standard
is the same as Pure 3D Refinement, which resolves refinements into all three directions. But this
option has smarter handling of 2.5D (surface mesh that has been extruded to become volume mesh)
cases.
Allow unstable patterns
allows non-standard refinement patterns. This improves the situation of heavy propagation of fine
elements.
Pure 3D refinement
resolves refinements into all three directions. This may lead to heavy propagation of fine elements.
See Figure 437: Resolve Refinements Options-Example 1 (p. 517) and Figure 438: Resolve Refinements Options-Example 2 (p. 518) for some examples of the different options.
Figure 437: Resolve Refinements Options-Example 1
Original Mesh
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
517
Edit Mesh
Standard and Pure 3D Refinement results in propagation of fine mesh in concave regions.
Allow Unstable Patterns
Figure 438: Resolve Refinements Options-Example 2
Original Mesh
Pure 3D Refinement
518
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Split Mesh
Standard
Allow Unstable Patterns
Split Mesh
The Split Mesh option allows you to split mesh elements at an individual level. This is one type
of refinement of elements.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
519
Edit Mesh
Figure 439: Split Mesh Options
The different options available under this menu are as follows:
Split Nodes
Split Edges
Swap Edges
Split Tri Elements
Split Internal Wall
Y-Split Hexas at Vertex
Split Prisms
Split Nodes
The Split Nodes option allows you to split nodes for triangle mesh and move them. Both nodes
will have the same constraint (point, curve or surface) as the original node. You need to specify
whether the vertex is a manifold or non-manifold one.
Non-manifold vertices are those where the outer edges of their adjacent elements do not form a closed
loop. This usually indicates elements that jump from one surface to another, forming a "tent-like"
structure. This would usually pose no problem for mesh quality but will represent a barrier in the free
domain that probably should not be there.
Figure 440: Manifold and Non-Manifold Vertices
Manifold
For manifold vertices, select the node with the left mouse button and accept the selection with the
middle mouse button. Proceed to move the selected nodes with the left mouse button. New triangles
will be created that are attached to the new node.
Non-manifold
For non-manifold vertices, select the node with the left mouse button. All surface elements connected
to that node will then be highlighted. Select the surface elements that will be attached to the new node,
520
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Split Mesh
and press the middle mouse key to accept. Then move the node with the left mouse button. No new
triangles will be created.
Figure 441: Split Node of Non-Manifold Vertex
Split Edges
The Split Edges option allows you to split selected edges into two, as well as the adjacent elements.
The following methods are available:
Selected
allows you to split the selected edges.
For this method, the following options also apply:
Propagate
The split edge operation will propagate through the mesh until the propagation is stopped by
a tri element or it exits to the ORFN region.
Project
projects the newly created nodes onto the geometry.
Split Ratio
specifies a factor between 0 and 1 to determine the location of the split along the edge.
Note
This option is available only for Hexa mesh.
Double walls
A double wall element is a tetra element that has all four nodes on the surface (two triangle faces on
the surface). The fix is to split the edge spanning the volume so each tetra element has only one face
on the surface. See the example shown below.
Figure 442: Double Wall Element
Double Wall Element
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
521
Edit Mesh
Double Wall Element Split Into Two Elements
Interior spanning
If a tetra element that is located in a gap of the geometry has its nodes on two different surfaces, the
analysis of that element may not yield sufficient results. This option splits the edges of all elements located
between the different surfaces and are not connected to a triangle element (i.e., all edges that are not
boundary edges). This will create an additional node on the edge, which will provide another face for
analysis and a more accurate result. See Figure 443: Gap with Spanning Edges (p. 523) for an example.
522
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Split Mesh
Figure 443: Gap with Spanning Edges
Gap with Spanning Edges
Interior Spanning Edges Split
All spanning
is the same as Interior spanning, except that all edges, including boundary edges, will be split.
Figure 444: All Spanning Edges Split
Swap Edges
The Swap Edges option swaps edges of two adjacent triangles. The original edge will be replaced
by an edge that connects the other two corners of the triangles, as shown in Figure 445: Swap Edges
Example (p. 524)
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
523
Edit Mesh
Figure 445: Swap Edges Example
Interactive Method
allows you to select the edge to be swapped.
Automatic Method
There are two options for the Automatic method:
• By Quality
This swaps edges to improve the mesh quality to the specified minimum quality with the specified
number of iterations. The quality metric that is used is Triangle Aspect Ratio.
• By Deviation
This swaps edges to minimize surface deviation to the specified maximum deviation with the
specified number of iterations. Quality is taken into account while swapping, and edges may be
swapped to improve the quality, provided it does not make the deviation worse. Also the quality
of the mesh may restrict some edges from being swapped even if the deviation would be improved.
In Figure 446: Swap Edges by Deviation (p. 524), the highlighted edge could be swapped to improve
the deviation value. However, because the resulting triangles are of poor quality, the edge will
not be swapped by the automatic algorithm.
Figure 446: Swap Edges by Deviation
Edge to be Swapped
Swapped Edge Resulting in Bad Quality
Elements
524
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Split Mesh
Split Tri Elements
The Split Tri Elements option allows you to split selected tri elements into three triangles. The
split location is at the centroid of the element.
An example of Split Element is shown in Figure 447: Split Element Example (p. 525)
Figure 447: Split Element Example
Split Internal Wall
The Split Internal Wall option creates pairs of coincident triangles and nodes on the internal wall.
Thus, the internal wall is logically treated as an actual wall with a “gap” in between it and the outer
wall. This option is applicable for Tetra mesh only.
Y-Split Hexas at Vertex
The Y-Split Hexas at Vertex option splits hexa elements at the vertex in a Y-Grid fashion. This
can be used to split degenerate unstructured hexas of pyramid or prism shape to improve the quality
as shown in the example below. Only elements connected at the vertex will be affected. This can be
used for surface mesh as well.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
525
Edit Mesh
Figure 448: Y-Split Hexas at Vertex Example
Split Prisms
The Split Prisms option allows you to create a few prism layers and then split them. This method
is faster and can be more robust than growing the same total number of prism layers using the Mesh
Prism option.
Selected Prism Surface Parts
specifies the selected prism surface parts. Clicking the icon
will open a window with a list of
prism surface parts. The prism layers on the selected surface parts will be split. If no shell mesh part
is selected, then all surface prism parts will be automatically selected.
Selected Prism Volume Parts
will open a window with a list of
specifies the selected prism volume parts. Clicking the icon
prism volume parts. If volume parts are selected, only the prism layers of the selected surface parts
that belong to these volumes will be split. If no volume parts are selected, the prism layers for all
the selected surface parts will be split regardless of the volume part.
Method
specifies the method for splitting prism layers.
Fix ratio
allows you to split a prism layer such that the specified Prism ratio is applied to its resulting
layers.
Fix initial height
allows you to split the first layer such that its first sub-layer is the specified Initial layer height.
Number of layers
specifies the number of layers to result from each existing layer.
Split only specified layers
allows you to split only specific prism layers.
Layer numbers (0,1,2...)
specifies which prism layers are to be split. The first prism layer is 0, the second layer is 1, etc.
526
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Move Nodes
Do not split attached pyramids
when enabled, the pyramidal elements that are attached to the prism layers will not be split. This
option is disabled by default.
Note
Using this option will result in hanging nodes in the mesh because multiple prism
side faces will be covered by one pyramid's base face. Subsequent mesh checks will
find uncovered faces and surface orientation errors. Most solvers cannot accept
these hanging-nodes, others such as ANSYS Fluent prefer pyramids this way because
they will have better aspect ratios than if they were split thin along with the adjacent
prisms.
Move Nodes
The Move Nodes options are used to move nodes using various methods. Nodes projected to a
prescribed point will not be able to be moved. Nodes that are projected to a curve will be constrained
to active curves. Nodes projected to a surface will be constrained to active surfaces. Internal volumetric
nodes can move along the plane defined by the screen. The different options for moving nodes are
shown below.
Figure 449: Move Nodes Options
Interactive
The Interactive option allows you to select the node with the left mouse button and move it interactively.
Move Nodes Type
You can select Single to move single nodes, or Multiple, to move multiple nodes simultaneously.
Select
specifies the nodes to be moved.
Allow Inversion
if enabled, node movement will be allowed to invert or twist elements. If disabled, node movement will
be constrained so that elements cannot be twisted.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
527
Edit Mesh
Project to
• All geometry
projects nodes to the nearest geometry entities.
• Active Parts
project the nodes of active parts only. Active parts include those that are enabled in the Model
tree but not visible on the screen.
• None
nodes will not be projected.
Exact
The Exact option allows you to modify the coordinates of selected nodes. The nodes may be
moved individually or in relation to a reference location.
Multiple nodes can be selected and modified at the same time. Typically, this function is used to
modify a number of nodes to one specific coordinate, for example Y=0, to ensure a true symmetry
plane.
Method
Offset
allows you to select the coordinate direction and units of distance to offset the selected nodes.
Position
allows you to select the Reference location of the nodes to be moved and based on its position,
modify the X, Y, and Z (or R, Theta, and Z) directions of the selected nodes. The reference location
can either be an existing node, or a position on the screen.
Set
specifies the appropriate coordinate system and direction to move the nodes.
• Cartesian Coordinate System
You can select the direction to move the nodes: X, Y, or Z and enter the number of units of distance.
• Cylindrical Coordinate System
You can select the direction to move the nodes: R, θ, or Z and enter the number of units of distance.
Select Nodes
specifies the nodes selected. Select the nodes to be moved and click Apply. After selecting a node, its
location coordinates will be displayed in the message window.
Offset Mesh
528
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Move Nodes
Elements
specifies the shell elements to be offset. Select the shell elements to offset in the normal direction. The
normal direction of the elements, both the selected elements and the elements connected to those selected, must be consistent.
Distance
specifies the distance to offset the selected elements.
Note
Offset will change the location of nodes, but will not change the number (or definition)
of selected elements. The new node location will be based on the normal direction of
all the elements connected to this node.
Align Nodes
Reference Direction
defines the reference direction. Select two nodes to indicate the reference direction.
Nodes
specifies the nodes to be aligned by the specified reference direction.
Redistribute Prism Edge
The Redistribute Prism Edge option allows you to redistribute prism layers to a specified constant
first layer thickness or a specified growth ratio spanning the local prism column thickness. This option
works with prism layers as well as a combination of prism and hexa inflation layers. A prism layer is
constrained by three parameters which calculate the fourth (see the Prism Meshing Parameters section).
Total Height is set during prism growth, and can be varying if you left the Initial Height as zero. The
number of layers can be set during the prism growth or adjusted with split prisms (see the Split Prisms
option). An initial Height Ratio is set in the Prism Meshing Parameters, but can be adjusted by this
Redistribute Prism Edge option. With Total Height and Number of Layers now fixed, you can use
this option to adjust the Initial Height or Height Ratio and force the calculation of the other.
Note
The redistribution will not move nodes connected to pyramids, but will redistribute other
prisms in that layer, and above.
Method
Fix ratio
allows you to specify a constant (fixed) growth ratio for redistributing the prisms. Note that the redistribution is calculated for each column of prisms; if the prism total height varies, the initial height
will vary in order to maintain a fixed ratio.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
529
Edit Mesh
Figure 450: Prism Redistributed by Ratio
Fix initial height
allows you to specify the desired initial height value of the prism layers in absolute units of the
model, not the reference size. Note that the redistribution is calculated for each column of prisms,
so specifying an initial height may result in varying ratios if the individual column Total Height
varies.
530
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Move Nodes
Figure 451: Prism Redistributed by Initial Height
Redistribute locked prism elements
when enabled, allows you to redistribute prism elements which have been locked (refer to Lock/Unlock
Elements (p. 534) for details). When this option is disabled (default), the locked prism elements will be
ignored during the redistribute operation.
Locked prism elements, if any, will be reported in the message window, when the Redistribute
Prism Edge DEZ is opened. Locked elements can also be highlighted in the display by enabling
Mesh > Locked Elements in the Display Tree.
Use local parameters
allows the use of the initial height or growth ratio defined locally on curves, surfaces, or parts for the
prism mesh redistribution. If the Use local parameters option is enabled, and the local values are either
not set or set to zero, the default value for the initial height or growth ratio will be used.
In Figure 452: Prism Redistributed with the Use local parameters Option (p. 531), the prism layer is
redistributed based on initial height. The Use local parameters option is used, and the prism mesh
redistribution accounts for the initial height set locally on the detail surface.
Figure 452: Prism Redistributed with the Use local parameters Option
Before Redistribution
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
531
Edit Mesh
After Redistribution
Project Node to Surface
The Project Node to Surface option allows you to project nodes to surfaces. Select from the following methods.
Nearest
Projects selected nodes to the nearest surfaces.
Direction
Projects selected nodes in a specified direction. If there is no surface in the specified direction, the node
will be projected to the nearest surface along the specified vector.
Explicit
Specify the X, Y, and Z offsets to define the vector for the direction that the node is to be projected.
Vector
Select two points to define the vector for the direction that the node is to be projected.
532
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Move Nodes
Always normal
If enabled, then the node will be projected only if the angle between the surface normal and the defined
vector is less than 5 degrees. If the angle is greater than 5 degrees, the node will not be projected and
a message will be displayed in the message window.
Project to
Specify whether to project nodes to All Parts, or to only Active Parts.
Note
Active parts are determined by the Parts branch of the tree. Active status is not affected
by enabling and disabling entities or blanking specific entities. If you do not want nodes
to be projected to certain entities, you may need to place those entities into a separate
part and disable it (deactivate it) in the model tree.
Project Node to Curve
The Project Node to Curve option allows you to project the selected node to the nearest curve
or a specified curve. The movement of the node will then be restricted along the curve.
Nodes to Project
Select the nodes to be projected.
Project by Tolerance
If enabled, all of the selected nodes that are closer to the selected curves by the specified tolerance are
projected and moved to the curves. If disabled, the selected nodes will be projected and moved to the
nearest curve.
Tolerance
Specify the tolerance value.
Curve(s)
Select the curves that the nodes are to be projected to.
Select
Select the nodes from the display.
Project Node to Point
The Project Node to Point option allows you to project a selected node to a particular point.
Nodes to Project
Select the nodes to project.
Projection Method
• Explicit
To project nodes to a specified point.
– Point
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
533
Edit Mesh
To project the node to a selected point.
– Self
To project the node to the point at the same location.
• By Tolerance
All of the selected nodes that are closer to the selected points by the specified tolerance are
projected and moved to the points.
Un-Project Nodes
The Un-Project Nodes option allows you to un-project a projected node. The node will then be
allowed unrestricted movement.
Select
Select the nodes from the display.
Lock/Unlock Elements
The Lock/Unlock Elements option allows you to lock or unlock elements. Locked elements will
prevent automatic operations such as mesh smoothing or coarsening from moving the nodes. Locked
elements can be highlighted by enabling Mesh > Locked Elements in the Display Tree.
Snap Project Nodes
The Snap Project Nodes option allows you to project nodes to their associated geometry. Select
from the following methods.
Nearest
Projects selected nodes to the closest location on its associated geometry.
Direction
Projects selected nodes to their associated geometry along the specified direction.
Explicit
Specify the X, Y, and Z offsets to define the vector for the direction that the node is to be projected.
Vector
Select two points to define the vector for the direction that the node is to be projected.
Always normal
If enabled, then the node will be moved only if the angle between the surface normal and the defined
vector is less than 5 degrees. If the angle is greater than 5 degrees, the node will not be projected and
a message will be displayed in the message window.
534
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Transform Mesh
Project to
Specify whether to project nodes to All Parts, or to only Active Parts.
Note
Active parts are determined by the Parts branch of the tree. Active status is not affected
by enabling and disabling entities or blanking specific entities. If you do not want nodes
to be projected to certain entities, you may need to place those entities into a separate
part and disable it (deactivate it) in the model tree.
Update Projection
The Update Projection option updates the projection of all nodes in the mesh. Nodes will be
projected to a surface, curve or point.
Project Nodes to Plane
The Project Nodes to Plane option allows you to project a node to a plane.
Note
This option is similar to the Project Nodes to Surface option, except it does not require a
surface and offers less control over how the projection is done.
Select
specifies the nodes selected for projection.
Plane Setup Method
specifies the method for defining the plane.
Point and Plane
defines the plane by a point and the normal. Select the point and specify the normal to the plane.
Three Points
defines a plane passing through the three specified points.
Transform Mesh
The Transform Mesh option can be used for transforming a portion or all of the mesh. This is
useful when the mesh domain has symmetry. One section of the domain can be meshed and then rotated
or translated in order to cover the complete domain.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
535
Edit Mesh
Figure 453: Mesh Transformation Tools Options
The different options are shown in Figure 453: Mesh Transformation Tools Options (p. 536). It is possible
to use more than one method at a time.
Translate
Rotate
Mirror
Scale
Translate and Rotate
Translate
The Translate option is used to move elements laterally without rotation.
Select
specifies the elements for translation.
Copy
If enabled, the original mesh will be kept intact, and an exact copy of the mesh with duplicated nodes
and elements will be generated at the selected location.
Number of copies
specifies the number of copies to generate. If at least one copy is generated, than you have the option
to Merge nodes.
Increment Parts
To add the newly created copies of mesh to an existing part, click on the Select Parts icon. Select the
part name from the window that opens up. If no part is selected, then the copies will be added to a
new part.
Merge nodes
automatically merges duplicated nodes when the mesh copies are adjacent to or overlapping one another. This uses a merge nodes tolerance setting to control the merge. Selecting merge nodes activates
the options for setting the Tolerance Method and Deleting duplicate elements.
Tolerance Method
allows you to determine how the merge tolerance should be specified. The Automatic option is recommended and will automatically calculate the tolerance as one tenth of the minimum edge length of all
selected elements. If the User defined option is chosen, then an absolute tolerance can be set in the
Tolerance field. The projection of the nodes are ignored during merging. There is also some internal
code to prevent collapsing edges between nodes within the tolerance.
536
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Transform Mesh
Delete duplicate elements
deletes duplicated elements if after merging nodes the copies overlap or are adjacent.
Translation Method
• Explicit
Enter the offset distance in the X, Y, and Z directions to translate the selected elements.
• Vector
Define a vector by selecting two points. Elements will be moved in the direction of the defined
vector.
Rotate
The Rotate option is used to rotate elements about a defined point. This is an extremely useful
tool while meshing a circular domain. Mesh only one section of the domain, and rotate it to generate
the complete domain.
Select
specifies the elements for rotation.
Copy
If enabled, the original mesh will be kept intact, and an exact copy of the mesh with duplicated nodes
and elements will be rotated as specified.
Number of copies
specifies the number of copies to generate. If at least 1 copy is generated, than you have the option to
Merge nodes.
Increment Parts
To add the newly created copies of mesh to an existing part, click on the Select Parts icon. Select the
part name from the window that opens up. If no part is selected, then the copies will be added to a
new part.
Merge nodes
automatically merges duplicated nodes when the mesh copies are adjacent to or overlapping one another. This uses a merge nodes tolerance setting to control the merge. Selecting merge nodes activates
the options for setting the Tolerance Method and Deleting duplicate elements.
Tolerance Method
allows you to determine how the merge tolerance should be specified. The Automatic option is recommended and will automatically calculate the tolerance as one tenth of the minimum edge length of all
selected elements. If the User defined option is chosen, then an absolute tolerance can be set in the
Tolerance field. The projection of the nodes are ignored during merging. There is also some internal
code to prevent collapsing edges between nodes within the tolerance.
Delete duplicate elements
deletes duplicated elements if after merging nodes the copies overlap or are adjacent.
Rotation Axis
specifies the axis of rotation. Select the axis of rotation as one of the coordinate axes, or a vector defined
by two selected points.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
537
Edit Mesh
Angle
Enter the angle of rotation.
Center of Rotation
Define the point about which the elements will be rotated.
• Origin
The origin of the model's global coordinate system, (0 0 0).
• Centroid
The center of the bounding box of the selected elements.
• Selected
Any point selected from the display.
Mirror
The Mirror option relocates the mesh domain to its mirror image across a plane. A copy of the
selected mesh can also be made as a mirror reflection while the original mesh is kept intact.
Select
specifies the elements to be mirrored.
Copy
If enabled, the original mesh will be kept intact, and an exact copy of the mesh with duplicated nodes
and elements will be generated at the selected location. This will activate the option to Merge nodes.
Increment Parts
To add the newly created copies of mesh to an existing part, click on the Select Parts icon. Select the
part name from the window that opens up. If no part is selected, then the copies will be added to a
new part.
Merge nodes
automatically merges duplicated nodes when the mesh copies are adjacent to or overlapping one another. This uses a merge nodes tolerance setting to control the merge. Selecting merge nodes activates
the options for the Tolerance Method and Delete duplicate elements.
Tolerance Method
allows you to determine how the merge tolerance should be specified. The Automatic option is recommended and will automatically calculate the tolerance as one tenth of the minimum edge length of all
selected elements. If the User defined option is chosen, then an absolute tolerance can be set in the
Tolerance field. The projection of the nodes are ignored during merging. There is also some internal
code to prevent collapsing edges between nodes within the tolerance.
Delete duplicate elements
deletes duplicated elements if after merging nodes the copies overlap or are adjacent.
Reflection Plane Axis (Normal)
specifies the axis or vector that defines the normal to the mirror plane. The vector may pass through
the plane.
538
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Transform Mesh
Point of Reflection
Select the point about which the selected mesh elements are to be reflected.
• Origin
The origin of the model's global coordinate system, (0 0 0).
• Centroid
The center of the bounding box of the selected elements.
• Selected
Any point selected from the display.
Scale
The Scale option can be used to re-size the selected mesh domain by specifying factors in all three
coordinate directions.
Copy
If enabled, the original mesh will be kept intact, and an exact copy of the mesh with duplicated nodes
and elements will be resized as specified.
Increment Parts
To add the newly created copies of mesh to an existing part, click on the Select Parts icon. Select the
part name from the window that opens up. If no part is selected, then the copies will be added to a
new part.
Scale Mesh Factors
Enter the scale factor for the three directions X, Y, and Z.
Center of Transformation
Select the base point for scaling.
• Origin
The origin of the model's global coordinate system, (0 0 0).
• Centroid
The center of the bounding box of the selected elements.
• Selected
Any point selected from the display.
Translate and Rotate
The Translate and Rotate option allows you to translate and rotate the mesh simultaneously. The
reference location and target locations can be defined by 3 points, a curve or LCS and the mesh is
translated and rotated to match.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
539
Edit Mesh
Copy
If enabled, a copy of the selected entities will be created in the new location.
IncrementParts
To add the newly created copies of entities to a new part, click the IncrementParts icon. A window will
open with the list of the parts of the selected entities. If a part is selected, the new entities will be placed
in a new part named [old_part_name]_0. For multiple copies, each copy will be placed in a separate
part, for example, MESH_1, MESH_2, MESH_3, etc.
Translate and Rotate Method
The three options for method are as follows:
3 points –> 3 points
Select six points in all. The first three points will be used as the reference for the entity to be transformed. The second set of three points is used to define the transformation. The result will match
the first points of both sets, and the direction from the first to the second point, and the plane
defined by the third point.
Curve –> Curve
Select two curves. The first curve is used as a reference for the entity to be transformed. The second
curve is used to define the transformation. The result will match the beginning (parameter = 0) of
both curves, the direction from parameter 0 to 0.5, and the plane defined by the end (parameter 1)
of the curves. A curve used to define the transformation can be included in the entities selected to
be transformed.
LCS –> LCS
Click Show LCS to view any defined coordinate systems. Select two local coordinate systems.
The result will match the origins and align the axes of the first LCS to the second LCS.
Convert Mesh Type
The Convert Mesh Type options are used to change one element type to another.
Figure 454: Convert Mesh Type Options
The available options are shown in Figure 454: Convert Mesh Type Options (p. 540).
Tri to Quad
Quad to Tri
Tetra to Hexa
All Types to Tetra
Shell to Solid
Create Mid Side Nodes
Delete Mid Side Nodes
540
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Convert Mesh Type
Tri to Quad
The Tri to Quad option allows you to convert a triangular surface mesh to quadrilateral surface
mesh. This is applicable for all visible surfaces.
Elements
specifies the triangular elements to be converted.
Surface Projection
contains options for projecting the newly created elements to the nearest entity of the geometry.
Quadrization
If this option is enabled, then the quadratic elements will be converted.
Note
Quadrization can only be done on the entire mesh.
Mesh Improvement
improves mesh quality after conversion. Select from the following range:
• 0 = No improvement steps.
• 1 = Stop improvement if less than 20% of the total elements are free triangles. This is the default
value.
• 2 = Stop improvement if less than 2% of the total elements are free triangles.
• 3 = Perform as many improvement steps as needed to complete the conversion.
Max Skewness
specifies the maximum allowable skewness for conversion.
Max Warpage
specifies the maximum allowable warpage for conversion.
Quad to Tri
The Quad to Tri option divides each quad element into two triangles. The diagonal edge will be
placed so as to make the minimum internal angle as large as possible.
Method
• Shells Only
divides the quad elements only into triangle elements.
– Shells
specifies the shell elements to be converted.
• Through Hexas
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
541
Edit Mesh
splits the attached hexa elements into two prisms and propagates the split into the volume. This
will result in a column of hexas split into prisms.
– Split Face Nodes
splits the face nodes of quad element. Select diagonally opposite nodes of the quad element.
Tetra to Hexa
The Tetra to Hexa option allows you to convert tetrahedral mesh to hexahedral mesh.
Method
• 1 tetra to 4 hexa
This option will subdivide selected tetra elements into four hexa elements by creating a node at
the center of the tetra, at the centroid of the tri faces of the tetra. The 4 hexa elements are created
by connecting these nodes.
Figure 455: Example of 1 Tetra to 4 Hexa
Project nodes
If disabled, the midface nodes that are created will be left linear and will not be projected. If
enabled, the node will be projected in the manner determined by the Normal to elements
option.
Normal to elements
If this is enabled, the node will be projected normal to the triangle face. If the angle between
the normal direction and the projected point is greater than 5 degrees, then the node will
be left unprojected. If this option is disabled, the node will be projected to the closest surface.
The Project nodes option will project new face nodes onto the geometry.
• 12 tetra to 1 hexa
Works on Octree generated mesh to convert groups of 12 tetras to 1 hexa element.
Note
This only works on Octree generated mesh because that algorithm started with Cartesian
mesh which it converted to tetras with a 1 to 12 process.
542
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Convert Mesh Type
The primary control is to specify the Min aspect ratio for the newly created hexa elements,
clumps of tetras that would produce a hexa of lower quality are not converted. Pyramids are used
to create a conformal interface between converted hexas and the surrounding tetra elements.
Uniform regions of Octree mesh convert most effectively. Octree size transition regions cannot
be converted; use density boxes to control where the size transitions happen (away from critical
regions). Also, reducing the number of transitions (more uniform sizing) can result in a higher
conversion rate. If the mesh against the surface is smoothed, it may not convert as well. You can
disable surface smoothing (Octree tetra global mesh parameter) if you want hexas to the
boundary. You can select either All tetra elements or elements from selected Volume element
parts for the conversion.
In Figure 456: Example for Conversion of 12 Tetra to 1 Hexa (p. 543), the Octree tetra mesh for a
disk drive (figure (A)) is converted to an Octree hexa hybrid mesh (figure (B)). This example has
a large number of transitions as well as prism elements. These transitions, smoothing, and non
Octree element types reduce the conversion rate. From the count of element types before and
after the conversion (TETRA_4 : 4220472 converted to TETRA_4 : 2004355 and HEXA_8 : 179262),
note that the final number of elements is reduced by approximately half without coarsening the
mesh.
Figure 456: Example for Conversion of 12 Tetra to 1 Hexa
(A) Octree Tetra Mesh With Prisms for the Disk
Drive Before Conversion
(B) Octree Hexa Hybrid Mesh for the Disk Drive
After Conversion
Element types:
Element types :
NODE : 150
NODE : 150
LINE_2 : 11493
LINE_2 : 11726
TETRA_4 : 4220472
TETRA_4 : 2004355
TRI_3 : 445817
HEXA_8 : 179262
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
543
Edit Mesh
PENTA_6 : 1788782
TRI_3 : 434319
QUAD_4 : 2898
PENTA_6 : 1748756
PYRA_5 : 11186
QUAD_4 : 11786
PYRA_5 : 176324
Note
Only tetras are converted, not prisms. Also, prisms cannot grow into hexa elements,
so you need to maintain a layer of tetras near walls where you intend to grow prisms
or insert prism layers before using the 12 Tetra to 1 Hexa. conversion.
Aligning the Octree mesh with the principal model directions (such as along a pipe or wall) can
further increase the conversion rate and result in hybrid mesh that is better aligned with the flow.
Note
The Use active coordinate system option must be enabled when converting oriented
Octree tetra mesh to oriented hexa hybrid mesh.
Figure 457: LCS Oriented Octree Tetra Mesh Converted to LCS Oriented Hexa
Mesh
All Types to Tetra
The All Types to Tetra option converts all element types into tetra elements.
All to Tetra
Converts all elements into tetra elements. The selected elements do not have to be a specific initial
element type.
Selected elements
If enabled, you can select which mesh elements to convert to tetra elements. Otherwise the full mesh
of all types of volume elements will be converted to tetra elements.
544
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Convert Mesh Type
Make consistent
If enabled, then elements that are attached to mesh elements that are converted to tetra will be
automatically edited to keep the mesh consistent.
1 Prism to 3 Tetra
Subdivides each prism element into three tetra elements whose edges extend along the quad faces of
the former prism.
Figure 458: 1 Prism to 3 Tetra
Shell to Solid
The Shell to Solid option converts 2D elements into 3D elements.
Selected elements
If enabled, you can select which 2D elements are to be extruded into 3D elements.
Thickness
allows you to specify a thickness value of the 3D elements.
Square corners
If enabled, square corners will be formed. If elements at an L-bracked are being extruded, then by default
the corner will be rounded, as the node extrusions are given an absolute valued based on thickness.
This function will cause the node extrusions to be multipled by a factor of the angle, so that a sharp
corner results. See Figure 459: Shell to Solid Conversion Without Sharp Corners Option (p. 546) and Figure 460: Shell to Solid Conversion With Sharp Corners Option (p. 546).
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
545
Edit Mesh
Figure 459: Shell to Solid Conversion Without Sharp Corners Option
Figure 460: Shell to Solid Conversion With Sharp Corners Option
Hexa at T-connections
If enabled, hexa elements will be formed at T-connections.
Create Mid Side Nodes
The Create Mid Side Nodes option allows you to create mid side nodes on all the elements of
the mesh, as shown in Figure 461: Create Mid Side Nodes Example (p. 547).
546
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Convert Mesh Type
Figure 461: Create Mid Side Nodes Example
Mid face node
If enabled, nodes will be created at the center of each face.
Create node on interface
This option is used when creating mid side nodes on the interface between selected elements and the
elements attached to them. If enabled, then the edges of the attached elements will also become
quadratic. If disabled, then the edges that are common to both the selected elements and attached
elements will remain linear.
Project to geometry
If enabled, the newly created nodes will be projected to the nearest geometry.
Calculate projection
When a quadratic node is created, it will be projected to all marked curves or surfaces of its linear
neighbors, and also the minimum projection will be calculated. The actual projection will be compared
to the minimum projection and checked to see if it is within the specified tolerance. If not, the minimum
projection will be used.
Check max
If any of the following three conditions is enabled, then the mid side node that exceeds the required
condition(s) will not be projected. For the following max conditions refer to Figure 462: Check Max
Conditions (p. 548).
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
547
Edit Mesh
Figure 462: Check Max Conditions
• Check deviation
The distance between the end nodes B1 and B2, multiplied with the value of the Midnode max
deviation results in R. Next, imagine a line through mid node D, and perpendicular to line B1B2. If the position of the projected node falls outside a distance R from the line, then the node
will be moved on the geometry so that it falls within this range. If this is not possible, it will not
be projected.
• Check angle
This refers to the angles (A1 and A2) between the positions of the element edge before and after
projection. If projecting a mid node would create an angle above the Midnode max angle, then
the mid node will not be projected.
• Check chord
The distance between the chord (B1-B2) and the projected mid node is restricted to the specified
Max deviation from chord, defined in terms of % of the chord length. If this distance is exceeded
then the node will be moved on the line (which is defined by the projected mid node and its
projection to the chord) to the position of the maximum deviation.
Only selected elements
If enabled, you may select the elements to which the operation will be applied.
Tetra 10 elements
• Standard check
If enabled, each projected mid node will be checked for negative values on the determinants at
Gaussian integration points of all Tetra 10 elements to which the mid node belongs. If this check
fails for at least one element then the dimension of the mid node will be increased, i.e., if it was
projected to curves it will now be projected to surfaces, and then this check will be done again.
Or if the mid node had been projected to surface, it will now be linearized.
• Strong check
If enabled, a stronger check with respect to the Tetra 10 elements of the mid node will be done.
Automatic refinement
This is available only in the case of tetrahedral elements. For all elements a temporary mid node will be
created on each element edge (with projection) and it will be checked with respect to some diagnostic
548
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Adjust Mesh Density
criteria for the attached tetrahedrals. If any of the criteria is not fulfilled, the element edge will be refined.
In general it is not advisable to use this option.
Smooth refinement
If enabled, the mesh will be smoothed with 5 iterations to reach an aspect ratio of 0.25 for the tetra
elements.
Delete Mid Side Nodes
The Delete Mid Side Nodes option allows you to delete mid side nodes. Mid Side Nodes can be
deleted from the entire mesh or from selected elements/nodes in two different ways.
Elements or Nodes
Either elements or nodes can be selected.
Selected elements/nodes
If enabled, it allows you to delete mid side nodes from selected elements or to delete selected quadratic
nodes.
Convert Quadratic elements to multiple Linear elements
If disabled, this option will simply delete the midside/midface nodes without disturbing any other nodes.
If enabled, this option will refine the mesh in such a way that all midside/midface nodes will become
mesh nodes.
Keep interface node
This option is used when mid side nodes are deleted from selected elements that are attached to other
quadratic elements. If enabled, then the selected elements will become linear, but nodes on the interface
of the selected elements and the attached quadratic elements will remain.
Adjust Mesh Density
The Adjust Mesh Density options allow you to refine or coarsen the entire mesh or only at a
particular location.
Figure 463: Adjust Mesh Density Options
The following options related to this feature are shown in Figure 463: Adjust Mesh Density Options (p. 549).
Refine All Mesh
Refine Selected Mesh
Coarsen All Mesh
Coarsen Selected Mesh
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
549
Edit Mesh
Refinement
Refines, or subdivides, elements. This applies only to triangular surface elements, quads, and tetra elements. While refining triangular surface elements, if tetra elements are connected to the tri surface elements, the tetra's edges connected to the tri's will be subdivided so that the mesh remains conformal.
Similarly, refining tetra elements will subdivide adjacent tetra or tri element edges so that the mesh remains conformal.
Coarsening
Coarsens a tetrahedral or tetra/prism hybrid mesh. Elements in the mesh will be coarsened by collapsing
edges (merging nodes) and removing degenerate elements, but no operation will be performed that
would yield an element with an aspect ratio worse than what is specified. The degree of coarsening
(number of elements before vs. number of elements after) is automatically determined and reported in
the Message window. Disconnected vertices are automatically deleted after coarsening.
Refine All Mesh
The Refine All Mesh option refines all of the visible displayed elements. The different methods
are described below.
Pure refinement
Refines the mesh by splitting the edges and then performing swapping to improve element quality.
Note
In cases where adjacent tetra are connected by an edge only (not a face), the edge is
split, but then cannot be swapped to improve the quality. This may result in lower element
quality (see Figure 464: Refinement by Edge Splitting (p. 550)).
Figure 464: Refinement by Edge Splitting
Steps
specifies the number of refinement steps to be completed.
Project Nodes
projects the new nodes of the subdivided elements on the geometry.
Note
It is necessary to have a Tetin file loaded for the nodes to be projected.
550
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Adjust Mesh Density
On Surface Only
allows you to refine only the surface mesh. This option only splits edges on the surface and then
performs swapping to improve element quality.
Tip
The On Surface Only option is useful when you need to refine only the surface mesh.
As the volume mesh is not refined, the quality problems seen in Figure 464: Refinement
by Edge Splitting (p. 550) will be avoided.
By Mid Side Nodes Only
refines the mesh using mid-side nodes. This option produces a more uniform mesh (see Figure 465: Refinement by Mid Side Nodes Only (p. 551)).
Figure 465: Refinement by Mid Side Nodes Only
Note
The By Mid Side Nodes Only option can only be used globally, and not for local
refinement.
Surface deviation
For surface elements (triangles), this option subdivides the elements based on the surface deviation
computed. The surface deviation is the distance from the centroid of the element to the surface, in the
direction normal to the surface as illustrated in Figure 466: Surface Deviation (p. 551).
Figure 466: Surface Deviation
Max Surface Deviation
specifies the maximum allowable surface deviation. If the computed surface deviation is greater than
the defined value, the element will be subdivided.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
551
Edit Mesh
Max Steps
is the number of refinement steps. The number of sub elements that are created is determined by
the formula, 4n, where n is the Max steps value. One step will break an element into 4 sub elements,
2 will yield 16 sub elements, etc.
On Surface Only
allows you to refine only the surface mesh.
Edge length
• Max edge length
specifies the maximum edge length after refinement.
• Weak refinement
If enabled, the refinement will not be propagated strongly into the neighboring regions.
• Max steps
the number of refinement steps.
• Project nodes
projects the new nodes of the subdivided elements on the geometry.
Note
It is necessary to have a Tetin file loaded for the nodes to be projected.
Refine Selected Mesh
The Refine Selected Mesh option refines selected elements from the mesh.
The methods for refining selected mesh are the same as described in Refine All Mesh (p. 550).
Coarsen All Mesh
The Coarsen All Mesh coarsens all of the visible displayed elements.
Min aspect ratio
the minimum aspect ratio (the circumsphere ratio) allowed for the resulting coarsened elements. The
lower the minimum aspect ratio, the more elements in the mesh will be coarsened.
Max size
is the largest tetra size allowed by coarsening. Only elements below this size will be coarsened, and only
up to this size. The larger this value, the more the mesh will be coarsened.
552
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Adjust Mesh Density
Max surface deviation
For surface elements (triangles), this option coarsens the elements based on the distance from the
centroid of the element to the surface, in the direction normal to the surface. If this distance is less than
the defined Max Surface Deviation, the elements will be coarsened.
Number of Iterations
is the number of smoothing iterations. Smoothing will be automatically performed after the coarsening
process if this number is nonzero.
Coarsen surface
If this is enabled, then surface triangular elements will also be coarsened. If disabled, only tetra and
prism volume elements are coarsened.
Maintain surface sizes
If this is enabled, it will attempt to coarsen up to the sizes prescribed on the geometry (points, curves
and surfaces). Local coarsening can be achieved this way by only changing tetra sizes on specific entities.
When tetra mesh is generated, the elements are divided to these sizes. So if no tetra sizes are changed
after generating the tetra mesh, then enabling this option will prevent any coarsening from being performed.
Parts to freeze
specifies the parts which will not be coarsened. Nodes of these parts will remain fixed. If there is only
one volume part, and this part is frozen, no coarsening will be performed.
Coarsen Selected Mesh
The Coarsen Selected Mesh option coarsens selected elements from the mesh.
Note
This feature works for quad and quad dominant mesh, but not all tri mesh. In order to coarsen
selected all tri or mostly tri mesh, freeze the parts that are not to be coarsened and then use
Coarsen All Mesh.
Elements
specifies the elements selected for coarsening.
Min aspect ratio
the minimum aspect ratio (the circumsphere ratio) allowed for the resulting coarsened elements. The
lower the minimum aspect ratio, the more elements in the mesh will be coarsened.
Max size
is the largest tetra size allowed by coarsening. Only elements below this size will be coarsened, and only
up to this size. The larger this value, the more the mesh will be coarsened.
Max surface deviation
For surface elements (triangles), this option coarsens the elements based on the distance from the
centroid of the element to the surface, in the direction normal to the surface. If this distance is less than
the defined Max Surface Deviation, the elements will be coarsened.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
553
Edit Mesh
Number of Iterations
is the number of smoothing iterations. Smoothing will be automatically performed after the coarsening
process if this number is nonzero.
Maintain surface sizes
If this is enabled, it will attempt to coarsen up to the sizes prescribed on the geometry (points, curves
and surfaces). Local coarsening can be achieved this way by only changing tetra sizes on specific entities.
When tetra mesh is generated, the elements are divided to these sizes. So if no tetra sizes are changed
after generating the tetra mesh, then enabling this option will prevent any coarsening from being performed.
Renumber Mesh
The Renumber Mesh option renumbers all of the elements so that the cell numbering from minimum to maximum is along a defined direction. This is used to speed up the computation of the solution.
Figure 467: Renumber Mesh Options
The different options are shown in Figure 467: Renumber Mesh Options (p. 554).
User Defined
Optimize Bandwidth
User Defined
Renumber Elements
enables renumbering of the elements.
Starting element number
starts element numbering from the specified number.
Element number range
gives range of existing element numbers.
Renumber Nodes
enables the renumbering of the nodes.
Starting node number
starts node numbering from the given node number.
Node number range
gives range of existing node numbers.
554
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Assign Mesh Thickness
Method
• By Parts
renumbers elements and/or nodes one part at a time.
• All elements/nodes
renumbers all the elements and nodes.
• Selected Elements
renumbers only the selected elements.
• Selected nodes
renumbers only the selected nodes.
Direction
the global axes direction in which to renumber elements or nodes. For the X axis, the direction is 1 0 0.
Skip 0-numbered Elements and Nodes
If enabled, the 0-numbered elements and nodes will be skipped for renumbering.
Optimize Bandwidth
The Optimize Bandwidth option renumbers nodes to minimize the bandwidth of the element/node
matrix.
Iterations
number of iterations to reorder node numbers.
Profile
minimizes the number of elements in the profile of the global system matrix. This option supports
solvers which eliminate operations on zeros outside the profile using a skyline storage scheme.
Bandwidth
minimizes the bandwidth of the global system matrix.
Assign Mesh Thickness
The Assign Mesh Thickness options available are shown in Figure 468: Adjust Mesh Thickness
Options (p. 556)
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
555
Edit Mesh
Figure 468: Adjust Mesh Thickness Options
Note
Uniform shell thickness can also be applied under Properties > Define 2D Element properties, but that definition is stored in an attribute file and not in the mesh. Thickness applied
here becomes the default when setting up properties for 2D elements. Variable thickness
should always be applied here before defining 2D element properties.
Method
• Calculate
Mesh thickness will be assigned automatically to each node of the surface element from the
thickness information stored on the surface geometry at that location. This thickness can come
automatically from the midsurfacing process (including varying thickness) or be applied manually
with Repair Geometry > Adjust varying thickness.
The thickness is defined normal to the surface in both directions. The thickness can be viewed
from the display tree by right clicking Mesh > Shells > Shell Thickness.
Calculate from solid
allows you to extract the thickness information of shell elements from the solid geometry around
the shells. This is used when the midsurface thickness information is not present on the surfaces.
To use this, load the original solid geometry. The shells mesh should be within this geometry. Select
the part of the solid to calculate the thickness. This method uses the nearest point projection for
thickness calculation. The average of the thickness in both directions is used for each node.
Piercing
is an alternative method for calculating the thickness from a solid. It may be preferable for surfaces
with greater thickness where the nearest point method may not be appropriate.
Note
The nearest point projection and piercing methods lead to similar results for surfaces
with small thickness.
• Remove
Removes the mesh thickness assigned to the nodes of the surface elements.
556
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Reorient Mesh
• Modify selected nodes
Individual nodes of surface element can be assigned a specified thickness.
Reorient Mesh
The Reorient Mesh option changes the direction of the normals of selected elements or all the
elements in a particular manner.
Figure 469: Reorient Mesh Options
The options for reorienting the mesh are shown in Figure 469: Reorient Mesh Options (p. 557).
Reorient Volume
Reorient Consistent
Reverse Direction
Reorient Direction
Reverse Line Element Direction
Change Element IJK
Reorient Volume
Reorients the normals of the displayed elements to point into the volumetric domain (inwards) or
away from the domain (outwards). By default, all of the face normals will be reoriented to point into
the domain, unless there are orientation errors.
Outwards
If toggled ON, all the normals will be oriented in the outward direction.
Reorient Consistent
Aligns all the normals of the displayed elements to have the same orientation (inwards or outwards)
as the selected element. This works for all elements connected to the domain of the selected surface
element. Any mesh disconnected from this mesh will not be affected. This operation will work across
different parts.
Active parts
If toggled ON, only the elements in the parts that are turned ON in the Parts Display Tree will be
reoriented.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
557
Edit Mesh
Reverse Direction
Reverses the normals of the selected elements.
Elements
To select the elements from the display whose orientation is to be changed.
Filter by Screen Normal
This will reverse the normal of only those elements whose normal is in the opposite direction with respect
to the screen view factor.
Reorient Direction
Changes the normal direction of the displayed elements according to a specified X Y Z vector.
Since a face normal can only point in two possible opposing directions, the normal will point in the
direction closest to that of the specified vector.
Reverse Line Element Direction
Reverses the line element direction.
Change Element IJK
There are four different methods available to change the IJK indices of an element.
IJK –> KIJ
For the selected element(s), the indices will be changed from IJK to KIJ.
Set Origin
For the selected element(s), the origin will be set at the specified node.
Align Element
Aligns all elements with reference to a selected element.
Set IJK
Allows you to set the current IJK indices of the selected element(s) to new IJK indices.
Set I
Select which of the current indices to mark as the new I index.
Set J
Select which of the current indices to mark as the new J index.
Set K
Select which of the current indices to mark as the new K index.
Delete Nodes
Deletes the selected visible nodes from the display.
558
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Edit Distributed Attribute
Delete Elements
Deletes the selected elements from the display.
Edit Distributed Attribute
Makes the element with a distributed attribute visible. For example, if a model has distributed
boundary conditions, this option allows you to view and edit the BC at an element or node basis.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
559
560
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Properties
Figure 470: Properties Menu
After a model is meshed, you may define or edit material and element properties using the options in
the Properties menu. The options are as follows:
Load Material From File
Load Material From Library
Write Material File
Create Material Property
Create Material Property Table
Define Point Element Properties
Define 1D Element Properties
Define 2D Element Properties
Define 3D Element Properties
Note
In this section, the terminology used is the same as Nastran terminology. The Nastran
manual may be a resource for terminology.
The following types of element properties can be defined. The elements are grouped by dimensionality.
• 0D (Point) element properties (MASS elements)
• 1D (Line) element properties
– Bars
– Rigid Beams
→ RBAR
→ RBE2
→ RBE3
– Rod Connection
– Damper Connection
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
561
Properties
– Spring
– Viscous Damper
– Beam
– Gap
– Beam with Cross section
• 2D (Shell) element properties
– Shell
– Shear
– Layered Composite
• 3D (Solid) element properties
Load Material From File
Existing material files can be loaded using the Load Material From File option, or using the File
> Parameters > Open Parameters option. In either case, a file browser will open for you to select a
material file (*.mat). Loaded material files will be listed in the Display tree, under Material Properties.
The following Nastran materials are supported:
• MAT1 (Linear isotropic material properties)
• MAT2 (Linear anisotropic material properties for two-dimensional elements)
• MAT8 (Orthotropic material properties for isoparametric shell elements)
• MAT9 (Anisotropic material properties for isoparametric solid elements)
• MATS1 (Stress-dependent properties for nonlinear materials)
• MATT1 (Temperature-dependent properties for MAT1 entry fields via TABLEMi entries)
• MATT2 (Temperature-dependent properties for MAT2 entry fields via TABLEMj entries)
• MATT9 (Temperature-dependent properties for MAT9 entry fields via TABLEMk entries)
Load Material From Library
The Load Material From Library icon is located on the pull-down menu under the Load Material
From File icon. The following material files can be loaded from the Material Library:
• Steel
• Magnesium Alloy
• Copper Alloy
562
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Material Property
• Aluminum Alloy
• Polyethylene
• Stainless Steel
• Concrete
• Titanium Alloy
• Grey Cast Iron
The units for these materials are mm/C/MPa.
Write Material File
The Write Material File option allows you to save existing material property definitions to a material file (*.mat).
Create Material Property
The Create Material Property option opens a DEZ where you define the Name, ID, and Type of
material.
Figure 471: Define Material Property DEZ
Material Name
specifies the name of the material being defined.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
563
Properties
Material ID
specifies the ID of the material (MID). Nastran property cards reference this ID.
Type
Each type has its own material properties DEZ, and is described in the subsequent sections.
The different material types are:
Isotropic
Shell Element Anisotropic
Solid Element Anisotropic
Shell Element Orthotropic
Isotropic Thermal Material
Anisotropic Thermal Material
Isotropic
Each material property described below can be selected as Constant or Varying. For varying properties,
a material property table can be defined separately as described in Create Material Property Table (p. 566).
Young’s Modulus (E)
Within the elastic limit, the ratio of direct stress to the strain produced is called the Young’s modulus
(E).
Shear Modulus (G)
Within the elastic limit, the ratio of shear stress to shear strain.
Typically, this field is left blank. Nastran will calculate the value of Shear Modulus internally, based
on the following formula:
E = 2*(1+NU)*G,
where NU is the value of Poisson’s ratio.
Poisson’s Ratio (NU)
The ratio of lateral strain to longitudinal strain.
Mass Density (RHO)
The density of a material is its weight per unit volume (in SI units). This value will be used to automatically
calculate the mass of all structural elements.
This value should be consistent with PARAM, WTMASS card value for Nastran runs.
Thermal Expansion Coefficient (A)
This coefficient (A) is used to calculate thermal strains when thermal loads exist on the structure.
Reference Temperature (TREF)
The reference temperature for the calculation of thermal loads or a temperature dependent thermal
expansion coefficient. Typically, it is defined at room temperature in degrees Kelvin.
Structural Element Damping Coefficient (GE)
This value is found by multiplying the critical damping ratio C/C0 by 2.0.
Stress Limits for Tension (ST)
This is an optional value, used only to compute margins of safety in certain elements and has no effect
on the computational procedures.
564
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Material Property
Stress Limits for Compression (SC)
This is an optional value, used only to compute margins of safety in certain elements and has no effect
on the computational procedures.
Stress Limits for Shear (SS)
This is an optional value, used only to compute margins of safety in certain elements and has no effect
on the computational procedures.
Material Coordinate System (MCSID)
This is used only for PARAM, CURV processing.
LS Dyna Material Type
This specifies the LS Dyna Materials type.
Shell Element Anisotropic
Anisotropic materials have different material properties in the horizontal and vertical directions.
The properties of anisotropic shell elements include the same material properties that are described in
the Isotropic (p. 564) Material Property section. Additional properties are described below:
Gij
Elements from the material property matrix for this material type as described in the Nastran manual.
Thermal Expansion Coefficient Vectors (Ai)
These values are the thermal expansion coefficient vectors.
Solid Element Anisotropic
The properties of anisotropic solid elements include the same material properties described in the
previous two sections. The properties that are unique to this material type are described below:
Gij
Elements of the 6 x 6 symmetric material property matrix for this material type in the Nastran material
coordinate system.
Shell Element Orthotropic
Orthotropic materials have three mutually perpendicular planes of elastic symmetry.
Modulus of Elasticity – Longitudinal (E1)
Modulus of elasticity in the longitudinal direction. It also defined as the fiber direction or 1-direction.
Modulus of Elasticity – Lateral (E2)
Modulus of elasticity in lateral direction. It also defined as the matrix direction or 2-direction.
Poisson’s Ratio (NU12)
The ratio of lateral strain to longitudinal strain.
G12
In-plane shear modulus.
G1Z
Transverse shear modulus in the 1-Z plane.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
565
Properties
G2Z
Transverse shear modulus for shear in the 2-Z plane.
Mass Density (RHO)
The density of a material is its weight per unit volume (in SI units).
Thermal Expansion Coefficient (Ai)
Thermal expansion coefficient in the i direction. (Real)
Reference Temperature (TREF)
The reference temperature for the calculation of thermal loads or a temperature dependent thermal
expansion coefficient.
Xt and Xc
Allowable stresses or strains in tension and compression, respectively, in the longitudinal direction. These
values are required if a failure index is desired.
Yt and Yc
Allowable stresses or strains in tension and compression, respectively, in the lateral direction. These
values are required if a failure index is desired.
S
Allowable stress or strain for in-plane shear.
Structural Damping Coefficient (GE)
This value is found by multiplying the critical damping ratio C/C0 by 2.0.
F12
Interaction term in the tensor polynomial theory of Tsai-Wu. Required if the failure index by the Tsai-Wu
theory is desired and if the value of F12 is different from 0.0.
STRN
For the maximum strain theory only. It indicates whether Xt, Xc, Yt, Yc and S are stress or strain allowable.
(Real = 1.0, strain allowable; blank for stress allowable)
Isotropic Thermal Material
Isotropic Thermal Material corresponds to MAT4 (Heat Transfer Material properties, Isotropic) in Nastran.
Using this option allows you to set one thermal conductivity for the model.
Anisotropic Thermal Material
Anisotropic Thermal Material corresponds to MAT5 (Thermal Material property definition) in Nastran.
Using this option allows you to set thermal conductivity for each plane.
Create Material Property Table
The Create Material Property Table option allows you to create a material property table for
defining varying material properties.
566
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Material Property Table
Figure 472: Define Material Property Table
Varying material properties can be defined with one of the following types of tables:
Enter the name and ID of the table, and select the table type. Click Edit Table to view the Table Editor,
as shown below.
Figure 473: Material Properties Table Editor
The following options are available in the Table Editor window:
• Define and save material properties by filling in the table entries.
• Load material properties from a file in a space delimited x-y data format.
• Display the material properties graph as shown in Figure 474: Material Properties Curve (p. 568)
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
567
Properties
Figure 474: Material Properties Curve
Define Point Element Properties
The Define Point Element Properties option allows you to define point element properties. These
properties correspond to Nastran CONM2 element properties, which are mainly to define the mass
values.
568
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Define Point Element Properties
Figure 475: Define Point Element DEZ
By defining individual point masses as separate parts, they are conveniently grouped under the Display
Tree for easy manipulation.
Part
specifies the part for which the point properties will be assigned.
PID
This is grayed out by default.
Properties Type
The only type of point element property is Mass Point.
Mass Type
There are two options for Mass Types:
• CONM1
The general form of defining a mass element.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
569
Properties
• CONM2
A more specific means of defining a mass element.
Scalar Mass
specifies the value for the scalar mass (SI units).
Define 1D Element Properties
The Define 1D Element Properties option allows you to define line (curve) element properties.
Choose the Type of 1D element from the drop-down list. Each type has its own DEZ.
Figure 476: Define Line Element DEZ
The following sections describe the types of 1D (line) element that can be defined.
Bar Element Properties
Rigid Elements Properties
Rod Connection Properties
Mass Connection Properties
Damper Connection Properties
Spring Properties
Viscous Damper Element Properties
Beam Element Properties
Gap Element Properties
Beam With Cross Section
Bar Element Properties
The properties for elastic bar elements are as follows:
570
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Define 1D Element Properties
The X axis of the LCS follows the bar from end A to end B. The Y axis of the LCS is used to calculate I2
(Iyy) and the Z axis for I1 (Izz).
The formulas that are referenced are available in Mechanics of Materials books or can be computed by
using section analysis programs.
Part
specifies the part name to which the defined property will be assigned.
Material
specifies the material name for the defined property.
PID
specifies the property ID. Nastran property cards reference this ID.
Type
Bar will be automatically selected.
Cross Section Area
the value of the cross sectional area of the geometry.
Moment of Inertia (I1)
the moment of inertia for the Z axis (Izz).
Moment of Inertia (I2)
the moment of inertia for the Y axis (Iyy).
Torsional Constant (J)
the torsional constant for the geometry. For a circular cross section, this value is the sum of Izz and Iyy.
Normal X1, X2, X3
are the components of the orienting vector.
LS-DYNA Beam formulation
Choose the LS-DYNA beam type.
Rigid Elements Properties
The three types of rigid elements are as follows:
Rigid Bar (RBAR)
Rigid Bar with Single Dependent Nodes (Nastran CBAR elements with associated PBAR cards).
Dependent DOF (CMA)
specifies the required degree of freedom for one end of the bar.
Dependent DOF (CMB)
specifies the required degree of freedom for the other end of the bar.
Independent DOF (CNA)
specifies the required Independent degree of freedom for one end of the bar.
Independent DOF (CNB)
specifies the required Independent degree of freedom for the other end of the bar.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
571
Properties
Enter the required degree of freedom for one end of the bar.
Rigid Body (RBE2)
Rigid Body with Multiple Dependent Nodes (Nastran RBE2 elements).
Dependent DOF
specifies the required degree of freedom for one end of the bar.
Rigid Body (RBE3)
Rigid Body with Multiple Independent Nodes having weighted average of motion (Nastran RBE3 elements).
Dependent DOF
specifies the dependent degree of freedom.
Independent DOF
specifies the independent degree of freedom.
Weighting Factor
specifies the weighting factor. The default is 1.
Rod Connection Properties
The properties for elastic rod connections are as follows:
Cross Sectional Area
the cross sectional area of the geometry.
Torsion Constant
the torsion constant of the element.
Torsion Coefficient
the coefficient that determines torsional stress.
Nonstructural Mass/Unit Length
nonstructural mass per unit length.
Mass Connection Properties
The properties for mass connections are as follows:
Scalar Mass
the value of scalar mass of the element.
Component C1 and C2
the component numbers.
Damper Connection Properties
This corresponds to the Nastran property card PDAMP.
Force/Unit Velocity
is the damping factor to be supplied.
Components C1 and C2
damping components.
572
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Define 1D Element Properties
LS-DYNA Material Type
Select either Type 66 or Type 74.
Spring Properties
A spring element may be defined by the properties of Stiffness, Damping Coefficient and Stress
Coefficient. This is associated with the Nastran PELAS card, which is used in conjunction with the
CELAS1 and CELAS3 element connectivity cards.
Select LS-DYNA Material as either Type 66 or Type 74.
Note
It is customary to define spring elements for each degree of freedom separately. For a six
degree of freedom bushing, you need to define 6 CELAS1 and 6 corresponding PELAS cards.
Also, spring elements should be defined by coincident nodes (zero length) so that they don’t
transfer unintended moments.
Viscous Damper Element Properties
Viscous damping element properties define the PVISC card needed for CVISC viscous damper elements.
Damping for Extension
the damping factor for extension.
Damping for Rotation
the damping factor for rotation.
LS-DYNA Material Type
Select either Type 66 or Type 74.
Beam Element Properties
The properties of a beam element are described below. This element may be used to model tapered
beams.
Cross Section Area
cross sectional area of the beam.
Moment of Inertia (I1)
area moment of inertia for bending in plane 1 about the neutral axis.
Moment of Inertia (I2)
area moment of inertia for bending in plane 2 about the neutral axis.
Moment of Inertia (I12)
This value should be 0.0
Torsional Constant (J)
is the torsional stiffness parameter.
Normal X1
the normal value for the X direction.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
573
Properties
Normal X2
the normal value for the Y direction.
Normal X3
the normal value for the Z direction.
LS-DYNA Beam formulation
specifies the LS-DYNA Beam formulation.
Gap Element Properties
The gap element properties are as follows:
Initial Gap (U0)
the initial gap opening.
Preload (F0)
is the preload.
Axial Stiffness of Closed Gap (KA)
axial stiffness for the closed gap.
Axial Stiffness of Open Gap (KB)
axial stiffness for the open gap.
Transverse Stiffness (KT)
transverse stiffness when the gap is closed. It is recommended that KT ≥ (0.1 * KA).
Coeff of Static Friction (MU1)
coefficient of static friction for the adaptive element or coefficient of friction in the y transverse direction
for the non adaptive gap element.
Coeff of Kinetic Friction (MU2)
coefficient of kinetic friction for the adaptive gap element or coefficient of friction in the z transverse
direction for the non adaptive gap element.
Max Allowable Penetration (TMAX)
maximum allowable penetration used in the adjustment of penalty values. The positive value activates
the penalty value adjustment.
Max Allowable Adjustment Ratio (MAR)
maximum allowable adjustment ratio for adaptive penalty values KA and KT.
Fraction of TMAX Defining Lower Bound (TRMIN)
fraction of TMAX defining the lower bound for the allowable penetration. (Default = 0.001)
Normal X1
the normal value for the X direction.
Normal X2
the normal value for the Y direction.
Normal X3
the normal value for the Z direction.
574
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Define 2D Element Properties
Beam With Cross Section
The Beam with Cross Section element properties are as follows:
Cross Section Group (GROUP)
specifies the Group Name.
Cross Section Type (TYPE)
the various types of beams that can be used are I, T, L, H, BOX, BAR, ROD, TUBE, HAT, CHAN.
Nonstructural Mass Per Unit Length (NSM)
Specify this value.
Set Cross Section Dimensions
specifies the cross section dimension values in the table.
Note
Every cross section type beam has its own Set Cross Section table.
Normal X1
the normal value for the X direction.
Normal X2
the normal value for the Y direction.
Normal X3
the normal value for the Z direction.
Define 2D Element Properties
The Define 2D Element Properties option allows you to define shell (surface) element properties.
Choose the Type of 2D element from the drop-down list. Each type has its own DEZ.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
575
Properties
Figure 477: Define Shell Element DEZ
The following sections describe the 2D (Shell) Elements that can be defined:
Shell Elements
Shear Elements
Layered Composite Elements
Select the part to which the defined property will be assigned, and the PID of the property. Nastran
property cards reference this ID.
Shell Elements
The properties for thin shells possessing membrane, bending, and transverse shear and coupling
properties (Nastran PSHELL cards) are as follows:
Material
specifies the material.
Thickness
specifies the thickness of the geometry.
Transversal Shear Material
By default, this is the same material selected for the Material option. You can however select a different
material.
576
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Define 2D Element Properties
Coupling Membrane/Bending Material
By default, this is the same material selected for the Material option. You can however select a different
material.
Bending Moment of Inertia Ratio
bending moment of inertia of the element.
Bending Material
By default, this is the same material selected for the Material option. You can however select a different
material.
Transverse Shear Thickness Ratio
is the ratio of transverse shear thickness.
Nonstructural Mass/Unit Length
is the nonstructural mass per unit length.
Shear Elements
The properties for shear elements (Nastran PSHEAR cards for CSHEAR element types) are as follows:
Material
specifies the material.
Thickness
specifies the thickness of the geometry.
Nonstructural Mass/Unit Length
is the nonstructural mass per unit length.
Layered Composite Elements
The properties of layered composite elements (Nastran PCOMP card) are as follows:
Distance reference plane to bottom Surface (Z0)
is the distance from the reference plane to the bottom surface.
Nonstructural Mass Per Unit Area (NSM)
is the nonstructural mass per unit area.
Allowable Shear Stress in Bonding (SB)
allowable interlaminar shear stress.
Failure Theory (FT)
The following Failure Theory options are available: HILL, HOFF, TSAI, STRN.
Reference Temperature (TREF)
is the reference temperature.
Damping Coefficient (GE)
the damping coefficient.
Laminate Options (LAM)
The following options are available:
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
577
Properties
• Blank
• SYM
• MEM
• BEND
Number of Layers
specifies the number of composite layers.
Define 3D Element Properties
For 3D solids like HEXA, PENTA, and TETRA shaped elements, no special property is required except
for the identification of the Part name, Material, PID, and the Local Coordinate System (LCS).
Figure 478: Define Volume Elements DEZ
Specify the coordinate system on which this property should have applied.
578
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Constraints
Figure 479: Constraints Menu
The Constraints menu contains options for defining constraints. The constraints may be defined either
on the geometry, or on the finite element model, or both. The methods to define constraints on the
model are described in the following sections:
Create Constraint / Displacement
Create Constraint Equation
Define Constrained Node Sets
Define Contact
Define Single Surface Contact
Define Initial Velocity
Define Planar Rigid Wall
Create Constraint / Displacement
Constraints or displacements can be placed on different entity types in the geometry.
As soon as the constraint is created, it will be added to the Display Tree under Constraints. Constraints
are grouped by sets. Multiple sets can be created with different constraints.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
579
Constraints
Figure 480: Create Constraint / Displacement Window
Name
The constraint name.
SPC Set
is the number given to the constraint set. This is common Nastran Terminology.
LCS
the coordinate system for the applied constraint or displacement.
SPC Type
specifies the SPC Type.
Node Set ID
specifies the ID number of the Node Set.
Entity Type
the type of entity to which the constraint or displacement will be applied.
580
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Constraint / Displacement
Directional Displacement
You can restrict the movement of the selected entities by disabling the fields. When enabled, you can
specify the specific value of the displacement.
Rotational Displacement
You can restrict the movement of the selected entities by disabling the fields. When enabled, you can
specify the specific value of the displacement.
Create Constraint / Displacement on Point
In the example in Figure 481: Constraints on Points or Nodes (p. 581), a constraint is placed on the
center node of the model.
Figure 481: Constraints on Points or Nodes
Create Constraint / Displacement on Curve
Constraints can also be applied on lines or edges of the parts to restrict its movement in desired
degrees of freedom, as shown in Figure 482: Constraints on Curves (p. 582).
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
581
Constraints
Figure 482: Constraints on Curves
Create Constraint / Displacement on Surface
Constraints can also be placed on surfaces. In Figure 483: Constraints on Surfaces (p. 582), the
constraint is placed on the highlighted surface.
Figure 483: Constraints on Surfaces
582
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Define Constrained Node Sets
Create Constraint / Displacement on Subset
Constraints can also be placed on subsets of parts. Select the subsets on which the constraint
should be applied.
Note
The subset must already be created.
Create Constraint / Displacement on Part
Constraints can also be placed on parts. Select the parts on which the constraint should be applied.
Create Constraint Equation
This option allows you to create a multipoint constraint equation of the form: ∑
=
where Aj is a real number, and A1 is non-zero.
A mesh must be loaded in order to define a constraint equation.
Name
the name of the constraint equation.
MPC Set
the set identification number.
LCS
select the Coordinate System from the drop down list.
Node Set ID
specifies the ID number of the Node Set.
The dependent and independent nodes, DOF, and coefficients can be specified.
Define Constrained Node Sets
In order to define constrained node sets, a mesh must be loaded.
Note
This option is available for the LS-DYNA, ANSYS, and Autodyn solvers.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
583
Constraints
The following parameters are specified:
Name
Enter the desired name for your set.
Node Set ID
Enter an identifier for your set.
Nodes
Click the Select node(s) icon and then choose the nodes to be constrained in the graphics window.
Type
Choose from Node set or Generalized weld using the drop-down list. The additional options are dependent on your choice.
Define Contact
The contact option is supported for ANSYS, Abaqus, and LS-DYNA solvers. Nastran does not support
contacts. If you need to model contact for Nastran it is recommended to use connectors in place of
contact. The options for contact vary by solver.
Contacts can be defined in a variety of ways as described in the following sections:
Automatic Detection
Manual Definition
Automatic Detection
584
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Define Contact
Contact Proximity Factor
defines the distance used to evaluate which mesh is within contact with mesh in other parts. For each
of the selected parts, mesh between the parts will be evaluated a contact region between the parts will
be created.
Note
A mesh file must be loaded for this feature.
Parts
specifies the parts for which contact will be defined. By limiting the number of parts and modifying the
contact proximity factor, you can control the contact regions.
Note
Often it is easiest to select all parts.
Create one contact group for all parts
if enabled, one contact group will be created for all the selected parts.
Static Coefficient of Friction
The static coefficient of friction (µ) between two surfaces is defined as the ratio of the tangential force
(F) required to produce sliding divided by the normal force between the surfaces (N):
µ = F /N
The static coefficient of friction is used in the contact definition to define the resistance of the two
parts under contact.
LS-DYNA Contact Options
The contact cards that are supported are listed in the figure below. For further details, refer to the LSDYNA manual.
Figure 484: Define Contact Options
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
585
Constraints
Automatic Contact Option
For further details, refer to the LS-DYNA manual.
Dynamic Coefficient of Friction
The dynamic coefficient of friction or kinetic friction is used to define the friction under contact when
the two parts are in motion relative to each other (in contrast to the static coefficient of friction).
Manual Definition
Contacts can also be manually defined for shell elements.
Name
the name of the contact, which will appear in the Display Tree.
Contact Surfaces
specifies the surfaces or shell elements that make up the contact region.
Target Surfaces
specifies the surfaces or shell elements that make up the target region.
The remaining parameters are the same as described in Automatic Detection (p. 584)
Define Single Surface Contact
This option allows you to define a single surface contact.
Note
This option is available only for the LS-DYNA solver.
Name
the name of the contact, which will appear in the Display Tree.
Contact Surfaces
specifies the surfaces or shell elements that make up the contact region.
Static Coefficient of Friction
The static coefficient of friction (µ) between two surfaces is defined as the ratio of the tangential force
(F) required to produce sliding divided by the normal force between the surfaces (N):
µ=F/N
The static coefficient of friction is used in the contact definition to define the resistance of the two
parts under contact.
Dynamic Coefficient of Friction
The dynamic coefficient of friction or kinetic friction is used to define the friction under contact when
the two parts are in motion relative to each other (in contrast to the static coefficient of friction).
LS-DYNA Contact Options
There are three types of contact options:
586
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Define Planar Rigid Wall
AUTOMATIC_SINGLE_SURFACE
SINGLE_SURFACE
ERODING_SINGLE_SURFACE
For further details, refer to the LS-DYNA manual.
Define Initial Velocity
This option defines initial nodal point translational velocities using nodal sets. This may also be
used for sets in which some nodes have other velocities.
Note
This option is available only for the LS-DYNA solver.
Name
the name of the velocity, which will appear in the Display Tree.
Points
Nodes/Points which are to have defined velocities.
Directional Velocity
specifies the X, Y and Z components of the Translational Velocity.
Rotational Velocity
specifies the X, Y and Z components of the Rotational Velocity.
Define Planar Rigid Wall
This option allows you to define planar rigid walls.
Note
This option is available only for the LS-DYNA solver.
Name
the name of the rigid wall that will be updated in the Display Tree.
Points
Points/0D elements for which you want to define a rigid wall.
Offset
all nodes within this offset distance to the grid wall are included as slave nodes for the rigid wall.
Head Coordinates
coordinates for the head of any outward normal vector, originating on the wall (tail) and terminating in
space (head).
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
587
Constraints
Tail Coordinates
coordinates for the tail of any outward normal vector, originating on the wall (tail) and terminating in
space (head).
Interface Friction Data
• Type/Coulomb Coeff Value
– EQ 0.0, frictionless sliding after contact.
– EQ 1.0, no sliding after contact.
– 0.0 < FRIC < 1, Coulomb friction coefficient.
– EQ 2.0, node is welded after contact with frictionless sliding.
– EQ 3.0, node is welded after contact with no sliding.
• Critical Normal Velocity for Weld
Critical normal velocity at which the nodes are welded to the wall.
588
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Loads
External and internal loading can be applied in a variety of ways. These loads could be gravity (weight
of the structure) acting on the parts, pressure, forces or moments acting on a set of geometric or meshed
entities, velocities and accelerations, or temperature loading.
The Loads Menu options are described in the following sections.
Create Force
Place Pressure
Create Temperature Boundary Condition
Figure 485: Loads Menu
Create Force
External forces or moments can be applied to different entities.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
589
Loads
Figure 486: Create Force Window
Name
Assign a name to the force.
Load Set
Loads are separated into different sets for different properties. Sets are labelled with integer values.
LCS
Select the local coordinate system.
Scale
The scale factor for the value of the force.
Node Set ID
specifies the ID number of the Node Set.
Entity Type
Select the entity type to which the forces or moments will be applied.
Force Type
• Uniform
The force is uniformly distributed on all the nodes of the selected entities.
590
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Force
• Total
The force is distributed among all the nodes of the selected entities as per FEA concepts.
Forces
Enter the values of the forces and moments for the corresponding directions.
Note
Applied forces will be represented by a blue arrow, and moments by a brown arrow. If
both are applied at any location then a brown arrow will represent both the force and
moment.
Create Force on Point
External forces or moments can be applied to geometric points or nodes with this option.
Figure 487: Example of Externally Applied Forces
Create Force on Curve
Forces or moments can also be applied on geometric lines or curves before meshing, as shown
in the example below. Force or moment values will be enforced on all the nodes created on the specified
curves after meshing.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
591
Loads
Figure 488: Example of Edge Loading
Create Force on Surface
Forces or moments can also be applied on surfaces before meshing.
Create Force on Subset
Forces or moments can be applied on subsets of entities with the same options as described
above.
Note
The subset must already be created.
Create Force on Part
Forces or moments can be applied on parts with the same options as described above.
Place Pressure
Pressures can be defined to apply to surfaces, subsets, or parts. The metric unit of pressure is
N/mm2, and the pressure is applied to all elements on the entity once meshing is done.
592
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Place Pressure
Figure 489: Place Pressure Window
Name
Assign a name to the pressure.
Load Set
Loads for different properties are grouped by sets. Sets are labelled by integer values.
Entity Type
Select the entities to which the pressure is to be applied.
Pressure Type
• Uniform Normal Pressure Load
Enter the magnitude of the pressure that will be uniformly applied.
• General Pressure Load
Enter the parameters to define the General Pressure Load.
Place Pressure on Surface
Pressure can be applied to surfaces or shell elements. When writing out to an output file, the
pressure will be applied to the shell elements or the attached faces of the solid element, depending
on what solver is chosen and the type of pressure. The direction the pressure is applied is based on
the surface normals of the shell elements, or is applied into the volume for volume mesh. A circle
symbol will be displayed on a surface to indicate application of pressure, as shown in the figure below.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
593
Loads
Figure 490: Pressure on Surface Example
Place Pressure on Subset
Pressures to a subset of geometric or mesh entities are defined with the same options. The subset
must already be created.
Place Pressure on Part
Pressures to a subset of geometric or mesh entities are defined with the same options.
Create Temperature Boundary Condition
The metric unit of temperature used is °K (Kelvin scale).
Figure 491: Create Temperature Boundary Condition Window
Name
Name of the Temperature Set.
594
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Temperature Boundary Condition
Temperature Set
Set number for the defined Temperature.
Node Set ID
specifies the ID number of the Node Set.
Entity Type
Select the entities to which the temperature boundary condition is to be applied.
Temperature Type
This option applies to points only. The temperature load will be applied uniformly.
Temperature
The value of the temperature acting on the selected entities.
Temperature on Point
Temperatures can be applied to curves. In the following example, thermal boundary curves are
indicated by highlighted dots on the nodes.
Figure 492: Thermal Loading on Nodes
Temperature on Curve
Temperatures can be applied to curves. In the following example, thermal boundary curves are
indicated by highlighted dots on the curves.
Figure 493: Temperature on Curves Boundary Condition Example
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
595
Loads
Temperature on Surface
Temperatures can be applied to surfaces. In the following example, thermal boundary conditions
are indicated by highlighted dots on the surfaces.
Figure 494: Surface Temperature Boundary Condition Example
Temperature on Body
Temperatures can be applied to bodies as well. In the following example, thermal boundary conditions are indicated by highlighted dots on the bodies.
Figure 495: Body Temperature Boundary Condition Example
596
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Create Temperature Boundary Condition
Temperature on Subset
Temperatures can be also be applied to subsets. The subset must already be created.
Temperature on Part
Temperatures can be also be applied to parts.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
597
598
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Solve Options
Figure 496: Solve Options Menu
After setting up the different loading conditions on the geometry and mesh of a model, the Solve
Options Menu enables you to set specific options for your analysis.
If you selected a Common Structural Solver in the Solver Setup DEZ, (see Settings > Solver), your
selection will be visible in the Method drop-down list. If not, choose a Solver method at this time. Your
choices are NASTRAN, ANSYS, LS-DYNA, Abaqus, or Autodyn.
Note
To run ANSYS through the FEA functionality, you need to add the following environment
variables:
ANSYS_EXEC_PATH and ANSYSnn_PRODUCT.
The variable ANSYS_EXEC_PATH has to point to the “ansys.exe” file in the ANSYS installation
area.
The variable ANSYSnn_PRODUCT has to be set for the ANSYS Product through which analysis
will be done. Here, nn is the ANSYS version. The ANSYS product list is given below.
License
Feature
Product Description
ane3fl
ANSYS/Multiphysics
ANSYS
ANSYS/Mechanical\ U
ane3
ANSYS/Mechanical/Emag\ 3D
Anfl
ANSYS/Mechanical/FLOTRAN
ane3flds
ANSYS/Multiphysics/LS-DYNA
Ansysds
ANSYS/Mechanical/LS-DYNA
ane3ds
ANSYS/Mechanical/Emag\ 3D/LS-DYNA
Anflds
ANSYS/Mechanical/FLOTRAN/LS-DYNA
ane3fldp
ANSYS/Multiphysics/DYNAPrepPost
Ansysdp
ANSYS/Mechanical/DYNAPrepPost
ane3dp
ANSYS/Mechanical/Emag\ 3D/DYNAPrepPost
Anfldp
ANSYS/Mechanical/FLOTRAN/DYNAPrepPost
Struct
ANSYS/Structural\ U
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
599
Solve Options
600
License
Feature
Product Description
ste3
ANSYS/Structural/Emag\ 3D
Stfl
ANSYS/Structural/FLOTRAN
ste3fl
ANSYS/Structural/Emag\ 3D/FLOTRAN
Structds
ANSYS/Structural/LS-DYNA
ste3ds
ANSYS/Structural/Emag\ 3D/LS-DYNA
Stflds
ANSYS/Structural/FLOTRAN/LS-DYNA
Ste3flds
ANSYS/Structural/Emag\ 3D/FLOTRAN/LS-DYNA
Structdp
ANSYS/Structural/DYNAPrepPost
Ste3dp
ANSYS/Structural/Emag\ 3D/DYNAPrepPost
Stfldp
ANSYS/Structural/FLOTRAN/DYNAPrepPost
Ste3fldp
ANSYS/Structural/Emag\ 3D/FLOTRAN/DYNAPrepPost
Prf
ANSYS/Professional
prfe3
ANSYS/Professional/Emag\ 3D
Prffl
ANSYS/Professional/FLOTRAN
prfe3fl
ANSYS/Professional/Emag\ 3D/FLOTRAN
ane3fl1
ANSYS/Multiphysics\ 1
ane3fl2
ANSYS/Multiphysics\ 2
ane3fl3
ANSYS/Multiphysics\ 3
Ansysuh
ANSYS/University\ High
Ansysul
ANSYS/University\ Low
Ansysrf
ANSYS/ResearchFS
struct1
ANSYS/Structural1
struct2
ANSYS/Structural2
struct3
ANSYS/Structural3
Mpba
ANSYS/Multiphysics\ Batch
Meba
ANSYS/Mechanical\ Batch
Prba
ANSYS/Professional\ Batch
Stba
ANSYS/Structural\ Batch
Mpbach
ANSYS/Multiphysics\ Batch\ Child
Mebach
ANSYS/Mechanical\ Batch\ Child
Prbach
ANSYS/Professional\ Batch\ Child
Stbach
ANSYS/Structural\ Batch\ Child
Debach
ANSYS/DesignSpace\ Batch\ Child
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Setup Solver Parameters
License
Feature
Product Description
Profea
ANSYS/ProFEA
Note
The LS-DYNA deck does not handle units. The user is responsible to use consistent units for
all data.
Since Autodyn uses LS-DYNA data, the same caveat applies.
The following sections will address the Solve Options available. Each section is further split based on
Solver selection.
Setup Solver Parameters
Setup Analysis Type
Setup a Subcase
Write/View Input File
Submit Solver Run
Setup Solver Parameters
Use this option to configure the parameters for the selected Solver.
The Setup Solver Parameters window has different options for different Solvers, as explained below.
NASTRAN Setup Solver Parameters
ANSYS Setup Solver Parameters
LS-DYNA Setup Solver Parameters
Note
There are no additional parameters for Abaqus Solver or Autodyn Solver setup
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
601
Solve Options
NASTRAN Setup Solver Parameters
The different types of analysis that can be performed are: Linear Static Analysis, Modal Analysis and
Legacy analysis. Each analysis requires various parameters and inputs, which are explained in the following
sections.
Eigenvalue Extraction (EIGR / EIGRL)
• Method ID (SID)
Set ID number (Unique integer > 0)
• V1, V2
For vibration analysis, the frequency range of interest.
• Number of Modes (ND)
Number of frequencies desired.
Buckling Analysis (EIGB)
• Method ID (SID)
Set ID number (Unique integer > 0)
• SINV
Enhanced inverse power method.
602
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Setup Solver Parameters
• INV
Inverse power method.
• Lower / Upper Eigenvalues (L1, L2)
The Eigenvalue range of interest. Eigenvalues are the factors by which the pre-bucking state of
stress is multiplied to produce buckling in the shape defined by the corresponding Eigenvector.
• Desired Number of Positive / Negative Roots (NDP, NDN)
• NORM
Method for normalizing eigenvectors. The MAX option (default) normalizes eigenvectors to the
unit value of the largest component in the analysis set. The POINT option normalizes eigenvectors
to the unit value of the component defined in the G and C fields, where G is the Grid or scalar
point ID, and C is the Component number. The value for NORM defaults to MAX if the defined
component is zero.
Nonlinear Static Analysis Control (NLPARM)
• Number of Increments (NINC)
0<Integer<1000, Default=10.
• Incremental Time Intervals (DT)
Incremental time interval for creep analysis. The unit of DT must be consistent with units used
for the CREEP entry that defines its characteristics.
• KMETHOD
The stiffness update strategy.
• Number of Iterations (KSTEP)Number of iterations before the stiffness update for the ITER method.
The stiffness matrix is updated on convergence if KSTEP is less than the number of iterations that
were required for convergence with the current stiffness.
• Max Iterations (MAXITER)The limit on the number of iterations for each load increment.
• CONV
Flags to select convergence criteria. U=Displacement error, P=Load equilibrium error, W=work
error and the error tolerances (EPSU, EPSP, and EPSW) define the convergence criteria.
• INTOUT
Intermediate output flag. Controls the output requests for displacements, element forces and
stresses, etc.
• Max Divergence (MAXDIV)
The limit on the probable divergence condition per iteration before the solution is assumed to
diverge. (Integer not equal to 0: Default=3)
• Manimum Number of Quasi-Newton (MAXQN)
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
603
Solve Options
Newton correction vectors to be saved in the database.
• Max Number of Line Search (MAXLS)
Maximum number of line searches allowed for each iteration.
• Fraction of Effective Stress (0.0–1.0) (FSTRESS)
Fraction of effective stress used to limit the sub-increment size in the material routines.
• Line Search Tolerance (0.01–0.9) (LSTOL)
Line search tolerance.
• Max Number of Bisections (MAXBIS)
Maximum number of bisections allowed for each load increment.
• Max Ratio (1.0–40.0) (MAXR)
Maximum ratio for the adjusted arc length increment relative to the initial value.
• Max Value of Incremental Rotation (RTOLB)
Maximum value of incremental rotation (in degrees) allowed per iteration to activate bisection.
Transient Time Step (TSTEP)
Defines the step intervals at which a solution will be generated, and the output in transient analysis.
• Number of Time Steps
Number of time steps of value DTi (integer greater than or equal to 1)
Frequency (FREQ / FREQ1 / FREQ2)
• Frequency List (FREQ)
– Number of Frequencies
Defined number of frequencies.
• Frequency List (FREQ1)
The Frequency List (FREQ1) options define a set of frequencies to be used in the solution of frequency response problems, specified by the First Frequency (F1), the Frequency Increment
(DF), and the Number of Frequency Increments (NDF) desired.
• Frequency List (FREQ2)
The Frequency List (FREQ2) options define a set of frequencies to be used in the solution of frequency response problems, specified by the First Frequency (F1), the Frequency Increment
(DF), and the Number of Logarithmic Increments (NF).
Dynamic Load (DAREA / DELAY / DPHASE)
• Load Scale Factor (DAREA)
604
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Setup Solver Parameters
Defines scale (area) factors for static and dynamic loads. In dynamic analysis, DAREA is used in
conjunction with RLOADi and TLOAD entries.
– Pi
Grid, extra or scalar point identification number. (Integer >0)
– Ci
Component number (Integer 1 through 6 for grid point, blank or 0 for extra scalar point).
– Ai
Scale (area) factor.
• Dynamic Load Time Delay (DELAY)
– Pi
Grid, extra or scalar point identification number. (Integer >0)
– Ci
Component number (Integer 1 through 6 for grid point, blank or 0 for extra scalar point).
– Ti
Time delay for designated point Pi and component Ci.
• Dynamic Load Phase Lead (DPHASE)
Defines the phase lead term theta in the equation of the dynamic loading function.
– Pi
Grid, extra or scalar point identification number. (Integer >0)
– Ci
Component number (Integer 1 through 6 for grid point, blank or 0 for extra scalar point).
– THi
Phase lead theta in degrees.
Dynamic Excitation (TLOAD/RLOAD)
• Transient Response (TLOAD1)
Defines a time dependent dynamic load or enforced motion, for use in transient response analysis.
– DAREA
Identification number of DAREA set or a thermal load set that defines enforced acceleration
using large mass or SPC/SPCD data.
– DELAY
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
605
Solve Options
Identification number of delay entry set.
– EXCITATION TYPE
Defines the type of dynamic excitation.
– TABLEDi
Identification number of TABLEDi entry.
• Transient Response (TLOAD2)
Includes the same parameters as Transient Response (TLOAD1), in addition to the parameters:
Time Constants (T1, T2), Frequency (F), Phase Angle (P), Exponential Coef. (C), and Growth
Coef. (B).
• Frequency Response (RLOAD1)
Defines a frequency dependent dynamic excitation for use in frequency response problems.
• Frequency Response (RLOAD2)
Includes the same parameters as Frequency Response (RLOAD1).
Dynamic Load Combination (DLOAD)
Defines a dynamic loading condition for frequency response or transient response problems as a linear
combination of load sets defined via RLOAD1 or RLOAD2 entries for frequency response, or TLOAD1 or
TLOAD2 entries for transient response.
• Global Scale Factor (S)
The Global Scale Factor.
• Number of loads
The number of Load Set ID numbers of RLOAD1, RLOAD2, TLOAD1, and TLOAD2.
Static Load Combination (LOAD)
Defines a static load as a linear combination of load sets.
• Global Scale Factor (S)
The Global Scale Factor.
• Number of loads
The number of Load Set ID numbers used to define the LOAD.
Single-Point Constraint Combination (SPCADD)
Defines a single-point constraint set as the combination of other defined single-point constraint sets.
Multi-Point Constrant Combination (MCADD)
Defines a multipoint constraint set as combination of other multippoint constraint sets.
606
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Setup Solver Parameters
Default Grid Point Temperature (TEMPD)
Defines a temperature value for all grid points of the structural model that have not been given a temperature on a TEMP entry.
Acceleration or Gravity Load (GRAV)
Defines acceleration vectors for gravity or other acceleration loading.
• LCS
Identify the local coordinate system.
• MB
Indicates whether the local coordinate system (LCS) is defined in the main Bulk Data Section (MB
= -1) or the partitioned superelement Bulk Data Section (MB = 0). Coordinate systems referenced
in the main Bulk Data Section are defined relative to the assembly basic coordinate system, which
is fixed. This feature is useful when a superelement defined by a partitioned Bulk Data section is
rotated or mirrored.
• Scale Factor
Scale factor of the acceleration vector.
• Vector Components
Acceleration vector components measured in the specified coordinate system.
Include File (INCLUDE)
Inserts an external file (*.dat, *.nas, *.bdf ) into the input file using an INCLUDE statement.
ANSYS Setup Solver Parameters
Use the drop down list to select the Method of Global motion that is to be specified, if any.
Acceleration or Gravity
• Parameter Name
The name of the load.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
607
Solve Options
• Scale Factor
Scale factor of the acceleration vector.
• Direction
Specify the acceleration vector components.
Rotational Velocity
The X, Y, and Z components can be specified. Also, the Spin Softening Key can be decreased or not
modified.
Rotational Acceleration
The X, Y, and Z components can be specified.
LS-DYNA Setup Solver Parameters
Base Acceleration or Gravity Load
Defines acceleration vectors for gravity or other loading.
Note
Only one gravity vector can be defined for the LS-DYNA file.
• Parameter Name
The name of the load.
• Scale Factor
Scale factor of the acceleration vector.
• Direction
Specify the acceleration vector components.
608
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Setup Analysis Type
Setup Analysis Type
This option allows you to setup the parameters for the different types of analysis.
The following sections describe the parameters that are specific to each analysis type.
NASTRAN Setup Analysis Type
ANSYS Setup Analysis Type
LS-DYNA Setup Analysis Type
Abaqus Setup Analysis Type
Autodyn Setup Analysis Type
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
609
Solve Options
NASTRAN Setup Analysis Type
Run Time (TIME)
The maximum allowable execution time in CPU minutes. By default, it is set to 99999. You can increase
this if necessary.
Max Output Lines (MAXLINES)
The maximum number of output lines to the solver. In any run, if MAXLINES exceeds the set value (99999
is the default), then the program will terminate.
610
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Setup Analysis Type
Write Input Lines (ECHO)
Controls the Input file for the Nastran solver. The following options are available:
• NONE
Suppresses printing of the Bulk Data into the Nastran Input file.
• SORT
Writes the Bulk Data section in small field format as well as sorted alphabetically into the Nastran
input file.
• UNSORT
Writes the Bulk Data section exactly as it is input.
• BOTH
Write both the SORT and UNSORT formats.
• PUNCH
Punches the Bulk Data to an ASCII file.
Case Control Cards
Output Title (TITLE)
To specify a title that will appear on the first heading line of each output page.
Output SubTitle (SUBTITLE)
To specify a subtitle that will appear on the second heading line for each output page.
Output Label (LABEL)
To specify a label that will appear on the third heading line of each output page.
Linear Static Analysis (Sol 101)
Mass Multiplier (WTMASS)
This value will be multiplied to the structural mass matrix when the mass of the structure is calculated.
Rotation Stiffness Adjustment (K6ROT)
It specifies the stiffness to be added to the normal rotation for Shell and Tri elements. The default is 0,
but you can change its value between 1 to 100 to suppress singularities for geometric nonlinear analysis.
Max Ratio (MAXRATIO)
The default value for the MAXRATIO is 1.0E7.
Coupled Mass (COUPMASS)
The default value is -1.
Constrain Singularities (AUTOSPC)
AUTOSPC specifies the action to take when singularities exist in the stiffness matrix. If enabled, the singularities will be constrained automatically.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
611
Solve Options
Grid Weights (GRDPNT)
This option will execute the grid point weight generator. It specifies the identification number of the
grid point to be used as a reference point.
Single Point Constraints (SPC)
Sets this value (positive integer) for the solution. It will set the same number of Single Point Constraint
in the input data form.
Load Set (LOAD)
Assigns an external static load set (positive integer) to the solution. It will set the same number of Load
Constraints in the input data form.
Temperature Set (TEMP)
Selects the temperature set to be used in either material property calculations or thermal loading in
heat transfer and structural analysis.
Output Requests
These output requests (Displacement, Stress, Strain, Element Strain Energy) can be set to ALL or NONE.
Modal (Sol 103)
The Parameters and Output Requests data that is needed to perform Modal analysis is described in
Linear Static Analysis (Sol 101) (p. 611).
Buckling Analysis (Sol 105)
The Parameters and Output Requests data that is needed to perform Buckling analysis is described in
Linear Static Analysis (Sol 101) (p. 611).
Nonlinear Static (Sol 106)
The Parameters and Output Requests data for performing Nonlinear Static analysis is described in Linear
Static Analysis (Sol 101) (p. 611).
Direct Frequency Response (Sol 109)
The Parameters and Output Requests data that is needed to perform this analysis is described in Linear
Static Analysis (Sol 101) (p. 611). The additional data needed is described below.
Parameters (PARAM)
• Structural Coefficient (G)
This value is equal to C/C0 multipled by a factor of 2.
Case Control Cards
• Dynamic Load
Select a dynamic load to be applied in a transient or frequency response problem.
• Frequency
Select a frequency to be applied in a transient or frequency response problem.
612
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Setup Analysis Type
Direct Transient Response (Sol 109)
The Parameters and Output Requests data that is needed to perform this analysis is described in Linear
Static Analysis (Sol 101) (p. 611). The additional data needed is described below.
Parameters (PARAM)
• Structural Coefficient (G)
This value is equal to C/C0 multipled by a factor of 2.
• Structural Coefficient (W3)
The default value is 0.
Output Requests
• Velocity
Requests the form and type of velocity vector output.
Case Control Cards
• Dynamic Load
Select a dynamic load to be applied in a transient or frequency response problem.
• Frequency
Select a frequency to be applied in a transient or frequency response problem.
Modal Frequency Response (Sol 111)
The Parameters and Output Requests data that is needed to perform this analysis is described in Linear
Static Analysis (Sol 101) (p. 611). The additional data needed is described below.
Output Requests
• Velocity
Requests the form and type of velocity vector output.
• Acceleration
Requests the acceleration output.
Case Control Cards
• Dynamic Load
Select a dynamic load to be applied in a transient or frequency response problem.
• Frequency
Select a frequency to be applied in a transient or frequency response problem.
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
613
Solve Options
• Structural Damping (SDAMPING)
ANSYS Setup Analysis Type
Two different categories of analysis are supported for the ANSYS solver: Structural and Thermal Analysis. The following sections describe the parameters for each type of analysis.
Structural Analysis
For Structural Static analysis, select the type of solver:
• Auto
– Number of Substeps
Number of substeps to be used for this load step (the time step size or frequency increment).
– Large Deformation Key
If Ignore is selected, than it will not include large deflection effects in a static or full transient
analysis. For the Include option, it will be incorporated in the analysis.
• Direct
Enter the Number of Substeps and select the Large Deformation Key option.
• PCG
This is a Pre-conditioned Conjugate Gradient iterative equation solver. It requires less disk space
and is faster for large models.
Enter the Number of Substeps and select the Large Deformation Key option.
– Tolerance
Solver tolerance value (defaults to 1.0e-8).
614
ANSYS ICEM CFD 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information of ANSYS, Inc. and its subsidiaries and affiliates.
Setup Analysis Type
– Convergence multiplier
Multiplier user to control the maximum number of iterations performed during a convergence
calculation. The recommended range for the multiplier is 1.0 ≤ multiplier ≤ 3.0.
The Structural Modal Analysis, the following parameters can be defined for the Mode Extraction
Method.
Block Lanczos
This is a modal analysis method that is supported in the FEA functionality of ANSYS ICEM CFD.
Number of Modes to Extract
Number of modes to extract for the analysis.
Beginning (Lower End) Frequency
Beginning or lower end of the range of frequency. It also represents the first shift point for the eigenvalue
iterations.
Ending (Upper End) Frequency
Ending or upper end of the range of frequency. The default value is 1.0E8.
Mode Shape Normalization Key
If set to OFF, it normalizes the mode shape to the mass matrix. If set to ON , it normalizes the mode
shapes to unity instead of to the mass matrix.
Constraint Equation Processing Key
There are four options for different constraint equations to be used during analysis: Default, Quick
Lagrange, Accurate Lagrange, and Direct Elimination.
Element Calculation Key
Number of modes to expand and write for a modal analysis. If OFF is selected, then it will not calculate
element results and reaction forces. If ON is selected, along with the nodal degree of