Trelis 15.0 User Documentation

Trelis 15.0 User Documentation
Trelis 15.0 User Documentation
Table of Contents
1.
Trelis15.0 User Documentation _________________________________________________________________ 1
2.
Key Features ________________________________________________________________________________ 3
Geometry Creation, Modification, and Healing
Non-Manifold Topology
Geometry Decomposition
Mesh Generation
Boundary Conditions
Element Types
Graphics Display Capabilities
Graphical User Interface
Command Line Interface
3
3
3
3
3
3
4
4
4
3.
Hardware Requirements ______________________________________________________________________ 5
4.
Trademark Notice ____________________________________________________________________________ 7
5.
How to Use This Manual ______________________________________________________________________ 9
6.
Introduction ________________________________________________________________________________ 11
7.
Trelis Support ______________________________________________________________________________ 13
8.
Starting and Exiting a Trelis Session ___________________________________________________________ 15
Starting the Session
Windows File Association
Exiting the Session
Resetting the Session
Abort Handling
9.
15
15
15
15
15
Execution Command Syntax __________________________________________________________________ 17
Passing Variables into a CUBIT Session
19
10.
Initialization Files ___________________________________________________________________________ 21
11.
Environment Variables _______________________________________________________________________ 23
12.
Command Syntax ___________________________________________________________________________ 25
13.
Command Line Help _________________________________________________________________________ 27
14.
Environment Commands _____________________________________________________________________ 29
Working Directory
File Manipulation
CPU Time
Comment
History
29
29
30
30
30
iii
Trelis 15.0 User Documentation
Error Logging
Determining the Trelis Version
Echoing Commands
Digits Displayed
15.
Saving and Restoring a Trelis Session__________________________________________________________ 33
Cubit File Method
New
Open '<filename>'
Save
Import
Export
16.
40
41
42
42
View Navigation in the GUI ___________________________________________________________________ 43
Rotations
Zooming
Panning
19.
35
36
Command Panel Functionality ________________________________________________________________ 39
ID Input Entry Methods
Right-Click Context Menu for ID Input Fields
Value Fields
Advancing Pickwidgets
18.
33
33
33
33
34
34
Trelis Application Window ____________________________________________________________________ 35
Context Sensitive Help in the GUI
Customizing the Application Window
17.
30
31
31
31
43
44
45
Selecting Entities in the GUI __________________________________________________________________ 47
Pre-Selection
Polygon and Box Select
47
48
20.
Key Press Commands for the GUI _____________________________________________________________ 49
21.
Right Click Commands for the GUI Graphics Window _____________________________________________ 51
With Entity Selected
Without Entity Selected
51
51
22.
Viewing Curve Valence_______________________________________________________________________ 53
23.
Geometry Tree ______________________________________________________________________________ 55
Drag and Drop
Picked Group
Right-Click Menu Functions
24.
Geometry Power Tools _______________________________________________________________________ 59
Geometry Analysis Tools
Geometry Repair Tools
Right Click Menu
iv
57
57
57
59
61
63
Table of Contents
25.
Meshing Tools ______________________________________________________________________________ 65
Right Click Context Menu
26.
Mesh Quality Tools __________________________________________________________________________ 67
Mesh Quality Tool Buttons
Right-Click Context Menu Items
27.
76
76
Toolbars ___________________________________________________________________________________ 77
File
Display
Select
31.
73
73
73
73
74
74
74
74
Journal File Editor __________________________________________________________________________ 75
Journal Editor Toolbar
Other Functionality Available in the Journal Editor
30.
70
70
70
70
70
71
Command Line Workspace ___________________________________________________________________ 73
Command Window
Entering Commands
Repeating Commands
Focus Follows Cursor
Error Window
History Window
Script Window
Docking and Undocking the Input Window
29.
68
68
Property Page ______________________________________________________________________________ 69
Editing Entity Attributes from the Property Page
General Attributes
Geometry Attributes
Meshing Attributes
Boundary Condition Attributes
Metadata Attributes
28.
65
77
77
78
Options Menu ______________________________________________________________________________ 79
Custom Tools
Display Preferences
General Preferences
Geometry Defaults
History Preferences
Trelis History Preferences
Label Defaults
Layout Preferences
Trelis Layout Settings
Mesh Defaults
Mouse Settings
Post Processor Settings
Quality Defaults
79
79
79
80
80
80
80
80
81
81
81
81
81
v
Trelis 15.0 User Documentation
32.
Creating Custom Toolbar Buttons _____________________________________________________________ 83
33.
Undo Button _______________________________________________________________________________ 85
Limitations
34.
85
Journal File Creation and Playback ____________________________________________________________ 87
Recording a Session
Replaying a Session
87
87
35.
Controlling Playback of Journal Files __________________________________________________________ 89
36.
Automatic Journal File Creation _______________________________________________________________ 91
Controlling Automatic Journal File Creation
Recording Graphics Commands
Recording Entity IDs and Names
Recording APREPRO Commands
Recording Errors
91
91
91
91
92
37.
Idless Journal Files _________________________________________________________________________ 93
38.
Command Line View Navigation: Zoom, Pan and Rotate ___________________________________________ 95
Rotation
Panning
Zooming
39.
Mouse Based View Navigation: Zoom, Pan and Rotate ____________________________________________ 97
Changing the View Transformation Button Bindings
Saving and Restoring Views
40.
107
107
108
108
108
108
108
109
Mesh Visualization _________________________________________________________________________ 111
Notes on Mesh Slicing
Mesh Slicing Command
vi
104
104
Drawing and Highlighting Entities ____________________________________________________________ 107
Drawing Other Objects
Displaying Entity Orientation
Volume Sources and Targets
Model Axis
Surface Isoparameter Lines
Surface Overlap
Volume Overlap
Geometry Preview
43.
101
Graphics Modes ___________________________________________________________________________ 103
Displaying Using the Element Facets
Displaying Composite Surface Lines
42.
98
99
Updating the Display _______________________________________________________________________ 101
Prevent Graphics From Updating
41.
95
95
95
111
111
Table of Contents
44.
Graphics Clipping Plane ____________________________________________________________________ 113
Examples
114
45.
Entity Labels ______________________________________________________________________________ 115
46.
Colors ___________________________________________________________________________________ 117
Specifying Colors in Commands
User-Defined Colors
Assigning Colors
Assigning Global Colors
117
117
118
119
47.
Geometry and Mesh Entity Visibility___________________________________________________________ 121
48.
Graphics Camera __________________________________________________________________________ 123
Changing Camera Attributes Directly
123
49.
Graphics Lighting Model ____________________________________________________________________ 125
50.
Graphics Window Size and Position___________________________________________________________ 127
Using Multiple Windows
127
51.
Saving Graphics Views _____________________________________________________________________ 129
52.
Hardcopy Output __________________________________________________________________________ 131
Screen Capture Programs
53.
Miscellaneous Graphics Options _____________________________________________________________ 133
Silhouette Lines
Line Width
Highlight Line Width
Text Size
Point Size
Graphics Status
Graphics Scale
Model Axis
Corner Axis (Triad)
Resetting the Graphics
Shrink
Facet Tolerance
54.
131
133
133
133
134
134
134
134
134
134
135
135
136
Command Line Entity Specification ___________________________________________________________ 139
Types of Entity Range Input
Precedence of "Except" and "In"
Placement in Trelis Commands
139
140
141
vii
Trelis 15.0 User Documentation
55.
Entity Selection ____________________________________________________________________________ 143
56.
Environment Control _______________________________________________________________________ 145
57.
Extended Command Line Entity Specification __________________________________________________ 147
Extended Parsing Syntax
Keywords
Functions
Precedence
58.
Selecting Entities with the Mouse _____________________________________________________________ 151
Entity Selection
Query Selection
Multiple Selected Entities
Information About the Selection
Picked Group
Substituting Selection into Other Commands
59.
163
163
163
163
164
164
164
165
165
Specifying a Direction ______________________________________________________________________ 167
Vector (XYZ values)
Last Direction Used
Positive or Negative X,Y,Z Direction Vectors
On Curve Tangent
On Surface Normal
From Location
Rotate
Cross
viii
157
157
157
158
158
158
158
158
158
159
159
160
160
160
Specifying a Location on a Curve _____________________________________________________________ 163
Arc Center
Start, Midpoint, or End
Fraction
Distance
{Close_To|At} Location
Extrema
Segment
Crossing
Previewing a Location on a Curve
61.
152
153
153
153
153
154
Specifying a Location_______________________________________________________________________ 157
Position (XYZ values)
Last Location Used in a Command
Node or Vertex
On a Curve
On a Surface
On a Plane
Center
Extrema
Fire Ray
Between
Move
Swing
Multiple Location Specification
Previewing a Location
60.
147
147
148
149
167
167
167
168
168
168
169
169
Table of Contents
Reverse
Previewing a Direction
62.
Specifying an Axis _________________________________________________________________________ 171
Last
Specify an origin and a vector
Revolve an axis about an axis
Previewing an Axis
63.
169
169
171
171
171
172
Specifying a Plane _________________________________________________________________________ 173
Location and Normal Vector
Location and Two Vectors on the Plane
Two Locations and Vector on the Plane
Three Points on the Plane
Plane defined by a Surface
Plane Normal to a Curve
Plane Defined by a Non-linear curve
Plane Defined by a two linear curves
Normal Vector and Coefficient
Coordinate Plane
Last Location Used
Previewing a Plane
Preview a Cylindrical Plane
173
174
174
175
175
176
177
177
177
177
178
178
178
64.
Drawing a Location, Direction, or Axis _________________________________________________________ 181
65.
List Model Summary________________________________________________________________________ 183
66.
List Geometry _____________________________________________________________________________ 185
67.
List Mesh _________________________________________________________________________________ 187
68.
List Special Entities ________________________________________________________________________ 189
69.
List Trelis Environment _____________________________________________________________________ 191
Message Output Settings
Graphical Display Information
Memory Usage Information
191
193
193
70.
ACIS Geometry Kernel ______________________________________________________________________ 195
71.
Mesh-Based Geometry ______________________________________________________________________ 197
Creating Mesh-Based Geometry Models
Improving Mesh-Based Geometry Models for Meshing
Meshing Mesh-Based Models
Exporting Mesh-Based Geometry
72.
197
198
199
199
Importing ACIS Files________________________________________________________________________ 201
Import Options
Importing ACIS files at startup
201
201
ix
Trelis 15.0 User Documentation
73.
Importing FASTQ Files ______________________________________________________________________ 203
74.
Importing STEP Files _______________________________________________________________________ 205
Import Options
Exporting a STEP file from Pro/Engineer
75.
Importing IGES Files _______________________________________________________________________ 207
Import Options
76.
205
205
207
Importing Facet Files _______________________________________________________________________ 209
Facet File Format
Feature Angle
Smooth Curves and Surfaces
Merge
Make elements
Stitch
Improve
210
210
210
211
211
211
211
77.
Importing Granite Files _____________________________________________________________________ 213
78.
Creating Vertices __________________________________________________________________________ 215
79.
Creating Curves ___________________________________________________________________________ 219
80.
Creating Surfaces __________________________________________________________________________ 225
81.
Creating Volumes __________________________________________________________________________ 239
82.
Creating Bricks ____________________________________________________________________________ 249
83.
Creating Cylinders _________________________________________________________________________ 251
84.
Creating Prisms ___________________________________________________________________________ 253
85.
Creating Frustums/Cones ___________________________________________________________________ 255
86.
Creating Pyramids _________________________________________________________________________ 257
87.
Creating Spheres __________________________________________________________________________ 259
88.
Creating Toruses___________________________________________________________________________ 261
89.
Align Command ___________________________________________________________________________ 263
90.
Copy Command ___________________________________________________________________________ 265
91.
Move Command ___________________________________________________________________________ 267
Moving Other Geometric Entities
x
267
Table of Contents
Moving Bodies Relative to Other Geometric Entities
Moving Merged Entities
Move Undo
268
268
268
92.
Scale Command ___________________________________________________________________________ 269
93.
Rotate Command __________________________________________________________________________ 271
Rotating Merged Entities
271
94.
Reflect Command __________________________________________________________________________ 273
95.
Intersect __________________________________________________________________________________ 275
96.
Subtract __________________________________________________________________________________ 277
97.
Unite _____________________________________________________________________________________ 279
98.
Chop Command ___________________________________________________________________________ 281
99.
Web Cutting by Sweeping Curves or Surfaces __________________________________________________ 283
Web Cutting by Sweeping a Surface Along a Trajectory
Web Cutting by Sweeping a Surface About an Axis
Web Cutting by Sweeping a Curve(s) Along a Trajectory
Web Cutting by Sweeping a Curve(s) About an Axis
283
284
285
285
100. ___________________________________________________________________ W
eb Cutting Options _________________________________________________________________________ 287
101. ___________________________________________________________________ W
eb Cutting with a Planar or Cylindrical Surface__________________________________________________ 289
Coordinate Plane
Planar Surface
Plane from 3 Points
Plane Normal to Curve
General Plane Specification
Cylindrical Surface
Cone Surface
289
289
289
290
290
291
291
xi
Trelis 15.0 User Documentation
102. ___________________________________________________________________ W
eb Cutting using a Tool or Sheet Body_________________________________________________________ 293
103. ___________________________________________________________________ W
eb Cutting with an Arbitrary Surface __________________________________________________________ 295
104. ___________________________________________________________________ S
plit Curve _________________________________________________________________________________ 297
105. ___________________________________________________________________ S
plit Periodic Surfaces _______________________________________________________________________ 299
106. ___________________________________________________________________ S
plit Surface _______________________________________________________________________________ 301
Split Across
Split Extend
Split (Automatically)
Split Skew
301
302
304
316
107. ___________________________________________________________________ S
ection Command___________________________________________________________________________ 319
108. ___________________________________________________________________ S
eparating Multi-Volume Bodies _______________________________________________________________ 321
109. ___________________________________________________________________ S
eparating Surfaces from Bodies ______________________________________________________________ 323
110. ___________________________________________________________________ A
nalyzing Geometry _________________________________________________________________________ 325
Healer Settings
325
111. ___________________________________________________________________ H
ealing Attributes ___________________________________________________________________________ 327
112. ___________________________________________________________________ A
uto Healing _______________________________________________________________________________ 329
113. ___________________________________________________________________ S
pline Removal _____________________________________________________________________________ 331
114. ___________________________________________________________________ W
hat if Healing is Unsuccessful?_______________________________________________________________ 333
115. ___________________________________________________________________ T
weaking Vertices ___________________________________________________________________________ 335
Tweaking a Vertex With a Chamfer
Tweaking a Vertex With a Non-Equal Chamfer
Tweaking a Vertex With a Fillet Radius
xii
335
336
336
Table of Contents
116. ___________________________________________________________________ T
weaking Curves ___________________________________________________________________________ 339
Create a Chamfer or Fillet
Tweaking a Curve Using an Offset Distance
Removing a Curve
Tweaking a Curve Using Target Surfaces, Curves, or Plane
Tweaking a Pair of Curves to a Corner
339
340
341
342
343
117. ___________________________________________________________________ T
weaking Surfaces __________________________________________________________________________ 345
Tweaking a Surface Using an Offset
Tweaking a Surface by Moving
Tweaking Surfaces to Target Surfaces
Removing a Surface
Tweaking a Conical Surface
Tweaking Doublers to Target Surfaces
Removing Holes and Slots from Sheet Bodies
Removing Fillets from Sheet Bodies
345
346
346
347
347
348
350
352
118. ___________________________________________________________________ T
weak Remove Topology _____________________________________________________________________ 355
Example
355
119. ___________________________________________________________________ T
weak Volume Bend _________________________________________________________________________ 359
120. ___________________________________________________________________ R
emoving Vertices __________________________________________________________________________ 361
121. ___________________________________________________________________ R
emoving Surfaces __________________________________________________________________________ 363
Remove Sliver Surface
363
122. ___________________________________________________________________ A
utomatic Forced Sweepability ________________________________________________________________ 365
123. ___________________________________________________________________ A
utomatic Small Curve Removal _______________________________________________________________ 367
124. ___________________________________________________________________ A
utomatic Small Surface Removal _____________________________________________________________ 369
125. ___________________________________________________________________ A
utomatic Surface Split ______________________________________________________________________ 371
126. ___________________________________________________________________ R
egularizing Geometry _______________________________________________________________________ 373
127. ___________________________________________________________________ F
inding Surface Overlap _____________________________________________________________________ 375
Facetted Representation
Find Overlap Settings
375
376
xiii
Trelis 15.0 User Documentation
128. ___________________________________________________________________ V
alidating Geometry _________________________________________________________________________ 379
129. ___________________________________________________________________ D
ebugging Geometry ________________________________________________________________________ 381
130. ___________________________________________________________________ G
eometry Accuracy __________________________________________________________________________ 383
131. ___________________________________________________________________ T
rimming and Extending Curves_______________________________________________________________ 385
Trimming a Curve
Extending a Curve
385
386
132. ___________________________________________________________________ S
titching Sheet Bodies _______________________________________________________________________ 389
133. ___________________________________________________________________ I
mprinting Geometry ________________________________________________________________________ 391
Regular Imprinting
Tolerant Imprinting
Mesh-Based Imprinting
Imprint Settings
391
392
392
393
134. ___________________________________________________________________ M
erging Geometry ___________________________________________________________________________ 395
Merge geometry automatically
Test for merging in a specified group of geometry
Force merge specified geometry entities
Preventing geometry from merging
Other Merge Commands
395
395
395
396
396
135. ___________________________________________________________________ E
xamining Merged Entities ___________________________________________________________________ 397
136. ___________________________________________________________________ M
erge Tolerance_____________________________________________________________________________ 399
Finding Nearly Coincident Entities
399
137. ___________________________________________________________________ U
nmerging _________________________________________________________________________________ 401
138. ___________________________________________________________________ U
sing Geometry Merging to Verify Geometry_____________________________________________________ 403
139. ___________________________________________________________________ C
omposite Curves___________________________________________________________________________ 405
140. ___________________________________________________________________ C
omposite Surfaces _________________________________________________________________________ 407
Controlling the Surface Evaluation Method for Composite Surfaces
Composite Determination
xiv
407
407
Table of Contents
141. ___________________________________________________________________ P
artitioned Curves __________________________________________________________________________ 409
142. ___________________________________________________________________ P
artitioned Surfaces _________________________________________________________________________ 411
Partitioning with Vertices and Nodes
Partitioning with Hard Points
Partitioning with Polylines
Partitioning with Curves
Partitioning with Mesh Edges
Partitioning with Faces or Triangles
411
411
411
412
413
413
143. ___________________________________________________________________ P
artitioned Volumes _________________________________________________________________________ 415
144. ___________________________________________________________________ U
sing Mesh Intersections to Partition Surfaces___________________________________________________ 417
145. ___________________________________________________________________ R
emoving Partitions _________________________________________________________________________ 419
146. ___________________________________________________________________ C
ollapse Angle______________________________________________________________________________ 421
147. ___________________________________________________________________ C
ollapse Curve _____________________________________________________________________________ 425
148. ___________________________________________________________________ C
ollapse Surface ____________________________________________________________________________ 427
149. ___________________________________________________________________ S
implify Geometry __________________________________________________________________________ 429
Feature Angle
Automatically Compositing Curves
Respecting Vertices, Curves and Surfaces
Respecting Imprints
Using Local Normals
Other Options
430
430
430
430
431
431
150. ___________________________________________________________________ D
eleting Virtual Geometry ____________________________________________________________________ 433
Removing Virtual Geometry
Using The Delete Command With Composites
Using the Delete Command With Partitions
433
433
433
151. ___________________________________________________________________ G
eometry Orientation ________________________________________________________________________ 435
Adjusting Orientation
435
152. ___________________________________________________________________ B
asic Group Operations ______________________________________________________________________ 437
Geometry Groups
Modifying groups by comparing common entities
437
437
xv
Trelis 15.0 User Documentation
Mesh Groups
Deleting Groups
Cleaning Out Groups
438
438
438
153. ___________________________________________________________________ G
roups in Graphics __________________________________________________________________________ 439
154. ___________________________________________________________________ P
ropagated Hex Groups ______________________________________________________________________ 441
Propagated Hex Group Starting on a Surface
Ending at a Surface
Number of Times
Ending at a Surface with Multiple
Number of Times with Multiple
Ending at Surface with Direction
Number of Times with Direction
Propagated Hex Group Starting on a Face
Ending at a Surface
Ending at a Face
Number of Times
Ending at a Surface with Multiple
Ending at a Face with Multiple
Number of Times with Multiple
Ending at Face with Direction
Ending at Surface with Direction
Number of Times with Direction
Naming Convention for Propagated Hex Groups
441
441
441
442
442
442
443
443
443
443
444
444
444
444
445
445
445
446
155. ___________________________________________________________________ S
eeded Mesh Groups ________________________________________________________________________ 449
156. ___________________________________________________________________ Q
uality Groups______________________________________________________________________________ 453
157. ___________________________________________________________________ E
ntity Names _______________________________________________________________________________ 455
Valid and Invalid Names
Reconciling Duplicate Names
Automatic Name Creation
Automatic Name Propagation
Naming Merged Entities
455
455
455
456
456
158. ___________________________________________________________________ E
ntity IDs __________________________________________________________________________________ 459
Element Ids
Gaps in ID space
Renumbering IDs
Volume ID
xvi
459
459
459
459
Table of Contents
159. ___________________________________________________________________ A
ttribute Behavior ___________________________________________________________________________ 461
160. ___________________________________________________________________ A
ttribute Types _____________________________________________________________________________ 463
161. ___________________________________________________________________ A
ttribute Commands _________________________________________________________________________ 465
Control By Attribute Type or Geometric Entity
465
162. ___________________________________________________________________ U
sing Trelis Attributes _______________________________________________________________________ 467
163. ___________________________________________________________________ E
ntity Measurement _________________________________________________________________________ 469
Measure Between
Measure Small
Measure Angle
Measure Void
469
469
469
470
164. ___________________________________________________________________ E
xporting ACIS Files _________________________________________________________________________ 471
165. ___________________________________________________________________ E
xporting STEP Files ________________________________________________________________________ 473
166. ___________________________________________________________________ E
xporting IGES Files_________________________________________________________________________ 475
167. ___________________________________________________________________ E
xporting Facet Files ________________________________________________________________________ 477
168. ___________________________________________________________________ G
eometry Deletion ___________________________________________________________________________ 479
169. ___________________________________________________________________ M
eshing the Geometry _______________________________________________________________________ 481
Default Scheme and Interval Selection
Continuing Meshing After a Mesh Failure
481
481
170. ___________________________________________________________________ I
nterval Firmness ___________________________________________________________________________ 483
Precedence
483
171. ___________________________________________________________________ E
xplicit Specification of Intervals ______________________________________________________________ 485
172. ___________________________________________________________________ A
utomatic Specification of Interval Size _________________________________________________________ 487
Automatic Interval Size Specification
Maximum Spanning Angle on Arcs
488
489
xvii
Trelis 15.0 User Documentation
173. ___________________________________________________________________ I
nterval Matching ___________________________________________________________________________ 491
174. ___________________________________________________________________ P
eriodic Intervals ___________________________________________________________________________ 493
175. ___________________________________________________________________ R
elative Intervals ____________________________________________________________________________ 495
176. ___________________________________________________________________ M
esh Interval Preview ________________________________________________________________________ 497
177. ___________________________________________________________________ B
ias, Dualbias ______________________________________________________________________________ 499
178. ___________________________________________________________________ C
ircle _____________________________________________________________________________________ 501
179. ___________________________________________________________________ C
urvature __________________________________________________________________________________ 503
180. ___________________________________________________________________ E
qual _____________________________________________________________________________________ 505
181. ___________________________________________________________________ H
ole_______________________________________________________________________________________ 507
182. ___________________________________________________________________ M
apping ___________________________________________________________________________________ 509
183. ___________________________________________________________________ P
ave ______________________________________________________________________________________ 511
Element Shape Improvement
Controlling Flattening of Elements
Controlling the Grid Search for Intersection Checking
Controlling the Paver Sizing Function
Controlling Paver Cleanup
xviii
511
512
512
512
512
Table of Contents
184. ___________________________________________________________________ P
entagon __________________________________________________________________________________ 515
185. ___________________________________________________________________ P
inpoint ___________________________________________________________________________________ 517
186. ___________________________________________________________________ P
olyhedron ________________________________________________________________________________ 519
187. ___________________________________________________________________ S
phere ____________________________________________________________________________________ 523
188. ___________________________________________________________________ S
Transition _________________________________________________________________________________ 525
189. ___________________________________________________________________ S
tretch ____________________________________________________________________________________ 529
190. ___________________________________________________________________ S
tride _____________________________________________________________________________________ 531
191. ___________________________________________________________________ S
ubmap ___________________________________________________________________________________ 533
192. ___________________________________________________________________ S
urface Vertex Types ________________________________________________________________________ 537
Surface Vertex Commands
Listing and Drawing Vertex Types
Triangle Vertex Types
Adjusting the Automatic Vertex Type Selection Algorithm
Volume Curve Types
537
538
538
538
539
193. ___________________________________________________________________ S
weep _____________________________________________________________________________________ 541
Multisweep
•
Grouping Sweepable Volumes
Node Redistribution
543
545
545
194. ___________________________________________________________________ T
etMesh ___________________________________________________________________________________ 549
Discussion
Tetmesher Options
Using tets as the basis of an unstructured hexahedral mesh
Conforming the tetmesh to internal features
Generating a Tetmesh from a Skin of Triangles
549
550
551
551
553
xix
Trelis 15.0 User Documentation
195. ___________________________________________________________________ T
etprimitive ________________________________________________________________________________ 555
196. ___________________________________________________________________ T
riDelaunay ________________________________________________________________________________ 557
197. ___________________________________________________________________ T
riAdvance ________________________________________________________________________________ 559
198. ___________________________________________________________________ T
riMap ____________________________________________________________________________________ 561
199. ___________________________________________________________________ T
riMesh ___________________________________________________________________________________ 563
200. ___________________________________________________________________ T
riPave ____________________________________________________________________________________ 565
201. ___________________________________________________________________ T
riPrimitive ________________________________________________________________________________ 567
202. ___________________________________________________________________ R
adialmesh ________________________________________________________________________________ 569
203. ___________________________________________________________________ H
Tet _______________________________________________________________________________________ 575
Unstructured
Structured
575
576
204. ___________________________________________________________________ Q
Tri _______________________________________________________________________________________ 577
205. ___________________________________________________________________ T
Hex ______________________________________________________________________________________ 579
206. ___________________________________________________________________ T
Quad _____________________________________________________________________________________ 581
207. ___________________________________________________________________ C
opying a Mesh _____________________________________________________________________________ 583
208. ___________________________________________________________________ M
irroring a Mesh ____________________________________________________________________________ 585
209. ___________________________________________________________________ A
utomatic Scheme Selection __________________________________________________________________ 587
Default Scheme Selection
Auto Scheme Selection General Notes
Scheme Firmness
Surface Auto Scheme Selection
Volume Auto Scheme Selection
xx
587
587
588
589
589
Table of Contents
210. ___________________________________________________________________ P
arallel Meshing ____________________________________________________________________________ 591
211. ___________________________________________________________________ M
etrics for Edge Elements ____________________________________________________________________ 593
Quality Metric Definitions:
Comments on Algebraic Quality Measures
593
593
212. ___________________________________________________________________ M
etrics for Triangular Elements ________________________________________________________________ 595
Approximate Triangular Quality Definitions:
Comments on Algebraic Quality Measures
References for Triangular Quality Measures
595
595
596
213. ___________________________________________________________________ M
etrics for Quadrilateral Elements _____________________________________________________________ 597
Quadrilateral Quality Definitions
Comments on Algebraic Quality Measures
References for Quadrilateral Quality Measures
Details on Robinson Metrics for Quadrilaterals
597
598
598
599
214. ___________________________________________________________________ M
etrics for Tetrahedral Elements _______________________________________________________________ 601
Tetrahedral Quality Definitions
References for Tetrahedral Quality Measures
601
602
215. ___________________________________________________________________ M
etrics for Hexahedral Elements _______________________________________________________________ 603
Hexahedral Quality Definitions
References for Hexahedral Quality Measures
603
604
216. ___________________________________________________________________ M
esh Quality Command Syntax ________________________________________________________________ 605
Quality Options
Scope
Draw
List
Filter
605
605
605
606
606
217. ___________________________________________________________________ M
esh Quality Example Output _________________________________________________________________ 609
218. ___________________________________________________________________ A
utomatic Mesh Quality Assessment ___________________________________________________________ 611
219. ___________________________________________________________________ C
ontrolling Mesh Quality _____________________________________________________________________ 613
Skew Control
Propagate Curve Bias
Adjust Boundary
613
613
614
xxi
Trelis 15.0 User Documentation
220. ___________________________________________________________________ C
oincident Node Check ______________________________________________________________________ 615
221. ___________________________________________________________________ M
esh Topology Check ________________________________________________________________________ 617
222. ___________________________________________________________________ C
entroid Area Pull ___________________________________________________________________________ 621
223. ___________________________________________________________________ E
quipotential _______________________________________________________________________________ 623
224. ___________________________________________________________________ L
aplacian __________________________________________________________________________________ 625
225. ___________________________________________________________________ S
mart Laplacian ____________________________________________________________________________ 627
226. ___________________________________________________________________ C
ondition Number ___________________________________________________________________________ 629
227. ___________________________________________________________________ M
ean Ratio _________________________________________________________________________________ 631
228. ___________________________________________________________________ W
inslow____________________________________________________________________________________ 633
229. ___________________________________________________________________ U
ntangle ___________________________________________________________________________________ 635
230. ___________________________________________________________________ E
dge Length _______________________________________________________________________________ 637
231. ___________________________________________________________________ M
esh Refinement ____________________________________________________________________________ 639
Global Mesh Refinement
Refining at a Geometric or Mesh Feature
Hexahedral Refinement Using Sheet Insertion
Refining at a Geometric Feature
Refining along a path
Refining a Hex Sheet
Directional Refinement
Hex Sheet Drawing
Local Refinement of Triangles and Edges
'N' Tets Through the Thickness Refinement
Measuring the Number of Tets through the Thickness
Parallel Refinement
xxii
639
640
643
643
643
644
646
648
648
649
650
650
Table of Contents
232. ___________________________________________________________________ M
esh Pillowing ______________________________________________________________________________ 653
233. ___________________________________________________________________ M
esh Coarsening ____________________________________________________________________________ 655
Hexahedral Coarsening
Extracting a Single Hex Sheet
Extracting multiple sheets along a curve
Uniform hex coarsening
655
655
655
656
234. ___________________________________________________________________ N
ode and Nodeset Repositioning ______________________________________________________________ 657
235. ___________________________________________________________________ C
ollapsing Mesh Edges ______________________________________________________________________ 659
236. ___________________________________________________________________ A
lign Mesh _________________________________________________________________________________ 661
237. ___________________________________________________________________ C
reating and Merging Mesh Elements __________________________________________________________ 663
Creating Mesh Elements
Creating Hex and Tet Elements
Creating Wedge Elements
Creating Face and Tri Elements
Creating Edge Elements
Creating Nodes
Merging Nodes
663
663
665
665
666
666
666
238. ___________________________________________________________________ C
leaning Up a Tetrahedral Mesh _______________________________________________________________ 669
239. ___________________________________________________________________ M
esh Validity _______________________________________________________________________________ 671
240. ___________________________________________________________________ G
eometry Adaptive Sizing Function (Skeleton Sizing) _____________________________________________ 673
Skeleton Sizing Behaviors
Command Line Syntax
Basic Arguments
Scaling and Accuracy Arguments:
Advanced Arguments
Lattice Arguments:
Source Entity Arguments
Skeleton with Other Sizing Controls
Limitations
675
675
675
675
676
676
676
676
677
xxiii
Trelis 15.0 User Documentation
241. ___________________________________________________________________ B
ias Sizing Function _________________________________________________________________________ 679
242. ___________________________________________________________________ C
onstant Sizing Function _____________________________________________________________________ 685
243. ___________________________________________________________________ C
urvature Sizing Function ____________________________________________________________________ 687
244. ___________________________________________________________________ L
inear Sizing Function _______________________________________________________________________ 689
245. ___________________________________________________________________ I
nterval Sizing Function _____________________________________________________________________ 691
246. ___________________________________________________________________ I
nverse Sizing Function _____________________________________________________________________ 693
247. ___________________________________________________________________ E
xodus II-based Field Function ________________________________________________________________ 695
Curve Meshing with Exodus II - based Field Functions
696
248. ___________________________________________________________________ I
mporting Exodus II Files ____________________________________________________________________ 697
Importing a Free Mesh Without Geometry
Importing a Mesh Onto Existing Geometry
Importing a Mesh with Nodeset Associativity
Importing a Mesh onto Modified Geometry
Mesh Import Tolerance
Specifying a Portion of the Mesh to be Imported
Unique Genesis IDs and Shell Options
Nodeset Ordering
Creating Mesh-Based Geometry on Import
File Name
Blocks
Start ID
Nodesets/Sidesets
Feature Angle
Smooth Curves and Surfaces
Apply Deformations
Merge
Merge Nodes
Export Facets
xxiv
697
698
698
698
699
699
699
699
699
700
700
700
700
701
701
702
703
703
703
Table of Contents
249. ___________________________________________________________________ I
mporting Abaqus Files ______________________________________________________________________ 705
250. ___________________________________________________________________ I
mporting I-DEAS Files ______________________________________________________________________ 707
251. ___________________________________________________________________ I
mporting Patran Files _______________________________________________________________________ 709
252. ___________________________________________________________________ I
mporting 2D Exodus Files ___________________________________________________________________ 711
253. ___________________________________________________________________ M
esh Deletion ______________________________________________________________________________ 713
Automatic Mesh Deletion
713
254. ___________________________________________________________________ F
ree Meshes _______________________________________________________________________________ 715
Creating a free mesh
Disassociating a mesh from its geometry
Creating Mesh-Based Geometry to fit a Free Mesh
Merging a free mesh
Free Mesh Transformation Operations
Extruding Mesh Elements
Offsetting Mesh Elements
Revolving Mesh Elements
Smoothing a free mesh
Mesh quality on a free mesh
Mesh refinement on a free mesh
Cleaning up a free mesh
Assigning boundary conditions
Skinning a free mesh
Deleting free mesh elements
Bottom-up element creation
Exporting free meshes
715
715
716
716
716
717
718
719
720
721
721
721
721
723
723
723
723
255. ___________________________________________________________________ S
kinning a Mesh ____________________________________________________________________________ 725
256. ___________________________________________________________________ E
lement Block Specification __________________________________________________________________ 727
Creating Element Blocks
Assigning a Name or Description to an Element Block
Defining the Element Type
Default Element Blocks
Duplicate Block Elements
Assigning Attributes to Blocks
Displaying Element Blocks
Deleting Element Blocks
Automatically Assigning Mesh Edges to a Block (Rebar)
Diagonal and Orthogonal Rebar Blocks
Specifying a set of nodes
Creating Spider Blocks
Creating Beam Blocks
Creating Spring Blocks
727
728
728
729
729
729
730
730
731
731
732
733
734
735
xxv
Trelis 15.0 User Documentation
2D Elements
Mixed Element Output
Adding Materials to a Block
735
735
736
257. ___________________________________________________________________ N
odeset and Sideset Specification _____________________________________________________________ 737
Creating Nodesets and Sidesets
Useful hint:
Assigning Names and Descriptions to Nodesets and Sidesets
Grouping Faces on a Surface into a Sideset
Grouping elements in voids and enclosures
Deleting Nodesets and Sidesets
Displaying Nodesets and Sidesets
Nodeset Associativity Data
Equation-Controlled Distribution Factors
Nodesets/Sidesets/Blocks Behavior with Geometric Entity Copy
737
738
739
739
740
740
741
741
742
743
258. ___________________________________________________________________ N
odeset and Sideset Specification _____________________________________________________________ 745
Creating Nodesets and Sidesets
Useful hint:
Assigning Names and Descriptions to Nodesets and Sidesets
Grouping Faces on a Surface into a Sideset
Grouping elements in voids and enclosures
Deleting Nodesets and Sidesets
Displaying Nodesets and Sidesets
Nodeset Associativity Data
Equation-Controlled Distribution Factors
Nodesets/Sidesets/Blocks Behavior with Geometric Entity Copy
745
746
747
747
748
748
749
749
750
751
259. ___________________________________________________________________ E
xodus II File Specification ___________________________________________________________________ 753
Exodus II Manual
Element Block Definition Examples
Multiple Element Blocks
Surface Mesh Only
Two-dimensional Mesh
753
753
753
753
753
260. ___________________________________________________________________ E
xodus II Model Title_________________________________________________________________________ 755
261. ___________________________________________________________________ E
xodus Coordinate Frames ___________________________________________________________________ 757
262. ___________________________________________________________________ D
efining Materials and Media Types ____________________________________________________________ 759
263. ___________________________________________________________________ B
oundary Condition Sets _____________________________________________________________________ 761
*** ABAQUS Parameters ***
*** NASTRAN Parameters ***
xxvi
761
761
Table of Contents
264. ___________________________________________________________________ U
sing Restraints ____________________________________________________________________________ 763
Displacements/Accelerations/Velocities
Fixed or Free
Displacement Combinations
Temperature
Top, Gradient, Middle, Bottom
763
765
765
765
766
265. ___________________________________________________________________ U
sing Loads ________________________________________________________________________________ 767
Forces
Using Pressure
Value
Pressure and Total Force
Top and Bottom
Using Heat Flux
Top and Bottom Values
Using Convection
Surrounding
Coefficient
767
767
768
768
768
768
769
769
769
769
266. ___________________________________________________________________ U
sing Contact Surfaces ______________________________________________________________________ 771
The Contact Region
The Contact Pair
Auto-Contact Tool
771
771
772
267. ___________________________________________________________________ U
sing Contact Surfaces ______________________________________________________________________ 773
The Contact Region
The Contact Pair
Auto-Contact Tool
773
773
774
268. ___________________________________________________________________ U
sing CFD Boundary Conditions ______________________________________________________________ 775
Inlet Velocity
Inlet Pressure
Inlet Massflow
Outlet Pressure
Farfield Pressure
Symmetry
775
775
775
776
776
776
269. ___________________________________________________________________ M
iscellaneous Boundary Condition Commands __________________________________________________ 777
Delete
List
Draw
Highlight
777
777
777
778
xxvii
Trelis 15.0 User Documentation
270. ___________________________________________________________________ E
xporting Sierra Files ________________________________________________________________________ 779
271. ___________________________________________________________________ D
efining PARAMS for NASTRAN _______________________________________________________________ 781
272. ___________________________________________________________________ F
inite Element Model ________________________________________________________________________ 783
273. ___________________________________________________________________ E
xporting an Exodus II File ___________________________________________________________________ 785
Element and Node ID Maps
Exporting a Parallel Mesh for pCAMAL
Converting an Exodus II file to ASCII
Controlling Exodus II Output Precision
Large Exodus Format
785
785
786
786
786
274. ___________________________________________________________________ I
nstancing Parts with ABAQUS _______________________________________________________________ 787
275. ___________________________________________________________________ E
xporting Fluent Grid Files ___________________________________________________________________ 789
276. ___________________________________________________________________ T
ransforming Mesh Coordinates_______________________________________________________________ 791
277. ___________________________________________________________________ A
utomatic Detail Suppression _________________________________________________________________ 793
Example
793
278. ___________________________________________________________________ A
utomatic Geometry Decomposition ___________________________________________________________ 795
279. ___________________________________________________________________ C
ohesive Elements __________________________________________________________________________ 797
Multiple Curves in FLATQUAD Blocks
797
280. ___________________________________________________________________ D
eleting Mesh Elements ______________________________________________________________________ 801
281. ___________________________________________________________________ F
eatureSize ________________________________________________________________________________ 803
282. ___________________________________________________________________ G
eometry Tolerant Meshing ___________________________________________________________________ 805
Initial Mesh Size
Fixing a Geometric Entity
Tolerance Fraction
Creating the tolerant mesh
Fem/New/Old Options
Free Mesh vs. Mesh-Based Geometry
Quadrilateral Surface Mesh
Examples
xxviii
806
806
806
806
807
807
807
808
Table of Contents
Limitations
Accumulated geometric error
Loss of Resolution due to initial faceting
Surface to Surface proximity
Mesh size on fixed geometry entities
810
810
810
811
812
283. ___________________________________________________________________ M
esh Cutting _______________________________________________________________________________ 813
Coordinate Plane
Planar Surface
Plane from 3 points
Extended Surface
Meshcut Options
Meshcutting Scope
Meshcutting Example
813
813
813
814
814
814
814
284. ___________________________________________________________________ M
esh Grafting_______________________________________________________________________________ 821
Grafting Options
Grafting Scope
821
821
285. ___________________________________________________________________ O
ptimize Jacobian ___________________________________________________________________________ 825
286. ___________________________________________________________________ R
andomize _________________________________________________________________________________ 827
287. ___________________________________________________________________ R
efine Mesh Boundary _______________________________________________________________________ 829
288. ___________________________________________________________________ S
culpting __________________________________________________________________________________ 831
289. ___________________________________________________________________ S
uper Sizing Function _______________________________________________________________________ 833
290. ___________________________________________________________________ T
est Sizing Function _________________________________________________________________________ 835
291. ___________________________________________________________________ T
ransition__________________________________________________________________________________ 837
292. ___________________________________________________________________ T
riangle Mesh Coarsening ____________________________________________________________________ 841
293. ___________________________________________________________________ W
hisker Weave ______________________________________________________________________________ 843
Whisker Weaving Basic Commands
Whisker Weaving Options
844
844
xxix
Trelis 15.0 User Documentation
294. ___________________________________________________________________ A
vailable Colors ____________________________________________________________________________ 847
295. ___________________________________________________________________ E
lement Numbering _________________________________________________________________________ 851
Node Numbering
Side Numbering
Triangular Shell Element Numbering
Node Ordering
Side Set Side Ordering
851
851
851
852
852
296. ___________________________________________________________________ F
ullHex vs. NodeHex Representation ___________________________________________________________ 855
297. ___________________________________________________________________ A
PREPRO Syntax ___________________________________________________________________________ 857
298. ___________________________________________________________________ A
PREPRO Rules ____________________________________________________________________________ 859
1. Functions
2. Variables
3. Numbers
4. Strings
5. Operators
6. Delimiters
7. Expressions
8. Algebraic Expressions
9. String Expressions
10. Relational Expressions
11. Conditional Expressions
859
859
859
859
859
859
859
859
860
860
860
299. ___________________________________________________________________ A
PREPRO Operators ________________________________________________________________________ 861
1. Arithmetic Operators
2. Assignment Operators
3. Relational Operators
4. Boolean Operators
5. String Operators
861
862
862
863
863
300. ___________________________________________________________________ A
PREPRO Predefined Variables _______________________________________________________________ 865
301. ___________________________________________________________________ A
PREPRO Units_____________________________________________________________________________ 867
302. ___________________________________________________________________ A
PREPRO Functions ________________________________________________________________________ 871
1. Mathematical Functions
2. CUBIT Functions
3.String Functions
871
873
879
303. ___________________________________________________________________ A
PREPRO Additional Functionality _____________________________________________________________ 883
1. File Inclusion
xxx
883
Table of Contents
2. Conditionals
3. Loops
883
883
304. ___________________________________________________________________ A
PREPRO Journaling ________________________________________________________________________ 885
APREPRO Comments
Significant Figures
885
885
305. ___________________________________________________________________ C
ubitInterface ______________________________________________________________________________ 887
Class Member Functions
Class Variables
Member Function Documentation
init(argv)
destroy()
set_cubit_interrupt(interrupt)
set_playback_paused_on_error(pause)
Bool is_playback_paused_on_error()
Bool developer_commands_are_enabled()
str get_version()
str get_revision_date()
str get_build_number()
str get_acis_version()
int get_acis_version_as_int()
str get_exodus_version()
str get_graphics_version()
print_cmd_options()
Bool is_modified()
set_modified()
Bool is_undo_save_needed()
set_undo_saved()
Bool is_command_echoed()
Bool is_volume_meshable(volume_id)
journal_commands(state)
Bool is_command_journaled()
str get_current_journal_file()
cmd(input_string)
silent_cmd(input_string)
[ int ] parse_cubit_list(type, int_list, include_sheet_bodies)
print_raw_help(input_line, order_dependent, consecutive_dependent)
int get_error_count()
[ str ] get_mesh_error_solutions(error_code)
float get_view_distance()
[ float ] get_view_at()
[ float ] get_view_from()
reset_camera()
unselect_entity(entity_type, entity_id)
Bool is_perspective_on()
Bool is_occlusion_on()
Bool is_scale_visibility_on()
Bool is_select_partial_on()
int get_rendering_mode()
set_rendering_mode(mode)
clear_preview()
str get_pick_type()
float get_mesh_edge_length(edge_id)
float get_meshed_volume_or_area(geom_type, entity_ids)
887
899
899
899
899
900
900
900
900
900
900
901
901
901
901
901
901
901
902
902
902
902
902
902
903
903
903
903
903
904
904
904
904
904
905
905
905
905
905
906
906
906
906
906
906
906
907
xxxi
Trelis 15.0 User Documentation
int get_mesh_intervals(geom_type, entity_id)
float get_mesh_size(geom_type, entity_id)
float get_auto_size(volume_id_list, size)
float get_quality_value(mesh_type, mesh_id, metric_name)
str get_mesh_scheme(geom_type, entity_id)
str get_mesh_scheme_firmness(geom_type, entity_id)
str get_mesh_interval_firmness(geom_type, entity_id)
Bool is_meshed(geom_type, entity_id)
Bool is_merged(geom_type, entity_id)
str get_smooth_scheme(geom_type, entity_id)
int get_hex_count()
int get_pyramid_count()
int get_tet_count()
int get_quad_count()
int get_tri_count()
int get_edge_count()
int get_node_count()
int get_volume_element_count(volume_id)
Bool volume_contains_tets(volume_id)
int get_surface_element_count(surface_id)
[ int ] get_hex_sheet(node_id_1, node_id_2)
Bool is_visible(geom_type, entity_id)
ERROR: EOF in multi-line statement
Bool is_virtual(geom_type, entity_id)
ERROR: EOF in multi-line statement
Bool contains_virtual(geom_type, entity_id)
ERROR: EOF in multi-line statement
[ int ] get_source_surfaces(volume_id)
[ int ] get_target_surfaces(volume_id)
int get_common_curve_id(surface_1_id, surface_2_id)
int get_common_vertex_id(curve_1_id, curve_2_id)
str get_merge_setting(geom_type, entity_id)
str get_curve_type(curve_id)
str get_surface_type(surface_id)
[ float ] get_surface_normal(surface_id)
[ float ] get_surface_centroid(surface_id)
str get_surface_sense(surface_id)
[ str ] get_entity_modeler_engine(geom_type, entity_id)
[ float ] get_bounding_box(geom_type, entity_id)
[ float ] get_total_bounding_box(geom_type, entity_list)
float get_total_volume(volume_list)
str get_entity_name(geom_type, entity_id)
int get_entity_color_index(entity_type, entity_id)
Bool is_multi_volume(body_id)
Bool is_sheet_body(volume_id)
Bool is_interval_count_odd(surface_id)
Bool is_periodic(geom_type, entity_id)
Bool is_surface_planer(surface_id)
Bool get_undo_enabled()
int number_undo_commands()
[ str ] get_aprepro_vars()
str get_aprepro_value_as_string(var_name)
Bool get_node_constraint()
str get_vertex_type(surface_id, vertex_id)
[ int ] get_relatives(source_geom_type, source_id, target_geom_type)
[ int ] get_adjacent_surfaces(geom_type, entity_id)
[ int ] get_adjacent_volumes(geom_type, entity_id)
[ int ] get_entities(geom_type, include_sheet_bodies)
xxxii
907
907
908
908
908
909
909
909
910
910
910
911
911
911
911
911
911
912
912
912
912
912
913
913
913
913
913
914
914
914
914
915
915
915
915
916
916
916
917
917
917
918
918
918
918
919
919
919
920
920
920
920
920
920
920
921
921
922
Table of Contents
[ int ] get_list_of_free_ref_entities(geom_type)
int get_owning_body(geom_type, entity_id)
int get_owning_volume(geom_type, entity_id)
int get_owning_volume_by_name(entity_name)
float get_curve_length(curve_id)
float get_arc_length(curve_id)
float get_distance_from_curve_start(x, y, z, curve_id)
float get_curve_radius(curve_id)
[ float ] get_curve_center(curve_id)
float get_surface_area(surface_id)
float get_volume_area(volume_id)
float get_hydraulic_radius_surface_area(surface_id)
float get_hydraulic_radius_volume_area(volume_id)
[ float ] get_center_point(entity_type, entity_id)
int get_valence(vertex_id)
float get_distance_between(vertex_id_1, vertex_id_2)
print_surface_summary_stats()
print_volume_summary_stats()
int get_volume_count()
int get_surface_count()
int get_vertex_count()
int get_curve_count()
int get_curve_count(target_volume_ids)
Bool is_catia_engine_available()
[ int ] evaluate_exterior_angle(curve_list, test_angle)
[ int ] get_small_curves(target_volume_ids, mesh_size)
[ int ] get_smallest_curves(target_volume_ids, num_to_return)
[ int ] get_small_surfaces(target_volume_ids, mesh_size)
[ int ] get_narrow_surfaces(target_volume_ids, mesh_size)
[ int ] get_small_and_narrow_surfaces(target_ids, small_area, small_curve_size)
[ int ] get_surfs_with_narrow_regions(target_ids, narrow_size)
[ int ] get_small_volumes(target_volume_ids, mesh_size)
[ int ] get_blend_surfaces(target_volume_ids)
[ int ] get_small_loops(target_volume_ids, mesh_size)
[ int ] get_tangential_intersections(target_volume_ids, upper_bound, lower_bound)
[ int ] get_coincident_vertices(target_volume_ids, high_tolerance)
[ [ str ] ] get_solutions_for_near_coincident_vertices(vertex_id1, vertex_id2)
[ [ str ] ] get_solutions_for_imprint_merge(surface_id1, surface_id2)
[ [ str ] ] get_solutions_for_small_surfaces(surface_id, small_curve_size, mesh_size)
[ [ str ] ] get_solutions_for_small_curves(curve_id, small_curve_size, mesh_size)
[ [ str ] ] get_solutions_for_surfaces_with_narrow_regions(surface_id, small_curve_size, mesh_size)
[ int ] get_overlapping_volumes(target_volume_ids)
[ [ int ] ] get_mergeable_vertices(target_volume_ids)
[ [ str ] ] get_solutions_for_blends(surface_id)
[ [ int ] ] get_blend_chains(surface_id)
float get_merge_tolerance()
str get_exodus_entity_name(entity_type, entity_id)
str get_exodus_entity_description(entity_type, entity_id)
[ float ] get_all_exodus_times(filename)
int get_block_id(entity_type, entity_id)
[ int ] get_block_ids(mesh_geom_file_name)
[ int ] get_block_id_list()
[ int ] get_nodeset_id_list()
[ int ] get_sideset_id_list()
[ int ] get_bc_id_list(bc_type_in)
str get_bc_name(bc_type_in, bc_id)
[ int ] get_nodeset_id_list_for_bc(bc_type_in, bc_id)
[ int ] get_sideset_id_list_for_bc(bc_type_in, bc_id)
922
922
923
923
923
924
924
924
924
925
925
925
925
925
926
926
926
926
926
927
927
927
927
927
927
928
928
928
929
929
929
929
930
930
930
930
931
931
931
932
932
932
932
933
933
933
933
934
934
934
935
935
935
935
935
936
936
936
xxxiii
Trelis 15.0 User Documentation
int get_next_sideset_id()
int get_next_nodeset_id()
int get_next_block_id()
[ int ] get_block_volumes(block_id)
[ int ] get_block_surfaces(block_id)
[ int ] get_block_curves(block_id)
[ int ] get_block_vertices(block_id)
[ int ] get_block_nodes(block_id)
[ int ] get_block_edges(block_id)
[ int ] get_block_tris(block_id)
[ int ] get_block_faces(block_id)
[ int ] get_block_pyramids(block_id)
[ int ] get_block_tets(block_id)
[ int ] get_block_hexes(block_id)
[ int ] get_volume_hexes(volume_id)
[ int ] get_volume_tets(volume_id)
[ int ] get_nodeset_volumes(nodeset_id)
[ int ] get_nodeset_surfaces(nodeset_id)
[ int ] get_nodeset_curves(nodeset_id)
[ int ] get_nodeset_vertices(nodeset_id)
[ int ] get_nodeset_nodes(nodeset_id)
[ int ] get_nodeset_nodes_inclusive(nodeset_id)
[ int ] get_sideset_curves(sideset_id)
[ int ] get_curve_edges(curve_id)
[ int ] get_sideset_surfaces(sideset_id)
[ int ] get_sideset_quads(sideset_id)
[ int ] get_surface_quads(surface_id)
[ int ] get_surface_tris(surface_id)
str get_entity_sense(source_type, source_id, sideset_id)
str get_wrt_entity(source_type, source_id, sideset_id)
Bool is_using_shells(sideset_id)
[ str ] get_geometric_owner(mesh_entity_type, mesh_entity_list)
[ int ] get_volume_nodes(vol_id)
[ int ] get_surface_nodes(surf_id)
[ int ] get_curve_nodes(curv_id)
int get_vertex_node(vert_id)
int get_id_from_name(name)
[ int ] get_group_groups(group_id)
[ int ] get_group_volumes(group_id)
[ int ] get_group_surfaces(group_id)
[ int ] get_group_curves(group_id)
[ int ] get_group_vertices(group_id)
[ int ] get_group_nodes(group_id)
[ int ] get_group_edges(group_id)
[ int ] get_group_quads(group_id)
[ int ] get_group_tris(group_id)
[ int ] get_group_tets(group_id)
[ int ] get_group_hexes(group_id)
int get_next_group_id()
delete_all_groups()
delete_group(group_id)
set_max_group_id(max_group_id)
int create_new_group()
remove_entity_from_group(group_id, entity_id, entity_type)
add_entity_to_group(group_id, entity_id, entity_type)
[ int ] get_mesh_group_parent_ids(element_type, element_id)
Bool is_mesh_element_in_group(element_type, element_id)
Bool is_part_of_list(target_id, id_list)
xxxiv
936
937
937
937
937
937
938
938
938
938
939
939
939
939
939
940
940
940
940
941
941
941
941
942
942
942
942
942
943
943
943
944
944
944
945
945
945
945
945
946
946
946
946
946
946
947
947
947
947
947
947
948
948
948
948
949
949
949
Table of Contents
int get_last_id(entity_type)
str get_assembly_classification_level()
str get_assembly_classification_category()
str get_assembly_weapons_category()
str get_assembly_metadata(volume_id, data_type)
Bool is_assembly_metadata_attached(volume_id)
str get_assembly_name(assembly_id)
str get_assembly_path(assembly_id)
str get_assembly_description(assembly_id)
int get_assembly_instance(assembly_id)
str get_assembly_file_format(assembly_id)
str get_assembly_units(assembly_id)
str get_assembly_material_description(assembly_id)
str get_assembly_material_specification(assembly_id)
int get_exodus_id(entity_type, entity_id)
str get_geometry_owner(entity_type, entity_id)
[ int ] get_connectivity(entity_type, entity_id)
[ int ] get_expanded_connectivity(entity_type, entity_id)
[ int ] get_sub_elements(entity_type, entity_id, dimension)
[ float ] get_nodal_coordinates(node_id)
Bool get_node_position_fixed(node_id)
str get_sideset_element_type(sideset_id)
str get_block_element_type(block_id)
int get_exodus_element_count(entity_id, entity_type)
int get_block_attribute_count(block_id)
float get_block_attribute_value(block_id, index)
[ str ] get_valid_block_element_types(block_id)
int get_nodeset_node_count(nodeset_id)
int get_geometry_node_count(entity_type, entity_id)
str get_mesh_element_type(entity_type, entity_id)
Bool is_on_thin_shell(bc_type_in, entity_id)
Bool temperature_is_on_solid(bc_type_in, entity_id)
Bool convection_is_on_solid(entity_id)
Bool convection_is_on_shell_area(entity_id, shell_area)
float get_convection_coefficient(entity_id, cc_type)
float get_bc_temperature(bc_type, entity_id, temp_type)
Bool temperature_is_on_shell_area(bc_type, bc_area, entity_id)
Bool heatflux_is_on_shell_area(bc_area, entity_id)
float get_heatflux_on_area(bc_area, entity_id)
int get_cfd_type(entity_id)
float get_contact_pair_friction_value(entity_id)
float get_contact_pair_tolerance_value(entity_id)
Bool get_contact_pair_tied_state(entity_id)
Bool get_contact_pair_general_state(entity_id)
Bool get_contact_pair_exterior_state(entity_id)
int get_displacement_coord_system(entity_id)
str get_displacement_combine_type(entity_id)
float get_pressure_value(entity_id)
str get_pressure_function(entity_id)
float get_force_magnitude(entity_id)
float get_moment_magnitude(entity_id)
[ float ] get_force_direction_vector(entity_id)
[ float ] get_force_moment_vector(entity_id)
str get_constraint_type(constraint_id)
str get_constraint_reference_point(constraint_id)
str get_constraint_dependent_entity_point(constraint_id)
float get_material_property(mp, entity_id)
int get_media_property(entity_id)
949
950
950
950
950
951
951
951
951
951
952
952
952
952
953
953
953
954
954
955
955
955
955
955
956
956
956
957
957
957
957
957
958
958
958
958
958
959
959
959
959
959
960
960
960
960
960
960
961
961
961
961
961
961
962
962
962
962
xxxv
Trelis 15.0 User Documentation
[ str ] get_material_name_list()
[ str ] get_media_name_list()
set_label_type(entity_type, label_flag)
int get_label_type(entity_type)
Body body(id_in)
Volume volume(id_in)
Surface surface(id_in)
Curve curve(id_in)
Vertex vertex(id_in)
reset()
Body brick(width, depth, height)
Body sphere(radius, x_cut, y_cut, z_cut, inner_radius)
Body prism(height, sides, major, minor)
Body pyramid(height, sides, major, minor, top)
Body cylinder(hi, r1, r2, r3)
Body torus(r1, r2)
Vertex create_vertex(x, y, z)
Curve create_curve(v0, v1)
Body create_surface(curves)
[ Body] sweep_curve(curves, along_curves, draft_angle, draft_type, rigid)
Body copy_body(init_body)
[ Body] tweak_surface_offset(surfaces, distances)
[ Body] tweak_surface_remove(surfaces, extend_ajoining, keep_old, preview)
[ Body] tweak_curve_remove(curves, keep_old, preview)
[ Body] tweak_curve_offset(curves, distances, keep_old, preview)
[ Body] tweak_vertex_fillet(verts, r0, keep_old, preview)
[ Body] subtract(tool_in, from_in, imprint_in, keep_old_in)
[ Body] unite(body_in, keep_old_in)
move(entity, vector, preview)
scale(entity, factor, preview)
reflect(entity, axis, preview)
[ int ] get_volumes_for_node(node_name, node_instance)
int get_mesh_error_count()
962
963
963
963
963
963
963
964
964
964
964
964
965
965
965
966
966
966
967
967
967
967
968
968
968
969
969
969
970
970
970
970
970
306. ___________________________________________________________________ P
yObservable ______________________________________________________________________________ 971
Inheritance
Class Member Functions
Member Function Documentation
notify_observers(event_type)
971
971
972
972
307. ___________________________________________________________________ P
yObserver ________________________________________________________________________________ 973
Class Member Functions
Member Function Documentation
register_observable(observable)
unregister_observable(observable)
notify_observers(observable, event_type)
973
973
973
973
973
308. ___________________________________________________________________ E
ntity _____________________________________________________________________________________ 975
Inheritance
Class Member Functions
Member Function Documentation
destroy_cubit_entity()
[ float ] bounding_box()
xxxvi
975
975
975
975
975
Table of Contents
[ float ] center_point()
int id()
is_visible(visibility_flag)
int is_visible()
is_transparent(transparency_flag)
int is_transparent()
976
976
976
977
977
977
309. ___________________________________________________________________ G
eomEntity ________________________________________________________________________________ 979
Inheritance
Class Member Functions
Member Function Documentation
mesh()
Bool is_meshed()
smooth()
remove_mesh()
str entity_name()
entity_name(name)
[ str ] entity_names()
int num_names()
remove_entity_name(name)
remove_entity_names()
int dimension()
[ Body] bodies()
[ Volume] volumes()
[ Surface] surfaces()
[ Curve] curves()
[ Vertex] vertices()
979
979
979
979
980
980
980
981
981
981
982
982
982
982
983
983
983
984
984
310. ___________________________________________________________________ B
ody ______________________________________________________________________________________ 985
Inheritance
Class Member Functions
Member Function Documentation
[ float ] get_mass_props()
int point_containment(loc_in)
float volume()
Bool is_sheet_body()
985
985
985
985
985
986
986
311. ___________________________________________________________________ S
urface ____________________________________________________________________________________ 987
Inheritance
Class Member Functions
Member Function Documentation
color(value)
int color()
[[Curve]] ordered_loops()
[ float ] normal_at(location)
[ float ] closest_point_trimmed(location)
[ float ] closest_point_trimmed(location)
int point_containment(point_in)
[ float ] principal_curvatures(point)
[ float ] position_from_u_v(u, v)
[ float ] u_v_from_position(location)
[ float ] get_param_range_U()
[ float ] get_param_range_V()
987
987
987
987
988
988
988
989
989
990
990
990
991
991
991
xxxvii
Trelis 15.0 User Documentation
float area()
Bool is_planar()
Bool is_cylindrical()
992
992
992
312. ___________________________________________________________________ C
urve _____________________________________________________________________________________ 995
Inheritance
Class Member Functions
Member Function Documentation
color(value)
int color()
[ float ] tangent(point)
[ float ] curvature(point)
[ float ] closest_point(point)
[ float ] closest_point_trimmed(point)
float length()
[ float ] curve_center()
[ float ] position_from_fraction(fraction_along_curve)
float start_param()
float end_param()
float u_from_position(position)
[ float ] position_from_u(u_value)
float u_from_arc_length(root_param, arc_length)
float fraction_from_arc_length(root_vertex, length)
[ float ] point_from_arc_length(root_param, arc_length)
float length_from_u(parameter1, parameter2)
Bool is_periodic()
995
995
996
996
996
996
997
997
997
998
998
999
999
999
1000
1000
1000
1001
1001
1002
1002
313. ___________________________________________________________________ V
ertex ____________________________________________________________________________________ 1003
Inheritance
Class Member Functions
Member Function Documentation
color(value)
int color()
[ float ] coordinates()
1003
1003
1003
1003
1003
1004
314. ___________________________________________________________________ V
olume ___________________________________________________________________________________ 1005
Inheritance
Class Member Functions
Member Function Documentation
float volume()
color(value)
int color()
[ float ] principal_axes()
[ float ] principal_moments()
[ float ] centroid()
1005
1005
1005
1005
1005
1006
1006
1006
1007
315. ___________________________________________________________________ C
ubitFailureException ______________________________________________________________________ 1009
Class Member Functions
Member Function Documentation
str what()
xxxviii
1009
1009
1009
Table of Contents
316. ___________________________________________________________________ I
nvalidEntityException _____________________________________________________________________ 1011
Class Member Functions
Member Function Documentation
str what()
1011
1011
1011
317. ___________________________________________________________________ I
nvalidInputException ______________________________________________________________________ 1013
Class Member Functions
Member Function Documentation
str what()
1013
1013
1013
318. ___________________________________________________________________ F
ASTQ ___________________________________________________________________________________ 1015
319. ___________________________________________________________________ P
eriodic Space Filling Models (Tile) ___________________________________________________________ 1019
Initial setup
Creating Nodesets
Smoothing
Example
1019
1019
1019
1020
320. ___________________________________________________________________ R
eferences ________________________________________________________________________________ 1021
321. ___________________________________________________________________ C
redits ___________________________________________________________________________________ 1025
322. ___________________________________________________________________ I
ndex ____________________________________________________________________________________ 1027
xxxix
Introduction | Environment | Geometry | Meshing | FE Model | ITEM | Tutorials | Appendix
Trelis15.0 User Documentation
Introduction - A quick overview of some of the main features and goals of the Trelis Mesh Generation Toolkit,
hardware requirements, and where to go for help.
Environment Control - A description of the Trelis user environment, including using the graphical user interface,
session control, command line syntax, journal files, graphics, entity picking, saving and restoring etc..
Geometry - A description of Trelis' geometry features including building geometry from scratch, manipulating
geometry in Trelis, importing and exporting geometry formats, etc...
Mesh Generation - A description of Trelis' mesh generation capabilities, including how to mesh geometry, meshing
and smoothing schemes, setting sizes and intervals, importing a mesh, etc...
Finite Element Model - How to set up the finite element model for analysis, including defining boundary conditions,
material properties, exporting the finite element model, etc.
Immersive Topology Environment for Meshing (ITEM) - A description of Trelis' interactive meshing wizard including
how to use the wizard, and a guide to geometry clean-up, setting up the finite element model, mesh generation in ITEM,
etc.
Appendix
Credits
Quick Reference
1
Key Features
Geometry Creation, Modification, and Healing
Trelis relies on the ACIS solid modeling kernel for geometry representation; there is also mesh-based geometry.
Geometry is imported or created within Trelis. Geometry is created bottom-up or through primitives. Trelis can also read
STEP, IGES, and FASTQ files and convert them to the ACIS kernel.
Once in Trelis, an ACIS model is modified through booleans, or tweaking curves and surfaces. Without changing the
geometric definition of the model, the topology of the model may be changed using virtual geometry. For example, virtual
geometry can be used to composite two surfaces together, erasing the curve dividing them.
Sometimes, an ACIS model is poorly defined. This often happens with translated models. The model can be healed inside
Trelis.
Non-Manifold Topology
Typical assembly meshes require contiguous mesh across multiple parts in an assembly. Trelis accomplishes this by
taking the two touching surfaces of neighboring volumes, and merging them into a single surface. There will be only one
mesh of the surface, and both volume meshes will share that surface mesh. (In contrast, some meshing packages keep
two surfaces, and take steps to ensure their mesh connectivity and positions match.)
These shared surfaces are called non-manifold topology. Geometric models are usually imported into Trelis as manifold
(non-shared) models; then, surfaces which pass a geometric and topological comparison are "merged". A similar
technique is used to merge model edges and vertices across parts. These comparisons are performed automatically, and
can optionally be restricted to subsets of the model (to allow representations of such features as slide lines).
Geometry Decomposition
Solid models often require decomposition to make them amenable to hexahedral meshing. Trelis contains a wide variety
of tools for interactive geometry decomposition, and a capability for performing automatic geometry decomposition is also
under development.
Mesh Generation
Trelis contains a variety of tools for generating meshes in one, two and three dimensions. While the primary focus of
Trelis is on generating unstructured quadrilateral and hexahedral meshes, algorithms are also available for structured
mesh generation and triangle/tetrahedral mesh generation. Several algorithms for generating mixed hex-tet meshes are
also being developed.
Boundary Conditions
Trelis uses different boundary conditions for EXODUS-II format and Non-Exodus formats such as ABAQUS, for importing
and exporting mesh data. EXODUS represents boundary conditions on meshes using Element Blocks, Nodesets, and
Sidesets. Element Blocks are used to group elements by material type. Nodesets are used to group nodes. Other analysis
programs can apply nodal boundary conditions to these sets, such as enforced displacement or nodal temperature
values. Sidesets are used to group sides of elements, such as faces of hexes or edges of quads. Other analysis programs
can apply face-based and edge-based boundary conditions to these sets, for example pressure or heat flux.
Using Element Blocks, Nodesets and Sidesets, a mesh and boundary conditions can be specified in an analysisindependent manner. Typically this specification is combined with an additional data file which designates the specific
type of boundary condition (temperature, displacement, pressure, etc.), along with boundary condition values.
Non-Exodus export formats such as Abaqus support more specific boundary condition sets. These sets may include
displacements, temperatures, forces, heatflux, pressure, or contact pairs.
Element Types
Trelis supports a wide variety of element types, including 1d, 2d, and 3d elements of various orders. Each block has a
unique element type. The element type is specified after the block is created, and after mesh generation (recommended).
Higher order nodes are generated when the element type is specified. Higher order nodes are projected to curved
geometry, depending on the user-settable node constraint flag.
3
Trelis 15.0 User Documentation
Graphics Display Capabilities
Trelis uses the VTK package for its graphics and rendering engine. Trelis can display geometric and mesh entities in
several modes, including hidden line, shaded, transparent or wireframe modes. Trelis supports screen picking of
geometric and mesh entities, as well as mouse-controlled view transformations like rotate, pan, and zoom. VTK takes
advantage of hardware acceleration on most supported platforms. Image files of any displayed image can also be
generated. Trelis can also be run without graphics, to allow execution in batch mode or over slow network connections.
Graphical User Interface
A full graphical user interface (GUI) with the standard look and feel consistent with major platforms is available on all
supported Trelis platforms. The GUI version can improve productivity, making new users aware of the wide range of Trelis
capabilities, and freeing new and experienced users from having to remember esoteric syntax. The GUI and non-GUI
versions create and play back identical journal files, making it easier to switch from one environment to the other.
Command Line Interface
In the command line interface, commands are specified by text rather than mouse clicks. Commands can be entered
interactively or in batch mode by playing back a journal file. The command line interface is available in the GUI through a
window. The non-GUI version supports graphical picking and echoing to the command line, and also mouse-driven view
transformations, but no menus and dialog boxes. The command line and GUI dialog boxes support the APREPRO
preprocessor, which allows parameterization of input. The non-GUI version is available on all platforms, including
Windows.
4
Hardware Requirements
Trelis is available on the following platforms:
•
•
•
Linux glibc 2.5+ 32 and 64 bit (e.g. Redhat 5, 6 Fedora 6, SUSE 11; OpenSUSE 10.2, 11, 12 (10.3 32-bit only);
Debian 5, 6; Ubuntu 8.04, 10.04, 12.04; )
Windows XP/Vista/7, 32 and 64 bit
Mac 10.6+, Intel 64 Bit
The Graphical User Interface version is available on all platforms.
For best results, local displays supporting OpenGL 1.5 is recommended.
5
Trademark Notice
Trelis™ is a trademark of Computational Simulation Software, LLC.
ACIS™ is a proprietary format developed by Spatial Corporation.
GAMBIT™ is a trademark of Ansys, Inc.
Parasolid™ is a trademark of Siemens
SolidWorks™ is a trademark of SolidWorks Dassault Systemes
Pro/Engineer™ is a trademark of PTC
All other trademarks are the property of their respective owners.
7
How to Use This Manual
This manual provides specific information about the commands and features of Trelis. It is divided into chapters, which
roughly follow the process in which a finite element model is created, from geometry creation to mesh generation to
boundary condition application. Examples are provided in the tutorial chapter. Appendices contain advanced topics, alpha
commands, summary of APREPRO functions, FASTQ reference, a troubleshooting guide, and references.
Integrated in Trelis are algorithms and tools, which are in a user-beware state. As they are
further tested (often with the assistance of users) and improved, the tool becomes more
stable and production-worthy. Since documentation of the tool is necessary for actual use,
we have included the documentation of all available tools. However, a "hammer" icon is
placed next to some capabilities as a warning.
Certain portions of this manual contain information that is vital for understanding and
effectively using Trelis. These portions are highlighted with a "key" icon.
9
Introduction
•
•
•
•
•
How to Use this Manual
Key Features
Trelis Support
Hardware Requirements
Trademark Notice
Welcome to Trelis, the automated mesh generation toolkit. Trelis is developed jointly between Sandia National
Laboratories and Computational Simulation Software (www.csimsoft.com.) Sandia and csimsoft, along with other
development partners such as Caterpillar, Inc., develop the underlying toolkit library known as Cubit. csimsoft adds
capability and functionality to that library as well as a fully-functional user interface.
Trelis is a full-featured software toolkit for robust generation of two- and three-dimensional finite element meshes (grids)
and geometry preparation. Its main goal is to reduce the time to generate meshes, particularly large hex meshes of
complicated, interlocking assemblies. It is a solid-modeler based preprocessor that meshes volumes and surfaces for
finite element analysis. Mesh generation algorithms include quadrilateral and triangular paving, 2D and 3D mapping, hex
sweeping and multi-sweeping, tetrahedral meshing, and various special purpose primitives. Trelis contains many
algorithms for controlling and automating much of the meshing process, such as automatic scheme selection, interval
matching, sweep grouping, and also includes state-of-the-art smoothing algorithms
The Trelis environment is designed to provide the user with a powerful toolkit of meshing algorithms that require varying
degrees of input to produce a complete finite element model. Many Trelis users want to experiment with capabilities as
soon as possible. Hence, Trelis releases often contain algorithms which are not quite ready for production use. These
features are listed in the Appendix, and are accessible to the user by specifying a developer flag.
The overall goal of the Trelis project is to reduce the time it takes a person to generate an analysis model. Generating
meshes for complex, solid model-based geometries requires a variety of tools. Many Trelis tools are completely
automatic, while others require user input. Usually, the automatic choices can be over-ridden by the user if necessary.
Most meshing capabilities are integrated into the common Trelis framework; there are also stand-alone tools like Verde.
The user is encouraged to become familiar with all of the available tools, so that he can choose the right one for the job.
11
Trelis Support
Trelis users can get product support and help in several ways, depending on the support package purchased.
1) Email: all users can send requests for help or bug reports to [email protected]
2) Forum: all users can visit our user-supported forum at: http://www.csimsoft.com/forum/
3) The www.csimsoft.com site also includes links to frequently asked questions, training videos, user documentation,
and other aids.
4) Telephone: premium support users may call our offices at 801-717-2296.
13
Starting and Exiting a Trelis Session
The following commands are used to control Trelis execution.
Starting the Session
The command line version of Trelis can be started on UNIX machines by typing "Trelis" at the command prompt from
within the Trelis directory. If you have not yet installed Trelis, instructions for doing so can be found in Licensing,
Distribution and Installation. A Trelis console window will appear which tells the user which Trelis version is being run and
the most recent revision date. A graphics window will also appear unless you are running with the -nographics option.
For a complete list of startup options see the Execution Command Syntax section of this document. Trelis can also be run
with initialization files or in batch mode.
Windows File Association
Windows users have the option to associate .cub, .sat, and .jou files with Trelis. This means that double-clicking on one
of these files will open it automatically in Trelis. This option is available during the installation process
Exiting the Session
The Trelis session can be discontinued with either of the following commands
Exit
Quit
Resetting the Session
A reset of Trelis will clear the Trelis database of the current geometry and mesh model, allowing the user to begin a new
session without exiting Trelis. This is accomplished with the command
Reset [Genesis | Block | Nodeset | Sideset]
A subset of portions of the Trelis database to be reset can be designated using the qualifiers listed. Advanced options
controlled with the Set command are not reset.
You can also reset the number of errors in the current Trelis session, using the command
Reset Errors <value>
which will set the error count to the specified value, or zero if the value is left blank.
Abort Handling
In the event of a crash, Trelis will attempt to save the current mesh as "crashbackup.cub" in the current working directory
just before it exits.
To disable saving of the crashbackup.cub file set an environment variable CUBIT_NO_CRASHSAVE equal to true. Or,
use the following command:
Set Crash Save [On|Off]
This command will turn on or off crashbackup.cub creation during a crash on a per-instance basis. To minimize the effects
of unexpected aborts, use Trelis' automatic journaling feature, and remember to save your model often.
15
Trelis 15.0 User Documentation
16
Execution Command Syntax
To run CUBIT from the command line:
cubit [options and args] [journalFile(s)]
claro [options and args] [journalFile(s)|python historyFile(s)]
Claro is the GUI version of CUBIT, which includes a python interpreter. To run a python script in CUBIT from the
command line, run claro instead of cubit.
Command options for the command line are:
cubit
-help (Print this summary)
-Include <$val> (Specify a journal file)
-input $val (Playback commands in file $val)
-solidmodel <$val> (Read .sat or .cub from file $val)
-fastq <$val> (Read FASTQ file $val)
-initfile <$val> (Read $val as initialization file instead
of $HOME/.cubit)
-batch (Batch Mode - No Interactive Command Input)
-nographics (Do not display graphics windows)
-noinitfile (Do not read .cubit file)
-noecho (Do not echo commands to console)
-nojournal (Do not write journal file)
-nodeletions (Do not allow file deletions)
-journalfile <$val> (Name of journal file, will be overwritten)
-restore [$val] (Name of restore file (default = cubit_geom.save.sat))
-maxjournal [$val] (Maximum number of journal files to write)
-warning [$val] (Warning Messages On/Off)
-information [$val] (Informational Messages On/Off)
-debug <$val> (Set specified flags on, e.g. 1,3,7-9
enables 1,3,7,8,9))
-display <$val> (Specify display to be used for
graphics window)
-driver <$val> (Specify the type of driver to be used for
graphics display)
-nooverwritecheck (Do not perform file export overwrite check)
-variable=<value> (Assign an aprepro variable a value)
Each of these are optional. If specified, the quantities in square brackets, [$val], are optional and the quantities in angle
brackets, <$val>, are required.
Options are summarized in more detail below:
-help
Print a short usage summary of the command syntax to the
terminal and exit.
-initfile <$val>
Use the file specified by <$val> as the initialization file
instead of the default set of initialization files. See
Initialization Files
-noinitfile
Do not read any initialization file. This overrides the default
behavior described in Initialization Files
-solidmodel <$val>
Read the ACIS solid model geometry or .cub file information
from the file specified by <$val> prior to prompting for
interactive input.
-batch
Specify that there will be no interactive input in this
execution of CUBIT. CUBIT will terminate after reading the
17
Trelis 15.0 User Documentation
initialization file, the geometry file, and the input_file_list.
-nographics
Run CUBIT without graphics. This is generally used with the
-batch option or when running CUBIT over a line terminal.
-display
Sets the location where the CUBIT graphics system will be
displayed, analogous to the -display environment variable
for the X Windows system. Unix only.
-driver <type>
Sets the <type> of graphics display driver to be used.
Available drivers depend on platform, hardware, and system
installation. Typical drivers include X11 and OpenGL.
-nojournal
Do not create a journal file for this execution of CUBIT. This
option performs the same function as the Journal Off
command. The default behavior is to create a new journal
file for every execution of CUBIT.
-journalfile <file>
Write the journal entries to <file>. The file will be overwritten
if it already exists.
-maxjournal <$val>
Only create a maximum of <$val> default journal files.
Default journal files are of the form cubit#.jou where # is a
number in the range 01 to 999.
-nodeletions
Turn off the ability to delete files with the delete file
'<filename>' command.
-nooverwritecheck
Turn off the file overwrite check flag. Files that are written
may then overwrite (erase) old files with the same name
with no warning. This is typically useful when re-running
journal files, in order to overwrite existing output files. See
the set File Overwrite Check [ON|off] command.
-restore
Restore the specified filename (or "cubit_geom") mesh and
ACIS files, e.g. cubit_geom.save.g and
cubit_geom.save.sat.
-noecho
Do not echo commands to the console. This option performs
the same function as the Echo Off command. The default
behavior is to echo commands to the console.
-debug=<$val>
Set to "on" the debug message flags indicated by <$val>,
where <$val> is a comma-separated list of integers or
ranges of integers, e.g. 1,3,8-10.
-information={on|off}
Turn {on|off} the printing of information messages from
CUBIT to the console.
-warning={on|off}
Turn {on|off} the printing of warning messages from CUBIT
to the console.
-Include=<path>
Allows the user to specify a journal file from the command
line.
-fastq=<file>
Read the mesh and geometry definition data in the FASTQ
file <file> and interpret the data as FASTQ commands. See
T. D. Blacker, FASTQ Users Manual Version 1.2, SAND88-
18
Execution Command Syntax
1326, Sandia National Laboratories, (1988). for a
description of the FASTQ file format.
<input_file_list>
Input files to be read and executed by CUBIT. Files are
processed in the order listed, and afterwards interactive
command input can be entered (unless the -batch option is
used.)
<variable=value>
APREPRO variable-value pairs to be used in the CUBIT
session. Values can be either doubles or character type
(character values must be surrounded by double quotes.),
Command options can also be specified using the
CUBIT_OPT environment variable. (See Environment
Variables .)
Passing Variables into a CUBIT Session
To pass an aprepro variable into a CUBIT Session, start cubit with the variable defined in quotes i.e. cubit
"some_var=2.3"
19
Initialization Files
Trelis can execute commands on startup, before interactive command input, through initialization files. This is useful if the
user frequently uses the same settings.
On Unix or Windows, the following files are played back in order, if they exist, at startup:
<$TRELIS_DIR/.Trelis.install
$HOMEDRIVE$HOMEPATH/.Trelis
$HOME/.Trelis
$(current working directory)/.Trelis
Where $(current working directory) is determined by the program itself and words starting with '$' are environment
variables.
If the -initfile <filename> option is used on the command that starts Trelis, then the other init files are skipped and only
the specified filename is played back.
The $TRELIS_DIR file is installation specific. The $HOME file is user specific. The $PWD file is run-specific, read when
starting up Trelis from a particular meshing problem's subdirectory.
These files are typically used to perform initialization commands that do not change from one execution to the next, such
as turning off journal file output, specifying default mouse buttons, setting geometric and mesh entity colors, and setting
the size of the graphics window.
21
Environment Variables
Trelis can interpret the following environment variables. These settings are only applicable to the Command Line Version
of Trelis and do not apply to the Graphical User Interface. See also the CUBIT_STEP_PATH and CUBIT_IGES_PATH
environment variables. See also the CUBIT_DIR, HOMEDRIVE and HOMEPATH settings.
DISPLAY
The graphics window or GUI will pop-up on the specified X-Window display. This
is useful for running Trelis across a network, or on a machine with more than one
monitor. Unix only.
CUBIT_OPT
Execution command line parameter options. Any option that is valid from the
command line may be used in this environment variable. See Execution
Command Syntax.
CUBIT_Journal
Specifies path and name to use for journal file. The specified path may contain
the following %-escape sequences:
%a - abbreviated weekday name
%A - full weekday name
%b - abbreviated month name
%B - full month name
%d - date of the month [01,31]
%H - hour (24-hour clock) [00,23]
%I - hour (12-hour clock) [01,12]
%j - day of the year [1,366]
%m - month number [1,12]
%M - minute [00,59]
%n - replaced with the next available number between 01 and 999.
%p - "a.m." or "p.m."
%S - seconds [00,61]
%u - weekday [1,7], 1 is Monday
%U - week of year [00,53]
%w - weekday [0,6], 0 is Sunday
%y - year without century [00,99]
%Y - year with century (e.g. 1999)
%% - a '%' character
The default value is "Trelis%n.jou". This creates journal files in the current
directory named "cubit00.jou", "cubit01.jou", "cubit02.jou", etc. To keep the same
naming scheme but create the files the /tmp directory, set CUBIT_JOURNAL to
"/tmp/Trelis%n.jou"
To create journal files in directories according to the day of the week, first create
directories named "Mon", "Tues", etc. Trelis will not create them for you. Next set
CUBIT_JOURNAL to
"%a/%n.jou". This will create journal files named "01.jou" through "999.jou" in the
appropriate directory for the current day of the week.
23
Trelis 15.0 User Documentation
24
Command Syntax
The execution of Trelis is controlled either by entering commands from the command line or by reading them in from a
journal file. Throughout this document, each function or process will have a description of the corresponding Trelis
command; in this section, general conventions for command syntax will be described. The user can obtain a quick guide
to proper command format by issuing the
<keyword> help
command; see Command Line Help for details.
Trelis commands are described in this manual and in the help output using the following conventions. An example of a
typical Trelis command is:
Volume <range> Scheme Sweep [Source [Surface] <range>] [Target [Surface] <range>] [Rotate {on |
OFF}]
The commands recognized by Trelis are free-format and abide by the following syntax conventions.
1.
2.
3.
4.
Case is not significant.
The "#" character in any command line begins a comment. The "#" and any characters following it on the same
line are ignored. Although note that the "#" character can also be used to start an Aprepro statement. See the
Aprepro documentation for more information.
Commands may be abbreviated as long as enough characters are used to distinguish it from other commands.
The meaning and type of command parameters depend on the keyword. Some parameters used in Trelis
commands are:
Numeric: A numeric parameter may be a real number or an integer. A real number may be in any legal C or
FORTRAN numeric format (for example, 1, 0.2, -1e-2). An integer parameter may be in any legal decimal
integer format (for example, 1, 100, 1000, but not 1.5, 1.0, 0x1F).
String: A string parameter is a literal character string contained within single or double quotes. For example,
'This is a string' .
Filename: When a command requires a filename, the filename must be enclosed in single or double quotes. If
no path is specified, the file is understood to be in the current working directory. After entering a portion of a
filename, typing a '?' will complete the filename, or as much of the filename as possible if there is more than one
possible match.
A filename parameter must specify a legal filename on the system on which Trelis is running. The filename may
be specified using either a relative path (../Trelis/mesh.jou), a fully-qualified path
(/home/jdoe/Trelis/mesh.jou), or no path; in the latter case, the file must be in the working directory (See
Environment Commands for details.) Environment variables and aliases may also be used in the filename
specification; for example, the C-Shell shorthand of referring to a file relative to the user's login directory
(~jdoe/Trelis/mesh.jou) is valid.
Toggle: Some commands require a "toggle" keyword to enable or disable a setting or option. Valid toggle
keywords are "on", "yes", and "true" to enable the option; and "off", "no", and "false" to disable the option.
5.
Each command typically has either:
* an action keyword or "verb" followed by a variable number of parameters. For example:
Mesh Volume 1
Here Mesh is the verb and Volume 1 is the parameter.
* or a selector keyword or "noun" followed by a name and value of an attribute of the entity indicated. For
example:
Volume 1 Scheme Sweep Source 1 Target 2
25
Trelis 15.0 User Documentation
Here Volume 1 is the noun, Scheme is the attribute, and the remaining data are parameters to the Scheme
keyword.
The notation conventions used in the command descriptions in this document are:
•
•
•
•
•
•
•
26
The command will be shown in a format that looks like this:
A word enclosed in angle brackets ( <parameter> ) signifies a user-specified parameter. The value can be an
integer, a range of integers, a real number, a string, or a string denoting a filename or toggle. The valid value
types should be evident from the command or the command description.
A series of words delimited by a vertical bar ( choice1 | choice2 | choice3 ) signifies a choice between the
parameters listed.
A toggle parameter listed in ALL CAPS signifies the default setting.
A word that is not enclosed in any brackets, or is enclosed in curly brackets ( {required} ) signifies required
input.
A word enclosed in square brackets ( [optional] ) signifies optional input which can be entered to modify the
default behavior of the command.
A curly bracket that is inside a square bracket (e.g. [Rotate {on|OFF}] ) is only required if that optional modifier
is used.
Command Line Help
In addition to the documentation you are currently viewing, Trelis can give help on command syntax from the command
line. For help on a particular command or keyword, the user can simply type help <keyword> . In addition, if the user has
typed part of a command and is uncertain of the syntax of the remainder of the command, they can type a question mark
? and help will be printed for the sequence of keywords currently entered. It is important to note that if the user has typed
the keywords out of order, then no help will be found. If the user is not sure of the correct order of the keywords, the
ampersand & key will search on all occurrences of whatever keywords are entered, regardless of the order. The results of
this type of command are shown in the following listing.
Trelis> volume 3 label ?
Completing commands starting with: volume, label.
Help not found for the specified word order.
Trelis> volume 3 label &
Help for words: volume & label
Label Volume [ on | off | name [only|id] | id | interval | size | scheme | merge | firmness ]
Trelis> label volume 3 ?
Completing commands starting with: label, volume.
Label Volume [on|off|name [only|ids]|ids|interval|size|scheme|merge|firmness]
27
Environment Commands
•
•
•
•
•
•
•
•
•
Working Directory
File Manipulation
CPU Time
Comment
History
Error Logging
Determining the Trelis Version
Echoing Commands
Digits Displayed
Working Directory
The working directory is the current directory where journal files are saved. To list the current directory type
pwd
The current path will be echoed to the screen. By default, the current directory is the directory from which Trelis was
launched. The command to change the current directory is
cd "<new_path>"
The new path may be an absolute reference, or relative to the current directory. The <TAB> key will complete unique file
references.
File Manipulation
A helpful addition is the ability to do a directory listing of a directory. The command for this is
ls ['<file_name>']
or
dir ['<file_name>']
Note also that you can delete files from the command line. The command for this is
Delete File ['<file_name>']
The file name may include the wildcard character *, but not the wildcard character ?, since the ? is used for command
completion. File deletion from the command line can also be disabled. If deletions are set to off files cannot be deleted
from the Trelis command line.
Set Deletions [ON|Off]
The mkdir command is used to create a new directory. The syntax for this command is:
Mkdir "<directory_name>"
29
Trelis 15.0 User Documentation
This creates a new directory with the specified name and path. The command accepts an absolute path, a relative path,
or no path. If a relative path is specified, it is relative to the current working directory, which can be seen by typing 'pwd' at
the Trelis command prompt. If no path is specified, the new directory is created in the current working directory.
The command succeeds if the specified directory was successfully created, or if the specified directory already exists. The
command fails if the new directory's immediate parent directory does not exist or is not a directory.
CPU Time
At times it is important to see how much cpu time is being used by a command. One function available to do this is the
timer command. The syntax for this command is:
Timer [Start|Stop]
The start option will start a CPU timer that will continue until the stop command is issued. The elapsed time will be printed
out on the command line. If no arguments are given, the command will act like a toggle.
Comment
This keyword allows you to add comments without affecting the behavior of Trelis.
Comment ['<text_to_print>'] [<aprepro_var>] [<numeric_value>]
The comment command can take multiple arguments. If an argument is an unquoted word, it is treated as an aprepro
variable and its value is printed out. Quoted strings are printed verbatim, and numbers are printed as they would be in a
journal string. For example:
Trelis> #{x=5}
Trelis> #{s="my string"}
Trelis> comment "x is" x "and s is" s
User Comment: x is 5 and s is my string
Journaled Command: comment "x is" x "and s is" s
History
This command allows you to display a listing of your previous commands.
History <number_of_lines>
For example, if you type history 10, the most recent 10 commands will be echoed to the input window.
Error Logging
[set] Logging Errors {Off | On File '<filename>'[Resume]}
This setting will allow users to echo error messages to a separate log file. The resume option will allow output to be
appended to existing files instead of overwriting them. For more information on Trelis environment settings see List Trelis
Environment.
30
Environment Commands
Determining the Trelis Version
To determine information on version numbers, enter the command
Version
. This command reports the Trelis version
number, the date and time the executable was compiled, and the version numbers of the ACIS solid modeler and the VTK
library linked into the executable. This information is useful when discussing available capabilities or software problems
with Trelis developers.
Echoing Commands
By default, commands entered by the user will be echoed to the terminal. The echo of commands is controlled with the
command:
[Set] Echo {On | Off}
Digits Displayed
Trelis uses all available precision internally, but by default will only print out a certain number of digits in order for columns
to line up nicely. The user can override that with the "set digits" command:
Set Digits [<num_to_list=-1>]
If the digits are set to -1, then the default number of digits for pretty formatting are used. If the digits are set to a specific
number, such as 15, more digits of accuracy can be displayed. This may be useful when checking the exact position and
size of geometric features.
The number of digits used for listing positions, vectors and lengths can be listed using the following command:
List Digits
Examples:
Trelis> set digits 6
Coordinates and lengths will be listed with up to 6 digits.
Trelis> set digits 20
For this platform, max digits = 15. Coordinates and lengths will be listed with up to 15 digits.
Trelis> set digits -1
To reset digits to default, use 'set digits -1'
The number of coordinate and length digits listed will vary depending on the context.
31
Saving and Restoring a Trelis Session
There are currently two ways to save/restore a model in Trelis. A file can be saved with either the Exodus or Cubit File
method. The method of choice is determined by a set command. The Trelis method is the default.
Set Save [exodus|cubit] [Backups <number>]
Cubit File Method
•
•
•
•
•
New
Open
Save
Import
Export
The Cubit file is a binary cross-platform compatible file for the storage of a Trelis model that is compact in size and
efficient to access. It includes both the geometry and the associated mesh, groups, blocks, sidesets, and nodesets. Mesh
and geometry are restored from the Trelis file in exactly the same state as when saved. For example, element faces and
edges are persistent, as well as mesh and geometry ids. The Graphical User Interface version of Trelis also provides a
toolbar with direct access to file operations using the Trelis File method described here.
New
Creates a new blank model with default name, closing the current model. The New command
essentially acts like the reset command.
Open '<filename>'
Opens an existing *.cub file, closing the current model.
Save
A default file name is assigned when Trelis is started (in very much the same way the journal files are
assigned on startup) in the form cubit01.cub, for example. The current model filename is displayed on
the title bar of the Trelis window. Typing save at any time during your session will save the current
model to the assigned *.cub file. The *.cub file includes the *.sat file and the mesh. Groups, blocks,
sidesets and nodesets are also saved within the *.cub file. To change the name of the current model,
or to save the model's current geometry to a different file, use the save as command. Note that 'save
<file.cub>' is NOT a valid command.
Save
Save As 'filename.cub' [Overwrite]
The set file overwrite command can be toggled on and off to allow overwriting when using the save as
command. The command is defaulted to not allow overwriting.
Set File Overwrite [On|OFF]
A backup file is created by default, allowing access to previous states of the model. The backup files
are named *.cub.1, *.cub.2... The user can set the total number of backups created per model with
the following command (the default number of backups is 99,999):
Set Save Backups <number>
33
Trelis 15.0 User Documentation
As soon as the number of model backups reaches the maximum, the lowest numbered backup file
will be removed upon subsequent backup creation.
To check on the status of a 'set' command, type in the command in question without any options. For
example, to check which save method is currently toggled, type:
Set Save
Import
Appends a *.cub file to an existing model.
Import Cubit 'filename.cub' [merge_globally]
Export
In addition to saving an entire model, one can use the export command to save only a portion of a
model. The geometry and associated mesh, groups, blocks, sidesets and nodesets are exported.
Only bodies or free surfaces, curves or vertices can be exported to a Trelis file.
Export Cubit 'filename.cub' entity-list
34
Trelis Application Window
The default Trelis Application Window is shown in the following image.
Figure 1. The Trelis Application Window
Graphics Window- The current model will be displayed here. Graphical picking and view transformations are done here.
Power Tools - Geometry tree hierarchy view, geometry analysis and repair tool, meshing tool, meshing quality tool, and
ITEM Wizard.
Property Page - The Property Page lists attributes of the current entity selection. Some of these properties can be edited
from the window.
Command Panel - Most Trelis commands are available through the command panels. The panels are arranged
topologically, by mode.
Command Line Workspace - The command line workspace contains both the Trelis command and error windows. The
command window is used to enter Trelis commands and view the output. The error window is used to view Trelis errors.
Drop Down Menus - Standard file operations, Trelis setup and defaults, display modes, and other functionality is
available in the pull-down menus.
Toolbars - The most commonly used features are available by clicking toolbar icons.
Context Sensitive Help in the GUI
The Graphical User Interface has a context-sensitive help system. To obtain help using a specific window or control panel,
press F1 when the focus is in the desired window. It may be necessary to click inside a text box to switch focus to a
particular window. If no context specific help is available, it will open the Trelis help documentation where you can search
for a particular topic.
35
Trelis 15.0 User Documentation
Customizing the Application Window
All windows in the Trelis Application can be Floated or Docked. In the default configuration, all windows are docked. When
a window is docked the user can click on the area indicated below.
Figure 2. A docked window. Click and drag to float.
By dragging with the left mouse button held down, the window will be un-docked from the Application Window. Dragging
the window to another location on the Application Window and releasing the mouse button will cause it to dock again in a
new location. The bounding box of the window will automatically change to fit the dimensions of the window as it is
dragged. Releasing the mouse button while the window is not near an edge will cause the window to Float. To stop the
window from automatically docking, hold the CONTROL key down while dragging.
36
CUBIT Application Window
Figure 3. A Floating Window
When a window is floating, as shown in Figure 3, it is possible to dock it by clicking the title bar of the window and
dragging it to its new docked location.
Note: Double clicking on the title bar of an floating window will cause the window to redock in its last docked position.
37
Command Panel Functionality
The Command Panel is arranged first by mode on the top row of buttons. Modes are arranged by task. All of the geometry
related tasks, for instance, can be found under the Geometry mode. When a mode is selected, a second row of buttons
becomes available. The second row of buttons shown depends on the selected mode. For example, if Geometry,
Meshing, or Materials and BCs is selected, the second button row will show entity types. Entities are those specific to the
mode.
•
•
•
Geometry panel entity level buttons include Volumes, Surfaces, Curves, Vertices, and Groups.
Meshing panel entity level buttons include Volumes, Surfaces, Curves, Vertices, Groups, Hexes, Tets, Quads,
Tris, Bars, and Nodes.
Materials and BCs entity level buttons include Exodus Nodesets, Exodus Sidesets, Exodus Blocks, Create
Boundary Conditions, Modify Boundary Conditions, List Boundary Conditions, Draw Boundary Conditions, Make
a Boundary Condition current, and Delete Boundary Conditions.
The second row of buttons for Analysis Setup and Post Processing are not arranged by entity. Rather, the buttons show
specific capabilities.
The third row of buttons contains Actions, such as Create, Delete, Modify, and so forth. The following shows an example
of Geometry/Volume actions.
Selecting an Action will display a command panel. The Geometry/Volume/Create command panel is shown below.
39
Trelis 15.0 User Documentation
All command panels are constructed similarly. Each abstracts a set of Trelis commands. Options are selected using
checkboxes, radio buttons, combo boxes, edit fields, and other standard GUI widgets. Each command panel includes an
Apply button. Pressing the Apply button will generate a command to Trelis. Nothing happens until and unless the Apply
button is pressed.
Note: The edit fields are free form, which means the user may enter any valid string into the
fields. Any string that is valid for the command line is valid for the command panel edit fields.
Where possible, default values are placed into edit fields. At any time, with the cursor placed over a blank portion of the
command panel, the user may right-click to select Reset Data which will clear all fields and replace default values.
ID Input Entry Methods
The ID Input Fields provide a location where Geometric IDs, required for the current command, can be entered. IDs can
be entered in several ways:
Simple Keyboard entry
ID numbers can be entered directly in the field. Each ID must be separated with a space. Select the field first before
typing.
Graphical selection
40
Command Panel Functionality
IDs can be entered automatically by selecting entities directly in the Graphics Window. The current entity available for
selection is based on the current entity selection mode. In some cases, not all entities of the current entity selection mode
will be available for picking. The program may automatically filter the applicable entities based on the context of the
current command
Geometry Tree selection
IDs may be entered by selecting the corresponding geometric entity from the geometry tree. To select multiple entities use
the <ctrl> key.
Ranges
A range of IDs may be typed into the field. For example:
1 to 5
will automatically enter all IDs from 1 to 5 inclusive in the field. Keywords such as all and except can also be used. Any
range that can be entered directly on a Trelis command line can also be used in the ID input field. See Command Line
Entity Specification for a description of the syntax.
As Part of Other Entities
Syntax can be entered in the ID Input field that will specify an entity based upon its topological relationship to other
entities For example, if a Vertex Selection Type Button was highlighted, entering
in surf 1
will automatically enter all vertices in surface 1 into the Input Field. Trelis has a rich set of syntax rules for specifying
entities based upon topology relationships. See Command Line Entity Specification for a description.
In Groups
Entities that are part of groups may be specified in the ID Input Field. For example, if the Vertex Selection Type Button is
highlighted, entering:
in picked
will automatically enter all vertices in the picked group into the active ID Input Field.
Dragged and Dropped
Entities can be dragged and dropped into the ID Input Field from the Tree View window.
Right-Click Context Menu for ID Input Fields
When the right mouse button is selected while in an ID Input Field, the following menu options will appear:
•
•
•
•
•
•
•
•
•
•
•
•
Done Selecting - Enters current selection and removes cursor from selection window
Select Other - Displays selection dialog
Select All - Selects all available entities and puts "select all" in input window
Highlight - Highlight the current selection
Zoom To - Zooms to current entity in the selection field within the graphics window
Rotate About - Change center of rotation to the center of selected entity
Draw - Draws the entities listed in the input field within the graphics window
Isolate - Turns visibility off for all entities other than the selected entities. Similar to draw command, but
entities remain hidden with a graphics refresh. Select All Visible in the graphics window to turn visibility back
on.
Visibility Off - Removes the current entity from the input window and hides it on the graphics screen
Mesh - Mesh the listed entities using either an assigned scheme or a default scheme where none is assigned
Delete Mesh - Deletes mesh on all entities listed in the input window
Reset Entity - rehighlights the entities listed in the input field within the graphics window
41
Trelis 15.0 User Documentation
•
•
List Info - Displays a sub menu of choices including basic, geometry, and mesh. Selecting the basic option will
list schemes, visibility, and interval assignments. The geometry option will add information about the geometry
and geometry engine. The mesh option will list information about mesh entities.
Delete - Deletes the current geometric object in the input window.
Value Fields
Integer and real values pertinent to the command are entered in this window. Input placed in parenthesis { } will be
evaluated when the command is executed. For example:
{10*0.02}
is valid input. Additionally, any APREPRO syntax is valid in the Value Field, including mathematical functions and boolean
operations. See the section, APREPRO for a description of syntax.
Advancing Pickwidgets
Some command panels have several id input fields such as the Mesh>Hex>Create panel. A convenience feature
implemented for such panels is an advancing pickwidget feature. Pressing the middle mouse button after selecting an
entity will advance to the next id input field.
42
View Navigation in the GUI
There are two different default paradigms for view navigation: Trelis command line and Trelis GUI. The user is allowed to
customize the mouse settings as desired. Mouse settings in the GUI are modified by accessing the Tools pull-down
menu, then select Options. The Mouse Settings dialog is shown below (See Mouse-Based Navigation for the command
line version).
Figure 1. Mouse Settings Dialog
Rotations
Where the cursor is in the graphics window will dictate how the view will be rotated. If the cursor is outside of an imaginary
circle, shown in Figure 2, the view will be rotated in 2d, around an axis normal to the screen. If it is inside the circle, as in
Figure 3, the rotations will be in 3d, about the current view spin center. The spin center can be changed to any x-y-z
location. The most common way is by zooming to an entity, which changes the spin center to the centroid of that entity.
The "view at" command will change the spin center without zooming:
View at vertex 3
43
Trelis 15.0 User Documentation
Figure 2. With the mouse pointer outside the circle the view is rotated about an axis normal to the screen
Figure 3. With the mouse pointer inside the circle the view is rotated about the current spin center
Zooming
To zoom, press the appropriate buttons or keys and move the cursor vertically, as shown in Figure 4. The wheel on a
wheel mouse will also zoom.
44
View Navigation in the GUI
Figure 4. Move the mouse pointer vertically to zoom in and out
Panning
To pan, press the appropriate buttons or keys and move the cursor horizontally or vertically, as shown in Figure 5.
Figure 5. Move the mouse pointer horizontally or vertically to pan the view
45
Selecting Entities in the GUI
Geometry, mesh entities, and boundary conditions can be selected with the left mouse button directly in the graphics
window. Before selecting any entity, however, the correct selection mode must be chosen. This dictates which entity types
will be available for selection in the graphics window. The Select Toolbars, which are located above the graphics window
by default, are used to change the entity selection modes.
Figure 1. The Selection Toolbar for Geometry and Mesh Entities
Figure 2. The Selection Toolbar for Boundary Conditions
Figures 1 and 2 shows the selection toolbars. Selecting one of the entity selection modes will only permit selection of that
particular entity type within the graphics window. These selections will not override a Pick Widget in the command panel.
If both volume and surface entities are picked on the select toolbar, a single click will select the surface while a double
click will select the volume. More detailed information on selecting and specifying entities can be found in Entity Selection
and Filtering .
Pre-Selection
When the mouse cursor is over an entity type that has been selected from the Pick toolbar, that entity will become
highlighted. This is called pre-selection and is used as a graphical guide to show which entity will be picked when the
mouse button is clicked.
Graphics pre-selection may slow down your graphics speed for large models. You can disable pre-selection from the
Tools->Options dialog box.
47
Trelis 15.0 User Documentation
Polygon and Box Select
The polygon/box selection feature allows you to select entities by drawing a box or polygon on the screen. To draw box on
the screen press and hold the <CTRL> button* while clicking and dragging the left mouse button. Release the left mouse
to complete the box select. To create a polygon selection, press and hold the <CTRL>* button while clicking and dragging
the left mouse button. Click the left mouse button to create another side for the polygon. Press either of the other buttons
to close the polygon and complete the selection. Only entities that are in active selection mode will be selected. To
change between the polygon or box method, press the Toggle Between Polygon/Box Select button on the Select Toolbar.
Clicking the Toggle Selected Enclosed/Extended button will toggle between Enclosed Selection and Extended Selection.
Enclosed selection will only select entities that are fully enclosed within the bounding box or polygon. Extended selection
will select entities that are either fully OR partially enclosed within the bounding box. Toggling the the Select X-Ray will
select entities that are hidden behind other entities. X-ray selection will only apply to smoothshade and hiddenline
graphics modes.
*Note: For Mac computers use the command (or apple) button for polygon or box select.
48
Key Press Commands for the GUI
Several commands have a key press shortcut. These commands will be executed with respect to the currently selected
entities; see the following table:
Shortcut
Key
Command
l
List information about the current entity to the output window.
i
Toggle the visibility of the selected entity (make invisible or visible).
e
Echo entity id to command line.
Select the next entity.
Select the previous entity.
0
Toggle picking of vertices.
1
Toggle picking of curves.
2
Toggle picking of surfaces.
3
Toggle picking of volumes.
4
Toggle picking of groups.
0
Toggle picking of mesh nodes
1
Toggle picking of mesh edges.
2
Toggle picking of mesh faces.
3
Toggle picking of mesh hexes.
F5
Refresh graphics window
S
Activate/inactivate graphics clipping plane
49
Right Click Commands for the GUI Graphics
Window
Clicking the Right mouse button in the graphics window will bring up a menu. One of two menus will appear, depending
on whether an entity is currently selected.
With Entity Selected
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
Select Other- Brings up a dialog with alternate entity selections
Zoom To - Zoom to the selected entity
Rotate About - Changes the center of rotation to the centroid of this entity
Draw - Draw the selected entity
Isolate - Turn all but the selected entities invisible
Add to BC/Group/Part - Opens a dialog box where you can add the selected entity to an existing boundary
condition, group, or part.
Remove from BC/Group/Part - Opens a dialog box where you can remove the selected entity from an existing
boundary condition, group, or part.
Add to Picked Group - Add this entity to the picked group.
Remove from Picked Group - Remove this entity from the picked group
Visibility Off - Turn selected entities invisible
Mesh - Mesh the selected entities
Measure - Measures between two entities, or two vertices on a curve.
Delete Mesh - Delete the mesh on selected entities (but not interval or scheme information)
Reset Entity - Reset selected entities by deleting mesh and interval information
List Info - Show the menu of additional list commands
Delete - Delete selected entities
Without Entity Selected
•
•
•
•
Reset Zoom - Reset zoom to original configuration
Refresh- Refresh the graphics display
All Visible - Make all entities visible
Display Options - Opens Options Menu to display options
51
Viewing Curve Valence
To view your model based on a color-coded curve valence scale, click on the curve valence button on the Display
Toolbar. Curve valence refers to the number of surfaces attached to each curve. Curves with exactly two surfaces
attached are shown in blue. Curves with exactly one surface are shown in red. Curves with more than two attached
surfaces are shown in white.
This tool is useful for quickly visualizing merged/unmerged topology. Merged curves will usually have a valence > 2, while
unmerged curves typically have a valence of 2. Curves with a valence of 1 may indicate a floating surface.
53
Geometry Tree
The geometry tree provides a complete graphical hierarchical representation of the parent child relationship of all
geometric entities. The tree is populated as the model is constructed by Trelis. In addition to showing a hierarchy of
geometric entities, the tree also shows Assembly Data, active Groups, and active Boundary Condition entities.
The tree works directly with the graphics window and picking. Selecting an entity in the tree will select the same entity in
the graphics window. Selecting an entity in the graphics window will highlight the tree entry if that entry is currently visible.
If an entity's visibility is turned off, the icon next to that entity in the geometry tree will disappear.
If the tree entry is not visible the user may press the Find button located at the bottom of the tree. The first occurrence of
the selected entity will be shown on the tree.
Virtual entities have a small (v) after the name to indicate that they are virtual entities.
55
Trelis 15.0 User Documentation
Figure 1. Geometry Tree Window
56
Geometry Tree
Drag and Drop
The Tree View window supports drag and drop of geometric entities into existing boundary condition sets. To create
boundary conditions, see the Materials and Properties menu on the main control panel, or right-click on one of the
boundary condition labels and select the "Create New" option from the context menu. Geometric entities or groups can be
added to blocks, nodesets, or sidesets by dragging and dropping inside the tree view window. Assembly data may also be
organized in the geometry tree window through drag and drop.
Picked Group
The current selections in the graphics window can be added to a "picked group" by selecting the "Add to Picked Group"
from the Right click menu. Selections can also be added to the picked group by dragging and dropping onto the group
from the geometry tree window. The picked group can be substituted into any commands that use groups. To remove an
item from the picked group, use the "Remove from Group" option in the right click menu in the geometry tree or from the
graphics window.
Figure 2. Picked Group
Right-Click Menu Functions
The geometry tree's context menu is sensitive to the type of item and the number of items selected. Functions that
apply to the item type and number of selected items are available from the context menu. These include the
following:
•
•
•
•
•
•
•
•
•
Zoom To - Available for all geometric entities
Rotate About - Change the center of rotation to the centroid of the entity without zooming
Fly-In - Animated zoom feature
Locate - Labels the selected entity in the graphics window
Draw - Draw this entity by itself.
Isolate - Similar to Draw command, but the display will not be refreshed with a graphics reset. To redisplay the
model, select All Visible from the graphics window right-click menu.
Transparency On/Off - Toggles transparency mode
Visibility On/Off - Toggles visibility
Rename - Allows you to rename entities from the tree. Clicking on a highlighted entity in the tree will do the
same thing. This will also work for boundary condition entities (blocks, nodesets and sidesets)
57
Trelis 15.0 User Documentation
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
58
Mesh - Mesh selected entity at current settings.
Delete Mesh - Available for meshed entities
Reset Entity - Deletes mesh, and returns all settings to default values.
Delete - Available when Volumes and Groups are selected.
Create New Assembly/Sub-assembly/Part - You must specify the absolute path to create a new assembly,
sub-assembly or part (e.g. /a1/p1). It may also be necessary to refresh the full tree before viewing changes.
Add Selected to Part- Add the selected volume in the graphics window to the selected part on the geometry
tree.
Remove from Metadata - Deletes the selected part or assembly metadata information. An assembly must be
empty to remove it
View Metadata - List metadata in the command line workspace
Rename Metadata - Allows you to rename a part or assembly
Clean Metadata - Removes all parts and assemblies that are not associated with any geometric entities.
List Volumes Without Parts - Lists all volumes that are not associated with a part in the output window
Show Part Name/Description -Toggles the display of the part name/description in the tree.
Goto Part - Finds the associated metadata part when a volume is selected.
Measure - Available when two entities are selected or 1 curve is selected
Refresh Full Tree - Used to return to main tree
Collapse Tree - Available when entities are selected.
View Descendants/Ancestors - Show this entity's individual hierarchy. Use the Refresh Full Tree option to
return to main tree view.
View Neighbors View adjacent entities. Use the Refresh Full Tree option to return to the main tree view.
Create New Volume - Available when the user right-clicks over the Volumes (parent) label. Opens the
geometry-volume-create panel
Import Geometry - Available when the user right-clicks over the Volumes (parent) label. Opens import dialog.
Create New Group - Available when the user right-clicks over the Groups (parent) label.
Clean Out Group - Available when groups are selected. Removes all entities from group.
Remove from Group - Available when groups are selected. Removes selected entity from the group.
Add Selected to Block/Nodeset/Sideset - Add the selected entity in the graphics window to the chosen block,
nodeset, or sideset in the geometry tree.
Delete Selected from Block/Nodeset/Sideset - Delete the selected entity in the graphics window from the
chosen block, nodeset, or sideset in the geometry tree.
Create New Block/Sideset/Nodeset - Available when the user right-clicks over the respective Boundary
Conditions (parent) label.
Create New <boundary condition> - Available when highlighting desired boundary condition in the tree
including CFD and FEA boundary conditions.
Draw Block/Sideset/Nodeset - Draws the selected block/nodeset/sideset on top of existing entities
Draw Sideset/Nodeset Only - Draws the selected nodeset/sideset independent of other entities
Delete Selected Boundary Condition - Deletes any selected boundary conditions
Draw Selected Boundary Condition - Draws selected boundary condition by itself
Draw Selected Boundary Condition (Add) - Draws multiple boundary conditions
List Selected Boundary Condition - Lists information about selected boundary conditions in the command line
window
Remove from Block/Sideset/Nodeset - Removes selected entity from the specified block, sideset or nodeset
Cleanup (Tets) - Issues cleanup command for selected block. Only applicable for blocks composed of tet
elements
Remesh (Tets) - Issues remesh command for selected block. Only applicable for blocks composed of tet
elements
List Info - List information about selected entity in the output window.
Geometry Power Tools
The geometry power tools are located on the Tree View window under the blue geometry tab. In many cases, a model will
fail to mesh because of problems with the geometry. Since the range of geometry problems is so wide, and because
these problems can be hard to diagnose, the Geometry Power Tool has several built-in tools designed to analyze and
repair these problems. The Geometry Repair Tool analyzes geometry for small angles, overlap, small features, bad
geometry definition, blend surfaces, close loops, or mergeable entities that may affect meshing capability. It also contains
a powerful toolkit of geometry modification methods to fix these problems. All of the common geometry clean-up tools are
now in one place on the GUI menu. In addition, there is a window that lists results from geometry analysis in a tree format,
making it easier to find, diagnose, and solve geometry problems. And Trelis will save your settings, so you can run the
same diagnostic tests each time you use the geometry power tools.
Figure 1. Geometry Power Tools
Geometry Analysis Tools
The geometry power tools contain an array of tests that can be run on geometry to diagnose potential problems for mesh
generation. To display a list of tests, click on the Show Options check box. By default all tests are selected and run on
geometry. Some tests may not apply to specific geometry, or may only need to be run once per geometry (i.e. bad
geometry definition test). Clicking on the box by each test will deselect it.
The geometry analysis inputs and tests are summarized below:
Shortest Edge Length -The shortest edge length is a value that is input by the user. It determines the minimum allowable
threshold for small features. It is used as an input to test for small curves, small surfaces, small volumes and close loops.
The default value for this is 1. This value should be changed relative to the size of the model. In a very broad sense, it
represents a desired mesh edge length. Curves and surfaces which are smaller than this size, and which may be
troublesome to mesh with the desired granularity, will be flagged and they can be removed or modified.
59
Trelis 15.0 User Documentation
Bad Angle Upper/Lower Bounds - The bad angle upper/lower bounds are tolerances set by the user to determine the
definition of small or large angles. The default values are set at 350 degrees for the large angle and 10 degrees for the
small angle. These values are used to test for angles between curves, surfaces, and at tangential intersections.
Bad Angle Check - The bad angle check will test for small angles between curves, surfaces, and at tangential
intersections. The test will only look for curves or surfaces that are adjacent.
Tangential Intersection - A tangential intersection is formed when two parallel surfaces share an
edge and have a 180 degree angle between them. The tangential intersection test is looking for the
condition where two surfaces that meet tangentially share a common edge, and each of the surfaces
has another edge which resides on a third face and forms a small angle as shown in the following
example. Surface 1 and Surface 2 are tangential to each other and share a common edge. Both
Surface 1 and 2 have another edge which resides on Surface 3 and forms a small angle at the vertex
common to all three surfaces.
Figure 2. Tangential Intersection
Mergeable Entities Check - As it suggests, this test is looking for entities that overlap and that can be merged. Pressing
the "Merge all" button on the Power Tools will automatically merge all entities flagged by the merge test.
Overlap Check - The overlap tests look for geometry that are either overlapping or coincident (exactly on top of each
other). Keep in mind that some of these problems may disappear with imprinting and merging.
Small Features Check - Small features may be necessary and desirable in a model, but many times they are the result of
poor geometry translation or import, or they may just not be important to the analysis. The small features tests look for
small curves, small surfaces, and small volumes. These tests rely on the user-defined short edge length parameter. Small
curves, including zero-length curves such as hardpoints, are compared directly against the defined parameter, and
flagged if they less than or equal to the given parameter. Small surfaces and volumes, on the other hand, are compared
against their hydraulic radius. For surfaces the hydraulic radius is 4*surface_area/perimeter. For volumes the hydraulic
radius is 6*volume/surface_area.
Bad Geometry Definition Check - Trelis uses third party libraries, such as ACIS from Spatial, Inc. for much of its
geometric modeling capabilities. The bad geometry definition check calls internal validation routines in these libraries,
when available, to check for errors in geometry definition. If the third party library does not provide validation capabilities,
this check will not return anything. Note: ACIS is a trademark of Spatial.
60
Geometry Power Tools
Blend Surface Check - A blend surface is a transition surface between two orthogonal planes, such as a fillet. The blend
surface check identifies the surfaces which meet this criterion. Many times these surfaces are candidates for the split
surface command or the remove surface command. The split surface command allows you to split these blend surfaces
into two surfaces, making it easier to mesh the volume. The remove surface command removes the surface and extends
the adjoining surfaces until they intersect.
Close Loops Check - Close loops (pronounced KLOS, not KLOZ) are two loops on a single surface for which the
shortest distance between loops is less than a user specified tolerance. The tolerance for close loops is the square of the
shortest edge length parameter. Close loops are common around holes and fillets, and are usually found where one loop
is entirely within the other loop. These surfaces are often candidates for removal, or tweaking.
Geometry Repair Tools
Note: Pressing most of the geometry tool buttons on the panel will only bring up applicable command panels on the
Control Panel. You must press the Apply button on the Control Panel to execute the command.
Split Surface Button
The split surface tool is used to split a surface into two surfaces. This is useful for blend surfaces, for example, where
splitting a surface may facilitate sweeping. To select a surface for splitting, click on the surface in the tree view. To select
multiple surfaces in the window, hold the CTRL key* while selecting surfaces (surfaces must be attached to each other).
Then press the split surface button to bring up the Control Panel window with the ids of selected surfaces in the text input
window. The split surface menu is located on the Control Panel under Geometry-Surface-Modify. You must press the
Apply button for the command to be executed. You can also bring up the Split Surface menu by selecting surfaces in the
tree view and selecting Split from the right click menu.
*Note: For Mac computers, use the command key (or apple key) to select multiple entities
Heal Button
The healing function in Trelis is used to improve ACIS geometry that has been corrupted during file import due to
differences in tolerances, or inherent limitations in the parent system. These errors may include: geometric errors in
entities, gaps between entities, and the absence of connectivity information (topology). To heal a volume, select the
volume in the geometry repair tree view. Then press the heal button. You may also press the heal button without a
geometry selected in the window, and enter it later. The Control Panel window will come up under the Geometry-VolumeModify option with the selected volume id highlighted. If no entity is selected, or if another entity type is selected, the input
window will be blank. You can also open the healing control panel by selecting Heal from the right click menu in the
geometry power tools window.
Tweak Button
The tweak command is used to eliminate gaps between entities or simplify geometry. The tweaking commands modify
geometry by offsetting, replacing, or removing surfaces, and extending attached surfaces to fill in the gaps. Tweaking can
be applied to surfaces, and it can be applied to curves with a valence no more than 2 at each vertex. It can also be
applied to some vertices. To tweak a surface, select the surface in the tree view. The Geometry-Surface-Modify control
panel will appear with the selected surface id in the input window.
Tweaking is available for curves. Tweaking a curve creates a blended or chamfered edge between two orthogonal
surfaces. The curve option is located on the Geometry-Curve-Modify panel under the Blend/Chamfer pull-down option.
Tweaking is also available for some vertices. Tweaking a vertex creates a chamfered or filleted corner between three
orthogonal surfaces. The vertex option is located on the Geometry-Vertex-Modify panel under the Tweak pull-down menu.
Note: Only curves with valence 2 or less at each vertex are candidates for tweaking. Any other curve will cause
the Geometry-Surface-Modify menu to appear.
Merge Button
The merge command is used to merge coincident surfaces, curves, and vertices into a single entity to ensure that mesh
topology is identical at intersections. Unlike other buttons on the geometry repair panel, the merge button acts as an
"Apply" button itself. All geometry that is listed under "mergeable entities" will be merged.
61
Trelis 15.0 User Documentation
Remove Button
The remove button is used to simplify geometry by removing unnecessary features. To use the remove feature, click on
the surface(s) in the Tree View. Right click and select the Remove Option, or click the Remove icon on the toolbar. The
Control Geometry-Surface-Modify control panel will appear, with the surface ids in the input window. The Remove control
panel can also be accessed from the right-click menu in the Geometry Power Tools window. Select options and press
apply.
Regularize Entity Button
The regularize button is used to remove unnecessary topology. Regularizing an entity will essentially undo an imprint
command.
Remove Slivers
The remove slivers button is used to remove surfaces with less than a specified surface area. When ACIS removes a
surface it extends the adjoining surfaces to fill the gap. If it is not possible to extend the surfaces or if the geometry is bad
the command will fail.
Auto Clean Geometry
The auto clean button is used to perform automatic cleanup operations on selected geometry. These automatic cleanup
operations include forcing sweepable configurations, automatically removing small curves, automatically removing small
surfaces, and automatically splitting surfaces.
Composite Button
The composite button is used to combine adjacent surfaces or curves together using virtual geometry . Virtual geometry is
a geometry module built on top of the ACIS representation. Surfaces may be composited to simplify geometry in order to
facilitate sweeping and mapping algorithms by removing constraints on node placement. It is important to note that solid
model operations such as webcut, imprint, or booleans, cannot be applied to models that have virtual geometry. Both
curves and surfaces may be composited.
Collapse Angle Button
The collapse angle button uses virtual geometry to collapse small angles. This is accomplished by partitioning and
compositing surfaces in a way so that the small angle gets merged into a larger angle. Pressing the collapse button on the
geometry power tools will open the collapse menu under Geometry-Vertex-Modify control panel. This panel can also be
opened by selecting Collapse from the right click menu in the Geometry Tools window.
Collapse Surface Button
Pressing this button will open the collapse surface panel on the main control panel. The collapse surface function uses
virtual geometry to eliminate small surfaces on the model to improve mesh quality. It is most useful for blend surfaces.
Collapse Curve Button
Pressing this button will open the collapse curve panel on the main control panel. The collapse curve command is used to
eliminate small curves using virtual geometry.
Reset Graphics Button
The reset graphics button will refresh the graphics window display.
62
Geometry Power Tools
Right Click Menu
The following right click menu is available from the geometry power tools. Specific options depend on the type of entity
selected.
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
Zoom To- Zoom to selected entity in the graphics window
Reset Zoom - Reset graphics window zoom
Fly-in - Animated zoom
Locate - Labels the selected entities in the graphics window. Refresh screen to hide.
Draw - Displays only selected entities by themselves.
Highlight - Highlights selected entities.
Draw with Neighbors - Displays only selected entities with all attached neighbors
Clear Highlights - Clears all highlighted entities and reset graphics
Reset Graphics - Reset graphics window
Tweak - Opens the tweak menu in the main control panel
Remove - Opens the remove menu in the main control panel
Remove Slivers - Opens the remove sliver menu in the main control panel
Remove all - Available when the clicking on an item in the "small surfaces" list. Opens the remove menu in the
main control panel with all surfaces in the category as inputs. The individual option will be selected on the panel
by default.
Split - Opens the split surface or split curve menu in the main control panel, depending on the type of entity
selected.
Auto Clean - Opens the auto clean menu in the main control panel.
Regularize - Issues the regularize command on selected entity.
Merge Selected - Merge selected entity from mergeable entities list
Merge All - Merge all entities listed in the mergeable entities list
(Virtual) Composite - Opens the composite menu in the main control panel
(Virtual) Collapse - Opens the collapse angle menu the main control panel
Collapse Surface (Virtual) - Opens the collapse surface menu on the main control panel
The following right click options are available when category headings are selected.
•
•
•
•
Analyze Geometry - Similar to pushing the Analyze button.
Highlight All - Highlight all members of this category.
Draw All - Display only members of this category.
Locate All - Label all members of this category.
63
Meshing Tools
The meshing power tool provides a tool for determining whether a geometry can be meshed using autoscheme, or if it
requires its scheme to be set explicitly. This tool is designed to help guide users through geometry decomposition process
by providing a convenient way to see which geometries need further modification or decomposition prior to meshing.
Figure 1. Meshing Power Tools
Entity Specification- The meshing power tool works for volumes or surfaces.
Options Button - Opens the Tools>Options dialog to change the visualization colors of surface schemes for the
meshing tool
Analyze Button - The Analyze button issues the autoscheme command for all selected volumes and surfaces.
Output Tree - The output from the meshing tool is displayed in tree format. Geometry is divided into "Scheme Set" and
"Scheme Not Set" divisions. The geometry is listed under these nodes. If autoscheme was successful, its assigned
scheme is also displayed.
Toggle Visibility Button - The meshing tool displays entities as red or green in the graphics window. Green means that
they are currently meshable using the autoscheme. Red means that they require their scheme to be set explicitly. Turning
this capability off will return the volumes and surfaces to their original colors.
Meshing Tools Buttons - Several meshing tools are available to the user from this window. Depending on the entity
selected, these are also available from the right-click context menu, and they are described below.
Right Click Context Menu
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
Zoom To - Zoom in on this element in the graphics window
Draw - Draw this entity by itself in the graphics window
Locate - Locates and labels entity in the graphics window
Rotate About - Issues Rotate about command for selected entity
Visibility On/Off - Toggle visibility
Reset Graphics- Reset graphics display
Set Size - Opens the Mesh/Entity/Interval panel on the control panel where you can set interval sizes for the
selected geometry
Set Scheme - Opens the Mesh/Entity/Mesh panel on the control panel where you can set a scheme for the
selected entities
Set Vertex Type - Available when surfaces are selected. Opens the Mesh/Surface/Mesh panel to set vertex
types.
Imprint/Merge- Opens the Geometry/Entity/Merge panel on the control panel. If you have entities selected in
the tree window it will input them to the imprint/merge command.
Webcut - Opens the Geometry/Volume/Webcut panel on the control panel. If a volume is selected in the
meshing tool window it will input it in the webcut panel.
Color Surfaces - Color surfaces based on their schemes. You can change the default colors by selecting the
Options button.
Restore Colors - Restores colors on selected entity or entity type
Mesh - Meshes the selected entities (bypassing control panel)
Delete Mesh - Deletes the mesh on selected entities
Unmerge - Unmerges selected entities
View Descendants - Opens a list of child entities and their meshing schemes. Press Analyze to return.
View Ancestors- Opens a list of parent entities and their meshing schemes. Press Analyze to return.
View Neighbors- Opens a list of bordering entities and their meshing schemes. Press Analyze to return.
65
Mesh Quality Tools
The mesh quality tool is located in the entity tree window under the quality tab. The Mesh Quality Tool works on meshed
entities to analyze mesh quality based on selected metrics. Output from the mesh quality analysis can be visualized using
color-coded scales. The mesh quality tool also contains tools to improve mesh quality including smoothing, refinement,
node merging, mesh validation, deleting mesh elements, and repositioning nodes.
Figure 1. Mesh Quality Tools
Entity Type - The mesh quality tools can only be applied to mesh entities including volumes, surfaces, hexahedra,
quadrilaterals, triangles, or tetrahedra.
Help Button - Opens context specific help for this topic.
Options Button - Clicking on this button will show the Tools>Option menu dialog that allows users to manually enter
metric range settings. The settings are persistent between sessions. For a description of quality metrics and default
ranges click on one of the following links:
•
•
•
•
Metrics for Hexahedral Elements
Metrics for Quadrilateral Elements
Metrics for Tetrahedral Elements
Metrics for Triangular Elements
Visual Button - Clicking on this button will open the Mesh/Entity/Quality command panel specific to the entity selected.
To visualize elements in the graphics window based on a color-coded quality scale, you must select the entities to
visualize and check the "Display Graphical Summary" check box. Once that box is selected, you must also make sure the
"Draw Mesh Elements" option is selected. Then press the Apply button
Analyze Button - This button starts the quality processing based on the metrics/filters selected.
67
Trelis 15.0 User Documentation
Output Window/Tree - The failed elements are shown in the tree under the heading "Poor Elements". For each
metric/filter the output will be listed in a tree format with the following nodes.
1.
2.
3.
4.
The top node on the tree is the name of the metric.
The next node under is the owning volume or surface when volumes or surfaces are analyzed.
The next node will be categories or groups of elements. Possible categories are:
o All Above Threshold - represents all mesh elements above the quality threshold upper range
o All Below Threshold - represents all mesh elements below the quality threshold lower range
o Top "n" - This will expand into a list, up to 50 elements long, of the worst offending elements above
the upper threshold range.
o Bottom "n" - This will expand into a list, up to 50 elements long, of the worst offending elements below
the lower threshold range.
At the lowest level of the tree are mesh elements.
The mesh elements can be sorted by quality or by numeric order. To change the way items are sorted, click on the
headings. The right-click or context menu will show various remedies depending on what is selected. Performing an
operation on a parent node will perform the same operation on all of the child nodes.
Mesh Quality Tool Buttons
The buttons on the bottom of the mesh quality tool window are some of the tools you may use to improve mesh quality
and include.
•
•
•
•
•
•
•
•
Smooth Button - Opens the Mesh>Entity>Smooth panel
Refine Button - Opens the Mesh>Entity>Refine panel
Move Node - Opens the Mesh>Node>Move Node panel
Merge Node - Opens the Mesh>Node>Merge Node panel
Delete Mesh Element - Deletes selected mesh entity
Validate Mesh - Issues the validate mesh command
Check Coincident Nodes - Issues the check coincident nodes command.
Refresh Graphics
Right-Click Context Menu Items
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
68
Draw - issues a draw command for any tree node below the metric name.
Color Code - Issues a 'quality .... draw mesh' command for any tree node below the metric name
Locate - Issues Locate for volume/surface/hex/quad/tet/tri. The locate command will draw and label selected
entities in the graphics window.
Fly-In - Issues Fly-in for volume/surface/hex/quad/tet/tri. The fly-in command is an animated zoom feature.
Zoom to - Issues Zoom command for volume/surface/hex/quad/tet/tri
Rotate About - Issues Rotate About command for volume/surface/hex/quad/tet/tri
Vis on/off - Issues visibility on/off for volume/surface
Smooth - Issues generic smooth command for volume/surface/hex/tet
Smooth Surface Parent - issues a smooth surface command for the surface parents of selected quads and
tris.
Delete Mesh - issues delete mesh propagate command for vol/surf
Delete Elements - issues delete element command for mesh entities in all categories except 'all'
Validate mesh - validates selected volume or surface
Check Coincident Nodes - checks for coincident nodes on volume or surface
Smooth Panel - brings up the correct smooth panel depending on what's selected
Smooth Surface Panel - bring up the smooth surface panel with correct surface ids for selected quads and tris
Merge Node Panel - brings up the panel to merge nodes
Move Node Panel - brings up the panel to move nodes
Reset Graphics - resets the display
Property Page
The Property Page is a window that lists properties about the current entity selection. Some of the properties, like Trelis
ID, entity type, or geometry engine, are listed for reference only. Other attributes, like name, or mesh intervals, color,
mesh scheme, or smooth scheme can be edited from the window. The Property Page is located on the left panel in the
GUI. The highlighted entity/entities in the graphics window are listed in the property page window. The Property Page also
lists information about selected mesh entities, boundary conditions, and assemblies. Selecting an object from the Tree
View will also open the object in the property page.
Figure 1. Property Page Window
The row of buttons on the top of the editor are shortcuts to common commands. These include:
>
Meshes the selected entity/entities at their current interval and scheme settings
Smooth selected entity using the current smoothing scheme
Preview mesh intervals on selected entity
Delete mesh on specified entity (do not propagate to lower order entities)
Reset entity to default settings and delete mesh
Calculates volumes and surface areas
Delete current entity
69
Trelis 15.0 User Documentation
Editing Entity Attributes from the Property Page
The Property Page provides a convenient way to change attributes on entities. . Some of the fields cannot be changed,
some can be edited from an input field, and others are edited by selecting from a list, or by opening the corresponding
window from the Control Panel.
If multiple entities are selected, the attributes that are similar to both entities will be shown. Changing an attribute from the
property page will change that attribute on both entities. If multiple entities are selected the total volume, surface area, and
length of all entities will be shown.
Below is a summary of properties listed for each attribute type.
General Attributes
•
•
•
•
Entity ID - Trelis ID for geometry or boundary condition element
Entity Type - Geometric type such as Volume, Surface, Curve, Vertex
Name - Name by which the entity can be referred to from within Trelis instead of using its ID. The entity name
can be edited from this window.
Color - Opens a dialog box with available colors. A color name can also be input directly into the text field. See
Appendix for a list of available colors.
Geometry Attributes
•
•
•
•
•
•
•
•
Is Merged - Returns "Yes" if this entity is merged
Is Virtual - Returns "Yes" if this entity is a virtual entity
Location - Returns the location of specified vertex.
Geometry Engine - ACIS or Mesh-Based Geometry
Volume - The volume of the specified body
Surface Area - Surface area of selected surface
Analytic Type - Returns the analytic type of entity (such as cone, sphere, etc)
Length - Length of selected curve
Meshing Attributes
•
•
•
•
•
•
•
•
•
Is Meshed - Returns "Yes" if the entity is already meshed
Number of Elements - Similar to "List Totals" command
Intervals - Number of mesh intervals on element. This can be edited from this window. The number must be an
integer
Interval Size - Interval size for element. Clicking on box will open the interval specification panel on the control
panel. The interval size can also be entered manually in the text box.
Meshed Volume - The meshed volume may be slightly different than the actual element volume due to the
mesh approximation on curved surfaces.
Meshed Area - The meshed area may be slightly different than the actual surface area due to mesh
approximation on curved edges.
Length of Meshed Edges - Combined total of mesh edge lengths on curve
Mesh Scheme - The mesh scheme for this entity. This can be changed from the property page by selecting
from the drop-down list.
Smooth Scheme - The smooth scheme for this entity. This can be changed from the property page by
selecting from the drop-down list.
Boundary Condition Attributes
•
•
70
ID - Boundary condition ID. This is an arbitrary user-defined ID that is exported with the finite element model.
This value can be edited from the property page
Name - A user-defined name that is included in the metadata for that object. This value can be edited from the
property page.
Property Editor
•
•
•
•
•
•
Description - A user-defined description that is included in the metadata for that object. This value can be
edited from the property page.
Color - Opens a dialog box with available colors. A color name can also be input directly into the text field. See
Appendix for a list of available colors.
Element Type - The finite element type for this block, nodeset, or sideset.
Element Count - The total number of elements for this block or sideset
Node Count - Total number of nodes (available for nodesets only)
Attribute Count and Attributes- The attributes represent material specification data that is associated with the
element block. These values can be changed in the property page. You can specify up to 10 attributes per
block.
Metadata Attributes
•
•
•
•
•
•
•
•
•
Type - The metadata type: Assembly, Sub-Assembly or Part
Name - The name for the assembly or part. This can be edited from the property window.
Instance - The numeric value associated with the part or assembly
Path - The absolute path of the part or assembly.
Description - The description of the part or assembly. This can be edited from the property page
Material Description - The name or description of the material of which this part is composed. Applies only to
parts. This can be edited from the property window.
Material Specification - The formal specification number of the material of which this part is composed. This
can be edited from the property window.
File Format - The name of the file system containing the original version of this entity. This can be edited from
the property page
Units - The unit system of this part or assembly. This can be edited from the property page
The part name, description and material description are available when the associated volume is selected, and not just
when the part is selected.
71
Command Line Workspace
The Command Line Workspace is the interface for command interaction between the user and the Trelis application. The
user can enter commands into this window as if they were using the command line version of Trelis. Journaled commands
will be echoed to this screen, even if they were not typed in manually. Thus, if the user wants to know what the command
sequence for a particular action on the GUI is, they can watch for the "Journaled Command:" line to appear. In addition,
this screen will contain important informational and error messages. The command window has the following four tabs:
1.
2.
3.
4.
Command
Error
History
Script
The Script window is hidden by default. To turn it on open the Tools-Options dialog and check the "Show Script Tab under
Layout/Trelis Layout.
Command Window
The command line workspace emulates the environment in the command line version of Trelis. Commands can be
entered directly by typing at the Trelis> prompt. This window also prints out error messages, informational messages, and
journaled commands.
Entering Commands
To enter commands in the command line workspace, the command window must be active. Activate the command
window by clicking anywhere inside the window. Commands are typed in at the Trelis> prompt. If you do not remember
the specific command sequence you can type help and the name of the command phrase. The input window will show all
of the commands that contain that word or phrase. Alternatively, if you know how a command starts, but do not remember
all of the options, you can type ? at the end of the command to show all possible command completions. See Command
Syntax for an explanation of command syntax rules.
Repeating Commands
Use the Up and Down arrow keys on the keyboard to recall previously executed commands.
Commands can be repeated in other ways as well.
•
•
Hitting the enter key while the cursor is on a previous command line will copy that command to the current
prompt.
The command window supports copy and paste for repeating commands.
Focus Follows Cursor
Beginning with version 13.0, Trelis includes a 'focus follows cursor' option for the command window. The option can be
enabled and disabled from the Tools/Options/General options panel. The setting is persistent between sessions and is
disabled by default.
Please note, the focus follows cursor behavior is available only in the command window. All other windows or widgets
require the user to click the mouse in order to grab focus.
73
Trelis 15.0 User Documentation
Error Window
The error window is located in the Command Line Workspace under the Error tab. If there are errors, a warning icon will
appear on the tab. The icon will disappear when you open the window to view errors. The error window only displays the
error output, which can make it easier to find and read the error output. The command that caused the error will be printed
along with the error information. If the command was from a journal file, the file name and number will be printed next to
the command.
History Window
The history window lists the last 100 commands. The number of commands listed can be configured in the options dialog
on the History page. You can re-run the commands in the history window using the context menu. You can also clear the
history using the context menu.
Script Window
Trelis boasts a robust Python interpreter built right into the graphical user interface. To create a Python script using the
Script tab, start typing at the "%>" prompt. At the end of each line, hit Enter to move to the next line . To execute the
script, press Enter at a blank line. Scripts may also be written in the Journal File Editor.
The Claro Python interpreter works as though you were entering lines from the Python command prompt. This means that
a blank line is interpreted as the end of a block. If you want to add whitespace for clarity you have to add a # mark for a
comment on any white line that is in a loop or a class.
One possible solution to this problem is to create two Python files. The first file can contain the complex set of Python
instructions(program.py) including blank lines. The second file will read and execute the first file. An example syntax for
the second file is given below.
f = file("program.py")
commandText = f.read()
exec(commandText)
You can then execute the second program within Trelis.
The interface between Trelis and python is the "Trelis" object. This object has a method called cmd which takes as an
argument a command string. Thus, the following command in the script window:
Trelis.cmd("create brick x 10")
will create a cube with sides 10 units long. The following script is a simple example that illustrates using loops, strings,
and integers in Python.
%>for i in range(4):
. . x=i*3
. . for j in range(4):
. . y=j*3
. . for k in range(4):
..
z=k*3
..
mystr="create vertex x "+str(x)+" y "+str(y)+" z "+str(z)
..
Trelis.cmd(mystr)
This simple script will create a grid of vertices four wide. Scripts can be more advanced, even creating customized
windows and toolbars. For a complete list of python/Trelis interface commands see the Appendix.
Docking and Undocking the Input Window
The command window can be undocked by clicking and dragging the left edge. If it is floating it can be redocked by
double-clicking the solid blue bar. By default, it will always be redocked in the bottom of the application window. To
change the size of the floating window, click and drag the edge of the window. To change the height of the docked
window, click and drag the top edge or right edge.
74
Journal File Editor
The Journal File Editor is a built-in, multi-document text editor that can read, edit, play, and translate Trelis journal files
and Python Scripts. To open the journal file editor, select the
Menu.
icon on the File Tools toolbar, or from the Tools
Figure 1. The Journal File Editor
The Journal File Editor can be used to create a new Python or Trelis command script. By default, a new journal file will be
in Trelis command syntax. You can change the default in the options dialog. On the "General" options page, under the
Journal Editor heading, you can select the default syntax. You can change the new journal file's syntax using the
translation buttons as well. When you have the correct syntax selected, enter the commands in the order you want them
executed. You can play the commands all at once using the play button on the toolbar. You can also play a few
commands at a time. Select the commands you want to play. Then, right click and select the "Play Selected" menu item.
The Journal File Editor can also be used to edit an existing journal file. Use the File > Open menu item to open the file you
want to edit. You still have all the command play options with an existing journal file.
75
Trelis 15.0 User Documentation
You can import commands entered in the Command Line Workspace. The File > Import menu item contains a list of
available imports. Select the tab you want to import from. Only the current commands will be imported from the command
line. Some of the commands you previously entered might not show up if you have the recommended text trimming turned
on. Text trimming improves the application's performance for speed and memory. It will trim off the oldest text in the
window when a size limit is reached. To get all the command from your current session, make sure that command
journaling is turned on.
The Journal File Editor can be used to edit Python or Trelis command scripts. It can also translate between the two forms.
Translating from Python to Trelis commands can cause commands to be lost. The Journal File Editor will warn you when
doing so.
The Journal File editor can be used to edit multiple files at the same time. Each document is displayed in its own tab. The
tab shows the journal file's syntax and name. If you close the Journal File Editor with unsaved data, it will prompt you to
save changes for each of the modified journal files you have open.
Journal Editor Toolbar
The Journal Editor's Toolbar provides quick access to several important functions.
•
•
•
•
•
•
•
•
•
•
•
New - Creates a new journal file. The new journal file is placed in a new tab.
Open - Used to select a journal file to open.
Save - Saves the current journal file.
Undo - Undo the last text change.
Redo - Redo the last text change, after Undo.
Cut - Standard text cut operation
Copy - Standard text copy operation
Paste - Standard text paste operation
Play Journal File - Plays the entire journal file
Translate to Python - Translates the current Trelis commands in the journal file to Python scripts.
Translate to Trelis - Translates the current Python script in the journal file to Trelis commands.
Other Functionality Available in the Journal Editor
The context ('right-click') menu in the journal editor includes several additional functions, including:
•
•
•
•
76
Comment Selected Lines - Highlight any text, select 'comment selected lines', and the highlighted lines will be
commented.
Uncomment Selected Lines - Highlight any text, select 'uncomment selected lines', and the highlighted lines
will be uncommented.
Clear - select this menu item to clear the contents of the journal file.
Find - Selecting 'find' from the context menu, or from the edit menu, will bring up a dialog enabling the user to
find text in the journal file. Options are available to do case-sensitive searches, change search direction, and so
forth.
Toolbars
The Trelis toolbars provide an effective way for accessing frequently used commands.
Below is a brief description of each of the available toolbars. To view a description of the function of each tool, hold the
mouse over the tool in the Trelis Application to display tool tips.
File
Provides Trelis (*.cub) file operations. This toolbar also includes Journal File operations.
Figure 1. File Toolbar
Display
Controls the display mode, checkpoint undo, zoom, perspective clipping plane, and curve valence display options in the
Graphics Window.
77
Trelis 15.0 User Documentation
Figure 2. Display Toolbar
Select
Controls the Entity Selection Mode for picking or selecting entities. Also controls options for box/polygon selection.
Figure 3. Select Toolbars
78
Options Menu
To change program preferences in the Graphical User Interface select: Tools > Options . The options menu includes:
•
•
•
•
•
•
•
•
•
•
•
Custom Tools
Display
General
Geometry Defaults
History and Trelis Journalling
Label Defaults
Layout
Mesh Defaults
Mouse Settings
Post Processor
Quality Defaults
Note: Mac users reach this dialog box by selecting the Trelis > Preferences menu.
Custom Tools
This menu controls the creation of Custom Toolbar buttons.
Display Preferences
This menu controls entity display features for the graphics window which include the following:
•
•
•
•
•
•
•
•
•
•
•
Display Triad in Graphics Window
Enable Pre-Selection
Background Color
Perspective Angle
Line Width
Highlight Line Width
Text Size
Ambient Intensity
Ambient Color
Light Intensity
Light Color
General Preferences
This menu controls general program options including the following:
•
•
•
•
Prompt for Unsaved Application Data - When this is checked and the user opens a new .cub file or exits the
application with unsaved changes, a dialog box will pop up asking if they want to save changes first. The user
can uncheck this option to prevent that dialog box from appearing. This is checked by default.
Prompt for Unsaved Journal Data - When this button is checked and the user closes the journal file editor
with unsaved changes the program will prompt to save the changes. The user can uncheck this button to
prevent the dialog box from appearing. It is checked by default.
Change to Script Directory for Playback - When this option is checked, Claro will change the working
directory to the directory the script is in when the script/journal file is run. When the script is finished, Claro will
change the directory back to the previous one. This is useful when using relative paths in a journal file. When
the option is unchecked, Claro won't change the directory when a journal file is run in which case the user may
have to manually change the working directory when their journal file has relative paths.
Prompt When Translating from Python - When checked, if the user translates a python script to a Trelis
journal file, the journal editor will warn them that commands may be lost. When unchecked, the journal editor
will not issue the warning. There is a checkbox on the warning dialog that sets this option as well.
79
Trelis 15.0 User Documentation
•
•
Default Syntax - Sets the default syntax to use when creating a new journal file in the editor. The Trelis option
is only available when the Trelis component is loaded.
Show Startup Splash Screen - Option to hide the startup splash screen on opening Claro.
Geometry Defaults
This menu controls the geometry defaults.
•
•
•
Vertex Size
Use Silhouette on Geometry
Silhouette pattern
The user can also change the default geometry engine to one of the following:
•
•
ACIS
Facets
The faceting tolerance can also be controlled from this menu to change the way facets are drawn in the graphics window.
History Preferences
This menu controls the input window history and journal file options. These include:
•
•
•
•
•
•
Maximum Number of Commands - The max number of commands kept in the current command history.
Comment Line Filtering - Whether to count comments in command history.
Maximum Number of Lines - Maximum number of lines in input window.
Journal Command History - Whether to use a journal file to save command history. Default is to use a journal
file.
Journal File Directory - Where the journal file will be saved. Default is the starting directory.
Journal File Name - The name of the journal file. A name will be given by default if one is not specified. The
default name for the GUI version of Trelis is historyxx.jou with xx as the highest used number between 01 and
999 incremented by 1.
Trelis History Preferences
•
•
Use Trelis Journaling - When this option is checked, Trelis journaling will be used. By default it is checked.
Output Log - When this option is checked, you can save error log to a separate output file.
Label Defaults
This menu controls the geometry and mesh entity labels in the graphics window.
•
•
Text Size
Label Geometry and Mesh Entities Toggles- Choose label visibility for each type of geometry or mesh entity
Layout Preferences
This menu option controls input window formatting and control panel docking options.
•
•
•
Font for command line workspace
Font size for command line workspace
Reset Window Layout Button - Used to reset GUI windows to their default positions
Also included in the layout preferences is a list of available windows with a checkbox to show/hide each window.
80
Options Menu
Trelis Layout Settings
This menu controls the layout of Trelis specific buttons and tabs on the GUI.
•
•
•
Show script tab - Shows the script tab on the command line window
Use Labels on Buttons- Option to apply a label to each button on the control panel
Preferred Location (currently under construction)
Mesh Defaults
•
•
•
•
•
Node Size
Element Shrink
Mesh Line Color - The same as "Color Lines" command.
Default Element Type - Tet/Tri or Hex/Quad
Surface Scheme Coloring (used in Meshing Power Tool) - This option allows you to select different colors for
surface schemes when visualized using the meshing power tools.
Mouse Settings
This menu controls mouse button controls. Pressing the Emulate Command Line Settings button will cause all of the
settings to simulate mouse controls in the command line version of Trelis. For a detailed description of mouse settings see
the View Navigation-GUI page.
Post Processor Settings
Post Processor Executable Directory - Option to browse for post processor executable directory.
Quality Defaults
This menu controls quality defaults for different quality metrics. For a description of the different quality metrics see the
respective pages:
•
•
•
•
Hexahedral metrics
Quadrilateral metrics
Tetrahedral metrics
Triangular metrics
81
Creating Custom Toolbar Buttons
If you have a string of commands that you use frequently, it can be beneficial to make a custom toolbar button. To create
a custom toolbar button open the Tools->Options menu. You can create up to 10 custom buttons. See Figure 1 for an
example toolbar button.
Figure 1. Making a custom toolbar button to create and mesh a perforated brick
The button can have Python or Trelis commands. These commands will be executed in consecutive order when the
button is pushed. You must click the Enabled check box to activate your custom button.
You can assign a pixmap to your custom buttons or use the default. You can also assign a tool tip.
The buttons are persistent from each run of Trelis. To remove a button, uncheck the Enabled button.
83
Undo Button
Trelis has an undo capability. To enable the Undo feature click on the "Enable Undo" button on the Toolbar.
Enable Undo Button
Alternatively to turn undo on and off, the following command may be used in the command line:
undo {on|off}
The Undo capability is implemented for geometry commands including webcutting, geometry creation, transformations,
and booleans. Multiple undos are also allowed. The commands will be undone in reverse order of their execution.
Limitations
•
The undo button is not currently enabled for most meshing commands
85
Journal File Creation and Playback
Recording a Session
Command sequences can be written to a text file, either directly from Trelis or using a text editor. Trelis commands can be
read directly from a file at any time during Trelis execution, or can be used to run Trelis in batch mode. To begin and end
writing commands to a file from within Trelis, use the command
Record '<filename>'
Record Stop
Once initiated, all commands are copied to this file after their successful execution in Trelis.
Replaying a Session
To replay a journal file, issue the command
Playback '<filename>'
Journal files are most commonly created by recording commands from an interactive Trelis session, but can also be
created using automatic journaling or even by editing an ASCII text file.
Commands being read from a file can represent either the entire set of commands for a particular session, or can
represent a subset of commands the user wishes to execute repeatedly.
Two other commands are useful for controlling playback of Trelis commands from journal files. Playback from a journal
file can be terminated by placing the Stop command after the last command to be executed; this causes Trelis to stop
reading commands from the current journal file. Playback can be paused using the Pause command; the user is prompted
to hit a key, after which playback is resumed.
Journal files are most useful for running Trelis in batch mode, often in combination with the parameterization available
through the APREPRO capability in Trelis. Journal files are also useful when a new finite element model is being built, by
saving a set of initialization commands then iteratively testing different meshing strategies after playing that initialization
file.
87
Controlling Playback of Journal Files
The following commands control the playback of Journal Files:
Stop
Pause
Sleep <duration_in_seconds>
Resume [<n>]
Where
Next [<n>]
The playback of a journal file can be interrupted in two ways. If the stop or pause commands are encountered in the
journal file and Trelis is reading commands from a terminal (as opposed to a redirected file), playback of the journal file
will halt after that command.
The sleep command pauses execution for the specified number of seconds. It can be used to build a delay into journal
files during presentations.
If journal files that are playing back contain playback commands themselves, there may be multiple current journal files.
The where lists all current journal files and where the journal files have paused. Each line contains the stack position (a
number), the filename and the current line in the file. Unless Trelis is running in batch mode, the first line is always
<stdin>. This just means that Trelis will return to the command prompt after the top-most journal file has completed.
The remaining portion of any active journal file may be skipped by specifying the stack position (first number on each line
of the output from the where command) of the file where you want to resume. Any remaining commands in active journal
files with lower stack positions will be skipped.
The next command steps through interrupted journal files line-by-line. The argument to the next command is the number
of lines to read before halting playback again. If no number is specified, the command will advance one line.
Journal playback can also be set to stop automatically when it encounters an error during playback. The command syntax
is:
Set Stop Error {On|OFF}
Setting the stop error to "on" will cause the file to halt for each error. The setting is turned off by default.
89
Automatic Journal File Creation
Controlling Automatic Journal File Creation
By default, Trelis automatically creates a journal file each time it is executed. The file is created in the current directory,
and its name begins with the word "Trelis " or "history", depending on the version of Trelis, followed by a number starting
with cubit01.jou and continuing up to a maximum of cubit999.jou. It is recommended that the user keep no more than
around 100 journal files in any directory, to avoid using up disk space and causing confusion. To that end, when the
journal name increments to more than cubit99.jou, a warning will be given on startup telling the user that there are at least
99 journal files, and to please clean out unused files. If the user has up through cubit999.jou, then the user is warned that
there are too many journal files in the current directory, and cubit999.jou will be re-used, destroying the previous contents.
When starting Trelis, the choice of journal file name to be used depends on whether it is creating a historyXX.jou file, or a
cubitXX.jou file. For historyXX.jou files, it will look for the highest used number in the current directory and increment it by
one. For example, if there are already journal files with names history01.jou, history02.jou, and history04.jou, Trelis will
use history05.jou as the current journal file. For cubitXX.jou files, Trelis will fill in gaps, starting with the lowest number.
For example, if there are already journal files with names cubit01.jou, cubit02, jou, and cubit04.jou, then Trelis will use
cubit03.jou as the current journal file.
Journal file names end with a ".jou" extension, though this is not strictly required for user-generated journal files. If no
journaling is desired, the user may start Trelis with the -nojournal command line option or use the command :
[Set] Journal {Off | On}
Turning journaling back on resumes writing commands to the same journal file.
Most Trelis commands entered during a session are journaled; the exceptions are commands that require interactive input
(such as Zoom Cursor), some graphics related commands, and the Playback command.
Recording Graphics Commands
All graphics related commands may be enabled or disabled with the command:
Journal Graphics {On | Off}
The default is Journal Graphics Off .
Recording Entity IDs and Names
When an entity is specified in a command using its name, the command may be journaled using the entity name, or by
using the corresponding entity type and id. The method used to journal commands using names is determined with the
command:
Journal Names {On | Off}
The default is Journal Names On .
If an entity is referred to using its entity type and id, the command will be journaled with the entity type and id, even if the
entity has been named.
Recording APREPRO Commands
APREPRO commands may be echoed to the journal file using the following command
[set] Journal [Graphics|Names|Aprepro|Errors] [on|off]
91
Trelis 15.0 User Documentation
See APREPRO Journaling for more information.
Recording Errors
The default mode for Trelis is to not journal any command that does not execute successfully. To turn this mode off and
echo all commands to the journal file, regardless of the success status, use the following command:
Journal Errors {On|OFF}
If a command did not execute successfully and the journal errors status is ON, then the unsuccessful command will be
written as a comment to the file. For example an unsuccessful command might look like the following in the journal file
## create brick x 10 x 10 z 10
Since Trelis recognizes this as erroneous syntax, it will issue an error when the command is issued, but will still write the
command to the journal file as a comment, prefixing the command with "##".
This option may be useful when tracking or documenting program errors.
92
Idless Journal Files
Journal files can also be created without reference to entity IDs. The purpose of this command is to enable journal files
created in earlier versions of Trelis to be played back in newer versions of Trelis. Using the "IDless" method, commands
entered with an entity ID will be journaled with an alternative way of referring to the entity. Changes in Trelis or ACIS often
lead to changes in entity IDs. For example, a webcut may result in volume 3 on the left and volume 4 on the right. In
another version of Trelis, those entity IDs may be swapped (4 on the left and 3 on the right). Playing an IDless journal file
makes the actual ID of an entity irrelevant. The syntax for this command is:
[set] Journal IDless {on|off|reverse}
The on option will enable idless journaling, and commands will be journaled without entity IDs. For example, "mesh
volume 1" may be journaled as "mesh volume at 3.42 5.66 6.32 ordinal 2".
Selecting the off option will cause commands to be journaled in the traditional manner (i.e., as they are entered).
The reverse option allows you to convert idless journal files back into an ID-based journal file where the new journal file
will reflect current numbering standards for IDs.
If you issue the command Journal IDless without any additional options, then the current status of ID journaling is
printed. At startup, this should be "off".
The most likely scenario for converting older journal is to use the record command during playback. The following is an
example.
journal idless on
record "my_idless.jou"
playback "my_journal.jou"
record stop
journal idless off
To record an idless journal file back into an id-based journal file you might use the following sequence.
journal idless reverse
record "new_id_based.jou"
playback "my_idless.jou"
record stop
journal idless off
Note: IDless conversions of APREPRO expressions are partially supported.
When IDless mode is set to ON, APREPRO functions such as Vx(id), that take an ID as an argument, are converted to
use (x, y, z, ord) as arguments such as Vx(x, y, z, ord), where (x, y, z) is the center point coordinates and ord is the
ordinal value. The ordinal values, 1..n, identifies each entity in a set of n entities that have a common center point. An
entity's ordinal value is based on its creation order with respect to the other entities within the same set.
When IDless mode is set to REVERSE (using the above example) Vx(x, y, z, ord) will be converted to Vx(id). Outside
these APREPRO functions, APREPRO expressions are not modified when converting a journal file to or from its IDless
form. Hence, expressions reduced to an entity ID, such as in the command "volume {x} size 10," are not
modified. Therefore, when moving a journal file from one version of Trelis to another, it may be necessary to manually
update IDs in APREPRO expressions.
93
Command Line View Navigation: Zoom, Pan and
Rotate
Commands used to affect camera position or other functions are listed below. All rotation, panning, and zooming
operations can include the Animation Steps qualifier, makes the image pass smoothly through the total transformation.
Animation also allows the user to see how a transformation command arrives at its destination by showing the
intermediate positions.
Rotation
Rotate <degrees> About [Screen | Camera | World] {X | Y | Z} [Animation Steps <number_steps>]
Rotate <degrees> About Curve <curve> [Animation Steps <number_steps>]
Rotate <degrees> About Vertex <vertex_1> Vertex <vertex_2> [Animation Steps <number_steps>]
Rotation of the view can be specified by an angle about an axis in model coordinates, about the camera's "At" point, or
about the camera itself. Additionally rotations can be specified about any general axis by specifying start and end points to
define the general vector. The right hand rule is used in all rotations.
Plain degree rotations are in the Screen coordinate system by default, which is centered on the camera's At point. The
Camera keyword causes the camera to rotate about itself (the camera's From point). The World keyword causes the
rotation to occur about the model's coordinate system. Rotations can also be performed about the line joining the two end
vertices of a curve in the model, or a line connecting two vertices in the model.
Panning
Pan [{Left|Right} <factor1>] [{Up|Down} <factor2>] [Screen | World ] [Animation Steps
<number_steps>]
Panning causes the camera to be moved up, down, left, or right. In terms of camera attributes, the From point and At
point are translated equal distances and directions, while the perspective angle and up vector remain unchanged. The
scene can also be panned by a factor of the graphics window size.
Screen and World indicate which coordinate system <factor> is in. If Screen is indicated (the default), <factor> is in
screen coordinates, in which the width of the screen is one unit. If World is indicated, <factor> is expressed in the model
units.
Zooming
Zoom Screen <factor> [Animation Steps <number_steps>]
Zoom <x_min> <y_min> <x_max> <y_max> [Animation Steps <number_steps>]
Zoom {Group | Body | Volume | Surface | Curve | Vertex | Hex | Tet | Face | Tri | Edge | Node}
<id_range> [Animation Steps <number_steps>] [Direction {options}]
Zoom cursor [click|drag][animation steps <number>]
Zoom Reset
Zoom Screen will move the camera <factor> times closer to its focal point. The result is that objects on the focal plane
will appear <factor> times larger.
Zooming on a specific portion of the screen is accomplished by specifying the zoom area in screen coordinates; for
example, Zoom 0 .25 .25 will zoom in on the bottom left quarter of the screen.
95
Trelis 15.0 User Documentation
Zooming on a particular entity in the model is accomplished by specifying the entity type and ID after entering Zoom. The
image will be adjusted to fit bounding box of the specified entity into the graphics window, and the specified entity will be
highlighted. You can specify a final direction to look at when zooming by using the direction option.
To center the view on all visible entities, use the Zoom Reset command.
The GUI tool bar buttons for controlling zoom in, zoom out, and zoom reset are as follows:
96
Mouse Based View Navigation: Zoom, Pan and
Rotate
The mouse can be used to navigate through the scene using various view transformations. These transformations are
accomplished by clicking a mouse button in the graphics window and dragging, sometimes while holding a modifier key
such as Shift or Control. When run with graphics on, Trelis is always in mouse mode; that is, mouse-based
transformations are always available, without needing to enter a Trelis command.
Mouse-based view transformations are accomplished by placing the pointer in the graphics window and then either
holding down a mouse button and dragging, or by clicking on a location in the graphics window. Some functions also
require one or more modifier keys to be held down; the modifier keys used in Trelis are Shift
and Control
.
Each of the available view transformations has a default binding to a mouse button-modifier key combination. This binding
can be changed by the user if desired. Transformations and button mappings are summarized in the following table.
Note: These settings are applicable only to the UNIX command line version of Trelis. For a description of the Graphical
User Interface Mouse Operations see GUI View Navigation.
The bindings are based on the following mouse button definitions:
Figure 1. Default Mouse Function Mappings for the Command Line
Table 1. Mouse Function Bindings for Zoom, Pan, and Rotate
Function
Description
Binding
Rotates the scene about the camera axis. Dragging the mouse near the
center of the graphics window will rotate the camera's X- or Y-axis;
dragging near the edge of the window will rotate about the Z-axis (i.e.
about the camera's line of sight). Type a u in the graphics window to see
the dividing line between the two types of rotation.
B1
Zoom
Zooms the scene in or out by clicking the mouse in the graphics window
and dragging up or down. If the mouse has a wheel, the wheel will also
zoom.
B2
Pan
"Drags" the scene around with the mouse
B3
Navigational
Zoom
Zooms the scene by moving both the camera and its focal point forward.
Telephoto
Zoom
Zooms the scene by decreasing the field of view.
Rotate
B2
B2
97
Trelis 15.0 User Documentation
Pan Cursor
Click on new center of view
B3
Changing the View Transformation Button Bindings
The default mapping of functions to mouse buttons, described in the Default Mouse Function Mappings table above,
can be modified. There are two ways to assign a function to a button/modifier combination.
First, you can use the command
Mouse Function <function_id> Button <1|2|3> [Shift][Control]
Type Help Mouse Function to see a list of function IDs that may be used in this command.
Second, you can assign functions interactively. To do so, first put the pointer into a graphics window and then hit the F
key. On-screen instructions will lead you through the rest of the process.
The GUI Options panel for managing the mouse bindings can be found at Tools/Options/Mouse, and is as follows:
98
Mouse Based View Navigation: Zoom, Pan and Rotate
Saving and Restoring Views
After performing view transformations, it may be useful to return to a previous view. A view is restored by setting the
graphics camera attributes to a given set of values. The following keys, pressed while the pointer is in the graphics
window, provide this capability:
V
- Restores the view as it was the last time Display was entered.
F1 to F12
- These function keys represent 12 saved views. To save a view, hold down the
Control key while pressing the function key. To restore that view later, press the same function key
without the Control key.
Note: In the Graphical User Interface version the F1, F2 and F3 keys are used as an alternate form of dynamic viewing,
therefore the ability to save views is not currently supported in the GUI.
You can also save a view by entering the command
99
Trelis 15.0 User Documentation
View Save [Position <1-12>] [Window <window_id>]
The current view parameters will be stored in the specified position. If no position is specified, the view can be restored by
pressing V in the graphics window. If a position is specified, the view can be restored with the command
View Restore Position <1-12> [Window <window_id>]
These commands are useful in as entries in a .Trelis startup file. For example, to always have F1 refer to a front view of
the model, the following commands could be entered into a .Trelis file:
From 0 1
At 0
Up 0 1 0
Graphics Autocenter On
View Save Position 1
The first three commands set the orientation of the camera. The fourth command ensures that the model will be centered
each time the view is restored. The final command saves the view parameters in position 1. The view can be restored by
pressing F1 while the cursor is in a graphics window.
Additionally, you can change the 'gain' on the mouse movements by changing the mouse gain setting, via the command:
Mouse Gain <value>
where a value of 3 would be 3X as sensitive to mouse movements, and a value of 0.5 would be half as sensitive.
Set ReverseZoom {on|off}
Another user preference, the direction of 'zooming' obtained by using the mouse can be 'flipped', by toggling the
reversezoom setting.
100
Updating the Display
Among the most common graphics-related commands is:
Display
This command clears all highlighting and temporary drawing, and then redraws the model according to the current
graphics settings. The GUI tool bar button for executing this command is:
Two related commands are:
Graphics Flush
Graphics Clear
Graphics Flush redraws the graphics without clearing highlighting or temporary drawing. Graphics Flush is useful when
a previously executed command modified the graphics and didn't update the screen and the user wishes to update the
display. The Graphics Clear command clears the graphics window without redrawing the scene, leaving the window
blank.
NOTE: Although most changes to the model are immediately reflected in the graphics display, some are not (for graphics
efficiency). Typing Display will update the display after such commands. Ctrl-R will also update the display as long as the
mouse is in the graphics window.
Prevent Graphics From Updating
For especially large models, it may take excessively long to update the display after an action has been performed. To
prevent the graphics from automatically updating, use the following command:
Graphics Pause
This command prevents the graphics window from being updated until the next time the Display command is issued.
NOTE: The Plot command is synonymous to the Display command, and either can be used with identical results.
101
Graphics Modes
By default, the scene is viewed as a smoothshaded model. That is, only curves and edges are drawn, and surfaces are
transparent. Surfaces can be drawn differently by changing the graphics mode:
Graphics Mode {Wireframe | Hiddenline | Smoothshade | Transparent } [Geometry | Mesh]
The GUI tool bar buttons for manipulating the graphics modes are as follows:
Examples and a brief description of each mode are shown below
WireFrame - Surfaces are invisible. (This mode can also be
accessed by typing 'wireframe' at the command prompt.)
HiddenLine - Surfaces are not drawn, but they obscure what is
behind them, giving a more realistic representation of the view. (This
mode can also be accessed by typing 'hiddenline' at the command
prompt.)
SmoothShade - Surfaces are filled and shaded. Shaded colors are
interpolated across the entire surface using the graphics lighting
model. This produces the most realistic results. (This mode can also
be accessed by typing 'shaded' at the command prompt.)
103
Trelis 15.0 User Documentation
Transparent - Renders surfaces as semi-transparent shaded images,
allowing objects to shine-through from behind. Is not supported on all
platforms, and generally requires advanced graphics hardware. (This
mode can also be accessed by typing 'transparent' at the command
prompt.)
This determines what pattern is used to draw lines behind surfaces (e.g. dotted, dashed, etc.; click here for a list of valid
line patterns).
Displaying Using the Element Facets
There is another option that is similar to a graphics mode, set with the command
Graphics Use Facets [On|Off]
This command determines how shaded and filled surfaces are drawn when they are meshed. If Graphics Use Facets is
on, the mesh facets (element faces) are used to render the model. This is particularly helpful for curved surfaces which
may cut through some of the mesh faces. A comparison of graphics facets on and off is shown below.
Figure 1. A meshed cylinder shown with graphics facets off (left) and graphics facets on (right); note how geometry facets
on the curved surface obscure mesh edges when facets are off.
Displaying Composite Surface Lines
Composite surfaces are surfaces that have been joined together using virtual geometry. By default, the underlying
surfaces are marked with dashed lines. To toggle this setting so that underlying surfaces are not shown, use the following
command:
Graphics Composite {On|Off}
104
Graphics Modes
Figure 2. A part shown with (a) composite surfaces displayed (b) composite surfaces not displayed
The GUI tool bar button for toggling the display of graphics composites is as follows:
105
Drawing and Highlighting Entities
In order to effectively visualize the model, it is often necessary to draw an entity by itself, or several entities as a group.
This is easily done with the command
Draw {Entity specification} [Color <color_spec>] [Zoom] [Add]
where Entity specification is an entity list as described in Command Line Entity Specification. This command clears the
display before drawing the specified entity or entities. Specification of a color will draw those entities in that color. This will
not permanently change the color of the entity. The zoom option will zoom in on the selected entities after drawing them in
the graphics window. If the add option is specified, the display is not cleared, and the given entity is added to what is
already drawn on the screen. The entities specified in this command are drawn regardless of their visibility setting (see
Geometry and Mesh Entity Visibility for more details about visibility).
Entities may also be drawn by selecting them with the mouse and then typing Ctrl-D while the mouse is in the graphics
window. This will clear the screen and then draw only those entities that are currently selected.
Entities can be highlighted using the command
Highlight {Entity specification}
This command highlights the specified entities in the current display with the current highlight color. Highlighting can be
removed using the command
Graphics Clear Highlight
To return to the normal display of the entire model, type Display.
The Locate command will label and point to the specified entity in the graphics window. The command syntax is:
Locate <entity_list>
Additionally, the visibility of individual entities, or sets of entities, can be controlled with the following visibility commands.
{Vertex|Curve|Surface|Volume|Body|Group} <range> [Geometry|Mesh] Visibility {on|off}
Edge [Visibility] {on|off}
{Mesh|Geometry} [Visibility]{on|off}
Drawing Other Objects
In addition to the common geometry, mesh and genesis entities, other objects may be drawn with variations of the Draw
command. As with the other Draw commands, typing Display after drawing these objects will restore the scene to its
normal display.
Displaying Entity Orientation
The normal to one or more surfaces, mesh faces, or mesh triangles may be drawn with the command
Draw {Surface | Face | Tri} <id_range> Normal [Length <length>] [Face | Tri]
If the Face or Tri qualifier is included in the Draw Normal command, the normals for all faces or tris that belong to the
specified surface are drawn.
The forward, or tangent, direction of a curve can be drawn with the command:
107
Trelis 15.0 User Documentation
Draw Curve <id_range> Tangent [Length <length>][Color <color_spec>]
If a color is not specified, the tangent is drawn in the same color as the curve.
Volume Sources and Targets
Once the source and target surfaces have been set on a volume that will be meshed with the sweep algorithm, the source
and target may be visually identified with the command
Draw Volume <volume_id_range> [Source][Target] [Length <size>]
If the Source keyword is included, the normal of the source surface or surfaces will be drawn in green into the specified
volume. If the Target keyword is included, the normal of the target surface or surfaces will be drawn in red into the
specified volume.
Model Axis
The model axis may be drawn with the command
Draw Axis [Length <length>]
The axis is drawn as three lines beginning at the model origin, one line in each of the three coordinate directions. The
length of those lines is determined by the length parameter, which defaults to 1.
Surface Isoparameter Lines
Isoparameter lines may be drawn on surfaces in the model using the command
Draw Surface <surface_id_range> Isoparametric [Number <number>| [u <number>] [v <number>]]
If you specify the Number of lines, then the number of u- and v-parameter lines will be equal. You may specify instead a
number of lines for each of the u and v parameters. The u-parameter lines will be drawn in red and the v-parameter lines
will be drawn in blue.
Surface Overlap
The overlapping regions between two surfaces may be drawn with the command
Draw Surface <id> <id>Overlap [Add]
This command will draw the curves of each of the surfaces in green, and the portion of the surfaces that overlap in red.
The Add keyword will draw the overlapping surfaces on top of the current graphics display. Without the Add keyword, the
display will only show the specified surfaces and their overlapping regions.
Volume Overlap
The overlapping region between two volumes may be drawn with the command
Draw Volume <id> <id> Overlap [Add]
This command will draw the input volumes in transparent mode and draw the volume(s) of intersection as red, shaded
solids. The Add keyword will draw the results on top of the current graphics display. Without the Add keyword, the display
will only show the specified volumes along with the intersection volume(s).
108
Drawing and Highlighting Entities
Geometry Preview
Several options are available for previewing geometry without actually generating it. This is typically used in conjunction
with webcutting and surface creation. The following Draw commands can be used for previewing geometry:
Draw Location On Curve
Draw Location
Draw Direction
Draw Line
Draw Polygon
Draw Axis
Draw Plane
Draw Cylinder
109
Mesh Visualization
A volume mesh can be viewed one layer at a time using a visualization tool known as mesh slicing. This tool divides the
elements of one or more volumes into axis-aligned layers, and then allows the mesh to be displayed one layer at a time.
Mesh slicing is especially useful to view the quality of swept meshes that are axis aligned.
Notes on Mesh Slicing
Mesh slicing is only intended to be a rough visualization tool. Because the average mesh edge length is used to
determine the thickness of each layer, a layer may be more than one element deep. Unstructured meshes, meshes with
large variations in edge length, and non-axis-aligned meshes will be more difficult to visualize with this tool.
Mesh Slicing Command
Mesh slicing can be started either by entering a keypress in the graphics window, which slices the mesh of the entire
model, or by entering the command
Graphics Slice {Body | Volume} <id_range> Axis {X | Y | Z}
which slices only the bodies or volumes indicated, with a plane along the axis specified.
Key presses in the graphics window which control mesh slicing are summarized in the following table.
Key
X,Y or Z
Action
Initiate mesh slicing using the X, Y or Z plane
K
Move the slicing plane in the positive coordinate direction
J
Move the slicing plane in the negative coordinate direction
S
Toggles drawing single or multiple slice layers in the view
Q
Exit from mesh slicing mode
See Graphics Clipping Plane for instructions on clipping the graphics using the GUI clipping plane.
111
Graphics Clipping Plane
The graphics clipping plane feature allows the user to temporarily cut parts of the model away to help visualize the interior
of a geometry or mesh. The command syntax is:
Graphics Clip {On|Off} [Location <location>] [Direction <direction>]
Graphics Clip Manipulation {On|Off}
The GUI tool bar buttons to enable and manipulate the Graphics Clipping Plane are shown below:
The first command activates the graphics clip manipulation tools in the graphics window. The keyboard shortcut "Shift-S"
while the graphics window is active will also activate the clipping plane. The manipulation of the clipping plane is
controlled as follows:
•
•
•
•
•
•
Red Line - Clicking and dragging the left mouse on plane bounded by a red tube moves the plane along the
arrow
Center Ball - Clicking and dragging the left mouse on the center ball moves the origin of the rotation plane
Arrow - Clicking and dragging the left mouse button on the arrow head or tail changes the direction on which
the plane moves
Right Mouse Button - Clicking and dragging the right mouse button on any part of the window resizes it
Middle Mouse Button - Clicking and dragging the middle mouse button on the red plane moves both the
center of rotation and the cutting plane
White Bounding Border - Clicking and dragging the left mouse on the white bounding border moves the whole
widget
Figure 1. Graphics Clipping Plane
113
Trelis 15.0 User Documentation
The second command turns on/off the visibility of manipulation widget in the graphics window. The clipping plane is still
active, but the controls are hidden. The normal mouse-based view navigation controls apply.
Examples
brick x 10
sphere rad 1
graphics clip on location -2 0 0
rotate -45 about y
#shows the sphere inside the brick
brick x 10
cylinder rad 2 z 12
subtract 2 from 1
mesh vol 1
quality vol 1 draw mesh
graphics clip on
#shows the mesh quality on interior elements
Figure 2. Viewing mesh quality of interior elements
114
Entity Labels
Most entities may be labeled with text that is drawn at the centroid of the entity.
Mesh entities can be labeled with their ID number or their Element ID. Element ID labels are only valid after putting the
mesh entities into a block.
Geometric entities can be labeled with their ID number or with other information.
Labels for groups of entity types can be turned on or off.
The following commands will accomplish this.
Label [On|Off|Name [Only|ID]|ID|Interval|Size|Merge|Firmness]
Label All [On|Off|Name [Only|ID]|ID|Interval|Size|Merge|Firmness]
Label Body [On|Off| Name [Only|ID] |ID|Interval|Size| Merge |Firmness]
Label Curve [On|Off|Name [Only|ID] |ID| Interval| Size| Merge| Firmness]
Label {Hex|Tet|Face|Tri|Edge} [On|Off|ElementId]
Label Element [On|Off]
Label Geometry [On|Off|Name [Only|ID] |ID| Interval| Size| Merge| Firmness]
Label Mesh [On|Off]
Label Node [On|Off|ElementId|SphereId]
Label Surface [On|Off|Name [Only|ID] |ID| Interval| Scheme| Size| Merge| Firmness]
Label Vertex [On|Off|Name [Only|ID] |ID|Interval| Size| Merge| Firmness]
Label Volume [On|Off|Name [Only|ID] |ID |Interval| Size |Scheme |Merge |Firmness]
The meaning of each of each label type is listed below. Note that some label types don't make sense for every entity type.
On - The same as IDs.
Name - Name of the entity, if the entity has been named. Default name otherwise.
Name Only - If the entity has been named, use the name as the label. Otherwise, don't use a label.
Name IDs - If the entity has been named, use the name as the label. Otherwise, use the ID as the
label.
Interval - The number of intervals set on the entity.
Firmness - Same as interval, but followed by a letter indicating the firmness of the interval setting
(see the Mesh Generation chapter for description of firmness settings.)
Merge - Whether or not the entity is mergeable. Note that this is sometimes not clear, because, for
example, a curve may show that it isn't mergeable because one of its owning surfaces may be
unmergeable, while another owning surface may be mergeable.
Size - The mesh size set on this entity.
ElementId - The Global Element Id of each element. Will only be labeled for hexes, tets, tris, etc.
which are in a block.
SphereId - The id of the sphere element associated with this node, if there is one. A sphere element
is only associated with a node if the node (or it's geometry owner) is put into a block.
115
Trelis 15.0 User Documentation
Note: Three dimensional entity types such as body will have their labels displayed in the center of the entity. Thus, in the
smooth shade and hidden line graphics modes the labels will be hidden
The GUI includes command panels to manipulate the labels settings for any given entity type. The command panel for the
Volumes labels settings is shown below as an example:
116
Colors
Specifying Colors in Commands
There are five ways to refer to a color in a command. They are
1.
2.
3.
4.
5.
<Color_Name>
User "name"
ID <id>
Default
Highlight
The first option uses the name of a pre-defined color as listed in the Available Colors Appendix. This option may not be
used for user-defined colors. An example of a pre-defined color assignment is given below:
color volume 1 lightblue
The second option is used with user-defined colors only. Include the name of the user-defined color in quotes. Pre-defined
colors will not work with this command.
color volume 1 user "mycolor"
The third option allows you to identify a pre-defined color by its ID. The color IDs are also listed in the Available Colors
appendix. This option is rarely used.
color volume 1 id 5
The default option is used to set an entity's color to its default value. The default color may also be specified in drawing
commands, but the command's behavior will be the same as if the color option had not been included at all.
color volume 1 default
The fifth option refers to the current highlight color.
draw curve 1 tangent color highlight
User-Defined Colors
Trelis has a palette of 85 pre-defined colors, listed in the Appendix under Available Colors. Users may also define their
own colors in addition to those defined by Trelis. Each color is defined by a name and by its RGB components, which
range from 0 to 1.
To define an additional color, use either of the commands
Color Define "<name>" RGB <r g b>
Color Define "<name>" R <r> G <g> B <b>.
A maximum of 15 user-defined colors may be stored at one time, so it may be necessary to clear a color definition. This is
done with the command
Color Release "<color_name>"
Color names can be listed with the command
Help Color
117
Trelis 15.0 User Documentation
They are also listed in the appendix of this manual, along with their RGB definitions. To view a chart of color names and
IDs, including those for user-defined colors, use the command
Draw Colortable
Assigning Colors
Colors may be assigned to all geometric entities, and to some other objects as well. To assign a color to an entity or other
object, use one of the following commands.
Color Axis Labels {<color_name>| id <color_id>}
Color Background {<color_name>| id <color_id>} [<color_name2>|id <color_id2>]
Color Block <block_id_range>{<color_name> | id <color_id>}
Color Body <body_id_range> [Geometry|Mesh] {<color_name>| id <color_id> | Default}
Color Curve <curve_id_range> [Geometry|Mesh] {<color_name>| id <color_id> | Default}
Color Group <group_id_range> [Geometry|Mesh] {<color_name>| id <color_id> | Default}
Color Highlight {<color_name>| id <color_id>}
Color Lines <color_name>
Color NodeSet <id_range> { <color_name> | id <color_id> | Default }
Color SideSet <id_range>{ <color_name> | id <color_id> | Default }
Color Surface <surface_id_range> [Geometry|Mesh] {<color_name>|Default}
Color Title {<color_name>|id <color_id>}
Color Volume <volume_id_range> [Geometry|Mesh] {<color_name>| id <color_id> | Default}
Including the Mesh keyword will change the color of the mesh belonging to the specified entity, without changing the color
of the entity geometry itself. Conversely, including the Geometry keyword will change the geometry color without changing
the mesh color. Including both keywords is identical to including neither keyword.
Colors are inherited by child entities. If you explicitly set the color for a volume, for example, all of its surfaces will also be
drawn in that color. Once you assign a color to an entity, however, it will remain that color and will no longer follow color
changes to parent entities. To make an entity follow the color of its parent after having explicitly set another color, use
Default as the color name in the color command.
Colors can also be assigned to nodesets, sidesets, and element blocks. These colors do not take effect, however, unless
the nodeset, sideset, or element block is drawn with a Draw command.
The background color and the color used to draw highlighted entities can be changed to any color.
By default, the axes are labeled with a white X, Y, and Z, indicating the three primary coordinate directions. If the
background is changed to white, these labels are impossible to read; the color used to draw axis labels can be changed to
any color. Changing the axis label color will change the text color for both the model axis and the triad (corner axis).
When several entity types are labeled, it can become difficult to determine which labels apply to which entities. To help
distinguish which entities are being referred to by the labels, you may want to change the color of labels for specific entity
types.
When a meshed surface is drawn in a shaded graphics mode, the mesh edges are not drawn in the same color as the
surface. This is to prevent confusion between mesh edges and geometric curves, and to make the mesh edges more
visible. The color used to draw mesh edges in this situation is known as the line color, and is gray by default; this color
can be changed to any color.
118
Colors
Assigning Global Colors
Colors may be assigned globally also. To assign a global color, use one of the following commands. Global color
assignment is useful if one desires all entities to appear the same.
Color Global {<color_name>| id <color_id> | default}
Color Global Surface {<color_name>| id <color_id> | default} Curve {<color_name>| id <color_id> |
default} Vertex {<color_name>| id <color_id> | default}
The first command assigns the desired color to all geometry entities. The color may be enter by color name or color id.
The default option resets colors to the default value.
The second command assigns the desired colors to surfaces, curves and vertices. All three value must be entered. For
example, users my select global colors for surface and vertex and specify that curves have default colors.
119
Geometry and Mesh Entity Visibility
The visibility of geometric and mesh entities can be turned on or off, either individually, by entity type, by general entity
class (mesh, geometry, etc.), or globally. Note that these commands do not refresh automatically. To refresh type display
or graphics flush or click in the display window.
The commands to set the visibility are:
{ {Body|Curve|Surface|Volume} <range> } [Mesh][Geometry] Visibility [On|Off]
Edge Visibility [On | Off]
Vertex [Visibility] [on|off]
{Mesh|Geometry} { [Visibility] [on|off] }
If the Mesh keyword is included, only the visibility of the mesh belonging to the specified entity is affected. Similarly, if the
Geometry keyword is included, only the visibility of the geometry is affected. Including neither keyword is identical to
using both keywords.
Entity visibility is also controlled via context (right-click) menus in the Tree and in the graphics window.
The GUI tool bar buttons for manipulating geometry and mesh visibility are the following:
Invisibility of geometry is inherited; visibility is not. For example, if a volume is invisible, its surfaces are also invisible
unless they also belong to some other visible volume. As another case, if the volume is visible, but a surface is set to
invisible, the surface will not follow its parent's visibility setting, but will remain invisible.
If edge visibility is off, mesh edges will not be drawn when mesh faces are drawn.
If vertex visibility is turned on, the vertices of the geometry become visible. The default for vertex visibility is off.
After turning mesh visibility off, all mesh will remain invisible until mesh visibility is turned on again. This is true no matter
what other visibility commands are entered.
Similarly, after turning geometry visibility off, all geometry will remain invisible until geometry visibility is turned on again.
This is true no matter what other visibility commands are entered.
121
Graphics Camera
One way to change what is visible in the graphics window is to manipulate the camera used to generate the scene. A
scene camera has attributes described below, and depicted graphically in Figure 1. The values of these camera attributes
determine how the scene appears in the graphics window.
These view settings may be accessed in the GUI via the Display/View Point menu.
Position (From) - The location of the camera in model coordinates.
View Direction (At) - The focal point of the camera in model coordinates.
Up Direction (Up) - The point indicating the direction to which the top of the camera is pointing. The Up point determines
how the camera is rotated about its line of sight.
Projection - Determines how the three-dimensional model is mapped to the two-dimensional graphics window.
Perspective Angle - Twice the angle between the line of sight and the edge of the visible portion of the scene.
Figure 1: Schematic of From, At, Up, and Perspective Angle
At any time, the camera can be moved back to its original position and view using the command
View Reset
To see the current settings of these attributes, use the command
List View
The current value of the view attributes will be printed to the terminal window, along with other useful view information
such as the current graphics mode and the width of the current scene in model coordinates.
Camera Attributes can be changed using the Rotate, Zoom and Pan commands, or directly as follows.
Changing Camera Attributes Directly
Camera attributes are most easily modified using interactive mouse manipulation (see Mouse-Based View Navigation) or
using the rotate, pan and zoom commands. However, the camera attributes can also be modified directly with the
following commands:
From <x y z>
At <x y z>
123
Trelis 15.0 User Documentation
At {Body|Volume|Surface|Curve|Vertex|Hex|Tet|Wedge|Tri|Face|Node}<id_list>
Up <x y z>
Graphics Perspective <On|Off>
Graphics Perspective Angle <degrees>
If graphics perspective is on, a perspective projection is used; if graphics perspective is off, an orthographic projection is
used. With a perspective projection, the scene is drawn as it would look to a real camera. This gives a three-dimensional
sense of depth, but causes most parallel lines to be drawn non-parallel to each other. If an orthographic projection is
used, no sense of depth is given, but parallel lines are always drawn parallel to each other.
In a perspective view, changing the perspective angle changes the field of view by changing the angle from the line of
sight to the edge of the visible scene. The effect is similar to a telephoto zoom with a camera. A smaller perspective angle
results in a larger zoom. This command has no effect when graphics perspective is off.
The GUI tool bar button for changing the graphics perspective mode is as follows:
124
Graphics Lighting Model
For shaded graphics display modes, the lighting model controls the intensity of the highlights and shadows for objects
displayed in the graphics window. Trelis offers two commands for controlling the lighting model.
Graphics Ambient Intensity {<intensity> | <r g b>}
Graphics Light Intensity {<intensity> | <r g b>}
The ambient intensity is the light available in the environment. There is no particular direction to the light source. In
contrast, the light intensity is the effect of a simulated light source placed at the viewer's line of sight. The light intensity
affects the intensity of the highlights and shadows, while the ambient intensity affects the brightness of the objects in the
overall scene.
An intensity value from 0 to 1 can be used, where 0 represents no light and 1 represents maximum. Alternatively r g b
color components can be used. This changes the color of the directional or ambient light source, affecting the resulting
color of the objects in the model.
The GUI Options panel for manipulating these settings is found under Tools/Options and is shown below:
125
Trelis 15.0 User Documentation
126
Graphics Window Size and Position
By default in the command line version, Trelis will create a single graphics window when it starts up (to run Trelis without
a graphics window, include -nographics on the command line when launching Trelis.) The graphics window position and
size is most easily adjusted using the mouse, like any other window on an X-windows screen. However, the size of the
graphics window can also be controlled using the following commands:
Graphics WindowSize <width_in_pixels> <height_in_pixels>
Graphics WindowSize Maximum
Graphics WindowSize Minimum
After using the Graphics WindowSize Maximum and Graphics WindowSize Minimum commands, the previous
window size can be restored by using the command
Graphics WindowSize Restore
The position of the graphics window can also be controlled using the Graphics WindowLocation command.
Graphics WindowLocation <x> <y>
The <x> and <y> coordinates refer to the distance in pixels from the upper left hand corner of the monitor.
In addition, on Unix workstations, the graphics window size and position can be controlled by placing the following line in
the user's .Xdefaults file:
Trelis.graphics.geometry XxY+xpos+ypos
where the X and Y are window width and height in pixels, respectively, and xpos and ypos are the offsets from the upper
left hand corner.
Using Multiple Windows
You can use up to ten graphics windows simultaneously, each with its own camera and view. Each window has an ID,
from 1 to 10, shown in the title bar of the window. Commands that control camera attributes apply to only one window at a
time, the active window. Currently, the display lists of all windows are identical.
The following commands are used to create, delete, and make active additional graphics windows. These commands are
also valid in the GUI (by typing at the command line prompt.)
Graphics Window Create [ID]
Graphics Window Delete <ID>
Graphics Window Active <ID>
127
Saving Graphics Views
The current graphics view can be saved and restored using the following commands:
View Save Position <n>
View Restore Position <n>
When you save a view, you save the camera settings in effect at the time the command is issued. When you restore the
view, the camera is returned to the saved position, orientation, and field of view.
If autocenter is on at the time you save the view, then restoring the view will automatically adjust the camera settings to
center on the entire model and fit the entire model on the screen, a lot like "zoom reset." You turn autocenter on by typing
"graphics autocenter on."
Example of how to save a top view:
at 0
from 0 1 0
up 1 0
graphics autocenter on
view save position 3
Use this command to restore that view:
view restore position 3
The view will then be looking down the y-axis, with the x-axis to the top and the z-axis to the right. The model will be
centered in the view and zoomed so that everything just fits into the graphics window. This is true even if the model is not
centered on the origin.
If autocenter is off when the "view save" command is issued, the camera is not adjusted to fit the scene into the graphics
window. Instead, it is placed exactly where it was at the time the "save" command was issued.
Note that many graphics commands, such as "at", "from", and "up", do not change what appears in the graphics window
until a "display" command is issued. They do, however, take immediate effect internally, and they do affect what is saved
by the "view save" command.
In the command line version of Trelis, you can save a view by holding down the shift key and pressing one of the function
keys (F1-F12). Each function key corresponds to a different saved view. A total of 12 views can be saved. A view can be
restored at a later time by pressing the appropriate function key WITHOUT holding down the shift key.
It may be useful to save views in your Trelis file so that they are available every time you run Trelis. Use Trelis to save
front, top, and side views in positions 1, 2, and 3. If views are saved in your Trelis file, it is convenient to add a "view
reset" command after the views have been saved. Then the graphics will initially appear as they would if the view
commands had not been included in your Trelis file.
129
Hardcopy Output
Trelis' Graphical User Interface provides the capability to print the contents of the graphics window directly to a
printer. Use File/Export/Screen Shot to access this functionality.
In addition, a command line option is provided for dumping the contents of the graphics window to postscript or image
files.
The command for generating hardcopy output files is:
Hardcopy '<filename>' {jpg | gif | bmp | pnm | tiff | eps} [Window <window_id>]
Each of these options saves the view in the specified window (or the current window), to the specified file, in the format
indicated. The file can then be sent to a printer or inserted into another document.
Screen Capture Programs
It should also be noted that many commercial applications are available for capturing screen images. In many cases,
these applications may be more convenient for interactively capturing and saving a portion of the screen than the
Hardcopy command discussed above. On UNIX platforms, the XV utility written by John Bradley is a good choice. In
some cases this utility or its equivalent may be included with your system software. For Windows users, the Print Screen
button will send a copy of the screen to the clipboard which can then be pasted into a paint program.
131
Miscellaneous Graphics Options
In addition to the commands discussed above, there are several other graphics system options in Trelis that can be
controlled by the user.
They include:
•
•
•
•
•
•
•
•
•
•
•
•
Silhouette Lines
Line Width
Highlight Line Width
Text Size
Point Size
Graphics Status
Graphics Scale
Model Axis
Corner Axis
Resetting the Graphics
Shrink
Facet Tolerance
Silhouette Lines
Some shapes, such as cylinders, are drawn with silhouette lines; these lines don't represent true geometric curves, but
help visualize the shape of a surface. Silhouette lines can be turned on or off with the command
Graphics Silhouette [On|Off]
The pattern used to draw silhouette lines can be set using the command
Graphics Silhouette Pattern [Solid | Dashdot | Dashed | Dotted | Dash_2dot | Dash_3dot | Long_dash
| Phantom]
Line Width
This option controls the width of the lines used in the wireframe, shaded, transparent, hiddenline and truehiddenline
displays. The default is 1 pixel wide. The command to set the line width is
Graphics LineWidth <width_in_pixels>
Highlight Line Width
This option controls the width of the lines used when highlighting an entity. Setting this to a width greater than the global
line width often makes it easier to locate highlighted entities. If this setting has not been changed, the line width set in the
command above is used. After using this command, it is necessary to refresh the graphics by either typing "display" or
clicking the Refresh Graphics button. The command to set the highlighting line width is
Highlight LineWidth <width_in_pixels>
133
Trelis 15.0 User Documentation
Text Size
This option controls the size of text drawn in the graphics window. The size given in this command is the desired size
relative to the default size. After using this command, it is necessary to refresh the graphics by either typing "display" or
clicking the Refresh Graphics button. The command to set the text size is
Graphics Text Size <size>
Point Size
This option controls the size of points drawn in the graphics window, such as vertices or heads of vectors; alternatively,
the size of points representing nodes or vertices can be set independently of the global point size. The commands to set
the point sizes are
Graphics Point Size <size>
Graphics [Node|Vertex] Point Size <size>
Graphics Status
All graphics commands can be disabled or re-enabled with the command
Graphics {On|Off}
While graphics are off, changes in the model will not appear in the graphics window, and all graphics commands will be
ignored. When graphics are again turned on, the scene will be updated to reflect the current state of the model.
Graphics Scale
A graphical scale can be drawn in the graphics window within the viewing area to obtain a bearing on model or part sizes.
The command to turn the graphical scale on and off is:
Graphics Scale [On|Off]
Model Axis
The model axis may be drawn in the scene at the model origin. The axis is controlled with the command
Graphics Axis [Type <AXIS | Origin>] [On|Off]
The command is used to specify whether the model axis is visible, and to determine how the axis is drawn. If you include
Type Axis , the axis will be drawn as three orthogonal lines; if you include Type Origin, the axis will be drawn as a circle at
the model origin.
Corner Axis (Triad)
By default, an axis appears in the corner of the graphics window. This corner axis, also called the triad, can be disabled or
re-enabled with the command
Graphics Triad [On | Off]
134
Miscellaneous Graphics Options
Resetting the Graphics
Many of the graphic options can be reset back to default values with the command:
Graphics Reset
The graphic options set to defaults are:
•
•
•
•
•
•
•
ambient and spot light intensity
background color
text size
graphics mode
silhouetting
point size
view type (Perspective)
In addition, this command also:
•
•
•
•
•
centers the view on all visible entities (Zoom Reset)
turns all labeling off
turns vertex visibility off
turns mesh and geometry visibility on
moves the graphics camera back to its original position (View Reset)
Shrink
The shrink graphics attribute allows you to view the elements shrunken about their centroid. This is useful for viewing 3D
meshes, permitting viewing of interior elements. It may also be useful for visually inspecting the mesh for missing
elements. To use the shrink option use:
graphics shrink <value>
draw hex <range>
draw tet <range>
etc...
where value is a number between 0 and 1. One (1) will shrink the elements to a point, while zero (0) will not shrink the
elements. The following figures illustrate the effect of element shrink on a hex mesh.
135
Trelis 15.0 User Documentation
Figure 1. Top: shrink=0.2, Bottom: shrink=0.5
Facet Tolerance
The graphics tolerance commands change the way that facets are drawn in the graphics window. It does not affect the
underlying geometry, just the graphics display. It can be useful to change the facet tolerance on large models if the
refresh speed is slow.
Graphics Tolerance [ [ANGLE|Distance] <val>|Default ]
136
Miscellaneous Graphics Options
Specifying an angle will change the maximum allowable angle between neighboring facets. The distance option will set a
maximum distance between adjacent facets. Increasing either of these numbers will result in coarser facets. The default
option will return values to their default settings.
The GUI Options panel for manipulating these settings is found under Tools/Options and is shown below:
137
Command Line Entity Specification
Trelis identifies objects in the geometry, mesh, and elsewhere using ID numbers and sometimes names. IDs and names
are used in most commands to specify which objects on which the command is to operate.
These objects can be specified in Trelis commands in a variety of ways, which are best introduced with the following
examples (the portion of each command which specifies a list of entities is shown in blue):
General ranges: Surface 1 2 4 to 6 by 2 3 4 5 Scheme Pave
Combined geometry, mesh, and genesis entities: Draw Sideset 1 Curve 3 Hex 2 4 6
Geometric topology traversal: Vertex in Volume 2 Size 0.3
Mesh topology traversal: Draw Edge in Hex 32
All keyword: ListBlock all
Expand keyword: my_curve_group expand Scheme Bias Factor 1.5
Except keyword: List Curve 1 to 50 except 2 4 6
In addition to the examples above, there is an extended parsing capability that allows entities to be specified by a general
set of criteria. See Extended Entity Specification for details. The following is a simple example of an extended entity
specification:
By Criteria: Draw Curve With Length > 3
Types of Entity Range Input
The types of entity range input available in Trelis can be classified in 4 groups:
1.
General range parsing
Entity IDs can be entered individually (volume 1), in lists (volume 1 2 3), in ranges (volume 3 to 7), and in
stepped ranges (volume 3 to 7 step 2). The word all may also be used to specify all entities of a given type.
An ID range has the form <start_id> to <end_id>. It represents each ID between start_id and end_id, inclusive.
A stepped ID range has the form <start_id> To <end_id> {Step|By} <step>. It represents the set of IDs
between start_id and end_id, inclusive, which can be obtained by adding some integer multiple of step to
start_id. For example, 3 to 8 step 2 is equivalent to 3 5 7.
The various methods of specifying IDs can be used together. For example:
draw surface 1 2 4 to 6 vertex all
2.
Topological traversal
Topological traversal is indicated using the "in" identifier, can span multiple levels in a hierarchy, and can go
either up or down the topology tree. For example, the following entity lists are all valid:
vertex in volume 3
volume in vertex 2 4 6
curve 1 to 3 in body 4 to 8 by 2
If ranges of entities are given on both sides of the "in" identifier, the intersection of the two sets results. For
example, in the last command above, the curves that have ids of 1, 2 or 3 and are also in bodies 4, 6 and 8 are
used in the command.
Topology traversal is also valid between entity types. Therefore, the following commands would also be valid:
139
Trelis 15.0 User Documentation
draw node in surface 3
draw surface in edge 362
draw hex in face in surface 2
draw node in hex in face in surface 2
draw edge in node in surface 2
3.
Exclusion
Entity lists can be entered then filtered using the "except" identifier. This identifier and the ids following it apply
only to the immediately preceding entity list, and are taken to be the same entity type. For example, the
following entity lists are valid:
curve all except 2 4 6
curve 1 2 5 to 50 except 2 3 4
curve all except 2 3 4 in surface 2 to 10
curve in surface 3 except 2 (produces empty entity list!)
4.
Group expansion
Groups in Trelis can consist of any number of geometry entities, and the entities can be of different type (vertex,
curve, etc.). Operations on groups can be classified as operations on the group itself or operations on all
entities in the group. If a group identifier in a command is followed immediately by the `expand' qualifier, the
contents of the group(s) are substituted in place of the group identifier(s); otherwise the command is interpreted
as an operation on the group as a whole. If a group preceding the `expand' qualifier includes other groups, all
groups are expanded in a recursive fashion.
For example, consider group 1, which consists of surfaces 1, 2 and curve 1. Surfaces 1 and 2 are bounded by
curves 2, 3, 4 and 5. The commands in Table 1, illustrate the behavior of the `expand' qualifier.
Table 1. Parsing of group commands; Group 1 consists of Surfaces 1-2 and Curve 1; Surfaces 1 and 2 are
bounded by Curves 2-5.
Command
Entity list produced
Curve in Group 1
Curve 1
Curve in group 1 expand
Curves 1, 2, 3, 4, 5
The `expand' qualifier can be used anywhere a group command is used in an entity list; of course, commands which apply
only to groups will be meaningless if the group id is followed by the `expand' qualifier.
Precedence of "Except" and "In"
Several keywords take precedence over others, much the same as some operators have greater precedence in coding
languages. In the current implementation, the keyword "Except" takes precedence over other keywords, and serves to
separate the identifier list into two sections. Any identifiers following the "Except" keyword apply to the list of entities
excluded from the entities preceding the "Except". Table 2 shows the entity lists resulting from selected commands.
Table 2. Precedence of "Except" and "In" keywords; Group 1 consists of Surfaces 1-2 and Curve 1.
Command
Entity list produced
Curve all except 1 in Group 1
(All curves except curve 1)
140
Command Line Entity Specification
Curve all except 2 3 4 in Surf 2 to 10
(All curves except 2, 3, 4)
In the first command, the entities to be excluded are the contents of the list "[Curve] 1 in Group 1", that is the intersection
of the lists "Curve 1" and "Curve in Group 1"; since the only curve in Group 1 is Curve 1, the excluded list consists of only
Curve 1. The remaining list, after removing the excluded list, is all curves except Curve 1.
In the second command, the excluded list consists of the intersection of the lists "Curve 2 3 4" and "Curve in Surf 2 to 10";
this intersection turns out to be just Curves 2, 3 and 4. The remaining list is all curves except those in the excluded list.
Placement in Trelis Commands
In general, anywhere a range of entities is allowed, the new parsing capability can be used. However, there can be
exceptions to this general rule, because of ambiguities this syntax would produce. Currently, the only exception to this rule
is the command used to define a sideset for a surface with respect to an owning volume.
141
Entity Selection
•
•
•
Command Line Entity Specification
Extended Command Line Entity Specification
Selecting Entities With the Mouse
Trelis Entity specification is a means of selecting objects or groups of objects. Entities can be selected from the command
line using entity specification parameters, or directly in the graphics window using the mouse. This chapter describes
these methods of entity selection.
143
Environment Control
•
•
•
•
•
•
•
Session Control
Graphical User Interface
Command Recording and Playback
Graphics Window Control
Entity Selection and Filtering
Location, Direction, and Axis Specification
Listing Information
The Trelis user interface is designed to fill multiple meshing needs throughout the design to analysis process. The user
interface options include a full graphical user interface, a modern command line interface as well as no-graphics and
batch mode operation. This chapter covers the interface options as well as the use of journal files, control of the graphics,
a description of methods for obtaining model information, and an overview of the help facility.
145
Extended Command Line Entity Specification
In addition to basic entity specification, entities may be specified using an extended expression. An extended expression
identifies one or more entities using a set of entity criteria. These criteria describe properties of the entities one wishes to
operate upon.
Extended Parsing Syntax
The most common type of extended parsing expression is in the following format:
{Entity_Type} With {Criteria}
Entity_Type is the name of any type of entity that can be used in a command, such as Curve, Hex, or SideSet. Criteria is
a combination of entity properties (such as Length), operators (such as >=), keywords (such as Not), and values (such as
5.3) that can be evaluated to true or false for a given entity. Here are some examples:
curve with length <1
surface with is_meshed = false
node with x_coord > 10 And y_coord > 0
Keywords
These are the keyword defined by extended parsing
Keyword
Description
These keywords are used the same way as in basic entity specification. For
example:
draw surface all
All, To, Step, By, Except, In,
Expand
draw surface 1 to 5 step 2 curve 1 to 3 in body 4 to 8 by 2
draw hex in face in surface 2
draw node in hex in face in surface 2 curve 1 2 5 to 50 except 2 3 4
Not
Not flips the logical sense of an expression - it changes true to false and false to
true. For example:
draw surface with not is_meshed
Of
The "of" operator is used to get an attribute value for a single entity, such as
"length of curve 5". Only attributes that return a single numeric value may be
used in an "of" expression. There must be only one entity specified after the "of"
operator, but it can be identified using any valid entity expression. An example of
a complete command which includes the "of" operator is:
list curve with length < length of curve 5 ids
These logic operators determine how multiple criteria are combined.
And, Or
draw surface with length > 3 or with is_meshed = false
< > <= >= = <>
These relational operators compare two expressions. You may use = or == for
"equals". <> means "not equal". For example:
147
Trelis 15.0 User Documentation
draw surface with x_max <= 3
draw volume with z_max <>12.3
These arithmetic operators work in the traditional manner.
+ - * /
draw surface with length * 3 + 1.2 > 10
()
Parentheses are used to group expressions and to override precedence. When
in doubt about precedence, use parentheses.
draw surface with length > 3 and ( with is_meshed = false or x_min > 1 )
Functions
The following functions are defined. Not all functions apply to all entities. If a function does not apply to a given entity, the
function returns 0 or false.
Keyword
Description
ID
the ID of an entity
Length
The length of a curve or edge
Area
The area of a surface.
Exterior_Angle
Works for curves with an exterior angle greater than (>), less than (<), or equal to
(=) a given angle in degrees. This is used if you want to do some operation, such
as refinement, on all the reentrant curves or curves with surfaces that form a
certain angle.
Is_Meshed
Whether a geometric entity has been meshed or not
Is_Spline
Whether a geometric entity is defined using a NURBS representation. Otherwise
the entity has an analytic representation.
Is_Plane
Whether a geometric surface is planar.
Is_Periodic
Whether a geometric surface is periodic, such as a sphere or torus.
Is_Sheetbody
A geometric entity is a sheetbody if it is a collection of surfaces that do not form a
solid.
Element_Count
The number of elements owned by this geometric entity. Only elements of the
same dimension as the entity are counted (number of hexes in a volume, number
of faces on a surface, etc.)
Dimension
The topological dimension of an entity (3 for volumes, 2 for surfaces, etc.).
X_Coord, Y_Coord, Z_Coord The x, y, or z coordinate of the point at the center of the entity's bounding box.
X_Min, Y_Min, Z_Min
The x, y, or z coordinate of the minimum extent of the entity's bounding box
X_Max, Y_Max, Z_Max
The x, y, or z coordinate of the maximum extent of the entity's bounding box
Is_Merged
148
Whether a geometry entity has a merge flag on. All geometric entities have one
Extended Command Line Entity Specification
set by default.
Is_Virtual
A flag that specifies whether an entity is virtual geometry. An entity is virtual if it
has at least one virtual (partition/composite) topology bridge.
Has_Virtual
An entity "has_virtual" if it is virtual itself, or has at least one child virtual entity
Is_Real
An entity "is_real" if it has at least one real (non-virtual) topology bridge.
Num_Parents
Used to specify geometry entities with a specified number of parent entities. May
be used to find "free curves" where num_parents=0 or non-manifold curves
where num_parents>2.
Precedence
For complicated expressions, which entities are referred to is influenced by the order in which portions of the expression
are evaluated. This order is determined by precedence. Operators with high precedence are evaluated before operators
with low precedence. You may always include parentheses to determine which sub-expressions are evaluated first. Here
all operators and keywords listed from high to low precedence. Items listed together have the same precedence and are
evaluated from left to right.
(, ) Expand Not *, / +, - <, >, <=, >=, <>, = And, Or Except In Of With
Because of precedence, the following two expressions are identical:
curve with length + 2 * 2 > 10 and length <= 20 in my_group
expand(curve with (((length + (2*2)) > 10 )and( length <= 20 ))) in ( my_group expand )
149
Selecting Entities with the Mouse
The following discussion is applicable only to the command line version of Trelis. See GUI Entity Selection for a
description of interactive entity selection with the Graphical User Interface.
Many of the commands in Trelis require the specification of an entity on which the command operates. These entities are
usually specified using an object type and ID (see Entity Specification) or a name. The ID of a particular entity can be
found by turning labels on in the graphics and redisplaying; however, this can be cumbersome for complicated models.
Trelis provides the capability to select with the mouse individual geometry or mesh entities. After being selected, the ID of
the entity is reported and the entity is highlighted in the scene. After selecting the entities, other actions can be performed
on the selection. The various options for selecting entities in Trelis are described below, and are summarized in Table 1:
Table 1. Picking and key press operations on the picked entities
Key
ctrl +
B1
shift +
ctrl +
B1
tab
Action
Pick entity of the current picking type.
Add picked entity of the current picking type to current picked entity list.
Query-pick; pick entity of current picking type that is below the last-picked entity.
n
Lists what entities are currently selected.
l
Lists basic information about each selected entity. This is similar to entering a List
command for each selected entity.
g
Lists geometric information about the selection. As if the List Geometry command were
issued for each entity. If there are multiple entities selected, a geometric summary of all
selected entities is printed at the end, including information such as the total bounding box
of the selection.
i
Makes the current selection invisible. This only affects entities that can be made invisible
from the command line (i.e. geometric entities.)
s
Draws a graphical scale showing model size in the three coordinate axes. This is a toggle
action, so pressing the 's' key again in the graphics window will turn the scale off.
151
Trelis 15.0 User Documentation
ctrl + z
Zoom in on the current selection.
e
Echo the ID of the selection to the command line.
a
Add the current selection to the picked group. Only geometry will be added to the group
(not mesh entities). If a selected entity is already in the picked group, it will not be added a
second time.
r
Remove the current selection from the picked group. If a selected entity was not found in
the picked group, this command will have no effect.
ctrl + r
Redisplays the model.
c
Clear the picked group. The picked group will be empty after this command.
m
Lists what entities are currently in the picked group.
d
Display and select the entities in the picked group.
ctrl + d
Draws the entity that is selected.
Details of selecting entities with a mouse are outlined in the following items:
•
•
•
•
•
•
Entity Selection
Query Selection
Multiple Selected Entities
Information about the Selection
Picked Group
Substituting the Selection into Commands
Entity Selection
Selecting entities typically involves two steps:
1. Specifying the type of entity to select
Clicking on the scene can be interpreted in more than one way. For example, clicking on a curve could be intended to
select the curve or a mesh edge owned by that curve. The type of entity the user intends to select is called the picking
type. In order for Trelis to correctly interpret mouse clicks, the picking type must be indicated. This can be done in one of
two ways. The easiest way to change the picking type is to place the pointer in the graphics window and enter the
dimension of the desired picking type and an optional modifier key. The dimension usually corresponds to the dimension
of the objects being picked:
152
Selecting Entities with the Mouse
Table 2. Picking Modes in Graphics Window
Number
Default pick
Number +shift pick
0
vertices
nodes
1
curves
edges
2
surfaces
all 2D elements
3
volumes
all 3D elements
4
bodies
If a Shift modifier key is held while typing the dimension, the picking type is set to the mesh entity of corresponding
dimension, otherwise the geometry entity of that dimension is set as the picking type. For example, typing 2 while the
pointer is in the graphics window sets the picking type so that geometric surfaces are picked; typing Shift-1 sets the
picking type so that mesh edges are picked. To differentiate between picking "tris" or "quads" use "pick face" or "pick tri"
The picking type can also be set using the command
Pick <entity_type>
where entity_type is one of the following: Body , Volume , Surface , Curve , Vertex , Hex , Tet , Face , Tri , Edge , Node ,
or DicerSheet .
2. Selecting the entities
To select an object, hold down the control key and click on the entity (this command can be mapped to a different button
and modifiers, as described in the section on Mouse-Based View Navigation). Clicking on an entity in this manner will first
de-select any previously selected entities, and will then select the entity of the correct type closest to the point clicked.
The new selection will be highlighted and its name will be printed in the command window.
Query Selection
If the highlighted entity is not the object you intended to selected, press the Tab key to move to the next closest entity.
You can continue to press tab to loop through all possible selections that are reasonably close to the point where you
clicked. Shift-Tab will loop backwards through the same entities.
Multiple Selected Entities
To select an additional entity, without first clearing the current selection, hold down the shift and control keys while clicking
on an object. You can select as many objects as you would like. By changing the picking type between selections, more
than one type of entity may be selected at a time. When picking multiple entities, each pick action acts as a toggle; if the
entity is already picked, it is "unpicked", or taken out of the picked entities list.
Information About the Selection
When an entity is selected, its name, entity type, and ID are printed in the command window. There are several other
actions which can then be performed on the picked entity list. These actions are initiated by pressing a key while the
pointer is in the graphics window. Table 1 summarizes the actions which operate on the selected entities.
Picked Group
There is a special group whose contents can be altered using picking. This group is named picked , and is automatically
created by Trelis. Other than its relationship to interactive picking, it is identical to other groups and can be operated on
from the command line. Like other groups, both geometric and mesh entities can be held in the picked group. Table 1 lists
the graphics window key presses used with the picked group.
153
Trelis 15.0 User Documentation
Note: It is important to distinguish between the current selection and the picked group contents. Clicking on a new entity
will select that entity, but will not add it to the picked group. De-selecting an entity will not remove an entity from the picked
group.
Substituting Selection into Other Commands
There are three ways to use mouse-based selection to specify entities in commands.
1. The Selection Keyword
You may refer to all currently selected entities by using the word selection in a command; the picked type and ID numbers
of all selected entities will be substituted directly for selection . For example, if Volume 1 and Curve 5 are currently
selected, typing
Color selection Blue
is identical to typing
Color Volume 1 Curve 5 Blue
Note that the selection keyword is case sensitive, and must be entered as all lowercase letters.
2. Echoing the ID of the Selection
Typing an e into a graphics window will cause the ID of each selected entity to be added to the command line at the
current insertion point. This is a convenient way to use entities of which you don't already know the name or ID.
As an added convenience, the picking type can be set based on the last word on the command line using the ` key. Note
that this is not the apostrophe key, but rather the left tick mark, usually found at the upper-left corner of the keyboard on
the same key as the tilde (~). For example, a convenient way to set the meshing scheme of a cylinder to sweep would be
as follows:
Volume (hit `, select cylinder, hit e) Scheme Sweep Source Surface (hit `, select endcap, hit e) Target
(select other endcap, hit e)
The result will be something similar to
Volume 1 Scheme Sweep Source Surface 1 Target 2
Notice that you must use the word Surface in the command, or ` will not select the correct picking type.
3. Using the Picked Group in Commands
Like other groups, the picked group may be used in commands by referring to it by name. The name of the picked group
is picked. For example, if the contents of the picked group are Volume 1 and Volume 2, the command
Draw picked
is identical to
Draw Volume 1 Volume 2
Note that picked is case sensitive, and must be entered as all lowercase letters.
154
Selecting Entities with the Mouse
155
Specifying a Location
Some commands require a specified location or point (such as create curve spline) for the command. A location is
basically an x-y-z position in the model. The following options determine a location specification:
•
•
•
•
•
•
•
•
•
•
•
•
•
[Position] <xval yval zval>
Last
[At] {Node|Vertex} <id_list>
[On] Curve <id_list> [location on curve options]
[On] Surface <id_list> [Close_To | At Location {options} | CENTER]
[On] Plane <options> [Close_To | At Location {options}]
Center Curve <id_list>
Extrema {Curve|Surface|Volume|Body|Group} <range> [Direction] {options} [Direction {options}] [Direction
{options}]
Fire Ray Location {options} Direction {options} At {Body|Volume|Surface|Curve|Vertex} <ids> [Maximum Hits
<val>] [Ray Radius <val>]
Between { Location <options> Location <options>} | { Location <options> Project {Curve|Surface} <id> } [Stop]
[Fraction <val>] }
[Move [all] {<xval yval zval> | {Dx|X|Dy|Y|Dz|Z} <val> | Direction {options} Distance <val>} ]
[Swing [all] [About] Axis {options} Angle <ang>]
Multiple Location Specification
Position (XYZ values)
[Position] <xval yval zval>
The most basic way to specify a location is to just give the xyz values of the location. In this case the following two
commands both draw a location at the coordinates (1, 2, 3), as the Position keyword is optional:
draw location position 1 2 3
draw location 1 2 3
Last Location Used in a Command
Last
The last option recalls the last location used in a command. For example, if the following command is entered after the
above position commands a location would be drawn at the position (1, 2, 3).
draw location last
Last locations do not carry over from Trelis session to Trelis session. The last location defaults to (0, 0, 0) if no location
has been used during the session.
Node or Vertex
[At] {Node|Vertex} <id_list>
Referring to a node or vertex simply returns the coordinates of that node or vertex. The command can also handle
multiple locations where multiple locations are needed to complete the command string. The following draws a location at
the coordinates of Vertex 5:
157
Trelis 15.0 User Documentation
draw location vertex 5
On a Curve
Various options are available to specify a location on a curve. See the section Specifying a Location On a Curve for
details.
On a Surface
[On] Surface <id_list> [Close_To | At Location {options} | CENTER]
If a surface is used to specify a location without other options, the geometrical center of the surface is found (the center
keyword is optional - the default). Otherwise, you can specify another general location and that location is projected to the
surface. For example, the following command will draw the location that is position (5,0,0) projected to surface 1:
draw location on surface 1 location 5 0 0
Any valid location options listed on this page can be used to specify the location that is projected to the surface.
On a Plane
[On] Plane <options> [Close_To | At Location {options}]
A location can be defined at the closest point on a plane to a location. See Specifying a Plane for plane options.
Center
Center Curve <id_list>
Finds the center of an arc - an error is returned if the curve is not an arc.
Extrema
Extrema {Curve|Surface|Volume|Body|Group} <range> [Direction] {options} [Direction {options}]
[Direction {options}]
The extrema option returns the location of the maximum value, on the specified entity or group, in the specified direction.
For example, the following places a vertex on a surface at the point of maximum y-axis value.
create vertex location extrema surf 1 direction y
Fire Ray
The fire ray command allows a user to identify a location, or set of locations, on an object by firing a ray at the object and
determining the intersections. A ray can be fired at a list of bodies, volumes, surfaces, curves, or vertices. The fire ray
command is:
158
Specifying a Location
Fire Ray Location {options} Direction {options} At {Body|Volume|Surface|Curve|Vertex} <ids>
[Maximum Hits <val>] [Ray Radius <val>]
The location options are described on this page. The direction options are described under Specifying a Direction. The
user can specify the maximum number of hits that he wishes to receive back from the command. If this value is omitted,
the command will return all intersections found. When firing a ray at a curve, a ray radius must be used. The ray radius is
the distance from the curve the ray must be to be considered a "hit." If no ray radius is used, the geometry engine default
is used.
Between
Between {Location <options> Location <options> } | {Location <options> Project {Curve|Surface}
<range>} [Stop] [Fraction <val>]}
The between option finds a location that is between two locations or a location and an entity. An optional fraction can be
given to specify the fractional distance from the first location to the second location or entity. For example, the following
will draw a location at (5, 0, 0):
draw location between location 0 0 0 location 10 0 0
The following will draw a location at (2.5, 0, 0) - 25% of the distance from (0, 0, 0) to (10, 0, 0):
draw location between location 0 0 0 location 10 0 0 fraction .25
The second item can be an entity:
draw location between location 0 0 0 vertex 2
draw location between location 0 0 0 surface 1
In the second case, location (0, 0, 0) is projected to surface 1, then the location that is between (0, 0, 0) and the projected
location is found.
Of course, any valid location can be used in the command. In the following example a location at the top center of the
brick is found:
brick x 10
draw location between location bet vert 3 vert 2
location bet vert 8 vert 5
The first location is between vertices 3 and 2, and the second location is between vertices 8 and 5.
Note: you can "swing" a location about an axis, "rotate" a direction about another direction, "revolve" an axis about
another axis and "spin" a plane about an axis. The only reason Trelis needs to use different keywords for each entity type
is because the Trelis command language does not support expressions (as in using parentheses). The keyword stop is
also used in the location/direction/axis/plane parsing as a partial workaround to this limitation. Using this stop keyword will
aid in parsing out extended location specifications. Insert a stop after the first location to let the parser know that where
the specifications begin and end.
Move
Move [All] { <xval yval zval> | {Dx|X|Dy|Y|Dz|Z} <val> | Direction {options} Distance <val> }
Any location can be optionally moved either a xyz distance or a certain distance in a given direction. As many moves as
desired can be strung together. For example, the following will return a location at (5, 0, 0):
159
Trelis 15.0 User Documentation
draw location 0 0 0 move 5 0 0
These examples add another move that basically moves the location (5, 0, 0) in a direction 45 degrees up and to the right
a distance of 10 (all three commands are equivalent - see sections on directions and rotations):
draw location 0 0 0 move 5 0 0 move {10*sind(45)} {10*sind(45)} 0
draw location 0 0 0 move 5 0 0 move direction 1 1 0 distance 10
draw location 0 0 0 move 5 0 0 move direction 1 0 0 rotate about 0 0 1 angle 45 dist 10
Swing
Swing [All] [About] Axis {options} Angle <ang>
Any location can be "swung" (rotated) about an axis by a certain angle. (See the section on specifying an axis for the axis
syntax). As with moves, multiple swings can be strung together. The following example rotates the location (2.5, 5, 5)
thirty degrees about an axis defined by Curve 11. Note that the right-hand rule is used to determine the direction of the
swing about the axis.
draw location 2.5 5 5 swing about axis curve 11 angle 30
Figure 1 - Swinging a Location
Multiple Location Specification
Location {options} Location {options}...
Multiple location specifications can be used in a single command. For example, the following command uses several
locations to create a spline curve at points (0,0,0), (1,2,3), (4,5,6), and (7,8,9).
create curve spline location 0 0 0 location 1 2 3 location 4 5 6 location 7 8 9
Previewing a Location
Sometimes it is advantageous to preview a location before using it in a command. A location can be previewed with the
Draw command. All of the options that can be used to specify locations in a command can be used to preview locations
as well. See above for a description of these options. The command syntax is:
160
Specifying a Location
Draw Location {options}
161
Specifying a Location on a Curve
Some commands require you to specify a location on a curve (i.e., webcutting with a plane normal to a curve). The
following are the options for specifying a location (or locations in the case of the segment option) on a curve:
•
•
•
•
•
•
•
•
•
{MIDPOINT|Start|End}
Arc Center
Fraction <val 0.0 to 1.0> [From Vertex <id> | Start|End]
Distance <val> [From {Vertex|Curve|Surface} <id> | Start | End ]
{{Close_To|At} Location {options} | Position <xval><yval><zval> | {Node|Vertex} <id>}
Extrema [Direction] {options} [Direction {options}] [Direction {options}]
Segment <num_segs>
Crossing {Curve|Surface} <id_list> [Bounded|Near]}
Previewing a Location
Arc Center
arc_center
The arc center option helps in identifying the location at the center of a given arc. Example: create vertex location on
curve 3 arc_center
Start, Midpoint, or End
{ MIDPOINT | Start | End |
These options simply specify the location that is the midpoint, start or end point of a curve. By default, the midpoint is the
understood location unless another location is specified.
Fraction
Fraction <val 0.0 to 1.0> [From Vertex <id> | Start|End] |
The fraction option simply finds the location that is a fractional distance along the curve. By default, the fraction references
the start of the curve; however, you can optionally specify which vertex to reference from.
Distance
Distance <d> [From {Vertex|Curve|Surface} <id> | Start | End ] |
The distance option not only can find a location that is a certain distance along the curve from the start or end of the
curve, but can also find a location (or locations if there is more than one solution) on a curve that is a specified distance
from another curve or a surface. If the From Curve option is used both curves must lie in the same plane.
draw location on curve 13 distance 7 from curve 2
163
Trelis 15.0 User Documentation
Figure 1 - Location on a Curve a Distance from Another Curve
{Close_To|At} Location
{{Close_To|At} Location {options} | Position <xval><yval><zval> |{Node|Vertex} <id>} |
These options take a location closest to the location on the curve.
Extrema
Extrema [Direction] {options} [Direction {options}] [Direction {options}]
The extrema option finds the maximum value location along a curve in a specified direction. For example:
create vertex location on curve 1 extrema ny
Creates a vertex on curve 1 at the location where the y axis value of the curve is at a minimum.
Segment
Segment <num_segs>
The segment option finds locations spaced evenly along the curve such as to break the curve into equal length
"segments" (of course the curve is not modified). You must specify a minimum of two segments (if two segments were
specified a location would be found at the center of the curve). The following example results in 4 locations:
draw location on curve 1 segment 5
create vertex on curve 1 segment 5
164
Specifying a Location on a Curve
Figure 2 - Five Segments on a Curve
Crossing
Crossing {Curve|Surface} <id_list> [Bounded|Near]}
The crossing option finds locations at the intersection of the curve and another curve or surface. By default, the curve(s)
and surface are extended to infinity and the intersections are calculated; if the bounded option is specified only
intersections that lie on the bounded entities will be returned. The near option is valid only for two linear curves. If near is
specified the nearest location between the two linear curves will be returned.
Previewing a Location on a Curve
A location on a curve can be previewed with the Draw command. All of the options that can be used for specifying a
location on a curve can be used to preview a location on a curve. See above for a description of these options. The
command syntax is:
Draw Location On Curve <curve id> {options}
165
Specifying a Direction
Some commands require a specified a direction or vector for the command. A direction is basically a xyz vector in the
model. The following options determine a direction specification:
•
•
•
•
•
•
•
•
•
[Vector] <xval yval zval>
Last
X|Y|Z|Nx|Ny|Nz
[On] | [Tangent] [At] Curve <id> {location on curve options}
[On] | [Normal] [At] Surface <id> [Location {options}]
[From] { Location {options} | {Node|Vertex} <id> }[Project] {Location {options} | [Entity]
{Node|Vertex|Curve|Surface} <id> }
[Rotate {options}]
[Cross [With] Direction {options}]
[Reverse]
Vector (XYZ values)
[Vector] <xval yval zval>
The most basic way to specify a direction is to just give the vector x-y-z components of the direction. The given vector
need not be a unit vector. The following three commands simply draw a direction in the x-direction (1, 0, 0) as the Vector
keyword is optional and unit vectors are not required:
draw direction vector 1 0 0
draw direction 1 0 0
draw direction 10 0 0
Last Direction Used
Last
The last option recalls the last direction used in a command. For example, if the following command is entered after the
above vector commands a direction location would be drawn in the x-direction (1, 0, 0).
draw direction last
Last directions do not carry over from Trelis session to Trelis session. The last direction defaults to (1, 0, 0) if no direction
has been used during the session.
Positive or Negative X,Y,Z Direction Vectors
X|Y|Z|Nx|Ny|Nz
The x|y|z|nx|ny|nz options assign the x direction, y direction, z direction, negative x direction, negative y direction and
negative z direction respectively.
167
Trelis 15.0 User Documentation
On Curve Tangent
[On] | [Tangent] [At] Curve <id> {location on curve options}
The curve option simply finds a tangent vector on a curve. Note that the on, tangent and at keywords are optional, as
well as the location on the curve. If no location is specified, the tangent at the start vertex of the curve is found. See the
section above, Specifying a Location on a Curve, for details on how to specify where along the curve the tangent vector is
found.
draw direction curve 1
draw direction on curve 1
draw direction tangent at curve 1
draw direction tangent at curve 1 distance 3
draw direction tangent at curve 1 fraction .5
draw direction tangent at curve 1 distance 2 reverse
Figure 1 - Tangents to a Curve
On Surface Normal
[On] | [Normal] [At] Surface <id> [Location {options}]
The surface option simply finds a normal vector on a surface. Note that the "on", "normal" and "at" keywords are optional,
as well as the location on the surface. If no location is specified, the normal vector at the center of the surface is found. If
a location is specified, the location is projected to the surface, then the normal vector is found.
draw direction on surface 1
draw direction on surface 1 location 1 2 0
From Location
[From] {Location {options} | Node|Vertex <id>} [Project] {Location {options} | [Entity]
{Node|Vertex|Curve|Surface} <id>}
The from location option finds a direction that is from one location to another or from a location to an entity. If the second
specification is an entity, the first location is projected to the entity to find the direction.
draw direction from vertex 1 vertex 2
draw direction from location on curve 1 fraction .5 surface 3
Note that when using an entity for the second specification, the Project and Entity keywords are generally optional.
However, it is sometimes necessary to remove ambiguity from the previous location specification. For example, the
following will not parse correctly:
168
Specifying a Direction
draw direction location on curve 1 distance 2 surface 3
In this case, the location on the curve is parsed as a distance 2.0 from surface 3. Instead, the desired behavior is to find
the location on curve 1 as a distance of 2.0 along the curve from the start of the curve, and project it to surface 3 to find
the direction. The following commands (all equivalent) achieve this behavior:
draw direction location on curve 1 distance 2 project surface 3
draw direction location on curve 1 distance 2 entity surface 3
draw direction location on curve 1 distance 2 project entity surface 3
Rotate
[Rotate {options}]
The rotate option allows you to rotate the direction about another vector. You can string together as many rotations as
necessary. For example:
draw direction 1 0 0 rotate about z 135 rotate about curve 1 angle 50
Options that can be used with rotate are as follows:
{Ax|X|Ay|Y|Az|Z [Angle] <angle>} | { {[About] | Towards} Direction {options} Angle <val> } [Rotate
(options)] [Origin (location)]
Ax, Ay, Az (or X,Y,Z) angles can be entered in any order. The optional specification of another rotate keyword in the
options indicated that multiple nested rotations are permitted.
Cross
[Cross [With] Direction {options}]
The cross option allows you to find the vector cross product of the direction with another direction.
Reverse
[Reverse]
This keyword simply reverses the direction specification.
Previewing a Direction
Sometimes it is helpful to preview a direction before using it in a command. A direction may be previewed using the Draw
command. The direction options are described above. See Specifying a Location for a list of location options.
Draw Direction {direction_options} [Location (location_options)]
169
Specifying an Axis
Some commands require a specified axis (such as webcut with a cylinder) and it is sometimes advantageous to view an
axis before modifying geometry. An axis is simply a vector with a specified origin. The following options determine an axis
specification:
•
•
•
Last
Specify a direction and a location
Revolve an axis about an axis
Last
Last
The last option recalls the last axis used in an axis command. The last axis does not carry over from Trelis session to
Trelis session.
Specify an origin and a vector
{Direction {options} [Origin [Location] {options}] [Length <val>] [Angle <val>]}
To specify an axis simply specify a vector (a direction) and an origin (a location). Notice that the command requires the
axis direction first because the origin defaults to 0 0 0 when not specified. An example of specifying an axis to draw a
location using the swing command is as follows:
draw location 1 0 0 swing about axis direction z ang 45
Figure 1 - Swinging a point about the z-axis
The location 1 0 0 was swung 45 degrees about an axis defined by a vector in the z direction and an origin at 0 0 0.
Revolve an axis about an axis
[Axis {options} Revolve [About] Axis {options} Angle <val>]
171
Trelis 15.0 User Documentation
To revolve one axis around another use the revolve keyword. The following example revolves the first axis (defined by the
y-axis and origin) around the second axis (defined by the z-axis and origin) by 45 degrees and draws the result.
draw axis direction y revolve axis direction z angle 45
Figure 2 - Revolving an axis about another axis
Previewing an Axis
Sometimes it is helpful to preview an axis before using it in a command. An axis may be previewed using the Draw
command. The options for previewing an axis are the same as the ones described above.
Draw Axis {options}
172
Specifying a Plane
Some commands require a specified plane (such as sweep curve target) for the command. The following options
determine a plane specification:
•
•
•
•
•
•
•
•
•
•
•
{Location|Vertex|Node} <origin> Direction <normal>
{Location|Vertex|Node} <origin> Direction <vec on plane> Direction <vec on plane>
{Location|Vertex|Node} <2 locations> Direction <vector on the plane>
{Location|Vertex|Node} <3 locations>
Surface <id> [at location <loc>]
[Normal To] Curve <id> [loc on curve options]
Direction <Normal> Coefficient <val>
Arc Curve <id>
Linear Curve <id> <id>
X|Xplane|Yz|Zy|Y|Yplane|Zx|Xz|Z|Zplane|Xy|Yx
Last
The following options apply to all of the plane specifications listed above:
•
•
•
•
[Offset <val>]
[Move { <xval yval zval> | {Dx|X|Dy|Y|Dz|Z} <val> | Direction {options} [Distance <val>]]
[[To] Location {options}]
[Spin [About] Axis {options} Angle <ang>]]
Location and Normal Vector
{Location|Vertex|Node} <origin> Direction <normal>
The first way to specify a plane is to specify a starting point and a direction vector:
draw plane location 1 2 3 direction 0 1 1
draw plane vertex 1 direction tangent at curve 1
Figure 1. Specifying a plane with a location and surface normal
To see the options for location specification, see Specifying a Location. Direction options can be found at Specifying a
Direction.
173
Trelis 15.0 User Documentation
Location and Two Vectors on the Plane
{Location|Vertex|Node} <origin> Direction <vec on plane> Direction <vec on plane>
It is also possible to select an origin point and 2 direction vectors on the plane.
.
Figure 2. Specifying a plane with a point and 2 in-plane vectors
Two Locations and Vector on the Plane
{Location|Vertex|Node} <2 locations> Direction <vector on the plane>
You can also specify 2 locations and 1 direction on the plane to define the plane.
draw plane vertex 1 2 direction 0 1 1
Figure 3. Specifying 2 locations and 1 direction on the plane
174
Specifying a Plane
Three Points on the Plane
{Location|Vertex|Node} <3 locations>
A plane can be defined by three locations, vertices, or nodes. The locations are specified using Location Specification.
draw plane vertex 1 2 3
draw plane vertex 1 2 location 3 4 5
Figure 4. A plane specified by three points
Plane defined by a Surface
Surface <id> [At Location <loc>]
The surface option uses and existing surface to define the plane. If it is not a planar surface, the optional location specifier
can be used to find the tangent plane of a specific point on the surface.
draw plane surface 1 at location 4 0 0
175
Trelis 15.0 User Documentation
Figure 5. Specifying a Tangent plane to a Surface
Plane Normal to a Curve
[Normal To] Curve <id> [loc on curve options]
The Normal to Curve option allows you to define a plane by using an existing curve. The direction of the curve will define
the surface normal of the new plane. The optional location argument specifies which point to use on the curve if it is not a
straight curve. If no location is specified the plane will originate at the midpoint of the curve. See Specifying a Location on
a Curve for more information on location options.
brick x 10
cylinder radius 3 z 12
subtract body 2 from 1
webcut body 1 xplane
draw plane normal to curve 30
176
Specifying a Plane
Figure 6. Draw Plane Normal to Curve
Plane Defined by a Non-linear curve
Arc Curve <id>
A plane can be defined by a single curve, provided that curve is not linear.
cylinder height 12 radius 3
draw plane arc curve 2
Plane Defined by a two linear curves
Linear Curve <id> <id>
A plane can be defined by a two linear curves, provided that the curves are not co-linear.
brick x 10
draw plane linear curve 2 3
Normal Vector and Coefficient
Direction <Normal> Coefficient <val>
The direction and coefficient option allows you to specify a plane based on a vector and an offset from the origin. The
Coefficient argument specifies how far to offset the plane from the origin
draw plane direction 1 2 3 coefficient 3
Coordinate Plane
X|Xplane|Yz|Zy|Y|Yplane|Zx|Xz|Z|Zplane|Xy|Yx
177
Trelis 15.0 User Documentation
A plane can be defined from any coordinate plane or combination thereof. The coordinate planes will pass through the
origin unless optional specifiers are included.
draw plane xplane
webcut volume 1 plane xz
Last Location Used
Last
The last option will return the plane most recently used in a command. Last locations do not carry over from Trelis session
to Trelis session. The last location defaults to (0, 0, 0) if no location has been used during the session.
The following options apply to all of the plane specification methods described above.
•
•
•
•
[Offset <val>]
[Move {<xval yval zval>| {Dx|X|Dy|Y|Dz|Z} <val> | Direction {options} [Distance <val>]]
[[To] Location {options}]
[Spin [About] Axis {options} Angle <ang>]]
A offset value will offset the plane in the direction of the surface normal.
The move option will displace the plane in the specified directions by the specified distance. The direction options are
outlined on Specifying a Direction.
The location option will move the plane to a specified location without rotating it. See Specifying a Location for location
options.
The spin option will rotate the plane around an axis. See Specifying an Axis for axis options.
Previewing a Plane
The ability to preview a plane prior to creating the plane or using it in a command is possible with the following
commands:
Draw Plane (options) [Graphics | {[Intersecting] {Body|Volume} <id_range>] [ [Extended] {Percentage|Absolute} <val>]}]
[Color 'color_name']
The options for specifying a plane are described above in the section on Plane Specification. By default, the commands
draw the plane just large enough to intersect the bounding box of the entire model with minimum surface area. Optionally,
you can give a list of bodies to intersect for this calculation. You can also extend the size of the surface by either a
percentage distance or an absolute distance of the minimum area size. The default color is blue, but you can specify a
different one. See the Appendix of the Trelis Users Guide for available colors in Trelis.
Preview a Cylindrical Plane
The ability to preview a cylindrical plane is possible with the following command:
Draw Cylinder Radius <val> Axis {x|y|z|Vertex <id_1> Vertex <id_2> | <xyz values>} [Center <x_val> <y_val> <z_val>]
[[Intersecting] Body <id_range>] [Extended Percentage|Absolute <val>] [Color 'color_name']
The cylinder is defined by a radius and the cylinder axis. The axis is specified as a line corresponding to a coordinate axis,
the normal to a specified surface, two arbitrary points, or an arbitrary point and the origin. The center point through which
the cylinder axis passes can also be specified.
178
Specifying a Plane
By default, the commands draw the cylinder just large enough to just intersect the bounding box of the entire model.
Optionally, you can give a list of bodies to intersect for this calculation. You can also extend the length of the cylinder by
either a percentage distance or an absolute distance of the cylinder length. The default color is blue, but you can specify a
different one. See the Appendix of the Trelis Users Guide for available colors in Trelis.
179
Drawing a Location, Direction, or Axis
Some commands require you to specify a location on a curve (i.e., webcutting with a plane normal to a curve). This
location can be previewed with the following options:
1.
2.
3.
4.
A fraction along the curve from the start of the curve, or optionally, from a specified vertex on the curve.
A distance along the curve from the start of the curve, or optionally, from a specified vertex on the curve.
An xyz position that is moved to the closest point on the given curve.
The position of a vertex that is moved to the closest point on the given curve.
Draw Location On Curve <curve id> {Fraction <f> | Distance <d> | Position <xval><yval><zval> |
Close_To Vertex <vertex_id>} [[From] Vertex <vertex_id> (optional for 'Fraction' & 'Distance')]
Some commands require a specified axis (such as webcut with a cylinder) and it is sometimes advantageous to view an
axis before modifying geometry. To draw a preview of an axis use the following command:
Draw Axis {options}
Some commands require a specified location or point (such as create curve spline) and it is sometimes advantages to
view a location before modifying or creating geometry. To draw a preview of a location use the following command:
Draw Location {options} [color <color_name>][no_flush]
Similar commands for drawing lines and polygons may also be useful.
181
List Model Summary
The following commands print identical summaries of the model: the number of entities of each geometric, mesh, and
special type
List Model
List Totals
The following output is generated from the list model command.
Trelis> list model
Model Entity Totals:
Geometric Entities:
0 assemblies
0 parts
2 groups
1 bodies
1 volumes
6 surfaces
12 curves
8 vertices
Mesh Entities:
6000 hexes
0 pyramids
0 tets
7876 faces
0 tris
9854 edges
7161 nodes
Special Entities:
1 element blocks
1 sidesets
1 nodesets
Journaled Command: list model
183
List Geometry
The following commands list information about the geometry of the model.
List Names [Group|Body|Volume|Surface|Curve|Vertex|All]
List {Group|Body|Volume|Surface|Curve|Vertex} <range> [Ids]
List {geom_list} [Geometry|Mesh [Detail]]
List {Group|Body|Volume|Surface|Curve|Vertex} <range> {X|Y|Z}
The first command lists the names in use, and the entity type and id corresponding to each name. Specifying all lists
names for all types; other options list names for a specific entity type. The names for an individual entity can be obtained
by listing just that entity. Sample output from the list names surface command is shown below. This output shows that, for
example, Surface 2 has the name ` BackSurface '.
______Name______ __Type__
BackSurface Surface 2
BottomSurface Surface 3
FrontSurface Surface 1
LeftSurface Surface 4
RightSurface Surface 5
TopSurface Surface 6
Id
_Propagated_
No
No
No
No
No
No
List Names Example
The second command provides information on the number of entities in the model and their identification numbers. If a
range is given then detailed information is given on each entity in that range, unless the ids option is also given. If the ids
option is used, just a list of ids is printed. This list can be very useful for large models in which several geometry
decomposition operations have performed. Sample output from the list surface command is shown below.
Trelis> list surface ids
The 6 surface ids are 1 to 6.
Trelis> list surf ids
The 108 surface ids are 192 to 266, 268 to 271, 273 to 301.
List Surface [range] Ids' Examples
The <range> can be very general using the general entity parsing syntax. Using a <range> gives a brief synopsis of the
local connectivity of the model, e.g. one can list the ids of the surfaces containing vertex 2; as shown in the listing below..
An intermediately detailed synopsis can be obtained by placing the range of entities in a group, then listing the group.
Trelis> list surface in vertex 2 ids
The 3 entity ids are 1, 5, 6.
Trelis> group "v2_surfs" equals surface in vertex 2
Trelis> list v2_surfs Group Entity 'v2_surfs' (Id = 3)
It owns/encloses 3 entities: 3 surfaces.
Owned Entities:
Mesh Scheme Interval: Edge
_____Name____ Type______Id +is meshed Count
FrontSurface Surface 1
map+
1H
0.1
TopSurface Surface 6
map+
1H
0.1
RightSurface Surface 5
map+
1H
0.1
Size
Using 'List' for Querying Connectivity.
The third command provides detailed information for each of the specific entities. This information includes the entity's
name and id, its meshing scheme and how that scheme was selected, whether it is meshed and other meshing
parameters such as smooth scheme, interval size and count. The entity's connectivity is summarized by a table of the
entity's subentities and a list of the entity's superentities. Also, the nodesets, sidesets, blocks, and groups containing the
entity are listed.
185
Trelis 15.0 User Documentation
Specifying geometry will additionally list the extent of the entity's geometric bounding box, the geometric size of the entity,
and depending on entity type, other information such as surface normal. See also the list {entities} x command below. If
multiple volumes, surfaces, or curves are selected, it will list the total volume, area, or length of all entities, and the total
geometric bounding box. If multiple volumes are selected, the centroid listed will be the composite centroid of the all of the
volumes.
Specifying mesh will additionally list the number of mesh entities of each type interior to the entity and on bounding
subentities. Mesh detail will list the ids of the mesh entities as well, following the format of the list ids command above.
The fourth command lists the entities sorted by either the x, y, or z coordinate of their geometric center. For example, in a
large, basically cylindrical model centered around z-axis, it is useful to list the surfaces of a volume sorted by z to identify
the source and target sweeping surfaces.
186
List Mesh
The following commands list mesh entity information.
List {Hex|Face|Edge|Node} <id_range>
List {Hex|Face|Edge|Node} <id_range> IDs
For both of these commands, the range can be very general, following the general entity parsing syntax. The first
command provides detailed information. For an entity, the information includes its id, owning geometry, subentities and
superentities. For a hex, the Exodus Id is also listed. For a node, its coordinates are listed. The second command just lists
the entity ids, and is usually used in conjunction with complex ranges.
187
List Special Entities
List {special_type} <range>
Special entities include (element) blocks, sidesets and nodesets (representing boundary conditions). Like the list
geometry and list mesh commands, if no range is specified then the number of entities of the given type is summarized.
Otherwise, listing a special entity prints the mesh and geometry it contains.
(Some special entities are of interest mainly to developers and are not described here, e.g. whisker sheets, and whisker
hexes.)
189
List Trelis Environment
The user may list information about the current Trelis environment such as message output settings, memory usage, and
graphics settings.
Message Output Settings
There are several major categories of Trelis messages.
•
•
•
•
•
Info (Information) messages tell the user about normal events, such as the id of a newly created body, or the
completion of a meshing algorithm.
Warning messages signal unusual events that are potential problems.
Error messages signal either user error, such as syntax errors, or the failure of some operation, such as the
failure to mesh a surface.
Echo messages tell the user what was journaled.
Debug messages tell developers about algorithm progress. There are many types of Debug messages, each
one concentrating on a different aspect of Trelis.
By default, Info, Warning, Error, and Echo messages are printed, and Debug messages are not printed. Information,
Warning and Debug message printing can be turned on or off (or toggled) with a set command; error messages are
always printed. Debugging output can be redirected to a file. Current message printing settings can be listed.
List {Echo|Info|Errors|Warning|Debug }
Set {Echo|Info|Warning} [On|Off]
[Set] Debug <index> [On|Off]
[Set] Debug <index> File <'filename'>
[Set] Debug <index> Terminal
Message flags can also be set using command line options, e.g. -warning={on|off} and -information={on|off}. Debug
flags can be set on with -debug=<setting>, where <setting> is a comma-separated list of integers or ranges of integers
denoting which flags to turn on. E.g. to set debug flags 1, 3, and 8 to 10 on, the syntax is -debug=1,3,8-10.
In addition to the major categories, there are some special purpose output settings.
[Set] Logging {Off|On File <'filename'> [Resume]}
List Logging
If logging is enabled, all echo, info, warning, and error messages will be output both to the terminal and to the logging file.
The resume option will append to the logfile, if it exists, instead of writing over it. If the logfile doesn't already exist, it will
be created.
List Journal Title "<title_string>"
The List Journal command lists which types of Trelis commands will be journaled and the file to which the journaled
commands are being written.
List Title
The List Title command will list the title to be written to the Exodus file. To assign a title to an exodus file, use the Title
command.
191
Trelis 15.0 User Documentation
List Default Block
Set Default Block {ON|off}
The List Default Block command lists which type of geometric entities for which blocks will automatically be generated at
export if no other blocks have been specified. The Set Default Block command will toggle whether these default blocks
are written, or not, during the export operation when no other blocks have been specified.
List Settings
The List Settings command lists the value of all the message flags, journal file and echo settings, as well as additional
information. The first section lists a short description of each debug flag and its current setting. Next come the other
message settings, followed by some flags affecting algorithm behavior.
Sample output
Trelis> list settings
Debug Flag Settings (flag number, setting, output to, description):
1 OFF terminal
options.
Debug Graphics toggle for some debug
2
OFF
terminal
Whisker weaving information
3
OFF
terminal
Timing information for 3D Meshing routines.
4
OFF
terminal
Graphics Debugging (DrawingTool)
5
OFF
terminal
FastQ debugging
6
OFF
terminal
Submapping graphics debugging
7
OFF
terminal
Knife progress whisker weaving information
8 OFF
debug
terminal
Mapping Face debug / Linear Programming
terminal
Paver Debugging
9
OFF
.
.
.
echo
= On
info
= On
journal
= On
journal graphics
= Off
journal names
= On
journal aprepro
= On
192
List Cubit Environment
journal file
= 'cubit11.jou'
warning
= On
logging
= Off
recording
= Off
keep invalid mesh = Off
default names
default block
catch interrupt
= Off
= Volumes
= On
name replacement character = '_', suffix character = '@'
Matching Intervals is fast, TRUE;
multiple curves will be fixed per iteration.
Note in rare cases 'slow', FALSE, may produce better meshes.
Match Intervals rounding is FALSE;
intervals will be rounded towards the user-specified intervals.
Graphical Display Information
List View
List view prints the current graphics view and mode parameters; See Graphics Window .
Memory Usage Information
Users are encouraged to use Unix commands such as `top' to check total Trelis memory use. Developers may check
internal memory usage with the following command:
List Memory [`<object type>']
Without an object type, the command prints memory use for all types of objects.
193
ACIS Geometry Kernel
ACIS is a proprietary format developed by Spatial Technologies. Trelis incorporates the ACIS third party libraries directly
within the program. The ACIS third party libraries are used extensively within Trelis to import, export and maintain the
underlying geometric representations of the solid model for geometry decomposition and meshing. There are many ways
to get geometry into the ACIS format. ACIS files can be exported directly from several commercial CAD packages,
including SolidWorks, AutoCAD, and HP PE/SolidDesigner. Third party ACIS translators are also available for converting
from native formats such as Pro Engineer. Trelis also uses the ACIS libraries for importing IGES and STEP format files.
As of version 15.0, Trelis supports the direct translation of Parasolid, SolidWorks, and Pro/Engineer files for an additional
license fee. Also as of version 15.0, Trelis can import geometry from an existing Gambit file.
Importing and creating geometry using the ACIS geometric modeling kernel currently provides the widest set of
capabilities within Trelis. All geometry creation and modification tools have been designed to work directly on the ACIS
representation of the model.
195
Mesh-Based Geometry
In contrast to the ACIS format, Mesh-Based Geometry (MBG) is not a third party library and has been developed
specifically for use with Trelis. Most of Trelis' mesh generation tools require an underlying geometric representation. In
many cases, only the finite element model is available. If this is the case, Trelis provides the capability to import the finite
element mesh and build a complete boundary representation solid model from the mesh. The solid model can then be
used to make further enhancement to the mesh. While the underlying ACIS geometry representation is typically nonuniform rational b-splines (NURBS), Mesh-Based Geometry uses a facetted representation. Mesh-Based Geometry can
be generated by importing either an Exodus II format file or a facet file.
•
•
•
•
Creating Mesh-Based Geometry Models
Improving Mesh-Based Geometry Models for Meshing
Meshing Mesh-Based Models
Exporting Mesh-Based Geometry
Many of the same operations that can be done with traditional CAD geometry can also be done with mesh-based
geometry. While all mesh generation operations are available, only some of the geometry operations can be used. For
example, the following can be done with geometric entities that are mesh-based:
•
•
•
Geometry Transformations
Merging
Virtual Geometry Operations
Some operations that are not yet available with mesh-based geometry include:
•
•
•
Booleans
Geometry Decomposition
Geometry Clean-Up
Creating Mesh-Based Geometry Models
Mesh based geometry models can be created in one of two ways
•
•
Importing Exodus II files
Importing facet files
While both of these methods create geometry suitable for meshing, there are some significant differences:
Exodus II files
Exodus II contains a mesh representation that may include 3D elements, 2D elements, 1D elements and even 0D
elements. It may also contain deformation information as well as boundary condition information. The import mesh
geometry command is designed to decipher this information and create a complete solid model, using the mesh faces as
the basis for the surface representations. Exodus II is most often used when a solid model that has previously been
meshed requires modification or remeshing. Importing an Exodus II file will generate both geometry and mesh entities,
assigning appropriate ownership of the mesh entities to their geometry owners. Deleting the mesh and remeshing, refining
or smoothing are common operations performed with an Exodus II model.
Facet files
The facet file formats supported by Trelis are most often generated from processes such as medical imaging,
geotechnical data, graphics facets, or any process that might generate discrete data. Importing a facet file will generate a
surface representation only defined by triangles. If the triangles in the facet file form a complete closed volume, then a
volume suitable for meshing may be generated. In cases where the volume may not completely close or may not be of
sufficient quality, a limited set of tools has been provided. In addition to the standard meshing tools provided in Trelis, it is
also possible to use the triangle facets themselves as the basis for an FEA mesh.
197
Trelis 15.0 User Documentation
Improving Mesh-Based Geometry Models for Meshing
In many cases, the triangulated representations that are provided from typical imaging processes are not of sufficient
quality to use as geometry representations for mesh generation. As a result, Trelis provides a limited number of tools to
assist in cleaning up or repairing triangulated representations.
1. Using tolerance on STL files
Stereolithography (STL) files, in particular, can be problematic. The import mechanism for STL provides a tolerance
option to merge near-coincident vertices.
2. Using the stitch option on AVS and facet files
The stitch option on the import facets|avs command provides a way to join triangles that otherwise share near-coincident
vertices and edges. This is useful for combining facet-based surfaces to generate a water-tight model.
3. Using the improve option on facet files.
The improve option on the import facets command will collapse short edges on the boundary of the triangulation. This
option improves the quality of the boundary triangles.
4. Smoothing faceted surfaces.
Individual triangles in a faceted surface representation may be poorly shaped. Just like mesh elements may be smoothed,
facets may also be smoothed in Trelis using the following command
Smooth <surface_list> Facets [Iterations <value>] [Free] [Swap]
To use this command, the surface cannot be meshed. Facet smoothing consists of a simple Laplacian smoothing
algorithm which has additional logic to make sure it does not turn any of the triangles in-side out. It also determines a local
surface tangent plane and projects the triangle vertices to this plane to ensure the volume will not "shrink". The iterations
option can be used to specify the number of Laplacian smoothing operations to perform on each facet vertex (The default
is 1).
The free option can be used to ignore the tangent plane projection. Used too much, the free option can collapse the
model to a point. One of two iterations of this option may be enough to clean up the triangles enough to be used for a
finite element mesh.
The swap option can be used to perform local edge swap operations on the triangulation. The quality of each triangle is
assessed and edges are swapped if the minimum quality of the triangles will improve.
5. Creating a thin offset volume
Offset surfaces may be generated from an existing facet-based surface. This would be used in cases where a thin
membrane-like volume might be required where only a single surface of triangles is provided. This command may be
accomplished by using the standard create body offset command
The result of this command is a single body with an inside and outside surface separated by a small distance which is
generally suitable for tet meshing. This command is currently only useful for small offsets where self-intersections of the
resulting surface would be minimal. It is most useful for bodies that may be initially composed of a single water-tight
surface.
6. Creating volumes from surfaces
A mesh-based geometry volume can be created from a set of closed surfaces. This can be accomplished in the same
manner as the standard create body surface command
Create Body Surface <surface_id_range>
This command is limited to surfaces that match triangles edges and vertices at their boundary. The command will
internally merge the triangles to create a water-tight model that would generally be suitable for tet meshing.
198
Mesh-Based Geometry
Meshing Mesh-Based Models
Mesh-Based models may be meshed just like any other geometry in Trelis by first setting a scheme, defining a size and
using the mesh command. This standard method of mesh generation can be somewhat time consuming and error prone
for complex facet models with thousands of triangles. Trelis also provides the option of using the facets themselves as a
surface triangle mesh, or as the input to a tetrahedral mesher. This may be accomplished with one of two options:
Mesh <entity_list> From Facets
This command will generate triangular finite elements for each facet on the surface. If the entity_list is composed of one
or more volumes, then the tetrahedral mesh will automatically fill the interior. This method is useful when further cleanup
and smoothing operations are needed on the triangles after import.
Import Facets <filename> Make_elements
The make_elements on the import facets command will generate the triangular finite elements on the surface at the time
the facets are read and created. This option is useful if no further modifications to the facets are necessary.
Creating triangular finite elements in this manner can greatly speed up the mesh generation process, however it is limited
to non-manifold topology. If the triangular elements are to be used for tetrahedral meshing (i.e. all edges of the
triangulation should be connected to no more than two triangles)
Exporting Mesh-Based Geometry
Mesh-Based geometry models and their mesh may be exported by one of the following methods:
•
•
Exporting to an Exodus II File
Exporting to a facet file
Exodus II
Exporting to an Exodus II file saves the finite element mesh along with any boundary conditions placed on the model. It
will not save the individual facets that comprise the mesh-based geometry surface representation. Importing an Exodus II
file saved in this manner will regenerate the surfaces only to the resolution of the saved mesh.
Facet files
Trelis also provides the option to save just the surface representation to a facet or STL file. The following commands can
be used for saving facet or STL files:
Export Facets 'filename' <entity_list> [Overwrite]
Export STL [ASCII|Binary] 'filename' <entity_list> [Overwrite]
These commands provide the option of saving specific surfaces or volumes to the facet file. If no entities are provided in
the command, then all surfaces in the model will be exported to the file. The overwrite option forces a file to overwrite any
file of the same name in the current working directory.
199
Importing ACIS Files
To import an ACIS file:
1.
2.
3.
4.
5.
6.
Select File and then Import.
Select the file to be imported.
Select ACIS from the Files of type drop-down menu.
Click Open. A new window will appear.
Optionally specify any appropriate settings from this window.
Click Finish.
Import Acis '<acis_filename>' [No_bodies][No_surfaces] [No_curves][No_vertices][Group
{'<name>'|<id>}] [Binary|Ascii] [Show_Each] [Sort] [Attributes_On] [Separate_Bodies]
[merge_gloabally] [Heal]
The import ACIS command is the primary mechanism for generating geometry within Trelis. ACIS parts can be
generated and saved with Trelis, but in most cases are developed within a 3rd party CAD package and exported for use in
Trelis. Trelis provides the capability to import ACIS solid models and make modifications to them so they can be meshed.
Trelis incorporates the commercial ACIS libraries developed and maintained by Spatial Inc. for reading and writing ACIS
format files. IGES and STEP format files can also be imported and exported to/from Trelis using the Spatial's libraries.
Import Options
It is possible to include free entities (vertices, curves and surfaces) in the file. The default operation is to read all entities in
the file whether they are included as part of a body or are free. By using any of the options no_bodies, no_surfaces,
no_curves, or no_vertices, the user may exclude certain types of free entities.
The group option of the import command will allow the user to create a group for each set of imported geometry. The
newly created group can later be accessed using the name or id specified with the group option.
The import capability of ACIS files supports both the ASCII format (.sat) and binary format (.sab). When importing, the
filename extension will determine the default file type, be it ASCII or binary. A (.sat) extension will default to ASCII, while a
(.sab) extension will default to binary. If you use a different file extension you can specify the type with the [binary|ascii]
option. Binary files can be significantly faster but are not guaranteed to be upward compatible, nor cross-platform
compatible. Therefore, it is recommended that models be archived in ASCII format.
Normally the numerical IDs of the geometric entities contained in the ACIS model are used directly within Trelis. The sort
option provides the capability to compress the IDs read from the ACIS file. The sort option does the same thing as the
compress ids sort command, but combines it with the import command to remove a step in the process.
The show_each option is a graphics option that applies to how the volumes are shown as they are imported. If there are
multiple volumes in the file, the graphics display will be updated between each volume during import.
The attributes_on option will enable attribute support for the file. Attributes include properties like entity color, entity id,
and meshing scheme. Including the attributes option will only affect the current import. The settings will be restored to
their previous settings after importing.
The separate_each option creates a separate body for each volume that is imported, preventing multi-volume bodies
from being imported.
When importing, the use may specify the scope of the merge using merge_globally. The default behavior is to merge
within the scope of the file being imported. With the merge_globally option, imported entities will merge with anything,
including entities already in the Trelis session that have merge attributes on them.
Use the heal option to heal the entities when importing.
Importing ACIS files at startup
ACIS files can also be imported using the "-solid" option when starting Trelis from the UNIX command prompt. (See
Execution Command Syntax for details.) Note that the filename must be enclosed in single or double quotes. This
command will create as many bodies within Trelis as there are bodies in the input file.
See also Exporting ACIS Files.
201
Trelis 15.0 User Documentation
202
Importing FASTQ Files
Trelis can read a FASTQ file and convert it into an ACIS model:
Import Fastq '<fastq_filename>'
Note that the filename must be enclosed in single or double quotes.
FASTQ is an older, 2d meshing tool; (Blacker 88.) FASTQ files are a series of commands much like a Trelis journal file.
All FASTQ commands are fully supported except for the "Body" command (it is unnecessary and ignored), the "corn"
(corner) line type, and some of the specialized mapping primitive "Scheme" commands. Standard mapping, paving, and
triangle primitive scheme commands are handled. The pentagon, semicircle, and transition primitives are not handled
directly, but are meshed using the paving scheme. The FASTQ input file may have to be modified if the Scheme
commands use any non-alphabetic characters such as `+', `(`, or `)'. Circular lines with non-constant radius are generated
as a logarithmic decrement spiral in FASTQ; in Trelis they will be generated as an elliptical curve.
Since a FASTQ file by definition will be defined in a plane, it must be projected or swept to generate three dimensional
geometry. Trelis supports sweeping options to convert imported FASTQ geometries into volumetric regions.
203
Importing STEP Files
The ACIS STEP translator provides bi-directional functionality for data translation between ACIS and the file format
standard STEP AP203.
STEP AP203 is an international standard which defines a neutral file format for representation of configuration control
design data for a product.
To import a STEP file:
1.
2.
3.
4.
5.
6.
Select File and then Import.
Select the file to be imported.
Select STEP from the Files of type drop-down menu.
Click Open. A new window will appear.
Optionally specify any appropriate settings from this window.
Click Finish.
Import Step '<step_filename>' [No_bodies][No_surfaces] [No_curves] [No_vertices] [HEAL|Noheal]
[Logfile ['filename'] [Display]] [Show_Each] [Group {'<name>'|<id>}] [Sort] [XML '<xml_filename>']
Import Options
It is possible to include free entities (vertices, curves and surfaces) in the file. The default operation is to read all entities in
the file whether they are included as part of a body or are free. By using any of the options no_bodies, no_surfaces,
no_curves, or no_vertices, the user may exclude certain types of free entities.
By default, bodies are automatically healed when imported - if this causes problems, you can disable this option by using
the noheal argument.
The logfile option specifies a file where informational messages generated during import of the STEP file will be written.
The display option will display the file.
The show_each option is a graphics option that applies to how the volumes are shown as they are imported. If there are
multiple volumes in the file, the graphics display will be updated between each volume during import.
The group option of the import command will allow the user to create a group for each set of imported geometry. The
newly created group can later be accessed using the name or id specified with the group option.
Normally the numerical IDs of the geometric entities contained in the STEP model are used directly within Trelis. The sort
option provides the capability to compress the IDs read from the STEP file. The sort option does the same thing as the
compress ids sort command, but combines it with the import command to remove a step in the process.
The xml option will read assembly information and other metadata from an XML file in the DART metadata XML format.
See the metadata documentation and the Analyst's Home Page for details.
Beginning with version 13.0, Trelis will read assembly information embedded in the imported STEP file. No additional
arguments are required. The resultant assembly/part structure will be displayed in the GUI's main entity tree.
Exporting a STEP file from Pro/Engineer
To export a STEP file from Pro/ENGINEER, from the Export STEP Dialog, Press Options.
In the file step_config.pro add the following:
STEP_EXPORT_FORMAT AP203_CD.
Also be sure your export option is set to Solids. If the geometry has problems in Trelis, you may need to increase the
geometry accuracy in Pro/ENGINEER.
See also Exporting STEP Files.
205
Trelis 15.0 User Documentation
206
Importing IGES Files
The ACIS IGES translator provides bi-directional functionality for data translation between ACIS and the IGES (Initial
Graphics Exchange Specification) format.
To import an IGES file:
1.
2.
3.
4.
5.
6.
Select File and then Import.
Select the file to be imported.
Select IGES from the Files of type drop-down menu.
Click Open. A new window will appear.
Optionally specify any appropriate settings from this window.
Click Finish.
Import Iges '<iges_filename>' [No_bodies] [No_surfaces] [No_curves] [No_vertices] [Group
{'<name>'|<id>}] [Nofreesurfaces] [HEAL|noheal] [Logfile ['filename'] [Display]] [Show_Each] [Sort]
Import Options
It is possible to include free entities (vertices, curves and surfaces) in the file. Default operation is to read all entities in the
file whether they are included as part of a body or are free. By using any of the options no_bodies, no_surfaces,
no_curves, or no_vertices, the user may exclude certain types of free entities.
The group option of the import command will allow the user to create a group for each set of imported geometry. The
newly created group can later be accessed using the name or id specified with the group option.
The nofreesurfaces option will automatically convert free surfaces to bodies. By default this option is off.
By default, bodies are automatically healed when imported - if this causes problems, you can disable this option by using
the noheal argument.
The logfile option specifies a file where informational messages generated during import of the STEP file will be written.
The display option will display the file.
The show_each option is a graphics option that applies to how the volumes are shown as they are imported. If there are
multiple volumes in the file, the graphics display will be updated between each volume during import.
Normally the numerical IDs of the geometric entities contained in the ACIS model are used directly within Trelis. The sort
option provides the capability to compress the IDs read from the ACIS file. The sort option does the same thing as the
compress ids sort command, but combines it with the import command to remove a step in the process.
Note that the IGES import and export functionality might not be available on all 64-bit platforms.
See also Exporting IGES Files.
207
Importing Facet Files
Trelis provides the capability to import a model composed of facets to create geometry. The command to import facets
from a file is:
To import a facets file
1.
2.
3.
4.
5.
6.
Select File and then Import.
Select the file to be imported.
Select Facets from the Files of type drop-down menu.
Click Open. A new window will appear.
Optionally specify any appropriate settings from this window.
Click Finish.
Import [Facets|AVS|STL] ''<filename>" [Feature_Angle] [LINEAR||Spline] [MERGE|No_merge]
[Make_elements] [Stitch] [Improve]
Facets are simply triangles that have been stitched together to form surfaces. Faceted geometry representations are
commonly used for graphics, bio-medical, geotechnical and many other applications that output a discrete surface
representation. Upon import, the resulting geometry representation is Mesh-Based Geometry. Figure 1. shows an
example of a faceted model and the resulting geometry created in Trelis.
Figure 1. Example of faceted model and the resulting solid model created in Trelis from the facets.
For convenience, the import facet command currently supports three different formats, facet, AVS and STL
•
•
Facet format: The facet file format is a simple ASCII file that contains vertex coordinates and connectivities.
The facet file format is described below.
AVS format: The AVS format is a general geometry format that can support a variety of polygonal shapes. In
Trelis' implementation of the AVS import, it will support only triangles.
209
Trelis 15.0 User Documentation
•
STL format: Perhaps the most common format in the industry is Stereolithography (STL). Trelis supports both
ASCII and binary forms of the STL format. While the STL format is adequate for graphics and visualization, it
can be problematic for geometry applications such as Trelis. Each triangle in the STL format is represented
independently. This means that multiple definitions of a single vertex are included in the file. Trelis will attempt
to merge duplicate vertices to form a water-tight surface. In cases where the vertex locations may not
correspond exactly, an optional tolerance argument may be used on the import command. The tolerance
option is used only for STL format files.
Facet File Format
The format for the ASCII facet file is as follows
nm
id1 x1 y1 z1
id2 x2 y2 z2
id3 x3 y3 z3
.
.
.
idn xn yn zn
fid1 id<1> id<2> id<3> [id<4>]
fid2 id<1> id<2> id<3> [id<4>]
fid3 id<1> id<2> id<3> [id<4>]
.
.
.
fidm id<1> id<2> id<3> [id<4>]
Where:
n = number of vertices
m = number of facet
id<i> = vertex ID if vertex i
x<i> y<i> z<i> = location of vertex i
fid<j> = facet ID if facet j
id<1> id<2> id<3> = IDs of facet vertices
[id<4>] = optional fourth vertex for quads
As noted above, the facets can be either quadrilaterals or triangles. Upon import, the facets serve as the underlying
representation for the geometry. By default, the facets are not visible once the geometry has been imported. To view the
facets, use the following command:
draw surf <id range> facets
Feature Angle
The feature angle option is used to specify the angle at which surfaces will be split by a curve or where curves will be
split by a vertex. 180 degrees will generate a surface for every facet, while 0 degrees will define a single, unbroken
surface from the shell of the mesh. The default angle is 135 degrees. This feature is identical to the feature angle option
available when importing Exodus II files.
Smooth Curves and Surfaces
This option permits the use of a higher order approximation of the surface when remeshing/refining the resulting
geometry. Default is to use the original facets themselves as the curve and surface geometry representation. If the facet
model to be imported is to represent geometry with curved surfaces, it may be useful to apply this option. If the Spline
option is selected, it will use a 4th order B-Spline approximation to the surface [Walton,96]. More information on using
smooth approximation of the facets is available in Importing an Exodus II File.
210
Importing Facet Files
Merge
This option allows the user to either merge or not merge the resulting surfaces. The default option is to merge adjacent
surfaces. This results in non-manifold topology, where neighboring surfaces share common curves. The no_merge
option, adjacent surfaces will generate distinct/separate curves.
Make elements
This option creates mesh elements from each of the facets on the facet surface.
Stitch
The stitch option is used with the facet or avs format files to try to merge vertices and triangles that are close. Figure 2
shows an example of where this might be employed. The model on the left contains facets that are not connected
between the red and blue groups. In this case, the surfaces will not be water-tight, even though the vertices on the
boundary between the two groups may be coincident. The stitch option attempts to eliminate the extra edge and vertex
between the groups to form the model on the right. This option can be useful when importing facet files for 3D meshing.
Trelis' 3D meshing algorithms require a water-tight (closed) set of surfaces.
Figure 2. Example use of the stitch option on import.
Improve
The improve option will collapse short edges on the boundary of the triangulation that are less than 30% the length of the
average edge length in the model. In some cases, short edges are the result of discrete boolean operations on the
triangulation which may result in edges that are of negligible length. This option is particularly useful for boundaries where
multiple surfaces come together at an edge. Figure 3. shows an example of where the improve option improved the
quality of the triangles at the boundary. This option is especially useful if the facets themselves will be used for the FEA
mesh.
211
Trelis 15.0 User Documentation
Triangles near a boundary that have not been
used the improve option
The same set of triangles where improve option
has collapsed edges
Figure 3. Example use of the improve option
212
Importing Granite Files
As of version 15.0, native Granite (Pro/Engineer) models can be directly read into Trelis via an add-on available from
csimsoft.
213
Creating Vertices
The basic commands available for creating new vertices directly in Trelis are:
•
•
•
•
•
•
XYZ location
On Curve - Fraction
On Curve - General
From Vertex
At Arc
At Intersection
1. XYZ location: The simplest form of this command is to specify the XYZ location of the vertex. It can also be created
lying on a curve or surface in the geometric model by specifying the curve or surface id; the position of the vertex will be
the point on the specified entity which is closest to the position specified on the command. With all of these commands,
the user is able to specify the color of the vertex.
To create a Vertex by specifying the XYZ location
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Vertex.
Click on the Create action button.
Select Coordinates from the drop-down menu.
Enter in the appropriate values for X Coordinate, Y Coordinate and Z Coordinate.
Select Curve or Surface from the Create On menu.
Enter in the appropriate values for Curve ID or Surface ID. This can also be done using the Pick Widget
function.
Optionally, specify the color.
Click Apply.
Create Vertex <x><y><z> [On [Curve | Surface] <id>] [Color <color_name>]
2. On Curve - Fraction: A vertex can be positioned a certain fraction of the arc length along a curve using the second
form of the command.
To create a Vertex from the On Curve options
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Vertex.
Click on the Create action button.
Select On Curve from the drop-down menu.
Enter in the appropriate value for Curve ID(s). This can also be done using the Pick Widget function.
Select Fraction, Distance, Position, Close to Vertex, Segments or Midpoint from the Specify Location
menu.
Enter in the remaining appropriate information for this menu.
Optionally, specify the color.
Click Apply.
Fraction: Divides the selected curve into segments based on the fraction value entered and creates a vertex at the end of
the first segment. Specify from which direction by seleting Start, End or Vertex. For example, create a vertex at .25 (1/4)
the length of a curve.
Distance: Creates a vertex on the selected curve the specified number of units away from the starting point (start, end,
vertex, curve and surface). For example, create a vertex a distance of 2 along a curve with length 5.
Position: Creates a vertex at the location entered into the X,Y and Z coordinates.
Close to Vertex: Creates a vertex on the selected curve at the closest point to a specified vertex.
Segments: Divides the selected curve into a specified number of segments and creates a vertex at each endpoint.
Midpoint: Creates a vertex at the Midpoint of the selected curve.
Vertex 3 in the following example was created with this command:
215
Trelis 15.0 User Documentation
create vertex on curve 1 fraction 0.25 from vertex 1
Figure 1. Create Vertex a Fraction of the length of a Curve
On Curve - General: A more general purpose form of the command is also available for creating vertices on curves:
Create Vertex On Curve <id_list> { MIDPOINT | Start | End | Fraction <val 0.0 to 1.0> [From Vertex
<id> | Start|End] | Distance <val> [From {Vertex|Curve|Surface} <id> | Start|End] | {{Close_To|At}
Location {options} | Position <xval><yval><zval>|{Node|Vertex} <id>} | Extrema [Direction] {options}
[Direction {options}] [Direction {options}] | Segment <num_segs> | Crossing {Curve|Surface} <id_list>
[Bounded|Near] } [Color <color_name>]
It allows the vertex to be created at a fractional distance along the curve, at an actual distance from one of the curves
ends, at the closest location to an xyz position or another vertex, or at a specified distance from a vertex, curve or surface.
You can also preview the location first with the command Draw Location On Curve (where the rest of the command is
identical to the Create Vertex form).
3. From Vertex: Create a vertex from an existing vertex.
Create Vertex from Vertex <id_list> [ On {Curve|Surface} <id> ] [Color <color_name>]
If 'on curve|surface' option is used, the vertex is positioned on that curve or surface. When the 'on curve|surface' is not
used, the new vertex is positioned on the existing vertex.
4. At Arc: Another form simply creates vertices at arc or circle centers.
To create a Vertex in the Center of an Arc
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Vertex.
Click on the Create action button.
Select Arc Center from the drop-down menu.
Enter in the appropriate value for Curve ID(s). This can also be done using the Pick Widget function.
Optionally, specify the color.
Click Apply.
Create Vertex Center Curve <id_list> [Color <color_name>]
5: At Intersection: The last form creates vertices at the intersection of two curves. If the bounded qualifier is used, the
vertices are limited to lie on the curves, otherwise the extensions of the curves are also used to calculate the
intersections. The near option is only valid for straight lines, where the closest point on each curve is created if they do not
actually intersect (resulting in two new vertices).
To create a Vertex at an Intersection
216
Creating Vertices
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Vertex.
Click on the Create action button.
Select At Intersection from the drop-down menu.
Enter in the appropriate values for Curve ID 1 and Curve ID 2. This can also be done using the Pick Widget
function.
Enter in any other appropriate settings from this menu.
Optionally, specify the color.
Click Apply.
Create Vertex AtIntersection Curve <id1> <id2> [Bounded] [Near] [Color <color_name>]
217
Creating Curves
Curves are created by specifying the bounding lower-order topology (i.e. the vertices) and the geometry (shape) of the
curve (along with any parameters necessary for that geometry). There are several forms of this command:
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
Straight
Parabolic, Circular, Ellipse
Spline
Copy
Arc Three
Arc End Vertices and Radius
Arc Center Vertex
Arc Center Angle
From Vertex Onto Curve
Offset
From Mesh Edges
Close_To
Surface Intersection
Projecting onto Surface
Helix
1. Straight: The first form of the command creates a straight line or a line lying on the specified surface. If a surface is
used, the curve will lie on that surface but will not be associated with the surface's topology.
To create a Straight Curve
1.
2.
3.
4.
5.
6.
7.
8.
9.
10.
11.
On the Command Panel, click on Geometry and then Curve.
Click on the Create action button
Select Line from the drop-down menu.
Click on Locations from the Build Using menu.
Click on the Location... button. Another menu will appear.
Select On Surface from the drop-down menu.
Enter in the appropriate value for Surface ID.
Enter in any other desired settings from this menu.
Click Apply.
Click on Vertext ID(s) from the Build Using menu.
In the Vertex ID(s) field, enter in the desired values to be used in creating the curve. This can also be done
using the Pick Widget function. Use the Command Key to select multiple values.
12. Click Apply.
Create Curve [Vertex] <vertex_id> [Vertex] <vertex_id> [On Surface <surface_id>]
Straight curves can be created using an axis. The syntax is as follows:
Create Curve Axis {options}
The length of the axis must be specified. Go to Location, Direction, and Axis Specification to see the axis command
description.
Additionally, several connected straight curves can be created with a single command. The syntax for the polyline
command is as follows:
Create Curve Polyline Location {options} Location {options} ...
Notice that two or more locations are used to define a polyline. See Location, Direction, and Axis Specification for the
location command description.
219
Trelis 15.0 User Documentation
2. Parabolic, Circular, Ellipse: The parabolic option creates a parabolic arc which goes through the three vertices. The
circular and ellipse options create circular and elliptical curves respectively that go through the first and last vertices.
To create a Curve with the Parabolic, Ellipse or Circular options
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Curve.
Click on the Create action button.
Select Conic Section from the drop-down menu.
Enter in the appropriate values for each Vertex. This can also be done using the Pick Widget function.
Select Ellipse, Circular or Parabolic from the Select menu.
Click Apply.
Create Curve [Vertex <vertex_id> [Vertex] <vertex_id> [[Vertex] <vertex_id>
[Parabolic|Circular|ELLIPSE [first angle <val=0> last angle <val=90>]]]
If 'ellipse' is specified, Trelis will create an ellipse assuming the vectors between vertices (1 and 3) and (2 and 3) are
orthogonal. v1-v3 and v2-v3 define the major and minor axes of the ellipse and v3 defines the center point. These vectors
should be at 90 degrees. If not, Trelis will issue a warning indicating the vertices are not sufficient to create an ellipse and
will then default to creating a spiral.
The angle options will specify what portion of the ellipse to create. If none are specified, first angle will default to 0 and
last angle to 90 and the ellipse will go from vertex 1 to vertex 2; if the vertices are free vertices they will be consumed in
the ellipse creation. First angle tells Trelis where to start the ellipse -- the angle from the first axis (v1 - v3)
specified. Last angle tells Trelis where to end the ellipse -- the angle from the first axis. The angle follows the right-hand
rule about the normal defined by (v1 - v3) X (v2 - v3).
3. Spline: The spline form of the command creates a spline curve that goes through the all input vertices or locations. To
create a curve from a list of vertices use the syntax shown below. The delete option will remove all of the intermediate
vertices used to create the spline leaving only the end vertices.
To create a Spline Curve
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Curve.
Click on the Create action button.
Select Spline from the drop-down menu.
Click on Vertex.
Enter in the desired values for Vertex ID(s). This can also be done using the Pick Widget function. Use the
command key to select multiple value.
Check the Delete Internal Vertices box.
Click Apply.
Create Curve [Vertex] <vertex_id_list> [Spline] [Delete]
Additionally, spline curves can be created by inputting a list of locations. Where the spline will pass through all of the
specified locations. The syntax is shown below:
Create Curve Spline {List of locations}
See Location, Direction, and Axis Specification to view the location specification syntax.
4. Copy: This command actually copies the geometric definition in the specified curve to the newly created curve. The
new curve is free floating.
220
Creating Curves
Create Curve From Curve <curve_id>
5. Combine Existing Curves: This command creates a new curve from a connected chain of existing ACIS curves.
To combine existing Curves
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Curve.
Click on the Create action button.
Select Combine from the drop-down menu.
Enter in the appropriate values in the Curve ID(s) field. This can also be done using the Pick Widget function.
Click Apply.
Create Curve combine curve <id_list> [delete]
6. Arc Three: The following command creates an arc either through 3 vertices or tangent to 3 curves. The Full qualifier
will cause a complete circle to be created.
To create an Arc through 3 Vertices or Curves
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Curve.
Click on the Create action button.
Select Arc or Circle from the drop-down menu.
Select 3 Vertices from the Build Using menu.
Enter in the appropriate in the Vertex ID(s) field. This can also be done using the Pick Widget function.
Click Apply.
Create Curve Arc Three {Vertex|Curve} <id_list> [Full]
7. Arc End Vertices and Radius: The following command creates an arc using two vertices, the radius and a normal
direction. The Full qualifier will cause a complete circle to be created.
To create a Curve with Vertices and Radius
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Curve.
Click on the Create action button.
Select Arc or Circle from the drop-down menu.
Select Vertices and Radius from the Build Using menu.
Enter in the appropriate ID values for Start Vertex and End Vertex. This can also be done using the Pick
Widget funcion.
Enter in the appropriate values for Radius and Normal. The Normal... button opens a separate window to
apply specific settings.
Click Apply.
Create Curve Arc Vertex <id_list>
Radius <value> Normal {<x> <y> <z> | {direction options} [Full]
Go to Location, Direction, and Axis Specification to see the direction command description.
8. Arc Center Vertex: The next form of the command creates an arc using the center of the arc and 2 points on the arc.
The arc will always have a radius at a distance from the center to the first point, unless the Radius value is given. Again,
the Full qualifier will cause a complete circle to be created.
To create an Arc Center Vertex
1.
2.
3.
4.
On the Command Panel, click on Geometry and then Curve.
Click on the Create action button.
Select Arc or Circle from the drop-down menu.
Select Vertex Center Point from the Build Using menu.
221
Trelis 15.0 User Documentation
5.
6.
7.
Enter in the appropriate ID values for Center Vertex, Start Vertex and End Vertex. This can also be done
using the Pick Widget function.
Enter in the appropriate values for Radius and Normal. The Normal... button opens a separate window to
apply specific settings.
Click Apply.
Create Curve Arc Center Vertex <center_id> <end1_id> <end2_id>
[Radius <value>] [Full]
[Normal {<x> <y> <z> | {direction options}]
Go to Location, Direction, and Axis Specification to see the direction command description.
Note: Requires 3 Vertices - first is the center, the other two are the end points of the arc. A normal direction is required
when the three points are colinear. Otherwise a normal direction is optional.
9. Arc Center Angle: This form of the command creates an arc using the center position of the arc, the radius, the normal
direction and the sweep angle.
To create an Arc using Arc Center Angle
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Curve.
Click on the Create action button.
Select Arc or Circle from the drop-down menu.
Select Center Angle from the Build Using menu.
Enter in the appropriate values for Radius, Start Angle and Stop Angle.
Enter in the appropriate values for Center and Normal. The Normal... and Center... buttons open a separate
window to apply specific settings.
Click Apply.
Create Curve Arc Center {<x=0> <y=0> <z=0> | {location options}
Radius <value>
Normal {<x> <y> <z> | {direction options}
Start Angle <value=0> Stop Angle <value=360>
Go to Location, Direction, and Axis Specification to see the location and direction command descriptions.
10. From Vertex Onto Curve: The following command will create a curve from a vertex onto a specified position along a
curve. If none of the optional parameters are given, the location on the curve is calculated as using the shortest distance
from the start vertex to the curve (i.e., the new curve will be normal to the existing curve).
Create Curve From Vertex <vertex_id> Onto Curve <curve_id> [Fraction <f> | Distance <d> | Position
<xval><yval><zval> | Close_To Vertex <vertex_id> [[From] Vertex <vertex_id> (optional for 'Fraction'
& 'Distance')]] [On Surface <surface_id>]
Note: Default = Normal to the Curve
11. Offset: The next command creates curves offset at a specified distance from a planar chain of curves. The direction
vector is only needed if a single straight curve is given. The offset curves are trimmed or extended so that no overlaps or
gaps exist between them. If the curves need to be extended the extension type can be Rounded like arcs, Extended
tangentially (the default -straight lines are extended as straight lines and arcs are extended as arcs), or extended
naturally.
To create Offset Curves
1.
2.
3.
4.
5.
222
On the Command Panel, click on Geometry and then Curve.
Click on the Create action button.
Select Offset from the drop-down menu.
Enter in the appropriate value for Curve ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate values in the Distance field.
Creating Curves
6.
7.
8.
Select Extended, Rounded or Natural from the Select menu.
Enter in the appropriate values for Direction. The Direction... button opens a separate window to apply specific
settings.
Click Apply.
Create Curve Offset Curve <id_list> Distance <val> [Direction <x> <y> <z>]
[Rounded|EXTENDED|Natural]
Note: Direction is optional for offsets of individual straight curves only
In all cases, the specified vertices are not used directly but rather their positions are used to create new vertices.
12. From Mesh Edges: This commands creates a curve from an existing mesh given a starting node and an adjacent
edge.
Create Curve From Mesh Node <id> Edge <id> [Length <val>]
The adjacent edge indicates which direction to propagate the curve.
The curve will be composed of mesh edges up to the specified length.
If no length is specified the curve will propagate as far as the boundary of the mesh. Figure 1 shows a example of a curve
generated from the mesh.
Figure 1. Example of curve created from mesh
The underlying geometry kernel used for this command is Mesh-Based geometry. The new curve will also be meshed with
the edges it was propagated through. A related command for assigning mesh edges directly to a mesh block is the Rebar
command. See Element Block Specification for more details.
Note: Full hexes or full tets must be used to propagate the curves through the interior of volume.
13. Close_To This option takes two geometric entities and creates the shortest possible curve between the two entities at
the location where the two entities are the closest. The two entities may NOT intersect. If two vertices are given, the
command will create a straight line between the two vertices.
Create Curve Close_To {Vertex|Curve|Surface|Volume|Body} <id_1>
{Vertex|Curve|Surface|Volume|Body} <id_2>
14. Surface Intersection The following command creates curves at surface intersections. Multiple curves can be created
from a single command.
223
Trelis 15.0 User Documentation
Create Curve Intersecting Surface <id_list>
15. Projecting onto a Surface The project command allows you to make an imprint of a surface or set of curves onto
another surface. The command syntax is as follows:
To project a Curve onto a Surface
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Curve.
Click on the Create action button.
Select Project from the drop-down menu.
Enter in the appropriate ID values for Curve ID(s) and Onto Surface ID(s). This can also be done using the
Pick Widget function.
Select either Imprint or Trim and any other appropriate settings.
Click Apply.
Project Curve <id_list> Onto Surface <surface_id> [Imprint [Keepcurve] [Keepbody]] [Trim]
Project Surface <id_list> Onto Surface <surface_id> [Imprint [Keepcurve] [Keepbody]]
The command takes a list of curves or surfaces, and a projection surface. If a list of curves is given, the result will be the
creation of a set of free curves on top of the projection surface. If a list of surfaces is given, the result will be the same as
selecting the curves that bound the surface (i.e. a group of free curves on the projecting surface).
The imprint option will imprint the resulting projected curves onto the projection surface. If this option is NOT given, the
new curves will lie coincident to the surface, but will not be part of the surface. Imprinting changes the topology of the
projection surface. Keepcurve option retains the new curves as both free curves, and curves in the projection surface. The
keepbody option retains the original body under the new imprinted body. When projecting curves, the trim option will
cause the curve to be trimmed to the target surface.
16. Creating a Helix: This command will create a helical curve. The command syntax is as follows:
To create a Helix
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Curve.
Click on the Create action button.
Select Helix from the drop-down menu.
Select an Axis from the Axis of Rotation menu
Enter in the appropriate values for Origin. The Origin... button opens a separate window to apply specific
settings.
Enter in the appropriate values for Helix Height and Angle.
Select Right-handed or Left-handed.
Click Apply.
Create Curve Helix { axis <xpoint ypoint zpoint xvector yvector zvector> | xaxis | yaxis | zaxis } location
(options) thread_distance <value> angle <value> [RIGHT_HANDED | left_handed]
axis = axis about which to create the helix
location (options) = starting point of the helix
thread_distance = distance between each 360 degree segment of the helix
angle = number of degrees in rotation of the helix
handedness = right-handed or left- handed threads
224
Creating Surfaces
There are two major ways to create surfaces in Trelis. First, surfaces can be created in Trelis by fitting an analytic or
spline surface over a set of bounding curves. In this case, the curves must form a closed loop, and only one loop of
curves may be supplied. The second method, is by sweeping a curve about an axis, along a vector, or along another
curve. The result of these surface creation commands is a "sheet body" or a body that has zero measurable volume (it
does however have a volume entity). This body may be decomposed with booleans and special webcutting commands or
it may be used as a tool to decompose other bodies. Booleans can be used to cut holes out of these surfaces.
The following options may be used for creating a surface in Trelis.
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
Bounding Curves
Bounding Vertices or Nodes
Copy
Extended Surface
Planar Surface
Net Surface
Offset
Skinning
Sweeping of Curves
Midsurface
Weld Profile
Meshed Entities
Circular Surface
Parallelogram
Ellipse
Rectangle
1. Bounding Curves: The first form of this command produces an analytic or spline surface fit to cover the bounding
curves.
To create a Surface by Bounding Curves
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Bounding Curves from the drop-down menu.
Enter in the appropriate values in the Curve ID(s) field. This can also be done using the Pick Widget function.
Click Apply.
Create Surface Curve <curve_id_1> <curve_id_2> <curve_id_3>...
Another version of this command creates a surface from a set of bounding curves that all lie on one surface. If the curves
are selected they must lie on the surface, and they must create a closed loop. The On Surface option forces the surface
to match the geometry of the underlying surface exactly.
Bound Curves with On Surface option
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Bounding Curves from the drop-down menu.
Click on the On Surface button.
Enter in the appropriate values for Curve ID(s) and On Surface. This can also be done using the Pick Widget
function.
Click Apply.
Create Surface Curve <id_list> On Surface <surface_id>
225
Trelis 15.0 User Documentation
2. Bounding Vertices or Nodes: The second form of this command uses vertices to fit an analytic spline surface. The
On Surface option creates the surface from a set of nodes and vertices that all lie on one surface and restrains the
surface to match the geometry of the underlying surface. The project option will project the nodes or vertices to the
specified surface.
To create a Surface by bounding Vertices or Nodes
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Vertex List from the drop-down menu.
Select Vertex or Node from the Select menu.
Enter in the appropriate value for Vertex ID(s) or Node ID(s). This can also be done using the Pick Widget
function.
Click on the On Surface button and enter the appropriate value in for Surface ID.
Click Apply.
Create Surface [Node|Vertex| <id_list> [On Surface <surface_id> {Project} ]
3. Copy: The next form creates a surface using the same geometric description of the specified surface. The new surface
will be a stand-alone sheet body that is geometrically identical to the user supplied surface.
To create a Surface by making a Copy
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Copy from the drop-down menu.
Enter in the appropriate value for Surface ID(s). This can also be done using the Pick Widget function.
Click on Transform Copied Surfaces and select Move, Rotate, Reflect or Scale.
Enter in the appropriate settings.
Click Apply.
Create Surface From Surface <surface_id>
4. Extended Surface: The fourth form of the command creates a surface that is extended from a given surface or list of
surfaces. The specified surface's geometry is examined and extended out "infinitely" relative to the current model in Trelis
(i.e. extended to just beyond the bounding box of the entire model). The given surfaces are extended as shown in the
table.
To create a Surface by Extending a Surface
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Extended Surface from the drop-down menu.
Enter in the appropriate value for Surface ID(s). This can also be done using the Pick Widget function.
Enter in any other appropriate settings.
Click Apply.
Create Surface Extended From Surface <surface_id>
Table 1. Surface Extension Results
Surface Type
Resulting Extended Surface
Spherical
Shell of Full Sphere
226
Creating Surfaces
Planar
Plane of infinite size relative to model
Toroidal
Shell of Full Torus
Conical, cone, cylinder...
Shell of outside conic axially aligned with given conic of infinite
height relative to model
Spline
Surface is extended to extents of the spline definition. This may not
be any further than the surface itself, so caution should be used
here.
Multiple surfaces can be offset at the same time to form a sheet body, by using the Create Sheet Extended from Surface
command.
5. Planar Surface: The following commands create planar surfaces. The first passes a plane through 3 vertices, the
second uses an existing plane, the third creates a plane normal to one of the global axes, and the fourth creates a plane
normal to the tangent of a curve at a location along the curve. By default, the commands create the surface just large
enough to intersect the bounding box of the entire model with minimum surface area. Optionally, you can give a list of
bodies to intersect for this calculation. You can also extend the size of the surface by either a percentage distance or an
absolute distance of the minimum area size. The plane can be previewed with the command Draw Plane [with]... (where
the rest of the command is the same as that to create the surface).
To create a Planar Surface through 3 vertices
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Planar Surface from the drop-down menu.
Select Vertex from the Create Planar Surface With Plane menu.
Enter in the appropriate values for Vertex ID 1, 2 and 3. This can also be done using the Pick Widget function.
Enter in any other appropriate settings from this menu.
Click Apply.
Create Planar Surface [With] Plane Vertex <v1_id> [Vertex] <v2_id> [Vertex] <v3_id> [Intersecting]
Body <id_range>] [Extended Percentage|Absolute <val>]
To create a Planar Surface using an Existing Plane
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Planar Surface from the drop-down menu.
Select Surface from the Create Planar Surface With Plane menu.
Enter in the appropriate value for Surface ID. This can also be done using the Pick Widget function.
Enter in any other appropriate settings from this menu.
Click Apply.
Create Planar Surface [With] Plane Surface <surface_id> [Intersecting] Body <id_range>] [Extended
Percentage|Absolute <val>]
To create a Planar Surface normal to one of the global axes
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Planar Surface from the drop-down menu.
Select XYZ from the Create Planar Surface With Plane menu.
Select XY Plane, ZX Plane or YZ Plane from the select menu.
Enter in the desired Offset Value.
Enter in any other appropriate settings from this menu.
Click Apply.
227
Trelis 15.0 User Documentation
Create Planar Surface [With] Plane {Xplane|Yplane|Zplane} [Offset <val>] [Intersecting] Body
<id_range>] [Extended Percentage|Absolute <val>]
To create a Planar Surface normal to curve
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Planar Surface from the drop-down menu.
Select Normal To Curve from the Create Planar Surface With Plane menu.
Enter in the appropriate Curve ID value. This can also be done using the Pick Widget function.
Select Fraction, Distance, Position or Near Vertex from the Select menu.
Enter in any other appropriate settings from this menu.
Click Apply.
Create Planar Surface [With] Plane Normal To Curve <curve_id>{Fraction <f>| Distance <d> |
Position <xval><yval><zval> | Close_to vertex <vertex_id>} [[From] Vertex <vertex_id> (optional for
'fraction' & 'distance')] [Intersecting] Body <id_range>] [Extended Percentage|Absolute <val>]
6. Net Surface: Net surfaces can be created with two different commands. A net surface passes through a set of curves
in the u-direction and a set of curves in the v-direction (these u and v curves would looked like a mapped mesh). The first
form of the command uses curves to create the net surface. The curves must pass within tolerance of each other to work.
The second form uses a mapped mesh to create the surface. The mapped mesh can be of a single surface or a collection
of mapped or submapped surfaces that form a logical rectangle. By default net surfaces are healed to take advantage of
any possible internal simplification.
To create a Net Surface from UV curves
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Net Surface from the drop-down menu.
Select From UV Curve from the select menu.
Enter in the appropriate values for U Curve ID(s) and V Curve ID(s). This can also be done using the Pick
Widget function.
Enter in any other appropriate settings from this menu.
Click Apply.
Create Surface Net U Curve <id_list> V Curve <id_list> [Tolerance <value>] [HEAL|Noheal]
To create a Net Surface from Mapped Surface
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Net Surface from the drop-down menu.
Select Mapped Surface from the select menu.
Enter in the appropriate value for Surface ID(s). This can also be done using the Pick Widget function. The
surface must be meshed.
Enter in any other appropriate settings from this menu.
Click Apply.
Create Surface Net [From] [Mapped] Surface <id_list> [Tolerance <value>] [HEAL|Noheal]
A suggested geometry cleanup method is to use a virtual composite surface to map mesh a set of complicated surfaces
then create a net surface from this mesh. Then the original surfaces can be removed with the noextend option and the
new net surface combined back onto the body.
7. Offset: The following command creates surfaces offset from existing surfaces at the specified distances.
To create a Surface offset from an Existing Surface
228
Creating Surfaces
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Offset from the drop-down menu.
Enter in the appropriate value for From Surface ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate value for Offset Value.
Enter in any other approrpriate settings from this menu.
Click Apply.
Create Surface Offset [From] Surface <id_list> Distance <val>
The surface offset command will only translate the existing surfaces, without extending or trimming them. An alternate
form of the command for sheet bodies will maintain connections between surface by extending or trimming as they are
offset, shown in Figure 1. On the left, the surfaces are offset using the surface offset command. On the left, the surface is
created by using the "sheet" version of the command.
Figure 1. Offsetting surfaces to form individual surfaces or sheet bodies
8. Skinning: The following command creates a skin surface from a list of curves. An example of a skin surface is to
create a surface through a set of parallel lines.
To create a Surface by Skinning
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Skin Curve from the drop-down menu.
Enter in the appropriate values for Curve ID(s). This can also be done using the Pick Widget function.
Click Apply.
Create Surface Skin Curve <id_list>
9. Sweeping of Curves: A curve or a set of curves can be swept along a path to create new surfaces. The path may be
specified as an axis and angle, a vector and distance, by indicating another curve or set of contiguous curves, or by
specifying a target plane. The following commands show the options available:
To sweep a Curve along an Axis
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Sweep from the drop-down menu.
Select Axis/Angle from the Sweep Method menu.
Enter in the appropriate value for Curve ID(s). This can also be done using the Pick Widget function.
Select the appropriate Axis from the Axis of Rotation menu.
Enter in the appropriate values for Angle and Steps.
229
Trelis 15.0 User Documentation
8.
9.
Enter in any other appropriate settings from this menu.
Click Apply.
Sweep Curve <curve_id_range> { Axis <xpoint ypoint zpoint xvector yvector zvector> | Xaxis | Yaxis |
Zaxis } Angle <degrees> [Steps <Number_of_sweep_steps>] [Draft_angle <degrees>] [Draft_type
<integer>] [Make_solid] [Include_mesh] [Keep][Rigid]
To sweep a Curve using a Vector
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Sweep from the drop-down menu.
Select Vector and Distance from the Sweep Method menu.
Enter in the appropriate value for Curve ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate values in the Vector X,Y,Z field.
Enter in any other appropriate settings from this menu.
Click Apply.
Sweep Curve <curve_id_range> Vector <xvector yvector zvector> [Distance <distance>] [Draft_angle
<degrees>] [Draft_type <integer>] [Include_mesh] [Keep] [Rigid]
To sweep a Curve along Curve
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Sweep from the drop-down menu.
Select Along Curve from the Sweep Method menu.
Enter in the appropriate value for Curve ID(s). This can also be done using the Pick Widget function.
Enter in any other appropriate settings from this menu.
Click Apply.
Sweep Curve <curve_id_range> Along Curve <refcurve_id_range> [Draft_angle <degrees>]
[Draft_type <integer>] [Include_mesh] [Keep] [Rigid]
To sweep a Curve using a Target Volume
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Sweep from the drop-down menu.
Select Target Volume from the Sweep Method menu.
Enter in the appropriate values for Volume ID and Curve ID(s). This can also be done using the Pick Widget
function.
Enter in the appropriate settings for Direction. Click on the Direction... button to open a separate window to
specify settings.
Enter in the appropriate settings for Plane. Click on the Plane... button to open a separate window to specify
settings.
Click Apply.
Sweep Curve <curve_id_range> Target Plane <options>
Sweep Curve <curve_id_range> Target {Volume|Body} <id> Direction {options} [Plane <options>]
[Unite]
In the first command, the steps options provides a way of faceting the sweep, so instead of a smooth round sweep, there
are facets to the surface. The make_solid option closes the newly-created surface to the axis, so that a solid is created
instead of a surface.
230
Creating Surfaces
In the above commands, the include_mesh option will create a surface mesh if the curve is already meshed (see figure
below). The keep option will keep the original curve while creating the surface.
The sweep curve target plane command sweeps a curve until it hits a target plane. The options for the target plane are
described under Specifying a Plane.
The last command sweeps a curve to a target volume or body and can only be used on sheet bodies. Use the direction
keyword to specify the sweep direction and the plane keyword to specify a stopping plane. The unite keyword will unite
the sheet bodies after sweeping
The other options are as follows:
draft_angle: determines how much drafting in of the surface is desired
draft_type:
0 => extended (draws two straight tangent lines from the ends of each segment until they intersect)
1 => rounded (create rounded corner between segments)
2 => natural (extends the shapes along their natural curve) ***
rigid: normally the curve will rotate to maintain its original orientation to the sweep path. The rigid option disallows this
rotation.
10. Midsurface: Multisurfaces may be created midway between pairs of surfaces using the following command:
To create a Surface midway between pairs
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Midsurface from the drop-down menu.
Enter the appropriate values for Volume ID and Surface ID Pairs. This can also be done using the Pick
Widget function.
Click Apply.
Create Midsurface {Body|Volume} <id> Surface <id11> <id12> ... <idN1> <idN2>
where N denotes the number of pairs of surfaces. An even number of surfaces must be specified, and the command will
group them by pairs in the order in which they are provided. The resulting surface will be trimmed by the specified body or
volume <id>. This replaces the Create Midplane command in previous versions of Trelis.
231
Trelis 15.0 User Documentation
Figure 2. Multisurface created with the Create Midsurface command
232
Creating Surfaces
Figure 3. Midsurface created from 2 pairs of cylindrical surfaces
Midsufaces can also be extracted without surface pair specification if the resulting surface is a single sheet of surfaces (no
T intersections).
For automatic midsurface extraction
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Auto Midsurface from the drop-down menu.
Enter the appropriate values for Volume ID(s). This can also be done using the Pick Widget function.
Enter the appropriate values for Lower Bounds and Upper Bounds.
Enter in any other appropriate settings from this menu.
Create Midsurface {Body|Volume} <id_range> Auto [Delete] [Transparent] [Thickness] [Limit
<lower_bound> <upper_bound>] [Preview]
Figure 4 shows a simple auto midsurface example. The command for the example is:
create midsurface volume 1 auto delete
233
Trelis 15.0 User Documentation
Figure 4. Midsurface created from a volume
The command option descriptions are listed below.
Auto enables the automatic mid-surface algorithm. Turning Auto off requires the user to specify a single surface pair to
create a mid-surface.
Transparent shows the successfully midsurfaced volumes as transparent in the graphics display
Thickness applies a 2D property to the created mid-surface geometry.
Limit search range gives the algorithm a range to find surface pairs within.
11. Weld Profile: Surfaces may be created by specifying a weld profile using the following command:
Create Surface Weld [Root] Location {options} Weld Surface <id_list> Length <val> [<val2>]
Weld surfaces can be used to create a simulated welded joint by sweeping the surface along the root curve and uniting
the new body to the model. An example of the command is illustrated below. For a detailed description of the location
specifier see Location Direction, and Axis Specification.
create surface weld root location vertex 25 weld surface 13 14 length 2
234
Creating Surfaces
Figure 5. Weld Profile surface with length and root specifications
12. Creating A Surface From Mesh Entities: Surfaces may be created from the boundaries of meshed volumes,
surfaces, and/or from individual quadrilateral mesh elements. The individual option makes it so you can enter multiple
surfaces at once, and not have them merged together into a larger surface, but instead retain their own original
boundaries. The optional tolerance value allows the user to specify a tolerance to which the resulting surface should be fit.
The default value is 0.001. If surface creation fails, increasing the tolerance value can help.
Create Acis [From] {Surface <id_range> | Volume <id_range> | Face < id_range> [Individual]}
[Tolerance <value>]
Figure 6. Acis Surface created from a Set of Quadrilaterals
13. Creating a Circular Surface: This command creates a 2D circular surface. The surface will be centered at the origin
and on the z-plane if a plane option is not specified.
To create a Cirular Surface using a radius
1.
2.
3.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Circle from the drop-down menu.
235
Trelis 15.0 User Documentation
4.
5.
6.
7.
Select Radius from the Specify Circle Using menu.
Enter in the appropriate Radius value.
Select XPlane, YPlane or ZPlane.
Click Apply.
create surface circle radius <value> {xplane|yplane|ZPLANE}
This command creates a 2D circular surface by specifying three vertices; the first vertex will be the center of the surface,
the second vertex will be used to define the radius of the surface, and the third vertex will assist in defining the plane that
the surface will lie in.
To create a 2D circular surface by specifying three vertices
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Circle from the drop-down menu.
Select Center Vertex from the Specify Circle Using menu.
Enter in the appropriate values for Center, Vertex 1 and Vertex 2. This can also be done using the Pick
Widget function.
Click Apply.
create surface circle center vertex <v1_id> <v2_id> <v3_id>
This command creates a 2D circular surface by forming a circular curve through three points.
To create a 2D circular surface by forming a circular curve through three points.
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Circle from the drop-down menu.
Select Vertex List from the Specify Circle Using menu.
Enter in the appropriate values for Vertex 1, Vertex 2 and Vertex 3. This can also be done using the Pick
Widget function.
Click Apply.
create surface circle vertex <v1_id> <v2_id> <v3_id>
14. Creating a Parallelogram: This command creates a 2D parallelogram surface, centered at the origin, by specifying
three corner vertices. These vertices will form three consecutive corners of the parallelogram surface.
To create a 2D parallelogram surface
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Parallelogram from the drop-down menu.
Enter in the appropriate values for Vertex 1, Vertex 2 and Vertex 3. This can also be done using the Pick
Widget function.
Click Apply.
create surface parallelogram vertex <v1_id> v2_<id> <v3_id>
15. Creating an Ellipse: This command creates a 2D elliptical surface, centered at the origin, by specifying at least a
major radius. On an x-y plane this radius will be the radius along the x-direction. The minor radius will be the radius
along the y-direction. By default, the surface will lie in the z-plane.
To create a 2D elliptical surface
236
Creating Surfaces
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Ellipse from the drop-down menu.
Select Radius from the Specify Ellipse Using menu.
Enter in the appropriate values for Major Radius and Minor Radius.
Select XPlane, YPlane or ZPlane.
Click Apply.
Create Surface Ellipse major radius <value> [minor radius <value>] [xplane|yplane|ZPLANE]
This command creates a 2D elliptical surface using three vertices. The first two vertices define the major and minor radii
of the ellipse surface. The third point defines the center of the ellipse. It is important to note that a line from v1_id to
v3_id must be orthogonal to a line from v2_id to v3_id, otherwise the command will fail.
To create a 2D elliptical surface using three vertices
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Ellipse from the drop-down menu.
Select Vertex List from the Specify Ellipse Using menu.
Enter in the appropriate values for Axis 1 Vertex ID, Axis 2 Vertex ID and Origin Vertex ID. This can also be
done using the Pick Widget function.
Click Apply.
Create Surface Ellipse vertex <v1_id> <v2_id> <v3_id>
16. Creating a Rectangle: This command creates a rectangular surface centered at the origin. If only a width value is
specified, the surface will be a square. On an x-y plane, the width value is the x-direction and the height is the ydirection. By default, the surface will lie in the z-plane.
To create a rectangular surface centered at the origin
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Rectangle from the drop-down menu.
Enter in the appropriate values for Width and Height (Optional).
Select XPlane, YPlane or ZPlane.
Click Apply.
Create Surface rectangle width <value> [height <value>] [xplane|yplane|ZPLANE]
237
Creating Volumes
Currently, Trelis can create volumes:
1.
2.
3.
4.
5.
6.
7.
from surfaces by sweeping a single surface into a 3D solid,
by offsetting an existing volume,
by extending one or more surfaces or sheet bodies
by sweeping a curve around an axis,
by stitching together surfaces that can form a closed volume,
by lofting from one surface to another surface, or
by thickening a surface body.
Sweeping of planar surfaces, belonging either to two- or three-dimensional bodies, is allowed, and some non-planar faces
can be swept successfully, although not all are supported at this time. The following methods for generating volumes are
described:
•
•
•
•
•
•
•
•
•
•
•
•
•
•
Sweep Surface Along Vector
Sweep Surface About Axis
Sweep Surface Along Curve
Sweep Surface Perpendicular
Sweep Surface to a Volume
Offset
Sheet extended from surface
Sweep Curve About Axis
Stitch Surfaces Together
Loft Surfaces Together
Thicken Surfaces
Sweep Surface
Sweep Surface along Direction
Sweep Surface along Helix
There are five forms of the sweep command; the syntax and details for each are given below. Common options for first
four forms are:
draft_angle: This parameter specifies the angle at which the lateral faces of the swept solid will be
inclined to the sweep direction. It can also be described as the angle at which the profile expands or
contracts as it is swept. The default value is 0.0.
draft_type: This parameter is an ACIS-related parameter and specifies what should be done to the
corners of the swept solid when a non-zero draft angle is specified. A value of 0 is the default value
and implies an extended treatment of the corners. A value of 1 is also valid and implies a rounded
(blended) treatment of the corners.
anchor_entity: The default behavior for the sweep command is to move the source surface along a
path to create a new 3D solid. The anchor_entity option instructs the sweep to leave the source
surface in its original location.
include_mesh: This option will sweep the source surface and existing mesh into a meshed 3D solid.
The mesh size is automatically computed using the Default auto interval specification.
The sweep operations have been designed to produce valid solids of positive volume, even though the underlying solid
modeling kernel library that actually executes the operation, ACIS, allows the generation of solids of negative volume (i.e.,
voids) using a sweep.
1. Sweep Surface Along Vector: Sweeps a surface a specified distance along a specified vector. Specifying the distance
of the sweep is optional; if this parameter is not provided, the face is swept a distance equal to the length of the specified
vector. The include_mesh option will create a volumetric mesh if the surface is already meshed as shown below. The
keep option will keep the original surface while creating the volume.
To sweep a Surface
239
Trelis 15.0 User Documentation
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Sweep from the drop-down menu.
Enter the value for theSurface ID(s). This can also be done using the Pick Widget function.
Click on Along Vector.
Enter in the appropriate values for X, Y and Z.
Enter in any other desired options from this menu.
Click Apply.
Sweep Surface {<surface_id_range>} Vector <x_vector y_vector z_vector> [Distance <distance_value>]
[switchside] [Draft_angle <degrees>] [Draft_type <0|1>][rigid][anchor_entity][include_mesh] [keep] [merge]
Surface mesh swept along a vector
2. Sweep Surface About Axis: Sweeps a surface about a specified vector or axis through a specified angle. The axis of
revolution is specified using either a starting point and a vector, or by a coordinate axis. This axis must lie in the plane of
the surfaces being swept. The steps parameter defaults to a value of 0 which creates a circular sweep path. If a positive,
non-zero value (say, n) is specified, then the sweep path consists of a series of n linear segments, each subtending an
angle of [( sweep_angle ) / ( steps-1 )] at the axis of revolution. The include_mesh option will create a volumetric mesh if
the surface is already meshed as shown below. The keep option will keep the original surface while creating the volume.
To sweep a Surface About an Axis
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Sweep from the drop-down menu.
Enter the value for the Surface ID(s). This can also be done using the Pick Widget function.
Click on About Axis.
Select the appropriate Axis of Rotation.
Enter in any other desired options from this menu.
Click Apply.
Sweep Surface {<surface_id_range>} Axis {<xpoint ypoint zpoint xvector yvector
zvector>|Xaxis|Yaxis|Zaxis} Angle <degrees> [switchside] [Steps <number_of_sweep_steps>]
[Draft_angle <degrees>] [Draft_type <0|1>][rigid][anchor_entity][include_mesh] [keep] [merge]
240
Creating Volumes
Surface swept around an axis of 50 degree angle
Specifying multiple surfaces that belong to the same body will not work as expected, as ACIS performs the
sweep operation in place. Hence, if a range of surfaces is provided, they ought to each belong to different bodies.
3. Sweep Surface Along Curve: This command allows the user to sweep a planar surface along a curve:
To sweep a Surface Along a Curve
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Sweep from the drop-down menu.
Enter the value for the Surface ID(s). This can also be done using the Pick Widget function.
Click on Along Curve.
Enter in the Curve ID.
Select any other appropriate settings from this menu.
Click Apply.
Sweep Surface <surface_id_range> Along Curve <curve_id> [Draft_angle <degrees>]
[Draft_type <0 | 1 | 2>][rigid][anchor_entity][include_mesh] [keep] [individual] [merge]
One of the ends of the curve must fall in the plane of the surface and the curve cannot be tangential to the surface. Sweep
along curve also supports an additional draft type "2" which implies a "natural" extension of the corners from their curves.
The include_mesh option will create a volumetric mesh if the surface is already meshed. The keep option will keep the
original surface while creating the volume.
Volume generated by sweeping a surface along a reference curve
241
Trelis 15.0 User Documentation
4. Sweep Surface Perpendicular: This command allows the user to sweep a planar surface perpendicular to the surface:
To sweep a Surface Perpendicular
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Sweep from the drop-down menu.
Enter the value for the Surface ID(s). This can also be done using the Pick Widget function.
Click on Perpendicular.
Enter in the desired Distance.
Enter in any other appropriate settings from this menu.
Click Apply.
Sweep Surface <surface_id_range> Perpendicular Distance <distance> [Switchside]
[Draft_angle <degrees>] [Draft_type <integer>][anchor_entity][include_mesh] [keep] [merge]
The sweeping plane must be planar in order to determine the sweep direction. The switchside option will reverse the
direction of the sweep.
The original surface is retained with the 'keep' option. A new volume is created by sweeping the surface along
the surface normal.
The include_mesh option will create a volumetric mesh if the surface is already meshed. The keep option will keep the
original surface while creating the volume.
5. Sweep Surface to a Volume: This command allows users to sweep a surface to a volume.
To sweep a Surface to a Volume
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Sweep from the drop-down menu.
Enter the value for the Surface ID(s). This can also be done using the Pick Widget function.
Click on Target Volume.
Enter in the appropriate values for Volume ID, Direction and Plane.
Click Apply.
Sweep Surface <surface_id_range> Target {Volume|Body} <id> [Direction {options}] [Plane
{options}]
The direction keyword can be used to control the direction of sweep. Without it, Trelis will determine the sweep direction
(usually normal to the sweeping surface). The plane option can be used to define a stopping plane.
242
Creating Volumes
6. Offset: The following command creates a body offset from another body or set of surfaces at the specified distance.
The new surfaces are extended or trimmed appropriately. A positive distance results in a larger body; a negative distance
in a smaller body.
To create a Sheet Offset from a Surface
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click the Create action button.
Select Offset from the drop-down menu.
Enter in the appropriate values for From Surface ID(s) and Offset Value.
Enter in any other desired settings from this menu.
Click Apply.
Create Body Offset [From] Body <id_range> Distance <value>
Create Sheet Offset From Surface <id_list> Offset <val> [Surface <id_list> Offset <val>] [Surface
<id_list> Offset <val> ...] [Preview]
Using the second form of the command, the sheet body can be created from a list of surfaces, and the surfaces may
offset by different distances. This command currently requires the original surfaces to be on solid bodies.
This option is also available for limited cases for facet-based surfaces.
7. Sheet Extended from Surface: The following command creates a body offset from another body or set of surfaces at
the specified distance. The new surfaces are extended or trimmed appropriately. A positive distance results in a larger
body; a negative distance in a smaller body.
To create a Sheet Extended from a Surface.
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Extended Surface from the drop-down menu.
Enter in the desired value for Surface ID(s).
Enter in any other appropriate settings from this menu.
Click Apply.
Create Sheet Extended From Surface <id_list> [Intersecting <entity_list>] [Extended
{Percentage|Absolute} <val>] [Preview]
This command allows multiple surfaces to be extended at the same time. Optionally, you can give a list of bodies to
intersect for this calculation. You can also extend the size of the surface by either a percentage distance or an absolute
distance of the minimum area size. The plane can be previewed with the preview option. Figure 1 shows a set of surfaces
being created using the extended absolute option.
243
Trelis 15.0 User Documentation
Figure 1. Sheet created from extending multiple surfaces
8. Sweep Curve About Axis: Sweeps a curve or set of curves about a given axis through a specified angle. The axis is
specified the same as in the Sweep Surface About Axis command. The steps, draft_angle, and draft_type options are the
same as are described above. To create the solid, the make_solid option must be specified, otherwise a surface will be
created, rather than a solid. If the rigid option is specified, then the curve or set of curves will remain oriented as originally
oriented, rather than rotating about the axis.
To sweep a Curve about an Axis
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Surface.
Click on the Create action button.
Select Sweep from the drop-down menu.
Enter in the value for the Curve ID(s). This can also be done using the Pick Widget function.
Select Axis/Angle from the Sweep Method Menu.
Enter in the appropriate Axis of Rotation.
Enter in any other desired settings from this menu.
Click Apply.
Sweep Curve <curve_id_range> {Axis <xpoint ypoint zpoint xvector yvector
zvector>|Xaxis|Yaxis|Zaxis} Angle <degrees> [Steps <Number_of_sweep_steps>] [Draft_angle
<degrees>] [Draft_type <integer>] [Make_solid] [Rigid]
9. Stitch Surfaces Together: A body can be created from various surfaces that form a closed volume with command
below. The geometry must be ACIS-type geometry (i.e. imported from IGES, STEP or fastq files) This option is also
available for limited cases for facet-based surfaces.
The heal option will attempt to close small gaps in the surface; the noheal option disables this behavior. The keep option
preserves the original surfaces.
All of the surfaces must form a closed water-tight volume for this command to succeed unless the sheet option is
specified. The sheet option allows for the creation of an open body.
244
Creating Volumes
To create a body with the Heal Option
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select From Bounding Surfaces from the drop-down menu.
Enter the value for the Surface ID(s). This can also be done using the Pick Widget function.
Select any other appropriate setting from this menu.
Click Apply.
Create {Body|Volume} Surface <surface_id_range> [HEAL|Noheal] [Keep] [Sheet]
10. Loft Surfaces Together: A body can be "lofted" between two surfaces to form a new body. Surfaces from solid
bodies and sheet bodies may be used to create a loft body. In order to create the loft body, two surfaces coincident to the
input surfaces are created. The loft body is extruded along the shortest path between the corresponding vertices that
define the shapes of the two copied surfaces. This new body is solid. The surfaces used to create the loft body are
unchanged.
To loft Surfaces to create a Volume
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Lofted Volume from the drop-down menu.
Enter the value for Surface ID(s). This can also be done using the Pick Widget function.
Select an other appropriate settings from this menu.
Click Apply.
Create {Body|Volume} Loft Surface <ids> [guide curve <id_list> [global_guides]]
[Takeoff_factors <one value per surface in order>=.001] [Takeoff_vector Surface <id>
{direction options}] [match vertex <ids>] [closed] [preview] [show_matching_curves]
Note:Source surface ids must be specified in lofting order.
Go to Location, Direction, and Axis Specification to see the direction command description.
The following options are available for lofting:
•
•
•
•
•
•
•
Guide curve: Multiple curves may be specified to guide the loft. The curves must touch each source surface. If
the global_guides option is specified the guides curves are applied in a global nature.
Takeoff_factors: Takeoff factors control how strongly the loft follows the takeoff vectors. When specifying
takeoff factors one value must be specified for each source surface.
Takeoff_vector: The takeoff vector controls the direction of the loft for each surface. The default takeoff vector
for each surface is the normal at the surface centroid. One takeoff vector may be specified for each surface.
Match vertex: This option guides the loft in how to match the vertices of the source surfaces. Multiple match
vertex sets may be specified. When specifying match vertices, one vertex id from each source surface must be
specified. The match vertices must be specified in loft order.
Closed: This option atempts to create a toroidal solid. The last source surface is lofted to the first source
surface.
Preview: This option will preview the linking curves of the final solid.
Show_matching_curves: This option will preview how the vertices of the source surfaces will be matched.
Lofting can be used to split a body in order to create a more structured mesh. Figure 2 below shows a single volume
swept from a large paved surface. Figure 3 shows this same volume after surfaces defined on the source and target
surfaces have been used to create a loft body. This original body was chopped with the loft body. The resulting two bodies
were merged. The yellow volume was swept as the volume in Figure 2 was but the purple volume was submapped,
producing a much more structured mesh overall.
245
Trelis 15.0 User Documentation
Figure 2. Mesh before loft. Single swept volume with a large paved face.
Figure 3. Mesh after loft. The yellow volume is paved and the purple volume is submapped.
11. Thicken Surfaces: A surface body can be thickened to create a volume body. The surface can be thickened in both
directions using the "both" keyword, thickened in the direction of surface normal using a positive depth, or thickened in the
opposite direction using a negative depth. To thicken multiple surfaces, all surface normals must be consistent.
To thicken a Surface
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Volume.
Click on the Modify Volumes action button.
Select Thicken from the drop-down menu.
Enter the appropriate values for Volumes ID(s) and Depth.
To Thicken the volume in both direction, check the Thicken in both directions box.
Click Apply.
Thicken [Volume|BODY] <id> Depth <depth> [Both]
12. Sweeping a Surface to a Plane: Sweeps a surface normal to a plane and towards the plane until the swept surface
reaches the plane. See plane options for ways to describe a plane.
To sweep a Surface to a Plane
1.
2.
3.
4.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Sweep from the drop-down menu.
Enter in the desired values for Surface ID(s) and Volume ID. This can also be done by using the Pick Widget
function.
5. Click on Target Volume.
6. Click on Plane.... Another menu will appear.
7. Enter in the appropriate settings.
8. Click Apply. The menu will disapear leaving the selected settings in the Plane field.
9. Enter in any other desired settings from this menu.
10. Click on Apply.
246
Creating Volumes
Sweep surface <id> target plane <options>
13. Sweep Surface along a Direction: Sweep a surface along a direction to create a volume. See direction options for
ways to specify a direction.
To sweep a Surface along a Direction
1.
2.
3.
4.
5.
6.
7.
8.
9.
10.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Sweep from the drop-down menu.
Enter in the desired values for Surface ID(s). This can also be done using the Pick Widget function.
Click on Direction from the Sweep Method menu.
Click on the Direction... button. Another menu will appear.
Enter in the appropriate settings.
Click Apply. The menu will disapear leaving the selected settings in the Direction field.
Enter in any other desired settings from this menu.
Click Apply.
Sweep Surface <surface_id_range> Direction (options)
[switchside] [draft_angle <degrees>]
[draft_type <integer>] [rigid] [anchor_entity] [include_mesh] [keep] [merge]
Surface extruded along -X direction without 'include_mesh' option
14. Sweep Surface along Helix: Sweep a surface along a helix, where the helix is defined by an axis, thread_distance
(distance between turns in axis direction), axis, and handedness (right_handed or left_handed.
To sweep a Surface or Curve along a Helix
1.
2.
3.
4.
5.
6.
7.
8.
9.
10.
On the Command Panel, click Geometry.
To sweep a surface, click on Volume. To sweep a curve, click on Surface.
Click on the Create action button.
Select Sweep from the drop-down menu.
Enter in the desired Surface or Curve ID(s). This can also be done using the Pick Widget function.
Select Helix from the Sweep Method menu.
Click the appriapte Axis from the Axis of Rotation menu.
Enter in the appropriate values for Helix Height and Rotation Angle.
Enter in any other desired settings
Click Apply.
Sweep {Surface|Curve} <id_range> Helix {axis <xpoint ypoint zpoint xvector yvector zvector> | xaxis |
yaxis | zaxis} thread_distance <val> angle <val> [RIGHT_HANDED|left_handed] [anchor_entity]
[include_mesh] [keep] [merge]
*** Specifying multiple Surfaces that belong to the same Body can cause the creation of invalid Bodies and is
discouraged. ***
247
Trelis 15.0 User Documentation
axis = axis about which to create the sweep
thread_distance = distance between each 360 degree segment of the helix
angle = number of degrees in rotation of the helix
handedness = right-handed or left- handed threads
Helical Sweep
248
Creating Bricks
The brick is a rectangular parallelepiped. A cubical brick is created by specifying only the width or x dimension.
To create a Brick
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Brick from the drop-down menu.
Enter in the desired values for the Brick Dimensions.
Click Apply.
A brick can be specified to occupy the bounding box of one or more entities, specified on the command line.
To create a Bounding Box
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Bounding Box from the drop-down menu.
Select the volume to be bounded.
Enter the appropriate settings.
Click Apply.
If the Tight option is specified with Bounding Box, the result is the smallest brick that can contain the entities specified,
which is the default behavior of the Bounding Box option.
If the Extended option is specified with Bounding Box, the result is a brick that is extended from a "tight" brick by the
input percentage or absolute value.
If a bounding box specification is used in conjunction with any of the other parameters (X, Y or Z), the parameters
specified override the bounding box results for that or those dimensions.
Command
[Create] Brick {Width|X} <width> [{Depth|Y} <depth>] [{Height|Z} <height>] [Bounding Box
{entity_type} <id_range>] [Tight] [[Extended] {Percentage| Absolute} <val>]]
249
Creating Cylinders
The cylinder is a constant radius tube with right circular ends.
To create a Cylinder
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Cylinder from the drop-down menu.
Enter in the desired values for Height and Radius.
Select Circular or Elliptical.
Click Apply.
Command
[Create] Cylinder [Height|Z] <val> Radius <val>
[Create] Cylinder [Height|Z] <val> Major Radius <val> Minor Radius <val>
Notes
•
•
A cylinder may also be created using the frustum command with all radii set to the same value.
Specifying major and minor radii can produce a cylinder with an oval cross section.
251
Creating Prisms
The prism is an n-sided, constant radius tube with n-sided planar faces on the ends of the tube.
To create a Prism
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Prism from the drop-down menu.
Enter in the desired values for Height, Number of Sides and Radius.
Select Circular or Elliptical.
Click Apply.
Command
[Create] Prism [Height|Z] <z-val> Sides <nsides> Radius <radius>
Notes
•
•
•
•
•
The radius defines the circumradius of the n-sided polygon on the end caps.
If a major and minor radius are used, the end caps are bounded by a circum-ellipse instead of a circumcircle.
The number of sides of a prism must be greater than or equal to three. A prism may also be created using the
pyramid command with all radii set to the same value.
If the Extended option is specified with Bounding Box, the result is a brick that is extended from a "tight" brick
by the input percentage or absolute value.
If a bounding box specification is used in conjunction with any of the other parameters (X, Y or Z), the
parameters specified override the bounding box results for that or those dimensions.
253
Creating Frustums/Cones
A frustrum is a general right elliptical cone with a top radius greater than 0.
To create a Cone or Frustrum
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Cone from the drop-down menu.
Enter in the desired values for Height, Top Radius and Radius.
Select Cirular or Elliptical.
Click Apply.
Command
[Create] Frustum [Height|Z] <z-height> Radius <x-radius> [Top <top_radius>]
[Create] Frustum [Height|Z] <z-height> Major Radius <radius> Minor Radius <radius> [Top
<top_radius>]
Notes
•
•
If used, Major Radius defines the x-radius and Minor Radius the y-radius.
If used, Top Radius defines the x-radius at the top of the frustum; the top y radius is calculated based on the
ratio of the major and minor radii.
255
Creating Pyramids
A pyramid is a general n-sided prism.
To create a Pyramid
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Pyramid from the drop-down menu.
Enter the desired values for Height, Number of Sides and Top Radius.
Select Circular or Elliptical.
Enter the desired value for the Radius.
Click Apply.
Command
[Create] Pyramid [Height|Z] <z-height> Sides <nsides> Radius <radius> [Top <top-x-radius>]
[Create] Pyramid [Height|Z] <z-height> Sides <nsides> [Major [Radius] <x-radius> Minor
[Radius] <y-radius> ] [Top <top-x-radius>]
257
Creating Spheres
The sphere command generates a simple sphere, or, optionally, a portion of a sphere or an annular sphere.
To create a Sphere
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Volume.
Click on the Create action button.
Select Sphere from the drop-down menu.
Enter the desired value for the Radius.
Fill out any other desired values or options on the menu.
Click Apply.
Command
[Create] Sphere Radius <radius> [Xpositive]|[Xnegative] [Ypositive]|[Ynegative]
[Zpositive]|[Znegative] [Delete] [Inner [Radius] <radius>]
Notes
•
•
If Xpositive/Xnegative, Ypositive/Ynegative, and/or Zpositive/Znegative are used, a sphere which occupies that
side of the coordinate plane only is generated, or, if the delete keyword is used, the sphere will occupy the other
side of the coordinate plane(s) specified. These options are used to generate hemisphere, quarter sphere or a
sphere octant (eighth sphere).
If the inner radius is specified, a hollow sphere will be created with a void whose radius is the specified inner
radius.
259
Creating Toruses
The torus command generates a simple torus
To create a Torus
1.
2.
3.
4.
5.
On the Command Planel, click on Geometry and then Volume.
Click on the Create action button.
Select Torus from the drop-down menu.
Enter the desired values for Major Radius and the Minor Radius.
Click Apply.
Command
[Create] Torus Major [Radius] <major-radius> Minor [Radius] <minor-radius>
Notes
•
•
Minor Radius is the radius of the cross-section of the torus; Major Radius is the radius of the spine of the
torus.
The minor radius must be less than the major radius.
261
Align Command
The align Operation is a combination of the rotate and move Operations. The align Operation will align the surface of a
given volume with any other surface in the model, such that the surface centroids are coincident and the normals are
pointing either in the same or opposite direction (depending on their initial alignment). The align Operation can also align a
face of a volume with the xy, yz, and xz planes and the vertices of a volume with the x, y, and z axes.
To use the Align Operation
1.
2.
3.
4.
5.
On the Commmand Panel, click on Geometry and then Volume.
Click on the Transform action button.
Select Align from the drop-down menu.
Enter the appropriate values for Volume ID(s), Surface ID and With Surface ID. This can also be done using
the Pick Widget function.
Click Apply.
Align Volume <id_range> Surface <surface_id> with Surface <surface_id>
[reverse][include_merged][preview]
Align Volume <id_range> {Surface <surface_id>| Vertex <vertex_id>} {{X|Y|Z Axis}|{XY|XZ|YZ
plane}}
[reverse][include_merged][preview]
Align Volume <id_range> Location {options} with Location {options} about Axis {options}
[include_merged][preview]
The first align command above will transform the specified volumes by computing a transformation that would align the
first surface with the second surface such that the surface centroids are coincident and the normals are pointing either in
the same or opposite direction (depending on their initial alignment). The first surface need not be in the specified
volumes.
The second form of the align command either aligns a face of a volume or two vertices (forming a direction) with the xy,
yz, and xz planes or the x, y, and z axes. If the [reverse] option is specified, the resulting alignment is flipped 180
degrees.
The third form of the command is a rotational alignment, where the specified entities are rotated about the specified axis,
where the angle of rotation is the angle between the first and second locations with respect to the axis.
This transformation is useful for aligning surfaces in preparation for geometry decomposition and aligning models for axissymmetric analysis. If the [include_merged] option is used, all entities that are merged with the specified volume will be
included in the align transformation also.
263
Copy Command
The copy command copies an existing entity to a new entity without modifying the existing entity. A copy can be made of
several entities at once, and the resulting new entities can be translated or rotated at the same time. The options for
copying entities are:
To copy an entity using Move
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry.
Click Volume, Surface, Curve, Vertex or Group.
Click on the Create action button.
Select Copy from the drop-down menu.
Select Move from the Copy Type menu.
Enter in the appropriate settings.
Click Apply.
Vertex <range> Copy [Move [X <dx>] [Y <dy>] [Z <dz>]] [Preview]
Vertex <range> Copy [Move <direction_options> [Distance <val>]] [Preview]
{Body|Volume|Surface|Curve|Vertex|Group} <range> Copy Move [X <dx>] [Y <dy>] [Z <dz>]
[Nomesh] [Repeat <value>] [Preview]
{Body|Volume|Surface|Curve|Vertex|Group} <range> Copy Move <direction_options> [Distance
<val>] [Nomesh] [Repeat <value>] [Preview]
To copy an entity using Reflect
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry.
Click Volume, Surface, Curve, Vertex or Group.
Click on the Create action button.
Select Copy from the drop-down menu.
Select Reflect from the Copy Type menu.
Enter in the appropriate settings.
Click Apply.
{Body|Volume|Surface|Curve|Vertex|Group} <range> Copy Reflect {X|Y|Z} [Nomesh] [Preview]
{Body|Volume|Surface|Curve|Vertex|Group} <range> Copy Reflect [Vertex <v1_id> [Vertex] <v2_id]
[Nomesh] [Preview]
{Body|Volume|Surface|Curve} <range> Copy Reflect <x> <y> <z> [Nomesh] [Preview]
To copy an entity using Rotate
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry.
Click Volume, Surface, Curve, Vertex or Group.
Click on the Create action button.
Select Copy from the drop-down menu.
Select Rotate from the Copy Type menu.
Enter in the appropriate settings.
Click Apply.
{Body|Volume|Surface|Curve} <range> Copy Rotate <angle> About {X|Y|Z} [Repeat <value>]
[Nomesh] [Preview]
{Body|Volume|Surface|Curve} <range> Copy Rotate <angle> About <x> <y> <z> [Nomesh] [Repeat
<value>] [Repeat <value>] [Preview]
265
Trelis 15.0 User Documentation
To copy an entity using Scale
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry.
Click Volume, Surface, Curve, Vertex or Group.
Click on the Create action button.
Select Copy from the drop-down menu.
Select Scale from the Copy Type menu.
Enter in the appropriate settings.
Click Apply.
{Body|Volume|Surface|Curve} <range> Copy Scale <scale> | X <val> Y <val> Z <val> [About Vertex
<id>] [Nomesh] [Repeat <value>] [Preview]
If the copy command is used to generate new entities, a copy of the original mesh generated in the original entity will also
be copied directly onto the new entity unless the nomesh option is used.
Several of the commands include the Repeat token. If that token is used the command will repeat itself value times.
This is currently limited to copies that do not interact with adjacent geometry through non-manifold topology. For details on
mesh copies, see the Mesh Duplication documentation.
266
Move Command
The move command moves a body, volume, free surface, free curve or free vertex by a specified offset.
To Move an Entity
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry.
Click Volume, Surface, Curve, Vertex or Group.
Click on the Transform action button.
Select Move from the drop-down menu.
Enter in the appropriate settings.
Click Apply.
Vertex <id_range> [Move [X <dx>] [Y <dy>] [Z <dz>]] [Copy] [Preview]
Vertex <id_range> Move <direction_options< [Distance <val>] [Copy] [Preview]
{Body|Volume|Surface|Curve|Vertex|Group} <id_range> [Move [X <dx>] [Y <dy>] [Z <dz>]] [Copy
[Nomesh]] [Preview]
{Body|Volume|Surface|Curve|Vertex|Group} <id_range> Move <direction_options> [Distance <val>]
[Copy [Nomesh]] [Preview]
where <dx> <dy> <dz> and <distance> represent relative offsets in the major axis directions. If the copy option is
specified, a copy is made and the copy is moved by the specified offset. The nomesh option will copy and move only the
geometry.
These forms of the Move command will only work on free surfaces and free curves. To move a curve or surface that is
part of a higher-order entity, the Move {entity} ... command is used.
Moving Other Geometric Entities
It is also possible to move bodies by specifying one of its child entities. For example, a body can by moved by specifying
one of its curves. However, if a lower-order entity is moved, the parent body and all related entities will also be moved.
The commands for moving bodies using a child entity are given below. Alternatively, the tweak command can be used to
move curves and surfaces without moving the parent body.
To Move an Entity
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry.
Click Volume, Surface, Curve, Vertex or Group.
Click on the Transform action button.
Select Move from the drop-down menu.
Select General Location from the Select Method menu.
Enter in the appropriate settings.
Click Apply.
Move {Vertex|Curve|Surface|Volume|Body|Group} <id_range> [Midpoint] Location <x> [<y> [<z>]]
[Include_Merged] [Preview]
Move {Vertex|Curve|Surface|Volume|Body|Group} <id_range> Location [Midpoint] [X <val>] [Y <val>]
[Z <val>] [Except [X] [Y] [Z]] [Include_Merged] [Preview]
Move {Vertex|Curve|Surface|Volume|Body|Group} <id_range> Normal to Surface <id> Distance <val>
[Include_Merged] [Preview]
Move {Vertex|Curve|Surface|Volume|Body|Group} <id_range> [Midpoint] General Location
<location_options> [Except [X] [Y] [Z]] [Include_Merged] [Preview]
267
Trelis 15.0 User Documentation
The first form of the command will move the entity to an absolute location. If moving a group, the centroid of the group is
moved to that location. The second form will move the entity by a relative distance in any of the xyz axis directions.
"Except" is used to preserve the x, y, or z plane in which the center of the entity lies. The third form of the command will
move the body along an axis defined by the outward-facing surface normal of another surface. The fourth form of the
command uses general location parsing to move the entity.
Moving Bodies Relative to Other Geometric Entities
It is also possible to move bodies relative to other geometric entities in the model. The following command takes as
arguments two geometric entities. The first entity is the one to move. The second entity is where it will be moved. In both
cases, the midpoints of the specified entity are used to determine the distance and direction of the move. In the case of
groups, centroids are used. "Except" is used to preserve the x, y, or z plane in which the center of the entity lies.
Move {Vertex|Curve|Surface|Volume|Body|Group} <id_range> [Midpoint] Location
{Vertex|Curve|Surface|Volume|Body|Group} <id> [Midpoint] [Except [X] [Y] [Z]] [Include_Merged]
[Preview]
Moving Merged Entities
The easiest way to move merged entities is by adding the include_merged keyword to the command. All entities that are
merged with the specified entities will move together.
The only other way that merged entities can be moved is by including each of the merged entities in the entity list.
Move Undo
The Undo option allows a user to reverse the most recent move. This command will only work for the Move {entity}
commands, and not the {Entity} Move commands. The syntax is:
Move Undo
268
Scale Command
The scale command resizes an entity (body, volume, surface, or curve) by a scaling factor. The scaling factor may be a
constant, or may differ in the x, y, and z directions. The entity chosen will be scaled about the point or vertex indicated. If
no point or vertex is entered, it will be scaled about the origin. Any mesh on the object will be scaled too, unless the
nomesh keyword is used.
To Scale an Entity
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry.
Click Volume, Surface, Curve, Vertex or Group.
Click on the Transform action button.
Select Scale from the drop-down menu.
Enter in the appropriate settings.
Click Apply.
{Body|Volume|Surface|Curve} <id_range> Scale {<scale> | x <val> y <val> z <val>} [About {<x> <y>
<z> | Vertex <id>}] [Nomesh] [Copy [Repeat <value>] [Group_Results]] [Preview]
If the copy option is specified, a copy of the entity is made and scaled the specified amount. Use the repeat option to
create multiple copies.
269
Rotate Command
The rotate command rotates a body about a given axis without adding any new geometry. If the Angle or any Components
are not specified they are defaulted to be zero.
To Rotate an Entity
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry.
Click Volume, Surface, Curve, Vertex or Group.
Click on the Transform action button.
Select Rotate from the drop-down menu.
Enter in the appropriate settings.
Click Apply.
Body <range> [Copy] Rotate <angle> About {X|Y|Z} [Preview]
Body <range> [Copy] Rotate <angle> About <x-comp> <y-comp> <z-comp> [Preview]
Rotate {Body|Volume|Surface|Curve|Vertex|Group} <id_range> about {X|Y|Z|<xval> <yval> <zval>}
Angle <val> [Include_Merged] [Preview]
Rotate {Body|Volume|Surface|Curve|Vertex|Group} <id_range> About Vertex <id> Vertex <id> Angle
<val> [Include_Merged] [Preview]
Rotate {Body|Volume|Surface|Curve|Vertex|Group} <id_range> About Normal of Surface <id> Angle
<val> [Include_Merged] [Preview]
Rotate {Body|Volume|Surface|Curve|Vertex|Group} <id_range> About Origin <xval> <yval> <zval>
Direction <xval> <yval> <zval> Angle <val> [Include_Merged] [Preview]
If the copy option is specified, a copy is made and rotated the specified amount.
Rotating Merged Entities
The easiest way to rotate merged entities is by adding the include_merged keyword to the command. All entities that are
merged with the specified entities will rotate together.
The only other way that merged entities can be rotated is by including each of the merged entities in the entity list.
271
Reflect Command
The reflect command mirrors the body about a plane normal to the vector supplied. The reflect command will destroy the
existing body and replace it with the new reflected body, unless the copy option is used.
To Reflect an Entity
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry.
Click Volume, Surface, Curve, Vertex or Group.
Click on the Transform action button.
Select Reflect from the drop-down menu.
Enter in the appropriate settings.
Click Apply.
{Body|Volume|Surface|Curve|Vertex|Group} <range> [Copy] Reflect <x-comp> <y-comp> <z-comp>
{Body|Volume|Surface|Curve|Vertex|Group} <range> [Copy] Reflect {X|Y|Z}
273
Intersect
The intersect operation generates a new body composed of the space that is shared by the two bodies being intersected.
Both of the original bodies will be deleted and the new body will be given the next highest body ID available.
To intersect an entity
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Volume.
Click on the Boolean action button.
Select Intersect from the drop-down menu.
Enter in the values for Body ID(s). This can also be done using the Pick Widget function.
Click Apply.
Intersect {Volume|[Body]} <range> [With {Volume|[Body]} <range>] [Keep] [Preview]
The keep option results in the original bodies used in the intersect being kept.
If the Preview option is included in the command, the input bodies will not be modified. The computed intersection volume
will be drawn as a red, shaded solid. For best results change the graphics mode to transparent or hidden line so the
intersection is visible. Otherwise the intersection volume will be hidden by the volumes being intersected.
275
Subtract
The subtract operation subtracts one body or set of bodies from another body or set of bodies. The order of subtraction is
significant - the body or bodies specified before the From keyword is/are subtracted from bodies specified after From.
The new body retains the original body's id. If any additional bodies are created, they will be given the next highest
available ids. The keep option simply retains all of the original bodies. The command is:
To subtract an entity
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Volume.
Click on the Boolean action button.
Select Subtract from the drop-down menu.
Enter in the values for Body ID(s) and Subtract Body ID(s). This can also be done using the Pick Widget
function.
Click Apply.
Subtract [Volume|BODY] <range> From [Volume|BODY] <range> [Imprint] [Keep]
The imprint option imprints the subtracted bodies onto the resultant body.
277
Unite
The unite operation combines two or more bodies into a single body.
To unite bodies
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Volume.
Click on the Boolean action button.
Select Unite from the drop-down menu.
Enter in the values for Body ID(s). This can also be done using the Pick Widget function.
Click Apply.
The Keep option preserves the original bodies and the new body created is given the next highest body ID available.
The include_mesh option creates a new meshed body from the original meshed bodies. For this function to work
properly, the original bodies must be merged.
Unite [Volume|BODY] <range> [With [Volume|BODY] <range>] [include_mesh] [Keep]
Unite Body {<range> | All} [Keep]
The second form of the command unites multiple bodies in a single operation. If the all option is used, all bodies in the
model are united into a single body. If the bodies that are united do not overlap or touch, the two bodies are combined into
a single body with multiple volumes.
The unite command allows sheet bodies to be united with solid bodies. To disable this capability you can turn the
following setting off:
Set Unite Mixed {ON|Off}
279
Chop Command
The chop command works similarly to a web cut command, but is faster. Given two bodies, the command will find the
intersection of the two bodies, and divide the main body into a body that lies outside the intersection, and a body that lies
inside the intersection. The tool body will be deleted, unless the keep option is specified. The syntax of the command is:
Chop [Volume|BODY] <id> with [Volume|BODY] <id> [keep] [nonreg]
The nonreg option results in the bodies being non-regularized.
281
Web Cutting by Sweeping Curves or Surfaces
Webcutting with sweeping creates a swept tool body in the same step as the web cut operation. There are 4 general ways
to web cut with sweeping:
•
•
•
•
Web Cutting by Sweeping a Surface Along a Trajectory
Web Cutting by Sweeping a Surface About an Axis
Web Cutting by Sweeping a Curve(s) Along a Trajectory
Web Cutting by Sweeping a Curve(s) About an Axis
Web Cutting by Sweeping a Surface Along a Trajectory
This command allows one or more surfaces to be swept, creating a volume that is used for the web cut. If more than one
surface is specified, the surfaces must contain coincident curves. The surfaces are swept along a direction and some
distance or perpendicular and some distance or along a curve. For best results the curve to sweep the surface along
should intersect one of the surfaces. The through_all option will sweep the surfaces along the trajectory far enough so as
to intersect all input bodies. The stop surface <id> option is used to identify a surface at which the sweep will stop. If
using this option when sweeping along a curve, the sweep will stop at the first place possible. The up_to_next option
indicates that the user wants to web cut with only the first water tight volume that forms as a result of the intersection
between sweep and union of all blank bodies. The [Outward|Inward] options specify a sweeping direction that is either
INTO the volume or OUT from the volume.
To sweep a surfvace along a curve or vector
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select Sweep Surface from the drop-down menu.
Enter in the appropriate values for Body ID(s) and Surface ID. This can also be done using the Pick Widget
function.
Select Vector or Along Curve from the Direction menu.
Enter in the appropriate settings from this menu.
Click Apply.
Webcut {Volume|Body|Group} <range> Sweep Surface <id_range> {Vector <x> <y> <z> [Distance
<distance>] | Along Curve <id>} [Through_all | Stop Surface <id> | Up_to_next ] [webcut_options]
To sweep a surface a perpendicular direction
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select Sweep Surface from the drop-down menu.
Enter in the appropriate values for Body ID(s) and Surface ID. This can also be done using the Pick Widget
function.
Select Perpendicular from the Direction menu.
Enter in the appropriate settings from this menu.
Click Apply.
Webcut {Volume|Body|Group} <id> Sweep Surface <id_range> Perpendicular {Distance <distance> |
Through_all | Stop Surface <id>} [OUTWARD|Inward] [webcut_options]
283
Trelis 15.0 User Documentation
sweeping a surface in a direction
resultant web cut
along a curve to a stop surface
resultant web cut
Figure 1. Examples of web cutting with swept surfaces
Web Cutting by Sweeping a Surface About an Axis
This command allows one or more surfaces to be swept, creating a volume that is used for the web cut. If more than one
surface is specified, the surfaces must contain coincident curves. The surface is swept about a user-defined axis or about
one of the x y z coordinate axes and a specified angle. The stop surface <id> option is used to identify a surface at
which the sweep will stop. The up_to_next option indicates that the user wants to web cut with only the first water tight
volume that forms as a result of the intersection between sweep and union of all blank bodies. For these 2 options to work
correctly the user must specify an angle large enough for the rotation to traverse the stop surface or the up_to_next
surface.
To sweep a surface by rotating about an axis
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select Sweep Surface from the drop-down menu.
Enter in the appropriate values for Body ID(s) and Surface ID. This can also be done using the Pick Widget
function.
Select Rotate About Axis from the Direction menu.
Enter in the appropriate settings from this menu.
Click Apply.
Webcut {Volume|Body|Group} <id> Sweep Surface <id_range> {Axis <xpoint ypoint zpoint xvector
yvector zvector> | Xaxis | Yaxis | Zaxis } Angle <degrees> [Stop Surface <id> | Up_to_next]
[webcut_options]
284
Web Cutting by Sweeping Curves or Surfaces
Web Cutting by Sweeping a Curve(s) Along a Trajectory
This command allows a curve(s) to be swept, creating a surface that is used for the web cut. If multiple curves are
specified, they must share vertices and form a continuous path. The curve(s) is swept along a direction and some
distance or along another curve. If sweeping a curve(s) along another curve, for best results the curve(s)-to-swept and the
curve to sweep along should intersect at some point. The stop surface <id> option is used to identify a surface at which
the sweep will stop. If using this option when sweeping along a curve, the sweep will stop at the first place possible. The
through_all option will sweep the curve(s) along the trajectory far enough so as to intersect all input bodies. For the web
cut to be successful, the swept curve(s) must completely traverse a portion of a blank body(s), cutting off a complete
piece of the blank body(s). Option through_all should not be used when defining the web cut with a vector and a distance
or along a curve.
To sweep a curve along a curve or vector
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select Sweep Curve from the drop-down menu.
Enter in the appropriate values for Body ID(s) and Curve ID. This can also be done using the Pick Widget
function.
Select Vector or Along Curve from the Direction menu.
Enter in the appropriate settings from this menu.
Click Apply.
Webcut {Volume|Body|Group} <id> Sweep Curve <id_range> {Vector <x> <y> <z> [Distance
<distance>| Along curve <id>] } [Through_all | Stop Surface <id>] [webcut_options]
Web Cutting by Sweeping a Curve(s) About an Axis
This command allows a curve to be swept, creating a surface that is used for the web cut. If multiple curves are specified,
they must share vertices and form a continuous path. The curve(s) is swept about a user-defined axis or about one of the
x y z coordinate axes and a specified angle. For the web cut to be successful, the swept curve(s) must completely
traverse a portion of a blank body(s), cutting off a complete piece of the blank body(s). The stop surface <id> option is
used to identify a surface at which the sweep will stop. For this option to work correctly the user must specify an angle
large enough for the rotation to traverse the stop surface.
To sweep a curve about an axis
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select Sweep Curve from the drop-down menu.
Enter in the appropriate values for Body ID(s) and Curve ID. This can also be done using the Pick Widget
function.
Select Rotate About Axis from the Direction menu.
Enter in the appropriate settings from this menu.
Click Apply.
Webcut {Volume|Body|Group} <id> Sweep Curve <id_range> {Axis <xpoint ypoint zpoint xvector
yvector zvector> | Xaxis | Yaxis | Zaxis } Angle <degrees> [Stop Surface <id>] [webcut_options]
285
Web Cutting Options
The following options can be used with all web cut commands:
[NOIMPRINT|Imprint [include_neighbors] ]: In its default implementation, web cutting results in the pieces not being
imprinted on one another; this option forces the code to imprint the pieces after web cutting. The include_neighbors option
will also imprint adjacent bodies.
[NOMERGE|Merge]: By default, the pieces resulting from an imprint are manifold; specifying this option results in a
merge check for all surfaces in the pieces resulting from the web cut.
[Group_results]: The various pieces resulting from the previous command are placed into a group named
`webcut_group'.
[Preview]: This option will preview the web cutting plane without executing the command.
287
Web Cutting with a Planar or Cylindrical Surface
The commands used to web cut with a planar or cylindrical surface in Trelis are:
•
•
•
•
•
•
•
Coordinate Plane
Planar Surface
Plane from 3 Points
Plane Normal to Curve
General Plane Specification
Cylindrical Surface
Cone Surface
Coordinate Plane
In the command's simplest form, a coordinate plane can be used to cut the model, and can optionally be offset a positive
or negative distance from its position at the origin.
To use a coordinate plane to webcut
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select Coordinate Plane from the drop-down menu.
Enter the appropriate values for Body ID(s). This can also be done using the Pick Widget tool.
Select YZ, ZX or XY.
Enter in the Offset Value.
Enter any other appropriate settings from this menu.
Click Apply.
Webcut {Volume|Body|Group} <id_range> [With] Plane {xplane|yplane|zplane} [Offset <val>] [rotate
<theta> about x|y|z <xval> <yval> <zval> [center <xval> <yval> <zval>]] webcut_options
The cutting plane can be rotated about a user-specified axis using the rotate option. The center of rotation can be moved
by using the center option.
Planar Surface
An existing planar surface can also be used to cut the model; in this case, the surface is identified by its ID as the cutting
tool.
To use an existing planar surface to webcut
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select General Plane from the drop-down menu.
Enter the appropriate values for Body ID(s). This can also be done using the Pick Widget tool.
Enter the appropriate settings for With Plane. By clicking the With Plane... button, another window appears to
specify settings.
Enter any other appropriate settings from this menu.
Click Apply.
Webcut {Volume|Body|Group} <id_range> [With] Plane Surface <surface_id> webcut_options
Plane from 3 Points
Any arbitrary planar surface can be used by specifying three vertices that define the plane, and can optionally be offset a
positive or negative distance from this plane.
289
Trelis 15.0 User Documentation
To use a planar surface by specifying three vertices
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select Plane From Vertices from the drop-down menu.
Enter the appropriate values for Body ID(s), Vertex 1 ID, Vertex 2 ID and Vertex 3 ID. This can also be done
using the Pick Widget tool.
Click Apply.
Webcut {Volume|Body|Group} <id_range> [With] Plane Vertex <vertex_1> [Vertex] <vertex_2>
[Vertex] <vertex_3> [Offset <value>] webcut_options
The plane to be used for the web cut can be previewed with the preview option in the general webcut options.
Plane Normal to Curve
The next command allows a user to specify an infinite cutting plane by specifying a location on a curve. The cutting plane
is created such that it is normal to the curve tangent at the specified location.
To specify the cutting plane by specifying the location on the curve
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select Plane From Curve from the drop-down menu.
Enter the appropriate values for Body ID(s) and Curve ID. This can also be done using the Pick Widget tool.
Select Fraction, Position, Distance or Near Vertex from the Position menu.
Enter any other appropriate settings from this menu.
Click Apply.
Webcut {Volume|Body|Group} <id_range> [With] Plane Normal To Curve <curve_id>
{Position <xval><yval><zval> | Close_To Vertex <vertex_id>} webcut_options
Webcut {Volume|Body|Group} <id_range> [With] Plane Normal To Curve <curve_id>
{Fraction <f> | Distance <d>} [[From] Vertex <vertex_id>] webcut_options
The position on the curve can be specified as:
1.
2.
3.
4.
A fraction along the curve from the start of the curve, or optionally, from a specified vertex on the curve.
A distance along the curve from the start of the curve, or optionally, from a specified vertex on the curve.
An xyz position that is moved to the closest point on the given curve.
The position of a vertex that is moved to the closest point on the given curve.
The point on the curve can be previewed with the Draw Location On Curve command and the plane to be used for the
web cut can be previewed with the preview option in the general webcut options.
General Plane Specification
A webcut plane can be defined using the general plane specification options in the Specifying a Plane section of the
documentation.
To webcut using general plane specification
1.
2.
3.
4.
5.
6.
7.
290
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select General Plane from the drop-down menu.
Enter the appropriate values for Body ID(s). This can also be done using the Pick Widget tool.
Enter the appropriate settings for With Plane. Click on the With Plane... button, another window appears to
specify settings.
Enter any other appropriate settings from this menu.
Click Apply.
Web Cutting with a Planar or Cylindrical Surface
Webcut {Volume|Body|Group} <id_range> [With] General Plane {options} webcut_options
Cylindrical Surface
Finally, a semi-infinite cylindrical surface can be used by specifying the cylinder radius, and the cylinder axis. The axis is
specified as a line corresponding to a coordinate axis, the normal to a specified surface, two arbitrary points, or an
arbitrary point and the origin. The "center" point through which the cylinder axis passes can also be specified.
To use a cylindrical surface to webcut
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select Cylinder from the drop-down menu.
Enter the appropriate values for Body ID(s). This can also be done using the Pick Widget tool.
Select Value or From Existing Arc from the Radius menu.
Enter in the appropriate values for Radius or Arc ID.
Select X Axis, Y Axis, Z Axis, Vector, Vertex Pair or Surface Normal from the Axis menu.
Enter any other appropriate settings from this menu.
8.
Click Apply.
Webcut {Volume|Body|Group} <range> [With] Cylinder Radius <val> Axis {x|y|z|normal of surface
<id>| vertex <id_1> vertex <id_2>| <x_val> <y_val> <z_val>>} [center <x_val> <y_val> <z_val>]
webcut_options
Cone Surface
A semi-infinite cone surface can be used by specifying the cone outer radius, and the cone inner radius. The axis is
specified as a location first of where the outer radius is applied and the second location of where the inner radius is
applied.
Cone
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select Cone from the drop-down menu.
Enter the appropriate values for Body ID(s). This can also be done using the Pick Widget tool.
Enter the appropriate values for Radius 1 and Radius 2.
Enter the appropriate settings for Location 1 and Location 2. Click on the Location... button, another window
appears to specify settings.
Enter any other appropriate settings from this menu.
Click Apply.
Webcut {Volume|Body|Group} <ids> [With] cone radius <val> <val> location {options} location {options}
[Imprint] [Merge] [group_results] [preview]
291
Web Cutting using a Tool or Sheet Body
Any existing body in the geometric model can be used to cut other bodies; the command to do this is:
To use an existing body to webcut
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select Tool from the drop-down menu.
Enter the appropriate values for Body ID(s). This can also be done using the Pick Widget function.
Click Apply.
Webcut {blank} tool [body] <id> [webcut_options]
This simply uses the specified tool body in a set of boolean operations to split the blank into two or more pieces.
Another form of the command cuts the body list with a temporary sheet body formed from the curve loop. This is the same
sheet as would be created from the command Create Surface Curve <id_list>.
To webcut with the body formed from the curve loop
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select Loop from the drop-down menu.
Enter the appropriate values for Body ID(s) and With Curve ID(s). This can also be done using the Pick
Widget function.
Click Apply.
Webcut {Body|Group} <id_range> [With] Loop [Curve] <id_range> NOIMPRINT|Imprint]
[NOMERGE|Merge] [group_results]
Webcut {Volume|Body|Group} <id_range> [With] Bounding Box {Body|Volume|Surface|Curve|Vertex
<id_range>} [Tight] [[Extended] {Percentage|Absolute} <val>] [{X|Width} <val>] [{Y|Height} <val>]
[{Z|Depth} <val>]] NOIMPRINT|Imprint] [NOMERGE|Merge] [group_results]
The final form of this command cuts a body with the bounding box of another entity. This bounding box may be tight or
extended.
Figure 1. Cylinder cut with bounding box of prism.
293
Trelis 15.0 User Documentation
294
Web Cutting with an Arbitrary Surface
An arbitrary "sheet" surface can also be used to web cut a body. This sheet need not be planar, and can be bounded or
infinite. The following commands are used:
To webcut using a sheet
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Volume.
Click on the Webcut action button.
Select Surface Extended from the drop-down menu.
Enter in the appropriate values for Body ID(s) and With Surface ID(s). This can also be done using the Pick
Widget function.
Click Apply.
Webcut {blank} with sheet {body|surface} <id> [webcut_options]
Webcut {blank} with sheet extended [from] surface <id> [webcut_options]
In its first form, the command uses a sheet body, either one that is pre-existing or one formed from a specified surface.
Note that in this latter case the (bounded) surface should completely cut the body into two pieces. Sheet bodies can be
formed from a single surface, but can also be the combination of many surfaces; this form of web cut can be used with
quite complicated cutting surfaces.
Extended sheet surfaces can also be used; in this case, the specified surface will be extended in all directions possible.
Note that some spline surfaces are limited in extent, and so these surfaces may or may not completely cut the blank.
295
Split Curve
The Split Curve command will split a curve without the need for geometry creation (unlike imprinting).
To split a curve
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Curve.
Click on the Modify action button.
Select Split from the drop-down menu.
Enter the appropriate value for Curve ID. This can also be done using the Pick Widget function.
Select Fraction, Vertex ID, By Location, Distance or Pick from the Split Method/Location menu.
Click Apply.
Split Curve <id> [location on curve options] [Merge] [Preview]
To split a curve, simply specify a location or a location on curve (see location specification). Using the Preview keyword
will draw the splitting location on the curve. The Merge keyword will merge any topology that contains the newly created
vertex.
297
Split Periodic Surfaces
Solids which contain periodic surfaces include cylinders, torii and spheres. Splitting periodic surfaces can in some cases
simplify meshing, and will result in curves and surfaces being added to the volume.
To split periodic surfaces
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Volume.
Click on the Modify action button.
Select Split Periodic from the drop-down menu.
Enter the appropriate value for Volume ID(s). This can also be done using the Pick Widget function.
Click Apply.
Split Periodic Body <id_range|all>
This command splits all periodic surfaces in a body or bodies.
299
Split Surface
The Split Surface command divides one or more surfaces into multiple surfaces. The command results are similar to
imprint with curve. However, curve creation is not necessary for splitting surfaces. Three primary forms of the command
are available.
•
•
•
•
Split Across
Split Extend
Split (Automatically)
Split Skew
The first form splits a single surface using locations while the second splits by extending a surface hard-line until it hits a
surface boundary. The split automatic splits either a single surface or a chain of surfaces in an automatic fashion.
Split Across
Two forms of Split Across are available
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Split from the drop-down menu.
Select By Location from the drop-down menu.
Enter in the appropriate value for Surface ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate settings on this menu.
Click Apply.
Split Surface <id> Across [Pair] Location <options multiple locs> [Preview [Create]]
Split Surface <id> Across Location <multiple locs> Onto Curve <id> [Preview] Create]]
This command splits a surface with a spline projection through multiple locations on the surface. See Location, Direction,
and Axis Specification for a detailed description of the location specifier. Figure 1 shows a simple example of splitting a
single surface into two surfaces. A temporary spline was created through the three specified locations (Vertex 5 6 7), and
this curve was used to split the surface.
split surface 1 across location vertex 5 6 7
Figure 1 - Splitting Across with Multiple Locations
The Pair keyword will pair locations to create multiple surface splitting curves (each defined with two locations). An even
number of input locations is required. Figure 2 shows an example:
301
Trelis 15.0 User Documentation
split surface 1 across pair vertex 5 7 6 8
Figure 2 - Splitting Across with Pair Option
The Preview keyword will show a graphics preview of the splitting curve. If the Create keyword is also specified, a free
curve (or curves) will be created - these are the internal curves that are used to imprint the surfaces.
The Onto Curve format of the command takes one or more locations on one side of the surface and projects them onto a
single curve on the other side of the surface. Figure 3 shows an example:
split surface 1 across vertex 5 6 onto curve 4
Figure 3 - Splitting Across with Onto Curve
Split Extend
The Split Extend function can be called with the following command:
Split Surface <id_list> Extend [Vertex <id_list> | AUTO] [Preview [Create]]
With the following settings:
Set Split Surface Extend Normal {on|OFF}
Set Split Surface Extend Gap Threshold <val>
Set Split Surface Extend Tolerance<val>
This command splits a surface by extending a surface hard-line until it hits a surface boundary. Figure 4 shows a simple
example of extending a curve. The hard-line curve was extended from the specified vertex until it hit the surface
boundary.
split surface 1 extend vertex 2
302
Split Surface
Figure 4 - Splitting by Extending Hard-line
The auto keyword will search for all hard-lines and extend them according to the Split Surface Extend settings. Figure 5
shows an example:
split surface 1 extend auto
Figure 5 - Splitting by Extending with Auto Option
The preview keyword will show a graphics preview of the splitting curve. If the create keyword is also specified, a free
curve (or curves) will be created - these are the internal curves that are used to imprint the surfaces.
The normal setting can be turned on or off. When it is on, Trelis will attempt to extend the hard-line so that it is normal to
the curve it will intersect. An example of this is in Figure 6:
set split surface normal on
split surface 1 extend vertex 2
Figure 6 - Splitting by Extending a Hard Line with Normal Setting ON
303
Trelis 15.0 User Documentation
Trelis uses the gap threshold to decide whether or not to extend a hard-line when the user specifies auto. If the distance
between a vertex on a hard-line and the curve it will hit is greater than the gap threshold, then Trelis will not extend that
hard-line. The default value is INFINITY, and can be set to any value. To reset the value back to INFINITY, set the gap
threshold to -1.0. Note: This setting only applies when using the keyword auto. An example of using the gap
threshold is shown in Figure 7:
set split surface gap threshold 2.0
split surface 1 extend auto
Figure 7 - Extending Hard-lines with Gap Threshold = 2.0.
(Notice Vertex 1 was not extended because it exceeded the gap threshold)
The tolerance setting can be used to avoid creating short curves on the surface boundary. If Trelis tries to extend a hardline that comes within tolerance of a vertex, it will instead snap the extension to the existing vertex. An example of this is
shown in Figure 8:
set split surface tolerance 1.0
split surface 1 extend vertex 2
Figure 8 - Extending Hard-lines with Tolerance
(Notice the extension snapped to Vertex 3)
Split (Automatically)
This form of the command splits a single surface or a chain of surfaces in an automatic fashion. It is most convenient for
splitting a fillet or set of fillets down the middle - oftentimes necessary to prepare for mesh sweeping. These surfaces
cannot have multiple curve loops.
To Split a surface
1.
2.
3.
4.
304
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Split from the drop-down menu.
Select Along Fillet from the drop-down menu.
Split Surface
5.
6.
Enter in the appropriate value for Surface ID(s). This can also be done using the Pick Widget function.
Click Apply.
Split Surface <id_list> [Corner Vertex <id_list>] [Direction Curve <id>] [Segment|Fraction|Distance
<val> [From Curve <id>]] [Through Vertex <id_list>] [Parametric <on|OFF>] [Tolerance <val>]
[Preview [Create]]
•
•
•
•
•
•
•
•
•
•
Logical Rectangle
Split Orientation
Corner Vertex <id_list>
Direction Curve <id>
Segment|Fraction|Distance <val> [From Curve <id>]
Through Vertex <id_list>
Parametric <on|OFF>
Tolerance <val>
Preview [Create]
Settings (Tolerance, Parametric, Triangle)
The volume shown in Figure 9 was quickly prepared for sweeping by splitting the fillets and specifying sweep sources as
shown (with the sweep target underneath the volume). The surface splits are shown in blue.
Figure 9 - Splitting Fillets to Facilitate Sweeping
Each surface is always split with a single curve along the length of the surface (or multiple single curves if the Segment
option is used). The splitting curve will either be a spline, arc or straight line.
Logical Rectangle
The Split Surface command analyzes the selected surface or surface chain to find a logical rectangle, containing four
logical sides and four logical corners; each side can be composed of zero, one or multiple curves. If a single surface is
selected (with no options), the logical corners will be those closest to 90 and oriented such that the surface will be split
parallel to the longest aspect ratio of the surface. If a chain of surfaces is selected, the logical corners will include the
two corners closest to 90 on the starting surface of the chain and the two corners closest to 90 on the ending surface of
the chain (the split will always occur along the chain).
In Figure 10, the logical corners selected by the algorithm are Vertices 1-2-5-6. Between these corner vertices the logical
sides are defined; these sides are described in Table 1. The default split occurs from the center of Side 1 to the center of
Side 3 (parallel to the longest aspect ratio of the surface), and is shown in blue.
305
Trelis 15.0 User Documentation
Figure 10 - Split Surface Logical Properties
Table 1. Listing of Logical Sides for Figure 10
Logical Side
Corner Vertices
Curve Groups
1
1-2
1
2
2-5
2,3,4
3
5-6
5
4
6-1
6
Figure 11 shows a surface along with 2 possibilities for its logical rectangle and the resultant splits.
306
Split Surface
Figure 11 - Different Possible Logical Rectangles for Same Surface
Table 2 shows various surfaces and the resultant split based on the automatically detected or selected logical rectangle.
Note that surfaces are always traversed in a counterclockwise direction.
Table 2 - Sample Surfaces and Logical Rectangles
Surface(s) (Resultant Split in Blue)
Ordered Corners (to form the Logical Rectangle)
1-2-3-4
(using aspect ratio)
4-1-2-3
(user selected)
307
Trelis 15.0 User Documentation
1-2-5-6
2-5-6-1
1-2-3-4
(split is always along the chain)
1-2-3-4
(notice triangular surfaces along the chain)
1-1-2-3
(note side 1 of the logical rectangle is collapsed; side 3 is
from vertex 2 to 3)
308
Split Surface
1-2-2-3
(note side 2 of the logical rectangle is collapsed)
1-2-3-4
1-2-4-4
1-1-2-2
1-1-2-2
(selected automatically)
Split Orientation
If a chain of surfaces are split, the surfaces will always be split along the chain. The command will not allow disconnected
surfaces.
For a single surface, the split direction logic is a bit more complicated. If no options are specified, the surface aspect ratio
determines the split direction - the surface will be split parallel to the longest aspect ratio side through the midpoint of each
curve. This behavior can be overridden by the order the Corner vertices are selected (the split always starts on the side
between the first two corners selected), the Direction option, the From Curve option, or the Through Vertex list.
Table 3 shows examples of the various split orientation methods. These options are explained in more detail in the
sections below.
Table 3 - Split Orientation Methods
Surface Example
Split Orientation Method
309
Trelis 15.0 User Documentation
Multiple surfaces are always split along the chain
Parallel to longest surface aspect ratio (default)
Corner Vertex 4 1 2 3
(split always starts on side 1 of the logical rectangle)
Direction Curve 1
From Curve 1 Fraction .75
or
From Curve 1 Distance 7.5
Through Vertex 5 6
Corner Specification
310
Split Surface
The Corner option allows you to specify corners that form logical rectangle the algorithm uses to orient the split on the
surface. When analyzing a surface to be split, the software automatically selects the corners that are closest to 90. The
Preview option displays the automatically selected corners in red. Sometimes incorrect corners are chosen, so you must
specify the desired corners yourself. The split always starts on the side between the first two corners selected and finishes
on the side between the last two corners selected. Figure 12 shows a situation where the user had to select corners to get
the desired split.
Figure 12 - Selecting the Desired Corners
The split can be directed to the tip of a triangular shaped surface by selecting that corner vertex twice (at the start or end
of the corner list) when specifying corners, creating a zero-length side on the logical rectangle. A shortcut exists whereas
if you specify only 3 corner vertices, the zero-length side will be directed to the first corner selected. If you specify only 2
corner vertices, a zero-length side will be directed to both the first and second corner you select. Table 4 shows these
examples. Note the software will automatically detect triangle corners based on angle criteria - the corner selection
methods for zero-length sides explained in this section need only be applied if the angles are outside of the thresholds
specified in the Set Split Surface Auto Detect Triangle settings.
Table 4 - Selecting Corners to Split to Triangle Tips
Surface
Corner Specification
1-2-4-4- or 4-4-1-2
or
4-1-2 (shortcut method)
1-1-2-2 or 2-2-1-1
or
1-2 or 2-1 (shortcut method)
Direction
The Direction option allows you to conveniently override the default split direction on a single surface. Simply specify a
curve from the logical rectangle that is parallel to the desired split direction. If Corners are also specified, the Direction
option will override the split orientation that would result from the specified corner order. The Direction option is not valid
on a chain of surfaces. Figure 13 shows an example.
311
Trelis 15.0 User Documentation
Figure 13 - Direction Specification Overrides Corner Order
Segment|Fraction|Distance
The Segment option allows you to split a surface into 2 or more segments that are equally spaced across the surface.
The Fraction option allows you to override the default 0.5 fractional split location. The Distance option allows you to
specify the split location as an absolute distance rather than a fraction. By specifying a From Curve, you can indicate
which side of the logical rectangle to base the segment, fraction or distance from (versus a random result). Table 5 gives
examples of these options.
Table 5 - Segment, Fraction, Distance Examples
Surface
Command Options
Segment 6 From Curve 1
Fraction .3 From Curve 1
Distance 3 From Curve 1
312
Split Surface
Through Vertex
The Through Vertex option forces the split through vertices on surface boundaries perpendicular to the
split direction. Use this option if the desired fraction is not constant from one end of the surface to another or if a split
would otherwise pass very close to an existing curve end resulting in a short curve. Through vertices can be used in
conjunction with the Fraction option - the split will linearly adjust to pass exactly through the specified vertices. It is not
valid with the Segment option. The maximum number of Through Vertices that can be specified is equal to the number of
surfaces being split plus one. The selected vertices can be free, but must lie on the perpendicular curves. Table 6 gives
several examples.
Table 6 - Through Vertex Examples
Surface(s)
Command Options
Fraction .3 From Curve 1 Through Vertex 9
Through Vertex 5 6 7 8
Parametric
By default, split locations are calculated in 3D space and projected to the surface. As an alternative, split locations can be
calculated directly in the surface parametric space. In rare instances, this can result in a smoother or more desirable split.
The command option Parametric {on|Off} can be used to split the given surfaces in parametric space. Alternatively, the
default can be overridden with the Set Split Surface Parametric {on|OFF} command.
Tolerance
A single absolute tolerance value is used to determine the accuracy of the split curves. A smaller tolerance will force more
points to be interpolated. The tolerance is also used when detecting an analytical curve (e.g., an arc or straight line)
versus a spline. A looser tolerance will result in more analytical curves. The default tolerance is 1.0. The command option
Tolerance <val> can be used to split the given surfaces using the given tolerance. Alternatively, the default tolerance can
be overridden with the Set Split Surface Tolerance <val> command.
It is recommended to use the largest tolerance possible to increase the number of analytical curves and reduce the
number of points on splines, resulting in better performance and smaller file sizes. The Preview option displays the
interpolated curve points. Table 7 shows the effect of the tolerance for a simple example.
Table 7 - Effect of Tolerance on Split Curve
Surface
Tolerance
313
Trelis 15.0 User Documentation
2.0
1.0
0.5
0.01
Preview
The Preview keyword will show a graphics preview (in blue) of the splitting curve (or curves) and the corner vertices (in
red) selected for the logical rectangle. The curve preview includes the interpolated point locations that define spline
curves. Note that if no points are shown on the interior of the curve, it means that the curve is an analytical curve (line or
arc). If the Create keyword is also specified, a free curve (or curves) will be created - these are the internal curves that are
used to imprint the surfaces. Table 8 shows some examples.
Table 8 - Graphics Preview
Surface
Curve Type
Spline
314
Split Surface
Arc (no preview points shown on interior of
curve)
Settings
This section describes the settings that are available for the automatic split surface command. To see the current values,
you can enter the command Set Split Surface, optionally followed by the setting of interest (without specifying a value).
Set Split Surface Tolerance <val>
This sets the default tolerance for the accuracy of the split curves. See the Tolerance section for more information.
Set Split Surface Parametric {on|OFF}
This sets the default for whether surfaces are split in 3D (default) or in parametric space. See the Parametric section for
more information.
Set Split Surface Auto Detect Triangle {ON|off}
Set Split Surface Point Angle Threshold <val>
Set Split Surface Side Angle Threshold <val>
The split surface command automatically detects triangular shaped surfaces as explained in the section on Corners. This
behavior can be turned off with the setting above. Two thresholds are used when detecting triangles - the Point Angle
threshold and the Side Angle threshold, specified in degrees. Corners with an angle below the Point Angle threshold are
considered for the tip of a triangle (or the collapsed side of the logical rectangle). Corners within the Side Angle threshold
of 180 are considered for removal from the logical rectangle. In order for a triangle to actually be detected, corners for
both the point and side criteria must be met. The default Point Angle threshold is 45, and the default Side Angle threshold
is 27. Figure 14 provides an illustration.
315
Trelis 15.0 User Documentation
Figure 14 - Triangle Detection Settings
Split Skew
The Split Skew function can be called with the following command:
Split Surface <id_list> Skew [Preview] [Create]
This command will split a surface or list of surfaces in a logical way to reduce the amount of skew in a quadrilateral mesh.
This function uses the control skew algorithm to determine where to make these logical splits. Users should note that Split
Skew can only be utilized effectively on surfaces that lend themselves to a structured meshing scheme. These surfaces
cannot have multiple curve loops. Figure 15 shows a simple example of a surface being split.
split surface 1 skew
Figure 15. Split Skew applied to an L-shaped surface
316
Split Surface
The Preview keyword will show a graphics preview of the splitting curves. If the Create keyword is also specified, free
curves will be created.
317
Section Command
This command will cut a body or group of bodies with a plane, keeping geometry on one side of the plane and discarding
the rest. The syntax for this command is:
Section {Body|Group} <id_range> [With] {Xplane|Yplane|Zplane} [Offset <value>] [NORMAL|Reverse]
[Keep]
Section {Body|Group} <id_range> With Surface <id> [NORMAL|Reverse] [Keep]
In the first form, the specified coordinate plane is used to cut the specified bodies. The offset option is used to specify an
offset from the coordinate plane. In the second form, an existing (planar) surface is used to section the model. In either
case, the reverse keyword results in discarding the positive side of the specified plane or surface instead of the other side.
The keep option results in keeping both sides; the section command used with this option is equivalent to webcutting with
a plane.
319
Separating Multi-Volume Bodies
The separate command is used to separate a body with multiple volumes into a multiple bodies with single volumes.
To separate a body
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Volume.
Click on the Modify action button.
Select Separate from the drop-down menu.
Enter in the appropriate value for Volume ID(s). This can also be done using the Pick Widget function.
Click Apply.
Separate {Body|Volume} <id_range|all>
Only very rarely will this command be needed. It is provided for the occasional instance that a multi-volume body is found.
Another related command allows the user to control the separation of bodies after webcutting. In most instances the user
will want to separate bodies after webcutting. One reason to possibly have this option turned off is to be able to keep track
of all the volumes during a webcut. Setting this option to "off" keeps all volumes in the same body. But the more common
approach is to name the original body and allow naming to keep track of volumes. This setting is on by default. The syntax
is:
Set Separate After Webcut [ON|Off]
321
Separating Surfaces from Bodies
The separate surface command is used to separate a surface from a sheet body or a solid body.
To separate a surface from a body
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Split from the drop-down menu.
Select Separate from the drop-down menu.
Enter in the appropriate value for Surface ID(s). This can also be done using the Pick Widget function.
Click Apply.
Separate Surface <range>
Separating a surface from a solid body will create a "hole" in the solid body. Thus the solid body will become a sheet
body. The newly separated surface will be also sheet body, but it will have a different id. Multiple surfaces can be
separated from a body at the same time, but each separated surface will result in a distinct sheet body, as if the command
had been performed on each surface individually.
323
Analyzing Geometry
The following operation analyzes the ACIS geometry and will indicate problems detected
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Modify action button.
Select Heal from the drop-down menu.
Select Analyze or Autoheal.
Enter in the Filename.
Enter in any other appropriate settings from this menu.
Click Apply.
Healer Analyze Body <id_range> [Logfile ['filename'] [Display]]
The logfile option writes the analysis results to the filename specified, or to 'healanalysis.log' by default. In the GUI
version of Trelis, the display option will write the results in a dialog window.
The outputs include an estimate of the percentage of good geometry in each body. The optional logfile will include
detailed information about the geometry analysis. By default Trelis will also highlight the bad geometry in the graphics and
give a printed summary indicating which entities are "bad". Sample output from this command is shown below:
Percentage good geometry in Body 9: 98%
HEALER ANALYSIS SUMMARY:
-----------------------Analyzed 1 Body: 9
Found 2 bad Vertices: 51, 52
Found 3 bad Curves: 76, 77, 80
Found 2 bad CoEdges. The Curves are: 76
Found 1 Bodies with problems: 9
Journaled Command: healer analyze body 9
Note that it is not necessary to analyze the geometry before healing; however, it can be useful to analyze first rather than
healing unnecessarily. Also note that healer analysis can take a bit of time, depending on the complexity of the geometry
and how bad the geometry is.
The validate geometry commands work independently of the healer and give more detailed information.
Healer Settings
You can control the outputs from the healer with the following commands:
Healer Set OnShow {Highlight|Draw|None}
Healer Set OnShow {Badvertices|Badcurves|Badcoedges|Badbodies|All} {On|Off}
Healer Set OnShow Summary {On|Off}
These settings allow you to highlight, draw or ignore the bad entities in the graphics. You can control which entity types to
display, as well as whether or not to show the printed summary at the end of analysis.
After you have analyzed the geometry (which can take some time), you can show the bad geometry again with the
"show" command. This command simply uses cached data (healing attributes - see the next section) from the previous
analysis.
Healer Show Body <id_list>
325
Trelis 15.0 User Documentation
326
Healing Attributes
Once the geometry is analyzed, the results are stored as attributes on the solid model - this allows you to use the "show"
command to quickly display the bad geometry again. The results attributes are automatically removed when the geometry
is exported or any boolean operations are performed. They can also be explicitly removed with the command
Healer CleanAtt Body <id_range>
You can force the results to be removed immediately after each analyze operation with the "CleanAtt" setting (this can
save a little memory):
Healer Set CleanAtt {On|Off}
327
Auto Healing
Healing is an extremely complex process. The general steps to healing are:
•
•
•
•
•
•
Preprocess - trim overhanging surfaces and clean topology (remove small curves and surfaces).
Simplify - converts splines to analytic representations, if possible.
Stitch - geometry cleanup and stitching loose surfaces together to form bodies.
Geometry Build - repairing and building geometry to correct gaps in the model.
Post-Process - calculating pcurves and further repairing bad geometry.
Make Tolerant Curves & Vertices - a last optional step that allows special handling of unhealed entities for
booleans - allowing inaccurate geometry to be tolerated.
Autohealing makes these steps automatic with the following command:
To use Autohealing
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Modify action button.
Select Heal from the drop-down menu.
Select Autoheal.
Enter in the Filename.
Enter in any other appropriate settings from this menu.
Click Apply.
Healer Autoheal Body <id_range> [Rebuild] [Keep] [Maketolerant] [Logfile ['logfilename'] [Display]]
The rebuild option unhooks each surface, heals it individually, then stitches all the surfaces back together and heals
again. In some cases this can more effectively fix up the body, although it is much more computationally intensive and is
not recommended unless normal healing is unsuccessful.
The keep option will retain the original body, putting the resulting healed body in a new body.
The maketolerant option will make the edges tolerant if ACIS is unable to heal them. This can result in successful
booleans even if the body cannot be fully healed - ACIS can then sometimes "tolerate" the bad geometry. Note that the
healer analyze command will still show these curves as "bad", even though they are tolerant. The validate geometry
commands however take this into consideration.
The output from the autoheal command can be written to a file using the logfile option; the default file name is
autoheal.log. The display option works as before, displaying the results in a window in the GUI version of Trelis.
329
Spline Removal
If healing fails to convert spline surfaces to analytic ones fails, the simplification tolerance can be modified and healing rerun:
healer default simplifytol .1
healer autoheal body 1
Spline surfaces can also be forced into an analytic form (use this command with caution):
Healer Force {Plane|Cylinder|Cone|Sphere|Torus} Surface <id_list> [Keep]
The Keep option will retain the original body and generate a new body containing analytic surfaces. Note: Spline curves
can be found using entity filters:
Execute Filter Curve Geometry_type Spline
331
What if Healing is Unsuccessful?
The ACIS healing module is under continued development and is improving with every release. However, there will often
be situations where healing is unable to fully correct the geometry. This might be okay, as meshing is rarely affected by
the small inaccuracies healing addresses. However, boolean operations on the geometry can fail if the bad geometry
must be processed by the operation (i.e., a webcut must cut through a bad curve or vertex).
Here are some possible methods to fix this bad geometry:
•
•
•
•
•
•
Return to the source of the geometry (i.e., Pro/ENGINEER) and increase the accuracy. Re-export the geometry.
Heal again using the rebuild option.
Heal again using the make tolerant option.
Remove the offending surface from the body (using the remove surface command), then construct new
surfaces from existing curves and combine the body back together.
Composite the surfaces over the bad area, mesh and create a net surface from the composite, remove the bad
surfaces and combine.
Export the geometry as IGES, import the IGES file into a new model and look for double surfaces or surfaces
that show up at odd angles using the find overlap commands. Delete and recreate surfaces as needed and
combine the surfaces back together into a body.
Contact the development team ([email protected]) if you need further help with fixing bad geometry.
333
Tweaking Vertices
The Tweak Vertex command can be used to do the following:
•
•
•
Tweaking a Vertex With a Chamfer
Tweaking a Vertex With a Non-Equal Chamfer
Tweaking a Vertex With a Fillet Radius
Tweaking a Vertex With a Chamfer
To tweak a vertex with a simple chamfer
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Vertex.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Enter the appropriate values for Vertex ID(s). This can also be done using the Pick Widget function.
Select Simple Chamfer from the drop-down menu.
Enter the appropriate value for Radius Value.
Click Apply.
Tweak Vertex <id_range> Chamfer Radius <value>[Keep] [Preview]
This form of the command creates a chamfered corner at the specified vertex. Can be use on volumes or free surfaces.
The 'keep' option creates another volume on which the tweak is applied; the original volume remains unmodified.
Figure 1. Tweak Vertex Chamfer
335
Trelis 15.0 User Documentation
Tweaking a Vertex With a Non-Equal Chamfer
To tweak a vertex with a complex chamfer
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Vertex.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Enter the appropriate values for Vertex ID(s). This can also be done using the Pick Widget function.
Select Complex Chamfer from the drop-down menu.
Enter the appropriate values for Chamfer Radius 1, Chamfer Radius 2 and Chamfer Radius 3.
Enter the appropriate values for each Along Curve.
Click Apply.
Tweak Vertex <id_range> Chamfer Radius <value> [Curve <id> Radius <value> Curve <id> Radius
<value> Curve <id>] [Keep] [Preview]
This next form of the command creates a non-equal chamfered corner at the specified vertex. Can only be used on
vertices of volumes. The 'keep' option creates another volume on which the tweak is applied; the original volume remains
unmodified.
Tweaking a Vertex With a Fillet Radius
To tweak a vertex with a fillet vertex
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Vertex.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Enter the appropriate values for Vertex ID(s). This can also be done using the Pick Widget function.
Select Fillet Radius from the drop-down menu.
Enter the appropriate value for Radius Value.
Click Apply.
Tweak Vertex <id_range> Fillet Radius <value> [Keep] [Preview]
This command replaces a vertex with a filleted radius. The command can only be used on free surfaces. The 'keep' option
creates another volume on which the tweak is applied; the original free surface remains unmodified.
336
Tweaking Vertices
Figure 2. Tweak Vertex Fillet
337
Tweaking Curves
The following options of the Tweak Curve command are available. Command syntax and description follow below.
•
•
•
•
•
Create a Chamfer or Fillet
Tweaking a Curve Using an Offset Distance
Removing a Curve
Tweaking a Curve Using a Target Surface, Curve, or Plane
Tweaking a Pair of Curves to a Corner
Create a Chamfer or Fillet
The Tweak Curve Chamfer or Fillet command is used to fillet or chamfer a curve. The radius value is the radius of the fillet
arc or chamfer cut distance. The command syntax is:
To tweak a curve using the chamfer or fillet radius
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Curve.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Enter the appropriate value for Curve ID(s). This can also be done using the Pick Widget function.
Select Fillet Radius or Chamfer Radius from the drop-down menu.
Enter in the appropriate information.
Click Apply.
Tweak Curve <id_range> {Fillet|Chamfer} Radius <value> [Keep] [Preview]
In addition to creating chamfers of a single cut distance, the chamfer can be specified be two values.
Tweak Curve <id_list> Chamfer Radius <val1> [<val2>] [Keep] [Preview]
Figure 1 shows a brick ('br x 10') chamfered with two different cut distances ('Tweak Curve 1 2 Chamfer Radius 2 4').
Figure 1 Chamfer with two different distances
Individual curves can also be filleted with different start and finish radius values. The syntax is:
339
Trelis 15.0 User Documentation
Tweak Curve <id> Fillet Radius <val1> [<val2>] [Keep] [Preview]
Figure 2 shows a brick ('br x 10') filleted with different start and end radius values (‘Tweak Curve 1 2 Chamfer Radius 2
4’).
Figure 2. Fillet with two different radii
For all Tweak Fillet and Tweak Chamfer variations, the keep option prevents the destruction of the original geometry after
the operation and the preview option temporarily displays the new geometry configuration without actually changing the
geometry.
Tweaking a Curve Using an Offset Distance
To tweak a curve using offset
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Curve.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Enter the appropriate value for Curve ID(s). This can also be done using the Pick Widget function.
Select Offset from the drop-down menu.
Enter in the appropriate Offset Value.
Click Apply.
Tweak Curve <id_list> Offset <val> [Curve <id_list> Offset <val>] [Curve <id_list> Offset <val>
...] [Keep] [Preview]
Tweaking curves a specified distance offsets the existing curves and extends the attached surfaces to meet them. A
positive offset value will enlarge the surface while a negative value will decrease the area of the attached surface.
Different offset values can be specified for each curve. The keep option prevents the destruction of the original geometry
after the operation. The preview option temporarily displays the new geometry configuration without actually changing the
geometry. Figure 3 shows an example of offsetting a curve a specified distance.
340
Tweaking Curves
Figure 3 Offsetting a set of curves a specified distance
Removing a Curve
To remove a curve
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Curve.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Enter the appropriate value for Curve ID(s). This can also be done using the Pick Widget function.
Select Remove from the drop-down menu.
Click Apply.
Tweak Curve <id_list> Remove [Keep] [Preview]
Similar to the Tweak Curve Remove command, the tweak curve remove function removes a specified curve from a sheet
body. Figure 4 shows a simple example of removing a curve from a sheet body.
Figure 4. Removing a curve from a sheet body
The keep option prevents the destruction of the original geometry after the operation. The preview option temporarily
displays the new geometry configuration without actually changing the geometry.
341
Trelis 15.0 User Documentation
Tweaking a Curve Using Target Surfaces, Curves, or Plane
Use Tweak Curve Target to offset a curve to a specified surface, plane or curve. Figure 5 shows an example of tweaking
a curve to several surfaces.
Figure 5 Tweaking a curve to multiple target surfaces
Similarly, a target plane can be specified using the Plane specification syntax.
To tweak a curve using a target surface
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Curve.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Enter the appropriate value for Curve ID(s). This can also be done using the Pick Widget function.
Select Target Surface from the drop-down menu.
Enter the appropriate value for Surface ID. This can also be done using the Pick Widget function.
Click Apply.
Tweak Curve <id_list> Target {Surface >id_list> [Limit Plane (options)] [EXTEND|Noextend] | Plane
(options)} [Max_area_increase <val>] [Keep] [Preview]
To tweak a curve using a target curve
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Curve.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Enter the appropriate value for Curve ID(s). This can also be done using the Pick Widget function.
Select Target Curve from the drop-down menu.
Enter the appropriate value for Curve ID. This can also be done using the Pick Widget function.
Click Apply.
Tweak Curve <id_list> Target Curve <id_list > [EXTEND|Noextend] [Max_area_increase <val>]
[Keep] [Preview]
If a target surface is supplied, the user can also use a limit plane if he wishes. A limit plane is a plane that the tweak will
stop at if the tweaked curve does not completely intersect the target surface. The limit plane must be used with the extend
option. See the help for Specifying a Plane for the options available to define a plane.
342
Tweaking Curves
It should be noted that if the source and target surfaces are from the same body the resulting geometry will be
automatically stitched. Single target surfaces are automatically extended so that the tweaked body will fully intersect the
target. Unfortunately, extending multiple target surfaces can sometimes result in an invalid target, so the option is given to
tweak to non-extended targets with the noextend option. In this case, the tweaked body must fully intersect the existing
targets for success. If you experience a failure when tweaking to multiple targets or the results are unexpected, it is
recommended to try the noextend option (NOTE: Tweaking to multiple targets is only implemented in the ACIS geometry
engine). If a value for the max_area_increasekeyword is given, Trelis will not perform the tweak if the resulting surface
area increases by more than the specified amount. The keyword expects a percentage to be entered (i.e. '50' for 50%). It
is recommended to always preview before using the tweak target commands.
For all tweak target variations, the keep option prevents the destruction of the original geometry after the operation and
the preview option temporarily displays the new geometry configuration without actually changing the geometry.
Although it may not be intuitive curves can also serve as the target geometry. Figure 6 shows an example of extending a
curve to another curve.
Figure 6 Tweaking a curve to a target curve
Notice that the source curve actually extends to the target curve as if the target were a surface.
Tweaking a Pair of Curves to a Corner
When creating mid-surface geometry it is often useful to extend surfaces to form a corner. To handle this specific but
common case use the tweak corner command.
To tweak a pair of curves to a corner
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Curve.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Enter the appropriate value for Curve ID(s). This can also be done using the Pick Widget function.
Select Corner from the drop-down menu.
Enter the appropriate value for Curve ID. This can also be done using the Pick Widget function.
Click Apply.
343
Trelis 15.0 User Documentation
Tweak Curve <id> <id> Corner [Preview]
Figure 7 shows a typical tweak corner example. Notice that surfaces are extended/trimmed to intersect at a corner.
Figure 7. Tweaking two curves to a corner
The preview option temporarily displays the new geometry configuration without actually changing the geometry.
344
Tweaking Surfaces
The following options of the Tweak Surface command are available. Command syntax and examples follow below.
•
•
•
•
•
•
•
•
Tweaking a Surface Using an Offset
Tweaking a Surface by Moving
Tweaking Surfaces to Target Surfaces
Removing a Surface
Tweaking a Conical Surface
Tweaking Doublers to Target Surface
Removing Holes and Slots from Sheet Bodies
Removing Fillets from Sheet Bodies
Tweaking a Surface Using an Offset
To tweak a surface using offset
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Select Offset from the drop-down menu.
Enter the appropriate value for Surface ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate Offset Value.
Click Apply.
Tweak Surface <id_list> Offset <val> [Surface <id_list> Offset <val>] [Surface <id_list> Offset <val>
...] [Keep] [Preview]
The Tweak Offset form of the command offsets an existing set of surfaces and extends the attached surfaces to meet
them. A positive offset value will offset the surface in the positive surface normal direction while a negative value will go
the other way. Different offsets may be specified for each surface. Figure 1 shows a simple example of offsetting. Note
that you can also offset whole groups of surfaces at once. The keep option will retain the original surfaces and curves.
Figure 1. Tweak Offset
345
Trelis 15.0 User Documentation
Tweaking a Surface by Moving
The Tweak move form of the command simply moves the given surfaces along a vector direction. The direction can be
specified either absolutely or relative to other geometry entities in the model (from entity centroid to location). Note that
when moving a surface for tweak, the surface is moved and the surface and the adjoining surfaces are extended or
trimmed to match up again. So, for example, moving a vertically oriented planar surface in the vertical direction will have
no effect. In this example, if you move the surface 10 in the x and 5 in the y the effect will be to move it simply 10 in the x.
You can also use this form of the command to move a protrusion around - just be sure to specify all of the surfaces on the
protrusion for moving. The last form of the command can be used to move a surface along another surface's normal.
To tweak a surface moving
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Select Move Delta Distance, Move Normal to Surface, Move to Entity or Move to Location from the dropdown menu.
Enter in the appropriate settings from this menu.
Click Apply.
Tweak Surface <id_range> Move {Vertex|Curve|Surface|Volume|Body} <id> Location
{Vertex|Curve|Surface|Volume|Body} <id> [Except [X][Y][Z]] [Keep] [Preview]
Tweak Surface <id_range> Move {Vertex|Curve|Surface|Volume|Body} <id> Location <x_val>
<y_val> <z_val> [Except [X][Y][Z]] [Keep][Preview]
Tweak Surface <id_range> Move <dx_val> <dy_val> <dz_val> [Keep] [Preview]
Tweak Surface <id_range> Move Direction <options> Distance <val> [Keep] [Preview]
Tweak Surface <id_range> Move Normal To Surface <id> Distance <val> [Except [X][Y][Z]]
[Keep][Preview]
Tweaking Surfaces to Target Surfaces
The Tweak target form of the command actually replaces the given surfaces with a copy of the new surfaces, then
extends and trims surfaces to match up. This can be useful for closing gaps between components or performing more
complicated modifications to models. The command syntax is:
To tweak a surface using a target surface
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Select Target Surface from the drop-down menu.
Enter the appropriate value for Surface ID(s) and Target Surface ID(s). This can also be done using the Pick
Widget function.
Click Apply.
Tweak {Curve|Surface} <id_list> Target {Surface <id_list> [Limit Plane (options)] [EXTEND|noextend]
| Plane (options)} [keep] [preview]
Tweak Surface <id_list> Replace [With] Surface <id_list> [Keep] [Preview]
The plane option allows a plane to be specified instead of target surface(s). If a target surface is supplied, the user can
also use a limit plane if he wishes. A limit plane is a plane that the tweak will stop at if the tweaked surface does not
completely intersect the target surface. The limit plane must be used with the extend option. See the help for Specifying a
Plane for the options available to define a plane.
346
Tweaking Surfaces
Single target surfaces are automatically extended so that the tweaked body will fully intersect the target. Unfortunately,
extending multiple target surfaces can sometimes result in an invalid target, so the option is given to tweak to unextended
targets with the noextend option. In this case, the tweaked body must fully intersect the existing targets for success. If
you experience a failure when tweaking to multiple targets or the results are unexpected, it is recommended to try the
noextend option (NOTE: Tweaking to multiple targets is only implemented in the ACIS geometry engine). It is
recommended to always preview before using the tweak target commands.
Figure 2 shows a simple example.
Figure 2. Tweak Surface Target (Viewed directly from the side)
Removing a Surface
The Tweak remove command allows you to remove surfaces from a model by extending the adjacent surfaces to fill in
the resulting gaps. It is identical to the Remove Surface command. See Removing Surfaces for a description of the
command options.
To remove a surface
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Select Remove from the drop-down menu.
Enter the appropriate value for Surface ID(s). This can also be done using the Pick Widget function.
Click Apply.
Tweak Surface <id_list> Remove [EXTEND|Noextend] [Keepsurface] [Keep][Preview]
Tweaking a Conical Surface
The Tweak cone form of the command is used to replace a conical projection with a flat circular surface. This command
is useful for simplifying bolt holes. The command syntax is.
To tweak a conial surface
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Select Cone from the drop-down menu.
Enter the appropriate value for Surface ID(s). This can also be done using the Pick Widget function.
Click Apply.
Tweak Surface <id_range> Cone [Preview]
347
Trelis 15.0 User Documentation
The following is a simple example illustrating the use of the tweak surface cone command.
Figure 3. Conical bolt hole before and after tweaking
Tweaking Doublers to Target Surfaces
The Tweak Doubler form of the command takes a specified surface and creates drop-down surfaces either normal to the
doubler surface or by a user specified vector to a target surface. This can be helpful in creating surfaces for weld
elements between midsurfaced geometry. The resulting surfaces do not create a bounding volume, and do not imprint
themselves onto the target surface. The command syntax is:
To tweak doublers to target surfaces
348
Tweaking Surfaces
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Select Doubler from the drop-down menu.
Enter the appropriate value for Surface ID(s) and Target Surface ID(s). This can also be done using the Pick
Widget function.
Enter in the appropriate values for Direction and Limit Plane. Click on the Direction... or Limit Plane... button,
a window will appear to specify settings.
Click Apply.
Tweak Surface <id_list> Doubler Surface <id_list> {[Limit Plane (options)] [EXTEND|noextend]}
[Internal] [Direction (options)] [Thickness] [Preview]
The user can also use a limit plane with a target surface. A limit plane is a plane that the tweak will stop at if the tweaked
surface does not completely intersect the target surface. If you use the limit plane option, you must also use the extend
option. See the help for Specifying a Plane for the options available to define a plane.
Single target surfaces are automatically extended so that the tweaked body will fully intersect the target. Unfortunately,
extending multiple target surfaces can sometimes result in an invalid target, so the option is given to tweak to unextended
targets with the noextend option. In this case, the tweaked body must fully intersect the existing targets for success. If
you experience a failure when tweaking to multiple targets or the results are unexpected, trying the noextend option is
recommended.
If the doubler surface has a thickness property value, you can propagate that thickness value to the newly created dropdown surfaces by using the thickness flag.
It is recommended to always preview before using the tweak doubler commands.
NOTE: This function only works for ACIS geometry.
Geometry
Output
Figure 3. Extending a doubler surface to target
The internal option will also include internal curves when the surface is extended (see Figure 4c). The direction option
will create a skewed surface along the given direction (see Figure 4d).
349
Trelis 15.0 User Documentation
Figure 4. Explanation of tweak doubler options (a) Original surfaces (b) No option flags used (c) Internal option
used - notice internal curves dropped down (d) Direction flag - notice skew
Removing Holes and Slots from Sheet Bodies
The Tweak Hole/Slot Idealize command takes a specified sheet body(s) and searches for either holes or slots (or both)
which meet the user's input parameters. This can be helpful in removing small holes or slots quickly and efficiently from
midsurfaced bodies where such level of detail isn't required. The command syntax is:
To remove holes and slots from sheet bodies
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Select Idealize/Remove from the drop-down menu.
Enter the appropriate value for Surface ID(s). This can also be done using the Pick Widget function.
Select Holes or Slots from the Select Feature to Idealize menu.
Enter in the appropriate settings from this menu.
Click Apply.
Tweak Surface <id_list> Idealize {[Hole Radius <val>] [Slot Radius <val> Length <val>]} [Exclude
Curve <id_list>] [Preview]
Below is a diagram showing the different parameters available for input by the user.
350
Tweaking Surfaces
Figure 5. Input parameters for tweak surface idealize command
#Hole Removal Example
tweak surface 13 idealize hole radius 6
Figure 6. Example of hole removal using tweak surface idealize command
The exclude option allows the user to specify individual curves that should not be deleted, even if they meet the search
criteria for removal. Figure 7 shows another hole removal example where several curves were excluded.
Figure 7. Example of hole removal using exclude option
Note: This feature is for ACIS geometry
351
Trelis 15.0 User Documentation
It is recommended to always preview before using the tweak command. Preview will highlight all curves slated to be
removed if the command is executed.
Removing Fillets from Sheet Bodies
The Tweak Fillet Idealize command takes a specified sheet body(s) and searches for either internal or external fillets (or
both) which meet the users' radius parameter. This can be helpful in removing fillets quickly and efficiently from
midsurfaced bodies where such level of detail isn't required. The command syntax is:
To remove fillets from sheet bodies
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Select Idealize/Remove from the drop-down menu.
Enter the appropriate value for Surface ID(s). This can also be done using the Pick Widget function.
Select Fillets from the Select Feature to Idealize menu.
Enter in the appropriate settings from this menu.
Click Apply.
Tweak Surface <id_list> Idealize Fillet Radius <val> {[Internal] [External]} [Exclude Curve <id_list>]
[Preview]
#Fillet Removal Example
tweak surface 13 idealize fillet radius 6 internal
Figure 8. Example of fillet removal using tweak surface idealize command
Note: This feature is for ACIS geometry
It is recommended to always preview before using the tweak command. Preview will show the result if the command is
executed.
352
Tweaking Surfaces
Figure 9. Preview of the tweak surface idealize command
353
Tweak Remove Topology
The Tweak Remove Topology command removes curves and surface from a model and replaces them with new
topology. The reconstruction of the new topology and the stitching of it into the model is done using real solid modeling
kernel operations. This command is intended to be used on small curves and surfaces in the model. The command tries
to find small curves/surfaces neighboring the specified topology and includes these neighbors in the removal process.
Thus, the command can often be used to remove networks of small features just by specifying a single curve or surface.
To use the tweak remove topology operation
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface or Curve.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Select Remove Topology from the drop-down menu.
Enter the appropriate value for Surface ID(s) and Curve ID(s). This can also be done using the Pick Widget
function.
Enter the appropriate value for Small Curve Size and Backoff Distance.
Click Apply.
Tweak Remove_Topology {Surface <id_range> | Curve <id_range> | Surface <id_range> Curve
<id_range>} Small_curve_size <val> Backoff_distance <val>
The small_curve_size is input by the user, and is used to calculate the small curves and surfaces. The
backoff_distance value specifies how far away from the original topology cuts are made to cut out the old topology and
stitch in the new topology. The removed topology is replaced by simplified topology where possible often resulting in a
dimension reduction of the original topology. Extraneous curves that are introduced during the cutting and stitching
process are regularized out if possible using the solid modeling kernel regularize functionality or are composited out using
virtual geometry if the regularization is not possible.
Note: This command is currently only implemented for ACIS and Catia models.
Example
reset
set attribute on
import ACIS "test10.sat"
separate body all
set attribute off
Auto_clean Volume 1 Split_narrow_regions Narrow_size 2.2
tweak remove_topology curve 19 small_curve_size .21 backoff 1.5
355
Trelis 15.0 User Documentation
356
Tweak Remove Topology
Figure 1. Tweak Remove Topology command
357
Tweak Volume Bend
Entity bending bends a solid model around a given axis. In any bending operation, some material is stretched while other
material is compressed, but the topology of the model is maintained. The command syntax is:
Tweak {Volume|Body} <id_list> Bend Root <location_options> Axis <direction_vector> Direction
<direction_vector> Radius <val> angle <val> [Preview] [Keep] [Center_bend] [Location <options>]
Root and axis determine location for the bend. Direction determines direction of the bend. Radius and angle determine
how much to bend. Center_bend will bend both sides of the volume around the bend location instead of one side.
Location can be used to select only specific parts of a volume to bend.
Figure 1. Bending a volume
#Ex: Bend parts of a body specified by the location option
create brick width 11 height 1
create brick width 1 depth 10 height 10
create brick width 1 depth 10 height 10
create brick width 1 depth 10 height 10
move body 2 general location position -3 5 0
move body 3 general location position 0 5 0
move body 4 general location position 3 5 0
subtract body 2 from body 1
subtract body 3 from body 1
subtract body 4 from body 1
tweak volume 1 bend root 0 0 0 axis 1 0 0 direction 0 0 -1 radius 1 angle 3.14 location vertex 39 47
359
Removing Vertices
At times you may find that you have an extraneous vertex in your model. This would be a vertex connected to two and
only two edges. This stray vertex can cause unwanted mesh artifacts, due to the fact that a mesh node MUST lie on this
vertex, thereby disallowing the possibility of movement for better quality. Fortunately there is a relatively easy way of
getting rid of this stray vertex using the tweak surface command.
To replace with a surface
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Tweak from the drop-down menu.
Select Replace With Surface from the drop-down menu.
Enter the appropriate values for Surface ID(s) and replace with Surface ID. This can also be done using the
Pick Widget function.
Click Apply.
Tweak Surface <id> Replace With Surface <same_id>
Note that you are replacing a surface with itself. In doing so, the geometry engine will do an intersection check on that
surface, and should realize that the vertex doesn't need to be there.
361
Removing Surfaces
•
Remove Sliver Surfaces
The remove surface command removes surfaces from bodies. By default, it attempts to extend the adjoining surfaces to
fill the resultant gap. This is a useful way to remove fillets and rounds and other features such as bosses not needed for
analysis. See Figure 1 for an example of this process. The syntax for this command is:
To remove a surface
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Remove from the drop-down menu.
Enter the appropriate values for Surface ID(s). This can also be done using the Pick Widget function.
Enter any other appropriate settings from this menu.
Click Apply.
Remove Surface <id_range> [EXTEND|Noextend] [Keepsurface] [Keep] [Individual]
The noextend qualifier prevents the adjoining surfaces from being extended, leaving a gap in the body. This is sometimes
useful for repairing bad geometry - the surface can be rebuilt with surface from curves or a net surface, etc.., then
combined back onto the body.
The keep option will retain the original body and put the results of the remove surface in a new body. The keepsurface
option will retain the surface which was removed.
The individual option will remove surfaces one-by-one instead of as a group. If one removal fails, the rest are still
attempted. Without the individual option, no surface is removed unless they are all able to be removed.
This command is identical to the Tweak Surface Remove command.
Figure 1. Remove Surface Example
Remove Sliver Surface
This command uses the ACIS remove surface capability on surfaces that have area less than a specified area
limit. When ACIS removes a surface it extends the adjoining surfaces and intersects them to fill the gap. If it is not
possible to extend the surfaces or if the geometry is bad the command will fail. The syntax for this command is:
To remove slivers
1.
2.
3.
On the Command Panel, click on Geometry and then Volume.
Click on the Modify action button.
Select Remove Slivers from the drop-down menu.
363
Trelis 15.0 User Documentation
4.
5.
6.
Enter the appropriate values for Volume ID(s). This can also be done using the Pick Widget function.
Enter the appropriate values for Area Limit.
Click Apply.
Remove Slivers Body <id_range> [EXTEND|Noextend] [Keepsurface] [Keep] [Arealimit [<double>]]
Default Arealimit = 0.1
The noextend, keepsurface and keep options operate as for the remove surface command. The arealimit option allows
the user to set the area below which surfaces will be removed.
364
Automatic Forced Sweepability
In some cases, a volume can be "forced" into a sweepable configuration by compositing surfaces on the linking surfaces.
The automatic forced sweep command will attempt to automatically composite linking surfaces together to create a
sweepable topology. This command can be useful in cases where there are many linking surfaces that prohibit
sweepability and are not needed to define the mesh. It is assumed that the user has assigned the source and target
surfaces for the sweep prior to calling this function. Trelis will try to composite linking surfaces together to get rid of
problems such as 1) non-submappable linking surfaces, 2) interior angles between curves of a surface that deviate far
from multiples of 90 degrees, and 3) surfaces with curves smaller than the small curve size, if a small curve size is
specified. This command is incorporated into the ITEM GUI, but is also available from the command line using the
following command syntax.
To use automatic forced sweepability
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Modify action button.
Select Auto Clean from the drop-down menu.
Enter in the appropriate values for Volume ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate value for Small Feature Threshold Size.
Click Force Sweepability from the Select Auto Clean Method menu.
Click Apply.
Auto_clean Volume <id_range> Force_sweepability [Small_curve_size <val>]
The small_curve_size qualifier is an optional argument. If a curve size is specified, the command will try to remove
surfaces with curves smaller than this size by compositing the surface with adjacent surfaces.
Example
The following cylinder has been webcut and had surface splits so that it is not sweepable. The split surface command has
also introduced 3 small curves on the surfaces. After the source and target surfaces are set, the force sweepability
command is issued to automatically composite neighboring surfaces to make the volume sweepable and remove the
small curves. The results are shown in the image below.
auto_clean volume 1 force_sweepability small_curve_size .7
Figure 1. Linking surfaces are composited to force a sweepable volume topology
365
Trelis 15.0 User Documentation
366
Automatic Small Curve Removal
The automatic small curve removal command uses composites and collapse curves commands to automatically remove
small curves from a volume. This is useful for removing small or unnecessary details from a model to facilitate meshing
algorithms. The user enters a small curve size. Any curve smaller than this specified size will be removed. This command
is issued from the ITEM toolbar. More information can be found by reading the section entitled Small Details in the Model
in the ITEM documentation. This command can also be called from the command line. The syntax of this command is:
To remove small curves from a volume
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Modify action button.
Select Auto Clean from the drop-down menu.
Enter in the appropriate values for Volume ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate value for Small Feature Threshold Size.
Click Small Curves from the Select Auto Clean Method menu.
Click Apply.
Auto_clean Volume <id_range> Small_curves Small_curve_size <val>
Note: The automatic curve removal should be used with caution, as the user has little control over how curves are
removed.
Example:
The cylindrical model has 3 small curves just less than 0.7. The remove small curves command will remove two of the
small curves by compositing two neighboring surfaces and the third using the collapse curve functionality.
auto_clean volume 1 small_curves small_curve_size .7
Figure 1. Automatic small curve removal on a cylinder
367
Automatic Small Surface Removal
This auto clean command will attempt to remove small and narrow surfaces from the model by compositing them with
neighboring surfaces. The user specifies a small curve size value. This value is used in two different ways. First, a small
area is calculated as the small curve size squared. This value is used to compare against when looking for small surfaces.
The small curve size is also used to identify surfaces that are narrower than the small curve size.
To remove small and narrow surfaces from the model
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Modify action button.
Select Auto Clean from the drop-down menu.
Enter in the appropriate values for Volume ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate value for Small Feature Threshold Size.
Click Small Surfaces from the Select Auto Clean Method menu.
Click Apply.
Auto_clean Volume <id_range> Small_surfaces Small_curve_size <val>
Example
The cylindrical model has 2 small surfaces and a few narrow surfaces. The surfaces are composited to remove these.
Figure 1. Automatic small and narrow surface removal on a cylinder
369
Automatic Surface Split
This auto clean command will attempt to automatically split narrow regions of surfaces. In this context, any surface that
contains a portion that narrows down to a small angle is considered a narrow region. The command will use the split
command from the underlying solid modeling kernel. The user specifies a size that defines what is narrow. This command
also propagates the splits to neighboring narrow surfaces. This command is usually used as a preprocessor to the "tweak
remove_topology" command but can also be used on its own.
To automatically split narrow regions of surfaces
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Volume.
Click on the Modify action button.
Select Auto Clean from the drop-down menu.
Enter in the appropriate values for Volume ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate value for Small Feature Threshold Size.
Click Split Narrow Regions from the Select Auto Clean Method menu.
Click Apply.
Auto_clean Volume <id_range> Split_narrow_regions Narrow_size <val>
Example
The model has a surface that necks down to a narrow region. This surface also has some neighboring narrow surfaces to
which the splits are propagated.
Figure 1. Automatic small and narrow surface removal on a cylinder
371
Regularizing Geometry
The regularize command removes unnecessary topology, which in effect reverses the imprint operation. This can help
clean up the model from extra features that are unnecessary for the geometric definition of the model.
To remove unnecessary topology
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry.
Click on Volume, Surface, Curve or Vertex.
Click on the Modify action button.
Select Regularize from the drop-down menu.
Enter in the appropriate values for Volume ID(s), Surface ID(s), Curve ID(s) or Vertex ID(s). This can also be
done using the Pick Widget function.
Click Apply.
Regularize Body|Group|Surface|Curve|Vertex <range>
If you are frequently using web-cutting or other boolean operations to decompose your geometry, it may be convenient to
always generate regularized geometry. To set creation of regularized geometry during boolean operations use the
following command:
Set Boolean Regularize [ON | off]
373
Finding Surface Overlap
The surface overlap capability finds surfaces that overlap each other, with the capability to specify a distance and angle
range between them. This is useful for debugging geometry imprinting and merging problems, as well as for finding gaps
in large assembly models. Finding overlapping geometry is done using the command:
Find [Surface] Overlap [{Body|Surface|Volume} <id_list> [Filter_Sliver]
If a list of entities is not specified, all bodies in the model are checked. By default the command does not check the
surfaces within a given body against each other; rather, it only checks surfaces between bodies. This can be overridden
by inputting a surface list (i.e. find overlap surface all), or with a setting (see below).
The filter_sliver option will remove false positives from the list by weeding out sliver surfaces that have a merged curve
between them. The following pictures is an example of a sliver surface.
Figure 1. Example of a sliver surface
If curves 27 and 29 are merged before you run the find overlapping surface checkthe user will get the two surfaces in the
picture as an overlapping surface pair. However, if the filter_sliver keyword is used, Trelis will not find the two surfaces to
be overlapping.
Facetted Representation
This command works entirely off of the facetted surface representation of the model (the facetted representation is what
you see in a shaded view in the graphics). There are inherent advantages and disadvantages with this method. The
biggest advantage is avoidance of closest-point calculations with NURBS based geometry, which tends to be slow. This
method also eliminates possible problems with unhealed ACIS geometry. The disadvantage is working with a less
accurate (i.e., facetted) representation of the geometry. To circumvent problems with this facetted geometry, various
settings can be used to control the algorithm. For example, you might consider using a more accurate facetted
representation of the model - see below.
375
Trelis 15.0 User Documentation
Find Overlap Settings
Various settings are used to control the precision and handling of overlaps during the find overlap process. A listing of the
settings that find overlap uses is printed using the command:
Find [Surface] Overlap Settings
These settings, and the commands used to control them, are described below.
Facet - Absolute/Angle - The angular tolerance indicates the maximum angle between normals of adjacent surface
facets. The default angular tolerance is 15 - consider using a value of 5 . This will generate a more accurate facetted
representation of the geometry for overlap detection. This can be particularly useful if the overlap command is not finding
surface pairs as you would expect, particularly in "curvy" regions. Note however that the algorithm will run slower with
more facets. The distance tolerance means the maximum actual distance between the generated facets and the surface.
This value is by default ignored by the facetter - consider specifying a reasonable value here for more accurate results.
Set Overlap [Facet] {Angle|Absolute} <value>
Gap - Minimum/Maximum - the algorithm will search for surfaces that are within a distance from the minimum to
maximum specified. The default range is 0 to 0.01. Testing has shown this to be about right when searching for coincident
surfaces. Gaps can be found by using a range such as 3.95 to 5.05.
Set Overlap {Minimum|Maximum} Gap <value>
Angle - Minimum/Maximum - the algorithm will search for surfaces that are within this angle range of each other. The
default range is 0.0 to 5.0 degrees. Testing has shown that this range works well for most models. It is usually necessary
to have a range up to 5.0 degrees even if you are looking for coincident surfaces because of the different types of faceting
that can occur on curvy type surfaces. For example, for the case of a shaft in a hole, the facets of the shaft usually won't
be coincident with the facets of the hole, but may be offset by a certain distance circumferentially with each other. The 5
degree max angle range will account for this. If you find that the algorithm is not finding coincident surfaces when it
should, you can increase the upper range of this value. Note that this parameter is useful also for finding plates coming
together at an angle.
Set Overlap {Minimum|Maximum} Angle <value>
Normal - this setting determines whether to search for surfaces whose normals point in the same direction as each other
(same), away from each other (opposite) or either (any). The default is ANY, but it may be useful to limit this search to
opposite, as this would be the usual case for most finds.
Set Overlap Normal {ANY|opposite|same}
Tolerance - two individual facets must overlap by more than this area for a match to be found. Consider the two
cylindrical curves at the interface of the shaft and the block in Figure 2. Note that some of the facets actually overlap, even
though the curves will analytically be coincident. You can filter out false matches by increasing the overlap tolerance
area. The default value for this setting is 0.001.
Set Overlap Tolerance <value>
376
Finding Surface Overlap
Figure 2. Possible false find due to overlap (tolerance will prevent finding match)
Group - the surface pairs found can optionally be placed into a group. The name of the group defaults to
"overlap_surfaces".
Set Overlap Group {on|OFF}
List - by default the command lists out each overlapping pair - this can be turned off using the command:
Set Overlap List {ON|off}
Display - by default the command clears the graphics and displays each overlapping pair - this can be turned off using
the command:
Set Overlap Display {ON|off}
Body - by default the command will not search for overlapping pairs within bodies - only between different bodies. Turn
this setting on to search for pairs within bodies. Note however that this will slow the algorithm down.
Set Overlap [Within] {Body|Volume} {on|OFF}
Imprint - If on, Trelis will imprint the overlapping surfaces that it finds together. This will often force imprints that just
imprinting bodies together will miss. For each pair of overlapping surfaces, the containing body of one surface is imprinted
with the individual curves of the other surface, until the resulting surfaces no longer overlap.
Set Imprint {on|OFF}
377
Validating Geometry
To validate the geometry and topology
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry.
Click on Volume, Surface, Curve or Vertex.
Click on the Modify action button.
Select Validate from the drop-down menu.
Enter in the appropriate values for Volume ID(s), Surface ID(s), Curve ID(s) or Vertex ID(s). This can also be
done using the Pick Widget function.
Enter in the appropriate settings for the Validation/check level.
Click Apply.
Validate {Body|Volume|Surface|Curve|Vertex|Group} <id_range>
Validate {Volume|Surface|Curve|Vertex} <range> Mesh
The Validate {...} mesh command performs a connectivity check of the mesh elements to determine the validity of the
mesh.
More rigorous checking can be accomplished with the validate geometry commands by specifying a higher check level.
Use the following command to accomplish this:
set AcisOption Integer 'check_level' <integer>
where integer is one of the following:
10 = Fast error checks
20 = Level 10 checks plus slower error checks (default)
30 = Level 20 checks plus D-Cubed curve and surface checks
40 = Level 30 checks plus fast warning checks
50 = Level 40 checks plus slower warning checks
60 = Level 50 checks plus slow edge convexity change point checks
70 = Level 60 checks plus face/face intersection checks
You can also get more detailed output from the validate command with (the default is off):
set AcisOption Integer 'check_output' on
Note that some of the ids listed in the output of the validate command are currently meaningless, e.g. those for coedges.
The validate command can also check for consistent surface normals and return a list of offending surfaces. The syntax
for the command is as follows:
Validate [Body] <body_id> Normal [Reference [Surface] <surface_id>] [Reverse]
Using the "reference" keyword, a reference surface is compared to the normal consistency of all other specified surfaces.
Inconsistent surfaces can be reversed using the "reverse" keyword.
379
Debugging Geometry
The following command checks for inconsistencies in the Trelis topological model, by checking the specified entities and
all child topology and/or comparing to solid model topology:
Geomdebug Validate [compare] <entity_list>
This command checks for:
•
•
•
•
•
Consistent CoFace senses
Loops are closed/complete
Consistent CoEdge senses
Correct vertex order on curves w.r.t. parameterization
Correct tangent direction of curves w.r.t. parameterization
Related Commands:
Geomdebug Vertex <vertex_id>
Geomdebug Curve <curve_id>
Geomdebug Surface <surface_id>
Geomdebug body <body_id>
Geomdebug Containment {Curve | Surface} <id> {Location (options) | Node <id_list>}
The following command prints info about GeometryEntities owned by specified entity:
Geomdebug Geometry <entity_list> [interval <n>] [index <n>] [TEXT] [GRAPHIC] [attributes]
The following command lists (TopologyBridge) topology for specified entity:
Geomdebug solidmodel <entity_list> [index <n>] [depth<n>|up<n>|down<n>]
The following command lists GroupingEntities.
Geomdebug GPE <entity_list>
381
Geometry Accuracy
The accuracy setting of the ACIS solid model geometry can be controlled using the following command:
[set] Geometry Accuracy <value = 1e-6>
Some operations like imprinting can be more successful with a lower accuracy setting (i.e., 0.1 to 1e-5). However, it is not
recommended to change this value. Be sure to set it back to 1e-6 before exporting the model or doing other
operations as a higher setting can corrupt your geometry.
383
Trimming and Extending Curves
To trim or extend curves
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Curve.
Click on the Modify action button.
Select Trim from the drop-down menu.
Enter in the appropriate values for Volume ID(s). This can also be done using the Pick Widget function.
Select Curve or Vertex from the Trim At menu.
Enter in the appropriate settings for this menu.
Click Apply.
Trim Curve <id> AtIntersection {Curve|Vertex <id>} Keepside Vertex <id> [near]
Curves can be trimmed or extended where they intersect with another curve or at a vertex location. When trimming to
another curve, the curves must physically intersect unless they both are straight lines in which case the near option is
available. With the near option the closest intersection point is used to the other line - so it is possible to trim to a curve
that lies in a different plane. When trimming to a vertex, if the vertex does not lie on the curve, it is projected to the closest
location on the curve or an extension of the curve if possible.
The Keepside vertex is needed to determine which side of the curve to keep and which side to throw away. This vertex
need not be one of the curve's vertices, nor does it need to lie on the curve. However, if it is not on the curve it will be
projected to the curve and that location will determine which side of the curve to keep.
If the curve is part of a body or surface, it is simply copied first before trimming/extending. If it is a free curve a new curve
is created and the old curve is removed. The figures below show several examples of trimming/extending curves.
Trimming a Curve
Figure 1. Trimming a Curve to an Intersecting Curve
385
Trelis 15.0 User Documentation
Figure 2. Trimming a Curve to a Non-Intersecting Curve Using the Near Option
Figure 3. Trimming a Curve to a Vertex
Extending a Curve
Figure 4. Extending a Curve to An Intersecting Curve
386
Trimming and Extending Curves
Figure 5. Extending a Curve to a Non-Intersecting Vertex Using the Near Option
387
Stitching Sheet Bodies
The stitch command stitches together the specified sheet bodies into either a larger sheet body or a solid volume(s). The
tolerance value can be used when these sheet bodies don't line up exactly along the edges. This is common for IGES and
STEP models. Only manifold stitching is performed, i.e., edges will be shared with no more than two surfaces.
To stitch specified sheet bodies together
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Volume.
Click on the Modify action button.
Select Stitch from the drop-down menu.
Enter in the appropriate values for Volume ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate value for Tolerence Value.
Click Apply.
Stitch {Body|Volume} <id_range> [Tolerance <value>] [No_tighten_gaps]
This command has three stages to it:
1.
2.
3.
Stitch the surfaces together along overlapping edges Normally IGES and some STEP files do not contain
topological information that links surfaces together to share bounding curves. Stitching is an operation that
builds up this topological information.
Simplify geometry The command replaces splines with analytics where possible.
Tighten up gaps (inaccuracies) between the sheet bodies The command will build the geometry necessary
to tighten the gaps in the model.
When the stitch operation completes, a print statement lets the user know if the resulting body is not a closed, solid body.
If the no_tighten_gaps option is included, the third step of the stitching process is excluded. This may be necessary in
very large or complex models, where the regular approach fails.
389
Imprinting Geometry
To produce a non-manifold geometry model from a manifold geometry, coincident surfaces must be merged together (See
Geometry Merging); this merge can only take place if the surfaces to be merged have like topology and geometry. While
various parts of an assembly will typically have surfaces, which coincide geometrically, an imprint is necessary to make
the surfaces have like topology. There are three types of imprinting:
•
•
•
Regular Imprinting
Tolerant Imprinting
Mesh-Based Imprinting
To preview which surfaces can or should be imprinted, or to force imprints that the regular imprint command misses, the
Find Overlap command can be used.
Regular Imprinting
To imprint bodies together
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Volume.
Click on the Imprint Merge action button.
Select Imprint from the drop-down menu.
Enter in the appropriate values for Body ID(s). This can also be done using the Pick Widget function.
Click Apply.
Imprint [Volume|BODY] <range> [with [Volume|BODY] <range>] [Keep]
A body can also be imprinted with curves, vertices or positions, and surfaces can be imprinted with curves. It is useful to
imprint bodies or surfaces with curves to eliminate mesh skew, generate more favorable surfaces for meshing, or create
hard lines for paving. Imprinting with a vertex or position can be useful to split curves for better control of the mesh or to
create hard points for paving.
To imprint bodies with curves, vertices or positions
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Geometry and then Volume.
Click on the Imprint Merge action button.
Select Imprint from the drop-down menu.
Enter in the appropriate values for Body ID(s). This can also be done using the Pick Widget function.
Click the box With.
Select Curve ID(s), Vertex ID(s) or Location. and enter in the appropriate values.
If Location is selected, click on the Location... button. Another window will appear to specify setting.
Click Apply.
Imprint Body <body_id_range> [with] Curve <curve_id_range> [Keep]
Imprint Body <body_id_range> [with] Vertex <vertex_id_range> [Keep]
Imprint {Volume|Body} [with] Position <coords> [position <coords> ... ]
Imprint Surface <surface_id_range> [with] Curve <curve_id_range> [Keep]
An Imprint All will imprint all bodies in the model pairwise; bounding boxes are used to filter out imprint calls for bodies
which clearly don't intersect.
Imprint [Body] All
391
Trelis 15.0 User Documentation
Tolerant Imprinting
Normal imprinting may be ineffective for some assembly models that have tolerance problems, generating unwanted
sliver entities or missing imprints altogether. Tolerant imprinting is useful for dealing with these tolerance challenged
assemblies. To determine coincident and overlap entities, tolerant imprinting uses the merge tolerance. The commands
also include an optional tolerance value that will be used for the purposes of the single command. Specifying an optional
tolerance value will not change the default, system tolerance value.
A limitation of tolerant imprinting is that it cannot imprint intersecting surfaces onto one another, as normal imprinting can.
Tolerant imprinting imprints only overlapping entities onto one other.
To tolerant imprint
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry and then Volume.
Click on the Imprint Merge action button.
Select Tolerant Imprint from the drop-down menu.
Enter in the appropriate values for Body ID(s). This can also be done using the Pick Widget function.
Click Apply.
Imprint Tolerant {Body|Volume} <range> [tolerance <value>]
Tolerant imprinting can also be used to imprint curves onto surfaces, provided that the tolerance between surface and
curve(s) falls within the merge tolerance. The 'merge' option will merge the owning volume of the specified surface with all
other volumes that share any curves with this surface.
To tolerant imprint curves onto surfaces
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Imprint Merge action button.
Select Tolerant Imprint from the drop-down menu.
Select With Curve ID(s).
Enter in the appropriate values for Body ID(s) and With Curve ID(s). This can also be done using the Pick
Widget function.
Click Apply.
Imprint Tolerant Surface <id> with Curve <id_range> [merge] [tolerance <value>]
Imprint Tolerant Surface <id> <id> with Curve <id_range> [merge] [tolerance <value>]
Imprint Tolerant Surface <id><id> [tolerance <value>]
The second form of the command imprints the specified bounding curves of one surface onto another surface and vice
versa. Any specified curves that are not bounding either of the two specified surfaces will not be imprinted. The 'merge'
option will merge all the volumes sharing any curve of these two surfaces, after the imprint.
It is recommended that normal imprinting be used when possible and tolerant imprinting be used only when normal
imprinting fails.
Mesh-Based Imprinting
Another form of the imprint command,
Imprint Mesh {Body | Volume} <id_list>
uses coincident mesh entities and virtual geometry to create imprints. See the Partitioned Geometry section for more
information on this command.
392
Imprinting Geometry
Imprint Settings
After imprint operations, an effort is made to remove sliver entities: sliver curves and surfaces. Previously, all curves in
participating bodies less than 0.001 were removed. Newer versions of Trelis changed this because there might be times
when the user wants sliver curves/surfaces to be generated during an imprint operation. In order to give the user more
control over the cleanup of these sliver entities after imprint operations, a command was implemented so that the user can
set an 'imprint sliver cleanup tolerance'. The default tolerance for curves is the merge tolerance 0.0005. The default
tolerance for surfaces is a suitable tolerance chosen internally based on the bounding box of the entity. Sliver surfaces are
removed whose maximum gap distance among the long edges is smaller than the tolerance and who have at most three
long edges. A long edge is an edge whose length is greater than the specified tolerance.
Set {Curve|Surface} Imprint Cleanup Tolerance <value>
393
Merging Geometry
The steps of the geometry merging algorithm used in Trelis are outlined below:
1.
2.
3.
4.
5.
Check lower order geometry, merge if possible
Check topology of current entities
Check geometry of current entities
If both entities are meshed, check topology of meshes.
If geometric topology, geometry, and mesh topology are alike, merge.
Thus, in order for two entities to merge, the entities must correspond geometrically and topologically, and if both are
meshed must have topologically equivalent meshes. The geometric correspondence usually comes from constructing the
model that way. The topological correspondence can come from that process as well, but also can be accomplished in
Trelis using Imprinting.
If both entities are meshed, they can only be merged if the meshes are topologically identical. This means that the entities
must have the same number of each kind of mesh entity, and those mesh entities must be connected in the same way.
The mesh on each entity need not have nodes in identical positions. If the node positions are not identical, the position of
the nodes on the entity with the lowest ID will be used in the resulting merged mesh.
There are several options for merging geometry in Trelis.
Merge geometry automatically
Merge All [Group|Body|Surface|Curve|Vertex] [group_results][tolerance <value>]
All topological entities in the model or in the specified bodies are examined for geometric and topological correspondence,
and are merged if they pass the test.
If a specific entity type is specified with the Merge all, only complete entities of that type are merged. For example, if
Merge all surface is entered, only vertices which are part of corresponding surfaces being merged; vertices which
correspond but which are not part of corresponding surfaces will not be merged. This command can be used to speed up
the merging process for large models, but should be used with caution as it can hide problems with the geometry.
Test for merging in a specified group of geometry
Merge {Group|Body|Surface|Curve|Vertex} <id_range>[With {Group|Body|Surface|Curve|Vertex}
<id_range>][group_results][tolerance<value>]
All topological entities in the specified entity list, as well as lower order topology belonging to those entities, are examined
for merging. This command can be used to prevent merging of entities which correspond and would otherwise be merged,
e.g. slide surfaces.
Force merge specified geometry entities
Merge Vertex <id> with Vertex <id> Force
Merge Curve <id> with Curve <id> Force
Merge Surface <id> with Surface <id> Force
This command results in the specified entities being merged, whether they pass the geometric correspondence test or
not. This command should only be used with caution and when merging otherwise fails; instances where this is required
should be reported to the Trelis development team.
395
Trelis 15.0 User Documentation
Preventing geometry from merging
Body <id_range> Merge [On | Off]
Volume <id_range> Merge [On | Off]
Surface <id_range> Merge [On | Off]
Curve <id_range> Merge [On | Off]
Vertex <id_range> Merge [On | Off]
These commands provide a method for preventing entities from merging. If merging is set to off for an entity, merging
commands (e.g. "merge all") will not merge that entity with any other.
Other Merge Commands
Set Merge Test BBox {on|OFF}
This is an additional test for merging to see if a pair of surfaces should merge. First, it creates a bounding box for each
surface by summing individual bounding boxes of each of the surface's curves. A comparison is then made to see if these
two bounding boxes are within tolerance. This can help to weed out any potential incorrect merges that can result from
non-tight bounding boxes.
Set Merge Test InternalSurf {on|OFF|spline}
This is an extra check when merging surfaces. A point on one surface, closest to its centroid is found. Another point,
closest to this point is found on the other surface. If these two points are not within merge tolerance, the two surfaces will
not be merged. If set to on, all surface types will be included in this check. If set with the spline option, then splines are
only checked this way; analytic surfaces are excluded. This is another check to prevent incorrect merges from occurring.
396
Examining Merged Entities
There are several mechanisms for examining which entities have been merged. The most useful mechanism is assigning
all merged or unmerged entities of a specified type to a group, and examining that group graphically. This process can be
used to examine the outer shell of an assembly of volumes, for example to verify if all interior surfaces have been merged.
To put all the merged or unmerged entities of a given type into a specified group, use the command:
Group {<`name'>|<id>} [Surface | Curve | Vertex] [Merged | Unmerged]
If the entity type is unspecified, surfaces will be assumed.
Entities can also be labeled in the graphics according to the state of their merge flag. See the Preventing geometry from
merging section for information on controlling the merge flag. To turn merge labeling on for a specified entity type, use the
command
Label {Vertex | Curve | Surface} Merge
397
Merge Tolerance
Geometric correspondence between entities is judged according to a specified absolute numerical tolerance. The
particular kind of spatial check depends on the type of entity. Vertices are compared by comparing their spatial position;
curves are tested geometrically by testing points 1/3 and 2/3 down the curve in terms of parameter value; surfaces are
tested at several pre-determined points on the surface. In all cases, spatial checks are done comparing a given position
on one entity with the closest point on the other entity. This allows merging of entities which correspond spatially but
which have different parameterizations.
The default absolute merge tolerance used in Trelis is 5.0e-4. This means that points which are at least this close will
pass the geometric correspondence test used for merging.
To specify the merge tolerance
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry.
Click Volume, Surface, Curve or Vertex.
Click on the Imprint Merge action button.
Select Merge from the drop-down menu.
Enter in the appropriate values for Body ID(s), Surface ID(s), Curve ID(s) or Vertex ID(s). This can also be
done using the Pick Widget function.
Select Set Tolerance and enter in the appropriate value for Tolerance.
Click Apply.
Merge Tolerance <val>
If the user does not enter a value, the current merge tolerance value will be printed to the screen. There is no upper
bound to the merge tolerance, although in experience there are few cases where the merge tolerance has needed to be
adjusted upward. The lower bound on the tolerance, which is tied to the accuracy of the solid modeling engine in Trelis, is
1e-6.
Finding Nearly Coincident Entities
These commands find vertex-vertex, vertex-curve and vertex-surface pairs whose separation is within the specified
tolerance range. If a tolerance range isn't specified the default will be from merge tolerance to 10*merge tolerance. It is
useful for determining if you need to expand merge tolerance to accomodate sloppy geometry.
Find Near Coincident Vertex Vertex {Body|Volume} <id_range> [low_tol <value>] [high_tol <value>]
Find Near Coincident Vertex Curve {Body|Volume} <id_range> [low_tol <value>] [high_tol <value>]
Find Near Coincident Vertex Surface {Body|Volume} <id_range> [low_tol <value>] [high_tol <value>]
399
Unmerging
The unmerge command is used to reverse the merging operation. This is often in cases where further geometry
decomposition must be done.
To unmerge
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry.
Click Volume,Surface or Curve.
Click on the Imprint Merge action button.
Select Unmerge from the drop-down menu.
Enter in the appropriate values for Body ID(s), Surface ID(s) or Curve ID(s). This can also be done using the
Pick Widget function.
Click Apply.
Unmerge {all|<entity_list> [only]}
Un-merging an entity means that the specified geometric entity and all lower-order (or child) entities will no longer share
non-manifold topology with any other entities. For example, if a body is unmerged, that body will no longer share any
surfaces, curves, or vertices with any other body.
[Set] Unmerge Duplicate_mesh {On|OFF}
If any meshed geometry is unmerged, the mesh is kept as necessary to keep the mesh of higher-order entities valid. For
example, if a surface shared by two volumes is to be unmerged and only one of the volumes is meshed, the surface mesh
will remain with whichever surface is part of the meshed volume.
When unmerging meshed entities, the default behavior of the code is that the placement if the mesh is determined by the
following rules:
•
•
•
If neither entity has meshed parent entities, the mesh is kept on one of the two entities.
If one entity has a meshed parent entity, the mesh is kept on
that entity.
If both entities have meshed parents, the mesh is kept on one
and copied on the other.
If unmerge duplicate_mesh is turned on, the rules described above are overwritten and whenever a meshed entity is
unmerged the mesh is always copied such that both entities remain meshed.
To get back to the default behavior, turn unmerge duplicate_mesh off.
401
Using Geometry Merging to Verify Geometry
Geometry merging is often used to verify the correctness of an assembly of volumes. For example, groups of unmerged
surfaces can be used to verify the outer shell of the assembly (see Examining Merged Entities.) There is other information
that comes from the Merge all command that is useful for verifying geometry.
In typical geometric models, vertices and curves which get merged will usually be part of surfaces containing them which
get merged. So, if a Merge all command is used and the command reports that vertices and curves have been merged,
this is usually an indication of a problem with geometry. In particular, it is often a sign that there are overlapping bodies in
the model. The second most common problem indicated by merging curves and vertices is that the merge tolerance is set
too high for a given model. In any event, merged vertices and curves should be examined closely.
403
Composite Curves
To use the composite create operation for a curve
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Curve.
Click on the Modify action button.
Select Composite from the drop-down menu.
Enter in the appropriate settings for Curve ID(s). This can also be done using the Pick Widget function.
Select Create from the Select menu.
Enter in the appropriate values for Keep Vertex ID and Max Curve Angle.
Click Apply.
Composite Create Curve <id_range> [Keep Vertex <id_list>] [Angle <degrees>]
The additional arguments provide two methods to prevent vertices from being removed from the model or composited
over. The first method, keep vertex explicitly specifies vertices which are not to be removed. This option can also be used
to control which vertex is kept when compositing a set of curves results in a closed curve.
The angle option specifies vertices to keep by the angle between the tangents of the curves at that vertex. A value less
than zero will result in no composite curves being created. A value of 180 or greater will result in all possible composites
being created. The default behavior is an empty list of vertices to keep, and an angle of 180 degrees.
405
Composite Surfaces
To use the composite create operation for a surface
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Composite from the drop-down menu.
Enter in the appropriate settings for Surface ID(s). This can also be done using the Pick Widget function.
Select Create from the Select menu.
Enter in the appropriate values for Max Surface Angle, Keep Vertex ID and Max Curve Angle.
Click Apply.
Composite Create Surface <id_range> [Angle <degrees>] [Nocurves] [Keep [Angle <degrees>]
[Vertex <id_list>]]
Related Commands
Graphics Composite {on|off}
The angle argument prevents curves from being removed from the model or composited over. Composites will not be
generated where the angle between surface normals adjacent to the curve is greater than the specified angle.
When a composite surface is created, the default behavior is also to composite curves on the boundary of the new
composite surface.
Curves are automatically composited if the angle between tangents at the common vertex is less than 15 degrees. The
nocurves option can be used to prevent any composite curves from being created.
The keep keyword can be used to change the default choice of which curves to composite. The arguments following the
keep keyword behave the same as for explicit composite curve creation. The nocurves and keep arguments are mutually
exclusive.
Controlling the Surface Evaluation Method for Composite
Surfaces
It typically takes longer to mesh a single composite surface than to mesh the surfaces used in the creation of the
composite. To improve speed, composite surfaces use an approximation method to evaluate the closest point to a
trimmed surface. However, this evaluation method may give poor results for composites of highly convoluted surfaces.
The virtual geometry module provides a way to change the way surfaces are evaluated using the following command:
Composite Closest_pt Surface <id> {Gme|Emulate}
The default behavior is to use the emulate method, as it is typically considerably faster. Specifying the gme option will
force the specified composite surface to use the exact calculation of the closest point to a trimmed surface, as provided by
the solid modeler. The gme option, however, can be considerably slower.
Composite Determination
The composite create surface command is non-deterministic in some circumstances. When three or more adjacent
surfaces are to be composited, all the surfaces may not be able to be composited into a single surface as illustrated in
Figure 1. In this case different subsets of the surfaces may be composited and the command will choose arbitrary subsets
to composite. As an example, there are three surfaces A, B, and C, all adjacent to each other. The common curve
between A and B is AB, the common curve between B and C is BC, and the common curve between A and C is CA. If the
curve BC cannot be removed, either due to the angle specified in the composite command, or because there is a fourth
surface, D, also using that curve, the command will arbitrarily choose to either composite A and B or A and C.
407
Trelis 15.0 User Documentation
Figure 1. In some cases, the program will make a determination of which surfaces to composite.
408
Partitioned Curves
There are four methods for specifying locations at which to partition curves:
The first two forms of the command create additional vertices and use those vertices to split a curve. The third form of the
command uses existing vertices to split the curve. The fourth form of the command uses existing nodes to split the curve.
To partition curves by using verticies
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Curve.
Click on the Modify action button.
Select Partition from the drop-down menu.
Select Create Using Vertices from the drop-down menu.
Enter in the appropriate values for Cure ID(s) and Vertex ID(s). This can also be done using the Pick Widget
function.
Click Apply.
Using the fraction option, vertices are created at the specified fractions along the curve (in the range [0,1].)
Subsequently, the curve is split at each vertex, resulting in n+1 new curves, where n is the number of fraction values
specified.
To partition curves by using a fraction list
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Curve.
Click on the Modify action button.
Select Partition from the drop-down menu.
Select Create Using Fraction List from the drop-down menu.
Enter in the appropriate values for Cure ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate values for Fraction List.
Click Apply.
Using the position option, vertices are created at the closest location along the curve to each of the specified position.
Subsequently, the curve is split at each vertex, resulting in n+1 new curves, where n is the number of positions specified.
To partition curves by using coordinates
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Curve.
Click on the Modify action button.
Select Partition from the drop-down menu.
Select Create Using Coordinates from the drop-down menu.
Enter in the appropriate values for Cure ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate values for X Position, Y Position and Z Position.
Click Apply.
If the node option is used, meshed curves may be partitioned. The specified nodes must lie on the curve to be partitioned.
The curve is split at each node specified, and any other mesh entities are divided appropriately amongst the curve
partitions.
To partition curves by using nodes
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Curve.
Click on the Modify action button.
Select Partition from the drop-down menu.
Select Create Using Nodes from the drop-down menu.
Enter in the appropriate values for Cure ID(s) and Node ID(s). This can also be done using the Pick Widget
function.
Click Apply.
Partition Create Curve <curve_id> {Fraction <fraction_list> | Position <xpos> <ypos> <zpos> | [with]
<vertex_list> | <node_list> }
409
Trelis 15.0 User Documentation
410
Partitioned Surfaces
There are several forms of the command to partition a surface. A surface may be partitioned using hard points, curves,
polylines, mesh edges, mesh faces or mesh triangles.
•
•
•
•
Partitioning with Vertices or Nodes
Partitioning with Curves
Partitioning with Mesh Edges
Partitioning with Mesh Faces or Triangles
Partitioning with Vertices and Nodes
Partitioning with Hard Points
There are two methods of partitioning a surface using vertices and nodes. The first method is to create a set of hard
points using nodes, vertices, or coordinates that constrain the mesh to particular points on the surface.
To partition a surface using vertices and nodes
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Partition from the drop-down menu.
Select Create With Nodes or Create With Verticies from the drop-down menu.
Enter in the appropriate value for Surface ID(s) as well as Vertex ID(s) or Node ID(s). This can also be done
using the Pick Widget function.
Click Apply.
Partition Create Surface <id> Vertex <id_list> [Individual]
Partition Create Surface <id> Node <id_list> [Individual]
Partitioning with Polylines
The second method is to define a polyline using a set of vertices or coordinates. This method splits the surface using a
polyline defined by a list of positions specified as either coordinate triples, or existing vertices. The polyline is projected to
the surface to define the curve for splitting the surface. If only one position is specified a zero-length curve with a single
vertex will be created The syntax is identical to above WITHOUT the individual option.
To partition a surface using coordinates
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Partition from the drop-down menu.
Select Create Using Coordinates from the drop-down menu.
Enter in the appropriate value for Surface ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate values for Position (X,Y,Z).
Click Apply.
Partition Create Surface <id> Position <x> <y> <z> [[Position] <x> <y> <z> ...]
To partition a surface using a set of vertices
1.
2.
3.
4.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Partition from the drop-down menu.
Select Create With Verticies from the drop-down menu.
411
Trelis 15.0 User Documentation
5.
6.
Enter in the appropriate values for Surface ID(s) and Vertex ID(s). This can also be done using the Pick
Widget function.
Click Apply.
Partition Create Surface <id> Vertex <id_list>
In the following simple example, the surface is partitioned using both methods. On the left half of the object, the surface is
partitioned using the individual option (vertices 11 12 15 13). On the right half, a polyline is used (vertices 9 10 16 14). All
of the free vertices can then be deleted, leaving the virtual curves shown in the second picture. Vertices 19 20 21 and 22
are all zero-length curves. The small 'v' in parentheses is to indicate that it is virtual geometry. The resulting mesh is
shown in the third picture. Notice that the polyline constrains the entire curve to the mesh, while the hardpoints constrain
only that individual point.
Figure 1. Partitioning a Surface Using Vertices
Partitioning with Curves
This form of the command splits the existing surface into several surfaces by creating curves that approximate the
projection of the specified existing curves onto the surface.
To partition a surface with curves
1.
2.
412
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Partitioned Surfaces
3.
4.
5.
6.
Select Partition from the drop-down menu.
Select Create With Curves from the drop-down menu.
Enter in the appropriate values for Surface ID(s) and Curve ID(s). This can also be done using the Pick
Widget function.
Click Apply.
Partition Create Surface <id> Curve <id_list>
Partitioning with Mesh Edges
Meshed surfaces may be partitioned with mesh edges. The specified mesh edges must be owned by the surface to be
partitioned. The shape of the curve(s) used to split the surface is specified by a set of mesh edges.
If the split location is specified by a series of mesh edges, and the specified mesh edges form a closed loop, the node
option may be used to control which node the vertex is created at.
To partition a surface using edges
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Partition from the drop-down menu.
Select Create With Edges from the drop-down menu.
Enter in the appropriate values for Surface ID(s) and Edge ID(s). This can also be done using the Pick Widget
function.
Optionally select Specify Nodes and enter the Node ID(s).
Click Apply.
Partition Create Surface <id> Edge <id_list> [Node <node_id>]
Partitioning with Faces or Triangles
Surfaces may also be partitioned by specifying a list of triangles or faces (quads). The boundary of the list will
automatically be detected and new curves and vertices created at the appropriate locations. Curves are created from the
mesh edges and used to split the surface. The surface mesh is split and assigned to the appropriate surface partitions.
To partition a surface using faces or triangles
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Partition from the drop-down menu.
Select Create With Quads or Create With Tris from the drop-down menu.
Enter in the appropriate values for Surface ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate values for Tris ID(s) or Quad/Face ID(s). This can also be done using the Pick Widget
function.
Click Apply.
Partition Create Surface <id> Face|Tri <id_list>
413
Partitioned Volumes
To partition a volume by giving a center and radius:
Partition Create Volume <id> Center [Location] {options} Radius <val>
This command splits the existing volume into two volumes. All volume elements that lie within the specified radius of the
specified center location are identified, and the exterior faces of these elements are used to create a surface and partition
the volume. The center can be specified with any of the location options.
Figure 1 shows an example of a partitioned volume. A cube that has been map meshed is partitioned using a center at
one of its vertices. The result is two distinct volumes with a surface separating the two. The interface surface is composed
of the faces of the interior hex elements.
Figure 1. A partitioned volume
This command may be useful for separating small regions of a meshed volume so that remeshing or mesh improvement
may be performed locally.
415
Using Mesh Intersections to Partition Surfaces
To assist in various mesh editing tasks such as joining, a mesh-based imprinting capability is provided. The command
Imprint Mesh {Body | Volume} <id_list>
determines imprint locations using the mesh on the surfaces of the specified bodies or volumes. Regions of coincidence
between the surfaces is determined by searching for coincident nodes in the mesh of the surfaces. Virtual geometry is
then used to partition the surfaces and curves at the boundary of these regions of coincident mesh.
The imprint mesh functionality differs from a normal geometric imprint in the following ways:
•
•
•
•
The location of the imprint is determined from coincidence of mesh nodes.
The mesh remains intact through the imprint operation.
Virtual geometry is used to create the imprint.
The imprinting can be done on all types of geometry (including mesh-based geometry, merged geometry, and
virtual geometry.)
The following is a trivial example of this capability. The following commands create two meshed blocks:
brick width 10
brick width 6
body 2 move x 8
volume 1 2 size 1
mesh volume 1 2
Figure 1 shows the results of these commands.
Figure 1. Two adjacent meshed volumes. The coincident meshes will form the basis of the imprint operation.
The mesh of the blocks can be joined by first doing a mesh-based imprint and then merging:
imprint mesh body 1 2
merge body 1 2
Figure 2. shows the results of the imprint operation. A meshed surface is created at the interface between the two meshed
volumes. The nodes on the new surface are shared by the neighboring hexahedra of both volumes.
417
Trelis 15.0 User Documentation
Figure 2. The imprinted surface. Adjacent volume meshes joined at the interface surface.
418
Removing Partitions
To remove partitions by merging or deleting
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry.
Click on Surface or Curve.
Click on the Modify action button.
Select Partition from the drop-down menu.
Enter in the appropriate values for Surface ID(s) or Curve ID(s).
Select Merge or Delete from the drop-down menu.
Click Apply.
Partition Merge {Curve|Surface|Volume} <id_list>
The command combines existing partitions where possible. This command is similar to the composite create command.
The difference is that this command is special-cased for partitions, and will result in more efficient geometric evaluations.
If all the partitions of a real solid model entity are merged, such that there is only one partition remaining, the virtual
geometry will be removed, and the original solid model geometry will be restored to the model.
The Trelis delete command can also be used for removing partitions. See Deleting Virtual Geometry for a description of its
use.
419
Collapse Angle
The collapse operation allows the user to collapse small angles using virtual geometry.
To collapse small angles
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Vertex.
Click on the Modify action button.
Select Collapse Angle from the drop-down menu.
Enter in the appropriate settings for Vertex ID. This can also be done using the Pick Widget function.
Enter in the appropriate setting on this menu for c1 and c2.
Click Apply.
Collapse Angle at Vertex <id> Curve <id1> [Arc_length1 <length>] Curve <id2> [Arc_length2
<length> | Same_size | Perpendicular | Tangent] [Composite_vertex <angle>] [Preview]
The collapse angle command is used to eliminate small angles at vertices, where curves meet at a tangential point. The
command will split each curve at a specified distance (?1 and ?2 ) as shown in Figure 1, and create two new vertices
along those curves. The remaining small angle will be composited into its neighboring surface using virtual geometry. The
options of the command allow you to specify where to split each curve. You must input a distance for the first curve ( ?1),
but the second location can be determined based on the length and direction of the first curve.
Figure 1. Collapse angle syntax
The arclength option will split each curve at a specified distance ?1 and ?2, (See Figure 1) measured from the vertex.
You must input at least one arclength for each of the options listed below.
The same_size option will split curve 2 so that the two resulting curves, ?1 and ?2, are the same length as shown in
Figure 2.
Figure 2. Collapse angle using the same_size option
The perpendicular option will split curve 2 so it is perpendicular to the split location on curve 1, as shown in Figure 3.
421
Trelis 15.0 User Documentation
Figure 3. Collapse angle using the perpendicular option
The tangent option will split curve 2 where a line tangent to curve 1 at the split location intersects curve 2, as shown in
Figure 4.
Figure 4. Collapse angle using the tangent option
The composite_vertex option automatically composites resulting surfaces if there are only two curves left at the vertex,
and the angle is less than a specified tolerance.
The preview option will preview composited surface before applying changes.
Figure 5. An example of a meshed surface that is generated after using the collapse angle command.
422
Collapse Angle
423
Collapse Curve
The collapse curve command allows the user to collapse small curves using virtual geometry. It is intended to be used in
cases where removing a small curve to simplify topology will facilitate meshing. The operation can be thought of as
reconnecting curves from one vertex on the small curve to the other vertex. If the user doesn’t specify which vertex to
keep during the operation Trelis will choose one of the vertices. The operation is performed using virtual partitions and
composites on the curves and surfaces surrounding the small curve. The command syntax is:
To collapse a curve
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Curve.
Click on the Modify action button.
Select Collapse from the drop-down menu.
Enter in the appropriate settings for Curve ID. This can also be done using the Pick Widget function.
Optionally select Collapse To. If this is done, enter in the appropriate settings for Vertex ID. This can also be
done using the Pick Widget function.
Enter in any other appropriate setting on this menu.
Click Apply.
Collapse Curve <id> [Vertex <id>] [Ignore] [Real_split]
The vertex keyword allows the user to specify which vertex on the small curve to keep during the operation or in other
words which vertex to "collapse to". Depending on the surrounding topological configuration some vertices cannot
currently be chosen so if the user specifies a vertex to collapse to that results in a complex topological configuration that
Trelis can’t currently handle the user will be notified and encouraged to pick a different vertex. If the user doesn’t specify a
vertex Trelis will attempt to choose the “best” vertex to keep based on surrounding topology and geometry. Currently, the
collapse curve command only handles curves where the vertex that is NOT retained has a valence of 3 or 4.
The ignore keyword allows the user to specify whether or not small portions of surfaces that are partitioned off of one
surface and composited with a neighboring surface during the collapse curve operation are considered when evaluating
the new composite surface. By specifying the ignore option the user tells Trelis that these small surfaces will be ignored
in future evaluations of the composite surface. This can be beneficial in cases where the small surface makes a sharp
angle with the neighboring surface it is being composited with. These first derivative discontinuities of composite surfaces
can make it difficult for the meshing algorithms to proceed and ignoring the small surfaces during evaluation can help
remedy this problem. By default the small surfaces will not be ignored.
The real_split option tells Trelis to use the solid modeling kernel's (ACIS) split surface functionality to do the splitting
rather than using virtual partitioning. The result is that you only have virtual composites at the end and no virtual partitions.
The main advantage of using this option is that the solid modeling kernel's split operation is often more reliable than the
virtual partition.
Figure 1 shows a typical example where the collapse curve command should be used to simplify the topology for
meshing.
425
Trelis 15.0 User Documentation
Figure 1. Example where the collapse curve operation is needed.
Figure 2 shows the above example after collapsing the small curve
Figure 2. Above example after collapsing the small curve.
426
Collapse Surface
The collapse surface command allows the user to remove surface boundaries from the model. This is accomplished by
splitting the surface at two given locations and combining it into two adjacent surfaces using virtual geometry operations.
The command syntax is:
To collapse a surface
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Geometry and then Surface.
Click on the Modify action button.
Select Collapse from the drop-down menu.
Enter in the appropriate settings for Surface ID and Into Surface ID(s). This can also be done using the Pick
Widget function.
Select Vertex, Position (X, Y, Z), Node or Location from the From Location menu and enter in the
appropriate values.
Select Vertex, Position (X, Y, Z), Node or Location from the To Location menu and enter in the appropriate
values.
Click Apply.
Collapse Surface <id> Across Location1 Location 2 With Surface <id_list> [Preview]
The locations option can use any of the general Trelis location commands. However, the vertex and curve options are
among the most useful location options. For example, the command
collapse surface 15 across vertex 128 curve 40 with surface 26 117
would split surface 15 by the line that is formed between vertex 128 and the midpoint of curve 40. It would then composite
the two parts of surface 15 that are adjacent to surfaces 26 and 117. The result is that three surfaces have been reduced
to two.
The collapse surface command is most useful in removing blended surfaces (i.e. fillets and chamfers) from a model. For
example, Figure 1 below shows a set of highlighted surfaces on a bracket. By collapsing all these surfaces the model
shown in Figure 2 is created. Collapsing the surfaces for this model simplifies the model and allows for the creation of a
higher quality mesh.
Figure 1. Bracket with chamfered edges.
427
Trelis 15.0 User Documentation
Figure 2. Bracket after highlighted edges have been collapsed
428
Simplify Geometry
Simplifying topology by compositing individually selected surfaces is often a tedious and time-consuming task. The
simplify command addresses the tedium by automatically compositing surfaces and curves based on selected criteria
between neighboring entities. Figure 1 shows a typical example of simplify command usage (‘simplify volume 1 angle 15’).
Figure 1. Typical Simplify command usage
The command syntax and discussion items are shown below.
To simplify topology by compositing selected surfaces
1.
2.
3.
4.
On the Command Panel, click on Geometry.
Clcik on Volume or Surface.
Click on the Modify action button.
Select Simplify from the drop-down menu.
429
Trelis 15.0 User Documentation
5.
6.
7.
8.
Enter the appropriate values for Surface ID(s) or Volume ID(s). This can also be done using the Pick Widget
function.
Optionally click Specify Angle and/or Specify 'Respect' Parameters.
Enter in the appropriate settings.
Click Apply.
Simplify {Volume|Surface|Curve} <range> [Angle< value >] [Respect {Surface <id_range> | Curve
<id_range> | Vertex <id_range>| Imprint | Fillet}] [Local_Normals] [Preview]
Feature Angle
Feature angle is defined as the angle between the average facet normals of two neighboring surfaces. If the angle is less
than the specified angle then the two surfaces are composited together (assuming any other specified criteria are met).
Feature angle is always used as criteria and if an angle is not specified the value is set to 15 degrees.
Automatically Compositing Curves
The simplify command can also be used to automatically composite curves using an angle tolerance. Curves will be
composited together only if they are explicitly specified in this command, and not as the result of two surfaces being
composited.
Respecting Vertices, Curves and Surfaces
Surfaces, curves, and vertices can be specified to prevent geometry features from automatically being composited. Figure
2 show an example of respecting a surface (‘simplify vol 1 angle 15 respect surf 289’).
Figure 2 Respecting a surface
For complex geometries, it is often useful to preview the simplify command and then add any respected geometry to the
command respect lists.
Respecting Imprints
Curves created by imprints can automatically be respected by the simplify command. Figure 3 shows an example of
geometry with split fillets.
430
Simplify Geometry
Figure 3 Respecting imprint geometry
Notice that in the split curves are respected by the Simplify command (‘simplify vol 1 angle 40 respect imprint’).
Using Local Normals
By default the command will compare the average normal of two adjacent surfaces to determine whether they should be
composited. By issuing the local_normal option, the test will be modifed slightly. The modified test will compare the
maximum difference between normals along the shared curve(s) for the two surfaces.
Figure 4. Comparison of surface normals using the average surface normal method (on the left) and local normal
method (on the right).
Other Options
The preview option shows what curves are respected without compositing any surfaces. It should also be pointed out that
multiple respect specifications can be chained together. For example:
Simplify volume 1 angle 15 respect curve 1 respect imprint respect fillet preview
431
Deleting Virtual Geometry
Removing Virtual Geometry
The following command removes all lower-order virtual geometry from the specified entities.
Virtual Remove <entity_list>
Examples:
virtual remove surface 5
Removes all composite and partition curves from surface 5.
virtual remove body all
Remove all virtual geometry from all bodies.
For removing individual virtual entities, see the sections of the documentation for each type of virtual entity:
•
•
•
•
Composite curves
Composite surfaces
Partition curves
Partition surfaces
Using The Delete Command With Composites
If the general delete command is invoked for a composite surface, the composite surface will be removed, and the
original surfaces used to define the composite will be restored to the model. The defining surfaces are NOT also deleted.
As with any other non-virtual surfaces, the delete command will fail if the composite has a parent volume.
To delete composite surfaces with a parent volume, the composite delete command can be used. The behavior is
analogous for composite curves.
If the delete command is used on a volume containing a composite surface or curve, or on a surface containing a
composite curve, the entire volume or surface will be deleted, including the original entities used to define the composite,
as those entities are also children of the entity being deleted.
Using the Delete Command With Partitions
It is recommended that the delete command not be used with partitions, as it may break subsequent usage of the merge
and delete forms of the partition command for other partitions of the same real geometry entity. However, if the delete
command is used for partitions, the behavior is to delete the specified partition, and when the last partition of the real
geometry is deleted, to restore the original geometry.
The delete command can also be used on parents of partitions. For example, a volume containing partitioned surfaces, or
a surface containing partitioned curves can be deleted. In this case, the specified entity will be deleted along with all of its
children, including the partition entities, and the original entities that were partitioned.
433
Geometry Orientation
The orientation of surface and curve geometry is the direction of the normal and tangent vectors respectively.
Each surface has a forward (or top) side. The evaluation of the surface normal at any point on the surface will return a
vector at that point, orthogonal to the surface and directed towards the forward side of the surface. The mesh faces
generated on each surface will have the same normal direction as their owning surface.
Each curve has a forward direction and a corresponding start and end vertex. The direction of the curve is from start to
end vertex. The evaluation of the tangent vector of the curve at any point along the curve will result in a vector that is both
tangent to the curve and pointing in the forward direction of the curve (towards the end vertex along the path of the curve.)
The mesh edges created on each curve will be oriented in the same direction as their owning curve. The exported nodes
and edges of a curve mesh will be written in the order they occur along the path of the curve.
Higher-dimension geometry has uses lower-dimension geometry with an associated sense (forward or reversed) for each
lower-dimension entity. For example, a volume as a sense for each surface used to bound the volume. If the surface
normal points outside the volume, then the volume uses the surface with a forward sense. If the surface normal points into
the interior of the volume, the volume uses the surface with a reversed sense. Similarly a surface is bounded by a set of
curves forming a loop such that the direction of the loop and the sense of each curve results in a cycle that is counterclockwise around the surface normal.
Adjusting Orientation
By default, a surface is oriented so that its normal points OUT of the volume of which it is a part. For a merged surface (a
surface which belongs to more than one volume) or a free surface (a surface that belongs to no volume, also known as a
sheet body), the orientation of the surface is arbitrary. The orientation of a surface influences the orientation of any
elements created on that surface. All surface elements have the same orientation as the surface on which they are
created. The following commands are available to adjust the normal-direction for a surface:
Surface <id_range> Normal Opposite
Surface <id_range> Normal Volume <id>
The orientation of a surface can be flipped from its current orientation by using the "Opposite" keyword. The orientation of
a merged surface can be set to point OUT of a specific volume by specifying that volume in the "Volume" keyword.
Occasionally, volumes will be created "inside-out". The command:
Reverse {Body|Volume} <body_id_range>
will turn a give volume or body inside out. This should be equivalent to reversing the normals on all the surfaces. This
shouldn't be encountered very often, as it is a very rare condition.
The following commands are available to adjust the tangent direction of a curve:
Curve <id_range> Tangent Opposite
Curve <id_range> Tangent {Forward|Reverse} Surface <id>
Curve <id_range> Tangent {Start|End} Vertex <id>
The first command reverses the tangent direction of the curve. The second command sets the tangent direction such that
it is used by a specific surface with a specified sense. The third command sets the tangent direction of the curve such that
the curve starts or ends with the specified vertex. For the latter two forms of the command, the curve must be adjacent to
the specified surface or vertex.
The below command can be used to change the orientation of multiple curves at once. With the direction option, the curve
will be oriented along the specified direction. With the location option, the vertex closest to the give location becomes the
start vert in the oriented curve. The curve orientation can be reversed using the opposite argument. Also, a vertex id can
be specified to make it the start vertex in the oriented curve.
435
Trelis 15.0 User Documentation
Curve <id_range> Orient Sense {direction (options)|location (options)|vertex <id_range>} [Opposite]
The above command is useful in changing the orientation of multiple curves at once using various options described. This
becomes helpful, e.g., when bias is applied on multiple curves. By default, bias depends on the orientation of the curve,
i.e., bias begins at start vertex.
436
Basic Group Operations
Geometry Groups
To create or add to a group
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Group.
Click on the Manage Groups action button.
Select Create/Add from the drop-down menu.
Enter in the desired name for the Group Name/ID.
Enter in the appropriate settings.
Click Apply.
The command syntax to create or modify a group is:
Group ["name" | <id>] Add <list of topology entities>
For example, the command,
group "exterior" add surface 1 to 2, curve 3 to 5
will create the group named Exterior consisting of the listed topological entities. Any of the commands that can be applied
to the "regular" topological entities can also be applied to groups. For example, mesh Exterior , list Exterior , or draw
Exterior .
Elements may specified by name as well. For example, the command
group 'interior' add surface name 'bill' 'john' 'fred'
will add the surfaces named 'bill' 'john' and 'fred' to the group 'interior'. A topological entity can be removed from a group
using the command:
Group ["name" | <id>] Remove <entity list>
The Xor operation can also be performed on entities in group. Xor means if an entity is already in the group, the command
will delete this entity from the group. If it is not in the group, the entity is then added to the group.
Group ["name" | <id>] Xor <entity list>
The Equals operation assigns the group to be exactly the same as the list given. All other existing members of the group
will be removed.
Group ["name" | <id>] Equals <entity list>
Modifying groups by comparing common entities
The Common_To operation looks for geometry entities that are related to the input elements, either as parents or children.
For example, specifying all curves common to two surfaces will give all of the curves that are attached to both of the
specified surfaces. The elements must be specified by name (specifying by id will not work), and the name must be
enclosed in single quotation marks. This option works for all of the group operators given above. The command syntax is:
Group ["name" | <id>] {Add|Equals|Remove|Xor} <entity_type> Common_to <entity_type> Name
'pattern' ['pattern'...]
The following is an example of the common_to operator.
437
Trelis 15.0 User Documentation
bri x 10
curve 2 name 'joe'
curve 3 name 'alf'
group 'mygroup' add surf common_to curve name 'joe' 'alf'
Mesh Groups
Groups may also contain mesh entities. The commands for adding and removing mesh entities are analogous to those for
geometric entities.
To create or add to a mesh group
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Group.
Click on the Manage Groups action button.
Select Create/Add from the drop-down menu.
Enter in the desired name for the Group Name/ID.
Enter in the appropriate settings.
Click Apply.
Group ["name" | <id>] Add {Hex|Face|Edge|Node <id_list>}
Group ["name" | <id>] Remove {Hex|Face|Edge|Node <id_list>}
Group ["name" | <id>] Xor {Hex|Face|Edge|Node <id_list>}
Deleting Groups
To delete a group
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Geometry and then Group.
Click on the Manage Groups action button.
Select Delete/Remove from the drop-down menu.
Select a group to delete.
Select delete and/or any other options from this menu.
Click Apply.
Delete Group <id range> [Propagate]
The option propagate will delete the group specified and all of its contained groups recursively.
Cleaning Out Groups
You can remove all of the entities in a group via the cleanout command:
Group <group_id_range> Cleanout [Geometry|Mesh] [Propagate]
By default all entities will be removed - optionally you can cleanout just geometry or mesh entities. As in delete, the
propagate option will cleanout the group specified and all of its contained groups recursively.
438
Groups in Graphics
In the GUI version of Trelis, groups may be picked with the mouse.
When displaying a group containing hexes, only the outside skin of the hexes will be displayed.
439
Propagated Hex Groups
•
•
Starting on a Surface
Starting on a Face
Propagated hex groups are a way of grouping hexes from a hex mesh using sweep-type criteria. For example, creating a
group containing all hexes between two specified mesh faces.
Note: the first examples below are based on first executing these commands:
brick width 10
volume 1 size 1
mesh volume 1
Propagated Hex Group Starting on a Surface
Starting on a surface can end at a surface or can end after the number of times the user specifies.
•
•
•
•
•
•
Ending at a Surface
Number of Times
Ending at a Surface with Multiple
Number of Times with Multiple
Ending at a Surface with Direction
Number of Times with Direction
Ending at a Surface
Group ['name' | <id>] Add Hex Propagate Surface <id> Target Surface <id>
Example
group 2 add hex propagate surface 1 target surface
Result: Group 2 will be created containing 1000 hexes
Number of Times
Group ['name' | <id>] Add Hex Propagate Surface <id> Times <number>
Example
group 2 add hex propagate surface 1 times 4
Result: Group 2 will be created containing 400 hexes
Both methods, ending at surface or number of times, can be used with the "multiple" option which will create several
groups depending upon the multiple number specified.
441
Trelis 15.0 User Documentation
Ending at a Surface with Multiple
Group ['name' | <id>] Add Hex Propagate Surface <id> Target Surface <id> Multiple <number>
Example
group 2 add hex propagate surface 1 target surface 2 multiple 2
Result: Five groups will be created and stored with their respective ids of multiple 2, these groups will be stored in the
parent group, Group 3, and Group 3 will be stored in the grand parent group, Group 2.
Number of Times with Multiple
Group ['name' | <id>] Add Hex Propagate Surface <id> Times <number> Multiple <number>
Example
group 2 add hex propagate surface 1 times 10 multiple 5
Result: Two groups will be created and stored with their respective ids of multiple 5, these two groups will be stored in the
parent group, Group 3, and Group 3 will be stored in the grand parent group, Group 2.
If number of times is specified and the direction is ambiguous, the surface direction or the node direction can be specified
to direct the propagation. If the end surface is specified, only a node direction can be specified to direct the propagation.
When specifying the node direction, the node has to be picked such that when the hexes are propagated, the picked node
lies in these propagated hexes. If that node is never reached while propagating, the direction is not found and zero hexes
will be included in the specified group.
Note: for the examples below, the result can be seen by executing these commands:
brick x 10
vol 1 size 1
brick width 10
body 2 move 10
volume all size 1
merge all
mesh volume all
Ending at Surface with Direction
Group ['name' | <id>] Add Hex Propagate Surface <id> Times <number> Direction Node <id>
Example
group 2 add hex propagate surface 6 target surface 12 direction node 1530
Result: Group 2 will be created containing 400 hexes
Note: The direction command and the multiple command can be combined (i.e. group 2 add propagate surface 6 times 4
multiple 2 direction node 1530)
442
Propagated Hex Groups
Number of Times with Direction
Group ['name' | <id>] Add Hex Propagate Surface <id> Times <number> Direction [surface <id> |
node <id>]
Example
group 2 add hex propagate surface 6 times 4 direction surface 4
group 2 add hex propagate surface 6 times 4 direction node 1530
Result: group 2 will be created containing 400 hexes
Propagated Hex Group Starting on a Face
When starting on a face, the propagation method can end at a surface, end at a face or can end after the number of times
the user specifies:
•
•
•
•
•
•
•
•
•
Ending at a Surface
Ending at a Face
Number of Times
Ending at a Surface with Multiple
Ending at a Face with Multiple
Number of Times with Multiple
Ending at a Face with Direction
Ending at a Surface with Direction
Number of Times with Direction
Ending at a Surface
Group ['name' | <id>] Add Hex Propagate [Source] Face <id range> Target Surface <id>
Example
group 2 add hex propagate face 1 11 21 target surface 2
Result: Group 2 will be created containing 30 propagated hexes (10 layers of 3 hexes)
Ending at a Face
Group ['name' | <id>] Add Hex Propagate [Source] Face <id> Target Face <id>
Example
group 2 add hex propagate face 1 target face 1721
Result: Group 2 will be created containing 5 propagated hexes (5 layers of 1 hex)
Note: Ending at a face requires starting at one face at one time, but ending at surface allows multiple start faces
443
Trelis 15.0 User Documentation
Number of Times
Group ['name' | <id>] Add Hex Propagate [Source] Face <id range> Times <number>
Example
group 2 add hex propagate face 2 times 4
Result: Group 2 will be created containing 4 propagated hexes (4 layers of 1 hex)
All of these methods, ending at surface, end at a face or number of times, can be used with the "multiple" option which will
create a grandparent (top-level), parent (mid-level, contained within the grandparent) and child (bottom level, contained
within the parent) groups. The child groups will contain each hex layer (specified number of layers per child group), all
organized into a single parent group, which is organized underneath the group ID given to the command. Subsequent
propagation commands could then be executed adding to the grandparent group, but creating a new parent and child
groups. This way multiple propagation "sets" can be stored in one grandparent group, if desired.
Ending at a Surface with Multiple
Group ['name' | <id>] Add Hex Propagate [Source] Face <id> Target Surface <id> Multiple <number>
Example
group 2 add hex propagate face 1 target surface 2 multiple 1
Result: Ten groups will be created and stored with their respective ids, one for each layer of hexes. These groups will be
stored in the parent group, Group 3, and Group 3 will be stored in the grand parent group, Group 2. A subsequent
propagation command could be executed adding to group 2 (the grandparent), which would create a single group
contained in group 2 (the parent), containing the hex layer groups (the children).
Ending at a Face with Multiple
Group ['name' | <id>] Add Hex Propagate [Source] Face <id> Target Surface <id> Multiple <number>
Example
group 2 add hex propagate face 1 target face 1721 multiple 1
Result: 5 groups will be created and stored with their respective ids, one for each layer of hexes. These groups will be
stored in the parent group, Group 3, and Group 3 will be stored in the grand parent group, Group 2. A subsequent
propagation command could be executed adding to group 2 (the grandparent), which would create a single group
contained in group 2 (the parent), containing the hex layer groups (the children).
Number of Times with Multiple
Group ['name' | <id>] Add Hex Propagate [Source] Face <id> Times <number> Multiple <number>
Example
444
Propagated Hex Groups
group 2 add hex propagate face 1 times 10 multiple
Result: Two groups will be created and stored with their respective ids, these two groups will be stored in the parent
group, Group 3, and Group 3 will be stored in the grand parent group, Group 2.
If the end surface or end face is ambiguous, a node direction can be specified to direct the propagation. When specify the
node direction, the node has to be picked such that when the hexes are propagated, the picked node lies in these
propagated hexes. If that node is never reached while propagating, the direction is not found and zero hexes will be
included in the specified group.
Ending at Face with Direction
Group ['name' | <id>] Add Hex Propagate [source] Face <id> Target Face <id> Direction Node <id>
Example
group 2 add hex propagate face 1721 target face 1 direction node334
Result: group 2 will be created containing 6 hexes
Ending at Surface with Direction
Group ['name' | <id>] Add Hex Propagate [Source] Face <id range> Target Surface <id> Direction
Node <id>
Example
group 2 add hex propagate face 1 target surface 2 direction node 334
Result: group 2 will be created containing 10 hexes
Note: The direction command and the multiple command can be used together (i.e. group 2 add propagate face 1721 end
face 1 multiple 2 direction node 334)
If number of times is specified and the direction is ambiguous, a surface direction or a node direction can be specified to
direct the propagation. The node direction has the same condition as when ending at a surface or face and that is it must
lie in the propagated hexes.
Number of Times with Direction
Group ['name' | <id>] Add Hex Propagate [Source] Face <id> Times <number>Direction [surface <id>
| node <id>]
Example
group 2 add hex propagate face 110 times 4 direction surface 2
group 2 add hex propagate face 1 times 4 direction node 269
445
Trelis 15.0 User Documentation
Result: group 2 will be created contained 4 hexes
Note: The direction command and the multiple command can be used together. (i.e. group 2 add propagate face 1721
times 4 multiple 2 direction surface 1)
Naming Convention for Propagated Hex Groups
A special naming convention can be used for the propagated hex groups, best described by an example.
The following command will create a hierarchy of logically named groups, as follows.
group 'W1P1T1' add propagate surf 1 end surf 2 multiple 1
The hierarchy looks like this:
W1
W1P1
W1P1T1
W1P1T2
W1P1T3
...
W1P1T10
Where W1P1 is contained within W1, and W1P1T1, W1P1T2, etc.. are contained within W1P1.
The software simply looks for numerical numbers in the group name and parses out the correct grandparent, parent and
child names from the substrings. There must be exactly 3 substrings in the group name, each ending with an integer for
the command to work properly.
A subsequent command:
group 'W1P2T1' add propagate surf 3 end surf 5 multiple 1
will add a parent group to W1, called W1P2, and the subsequent child groups:
W1
W1P1
W1P1T1
W1P1T2
W1P1T3
...
W1P1T10
W1P2
W1P2T1
W1P2T2
446
Propagated Hex Groups
W1P2T3
...
W1P2T10
447
Seeded Mesh Groups
It is also possible to automatically group surface mesh elements based on feature angles. Given a seed element, the
algorithm will loop over all adjacent elements and create groups of elements whose surface normals are similar, or which
fall within a certain radius. The command syntax is:
Group {<'name'>|<id>} {Add|Equals|Remove|Xor} Seed <mesh_entities> {Feature_angle <angle>
[Divergence]|Depth <number>}
The seed element may be a quad, tri, or node element. There are two methods of angle comparison for this command.
The feature angle option will compare angles of the each element to its adjacent elements by comparing surface normals.
In the case of nodes, the seed node surface normal will be the average of the adjacent faces or tris. Nodes will be added
if their attached faces meet the angle requirements. The divergence option will compare angles to the original seed
element's surface normal. The depth option will add elements within a certain radius.
The following figures illustrate the use of the seed method to create mesh groups using the feature angle and divergence
methods.
Trelis> group 'mygroup1' add seed face 269 feature_angle 45
449
Trelis 15.0 User Documentation
Trelis> group 'mygroup2' add seed face 269 feature_angle 45 divergence
The seed method of creating groups is particularly useful for creating groups on free meshes for the purpose of assigning
nodesets and sidesets.
The GUI command panel for this command is found by selecting
"Mode-Meshing", "Entity-Group", "Action-Manage Groups", then "Create with Seed." The command panel is shown below:
450
Seeded Mesh Groups
451
Quality Groups
Groups can also be formed from the hexes or faces obtained from the quality command. Each group formed using quality
can be drawn with its associated quality characteristics {i.e. jacobian low .2 high .3} automatically.
Group {<'name'>|id} {Add|Equals|Remove|Xor} Quality { Hex | Tet | Face | Tri | Volume | Surface |
Group } <id_range> { quality metric name (default is SHAPE) } [ High <value> ] [ Low <value> ] [ Top
<number> ] [ Bottom <number>]
The following example illustrates the use of quality groups:
group 2 add quality volume 1 jacobian
In this case, if the meshed brick from the section Propagated Hex Groups is used, Group 2 will be created and it will
contain 1000 hexes with quality characteristics.
The quality metric names can be found in the Quality Assessment section of the documentation.
453
Entity Names
By default, geometric entities in Trelis are referenced using an entity type (e.g. Surface, Volume) and an id, for example
"draw surface 1". However, geometric entities can also be assigned names, to simplify working with specific
entities. Once a name is assigned to an entity, that name can be used in any Trelis command in place of the entity type
and number. For example, if surface 1 were named 'mysurf1', the command above would be equivalent to "draw
mysurf1". Also, since entity names are saved with the geometry, this also provides a means for persistent identifiers for
geometric entities. Names can be added or removed using the following commands.
{Group|Body|Volume|Surface|Curve|Vertex} {Name | Rename} {`<entity_name>'| Default}
{Group|Body|Volume|Surface|Curve|Vertex} Remove Name {`<entity_name>'| All | Default}
The name of each topological entity appears in the output of the List command. In addition, topological entities can be
labeled with their names (see label command). A list of all names currently assigned and their corresponding entity type
and id (optionally filtered by entity type) can be obtained with the command
List Names [{Group|Body|Volume|Surface|Curve|Vertex|All}]
Notes:
•
•
In a merge operation, the surviving entity is given the name(s) of the deleted entity.
A geometric entity may have multiple names, but a particular name may only refer to a single entity.
Valid and Invalid Names
Although any string may be used as an entity name, only valid names may be used directly in commands. A name is valid
if it begins with a letter or underscore ("_"), followed by any combination of zero or more letters, digits, or the characters
".", "_", or "@". If an attempt is made to assign an invalid name to an entity, Trelis will generate a valid version of the
invalid name by replacing invalid characters with an underscore. Then both the valid and invalid versions of the name are
assigned to the entity. For example, assigning the name "123#" to a volume will result in the volume having two names,
"123#" and "_23_". The valid name can be used directly in commands (mesh _23_), while the invalid name can only be
referenced using a longer, less direct syntax (mesh volume with name "123#").
Reconciling Duplicate Names
When an attempt is made to assign the same name to two different entities, a suffix is added to the name of the second
entity to make it unique. The suffix consists of the "@" character followed by one or more letters or numbers. For example,
the following commands will result in volumes 1 to 3 having the names "hinge", "[email protected]", and "[email protected]", respectively:
volume 1 name "hinge"
volume 2 name "hinge"
volume 3 name "hinge"
To prevent this automatic "fixing" of names, the Fix Duplicate Names flag may be switched to off. If the user attempts to
assign a duplicate name while the flag is set to off, the name will remain unchanged.
Set Fix Duplicate Names [ON|Off]
Automatic Name Creation
Trelis provides an option for automatically assigning names to entities upon entity creation. This option is controlled with
the command:
Set Default Names {On|OFF}
455
Trelis 15.0 User Documentation
When this option is on, entities are assigned default names consisting of a geometry type concatenated with the entity id,
for example 'cur1', 'surf26', or 'vol62'.
Automatic Name Propagation
Trelis automatically propagates names through webcuts. If an entity that has been assigned the name "Gear" is split
through webcuts, the resulting bodies are named "Gear" and "[email protected]". Try the following example.
br x 10
volume 1 name "Cube"
webcut volume 1 xplane
webcut volume 1 2 yplane
webcut volume 1 2 3 4 zplane
label volume name
Figure 1. Name Propagation through Webcuts
You can operate on these propagated names using wildcards such as:
mesh volume with name 'Cube*'
block 1 volume with name 'Cube*'
Naming Merged Entities
When entities that have the same base name, such as "platform" and "[email protected]", are merged, the resulting entities is
assigned both names. The set merge base names on command tells Trelis that in this situation, it should merge the
names too. The command syntax is:
Set Merge Base Names [On|OFF]
For example:
456
Entity Names
brick x 10
vol 1 copy move 10
surf 6 name 'platform'
surf 10 name 'platform'
Surface 10 actually is named [email protected], since we don't want duplicate names
merge all
list surf 6
You see that surface 6 has both 'platform' and '[email protected]' as names. Now, for the contrasting example
brick x 10
vol 1 copy move 10
surf 6 name 'platform'
surf 10 name 'platform'
set merge base names on
merge all
list surf 6
You see that surface 6 has only 'platform' as its name.
457
Entity IDs
Topological entities (including groups) are assigned integer identification numbers or ids in Trelis in ascending order,
starting with 1 (one). Each new entity created within Trelis receives a unique id within the topological entity type. This id
can be used for specifying the entity in Trelis commands, for example "draw volume 3".
There is a separate id space for each type of topological entity. For example, all mesh nodes are given ids from 1 to n,
where n is an integer greater than or equal to the number of nodes in the model. Likewise, all hexahedra are given ids
from 1 to m, where m is an integer greater than or equal to the number of hexahedra in the model.
Element Ids
Each mesh entity (hex, tet, face, tri, edge, node, etc.) may also have a Global Element ID from an id space which is used
for all mesh entities. A mesh entity is only assigned a Global Element ID if it is in a block, and is the global id that will be
assigned to the element during Exodus export. The Global Element ID provides a single id space across all the different
element types.
Gaps in ID space
After working with a model for some time, various operations will cause gaps to be left in the numbering of the geometric
& mesh entities. The compress ids command can be used to eliminate these gaps:
Compress [Ids] [All] [Group|Body|Volume|Surface|Curve|Vertex|Element|Hex|Tet|Face|Edge|Node]
[Retainmax] [Sort]
Typing compress with no options or compress all will compress the ids of all entities; otherwise, the entity type for which
ids should be compressed can be specified. The retainmax argument will retain the maximum id for each entity type, so
that entities created subsequent to this command will receive ids greater than that value. If the sort qualifier is included,
the new id of each entity will be determined by its size and location. Small entities are given a lower id than large entities.
Entities that are the same size are sorted by their location, with lower x, y, and z coordinates leading to a lower id. If two
entities are found to have the same size and location, they are sorted according to their previous ids. This option can be
used to restore ids in translated models in a manner which leads to more persistence than purely random id assignment.
Renumbering IDs
The renumber command can be used to change the id numbers assigned to meshed entities.
Renumber {Node|Edge|Tri|Face|Hex|Tet|Wedge} <id_range> Start_id <id> [Uniqueids]
Any valid range specification can be used to specify the source ids. There is no requirement that the ids being
renumbered are consecutively numbered. The new id numbers will be consecutive beginning at the specified start id. For
the command to be successful there can be no existing ids within the effective range of the start id. If the resultant
destination range is not free of id numbers, the command will fail with an appropriate error.
Using the uniqueids keyword will result in the elements to be renumbered such that no element shares the same ID.
For convenience, all elements and nodes in a block can be renumbered with a single command:
Renumber block <id_range> [node_start_id <id>] [elem_start_id <id>] [localids]
By default, the Global Element ID is renumbered with the renumber block command. If localids is specified, the hex, tet,
face, tri, or edge id is renumbered instead.
Volume ID
The volume id command is used to renumber a single volume.
459
Trelis 15.0 User Documentation
Volume <old_id> Id <new_id>
This command replaces the volume's old_id with the new_id if no other is using the new_id number. Entity renaming only
works for volumes; it does not work for nodes, curves or surfaces.
460
Attribute Behavior
In this context, attributes are defined as data associated directly with a particular geometry entity. In Trelis' implementation
of attributes, these data can occupy one of three "states" at any given time: they can be stored in data fields on Trelis'
geometry entities; they can be stored in an intermediate representation, using Trelis' attribute objects; or they can exist
only on the ACIS objects. When they are stored on ACIS objects, those attributes are written to and read from disk files
with the geometry. This mechanism allows CUBIT-specific information to be stored and retrieved with the geometry data.
By default, attribute data is not stored with geometry. To enable the use of attributes, use the commands described in the
following sections.
461
Attribute Types
The attribute types currently implemented in Trelis are shown below.
Attribute Types
Description
Color
Entity Color
Composite vg
Used to restore composite virtual topology
Genesis entity
Membership in boundary conditions (block, sideset, nodeset)
Id
Entity Id
Mesh container
Handle to mesh defined for the owner
Mesh scheme
Meshing scheme (e.g. paving, sweeping, etc.)
Name
Entity name
Partition vg
Used to restore partition virtual topology
Smooth scheme
Smoothing scheme (e.g. Laplacian, Condition Number)
Unique Id
Unique entity id, used to cross-reference other entities
Vertex type
Used to define mesh topology at vertex for mapping/submapping
Virtual vg
Used to store virtual geometry entity(ies) defined on an entity
463
Attribute Commands
Most non-CUBIT-developer uses of attributes will be to use all or none of the attributes. Therefore, the most common
command to enable and disable the use of attributes is:
Set Attribute {On|Off}
When this option is on, all defined attributes will be saved with the geometry when the user enters the Export Acis
command.
When a geometry is imported into Trelis, any attributes defined on that geometry and recognized as Trelis attributes are
imported and put into an intermediate representation (that is, this information is not assigned directly to the geometry
entities). To find out which attributes are defined on a given set of entities, use the following command:
List [<entity_list>] Attributes [Type <attribute type>] [All] [Print]
If no entities are entered, attribute information for all the geometric entities defined in Trelis is printed.
The Type option can be used to list information about a specific attribute type; values for are the same as those in the
previous table.
If the All option is entered, information about all attribute types will be printed, even if there are none of those attributes
defined for the specified entities.
If the Print option is entered, the information stored in each attribute will be printed; this command is usually used only by
Trelis developers.
Control By Attribute Type or Geometric Entity
Attributes can be enabled or disabled by attribute type, to allow the use of only user-specified attribute types. To turn on
or off specific attributes, use the command:
Set Attribute <attribute type> {On|Off}
where <attribute type> is one of the types shown in the previous table.
Attributes can also be controlled to automatically write (update) and read (actuate) to/from solid model files automatically,
using the command:
Set Attribute <attribute_type> Auto {Actuate|Update} {On|Off}
Finally, attributes can be manually written to and read from the geometric entities, and removed from Trelis entities, using
the command
{geom_list} Attribute {All|Attribute_type} {Actuate|Remove|Update|Read|Write}
where geom_list is a list of geometry entities. This command is recommended only for developers' use.
465
Using Trelis Attributes
A typical scenario for using Trelis attributes would be as follows.
Construct geometry, merge, assign intervals, groups, etc. (i.e. normal Trelis session)
Enable automatic use of attributes using the command:
Set Attribute On
Export ACIS file (see Export Acis command).
Subsequent runs:
Enable automatic reading and actuating of attributes:
set attribute on
Import ACIS file (see Import Acis command)
Used in this manner, geometry attributes allow the user to store some data directly with the geometry, and have that data
be assigned to the corresponding Trelis objects without entering any additional commands.
467
Entity Measurement
To output various properties of entities, the following Measure command options are available.
•
•
•
•
Measure Between
Measure Small
Measure Angle
Measure Void
Measure Between
Measure Between { { Vertex|Curve|Surface |Volume|Node} <id1> | Location <options> | Plane
<options> | Axis <options> } With { {Vertex|Curve|Surface|Volume|Node} <id2> | Location
<options> | Plane <options> | Axis <options> }
Measure Between {Surface|Curve} <id1 > [Surface|Curve] <id2> [Node]
Measure Between {Vertex|Curve|Surface|Volume|Node|Edge|Face|Tri|Hex|Tet} <id1> With
{Vertex|Curve|Surface|Volume|Node|Edge|Face|Tri|Hex|Tet} <id2>
The Measure Between command outputs the distance from one entity, location, plane, or axis to the next. The two
entities in the command should be separated by the word "with". The result will always be the minimum distance between
entities. For example, measuring between two spheres will output the minimum distance between them, not the distance
between centroids. The example shown below will output the minimum distance between vertex 1 and surface 2.
measure between vertex 1 surface 2
The second form of the command is just for surfaces or curves and contains the Node argument. This argument attempts
to measure between corresponding nodes on a pair of surfaces or curves. The command tries to determine a one-to-one
mapping of nodes between the pair. It returns the greatest distance between any two nodal pairs, least distance between
any two nodal pairs, and average distance between all of the nodal pairs. The mapping algorithm works best on surfaces
if they are parallel.
The last form of the command measures between any geometry or mesh entities. The measurement to the mesh entities
is to their center (i.e. the averaged vector location of all of the nodes belonging to the mesh entity).
Measure Small
Measure Small {Length|Area|Volume|All} {Body|Surface} <id_list>
The Measure Small command locates all of the lengths, areas, or volumes smaller than the Measure Small Tolerance
setting. Entities meeting the small tolerance criteria are listed in the output window and typically highlighted in the view
port. The following two commands set the small tolerance to 0.1 and output all of the curves within body 1 with lengths at
or below the small tolerance.
set measure small tolerance 0.1
measure small length body 1
Measure Angle
Measure Angle { Direction <options> | Plane <options> | Axis <options> } With { Direction
<options> | Plane <options> | Axis <options> }
469
Trelis 15.0 User Documentation
The Measure Angle command displays the interior angle between the two entered entities. When a plane and a direction
are specified, the angle between the direction vector and its projection into the plane is displayed. The measured angle
represents the distance between the orientations of entities, and does not require the entities to intersect. Angles of model
features can be measured by using the various options associated with the Direction, Planes, and Axis commands.
measure angle direction tangent curve 1 with plane surf 1
Measure Void
Measure Void [Face | Tri] <range>[No_Checks]
The Measure Void command takes a closed list of quadrilaterals or triangles and calculates the volume of the internal
region defined by the given list of elements. This command assumes that the normals on the given elements are
consistently ordered. If the normals are pointing away from the interior of the void, the reported volume may be negative.
This command will check to ensure that the given elements do form a closed, manifold shell, otherwise an error is
reported. Common uses will be to calculate the volume of an internal void for use in determining bulk element properties
for a thermal analysis.
Rather than issuing an error, the no_check option does not check for closure of the faces and will compute a void volume
regardless of their watertightness. This is useful if faces are all touching, but may not have complete topological closure.
470
Exporting ACIS Files
Geometry can be exported from within Trelis to the ACIS "sat" (ASCII) and "sab" (binary) formats. These formats can be
used to exchange geometry between ACIS-compliant applications.
To export ACIS files:
1.
2.
3.
4.
5.
6.
7.
Select File and then Export.
Select the location for the file to be saved.
Enter a File Name.
Select ACIS from the Save as type drop-down menu.
Click Save. A new window will appear.
Optionally specify any appropriate settings from this window.
Click Finish.
Export Acis [Debug] 'filename' [<geometry_entity_list>] [Binary|Ascii] [Current] [Overwrite]
The filename should be enclosed in single or double quotes. By convention, binary and ASCII ACIS files use the .sab and
.sat filename extensions, respectively. If a geometry entity list is not specified, the entire ACIS model is exported. A
geometry entity list is specified in the same format used for other Trelis commands (See Entity Specification). Note that
the model is saved as manifold geometry, and will have that representation when imported back into Trelis (See NonManifold Topology and Geometry Merging.)
When exporting, the filename extension will determine the default file type, either ASCII or binary. A .sat extension will
default to ASCII; a .sab extension will default to binary. If you use a different file extension you can specify the type with
the [binary|ascii] option (with an unsupported extension exporting will default to ASCII but importing requires the type to
be specified). Binary files can be significantly faster but are not guaranteed to be upward compatible nor cross-platform
compatible (although testing has determined compatibility between NT and HP/UX).
In the GUI version, the current option will set the default filename for autosave (cntrl-S or File->Save (auto inc)) to the
imported filename. Also, the filename is then set in the window titlebar.
When exporting with the "file overwrite" option on, the software will check to see if the file exists already, and if it does,
exporting will fail in the command line version or ask to confirm the overwrite in the GUI version of Trelis. The overwrite
option will override this option and overwrite the file. The "file overwrite" option defaults to ON in the GUI version, OFF in
the command line version.
When exporting, you can set the version of the Acis geometry. This allows backwards compatibility to previous versions of
Trelis or other Acis-based applications. The command to change the Acis geometry engine version is:
Set Geometry Version [version_number]
where version_number can be one of the following:106, 107, 201, 300, 301, 401, 402, 403, 500, 501, 502, 503, 600,
601, 602, 603, 700, 701, 702, 703, 704, 705, 800, 1007, 1100, 1200, 1300, 1400, 1500, 1600, 1700, 1800, 1900, 2100,
2200. Note that you cannot set a version number that is higher than that of your current engine. For example, Trelis 6.0
was based on Acis 6.2, so you cannot set a geometry version of 700.
See also Importing ACIS Models.
471
Exporting STEP Files
Trelis can export geometry to the STEP format, an emerging standard for storing geometry and other information. The
STEP AP203 and STEP AP214 standards are supported. It is recommended to use AP214 for exchange of geometry
information with Trelis.
To export STEP files:
1.
2.
3.
4.
5.
6.
7.
Select File and then Export.
Select the location for the file to be saved.
Enter a File Name.
Select STEP from the Save as type drop-down menu.
Click Save. A new window will appear.
Optionally specify any appropriate settings from this window.
Click Finish.
Export Step 'filename' [<geometry_entity_list>] [Logfile ['filename'] [Display]] [Overwrite]
As with ACIS file export, you can specify which individual entities to export. If unspecified, all ACIS entities are exported.
The logfile option is used to save information regarding the conversion to STEP format. This information saved to a file
with the name specified by the user, or named 'step_export.log' by default. When running the GUI version of Trelis, the
logfile can be displayed in a dialog window by using the display option.
The overwrite option works the same as with ACIS file export.
See Importing STEP Files for information on setting up the STEP import and export functionality.
Note that the STEP import and export functionality might not be available on all 64-bit platforms.
473
Exporting IGES Files
The ACIS IGES translator provides bi-directional functionality for data translation between ACIS and the IGES (Initial
Graphic Exchange Standard) format.
To export IGES files:
1.
2.
3.
4.
5.
6.
7.
Select File and then Export.
Select the location for the file to be saved.
Enter a File Name.
Select IGES from the Save as type drop-down menu.
Click Save. A new window will appear.
Optionally specify any appropriate settings from this window.
Click Finish.
Export Iges 'filename' [<geometry_entity_list>] [Solid] [Logfile ['filename'] [Display]] [Overwrite]
As with ACIS file export, you can specify which individual entities to export. If unspecified, all ACIS entities are exported.
The logfile option is used to save information regarding the conversion to IGES format. This information saved to a file
with the name specified by the user, or named 'iges_export.log' by default. When running the GUI version of Trelis, the
logfile can be displayed in a dialog window by using the display option.
The solid option allows solid volumes to be exported as Manifold Solid B-Rep Objects (MSBO). Without this option, the
iges file is simply a collection of stand-alone surfaces.
The overwrite option works the same as with ACIS file export.
See Importing IGES Files for information on setting up the IGES import and export functionality.
Note that the IGES import and export functionality might not be available on all 64-bit platforms.
475
Exporting Facet Files
Facet files may be exported directly, or by converting from an ACIS representation.
To export a facet files:
1.
2.
3.
4.
5.
6.
7.
Select File and then Export.
Select the location for the file to be saved.
Enter a File Name.
Select Facets from the Save as type drop-down menu.
Click Save. A new window will appear.
Optionally select any appropriate settings from this window.
Click Finish.
Export Facets 'filename' <entity_list> [Overwrite]
The overwrite function allows you to overwrite an existing facet file.
477
Geometry Deletion
To delete geometry from the model
1.
2.
3.
4.
5.
On the Command Panel, click on Geometry.
Click on Volume, Surface, Curve or Vertex.
Select the Delete action button.
Enter in the appropriate value to be delete. This can also be done using the Pick Widget function.
Click Apply.
Delete [Body | Surface | Curve | Vertex] <id_range>
Any type of Body can be deleted, whether it is based on solid model geometry or another representation. Other entities
(Surface, Curve, Vertex) can be deleted when they are "free", i.e. when they are not contained in an entity of higher
topological order (Body, Surface or Curve, respectively); this type of geometry is often created from the lowest order
topology up.
479
Meshing the Geometry
After assigning interval or sizing attributes to a geometric entity and a meshing scheme is applied, the geometry is ready
to be meshed.
To mesh a geometric entity
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh.
Click onVolume, Surface, Curve or Vertex.
Click on the Mesh action button.
Enter in the appropriate value for Select Volumes, Select Surfaces, Select Curves or Vertex ID(s). This can
also be done using the Pick Widget function.
Enter in any other appropriate settings from this menu.
Click Mesh.
Mesh <entity> <id_range> [GLOBAL|Individual]
The <entity> to be meshed may be any one of the following:
Body
Volume
Surface
Curve
Vertex
The Global and Individual options affect how the constraints are gathered for interval matching. With the Global option,
the interval constraint equations are calculated from all entities in the entity list. The Individual option calculates the
interval constraint equations from each entity individually. The Global option is the default.
Default Scheme and Interval Selection
If either interval settings or schemes have not already been set on the entities being meshed, Trelis will do its best to
automatically set one or both of these attributes. See Auto Scheme Selection and Auto Specification of Intervals for a
description of how Trelis chooses these attributes. In cases where the automatic scheme selection algorithm fails to select
a scheme for the geometry, the meshing operation will fail. In this case explicit specification of the meshing scheme
and/or further geometry decomposition may be necessary.
Continuing Meshing After a Mesh Failure
Frequently when meshing large assemblies containing a number of volumes, the mesh command can be applied to a
group of volumes with the same mesh command. Typically, if a mesh failure is detected, the meshing operation will
continue to mesh the remaining volumes specified at the command line. The following command permits the user to
override this feature to discontinue meshing additional volumes and return to the command line immediately after a mesh
failure is detected:
Set Continue Meshing [ON|Off]
The default for this command is ON.
Turning this setting OFF is useful when meshing assemblies where a meshing failure of one volume would adversely
affect the meshing of adjoining volume(s). This occurs frequently when meshing a sweep group using the sweep scheme.
481
Interval Firmness
Before describing the methods used to set and change intervals, it is important that the user understand the concept of
interval firmness. An interval firmness value is assigned to a geometry curve along with an interval count or size; this
firmness is one of the following values:
hard: interval count is fixed and is not adjusted by interval size command or by interval matching
soft: current interval count is a goal and may be adjusted up or down slightly by interval matching or
changed by other interval size commands.
default: default firmness setting, used for detecting whether intervals have been set explicitly by the
user or by other tools
Interval firmness is used in several ways in Trelis. Each curve is assigned an interval firmness along with an interval count
or size. Commands and tools which change intervals also affect the interval firmness of the curves. Those same
commands and tools which change intervals can only do so if the curves being changed have a lower-precedence interval
firmness. The firmness settings are listed above in order of decreasing precedence. For example, some commands are
only able to change curves whose interval firmness is soft or default ; curves with hard firmness are not changed by these
commands.
More examples of interval setting commands and how they are affected by firmness are given in the following sections.
A curve's interval firmness can be set explicitly by the user, either for an individual curve or for all the curves contained in
a higher order entity, using the command:
{geom_list} Interval {Default | Soft | Hard}
All curves are initialized with an interval firmness of default , and any command that changes intervals (including interval
assignment) upgrades the firmness to at least soft .
Precedence
If a size is specified multiple times for a single entity, the following precedence is used:
•
•
The highest firmness command takes precedence.
Hard commands include "curve <id> interval <val>", and "{geometry_list} interval hard" will fix the size at the
current size.
Within a given firmness, the last-issued command takes precedence.
For example, if the user commands "surface 1 size 1" then "volume 1 size 2", and surface 1 is part of volume 1,
then surface 1 will have a size of 2.
483
Explicit Specification of Intervals
The density of mesh edges along curves is specified by setting the actual number of intervals or by specifying a desired
interval size. The number of intervals can be explicitly set curve by curve, or implicitly set by specifying the intervals on a
surface or volume containing that edge. For example, setting the intervals for a volume sets the intervals on all curves in
that volume.
To specify the number of intervals on a volume, surface or group
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh.
Click on Volume, Surface or Group.
Click on the Intervals action button.
Enter the appropriate value for Select Volumes, Select Surfaces or Select Groups. This can also be done
using the Pick Widget function.
Select Interval from the drop-down menu.
Enter in the appropriate value for Interval.
Click Apply and then Mesh.
To specify the number of intervals on a curve
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh and then Curve.
Click on the Mesh action button.
Enter the appropriate value for Select Curves. This can also be done using the Pick Widget function.
Select Equal from the drop-down menu.
Select Interval.
Enter in the appropriate value for Interval.
Click Apply Size and then Mesh.
{Curve|Surface|Volume|Body|Group} <range> Interval <intervals>
When setting interval counts for surfaces, volumes, bodies and groups, an interval's firmness of soft is assigned to the
owned curves. When setting the interval count for a curve, a firmness of hard is assigned.
The user can scale the current intervals with the following commands. Scaling is done on an entity by entity basis.
{Curve|Surface|Volume|Body|Group} <range> Interval Factor <factor>
485
Automatic Specification of Interval Size
In addition to specifying intervals explicitly based on a known count or size, Trelis is able to compute interval sizes
automatically based on characteristics of the model geometry.
To auto-size intervals on volumes and surfaces
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Mesh.
Click Volume or Surface.
Click on the Intervals action button.
Enter in the appropriate value for Select Volumes or Select Surfaces. This can also be done using the Pick
Widget function.
Select Auto from the drop-down menu.
Slide the icon on the Auto Factor menu to adjust the Interval Size.
Enter in any other appropriate settings from this menu.
Click Apply and then Mesh.
To auto-size intervals on curves
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh and then Curve.
Click on the Mesh action button.
Enter the appropriate value for Select Curves. This can also be done using the Pick Widget function.
Select Equal from the drop-down menu.
Select Auto Size.
Slide the icon on the Auto Factor menu to adjust the Interval Size.
Click Apply Size and then Mesh.
{geom_list} Size Auto [Factor <factor> ] [Individual] [Propagate]
Vertices are not valid in the geom_list for this command. Automatic interval size assignment works by examining the
geometric characteristics of the entities in the geom_list and assigning a heuristic size to the entities and their child
entities. The factor may be a floating point number between 1.0 and 10.0, where 1.0 represents a fine interval size and
10.0 represents a coarse size. Figure 1 shows an example of different auto size specification on a CAD model.
(a) auto size factor = 7.0
487
Trelis 15.0 User Documentation
(b) auto size factor = 5.0
(c) auto size factor = 1.0
The user may assign the interval size to be the arc length of the smallest curve contained in the specified entity or entities
using the following command:
{geom_list} Size Smallest Curve
Vertices are not allowed in the geom_list for this command. This command assigns a soft interval firmness.
Automatic Interval Size Specification
An automatic interval size with an auto size factor of 5 will automatically be computed and applied to any curve for which
the following is true:
1) Intervals have not been explicitly defined by the user for a curve or its owning entities.
2) An Interval size has not been explicitly defined by the user for a curve and it is not possible to determine an
interval size from its owning entities.
This automatic interval size is based upon all the geometry in the model. The automatic interval size specifications can be
overridden easily by specifying another auto size factor or an explicit interval size.
If an auto size factor of 5 is undesirable for most meshing operations, the default factor may be changed by using the
following command:
Set Auto Size Default <value>
488
Automatic Specification of Intervals
where value is a number from 1 to 10. This will be the default auto size factor used when either a factor has not been
specified on the size auto command or when an automatic interval size specification is used.
In previous versions of Trelis a default interval of 1 was assigned to all entities. If this behavior is still desired, the following
command may be used to enforce this condition:
Set Default Autosize [ON|off]
Maximum Spanning Angle on Arcs
On many CAD models, arcs or small holes require that a finer mesh be specified around these entities in order to maintain
reasonable mesh quality. To facilitate this, the user may specify the maximum angle an element edge may span on an
arc. To change or list the maximum arc span, use the following commands
Set Maximum Arc_Span <angle>
List Maximum Arc_Span
The angle parameter must be a positive value less than 360. The maximum arc span setting will only be used if there is
not already a user defined interval set on the arc, and if the interval setting produces mesh edges which exceed the
maximum spanning angle. Figure 2 shows the effect of three different maximum arc_span settings on a small hole using
the pave scheme.
Figure 2. Maximum arc_span settings of 90, 45 and 15 degrees respectively.
Default arc span setting: In addition to setting an automatic size factor, if there are otherwise no user-defined interval
sizes defined on an arc and no maximum arc_span has been set by the user when a tetrahedral mesh or triangle mesh
is defined, a maximum spanning angle of 60 degrees will be used. Removing the use of the arc_span setting can be
accomplished with the following:
Set Maximum Arc_Span Default
Note that once interval sizes have been defined when the entity has been meshed, it may be necessary to reset the
interval settings (reset {geom_list}) to use a new maximum arc span setting when remeshing.
489
Interval Matching
Each meshing scheme in Trelis imposes a set of constraints on the intervals assigned to the curves bounding the entity
being meshed. For example, meshing any surface with quadrilaterals requires that the surface be bounded by an even
number of mesh edges. This constrains the intervals on the bounding curves to sum to an even number. For a collection
of connected surfaces and volumes, these interval constraints must be resolved globally to ensure that each surface will
be meshable with the assigned scheme. The global solution technique implemented in Trelis is referred to as interval
matching.
When meshing a surface or volume, matching intervals is performed automatically. In some cases, interval matching
needs to be invoked manually, for example when meshing a collection of volumes, or a collection of surfaces not in a
common volume. Interval matching can also be called to check whether the assigned intervals and schemes are
compatible.
The command syntax for manually matching intervals is the following:
Match Intervals {Surface|Volume|Body|Group} <range>
Here the entity list can be any mixed collection of groups, bodies, volumes, surfaces and curves.
The interval matcher assigns intervals as close as possible to the user-specified intervals, while satisfying global interval
constraints. The goal is to minimize the relative change in pre-assigned intervals on all entities. Interval matching only
changes curves with interval firmness of soft or default .
Extra constraints can be added by the user to improve mesh quality locally; in particular, curves can be constrained to
have the same intervals using the command
Curve <range> Interval {Same|Different}
Specifying that curves have the "same" intervals stores them in a set. More curves may be added to an existing set, and
sets merged, by future commands. The current contents of the affected sets are printed after each command. A curve
may be removed from a set by specifying that its intervals are "different."
The interval assignment algorithm tries to find one good interval solution from among the possibly infinite set of solutions.
However, if many curves are hard-set or already meshed, there may be no solution. To improve the chances of finding a
solution, it is suggested that curves are soft-set whenever possible. Also, a solution might not exist due to the way the
local selections of corners and sides of mapped surfaces interact globally. If there is no solution, the following command
may help in determining the cause:
Match Intervals {Surface|Volume|Body|Group} <range> [Seed Curve <range>] [Assign Groups
[Only|Infeasible]] [Map|Pave]
Specifying Assign Groups will create groups that contain independent subproblems of the global problem. Specifying
Assign Groups Only will group independent subproblems, but the algorithm will not attempt to solve these subproblems.
Assign Groups Infeasible will put each independent subproblem with no solution into specially named groups. Often
poor corner choices and surface meshing schemes will be illuminated this way. If Map or Pave is specified, then only
subproblems involving mapping or paving constraints will be considered. If a Seed Curve is specified, then only those
subproblems containing that curve will be considered.
Advanced users may also wish to experiment with setting the following, which may change the interval solution slightly:
Set Match Intervals Rounding {on|off}
Set Match Intervals Fast {on|off}
Set Match Intervals Delta <interval_difference = 0.>
If set match intervals rounding is set to on, the intervals will be rounded to the nearest integer. If the setting is off, the
intervals will be rounded toward the user specified intervals.
491
Trelis 15.0 User Documentation
If set match intervals fast is set to off a single curve will be fixed per iteration. Note in rare cases this may produce
better meshes. If set match intervals fast is set to on multiple curves will be fixed per iteration.
Set match intervals delta allows the number of intervals assigned to a curve to be delta intervals away from optimal
unexpectedly. A larger value makes matching intervals faster, but the quality of the solution may be worse; Hint: try delta
= 1.0. Default is 0.0.
The user can also constrain the parity of intervals on curves:
{Curve|Surface|Volume} <range> Interval {Even | Odd}
If Even is specified, then during subsequent interval setting commands and during interval assignment, curves are forced
to have an even number of intervals. If the current number of intervals is odd, then it is increased by one to be even. If
Odd is specified then intervals may be either even or odd. Setting intervals to even is useful in problems where adjoining
faces are paved one by one without global interval assignment.
Rather than specifying a specific size or interval for a curve or surface, which may overconstrain the interval matcher, you
can specify an upper and lower bound that is acceptable. This would typically be used in a complex assembly where there
may be multiple intervals that may interact in order to get a compatible mapped/swept mesh through the assembly.
Surface <surface_id_range> {Interval|Size|Periodic Interval} {Lower|Upper} Bound {On|Off|<bound>}
492
Periodic Intervals
The number of intervals on a periodic surface, such as a cylinder, in the dimension that is not represented by a curve is
usually set implicitly by the surface size.
However, periodic intervals and firmness can be specified explicitly by the following commands:
Surface <range> Periodic Interval <intervals>
Surface <range> Periodic Interval {Default|Soft|Hard}
493
Relative Intervals
If the user needs fine control over mesh density, then for curvy or slanted sides of swept geometries, it is often useful to
treat curves as if they had a different length when setting interval sizes. For example, the user may wish to specify that a
slanting side curve and a straight side curve have the same "relative" length, despite their true length as shown in the
following figure. These are not interval matching constraints; interval matching may change intervals so that the userspecified ratio does not hold exactly.
The relative lengths of curves are set with the following command:
{geom_list} Relative Length <size>
The following command is used to assign intervals proportional to these lengths:
{geom_list} Relative Interval <base_interval>
For a curve with relative length x, setting a relative interval of y produces xy intervals, rounded to the nearest integer.
495
Mesh Interval Preview
It is sometimes useful to view the nodal locations/intervals on curves graphically before meshing (which can take
considerably more time). The command to do this is:
Preview Mesh {Body|Volume|Surface|Curve|Vertex} <id_range> [Hard]
To clear the display of the temporary nodes, simply issue a "display" command. The purpose of the hard option is that
only curves that have an interval firmness of hard will be previewed.
497
Bias, Dualbias
Applies to: Curves
Summary: Meshes a curve with node spacing biased toward one or both curve ends.
To use the bias scheme
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Curve.
Click on the Mesh action button.
Enter the values for Select Curves. This can also be done using the Pick Widget function.
Select Bias from the drop-down menu.
Select the desired option from the drop-down menu and enter in the appropriate settings.
Click on Apply Size and then Mesh.
Curve <range> Scheme Bias
Curve <range> Scheme Bias {Factor|First_Delta|Fraction} <double> [Start Vertex <range>] [preview]
Curve <range> Scheme Dualbias {Factor|First_Delta|Fraction} <double> [preview]
Curve <range> Scheme Bias Fine Size <double>
{Coarse Size <double> | Factor <double>} [Start Vertex <range>] [preview]
Curve <range> Scheme Dualbias Fine Size <double>
{Coarse Size <double> | Factor <double>} [preview]
Related Commands:
Curve <range> Reverse Bias
Set Maximum Interval <int>
See also Surface Sizing Function Type Bias
See also Curve Scheme Stretch
The main differences between scheme bias and stretch are the following: scheme stretch does not use strict geometric
series for node placement. If you specify scheme bias or dualbias using the "fine size" form, the interval count will be
hard-set to a value that fills in the curve.
Auto Bias
When using the command 'curve <range> scheme bias' with no additional parameters, an 'auto' setting will be enabled
by default for tet and tri meshing. This scheme honors sizes set at a curve's vertices and that vertex size will be used to
create a biased edge mesh. For example, two volumes with different sizes set on the volumes are merged. The sizes at
the vertices (averaged from sizes on the parent entities) will be used to create the biased edge mesh.
A user can set a size on a vertex with the following command:
Vertex <id> Size <size>
Discussion:
The Bias and DualBias schemes space the curve mesh unequally, placing more nodes towards (or away from) the ends
of the curve according to a geometric progression. The ratio of successive edges is the "factor," which may be greater
than or less than one. For bias, the series starts at the first vertex of the curve, or the "start vertex" if specified. For
dualbias, the series starts at both ends of the curve and meets in the middle.
The command behaves differently depending on which set of parameters are specified. There are three basic variables:
the interval count, the bias factor, or the first edge size. The curve length is a given, fixed quantity. The user can specify
any two of these variables, and the third will be automatically determined.
499
Trelis 15.0 User Documentation
If the "{Factor|First_Delta|Fraction}" form is specified, then the interval count is taken as a given. The interval count is
whatever was specified previously by an interval count or size command (see Interval Assignment). If "Factor" is
specified, then the first edge size will be automatically chosen so that the geometric progression of edges "fit" onto the
curve. If "first_delta" is specified, then the first edge length is exactly that absolute value, and the "factor" is automatically
chosen. If "fraction" is specified, then the first edge length is the curve length times that fraction, and again the "factor" is
automatically chosen.
If the "fine size" is specified, then the first edge length is exactly that absolute value. If the "factor" is specified, then the
interval count is automatically chosen. If an approximate coarse size is specified, then this also determines the factor, and
again the interval count is automatically chosen. If a surface sizing function type bias is used, then the curves of the
surface are sized using similar formulas.
If no start or end vertex is specified, the curve's start vertex is used as the starting point of the bias. (A curve's start vertex
can be identified by listing the curve from the "CUBIT>" prompt.)
If a curve needs to have its nodes distributed towards the opposite end, it can be easily edited using the reverse bias
command. Reversing the curve bias using this command is equivalent to setting a bias factor equal to the inverse of the
original bias factor. Reversing the bias can be performed on both meshed and unmeshed curves.
The maximum interval setting allows the user to set a maximum number of intervals on any bias curve. This value is
doubled for a curve with a dualbias scheme. It can be easy to accidentally specify a very large number of intervals and
this setting allows the user to place an upper limit the number of intervals.
The preview option will allow the user to preview mesh size and distribution on the curve before meshing.
The following figure shows the result of meshing edges with equal, bias and dualbias schemes.
500
Circle
Applies to: Surfaces
Summary: Produces a circle-primitive mesh for a surface
To create a circle mesh scheme on a surface
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Surface.
Click on the Mesh action button.
Enter the values for Select Surface. This can also be done using the Pick Widget function.
Select Circle from the drop-down menu.
Optionally, click on Advanced to further specify the settings.
Click on Apply Scheme and then Mesh.
Surface <range> Scheme [Sector] Circle [Interval <int>] [fraction <double>]
Discussion:
The Circle scheme is used in regions that should be meshed as a circle. A "circle" consists of a single loop of bounding
curves containing an even number of intervals. Thus, the circle scheme can be applied to circles, ellipses, ovals, and
regions with "corners" (e.g. polygons). The bounding curves should enclose a convex region. Non-planar bounding loops
can also be meshed using the circle primitive provided the surface curvature is not too great. The mesh resembles that
obtained via polar coordinates except that the cells at the "center" are quadrilaterals, not triangles. See Figure 1 for an
example of a circle mesh. Radial grading of the mesh may be achieved via the optional [intervals] input parameter. The
Fraction option has the range 0 < fraction < 1 and defaults to 0.5. Fraction determines the size of the inner portion of the
circle mesh relative to the total radius of the circle. The sector option was added to revert to legacy behavior which is not
recommended.
Figure 1. Circle Primitive Mesh
501
Curvature
Applies to: Curves
Summary: Meshes curves by adapting the interval size to the local curvature.
To mesh curves by adapting the interval size to the local curvature
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Curve.
Click on the Mesh action button.
Enter the values for Select Curves. This can also be done using the Pick Widget function.
Select Curvature from the drop-down menu.
Enter the appropriate Value.
Click on Apply Size and then Mesh.
Curve <range> Scheme Curvature <double>
Discussion:
The value of <double> controls the degree of adaptation. If zero, the resulting mesh will have nearly equal intervals. If
greater than zero, the smallest intervals will correspond to the locations of largest curvature. If less than zero, the largest
intervals will correspond to the locations of largest curvature. The default value of <double> is zero. Straight lines and
circular arcs will produce meshes with near-equal intervals. The method for generating this mesh is iterative and may
sometimes not converge. If the method does not converge, either the <double> is too large (over-adaptation) or the
number of intervals is too small. Currently, the scheme does not work on periodic curves.
503
Equal
Applies to: Curves
Summary: Meshes a curve with equally-spaced nodes
To mesh an equally-spaced curve
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh and then Curve.
Click on the Mesh action button.
Enter the values for Select Curves. This can also be done using the Pick Widget function.
Select Equal from the drop-down menu.
Select Approximate Size, Auto Size or Interval.
Enter the appropriate settings.
Click on Apply Size and then Mesh.
Curve <range> Scheme Equal
Discussion:
See Interval Assignment for a description of how to set the number of nodes or the node spacing on a curve.
505
Hole
Applies to: Annular Surfaces
Summary: Useful on annular surfaces to produce a "polar coordinate" type mesh (with the singularity removed).
To create a polar coordinate-like mesh
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Surface.
Click on the Mesh action button.
Enter the values for Select Surface. This can also be done using the Pick Widget function.
Select Hole from the drop-down menu.
Optionally, click on Advanced to further specify the settings.
Click on Apply Scheme and then Mesh.
Surface <surface_id_range> Scheme Hole [Rad_intervals <int>] [Bias <double>] [Pair Node <id>
With Node <id>]
Discussion:
A polar coordinate-like mesh with the singularity removed is produced with this scheme. The azimuthal coordinate lines
will be of constant radius (unlike scheme map) The number of intervals in the azimuthal direction is controlled by setting
the number of intervals on the inner and outer bounding loops of the surface (the number of intervals must be the same
on each loop). The number of intervals in the radial direction is controlled by the user input, rad_intervals (default is one).
A bias may be put on the mesh in the radial direction via the input parameter bias. The default bias of 0 gives a uniform
grading, a bias less than zero gives smaller radial intervals near the inner loop, and a bias greater than zero gives smaller
radial intervals near the outer loop.
The correspondence between mesh nodes on the inner and outer boundaries is controlled with the pair node "<loop nodeid> with node <loop node-id>" construct. One id on the inner loop and one id on the outer loop should be given to connect
the two nodes by a radial mesh line. Not choosing this option may result in sub-optimal node pairings with possible
negative Jacobians. To use this option, mesh the inner and outer curve loops and then determine the mesh node ids.
Figure 1. Example of Hole Scheme
507
Mapping
Applies to: Surfaces, Volumes
Summary: Meshes a surface/volume with a structured mesh of quadrilaterals/hexahedra.
To map on a surface
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Surface.
Click on the Mesh action button.
Enter the values for Select Surface. This can also be done using the Pick Widget function.
Select Map from the drop-down menu.
Optionally, click on Advanced to further specify the settings.
Click on Apply Scheme and then Mesh.
To map on a volume
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Volume.
Click on the Mesh action button.
Enter the values for Select Volumes. This can also be done using the Pick Widget function.
Select Map from the drop-down menu.
Click on Apply Scheme and then Mesh.
{Volume|Surface} <range> Scheme Map
Discussion:
A structured mesh is defined as one where each interior node on a surface/volume is connected to 4/6 other nodes.
Mappable surfaces contain four logical sides and four logical corners of the map; each side can be composed of one or
several geometric curves. Similarly, mappable volumes have six logical sides and eight logical corners; each side can
consist of one or several geometric surfaces. For example, in Figure 1 below, the logical corners selected by the algorithm
are indicated by arrows. Between these vertices the logical sides are defined; these sides are described in Table 1.
Figure 1. Scheme Map Logical Properties
Table 1. Listing of Logical Sides
Logical Side
Curve Groups
509
Trelis 15.0 User Documentation
Side 1
Curve 1
Side 2
Curve 2
Side 3
Curve 3, Curve 4, Curve 5
Side 4
Curve 6
Interval divisions on opposite sides of the logical rectangle are matched to produce the mesh shown in the right portion of
Figure 1. (i.e. The number of intervals on logical side 1 is equated to the number of intervals on logical side 3). The
process is similar for volume mapping except that a logical hexahedron is formed from eight vertices. Note that the
corners for both surface and volume mapping can be placed on curves rather than vertices; this allows mapping surfaces
and volumes with less than four and eight vertices, respectively. For example, the mapped quarter cylinder shown in
Figure 2 has only five surfaces.
Figure 2. Volume Mapping of a 5-surfaced volume
The mapper works on a bicubic interpolation of the points on the boundary to represent the surface. There may be times
that those points may not be on the surface exactly if the surface is not suitable for bicubic interpolation. The Mapping
Constraint flag tells the mapper to relax the nodes to the geometry or not.
Set Mapping Constraint {ON|off}
510
Pave
Applies to: Surfaces
Summary: Automatically meshes a surface with an unstructured quadrilateral mesh.
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Surface.
Click on the Mesh action button.
Enter the values for Select Surface. This can also be done using the Pick Widget function.
Select Pave from the drop-down menu.
Select On, Off or Extend from the Paver Cleanup menu.
Click on Apply Scheme and then Mesh.
Surface <range> Scheme Pave Related Commands:
[Set] Paver Diagonal Scale <factor (Default = 0.9)> [set] Paver Grid Cell <factor (Default = 2.5)>[set]
Paver LinearSizing {Off | ON} Surface <range> Sizing Function Type ...
[Set] Paver Smooth Method {DEFAULT | Smooth Scheme | Old}
[Set] Paver Cleanup {ON|Off|Extend}
Discussion:
Paving (Blacker, 91; White, 97) allows the meshing of an arbitrary three-dimensional surface with quadrilateral elements.
The paver supports interior holes, arbitrary boundaries, hard lines, and zero-width cracks. It also allows for easy
transitions between dissimilar sizes of elements and element size variations based on sizing functions. Figure 1 shows the
same surface meshed with mapping (left) and paving (right) schemes using the same discretization of the boundary
curves.
Figure 1. Map (left) and Paved (right) Surface Meshes
Element Shape Improvement
When meshing a surface geometry with paving, clean-up and smoothing techniques are automatically applied to the
paved mesh. These methods improve the regularity and quality of the surface mesh. By default the paver uses its own
smoothing methods that are not directly-callable from Trelis. Using one of Trelis' callable smoothing methods in place of
the default method will sometimes improve mesh quality, depending on the surface geometry and specific mesh
characteristics. If the paver produces poor element quality, switching the smoothing scheme may help. This is done by the
command:
[set] Paver Smooth Method {DEFAULT | Smooth Scheme | Old}
When the "Smooth Scheme" is selected, the smoothing scheme specified for the surface will be used in place of the
paver's smoother. See "Mesh Smoothing" for more information about the available smoothing schemes in Trelis.
511
Trelis 15.0 User Documentation
Controlling Flattening of Elements
The smoothers flatten elements, such as inserted wedges, that have two edges on the active mesh front. In meshes
where this "corner" is a real corner, flattening the element may give an unacceptable mesh. The following command
controls how much the diagonal of such an element is able to shrink.
[set] Paver Diagonal Scale <factor (Default = 0.9)>
The range of for the scale factor is 0.5 to 1.0. A scale factor of 1.0 will force the element to be a parallelogram as long as it
is on the mesh front. A value of 0.5 will allow the diagonal to be half its calculated length. The element may became
triangular in shape with the two sides on the mesh front being collinear.
Controlling the Grid Search for Intersection Checking
The paver divides the bounding box of a surface into a number of cells based on the average length of an element. It uses
these cells to speed intersection checking of new element edges with the existing mesh. If both very long and very short
edges fall in the same area, it is possible that a long edge which spans the search region is excluded from the intersection
check when it does intersect the new element. The following command allows the user to adjust the size of the grid cells.
[set] Paver Grid Cell <factor (Default = 2.5)>
The grid cell factor is a multiplier applied to the average element size, which then becomes the grid cell size. The
surface's bounding box is divided by this cell size to determine the number of cells in each direction. A larger cell size
means each cell contains more nodes and edges. A smaller cell size means each cell has fewer nodes and edges. A
larger cell size forces the intersection algorithm to check more potential intersections, which results in long paver times. A
smaller cell size gives the intersection algorithm few edges to check (faster execution) but may result in missed
intersections where the ratio of long to short element edges is great. Increase this value if the paver is missing
intersections of elements.
Controlling the Paver Sizing Function
The paving algorithm will automatically select a "linear" sizing function if the ratio the largest element to the smallest is
greater than 6.0 and no other sizing function is specified for the surface. This is usually desirable. When it is not, the user
can change this behavior with the command:
[set] Paver LinearSizing {Off | ON}
Setting paver linear sizing to "off" will keep the default behavior. The size of the element will be based on the side(s) of the
element on the mesh front. For a discussion of sizing functions, including how to automatically set up size transitions, see
Adaptive Meshing.
Controlling Paver Cleanup
The paver uses a mesh clean-up process to improve mesh quality after the initial paving operation. Clean-up applies local
connectivity corrections to increase the number of interior mesh nodes that are connected to four quadrilaterals.
Sometimes it fails to improve the mesh. The following command allows the user to control some aspects of the clean-up
process.
[Set] Paver Cleanup {ON|Off|Extend}
The default option is to clean-up the mesh. The off option will turn clean-up off and may give an invalid mesh. The extend
option enables a non-local topology replacement algorithm. The command without any option will list the current setting.
The extend option attempts to group several defective nodes in a region that may be replaced with a template that has
fewer defects. The images below show a mesh before and after using this option.
512
Pave
Figure 2. Paved mesh before using cleanup extend
513
Trelis 15.0 User Documentation
Figure 3. Paved mesh after using cleanup extend
514
Pentagon
Applies to: Surfaces
Summary: Produces a pentagon-primitive mesh for a surface
Syntax:
Surface <range> Scheme Pentagon
Discussion:
The pentagon scheme is a meshing primitive for 5-sided regions. It is similar to the triprimitive and polyhedron schemes,
but is hard-coded for 5 sided surfaces.
The pentagon scheme indicates the region should be meshed as a pentagon. The scheme works best if the shape has 5
well-defined corners; however shapes with more corners can be meshed. The algorithm requires that there be at least 10
intervals (2 per side) specified on the curves representing the perimeter of the surface. In addition, the sum of the intervals
on any three connected sides must be at least two greater than the sum of the intervals on the remaining two sides.
Figure 1 shows two examples of pentagon meshes.
Figure 1. Examples of Pentagon Scheme Meshes
515
Trelis 15.0 User Documentation
516
Pinpoint
Applies to: Curves
Summary:Meshes a curve with node spacing specified by the user.
To pinpoint where to place nodes on a curve
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Curve.
Click on the Mesh action button.
Enter the values for Select Curves. This can also be done using the Pick Widget function.
Select Pinpoint from the drop-down menu.
Enter the appropriate value for Distance(s) Along Curve:.
Click on Apply Size and then Mesh.
Curve <range> Scheme Pinpoint Location <list of doubles>
Discussion:
The Pinpoint scheme allow the user to specify exactly where on a curve to place nodes. The list of doubles are absolute
positions, measured from the start vertex. The user can enter as many as needed, and they do not need to be in
numerical order. Below is an example of a curve that has been meshed using the following scheme:
curve 2 scheme pinpoint location 1 4 5 6 6.2 6.4 6.6 9:
517
Polyhedron
Applies to: Surfaces and Volumes.
Summary: Produces an arbitrary-sided block primitive mesh for a surface or volume.
To use a polyhedron scheme on a volume or surface
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh.
Click on Volume or Surface.
Click on the Mesh action button.
Enter the values for Select Surfaces or Select Volumes. This can also be done using the Pick Widget
function.
Select Polyhedron from the drop-down menu.
Click on Apply Scheme and then Mesh.
Volume <range> Scheme Polyhedron
Surface <range> Scheme Polyhedron
Discussion:
The polyhedron scheme is a meshing primitive for 2d and 3d n-sided regions. This is similar to the triprimitive ,
tetprimitive, and pentagon schemes, except rather than 3, 4, or 5 sides, it allows an arbitrary number of sides. The
scheme works best on convex regions. Surfaces must have only one loop, and each vertex must be connected to exactly
two curves on the surface (e.g., no hardlines). Volumes must have only one shell, each vertex must be connected to
exactly three surfaces on the volume, and each surface should be meshed with scheme polyhedron. There are some
interval assignment requirements as well, which should be automatically handled by Trelis.
If the polyhedron scheme is specified for the volume, then the surfaces of the volume are automatically assigned scheme
polyhedron as well, unless they were hard-set by the user. Schemes should be specified on all volumes of an assembly
prior to meshing any of them. Scheme polyhedron attaches extra data to volumes; if Trelis is behaving strangely, the user
may need to explicitly remove that data with a reset volume all, or similar command.
Scheme polyhedron was designed for assemblies of material grains, where each volume is roughly a Voronoi region, and
the assembly is a periodic space-filling model (tile). Figure 1 shows two examples of polyhedron meshes.
519
Trelis 15.0 User Documentation
520
Polyhedron
Figure 1. Examples of Polyhedron Scheme Meshes
521
Sphere
Applies to: Volumes topologically equivalent to a sphere and having one surface.
Summary: Generates a radially-graded hex mesh on a spherical volume.
To create a mesh on a spherical volume
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Volume.
Click on the Mesh action button.
Enter the values for Select Volumes. This can also be done using the Pick Widget function.
Select Sphere from the drop-down menu.
Optionally, click on Advanced to further specify the settings.
Click on Apply Scheme and then Mesh.
Volume <range> Scheme Sphere [Graded_interval <int>] [Az_interval <int>] [Bias <val>] [Fraction
<val>]
Discussion:
This scheme generates a radially-graded mesh on a spherical volume having a single bounding surface. The mesh is a
straightforward generalization of the circle scheme for surfaces. The number of azimuthal intervals around the equator is
controlled by the az_interval input parameter. The number of radial intervals in the outer portion of the sphere is controlled
by the graded_interval input parameter. Azimuthal mesh lines in the outer portion of the sphere have constant radius. The
inner portion of the volume mesh forms a cube. The bias parameter controls the amount of radial grading in the outer
portion of the mesh (default=1 gives a uniform mesh). The fraction parameter (between 0 and 1) determines what fraction
of the sphere is occupied by the inner cube.
Figure 1. Sphere Scheme Example
523
STransition
Applies to: Surfaces
Summary:
Produces a simple transitional mapped mesh.
Syntax
:
Surface <surface_id_range> Scheme STransition [Triangle] [Coarse]
Discussion:
The STransition scheme transitions a mesh from one element density to another across a surface. This scheme is
particularly helpful when the Paving scheme produces a poor mesh. The following two figures show a specific case where
the STransition scheme may offer an improvement.
Pave scheme
STransition scheme
The coarse option forces the mesh to transition to a coarser mesh in the first layer.
STransition scheme with coarse option
For triangular surfaces, the STransition scheme with the triangle option will produce similar results when compared to the
Triprimitive scheme. However, STransition is capable of handling more varied interval settings. The following triangle fails
when using the Triprimitive scheme but succeeds with the STransition scheme.
525
Trelis 15.0 User Documentation
STransition scheme on a triangular surface with intervals
set to 3, 3, and 6.
The figures below show the STransition meshing scheme response to different shapes and interval settings.
STransition scheme on a rectangular surface with three
intervals set to 2 and one set to 4.
STransition scheme on a rectangular surface with
intervals set to 2, 3, 4, and 5.
The user also has the option of specifying END or SIDE surface vertex types.
526
STransition
STransition scheme on a hexagon surface with five intervals
set to 2, one interval set to 8, and user specified endpoints.
Note, that the Centroid Area Pull smoothing algorithm sometimes gives better results than the default Winslow smoothing
algorithm for STransition meshes.
527
Stretch
Applies to: Curves
Summary: Permits user to specify the exact size of the first and/or last edges on a curve.
To stretch a curve
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh and then Curve.
Click on the Mesh action button.
Enter the values for Select Curves. This can also be done using the Pick Widget function.
Select Stretch from the drop-down menu.
Select Size or Stretch Factor from the Size/Stretch menu.
Enter in the appropriate settings.
Click on Apply Size and then Mesh.
Curve <range> Scheme Stretch [First_size <double>] [Last_size <double>] [Start Vertex <id>]
Curve <range> Scheme Stretch [Stretch_factor <double>] [Start Vertex <id>]
Related Commands:
Scheme Bias and Dualbias.
Discussion:
This scheme allows the user to specify the exact length of the first and/or last edge on a curve mesh. Intermediate edge
lengths will vary smoothly between these input values. Reasonable values for these parameters should be used (for
example, the sizes must be less than the total length of the curve). If last_size is input, first_size must be input also. If
stretch_factor is input, neither first_size nor last_size can be input. This scheme does not currently work on periodic
curves.
529
Stride
Applies to: Curves
Summary: Mesh a curve with node spacing based on a general field function.
Syntax:
Curve <range> Scheme Stride
Discussion:
The ability to specify the number and location of nodes based on a general field function is also available in Trelis. With
this capability the node locations along a curve can be determined by some field variable (e.g. an error measure). This
provides a means of using Trelis in adaptive analyses. To use this capability, a sizing function must have been read in
and associated to the geometry (See Exodus II -based field function for more information on this process). After a sizing
function is made available, the stride scheme can be used to mesh the curves.
531
Submap
Applies to: Surfaces, Volumes
Summary: Produces a structured mesh for surfaces/volumes with more than 4/6 logical sides
To submap on a surface
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Surface.
Click on the Mesh action button.
Enter the values for Select Surface. This can also be done using the Pick Widget function.
Select SubMap from the drop-down menu.
Optionally, click on Advanced to further specify the settings.
Click on Apply Scheme and then Mesh.
To submap on a volume
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Volume.
Click on the Mesh action button.
Enter the values for Select Volumes. This can also be done using the Pick Widget function.
Select SubMap from the drop-down menu.
Click on Apply Scheme and then Mesh.
{Surface|Volume} <range> Scheme Submap
Related Commands:
{Surface|Volume} <range> Submap Smooth <on|off>
Discussion:
Submapping (Whiteley, 96) is a meshing tool based on the surface mapping capability discussed previously, and is suited
for mesh generation on surfaces which can be decomposed into mappable subsurfaces. This algorithm uses a
decomposition method to break the surface into simple mappable regions. Submapping is not limited by the number of
logical sides in the geometry or by the number of edges. The submap tool, however is best suited for surfaces and
volumes that are fairly blocky or that contain interior angles that are close to multiples of 90 degrees.
An example of a volume and its surfaces meshed with submapping is shown in Figure 1.
Figure 1. Quadrilateral and Hexahedral meshes generated by submapping
Like the mapping scheme, submapping uses vertex types to determine where to put the corners of the mapped mesh
(See Surface Vertex Types). For surface submapping, curves on the surface are traversed and grouped into " logical
sides " by a classification of the curves position in a local "i-j" coordinate system.
533
Trelis 15.0 User Documentation
Volume submapping uses the logical sides for the bounding surfaces and the vertex types to construct a logical "i-j-k"
coordinate system, which is used to construct the logical sides of the volume. For surface and volume submapping, the
sides are used to formulate the interval constraints for the surface or volume.
Figure 2 shows an example of this logical classification technique, where the edges on the front surface have been
classified in the i-j coordinate system; the figure also shows the submapped mesh for that volume.
Figure 2. Scheme Submap Logical Properties
In special cases where quick results are desired, submap cornerpicking can be set to OFF. The corner picking will be
accomplished by a faster, but less accurate algorithm which sets the vertex types by the measured interior angle at the
given vertex on the surface. In most cases this is not recommended.
Set Submap CornerPicking {ON|off}
After submapping has subdivided the surface and applied the mapped meshing technique mentioned above, the mesh is
smoothed to improve mesh quality. Because the decomposition performed by submapping is mesh based, no geometry is
created in the process and the resulting interior mesh can be smoothed. Sometimes smoothing can decrease the quality
of the mesh; in this case the following command can turn off the automatic smoothing before meshing:
{Surface|Volume} <range> Submap Smooth <on|off>
Surface submapping also has the ability to mesh periodic surfaces such as cylinders. An example of a periodic surface
meshed with submapping is shown in Figure 3. The requirement for meshing these surfaces is that the top and bottom of
the cylinder must have matching intervals.
Figure 3. Periodic Surface Meshing with Submapping
For periodic surfaces, there are no curves connecting the top and bottom of the cylinder. Setting intervals in this direction
on the surface can be done by setting the periodic interval for that surface (see Interval Assignment). No special
commands need to be given to submap a periodic surface, the algorithm will automatically detect the fact that the surface
is periodic. Currently, periodic surfaces with interior holes are not supported.
534
Submap
535
Surface Vertex Types
•
•
•
•
•
Surface Vertex Commands
Listing and Drawing Vertex Types
Triangle Vertex Types
Adjusting the Automatic Vertex Type Selection Algorithm
Volume Curve Types
Several meshing algorithms in Trelis "classify" the vertices of a surface or volume to produce a high quality mesh. This
classification is based on the angle between the edges meeting at the vertex, and helps determine where to place the
corners of the map, submap or trimesh, or the triangles in the trimap or tripave schemes. For example, a surface mapping
algorithm must identify the four vertices of the surface that best represent the surface as a rectangle. Figure 1 illustrates
the vertex angle types for mapped and submapped surfaces, and the correspondence between vertex types and the
placement of corners in a mapped or submapped mesh.
Figure 1. Angle Types for Mapped and Submapped Surfaces: An End vertex is contained in one element, a Side
vertex two, a Corner three, and a Reversal four.
The surface vertex type is computed automatically during meshing, but can also be specified manually. In some cases,
choosing vertex types manually results in a better quality mesh or a mesh that is preferable to the user. Vertex types have
a firmness, just as meshing schemes do. Automatically selected vertex types are soft, while user-set vertex types are
hard. Instead of a type, an angle in degrees can be specified instead.
Surface Vertex Commands
Vertex types are set using the following commands:
Surface <surface_id> Set [Vertex <vertex_id_range> [Loop_index <int>]] Type
{End|Side|Corner|Reversal}
Surface <surface_id> Set Vertex [<vertex_id_range> [Loop_index <int>]] Angle <value>
Surface <surface_id> Set [Vertex <vertex_id_range> [Loop_index <int>]] Type {Default|Soft|Hard}
If no vertices are specified, the command is applied to all vertices of each surface. The loop_index is used only for
vertices that are on the boundary of a single surface more than once.
Note that a vertex may be connected to several surfaces and its classification can be different for each of those surfaces.
The influence of vertex types when mapping or submapping a surface is illustrated in Figure 2. There, the same surface is
submapped in two different ways by adjusting the vertex types of ten vertices.
537
Trelis 15.0 User Documentation
Figure 2. Influence of vertex types on submap meshes; vertices whose types are changed are indicated above,
along with the mesh produced; logical submap shape shown below.
Listing and Drawing Vertex Types
Listing a surface lists the types of the vertices. The vertex type settings may also be drawn with the following commands:
Draw Surface <surface_id_range> {Vertex Angle|Vertex Type}
Triangle Vertex Types
For a surface that will be meshed with scheme trimap or tripave, the user may specify the angle below which triangles are
inserted:
Surface <surface_id_range> Angle <angle>
The user may also set whether to add a triangle at a particular vertex:
Surface <surface_id> Set [Vertex <vertex_id_range> [Loop_index <int>]] Type {Triangle|Nontriangle}
Adjusting the Automatic Vertex Type Selection Algorithm
The user may specify the maximum allowable angle at a corner with the following command:
Set {Corner|End} Angle <degrees>
The user may also give greater priority to one automatic selection criteria over the others by changing the following
absolute weights. The corner weight considers how large angles are at corners. The turn weight considers how Lshaped the surface is. The interval weight considers how much intervals must change. The large angle weight affects
only auto-scheme selection: surfaces with a large angle will be paved instead. Each weight's default is 1 and must be
between 0 and 10. The bigger a weight the more that criteria is considered.
538
Surface Vertex Types
Set Corner Weight <value>
Set Turn Weight <value>
Set Interval Weight <value>
Set Large Angle Weight <value>
An illustration of a mesh produced by the submapping algorithm is shown in Figure 2. The meshes produced by
submapping on the left and right result from adjusting the vertex types of the eight vertices shown.
Volume Curve Types
When sweeping, a 2.5 dimensional meshing scheme, curves perpendicular to the sweep direction can have a type with
respect to the volume. These types are usually automatically selected. The following commands are useful:
Draw Volume <surface_id_range> {Curve Angle|Curve Type}
List Volume <volume_id> Curve Type
Volume <volume_id> Set [Curve <curve_id_range>] Type {End|Side|Corner|Reversal}
Volume <volume_id> Set [Curve <curve_id_range>] Type {Default|Soft|Hard}
539
Sweep
Applies to: Volumes
Summary: Produces an extruded hexahedral mesh for 2.5D volumes.
To sweep a volume
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Mesh and then Volume.
Click on the Mesh action button.
Enter the appropriate value for Select Volumes. This can also be done using the Pick Widget function.
Select Sweep from the drop-down menu.
Select Specify Source and Target or Auto Select Source and Target.
Enter the appropriate settings.
Click Apply Scheme.
Click Mesh.
Volume <range> Scheme Sweep [Source [Surface] <range>] [Target [Surface] <range>]
[Propagate_bias]
[Sweep_smooth {auto | smart_affine | linear | residual | winslow} ]
[Sweep_transform {LEAST_SQUARES | Translate} ]
[Autosmooth_target {on | OFF} ]
Volume <range> Scheme Sweep Vector <xval yval zval>
Related Commands:
Set Multisweep [On|Off]
Multisweep Smoothing {ON|Off}
Multisweep Volume <range> Remove
Volume <range> Redistribute Nodes {ON|off}
Discussion:
The sweep algorithm (Knupp, 98, Scott et.al, 05) can sweep general 2.5D geometries and can also do pure translation or
rotations. A 2.5D geometry is characterized by source and target surfaces which are topologically similar. The hexahedral
mesh is swept (extruded) between source and target along a single logical axis. Bounding the swept hexahedra between
source and target surfaces, are the linking surfaces. Figures 1 and 2 show examples of source, target and linking
surfaces.
Command Options: The user can specify the source and target surfaces. The user can also specify a geometric vector
approximating the sweep direction, and let CUBIT determine the source and target surfaces. The user can specify just the
source surfaces, and let cubit guess the target, or "scheme auto" can also be used.
541
Trelis 15.0 User Documentation
Figure 1. Sweep Volume Meshing
Figure 2. Multiple Linking Surface Volume Meshing with Scheme Sweep
In general, the procedure for using the sweep scheme is to first mesh the source surfaces. Any surface meshing scheme
may be employed. Figure 1 displays swept meshes involving mapped and paved source surfaces. Linking surfaces must
have either mapping or submapping schemes applied. The sweep algorithm can also handle multiple surfaces linking the
source surface and the target surfaces. An example of this is shown in Figure 2. Note that for the multiple- linking-surface
meshing case, the interval requirement is that the total number of intervals along each multiple edge path from the source
surface to the target surface must be the same for each path. Once the appropriate mesh is applied to the source surface
and intervals assigned, the mesh command may be issued.
In many cases auto-scheme selection can simplify this process by recognizing sweepable geometries and automatically
select source and target surfaces. If the source and target surfaces are not specified, CUBIT attempts to automatically
select them. CUBIT also automatically sets curve and vertex types in an attempt to make the mesh of the linking surfaces
lead from a source surface to a target surface. These automatic selections may occasionally fail, in which case the user
must manually select the source/target surfaces, or some of the curve and vertex types. After making some of these
changes, the user should again set the volume scheme to sweep and attempt to mesh.
Occasionally the user must also adjust intervals along curves, in addition to the usual surface interval matching
requirements. For a given pair of source/target surfaces, there must be the same number of hexahedral layers between
them regardless of the path taken. This constrains the number of edges along curves of linking surfaces. For example, in
Figure 1 right, the number of intervals through the holes must be the same as along the outer shell.
Propagate_bias Option: The propagate_bias option attempts to preserve the source bias by propagating bias mesh
schemes from the curves of the source surface to the curves of the target surface.
Sweep_transform Option: Swept meshes are created by projecting points between the source and target surfaces using
affine transformations and then connecting them to form hexahedra. The method used to calculate the affine
transformations is set using the sweep_transform option.
542
Sweep
Least_squares: If the least_squares option is selected then affine transformations between the
source and target are calculated using a least squares method.
translate: If the translate option is selected then a simple translate affine transformation is calcuated
based upon the centroid of the source and target.
Sweep_smooth Option: To ensure adequate mesh quality, optional smoothing schemes are available to reposition the
interior nodes. The sweep tool permits five types of smoothing that are set with the following command prior to meshing a
volume whose mesh scheme is sweep:
Linear: If this option is selected, no layer smoothing is performed. The node positions are determined
strictly by the affine transformation from the previous layer. Good quality swept meshes can be
constructed using “linear” provided the volume geometry and meshed linking surfaces permit the
volume mesh to be created by a translation, scaling, and/or rotation of the source mesh. Volumes for
which this is nearly true may also produce acceptable quality with “linear”. As one would expect, this
option generates swept meshes more quickly than the other sweep smooth options. This option is
rarely needed since the next option produces better results with little time penalty.
Smart_affine: The “smart_affine” option does minimal smoothing of the interior nodes. Affine
transformations are used to project the source and target surfaces to the middle surface of the
volume. The position of the middle surface nodes is the average of the projected nodes from the
source and target surfaces. The error in projecting from source and target is computed, and this error
is linearly distributed back to the source and target.
Residual: The “residual” method is often used for meshing volumes that cannot be swept with the
“smart linear” method. It tends to produce better quality meshes than the “smart linear” method while
running faster than the Winslow-based smoother. The sweeping algorithm uses an affine
transformation to calculate the interior nodes’ positions, but the mesh on the linking surface
determines the positions of the nodes on the boundary of the layer. For the “residual” method, CUBIT
calculates corrective adjustments for interior nodes using the “residuals” from boundary nodes. The
“residual” is defined as the distance between the boundary node’s position (as determined by the
surface mesh) and the boundary node’s ideal position (as determined by the affine transformation of
the previous layer). Cubit computes the residual forward from the source and backward from the
target to get best the possible node position.
Winslow: Smooth scheme “winslow” smooths each layer using a weighted, elliptic smoother. The
weights are computed from the source mesh; they help maintain any biased spacing that occurs on
the source mesh. For example, one might want to use the “winslow” option if the source was a biased
mesh that was created using scheme circle. The biasing of the outer elements of the source mesh
may be destroyed if one of the other smooth options is used. The interior nodes are initially place
using the residual method.
AUTO: This is the default for the sweep_smooth option. “auto” causes the Sweeper to automatically
choose between “smart_affine” and “residual.” Auto will choose “off” if the layer needs little or no
smoothing or “residual” if it needs smoothing. Scheme “auto” does not guarantee that no negative
Jacobians are produced. This option produces acceptable results in most cases. If it fails to produce
a quality mesh, then choose one of the other sweep smooth options.
If none of these smooth schemes result in adequate mesh quality, one can consider trying one of the
volume smoothing schemes such as condition number or mean ratio.
Autosmooth_target Option: With this option turned on the target surface mesh is smoothed before the volume is swept.
Multisweep
While the basic sweeping algorithm requires a single target surface, the sweeping algorithm can also handle multiple
target surfaces. The multisweep algorithm works by recognizing possible mesh and topology conflicts between the source
and target surfaces and works to resolve these conflicts through the use of the virtual geometry capabilities in CUBIT.
Figure 4 shows some examples of volumes which have been meshed with the multisweep algorithm.
543
Trelis 15.0 User Documentation
Figure 4. Examples of Multisweep meshes.
Linear: If this option is active and/or target surfaces are omitted from the scheme setting command,
CUBIT will determine source and target surfaces (See Automatic Scheme Selection). Sweeping can
be further automated using the "sweep groups" command.
•
544
Limitations: Not all geometries are sweepable. Even some that appear sweepable may not
be, depending on the linking surface meshes. Highly curved source and target surfaces
may not be meshable with the current sweep algorithm.
Sweep
•
Grouping Sweepable Volumes
Swept meshing relies on the constraint that the source and target meshes are topologically
identical or the target surface is unmeshed. This results in there being dependencies
between swept volumes connected through non-manifold surfaces; these dependencies
must be satisfied before the group of volumes can be meshed successfully. For example, if
the model was a series of connected cylinders, the proper way to mesh the model would be
to sweep each volume starting at the top (or bottom) and continuing through each
successive connected volume.
With larger models and with models that contain volumes that require many source
surfaces, the process of determining the correct sweeping ordering becomes tedious. The
sweep grouping capability computes these dependencies and puts the volumes into
groups, in an order which represents those dependencies. The volumes are meshed in the
correct order when the resulting group is meshed.
To compute the sweep dependencies, use the command:
Group Sweep Volumes
This will create a group named "sweep_groups", which can then be meshed using the
command:
Mesh sweep_groups
In some automated meshing systems, the source and target surfaces are named using a
naming pattern. For example, all source surfaces might be given names "xxx.source" and
all target surfaces might be named "xxx.target". This allows the automated setting of the
sweep direction based on predetermined names rather than ids. The following command is
used to set the source and targets based on the naming pattern.
Set {Source|Target} Surface Pattern '<pattern>' [Include Volume
Name]
The pattern is checked against all surfaces in the model using a simple case-sensitive
substring match. All surfaces which contain that string of letters in their name will be
designated as either a source or target surface, depending on which option the user
specifies. For example:
br x 10
surface 1 name 'brick.top'
surface 2 name 'brick.bottom'
set source surface pattern 'top'
set target surface pattern 'bottom'
volume 1 scheme sweep
list volume 1 brief
Node Redistribution
Volume <range> redistribute nodes {ON|off}
With redistribute set to ON, the boundary nodes of a mappable surface are moved until the
spacing between the nodes are equivalent on the two opposing curves. In other words, the
parametric values of the nodes lying on the two opposite curves are matched.
Redistribute option ON will assist in avoiding the skewness of the mapped mesh. In the
below examples, the linking surfaces are meshed using mapped scheme, and with
redistribute option ON, the skewness is significantly avoided (see figures (4) and (5)).
Note:
545
Trelis 15.0 User Documentation
1. Redistribute option ON will affect all mapped surfaces, not just the linking
surfaces of a swept volume. Even though the example below shows a swept
volume, the command can be used independent of the sweeping command. That
is, it can be used while meshing surface models that contain mappable surfaces.
2. If the linking surfaces of a swept mesh contain submappable surfaces, then the
affect of redistribute option ON is generally not seen. The current implementation
is restricted to mappable surfaces only and doesn’t handle submappable
surfaces. In the future, we should be able to easily extend the redistribute option
to submappable surfaces.
Figure 1 - Linking surfaces of a many-to-one sweepable solid (shown in green) is
mappable
Figure 2 - Highly skewed elements on the linking mapped surface with 'redistribute
nodes OFF'
546
Sweep
Figure 3 - Quality of mesh with 'Redistribute Nodes OFF'
Figure 4 - High skew on the linking mapped surface can be avoided with
'Redistribute Nodes ON'
547
Trelis 15.0 User Documentation
Figure 5 - Quality of mesh with 'Redistribute Nodes ON'
548
TetMesh
Applies to: Volumes
Summary: Automatically meshes a volume with an unstructured tetrahedral mesh.
To create a tetmesh
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh and then Volume.
Click on the Mesh action button.
Enter the appropriate value for Select Volumes. This can also be done using the Pick Widget function.
Select Tetmesh from the drop-down menu.
Enter the appropriate settings.
Click Apply Scheme.
Click Mesh.
Volume <range> Scheme TetMesh
Related Commands:
[Set] Tetmesher Optimize Level <level>
[Set] Tetmesher Optimize Overconstrained {on|OFF}
[Set] Tetmesher Optimize Sliver {on|OFF}
[Set] Tetmesher Optimize Default
[Set] Tetmesher Boundary Recovery {on|OFF}
[Set] Tetmesher Interior Points {ON|off}
THex Volume All
Volume <volume_id> Tetmesh Respect {Face|Tri|Edge|Node} <range>
Volume <volume_id> Tetmesh Respect Clear
Volume <volume_id> Tetmesh Respect File '<filename>'
Volume <volume_id> Tetmesh Respect Location (options)
Tetmesh Tri <range> [Make {Block|Group} [<id>]]
Tetmesh Tri <range> {Add|Replace} {Block|Group} <id>
Discussion
The TetMesh scheme fills an arbitrary three-dimensional volume with tetrahedral elements. The surfaces are first
triangulated with one of the triangle schemes (TriMesh or TriAdvance) or a quadrilateral scheme with the quadrilaterals
being split into two triangles.
The Distene/INRIA tet-mesher is included in Trelis. This is a robust and fast tetrahedral mesher developed in France at
INRIA and distributed and maintained by Distene. Figure 1 shows a volume filled with tetrahedra by this algorithm.
549
Trelis 15.0 User Documentation
Figure 1. Tetrahedral Mesh generated with the TetMesh scheme. Surface meshing was performed with the
TriAdvance scheme.
Trelis uses three of the four Distene/INRIA tetmesher modules: standard, boundary recovery and anisotropic-scalar. The
fourth module, anisotropic-tensor is not available to the Trelis user at this time. If you need element sizing based on a
tensor field, please contact [email protected]
The boundary recovery module differs from the standard one in that it allows the surface mesh constraints to be relaxed
during tet-meshing. Once tet-meshing is done, the surface mesh constraints are reapplied. This allows tet-meshing of
volumes bounded by poor quality surface triangularizations. The anisotropic-scalar module allows the user to apply a
scalar sizing function to the volume, and this size is respected, as far as possible, throughout the mesh.
The standard and boundary recovery modules are at revision 4.2, while the anisotripic modules are at revision 3.5.
Tetmesher Options
The user may set options that control the operation of the tet-meshing algorithms. These tetmesher options are global
settings and apply to all tetmeshes generated until the option is changed by the user.
The Tetmesher Optimize options listed below are only available in the standard module and will be ignored by the others.
[Set] Tetmesher Optimize Level <level>
The Tetmesher Optimize Level command allows the user to control the degree of optimization. The optimization level is
an integer in the range 0 to 6, which represent optimization levels of none, light, medium, standard, strong, heavy, and
extreme. Greater values will result in greater computation time. The default is 3 or standard optimization.
[Set] Tetmesher Optimize Overconstrained {on|OFF}
550
TetMesh
The Tetmesher Optimize Overconstrained command enables or disables an additional optimization step that attempts to
eliminated tetrahedral elements that share multiple surface triangles. This optimization may improve the mesh for finite
element analysis. The default setting is off.
[Set] Tetmesher Optimize Sliver {on|OFF}
The Tetmesher Optimize Sliver command enables or disables an additional optimization step that attempts to eliminate
tetrahedral sliver elements. The default setting is off.
[Set] Tetmesher Optimize Default
The Tetmesher Optimize Default command restores the default optimizations values: level = 3 (standard),
overconstrained = off, and sliver = off.
[Set] Tetmesher Boundary Recovery {on|OFF}
The Tetmesher Boundary Recovery command allows the user to enable or disable the use of the boundary recovery
module. By default, the standard module is used if no sizing function is declared for the volume; the anisotropic-scalar
module is used if one is declared. Trelis selects the boundary recovery module if the minimum surface element condition
number is less than 0.2. This option allows the user to force Trelis to select the boundary recovery module instead of the
standard module even if the minimum surface element condition number is greater than 0.2. The default setting is off.
[Set] Tetmesher Interior Points {ON|off}
Infrequently, the user desires a model with as few interior points as possible. The Tetmesher Interior Points command
allows the user to enbale or disable the insertion of interior points. If interior points are disable, the tetmesher will attempt
to mesh the volume using only the exterior points. This may not be possible and a few points will be inserted to allow tetmeshing to complete. The default setting is on.
Using tets as the basis of an unstructured hexahedral mesh
Tet meshing can be used to generate hexahedral meshes using the THex command. Each of the tetrahedron can be
converted into 4 hexes, producing a fully conformal hexahedral mesh, albeit of poorer quality. These meshes can often be
used in codes that are less sensitive to mesh quality and mesh directionality. The THex command requires that all tets in
the model be converted to hexahedra with the same command.
Conforming the tetmesh to internal features
In some cases it is necessary for the finite element mesh to conform to internal features of the model. The tetmesh
scheme provides this capability provided the tetmesh respect command has been previously issued to define the features
that will be respected.
Volume <volume_id> Tetmesh Respect {Face|Tri|Edge|Node} <range>
The tetmesh respect command allows the user to specify mesh entities that will be part of a tetrahedral mesh. These
faces, triangles, edges, or nodes are inside the volume since all surface mesh features will appear in the final tetrahedral
mesh by default. These mesh entities specified to be respected can be generated from other meshing commands on free
vertices, curves, or surfaces.
551
Trelis 15.0 User Documentation
Figure 2. Example of using tetmesh respect to ensure node 9 is captured in the tetmesh.
Figure 2 is an example of using the tetmesh respect command to enforce a node at the center of a cube. Node 9 in this
example was generated by first creating a free vertex at the center location and meshing the vertex. (mesh vertex 9). The
following commands would then be used to generate the tetmesh that respected node 9.
volume 1 scheme tetmesh
tetmesh respect node 9
mesh volume 1
The tetmesh respect command can also be used to enforce multiple mesh entities. To accomplish this, the tetmesh
respect command may be issued multiple times. For example, If node12 and a triangle 2 inside volume 3 was to appear in
the volumetric mesh, the following commands could be used:
volume 3 scheme tetmesh
volume 3 tetmesh respect node 12
volume 3 tetmesh respect tri 2
mesh volume 1
Unlike the tetmesh respect command described above, the tetmesh respect file and tetmesh respect location
commands do not require underlying geometry.
Volume <volume_id> Tetmesh Respect File '<filename>'
Volume <volume_id> Tetmesh Respect Location (options)
These two commands create mesh data that only the tetmesher knows about. Thus, to respect a point at (1.0, 0.0, -1.0) in
your model, enter the command
volume 1 tetmesh respect location 1 0 -1
This is much simpler than creating the vertex, meshing it, and then respecting it.
If the model has many points that must be respected, use the file version of the command. First generate a file with all of
the points, edges, and triangles that should be respected. The format of the file is the format used by the facet file. Now,
use the following command to respect all of the information in the file for the given volume.
volume 2 tetmesh respect file 'my_points.facet'
Finally, the following command is used to remove the respected data from an entity.
Volume <volume_id> Tetmesh Respect Clear
The tetmesh respect clear command is the only way to remove respected data from a volume without deleting the volume.
Unfortunately, it removes all respected data from the volume. Therefore, if the model has a lot of data to be respected, it is
best to put it in a file or keep a journal file that can be edited.
552
TetMesh
Generating a Tetmesh from a Skin of Triangles
Tetmesh Tri <range> [Make {Block|Group} [<id>]]
Tetmesh Tri <range> {Add|Replace} {Block|Group} <id>
The Tetmesh Tri command generates a tetrahedral mesh from the list of triangles entered. The triangles must form a
closed surface. The command fails if they do not. The list of triangles may be a skin, and thus a command such as
'tetmesh tri in block 1' would be acceptable, should block 1 be a previously defined skin.
The first command form has optional arguments. If the make option and its arguments are present, then the specified
object receives the tet mesh. The command fails if an object with the optional identifier exists. If the object identifier is
omitted, the identifier is set to the next available block.
The second command form has two options, add and replace. Each option has a required, associated identifier. If the
identifier is missing or invalid, the command fails. The add option appends the tet mesh to the object. The replace option
removes any existing mesh from the object before adding the tet mesh.
553
Tetprimitive
Applies to: Volumes
Summary: Meshes a 4 "sided" object with hexahedral elements using the standard tetrahedron primitive.
To use a tetprimitive scheme
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh and then Volume.
Click on the Mesh action button.
Enter the appropriate value for Select Volumes. This can also be done using the Pick Widget function.
Select Tetprimitive from the drop-down menu.
Enter the appropriate settings.
Click Apply Scheme.
Click Mesh.
Volume <range> Scheme Tetprimitive [Combine Surface <range>] [Combine Surface <range>]
[Combine Surface <range>] [Combine Surface <range>]
Discussion:
The tetprimitive scheme is used to create a hexahedral mesh in a volume which fits the shape of a tetrahedral primitive.
The Tetprimitive scheme assumes that each of the four surfaces have been meshed with the triprimitive, or similar,
meshing scheme. If more than four surfaces form the tetrahedron geometry, the surfaces forming a logical side can be
combined using the combine option.
Figure 1. Sphere octant hex meshed with scheme Tetprimitive, surfaces meshed using scheme Triprimitive
555
TriDelaunay
Applies to: Surfaces
Summary: Automatically meshes parametric surface geometry with triangle elements.
To use a tridelaunay scheme
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Surface.
Click on the Mesh action button.
Enter the appropriate value for Select Surfaces. This can also be done using the Pick Widget function.
Select TriDelaunay from the drop-down menu.
Click Apply Scheme then click Mesh.
Surface <range> Scheme TriDelaunay
Discussion:
The scheme TriDelaunay is a parametric meshing algorithm. It can be run in two modes. The default mode (asp)
combines the Delaunay criterion for connecting nodes into triangles with an advancing-front approach for inserting nodes
into the mesh. This method maximizes the number of regular triangles in the mesh but does not guarantee the minimum
angle quality of the triangles. A guaranteed quality (gq) mode can be used for planar surfaces (only). This mode refines
the initial Delaunay configuration by placing points at the centroids of the worst triangles until the mesh has an acceptable
density. To switch between the two modes, use the following setting command.
[Set] Tridelaunay point placement {gq | guaranteed quality | asp}
TriDelaunay can also utilize a sizing function if one is defined for the surface.
Note: This algorithm is unstable for periodic surfaces which include a singularity point, E.G. spheres with poles, cone tips
and some types of toruses. Use scheme TriMesh, TriAdvance or QTri to mesh non-parametric or periodic parametric
surfaces.
557
TriAdvance
Applies to: Surfaces
Summary: Automatically meshes surface geometry with triangle elements.
Syntax:
Surface <range> Scheme TriAdvance
Discussion:
The triangle meshing scheme TriAdvance fills an arbitrary surface with triangle elements. It is an advancing front
algorithm which allows holes in the surface and transitions between dissimilar element sizes. It can use a sizing function
like the pave scheme if one is defined for the surface. Future development will add hard lines to this scheme's capabilities.
You specify this scheme for a surface by giving the command:
559
TriMap
Applies to: Surfaces
Summary: Places triangle elements at some vertices, and map meshes the remaining surface.
Syntax:
Surface <range> Scheme Trimap
Related Commands:
Surface <range> Vertex <range> Type {Triangle|Notriangle}
Discussion:
Some surfaces contain bounding curves which meet at a very acute angle. Meshing these surfaces with an allquadrilateral mesh will result in a very skewed quad to resolve that angle. In some cases, this is a worse result than
simply placing a triangular element to resolve that angle. This scheme resolves this situation by placing a triangular
element in these tight corners, and filling the remainder of the surface with a mapped mesh.
The algorithm can automatically compute whether a triangular element is necessary, along with where to place that
element. To override the choice of where triangular elements are used, the following command can be issued:
Surface <range> Vertex <range> Type {Triangle|Notriangle}
561
TriMesh
Applies to: Surfaces
Summary: Automatically meshes surface geometry with triangle elements using all available triangle meshing schemes.
To use a trimesh scheme
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Surface.
Click on the Mesh action button.
Enter the appropriate value for Select Surfaces. This can also be done using the Pick Widget function.
Select TriMesh from the drop-down menu.
Click Apply Scheme then click Mesh.
Surface <range> Scheme TriMesh
Discussion:
The scheme TriMesh automatically switches between TriDelaunay, TriAdvance, and the QTri schemes. First it tries the
TriDelaunay scheme if the surface is parametric and non-periodic. If that fails, it tries the TriAdvance scheme; and if that
fails it tries the QTri scheme. The QTri scheme first paves the surface and then cuts the quadrilateral elements in half to
form triangles. Figure 1 shows a surface meshed with the TriAdvance scheme, and Figure 2 shows the same surface
meshed using the Qtri method. The TriMesh scheme is the preferred triangle meshing scheme unless there is an
overriding reason to select one of the others. You specify this scheme for a surface by giving the command:
Surface <range> Scheme TriMesh
Figure 1. Triangle mesh generated with scheme TriAdvance
563
Trelis 15.0 User Documentation
Figure 2. Triangle mesh generated with QTri scheme
564
TriPave
Applies to: Surface
Summary: Places triangle elements at some vertices, and paves the remaining surface.
Syntax:
Surface <range> Scheme Tripave
Related Commands:
Surface <range> Vertex <range> Type {triangle|notriangle}
Discussion:
Similar to the trimap algorithm, but uses paving instead of mapping to fill the remainder of the surface with quadrilaterals.
The algorithm can automatically compute whether a triangular element is necessary, along with where to place that
element. To override the choice of where triangular elements are used, the following command can be issued:
Surface <range> Vertex <range> Type {triangle|notriangle}
565
TriPrimitive
Applies to: Surfaces
Summary: Produces a triangle-primitive mesh for a surface with three logical sides
To use a triprimitive scheme
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Surface.
Click on the Mesh action button.
Enter the appropriate value for Select Surfaces. This can also be done using the Pick Widget function.
Select TriPrimitive from the drop-down menu.
Click Apply Scheme then click Mesh.
Surface <range> Scheme Triprimitive [SMOOTH | nosmoothing]
Discussion:
The triprimitive scheme indicates that the region should be meshed as a triangle. A surface may use the triprimitive
scheme if three "natural", or obvious, corners of the surface can be identified. For instance, the surface of a sphere octant
(shown in the figure below) is handled nicely by the triprimitive scheme. The algorithm requires that there be at least 6
intervals (2 per side) specified on the curves representing the perimeter of the surface and that the sum of the intervals on
any two of the triangle's sides be at least two greater than the number of intervals on the remaining side. The following
figure illustrates a triprimitive mesh on a 3D surface.
By default, the triprimitive algorithm will smooth the mesh with an iterative smoothing scheme. This smoothing can be
disabled by using the "nosmoothing" option with this command. The quality of the mesh will often be significantly
degraded by disabling smoothing, but in certain cases the unsmoothed mesh may be preferred.
Figure 1. Surfaces meshed with scheme Triprimitive
567
Radialmesh
Summary: Creates a free cylindrical mesh with precise node locations based on input radii, angles, and offsets, then
creates mesh-based geometry to fit the mesh.
Syntax:
Create Radialmesh \
NumZ <val> [Span <val>] \
Zblock 1 [<offset val>] \
{Interval|Bias|Fraction|First Size} <val> \
[{Interval|Bias|Fraction|Last Size} <val>] \
Zblock 2 [<offset val>] \
{Interval|Bias|Fraction|First Size} <val> \
[{Interval|Bias|Fraction|Last Size} <val>] \
... NumZ \
NumR <val> {Trisection|Initial Radius<val>} \
Rblock 1 <offset radius val> \
{Interval|Bias|Fraction|First Size} <val> \
[{Interval|Bias|Fraction|Last Size} <val>] \
Rblock 2 <offset radius val> \
{Interval|Bias|Fraction|First Size} <val> \
[{Interval|Bias|Fraction|Last Size} <val>] \
... NumR \
NumA <val> [Full360] [Span <val>] \
Ablock 1 [<offset angle val>] \
{Interval|Bias|Fraction|First Angle} <val> \
[{Interval|Bias|Fraction|Last Angle} <val>] \
Ablock 2 [<offset angle val>] \
{Interval|Bias|Fraction|First Angle} <val> \
[{Interval|Bias|Fraction|Last Angle} <val>] \
... NumA
Discussion:
The purpose of the radialmesh command is to create a cylindrical mesh with precise node locations. Unlike all other
meshing commands which place nodes using smoothing algorithms to optimize element quality, node locations for the
radialmesh command are calculated based on the input radii, angles, and offsets. In addition, the radialmesh command
does not mesh existing geometry. Rather, it creates a mesh based on the input parameters, after which a mesh-based
geometry is created to fit the free mesh.
The radialmesh command requires input for the 3 coordinate directions (Z, radial, angular). The number of blocks in each
direction is specified with the numZ, numR, and numA values in the command. Each block forms a new volume in the final
mesh. All bodies in the mesh are merged to form a conformal mesh between blocks.
The Radialmesh command can create meshes which span any angle greater than 0.0 up to 360 degrees. In addition,
meshes can model either a tri-section (see Figure 1), or a non-trisection mesh (see Figure 2).
569
Trelis 15.0 User Documentation
Figure 1. Tri-section Radialmesh
Figure 2. Non-tri-section Radialmesh
The command to generate the mesh in Figure 1 is:
create radialmesh \
numZ 1 zblock 1 1 interval 5 \
numR 3 trisection rblock 1 2 interval 5 \
rblock 2 3 interval 5 \
rblock 3 4 interval 5 \
numA 1 span 90 ablock 1 interval 10
The command to generate the mesh in Figure 2 is:
create radialmesh \
numZ 1 zblock 1 1 interval 5 \
numR 1 initial radius 3 rblock 1 4 interval 5 \
numA 1 span 90 ablock 1 interval 10
A mesh can span an entire 360 degrees by using the “full360” keyword. For example, the mesh in Figure 3 was generated
with the following command:
570
Radialmesh
create radialmesh numZ 1 zblock 1 1 interval 5 \
numR 3 trisection rblock 1 1 interval 5 \
rblock 2 2 interval 5 \
rblock 3 3 interval 5 \
numA 5 full360 span ablock 1 interval 5 \
ablock 2 interval 5 \
ablock 3 interval 5 \
ablock 4 interval 5
Figure 4. Radialmesh using full360 option
After the mesh is generated, the radialmesh command fits the mesh with mesh based geometry. The surfaces created to
fit the mesh are given special names according to their location on the geometry. To see the names of the surfaces, issue
the command label surface name after creating a radialmesh. Also, if you create a tri-section mesh, the edges on the
center axis are given names. To see these names issue the command label curve name after creating a trisection
Radialmesh.
The user can control the number of intervals and the spacing of these intervals using the optional parameters in each
rblock, zblock and ablock. There are 11 combinations that these can be combined as listed below:
•
•
•
•
•
•
Interval Only- Example: "interval 5." The block will be meshed with 5 equally spaced intervals.
First Size Only- Example: “first size 2.5.” The block will be meshed with intervals of approximately 2.5 in length.
The total number of intervals is internally calculated and depends on the overall block length.
Fraction Only- Example: “fraction 0.3333.” The block will be meshed with intervals approximately
0.3333*overall block length.
Interval and Bias- Example: “interval 5 bias 1.5.” There will be 5 intervals on the block, which each interval
being 1.5 times the previous one. The length of each interval is calculated internally.
Interval and Fraction- Example: “interval 5 fraction 0.25.” There will be 5 intervals on the block, the first being
.25 of the length of the block with the remaining decreasing in size.
Interval and First Size- Example: “interval 5 first size 0.2.” There will be 5 intervals on the block, the first being
0.2 in length. The remaining intervals will increase or decrease to fill the blocks length.
571
Trelis 15.0 User Documentation
•
•
•
•
•
First Size and Last Size- Example: “first size 0.2 last size 0.4.” The first interval will be 0.2 in length. The last
interval will be 0.4 in length. The total number of intervals is internally calculated to allow for transition between
the 2 specified sizes.
First Size and Bias- Example “first size 0.2 bias 0.85.” The first interval will be 0.2 in length and the remaining
intervals will scale by a factor of 0.85 from one to the next until the block is filled. The total number of intervals is
internally calculated and depends on the overall block length.
Fraction and Bias- Example “fraction 0.25 bias 1.25.” The first interval will be 0.25 of the overall block length
and the remaining intervals will scale by a factor of 1.25 from one to the next until the block is filled. The total
number of intervals is internally calculated and depends on the overall block length.
Interval and Last Size- Example: “last size 1.5 interval 5.” The last interval will be 1.5 in length. The remaining
intervals will scale up or down to fit 5 intervals in the block.
Last Size and Bias- Example: “last size 2.0 bias 1.1.” The last interval will be 2.0 in length. The remaining
intervals will scale by 1.1 until the block is filled. The total number of intervals is internally calculated and
depends on the overall block length.
Figure 5 shows an example of a bias spaced mesh with the following command:
create radialmesh numZ 2 zblock 1 1 first size 0.2 \
zblock 2 10 first size 0.2 last size 1.0 \
numR 3 trisection rblock 1 1 interval 5 \
rblock 2 2 first size .25 \
rblock 3 5 first size .25 bias 2.0 \
numA 1 span 90 ablock 1 interval 5
572
Radialmesh
Figure 5. Radialmesh created with biased spacing
573
HTet
Applies to: Volumes
Summary: Converts an existing hex mesh into a conforming tetrahedral mesh.
Syntax:
HTet Volume <range> {UNSTRUCTURED | structured}
Discussion:
Unlike other meshing schemes in this section, The HTet command requires an existing hexahedral mesh on which to
operate. Rather than setting a meshing scheme for use with the mesh command, the HTet command works after an initial
hex mesh has been generated.
Two methods for decomposing a hex mesh into tetrahedra are available. Set the method to be used with the optional
arguments unstructured and structured. The unstructured method is the default. Figure 1 shows the difference between
the two methods:
Figure 1. Left: Unstructured method creates 6 tets per hex. Right: Structured method creates 28 tets per hex
Unstructured
This method creates 6 tetrahedra for every hexahedra. No new nodes will be generated. The orientation of the 6
hexahedra will be based upon the element node numbering, as a result orientations may change if node numbering
changes. This method is referred to as unstructured because the number of tetrahedra adjacent each node will be
relatively arbitrary in the final mesh. Tetrahedral element quality is generally sufficient for most applications, however the
user may want to verify quality before performing analysis.
575
Trelis 15.0 User Documentation
Structured
With this approach, 28 tetrahedra are generated for every hexahedra in the mesh. This method adds a node to each face
of the hex and one to the interior. Although this method generates significantly more elements, the orientation and quality
of the resulting tetrahedra are more consistent. Each previously existing interior node in the mesh will have the same
number of adjacent tetrahedra.
576
QTri
Applies to: Surfaces
Summary: Meshes surfaces using a quadrilateral scheme, then converts the quadrilateral elements into triangles.
Syntax:
Surface <range> Scheme Qtri [Base Scheme quad_scheme>]
QTri Surface <range>
Set QTri Split [2|4]
Set QTri Test {Angle|Diagonal}
Discussion:
QTri is used to mesh surfaces with triangular elements. The surface is, first, meshed with the quadrilateral scheme, and,
then, the generated quads are split along a diagonal to produce triangles. The first command listed above sets the
meshing scheme on a surface to QTri. The second form sets the scheme and generates the mesh in a single step.
In the first command, the user has the option of specifying the underlying quadrilateral meshing scheme using the base
scheme <quad_scheme> option. If no base scheme is specified, Trelis will automatically select a scheme. For nonperiodic surfaces, the base scheme will be set to scheme pave. For periodic surfaces, the base scheme will be set to
scheme map.
Generally, the second command, Qtri Surface <range>, is used on surfaces that have already been meshed with
quadrilaterals. If, however, this command is used on a surface that has not been meshed, a base scheme will
automatically be selected using CUBIT’s auto-scheme capabilities. The user can over-ride this selection by specifying a
quadrilateral meshing scheme prior to using the qtri command (using the Surface <range> Scheme <quad_scheme>
command).
In addition to the default 2 tris per quad, the set qtri split command may alter the QTri scheme so that it will split the quad
into 4 triangles per quad. Where the 4 option is used, an additional mesh node is placed at the centroid of each quad.
There are two methods that may be used to calculate the best diagonal to use for splitting the quadrilateral elements:
angle or diagonal. The angle measurement uses the largest angle, while the diagonal option uses the shortest diagonal.
The largest angle measurement will be more accurate but takes more time.
Also, the QTri scheme is used in the TriMesh command as a backup to the TriAdvance triangle meshing scheme.
Figure 1. Surface meshed with scheme QTri
577
Trelis 15.0 User Documentation
578
THex
Applies to: Volumes
Summary: Converts a tetrahedral mesh into a hexahedral mesh.
Syntax:
THex Volume <range>
Discussion:
The THex command splits each tetrahedral element in a volume into four hexahedral elements, as shown in Figure 1.
This is done by splitting each edge and face at its midpoint, and then forming connections to the center of the tet.
When THexing merged volumes, all of the volumes must be THexed at the same time, in a single command. Otherwise,
meshes on shared surfaces will be invalid. An example of the THex algorithm is shown in Figure 2.
Figure 1. Conversion of a tetrahedron to four hexahedra, as performed by the THex algorithm.
.
579
Trelis 15.0 User Documentation
Figure 2. A cylinder before and after the THex algorithm is applied.
580
TQuad
Applies to: Surfaces
Summary: Converts a triangular surface mesh into a quadrilateral mesh.
Syntax:
TQuad Surface <range>
Discussion:
The TQuad command splits each triangular surface element in four quadrilateral elements, as shown in Figure 1. This is
done by splitting each edge at its midpoint, and then forming connections to the center of the triangle. The result is the
same as using the THex algorithm, but only applies to surfaces. In general it is better to use a mapped or paved mesh to
generate quadrilateral surface meshes. However, the TQuad scheme may be useful for converting facet-based triangular
meshes to quadrilateral meshes when remeshing is not possible.
Figure 1. A triangle split into 3 quads using the TQuad scheme
581
Copying a Mesh
Applies to: Curves, Surfaces, Volumes
Summary: Copies the mesh from one entity to another
To copy a mesh on a curve
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Curve.
Click on the Copy/Morph action button.
Enter the values for Source Curve ID(s) and Target Curve ID(s). This can also be done using the Pick Widget
function.
Optionally, click on Optional Data to further specify the settings.
Click on Appy Scheme and then Mesh.
Curve <range> Scheme Copy source Curve <range> [Source Percent [<percentage> | auto]] [Source
[combine|SEPARATE]] [Target [combine|SEPARATE]] [Source Vertex <id_range>] [Target Vertex
<id_range>]]
Copy Mesh Curve <curve_id_range> Onto Curve <curve_id_range> [Source Node <starting node id>
<ending node id>] [Source Percent [<percentage>|auto]] [Source [combine|SEPARATE]] [Target
[combine|SEPARATE]] [Source Vertex <id_range>] [Target Vertex <id_range>]
To copy a mesh on a surface
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Surface.
Click on the Copy/Morph action button.
Enter the values for Source Surface ID(s) and Target Surface ID(s). This can also be done using the Pick
Widget function.
Optionally, click on Optional Data to further specify the settings.
Click on Appy Scheme and then Mesh.
Surface <range> Scheme Copy [Source Surface] <id> [[Source Curve <id> Target Curve <id>]
[Source Vertex <id> Target Vertex <id>] [Nosmoothing]
Copy Mesh Surface <surface_id> Onto Surface <surface_id> [Source Face <id_range>] [Source
Node <id> Target Node <id>] [Source Edge <id> Target Edge <id>] [Source Vertex <id> Target
Vertex <id>] [Source Curve <id> Target Curve <id>] [Nosmoothing]
To copy a mesh on a volume
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Volume.
Click on the Copy/Morph action button.
Enter the values for Source Volume ID(s) and Target Volume ID(s). This can also be done using the Pick
Widget function.
Optionally, click on Optional Data to further specify the settings.
Click on Appy Scheme and then Mesh.
Volume <range> Scheme Copy [Source Volume] <id> [[Source Surface <id> Target Surface <id>]
[Source Curve <id> Target Curve <id>] [Source Vertex <id> Target Vertex <id>]][Nosmoothing]
Copy Mesh Volume <volume_id> Onto Volume <volume_id> [Source Vertex <vertex_id> Target
Vertex <vertex_id> [Source Curve <curve_id> Target Curve <curve_id>] [Nosmoothing]
Related Commands:
Set Morph Smooth {on | off}
583
Trelis 15.0 User Documentation
Discussion:
If the user desires to copy the mesh from a surface, volume, curve, or set of curves that has already been meshed, the
copy mesh scheme can be used. Note that this scheme can be set before the source entity has been meshed; the source
entity will be meshed automatically, if necessary, before the mesh is copied to the target entity. The user has the option of
providing orientation data to specify how to orient the source mesh on the target entity. For example, when copying a
curve mesh, the user can specify which vertex on the source (the source vertex) gets copied to which vertex on the target
(the target vertex). If you need to reference mesh entities for the copy, use the Copy Mesh commands. If no orientation
data is specified, or if the data is insufficient to completely determine the orientation on the target entity, the copy
algorithm will attempt to determine the remaining orientation data automatically. If conflicting, or inappropriate, orientation
data is given, the algorithm attempts to discard enough information to arrive at a proper mesh orientation.
Curve mesh copying has certain options that allow the copying of just a section of the source curves' mesh. These options
are accessed through the extra keyword options. The percent option allows the user to specify that a certain percentage
of the source mesh be copied--in this context the auto keyword means that the percentage will be calculated based on the
ratio of lengths of the source and target curves. The combine and separate keywords relate to how the command line
options are interpreted. If the user wishes to specify a group of target curves that will each receive an identical copy of a
source mesh, then the target separate option should be used (this is the default). If, however, the user wishes the source
mesh to be spread out along the range of target curves, then the target combine option should be used. The source
curves are treated in a similar fashion.
Volume mesh copying depends on the surface copying scheme. Because of this, the target volume must not have any of
its surfaces meshed already.
Because of how the copying algorithm works, the target mesh might not be an exact copy of the source mesh. This
happens because of the effects of smoothing. If an exact copy is required, there are two possible solutions. The first
option is useful when the source and target surfaces or volumes are exact matches. If this criterion is met, the user may
specify the Nosmoothing option. That will disable any smoothing of the mesh on the target surface and thereby providing
an exact copy of the mesh. The second option is useful if the source and target surfaces are not identical. In this case the
user may set the morph smoothing flag on, which will activate a special smoother that will match up the meshes as closely
as possible.
584
Mirroring a Mesh
Applies to: Surfaces
Summary: Mirrors the mesh from one surface to another
To mirror a mesh
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Surface.
Click on the Mesh action button.
Enter the values for Select Surfaces. This can also be done using the Pick Widget function.
Select Mirror from the drop-down menu.
Optionally, click on Advanced to further specify the settings.
Click on Appy Scheme and then Mesh.
Surface <range> Scheme Mirror [Source Surface <id> [Source Vertex <id> Target Vertex <id>]]
[Nosmoothing]
Mirror Mesh Surface <surface_id> Onto Surface <surface_id> [Source Vertex <id> Target Vertex
<id> Source Curve <id> Target Curve <id> Source Node <id> Target Node <id>] [Nosmoothing]
Discussion:
The mirror scheme is very similar to the copy scheme. In order to understand what is changed, a discussion of the copy
command is in order. Depending on what the user enters for the copy scheme, the resulting mesh might be oriented one
of two ways. For example, if the user entered:
Surface 1 scheme copy source surface 2 source vertex 5 target vertex 1
then the algorithm would match vertex 1 with vertex 5, but then would have to make a guess about how to match the
curves. Lacking other pertinent data, the match will be a direct match, as is shown in the following figure:
Figure 1. Surface 1 copied onto surface 2
585
Trelis 15.0 User Documentation
Figure 2. Surface 1 mirrored onto surface 2
This default matching can be changed by specifying more information for matching, or the user can specify scheme
mirror. The mirror scheme sets up the copying information in such a way as to reverse the default orientation of the target
mesh, as is shown in the above figure (right).
There are times when the resulting mesh may not match the original mesh exactly due to smoothing. Using the
nosmoothing option will ensure that the resulting mesh matches the original mesh exactly.
The alternate form of the command copies the mesh immediately instead of setting a scheme first. This form of the
command can also use curves and mesh entities as references.
586
Automatic Scheme Selection
•
•
•
•
Default Scheme Selection
Automatic Scheme Selection General Notes
Surface Auto Scheme Selection
Volume Auto Scheme Selection
For volume and surface geometries the user may allow Trelis to automatically select the meshing scheme. Automatic
scheme selection is based on several constraints, some of which are controllable by the user. The algorithms to select
meshing schemes will use topological and geometric data to select the best quad or hex meshing tool. Auto scheme
selection will not select tet or tri meshing algorithms. The command to invoke automatic scheme selection is:
{geom_list} Scheme Auto
Specifically for surface meshing, interval specifications will affect the scheme designation. For this reason it is
recommended that the user specify intervals before calling automatic scheme selection. If the user later chooses to
change the interval assignment, it may be necessary to call scheme selection again. For example, if the user assigns a
square surface to have 4 intervals along each curve, scheme selection will choose the surface mapping algorithm.
However if the user designates opposite curves to have different intervals, scheme selection will choose paving, since this
surface and its assigned intervals will not satisfy the mapping algorithm's interval constraints. In cases where a general
interval size for a surface or volume is specified and then changed, scheme selection will not change. For example, if the
user specified an interval size of 1.0 a square 10X10 surface, scheme selection will choose mapping. If the user changes
the interval size to 2.0, mapping will still be chosen as the meshing scheme from scheme selection. If a mesh density is
not specified for a surface, a size based on the smallest curve on the surface will be selected automatically.
Default Scheme Selection
If the user does not set a scheme for a particular entity and chooses to mesh the entity, Trelis will automatically run the
auto scheme selection algorithm and attempt to set a scheme. In cases where the auto scheme selection fails to choose a
scheme, the meshing operation will fail. In this case explicit specification of the meshing scheme and/or further geometry
decomposition may be necessary.
The default scheme selection in Trelis, unless otherwise set, will attempt to set a quadrilateral or hexahedral meshing
scheme on the entity. If tet or tri meshing will always be the desired element shape, the following command can be used:
Set Default Element [Tet|Tri|HEX|QUAD|None]
Setting the default element to tet or tri will bypass the auto scheme selection and always use either the triadvance or
tetmesh schemes if the scheme has not otherwise been set by the user. The default settings of quad or hex will use the
automatic scheme selection.
Previous functionality of Trelis used a default scheme of map and interval of 1 for all surface and volume entities. For
backwards compatibility and if this behavior is still desired, the none option may be used on the set default element
command.
Auto Scheme Selection General Notes
In general, automatic scheme selection reduces the amount of user input. If the user knows the model consists of 2.5D
meshable volumes, three commands to generate a mesh after importing or creating the model are needed.
To automatically calculate the meshing scheme
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Volume.
Click on the Mesh action button.
Enter the appropriate value for Select Volumes. This can also be done using the Pick Widget function.
Select Automatically Calculate from the drop-down menu.
Click Apply Scheme then click Mesh.
volume all size <value>
587
Trelis 15.0 User Documentation
volume all scheme auto
mesh volume all
The model shown in the following figure was meshed using these three commands (part of the model is not shown to
reveal the internal structure of the model).
Figure 1. Non-trivial model meshed using automatic scheme selection
Scheme Firmness
Meshing schemes may be selected through three different approaches. They are: default settings, automatic scheme
selection, and user specification. These methods also affect the scheme firmness settings for surfaces and volumes.
Scheme firmness is completely analogous to interval firmness.
Scheme firmness can be set explicitly by the user using the command
{geom_list} Scheme {Default | Soft | Hard}
Scheme firmness settings can only be applied to surfaces and volumes.
This may be useful if the user is working on several different areas in the model. Once she/he is satisfied with an area's
scheme selection and doesn't want it to change, the firmness command can be given to hard set the schemes in that
area. Or, if some surfaces were hard set by the user, and the user now wants to set them through automatic scheme
selection then she/he may change the surface's scheme firmness to soft or default.
588
Automatic Scheme Selection
Surface Auto Scheme Selection
Surface auto scheme selection (White, 99) will choose between Pave, Submap, Triprimitive, and Map meshing schemes,
and will always result in selecting a meshing scheme due to the existence of the paving algorithm, a general surface
meshing tool (assuming the surface passes the even interval constraint).
Surface auto scheme selection uses an angle metric to determine the vertex type to assign to each vertex on a surface;
these vertex types are then analyzed to determine whether the surface can be mapped or submapped. Often, a surface's
meshing scheme will be selected as Pave or Triprimitive when the user would prefer the surface to be mapped or
submapped. The user can overcome this by several methods. First, the user can manually set the surface scheme for the
"fuzzy" surface. Second, the user can manually set the "vertex types" for the surface. Third, the user can increase the
angle tolerance for determining "fuzziness." The command to change scheme selection's angle tolerances is:
[Set] Scheme Auto Fuzzy [Tolerance] {value} (value in degrees)
The acceptable range of values is between 0 and 360 degrees. If the user enters 360 degrees as the fuzzy tolerance, no
fuzzy tolerance checks will be calculated, and in general mapping and submapping will be chosen more often. If the user
enters 0 degrees, only surfaces that are "blocky" will be selected to be mapped or submapped, and in general paving will
be chosen more often.
Volume Auto Scheme Selection
When automatic scheme selection is called for a volume, surface scheme selection is invoked on the surfaces of the
given volume. Mesh density selections should also be specified before automatic volume scheme selection is invoked due
to the relationship of surface and volume scheme assignment.
Volume scheme selection chooses between Map, Submap and Sweep meshing schemes. Other schemes can be
assigned manually, either before or after the automatic scheme selection.
Volume scheme selection is limited to selecting schemes for 2.5D geometries, with additional tool limitations (e.g. Sweep
can currently only sweep from several sources to a single target, not multiple targets); this is due to the lack of a
completely automatic 3D hexahedral meshing algorithm. If volume scheme selection is unable to select a meshing
scheme, the mesh scheme will remain as the default and a warning will be reported to the user.
Volume scheme selection can fail to select a meshing scheme for several reasons. First, the volume may not be
mappable and not 2.5D; in this case, further decomposition of the model may be necessary. Second, volume scheme
selection may fail due to improper surface scheme selection. Volume schemes such as Map, Submap, and Sweep require
certain surface meshing schemes, as mentioned previously.
589
Parallel Meshing
The set parallel meshing works with the export parallel command to generate a boundary mesh suitable for sweeping with
the pCAMAL application. Currently only the Trelis sweep scheme is affected, but the mapping and submapping schemes
may be in the future. The command syntax is:
Set Parallel Meshing {on|OFF}
For now, sweeping a volume in the parallel meshing mode will only generate the exterior shell of the volume, i.e, source,
linking, and target surfaces. This shell is written to an ExodusII file with the export parallel command.
To determine if you are currently in parallel meshing mode you may list the current status using the List Parallel
command.
List Parallel Meshing
591
Metrics for Edge Elements
The metrics used for edge elements in Trelis are summarized in the following table:
Function Name
Length
Dimension
Full Range
Acceptable Range
L^0
0 to inf
None
Quality Metric Definitions:
Length: Distance between beginning and ending nodes of an edge
Comments on Algebraic Quality Measures
1.
2.
The quality command for edge length only accepts edge elements as input; it does not accept geometry as
input.
The length metric is currently only available for edge elements. Edge elements are created by default when
curves and surfaces are meshed. Edge elements are not created for interior volume elements.
593
Metrics for Triangular Elements
The metrics used for triangular elements in Trelis are summarized in the following table:
Function Name
Dimension
Full Range
Acceptable Range
Reference
Element Area
L^2
0 to inf
None
1
Maximum Angle
degrees
60 to 180
60 to 90
1
Minimum Angle
degrees
0 to 60
30 to 60
1
Condition No
L^0
1 to inf
1 to 1.3
2
Scaled Jacobian
L^0
-1 to 1
0.2 to 1
2
Relative Size
L^0
0 to 1
0.25 to 1
3
Shape
L^0
0 to 1
0.25 to 1
3
Shape and Size
L^0
0 to 1
0.25 to 1
3
Distortion
L^2
-1 to 1
0.6 to 1
4
Approximate Triangular Quality Definitions:
Element Area: (1/2) * Jacobian at corner node
Maximum Angle: Maximum included angle in triangle
Minimum Angle: Minimum included angle in triangle
Condition No. Condition number of the Jacobian matrix
Scaled Jacobian: Minimum Jacobian divided by the lengths of 2 edge vectors
Relative Size: Min( J, 1/J ), where J is determinant of weighted Jacobian matrix
Shape: 2/Condition number of weighted Jacobian matrix
Shape & Size: Product of Shape and Relative Size
Distortion: {min(|J|)/actual area}*parent area, parent area = 1/2 for triangular element
Comments on Algebraic Quality Measures
Relative Size, Shape, and Shape & Size are algebraic metrics, which have well behaved properties. Trelis encourages the
use of these metrics over other metrics. These metrics are referenced to an ideal element which, in the case of triangular
elements, is an equilateral triangle. Thus deviations from an equilateral triangle are measured in various ways by the
algebraic metrics.
Relative size measures the size of the element vs. the size of reference element. If the element is twice or one-half the
size of the reference element, the relative size is one-half. By default, the size of the reference element is the average
size of all the elements that the quality command is currently evaluating.
595
Trelis 15.0 User Documentation
The shape and size metric measures how both the shape and relative size of the element deviate from that of the
reference element.
References for Triangular Quality Measures
1.
2.
3.
4.
596
Traditional.
Knupp, 2000.
P. Knupp, Algebraic Mesh Quality Metrics for Unstructured Initial Meshes, submitted for publication.
SDRC/IDEAS Simulation: Finite Element Modeling--User's Guide
Metrics for Quadrilateral Elements
The metrics used for quadrilateral elements in Trelis are summarized in the following table:
Function Name
Dimension
Full Range
Acceptable Range
Reference
Aspect Ratio
L^0
1 to inf
1 to 4
1
Skew
L^0
0 to 1
0 to 0.5
1
Taper
L^0
0 to +inf
0 to 0.7
1
Warpage
L^0
0 to 1
0.9 to 1.0
NEW
Element Area
L^2
-inf to inf
None
1
Stretch
L^0
0 to 1
0.25 to 1
2
Minimum Angle
degrees
0 to 90
45 to 90
3
Maximum Angle
degrees
90 to 360
90 to 135
3
Condition No.
L^0
1 to inf
1 to 4
4
Jacobian
L^2
-inf to inf
None
4
Scaled Jacobian
L^0
-1 to +1
0.5 to 1
4
Shear
L^0
0 to 1
0.3 to 1
5
Shape
L^0
0 to 1
0.3 to 1
5
Relative Size
L^0
0 to 1
0.3 to 1
5
Shear & Size
L^0
0 to 1
0.2 to 1
5
Shape & Size
L^0
0 to 1
0.2 to 1
5
Distortion
L^2
-1 to 1
0.6 to 1
6
Quadrilateral Quality Definitions
Aspect Ratio: Maximum edge length ratios at quad center
Skew: Maximum |cos A| where A is the angle between edges at quad center
597
Trelis 15.0 User Documentation
Taper: Maximum ratio of lengths derived from opposite edges
Warpage: Cosine of Minimum Dihedral Angle formed by Planes Intersecting in Diagonals
Element Area: Jacobian at quad center
Stretch: Sqrt(2) * minimum edge length / maximum diagonal length
Minimum Angle: Smallest included quad angle (degrees).
Maximum Angle: Largest included quad angle (degrees).
Condition No. Maximum condition number of the Jacobian matrix at 4 corners
Jacobian: Minimum pointwise volume of local map at 4 corners & center of quad
Scaled Jacobian: Minimum Jacobian divided by the lengths of the 2 edge vectors
Shear: 2/Condition number of Jacobian Skew matrix
Shape: 2/Condition number of weighted Jacobian matrix
Relative Size: Min( J, 1/J ), where J is determinant of weighted Jacobian matrix
Shear and Size: Product of Shear and Relative Size
Shape and Size: Product of Shape and Relative Size
Distortion: {min(|J|)/actual area}*parent area, parent area = 4 for quad
Comments on Algebraic Quality Measures
Shape, Relative Size, Shape & Size, and Shear are algebraic quality metrics that apply to quadrilateral elements. Trelis
encourages the use of these metrics since they have certain nice properties (see reference 5 below). The metrics are
referenced to a square-shaped quadrilateral element, thus deviations from a square are measured in various ways.
Shape measures how far skew and aspect ratio in the element deviates from the reference element.
Relative size measures the size of the element vs. the size of reference element. If the element is twice or one-half the
size of the reference element, the relative size is one-half. The reference element for the Relative Size metric is a square
whose area is determined by the average area of all the quadrilaterals on the surface mesh under assessment
Shape and size metric measures how both the shape and relative size of the element deviate from that of the reference
element.
The SHEAR metric is based on the condition number of the skew matrix. SHEAR is really just an algebraic skew metric
but, since the word skew is already used in the list of quad quality metrics, Trelis has chosen to use the word 'shear.'
Shear = 1 if and only if quadrilateral is a rectangle.
The Robinson 'skew' metric equals the ideal (zero) if the quad is a rectangle. It also attains the ideal if the quad is a
trapezoid, a kite, or even triangular!
References for Quadrilateral Quality Measures
1.
2.
3.
4.
5.
6.
598
(Robinson, 87)
FIMESH code.
Unknown.
(Knupp, 00)
P. Knupp, Algebraic Mesh Quality Metrics for Unstructured Initial Meshes, submitted for publication.
6. SDRC/IDEAS Simulation: Finite Element Modeling--User's Guide
Metrics for Quadrilateral Elements
Details on Robinson Metrics for Quadrilaterals
The quadrilateral element quality metrics that are calculated are aspect ratio, skew, taper, element area, and stretch. The
calculations are based on metrics described in (Robinson, 87). An illustration of the shape parameters is shown in Figure
1, below. The stretch metric is calculated by dividing the length of the shortest element edge divided by the length of the
longest element diagonal.
Figure 1. Illustration of Quadrilateral Shape Parameters (Quality Metrics)
599
Metrics for Tetrahedral Elements
The metrics used for tetrahedral elements in Trelis are summarized in the following table:
Function Name
Dimension
Full Range
Acceptable Range
Reference
Aspect Ratio Beta
L^0
1 to inf
1 to 3
1
Aspect Ratio Gamma
L^0
1 to inf
1 to 3
1
Element Volume
L^3
-inf to inf
None
1
Condition No
L^0
1 to inf
1 to 3
2
Jacobian
L^3
-inf to inf
None
2
Scaled Jacobian
L^0
-1 to 1
0.2 to 1
2
Shape
L^0
0 to 1
0.2 to 1
3
Relative Size
L^0
0 to 1
0.2 to 1
3
Shape and Size
L^0
0 to 1
0.2 to 1
3
Distortion
L^0
-1 to 1
0.6 to 1
4
Equivolume Skew
Fluent
Tet Squish
Fluent
Tetrahedral Quality Definitions
Aspect Ratio Beta: CR / (3.0 * IR) where CR = circumsphere radius, IR = inscribed sphere radius
Aspect Ratio Gamma: Srms**3 / (8.479670*V) where Srms = sqrt(Sum(Si**2)/6), Si = edge length
Element Volume: (1/6) * Jacobian at corner node
Condition No.: Condition number of the Jacobian matrix at any corner
Jacobian: Minimum pointwise volume at any corner
Scaled Jacobian: Minimum Jacobian divided by the lengths of 3 edge vectors
Shape: 3/Mean Ratio of weighted Jacobian Matrix
Relative Size: Min(J, 1/J), where J is the determinant of the weighted Jacobian matrix
Shape & Size: Product of Shape and Relative Size Metrics
Distortion: {min(|J|)/actual volume}*parent volume, parent volume = 1/6 for tet
601
Trelis 15.0 User Documentation
Equivolume Skew: (metric used by Fluent)
Tet Squish: (metric used by Fluent)
For tetra10 elements, the distortion metric can be used in conjunction with the shape metric to determine whether the midedge nodes have caused negative Jacobians in the element. The shape metric only considers the linear (parent) element.
If a tetra10 has a non-positive shape value then the element has areas of negative Jacobians. However, for elements with
a positive shape metric value, if the distortion value is non-positive then the element contains negative Jacobians due to
the mid-side node positions.
Note that, for tetrahedral elements, there are several definitions of the term "aspect ratio" used in literature and in software
packages. Please be aware that the various definitions will not necessarily give the same or even comparable results.
References for Tetrahedral Quality Measures
1.
2.
3.
4.
602
(Parthasarathy, 93)
(Knupp, 00)
P. Knupp, Algebraic Mesh Quality Metrics for Unstructured Initial Meshes, to appear in Finite Elements for
Design
and Analysis.
SDRC/IDEAS Simulation: Finite Element Modeling - User's Guide
Metrics for Hexahedral Elements
The metrics used for hexahedral elements in Trelis are summarized in the following table:
Function Name
Dimension
Full Range
Acceptable Range
Reference
Aspect Ratio
L^0
1 to inf
1 to 4
1
Skew
L^0
0 to 1
0 to 0.5
1
Taper
L^0
0 to +inf
0 to 0.4
1
Element Volume
L^3
-inf to inf
None
1
Stretch
L^0
0 to 1
0.25 to 1
2
Diagonal Ratio
L^0
0 to 1
0.65 to 1
3
Dimension
L^1
0 to inf
None
1
Condition No.
L^0
1 to inf
1 to 8
5
Jacobian
L^3
-inf to inf
None
5
Scaled Jacobian
L^0
-1 to +1
0.5 to 1
5
Shear
L^0
0 to 1
0.3 to 1
5
Shape
L^0
0 to 1
0.3 to 1
5
Relative Size
L^0
0 to 1
0.5 to 1
5
Shear & Size
L^0
0 to 1
0.2 to 1
5
Shape & Size
L^0
0 to 1
0.2 to 1
5
Distortion
L^0
0 to 1
0.6 to 1
6
Hexahedral Quality Definitions
Aspect Ratio: Maximum edge length ratios at hex center.
Skew: Maximum |cos A| where A is the angle between edges at hex center.
Taper: Maximum ratio of lengths derived from opposite edges.
603
Trelis 15.0 User Documentation
Element Volume: Jacobian at hex center.
Stretch: Sqrt(3) * minimum edge length / maximum diagonal length.
Diagonal Ratio: Minimum diagonal length / maximum diagonal length.
Dimension: Pronto-specific characteristic length for stable time step calculation. Char_length = Volume / 2 grad Volume.
Condition No. Maximum condition number of the Jacobian matrix at 8 corners.
Jacobian: Minimum pointwise volume of local map at 8 corners & center of hex.
Scaled Jacobian: Minimum Jacobian divided by the lengths of the 3 edge vectors.
Shear: 3/Mean Ratio of Jacobian Skew Matrix
Shape: 3/Mean Ratio of weighted Jacobian Matrix
Relative Size: Min(J, 1/J), where J is the determinant of weighted Jacobian matrix
Shear & Size: Product of Shear and Size Metrics
Shape & Size: Product of Shape and Size Metrics
Distortion: {min(|J|)/actual volume}*parent volume, parent volume = 8 for hex
References for Hexahedral Quality Measures
1.
2.
3.
4.
5.
6.
604
(Taylor, 89)
FIMESH code
Unknown
(Knupp, 00)
P. Knupp, Algebraic Mesh Quality Metrics for Unstructured
Initial Meshes, to appear in Finite Elements for Design
and Analysis.
SDRC/IDEAS Simulation: Finite Element Modeling - User's Guide
Mesh Quality Command Syntax
To view the quality of a mesh
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Mesh.
Click on Volume or Surface.
Click on the Quality action button.
Select Quality Metrics from the drop-down menu.
Enter the appropriate value for Volume ID(s) or Surface ID(s). This can also be done using the Pick Widget
function.
Specify the Quality Metric type to view from the Quality Metric drop-down menu.
Select Display Graphical Summary.
Click Apply.
Quality {geom_and_mesh_list} [metric name] [quality options] [filter options]
Where the list contains surfaces and volumes and groups that have been meshed with faces, triangles, hexes, and
tetrahedra; the list can also specify individual mesh entities or ranges of mesh entities.
If a specific metric name is given, only that metric or metrics are computed for the specified entities. Note that the metric
given must be one which applies to the given entities. To see a list of quality metrics for individual entities see the Mesh
Quality Assessment section and select the desired entity type: hexahedral, tetrahedral, quadrilateral, triangle. or edge
The metric name can also be more general than a specific metric. Four generalized options for metric name can be used:
Allmetrics: All of the metrics corresponding to the element type of the geom_and_mesh_list will be computed and
reported.
Algebraic: All algebraic metrics corresponding to the element type of the geom_and_mesh_list will be computed and
reported (e.g., Shape, Shear, Relative Size).
Robinson: All Robinson metrics corresponding to the element type of the geom_and_mesh_list will be computed and
reported (e.g., Aspect Ratio, Skew, Taper).
Traditional: All the traditional Trelis metrics corresponding to the element type of the geom_and_mesh_list will be
computed and reported (e.g., area, volume, angle, stretch, dimension).
If no metric name is supplied, the default metric is "Shape".
Quality Options
The quality options are:
Scope
[ Global | Individual ]
If the user specifies individual, one quality summary is generated for each entity specified on the command line. If the
user specifies global, or specifies neither, then one quality summary is generated for each mesh element type.
Draw
[ Draw [Histogram] [Mesh] [Monochrome] [Add] ]
605
Trelis 15.0 User Documentation
If the user specifies draw histogram, then histograms are drawn in a separate graphics window. The window contains
one histogram for each quality metric. If the user specifies draw mesh, then the mesh elements are drawn in the default
graphics window. A color-coded scale will appear in the graphics window. The histogram and mesh graphics are color
coded by quality: a small metric value corresponds to red, a large metric value to blue and in-between values according to
the rainbow. You can grab the side of color bar and resize it. The text gets smaller as the color bar width decreases. You
can also grab in the middle of the color bar and move it around. It can be repositioned to the bottom or top and it will
automatically change orientations. See Figure 1.
Figure 1. Quality Scale
If monochrome is specified, then the graphics are not color-coded. If add is specified, then the current display is not
cleared before drawing the mesh elements.
List
[ List [Detail] [Id] [Verbose Errors] ] [Geometry]
If the user specifies List, then the quality data is summarized in text form. List Detail lists the mesh elements by
ascending quality metric. List Id lists the ids of the mesh elements. If Verbose Errors is specified, then details about
unacceptable quality elements are printed out above the summaries. If Geometry is specified, then a list of the geometric
entities that own the elements will be printed.
Filter
There are several options available to filter the output of the quality command, using the following filter options :
606
Mesh Quality Command Syntax
[High <value>] [Low <value>]
Discards elements with metric values above or below value; either or both can be used to get elements above or below a
specified value or in a specified range.
[Top <number>] [Bottom <number>]
Keeps only number elements with the highest or lowest metric values. For example, " Quality hex all aspect ratio top 10
" would request the elements with the 10 highest values of the aspect ratio metric.
607
Mesh Quality Example Output
The typical summary output from the command quality surface 24 is shown in Figure 1. Figure 2 shows the
corresponding histogram. The colored element display resulting from the command quality surface 1 draw `Skew' is
shown Figure 3. A color legend is also printed to the console as shown in Figure 4.
Figure 1. Typical Summary for a Quality Command
609
Trelis 15.0 User Documentation
Figure 2. Histogram output from command "Quality Surface 24 Draw Histogram"
Figure 3. Graphical output of quality metric for command "Quality Surface 24 Skew Draw Mesh"
Figure 4. Legend for command "Quality Surface 1 Skew Draw Mesh"
610
Automatic Mesh Quality Assessment
Trelis performs an automatic calculation of mesh quality which warns users when a particular meshing scheme or other
meshing operation has created a mesh whose quality may be inadequate. These warnings are supplied in case the user
forgets to manually check the mesh quality.
Trelis automatically calculates the SHEAR quality of hexahedral and quadrilateral elements and the SHAPE quality of
tetrahedral and triangular elements. The SHEAR metric measures element skew and ranges between zero and one with a
value of zero signifying a non-convex element, and a value of one being a perfect, right-angled element. The SHAPE
metric also ranges between zero and one with a value of zero signifying a degenerate or inverted element and a value of
one signifying a perfect, equilateral element. The quality of the mesh is then defined to be the minimum value of the shear
metric for hexahedral and quadrilateral elements and the shape metric for tetrahedral and triangular elements, with the
minimum taken over the elements in the mesh.
If the quality of the mesh is zero, the code reports "ERROR: Negative Jacobian Element Generated" to the command
window. By default, if the quality of the mesh is positive but less than a certain threshold, the code reports "WARNING:
Poorly-Shaped Element Generated" to the command window. Also reported in this case is the ID of the offending element,
the value of its shear (or shape) metric, and the value of the threshold to which it was compared. The default value of the
threshold parameter is 0.2. Users may change the threshold value by issuing the command
Set Quality Threshold <double=0.2>
The user may also change what type of message is printed in the case of a poor quality, but positive Jacobian mesh. This
message can be printed as a warning (the default) or an error or can be turned off completely using the command
Set Print Quality { WARNING|Error|Off }
The above commands only affect the message generated for meshes with a quality greater than zero and less than the
given threshold value; an error will always be generated for meshes with a quality of zero (that is, for meshes containing
negative Jacobian elements).
611
Controlling Mesh Quality
If the quality of a model after meshing isn't acceptable, there are two options available to improve that quality. The user
can ask for more smoothing, or delete the mesh and start over. There are some commands that the user can invoke
before meshing the model which can help to improve mesh quality. Some of them are discussed here.
Skew Control
The philosophy behind the skew control algorithm is one of subdividing surfaces into blocky, four-sided areas which can
be easily mapped. The goal of this subdivide-and-conquer routine is to lessen the skew that a mesh exhibits on
submapped regions. By controlling the skew on these surfaces, the mesh of the underlying volume will also demonstrate
less skew.
To control skew or delete skew control
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Surface.
Click on the Control Skew action button.
Select Control Skew or Delete Control Skew from the drop-down menu.
Enter the appropriate value for Surface ID(s). This can also be done using the Pick Widget function.
Click Apply.
Control Skew Surface <surface_id_range> [Individual]
Delete Skew Control Surface {surface_list} [Propagate]
The keyword Individual is deprecated. Its purpose is to specify that surfaces should be processed without regards to the
other surfaces in the given list. This is not necessary, and could lead to problems with the final mesh. When the command
is entered, the algorithm immediately processes the surfaces, inserting vertices and setting interval constraints on the
resulting subdivided curves. In this way, the mesh is more constrained in its generation, and the resulting skew on the
model can be lessened. The only surfaces that can utilize this algorithm are those that lend themselves to a structured
meshing scheme, although future releases might lessen this restriction.
The user also has the ability to delete the changes that the skew control algorithm has made. This is done by using the
delete skew control command.
When the user requests the deletion of the skew control changes on a given surface, every curve on that surface will have
the skew control changes deleted, even if a given curve is shared with another surface on which skew control was
performed. If the user wishes to propagate the deletion of skew control to all surfaces which are affected by one (or more)
particular surfaces, the keyword propagate should be used.
Propagate Curve Bias
When a bias mesh scheme is applied to a curve, this sometimes creates skewing of the surface mesh that is attached.
Sometimes the user will want to ensure that the same bias is applied to curves on attached surfaces so that this skewing
is minimized.
To propagate curve bias
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh and then Curve.
Click on the Mesh action button.
Enter the appropriate value for Select Curves. This can also be done using the Pick Widget function.
Select Bias from the first drop-down menu.
Select Propagate Curve Bias from the second drop-down menu.
Select Volume, Surface or Group from the third drop-down menu and enter the appropriate settings.
Click Apply and then Mesh.
Propagate Curve Bias [Surface|Volume|Body|Group <id_list>]
This command will search out all simply mappable surfaces in the input list, find which curves of those have a bias
scheme set, and will propagate that bias across the mappable surfaces.
613
Trelis 15.0 User Documentation
Adjust Boundary
To adjust a boundary
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Surface.
Click on the Adjust Boundaries action button.
Enter the appropriate value for Surface ID(s). This can also be done using the Pick Widget function.
Enter the appropriate value for Angle.
Click Apply.
Adjust Boundary {Surface|Group} <id_range> [Angle <double>]
This command can be used to improve element quality for mapped or submapped surface meshes. Often, due to vertex
positions, the curve meshing for a surface will lead to a poor quality surface mesh. This command can be used to adjust
the curve meshes in an attempt to generate a better quality surface mesh. The command works by looking at the angle
the mesh edges leave the boundary. In a perfect mapped or submapped mesh, the mesh edges will be orthogonal to the
boundary, or will go off at 90 degree angles. The adjust boundary command looks at the deviation of the mesh edges, and
if it is greater than the prescribed angle deviation, it will move the node location such that it is 90 degrees, if possible. The
deviation angle by default is 5 degrees and can be changed by the user through the [Angle <double>] option in the
command. In order to modify the curve meshes, the surface meshes are first deleted then later remeshed after the curve
meshes have been repositioned and fixed. This command assumes that the volumes attached to the surface have not
been meshed, if they have been, the command will return an error message. It should be noted that this command, while
useful, may not always work due to interval constraints (i.e., you may need to change the intervals on the surface), or if
the surfaces are not very blocky.
614
Coincident Node Check
The ability to check for coincident nodes in the model is available in Trelis. It uses an efficient octal hash tree to make the
comparisons.
To check for coincident nodes
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh.
Click on Volume, Surface, Curve, Vertex or Group.
Click on the Quality action button.
Select Coincidence Check from the drop-down menu.
Select Coincident Nodes from the Type of Coincidence Check menu.
Enter the appropriate settings.
Click Apply.
Quality Check Coincident Node [ In ] [Group|Body|Volume|Surface|Curve|Vertex <id_range> ] [ Merge
[Delete] ] [ HIGHLIGHT|Draw [color <number>]] [List] [Into Group [names|id] ]
If no entity list is given, the command works on all the nodes in the model. If an entity list is given, then it compares the
nodes on those entities with the rest of the nodes in the model. By default the command highlights the coincident nodes in
the graphics window and lists the total number of coincident nodes found. You can also have it clear the graphics and
draw the nodes, and/or list the coincident node ids. Optionally, the coincident nodes found can be placed in a group.
If the model being operated on is from an imported universal file (i.e., no geometry exists in the model), you can merge
the coincident nodes with the merge option. In this case delete allows you to delete the extra nodes (recommended). If
you do not delete them they are placed into an output group.
You can control the tolerance used to check between nodes with the following setting (default = 1e-8):
set Node Coincident Tolerance [<value>]
615
Mesh Topology Check
To check mesh entities topology
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh.
Click on Hex, Tet, Quad, Tri or Edge.
Click on the Quality action button.
Select Topology Check from the drop-down menu.
Enter the appropriate value. This can also be done using the Pick Widget function.
Click Apply.
Quality Check Topology [[Hex <range>] [Tet <range>] [Face <range>] [Tri <range>]]
If no entity list is given, it will check the entire model. Multiple element types are also allowed. The command checks for
non-manifold boundaries (edges) in the element set entered. For quads and tris the command lists and highlights all
edges that have more than two tris or faces connected.
Figure 1. Topology check for quads and tris
For hexes and tets it looks for edges with two or more elements connected that do not share common faces.
Figure 2. Topology check for hexes and tets
Additional topology checks fall into three categories:
617
Trelis 15.0 User Documentation
•
•
•
- model edges
- coincident nodes
- coincident quadrilateral(faces) or triangles
Model Edge Check
The model edge check will find edges with adjoining quadrilaterals or triangles whose angles between the surface
normals exceed a specified value. The default angle is 40 degrees.
The following commands check for model edges:
To check for model edges on volumes, surfaces and groups
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh.
Click on Volume, Surface or Group.
Click on the Quality action button.
Select Model Edge Check from the drop-down menu.
Enter the appropriate values for Volume ID(s), Surface ID(s) or Group ID(s). This can also be done using the
Pick Widget function.
Enter the appropriate settings.
Click Apply.
Topology check model edge {group|volume|surface|curve} <id_range> [angle <value>]
DRAW|nodraw|highlight] [BRIEF|verbose] [RESULT GROUP[{<name>|{<id>}|nogroup]
To check for model edges on blocks, sidesets and nodesets
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Analysis Groups and Materials.
Click on Nodeset, Sideset or Block.
Click on the Manage action button.
Select Model Edge Check from the drop-down menu.
Enter the appropriate values for Nodeset ID(s), Sideset ID(s) or Block ID(s). This can also be done using the
Pick Widget function.
Enter the appropriate settings.
Click Apply.
Topology check model edge {block|sideset|nodeset} <id_range> [angle <value>] DRAW|nodraw|highlight]
[BRIEF|verbose] [RESULT GROUP[{<name>|{<id>}|nogroup]
To check for model edges on hexes, tets, quads/faces, tris or edges
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh.
Click on Hex, Tet, Quad, Trior Edge.
Click on the Quality action button.
Select Model Edge Check from the drop-down menu.
Enter the appropriate values for Hex ID(s), Tet ID(s), Quad ID(s), Tri ID(s)or Edge ID(s). This can also be
done using the Pick Widget function.
Enter the appropriate settings.
Click Apply.
Topology check model edge {hex|tet|face|tri|edge} <id_range> [angle <value>] DRAW|nodraw|highlight]
[BRIEF|verbose] [RESULT GROUP[{<name>|{<id>}|nogroup]
The optional angle parameter allows the user to specify a custom angle value against which the check will be performed.
The default angle is 40 degrees.
By default, the command will draw the model edges.
618
Mesh Topology Check
By default, very little information is output to the command line. The optional verbose parameter will output a list of the
flagged model edges.
By default, the model edges will be written to the group ‘model_edges’. Optionally, the user may specify no grouping, or
the user may specify the name or id of an existing group into which the model edges will be written. The contents of the
existing group will be replaced by the model edges.
Interface Checks
Trelis will verify the interfaces between sections of a model. The existence of coincident nodes, for example, may not
necessarily be an error in the model if the nodes are in sliding contact or are constrained by some type of multi-point
constraint. The existence of coincident quadrilaterals or triangles may indicate that the model is not correctly joined.
To check for coincident nodes.
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Node.
Click on the Quality action button.
Select Coincidence Chenck from the drop-down menu.
Select Coincident Nodes, Coincident Quadrilaterals/Faces or Coincident Triangles.
Enter the appropriate settings.
Click Apply.
Topology check coincident node {group|volume|surface|curve|vertex} <id_range> [tolerance <value>]
DRAW|nodraw|highlight] [BRIEF|verbose] [RESULT GROUP[{<name>|{<id>}|nogroup]
Topology check coincident node {block|sideset|nodeset} <id_range> [tolerance <value>]
DRAW|nodraw|highlight] [BRIEF|verbose] [RESULT GROUP[{<name>|{<id>}|nogroup]
Topology check coincident node {hex|tet|face|tri|edge|node} <id_range> [tolerance <value>]
DRAW|nodraw|highlight] [BRIEF|verbose] [RESULT GROUP[{<name>|{<id>}|nogroup]
The optional tolerance parameter allows the user to specify a custom tolerance value against which the check will be
performed. The default tolerance is 1.0 e-6.
The default group name is ‘coincident_nodes.’
All other options behave similarly to those described above under Model Edge Check.
To check for coincident quadrilaterals.
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Quad.
Click on the Quality action button.
Select Coincidence Chenck from the drop-down menu.
Select Coincident Nodes, Coincident Quadrilaterals/Faces or Coincident Triangles.
Enter the appropriate settings.
Click Apply.
Topology check coincident quad {group|volume|surface} <id_range> [tolerance <value>]
DRAW|nodraw|highlight] [BRIEF|verbose] [RESULT GROUP[{<name>|{<id>}|nogroup]
Topology check coincident quad {block|sideset|nodeset} <id_range> [tolerance <value>]
DRAW|nodraw|highlight] [BRIEF|verbose] [RESULT GROUP[{<name>|{<id>}|nogroup]
Topology check coincident quad {hex|tet|face} <id_range> [tolerance <value>] DRAW|nodraw|highlight]
[BRIEF|verbose] [RESULT GROUP[{<name>|{<id>}|nogroup]
The default group name is ‘coincident_quads.’
All other optional parameters behave similarly to those described above.
To check for coincident triangles.
619
Trelis 15.0 User Documentation
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Tri.
Click on the Quality action button.
Select Coincidence Chenck from the drop-down menu.
Select Coincident Nodes, Coincident Quadrilaterals/Faces or Coincident Triangles.
Enter the appropriate settings.
Click Apply.
Topology check coincident tri {group|volume|surface} <id_range> [tolerance <value>]
DRAW|nodraw|highlight] [BRIEF|verbose] [RESULT GROUP[{<name>|{<id>}|nogroup]
Topology check coincident tri {block|sideset|nodeset} <id_range> [tolerance <value>]
DRAW|nodraw|highlight] [BRIEF|verbose] [RESULT GROUP[{<name>|{<id>}|nogroup]
Topology check coincident tri {hex|tet|face|tri} <id_range> [tolerance <value>] DRAW|nodraw|highlight]
[BRIEF|verbose] [RESULT GROUP[{<name>|{<id>}|nogroup]
The default group name is ‘coincident_tris.’
All other optional parameters behave similarly to those described above.
620
Centroid Area Pull
Applies to: Surface Meshes
Summary: Attempts to create elements of equal area
To create elements of equal area
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Surface.
Click on the Smooth action button.
Select Centroid Area from the drop-down menu.
Enter in the appropriate values for Surface ID(s). This can also be done using the Pick Widget function.
Click Apply.
Surface <range> Smooth Scheme Centroid Area Pull [Free]
Discussion:
This smooth scheme attempts to create elements of equal area. Each node is pulled toward the centroids of adjacent
elements by forces proportional to the respective element areas (Jones, 74).
621
Equipotential
Applies to: Volume Meshes
Summary: Attempts to equalize the volume of elements attached to each node
To use edge length smoothing
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Volume.
Click on the Smoothing action button.
Select Equipotential from the drop-down menu.
Enter in the appropriate values for Volume ID(s). This can also be done using the Pick Widget function.
Optionally, select Specify Tolerance to set a specific Tolerance value.
Click Apply.
Volume <range> Smooth Scheme Equipotential [Free]
Discussion:
This smoother is a variation of the Equipotential (Jones, 74) algorithm that has been extended to manage non-regular
grids (Tipton, 90). This method tends to equalize element volumes as it adjusts nodal locations. The advantage of the
equipotential method is its tendency to "pull in" badly shaped meshes. This capability is not without cost: the equipotential
method may take longer to converge or may be divergent. To impose an equipotential smooth on a volume, each element
must be smoothed in every iteration--a typically expensive computation. While a Laplacian method can complete
smoothing operations with only local nodal calculations, the equipotential method requires complete domain information to
operate.
623
Laplacian
Applies to: Curve, Surface, and Volume meshes
Summary: Tries to make equal edge lengths
To use laplacian smoothing
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh.
Click on Volume, Surface or Curve.
Click on the Smoothing action button.
Select Laplacian from the drop-down menu.
Enter in the appropriate values for Volume ID(s), Surface ID(s) or Curve ID(s). This can also be done using
the Pick Widget function.
Optionally, select Specify Tolerance to set a specific Tolerance value.
Click Apply.
{Surface|Volume} <range> Smooth Scheme Laplacian [Free] [Global]
Discussion:
The length-weighted Laplacian smoothing approach calculates an average element edge length around the mesh node
being smoothed to weight the magnitude of the allowed node movement (Jones, 74). Therefore this smoother is highly
sensitive to element edge lengths and tends to average these lengths to form better shaped elements. However, similar to
the mapping transformations, the length-weighted Laplacian formulation has difficulty with highly concave regions.
Currently, the stopping criterion for curve smoothing is 0.005, i.e., nodes are no longer moved when smoothing moves the
node less than 0.005 * the minimum edge length. The maximum number of smoothing iterations is the maximum of 100
and the number of nodes in the curve mesh. Neither of these parameters can currently be set by the user.
Using the global keyword when smoothing a group of surfaces will allow smoothing of mesh on shared curves to improve
the quality of elements on both surfaces sharing that curve.
625
Smart Laplacian
Applies to: Surface and Volume meshes
Summary: Tries to make equal edge lengths while ensuring no degradation in element shape
To use smart laplacian smoothing
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh.
Click on Volume or Surface.
Click on the Smoothing action button.
Select Smart Laplacian from the drop-down menu.
Enter in the appropriate values for Volume ID(s) or Surface ID(s). This can also be done using the Pick
Widget function.
Click Apply.
{Surface|Volume} <range> Smooth Scheme Smart Laplacian
Discussion:
The Smart Laplacian smoothing approach is a variation on the standard Laplacian algorithm. The algorithm iteratively
loops over the mesh and updates nodes based on the location of their neighbors. First, a patch of elements is formed
around a given node. The quality of this patch is assessed to determine the quality of the worst shaped element. Then a
new candidate node position is calculated as the average of the neighboring nodes. The quality of the patch is assessed
again using the candidate node position. If there has been no degradation in the quality of the elements in the patch, the
candidate node position is accepted; otherwise, the candidate node position is rejected and the node is returned to its
previous position.
The Smart Laplacian smoother is intended to provide a reliable smoother that is nearly as fast as the Length-Weighted
Laplacian smoother. Due to the dual goals of this smoother, making equal edge length and improving element shape, it
will not always be able to make progress. However, it is often useful as a quick alternative to the more time-consuming
optimization methods like Mean Ratio or Condition Number. When this smoother fails to make significant progress, the
optimization methods can be tried.
The Smart Laplacian Smoother uses the Mean Ratio quality measure to assess element shape. This smoother is ensuring
no degradation in the minimum Mean Ratio. The Mean Ratio smoother is optimizing the same metric, but it is attempting
to improve the average Mean Ratio quality.
627
Condition Number
Applies to: Triangular or Quadrilateral Surface Meshes, Tetrahedral or Hexahedral Volume Meshes. Does not apply to
Mixed Element Meshes.
Summary: Optimizes the mesh condition number to produce well-shaped elements.
To use the condition number smoother
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Surface.
Click on the Smooth action button.
Select Condition Number from the drop-down menu.
Enter in the appropriate values for Surface ID(s). This can also be done using the Pick Widget function.
Enter in the appropriate settings for Condition Number and Time (minuetes).
Click Apply.
Surface <surface_id_range> Smooth Scheme Condition Number [beta <double=2.0>] [cpu
<double=10>]
Related Commands:
Untangle
Discussion:
The condition number smoother is designed to be the most robust smoother in Trelis because it guarantees that if the
initial mesh is non-inverted then the smoothed mesh will also be non-inverted. The price exacted for this capability is that
this smoother is not as fast as some of the other smoothers.
Condition Number measures the distance of an element from the set of degenerate (non-convex or inverted) elements.
Optimization of the condition number increases this distance and improves the shape quality of the elements. Condition
number optimization requires that the given mesh contain no negative Jacobians. If the mesh contains negative Jacobians
and this command is issued, Trelis automatically calls the Untangle smoother and attempts to remove the negative
Jacobians. If successful, condition number smoothing occurs next; the resulting mesh should have no negative Jacobians.
If untangling is unsuccessful, condition number smoothing is not performed.
There is no "fixed/free" option with this command; boundary nodes are always held fixed.
The command above only sets the smoothing scheme; to actually smooth the mesh one must subsequently issue the
command "smooth surface <surface_id_range>" or "smooth volume <volume_id_range>".
Stopping Criteria: Smoothing will proceed until the objective function has been minimized or until one of two user input
stopping criteria are satisfied. To input your own stopping criterion use the optional parameters 'beta' and 'cpu' in the
command above. The value of beta is compared at each iteration to the maximum condition number in the mesh. If the
maximum condition number is less than the value of beta, the iteration halts. In Trelis condition number ranges from 1.0 to
infinity, with 1.0 being a perfectly shaped element. Thus the smaller the maximum condition number, the better the mesh
shape quality. The default value of the beta parameter is 2.0. The value supplied for the "cpu" stopping criterion tells the
code how many minutes to spend trying to optimize the mesh. The default value is 10 minutes. Optimization may also be
halted by using "control-C" on your keyboard.
To view a detailed report of the smoothing in progress issue the command "set debug 91 on" prior to smoothing the
surfaces or volumes. You will get a synopsis of whether or not untangling is needed first and whether the stopping criteria
have been satisfied. In addition the following printout information is given for each iteration of the conjugate gradient
numerical optimization:
Iteration=n, Evals=m, Fcn=value1, dfmax=value2, time=value3 ave_cond=value4,
max_cond=value5, min_jsc=value6
n is the iteration count, m is the number of objective function evaluations performed per iteration, value1 is the value of
the objective function (this usually decreases monotonically), value2 is the norm of the gradient (does not always
decrease monotonically), and value3 is the cumulative cpu time (in seconds) spent up to the current iteration. The
minimum possible value of the objective function is zero but this is attained only for a perfect mesh. ave_cond,
max_cond, and min_jsc are the average and maximum condition number, and the minimum scaled jacobian. ave_cond
generally decreases monotonically because it is directly related to value1.
629
Trelis 15.0 User Documentation
630
Mean Ratio
Applies to: Triangular or Quadrilateral Surface Meshes, Tetrahedral or Hexahedral Volume Meshes. Does not apply to
Mixed Element Meshes.
Summary: Moves interior mesh nodes to optimize the average mean ratio metric value of the mesh.
To use mean ratio smoothing
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh.
Click on Volume or Surface.
Click on the Smoothing action button.
Select Mean Ratio from the drop-down menu.
Enter in the appropriate values for Volume ID(s) or Surface ID(s). This can also be done using the Pick
Widget function.
Enter the appropriate value for Time (minutes).
Click Apply.
Surface <surface_id_range> Smooth Scheme Mean Ratio [cpu <double=10>]
Volume <volume_id_range> Smooth Scheme Mean Ratio [cpu <double=10>]
Discussion:
Trelis includes a mean ratio smoother provided by MESQUITE, a mesh optimization toolkit by Argonne National
Laboratory and Sandia National Laboratories. (See Brewer, et al. 2003 for more details on the MESQUITE toolkit.) This
smoother is similar in purpose to the Condition Number smoother. However, the Mean Ratio smoother uses a second
order optimization method, and therefore it will often reach a near-optimal mesh more quickly than the Condition Number
smoother. The Mean Ratio smoother requires the initial mesh to be untangled, but the smoother is guaranteed to not
tangle the mesh. If the user attempts to call the Mean Ratio smoother on a tangled mesh, an untangler will first attempt to
untangle the mesh before calling the Mean Ratio smoother.
The Mean Ratio smoother's optimization process terminates when one of the following three criteria is met:
1.
2.
3.
The mesh is "close" to an optimal mesh configuration.
The maximum allotted time has been exceeded.
The user interrupts the smoothing process.
The user has control over the second and the third criteria only. For criterion 2, the default is for the smoother to terminate
after ten minutes even if a near-optimal mesh has not been reached. The user can change this time bound by specifying
the optional "cpu" argument in the command listed above. This argument takes a single, positive number that represents
the time (in minutes) that will be used as a time bound. If the user wishes to terminate the process early, criteria three
allows the user to "interrupt" (for example, on some platforms, by pressing CTRL-C) the process. If the process is
terminated early, the mesh will not revert to the original node positions; Trelis will instead keep the partially optimized
mesh.
631
Winslow
Applies to: Surface meshes
Summary: Elliptic smoothing technique for structured and unstructured surface meshes
To use winslow smoothing
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Surface.
Click on the Smooth action button.
Select Winslow from the drop-down menu.
Enter the appropriate values for Surface ID(s). This can also be done using the Pick Widget function.
Click Apply.
Surface <range> Smooth Scheme Winslow [Free]
Discussion:
Winslow elliptic smoothing (Knupp, 98) is based on solving Laplaces equation with the independent and dependent
variables interchanged. The method is widely used in conjunction with the mapping and submapping methods to give
smooth meshes with positive Jacobians, even on non-convex two-dimensional regions. The method has been extended in
Trelis to work on unstructured meshes.
633
Untangle
Applies to: Triangular or Quadrilateral Surface Meshes Tetrahedral or Hexahedral Volume Meshes. Does not apply to
Mixed Element Meshes.
Summary: Removes as many negative Jacobians from the mesh as possible by minimizing a certain objective function.
To use untangle smoothing
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh.
Click on Volume or Surface.
Click on the Smoothing action button.
Select Untangle from the drop-down menu.
Enter in the appropriate values for Volume ID(s) or Surface ID(s). This can also be done using the Pick
Widget function.
Enter the appropriate values for Scaled Jacobian and Time (minutes).
Click Apply.
Surface <surface_id_range> Smooth Scheme Untangle [beta <double=0.02>] [cpu <double=10>]
Volume <volume_id_range> Smooth Scheme Untangle [beta <double=0.02>] [cpu <double=10>]
Related Commands:
Condition Number
Discussion:
The Untangle 'smoother' is designed to eliminate negative Jacobians from a given mesh by moving nodes to appropriate
locations. If a mesh node is not involved in causing a negative Jacobian it will not be moved. If a mesh has no negative
Jacobians, the Untangler will not move any of the nodes. This smoother is not magic: if an untangled mesh does not exist
for the given mesh topology, the untangler will not untangle the mesh. Instead, it will do the best it can and exit gracefully.
An untangled mesh produced by this smoother will often have poor shape quality; in that case it is recommended that
untangling be followed by condition number smoothing. The untangle smoother is automatically called by the condition
number smoother.
There is no "fixed/free" option with this command; boundary nodes are always held fixed. As a result, users should be
aware that the volume untangler cannot succeed if the volume contains a surface mesh which contains a negative
Jacobian. In that case, one must first remove the surface mesh negative Jacobians by invoking the surface Untangler and
then invoke the volume Untangler.
The command above only sets the smoothing scheme; to actually smooth the mesh one must subsequently issue the
command "smooth surface <surface_id_range>" or "smooth volume <volume_id_range>".
Stopping Criteria: Untangling will proceed until the objective function has been minimized or the optional user input "cpu"
has been satisfied. The latter stopping criterion tells the code how many minutes to spend trying to untangle the mesh.
The default value is 10 minutes. Optimization may also be halted by using "control-C" on your keyboard.
Beta Parameter: An optional user input parameter "beta" plays a role in determining the optimal mesh. Optimization
proceeds until the minimum scaled Jacobian of the mesh is (roughly) greater than beta. To remove negative Jacobians
one would need beta=0 (however, as a safety margin, we choose beta=0.02 as the default). To further improve the scaled
Jacobian of the mesh, input a larger value of "beta". If a mesh with all scaled Jacobians greater than "beta" does not exist,
optimization will continue until the cpu time stopping criterion has been met. Therefore, it is best not to use "beta" values
too large (say, greater than 0.2) without also decreasing the cpu time limit.
To view a detailed report of the smoothing in progress issue the command "set debug 91 on" prior to smoothing the
surfaces or volumes. You will get a synopsis of whether or not untangling is needed and whether the stopping criteria are
satisfied. In addition the following printout information is given for each iteration of the conjugate gradient numerical
optimization:
Iteration=n, Evals=m, Fcn=value1, dfmax=value2, time=value3 min_jsc=value4
635
Trelis 15.0 User Documentation
n is the iteration count, m is the number of objective function evaluations performed per iteration, value1 is the value of
the objective function (this usually decreases monotonically), value2 is the norm of the gradient (does not always
decrease monotonically), and value3 is the cumulative cpu time (in seconds) spent up to the current iteration. The
minimum possible value of the objective function is zero; this value is attained only when the minimum scaled Jacobian of
the mesh exceeds "beta". The minimum scaled jacobian is also reported.
636
Edge Length
Applies to: Surfaces
Summary: This smoother tries to make all edge lengths equal
To use edge length smoothing
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Surface.
Click on the Smooth action button.
Select Edge Length from the drop-down menu.
Enter in the appropriate values for Surface ID(s). This can also be done using the Pick Widget function.
Click Apply.
Surface <range> Smooth Scheme Edge Length
Discussion:
Edge Length smoothing in Trelis is provided by MESQUITE, a mesh optimization toolkit by Argonne National Laboratory
and Sandia National Laboratories. (See Brewer, et al. 2003 for more details on the MESQUITE toolkit.) This smooth
scheme may be useful for lengthening the shortest edge length in paved meshes.
Interior node positions are adjusted in an optimization loop where the optimal element has an ideal shape (square) and
has an area equal to the average element area of the input mesh.
NOTE: This smoother should be avoided when the mesh contains high aspect-ratio elements that the user wants to keep.
Because this smoother essentially tries to make all the edge lengths equal, it is designed to work well on meshes whose
elements have aspect ratios close to 1. The farther from 1 the aspect ratio is, the less applicable this smoother will be.
637
Mesh Refinement
•
•
•
•
•
•
•
Global Mesh Refinement
Refining at a Geometric or Mesh Feature
Hexahedral Refinement Using Sheet Insertion
Directional Refinement
Local Refinement of Triangles and Edges
'N' Tets Through the Thickness Refinement
Parallel Refinement
Trelis provides several methods for conformally refining an existing mesh. Conformal mesh refinement does not leave
hanging nodes in the mesh after refinement operations, rather conformal mesh refinement provides transition elements to
the existing mesh. Both local and global mesh refinement operations are provided.
Global Mesh Refinement
The Refine Surface and Refine Volume commands provide capability for globally refining an entire surface or volume
mesh. Global refinement will only be used if the entire body is included in the command. Otherwise, the command will be
interpreted as local refinement (see below.) This distinction can be important because the global refinement algorithm
divides each element into fewer sub-elements than local refinement. The command syntax is:
To refine a volume and surface mesh
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh.
Click on Volume or Surface.
Click on the Refine action button.
Select General Refinement from the drop-down menu.
Enter the appropriate values for Volume ID(s) or Surface ID(s). This can also be done using the Pick Widget
function.
Enter the appropriate settings for Refinement Condition and Refinement Boundary.
Click Apply.
Refine Volume <range>numsplit<int>
Refine Surface <range>numsplit<int>
The numsplit option specifies how many times to subdivide an element. A value of 1 will split every triangle and
quadrilateral into four pieces, and every tetrahedron and hexahedron into eight pieces. Examples of global refinement on
each element are shown below.
original mesh
NumSplit = 1
NumSplit = 2
639
Trelis 15.0 User Documentation
original mesh
NumSplit = 1
NumSplit = 2
original mesh
NumSplit = 1
NumSplit = 2
original mesh
NumSplit = 1
NumSplit = 2
Figure 1. Example of uniform refinement for each of the mesh entities
Refining at a Geometric or Mesh Feature
Trelis also provides methods for local refinement around geometric or mesh features. Individual elements or groups of
elements can be refined in this manner using the following syntax.
To refine mesh entities
1.
2.
3.
4.
5.
6.
7.
640
On the Command Panel, click on Mesh.
Click on Hex, Tet, Quad, Tri, Edge or Node.
Click on the Refine action button.
Select General Refinement from the drop-down menu.
Enter the appropriate values for Hex ID(s), Tet ID(s), Quad ID(s), Tri ID(s), Edge ID(s) or Node ID(s). This can
also be done using the Pick Widget function.
Enter the appropriate settings for Refinement Condition and Refinement Boundary.
Click Apply.
Mesh Refinement
Refine {Node|Edge|Tri|Face|Tet|Hex} <range>
[NumSplit<int = 1>|Size <double> [Bias <double>]]
[Depth <int>|Radius <double>] [Sizing_Function]
[Smooth]
To refine geomentric entities
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh.
Click on Surface, Curve or Vertex.
Click on the Refine action button.
Select General Refinement from the drop-down menu.
Enter the appropriate values for Volume ID(s) or Surface ID(s). This can also be done using the Pick Widget
function.
Enter the appropriate settings for Refinement Condition and Refinement Boundary.
Click Apply.
Refine {Vertex|Curve|Surface} <range>
[NumSplit<int = 1>|Size <double> [Bias <double>]]
[Depth <int>|Radius <double>] [Sizing_Function]
[Smooth]
To use these commands, first select mesh or geometric entities at which you would like to perform refinement.
Refinement will be applied to all mesh entities associated with or within proximity of the entities. The all keyword may be
used to uniformly refine all elements in the model
The following is a description of refinement options.
NumSplit
Defines the number of times the refinement operation will be applied to the elements in the refinement region. For uniform
or global refinement, where all elements in the model are to be refined, A NumSplit value of 1 will split each triangle and
quadrilateral into four elements, and each tetrahedron and hexahedraon into eight elements. A numsplit of 2 would result
in 16 and 64 elements respectively. For uniform refinement, the total number of elements obeys the following:
1.
NE = NI * E^NumSplit
where NE is the final number of elements, NI is the initial number of elements and E is 4 or 8 for 2D and 3D elements
respectively.
In cases where only a portion of the elements are selected for refinement, the elements at the boundary between the
refined and non-refined elements will be split to accomodate a transition in element size. The transition pattern will vary
depending on the local features and surrounding elements. For non-uniform refinement of hexahedron, for a numsplit of 1,
each element in the uniform refinement zone will be subdivided into 27 (E=27) elements rather than 8. This affords
greater flexibility in transitioning between the refined and unrefined elements.
Size, Bias
The Size and Bias options are useful when a specific element size is desired at a known location. This might be used for
locally refining around a vertex or curve. The Bias argument can be used with the Size option to define the rate at which
the element sizes will change to meet the existing element sizes on the model. Figure 2 shows an example of using the
Size and Bias options around a vertex. Valid input values for Bias are greater than 1.0 and represent the maximum
change in element size from one element to the next. Since refinement is a discrete operation, the Size and Bias options
can only approximate the desired input values. This may cause apparent discontinuities in the element sizes. Using the
default smooth option can lessen this effect. It should also be noted that the Size option is exclusive of the NumSplit
option. Either NumSplit or Size can be specified, but not both.
641
Trelis 15.0 User Documentation
original mesh
Bias=2.0
Bias=1.5
Figure 2. Example of using the Size and Bias options at a Vertex.
Depth
The Depth option permits the user to specify how many elements away from the specified entity will also be refined.
Default Depth is 1. Figure 3 shows an example of using the depth option when refining at a node.
original mesh
Depth=1
Depth=2
Figure 3. Example of using the Depth option at a node to control how far from the node to propagate the
refinement.
Radius
Instead of specifying the number of elements to describe how far to propagate the refinement, a real Radius may be
entered. The effects of the Radius are similar to that shown in Figure 3, except that the elements whose centroid fall
within the specified Radius will be refined. Transition elements are inserted outside of this region to transition to the
existing elements.
Sizing Function
Refinement may also be controlled by a sizing function. Trelis uses sizing functions to control the local density of a mesh.
Various options for setting up a sizing function are provided, including importing scalar field data from an exodus file. In
order to use this option, a sizing function must first be specified on the surface or volume on which the refinement will be
applied. See Adaptive Meshing for a description of how to define a sizing function.
Smooth
The default mode for refinement operations is to NOT perform smoothing after splitting the elements. In many cases, it
may be necessary to perform smoothing on the model to improve quality. The smooth option provides this capability.
Controlling Regularity of Triangle Refinement
The default behavior of triangle refinement is to attempt to maximize element quality using the basic one->four template.
This can sometimes result in an irregular pattern, where one or more edges are swapped. To enforce regularity of the
triangle refinement pattern, regardless of quality, the folowing setting may be used.
642
Mesh Refinement
1.
Set Triangle Refine Regular {on|OFF}
Hexahedral Refinement Using Sheet Insertion
Several tools for refining a hexahedral mesh using sheet insertion and deletion are available in Trelis.
•
•
•
•
Refining at a Geometric Feature
Refining along a Path
Refining a Hex Sheet
Hex Sheet Drawing
Refining at a Geometric Feature
The following commands offer additional controls on refinement with respect to one or more geometric features of the
model.
An existing hexahedral mesh can be refined at a geometric feature using the following command:
Refine Mesh Volume <id> Feature {Surface | Curve | Vertex | Node} <id_range> Interval <integer>
This command refines the mesh around a given feature by adding sheets of hexes. These sheets can be generalized as
planes for surfaces, cylinders for curves, and spheres for vertices. The interval keyword specifies the number of intervals
away from the feature to insert the new sheet of hexes. For this command a single sheet of hexes is inserted into the
hexahedral mesh.
Figure 4 shows an example of this command where the feature at which refinement is to be performed is a curve. In this
case the interval chosen was, 2. This indicated that the elements 2 intervals away from the curve would be refined.
Figure 4. Example of Refinement at a curve
Refining along a path
Hexahedral meshes can be refined from a specific node and along a propagated path using the following command
Refine Mesh Start Node <id> Direction Edge <id> End Node <id> [Smooth]
643
Trelis 15.0 User Documentation
Figure 5 shows a swept mesh and it's cross section. The cross section view on the left shows a path that has been
propagated through the mesh between the start node and end node. This path is then projected along a chain of edges in
the direction given by the direction edge as shown in Figure 5 . The start node and end node must be on the same sweep
layer. This refinement procedure also requires the volume’s meshing scheme to be set to sweep. If the smooth keyword is
given the mesh will be smoothed after the refinement step is complete.
Figure 5. Refining a Mesh Along a Path
Refining a Hex Sheet
To use mesh sheet refinement to refine the elements in one or more hex sheets
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Volume.
Click on the Refine action button.
Select Mesh Sheet Refinement from the drop-down menu.
Select Node ID(s) or Edge ID and specify the value(s).
Select Factor or Greater Than (size) and specify the value(s).
Click Apply.
Refine Mesh Sheet [Intersect] { Node <id_1> <id_2> | Edge <id_range> } { Factor <double> |
Greater_than <size> } [Smooth] [in volume <id_range> [depth <num_layers]]
The node and edge keywords are used to define the hex sheet(s) to be refined. If the node option is chosen, only one
node pair can be entered (see Figure 6). If the edge option is chosen, one or more edges can be entered (see Figure 7).
Figure 6. Refine mesh sheet node 796 782 greater_than 6
644
Mesh Refinement
Figure 7. Refine mesh sheet edge 1584 1564 1533 1502 1471 greater_than 6
The factor and greater_than keywords are used to specify the refinement criteria for the selected hex sheet(s). If the
factor keyword is used, the length of the smallest edge in the hex sheet is determined and any edge in the hex sheet with
a length greater than the smallest length multiplied by the factor is refined. If the greater_than keyword is used, any edge
in the hex sheet with a length greater than the specified size is refined.
The intersect keyword is optional. It is used to more easily define multiple hex sheets to be refined. If the intersect
keyword is entered, the node and edge keywords are used to define a chord rather than a sheet (a chord is the twodimensional equivalent of the three-dimensional sheet). The chord will be limited to the surface(s) associated with the
nodes or edge entered, and all sheets intersecting the chord will be selected for refinement (see Figure 8). When the node
keyword is used with the intersect option, the nodes must define an edge on the surface of the mesh.
Figure 8. Refine mesh sheet intersect edge 1499 greater_than 6
The smooth keyword is also optional. When the smooth keyword is entered, the elements that have been refined are
smoothed in an attempt to improve element quality. Figure 9 shows the same command as Figure 8 with the addition of
the smooth keyword. Smoothing may or may not be beneficial, depending on the situation.
Figure 9. Refine mesh sheet intersect edge 1499 greater_than 6 smooth
645
Trelis 15.0 User Documentation
Directional Refinement
Mesh sheet refinement can also be used to refine a mesh in a particular direction. This can help control anisotropy. The
following command can be used as a short cut for specifying what sheets should be used in refinement.
Refine Volumes <id_range> using {Plane <options> | Surface <id_range> | Curve <id_range> } [ Depth
<num_layers> ] [ Smooth ]
The volumes specified indicate which hexes can be refined. A transition layer will be made out of hexes surrounding the
indicated volumes. If the depth option is used, additional layers of hexes around the specified volumes will be included in
the refinement region. Behind the using option, if the plane option is employed, all the edges in the volume which are
parallel to the plane (to a small tolerance) are used to specify the sheets to refine. If the surface or curve option is
employed instead, all the edges in the surfaces or curves will be used.
For example, Figure 10 and 11 shows directional refinement using the plane option. Directional refinement can be used
iteratively with sheet dicing to reduce or create anisotropy of any level.
Figure 10. Starting mesh
646
Mesh Refinement
Figure 11. Refine volume 1 using plane xplane depth 1
Figure 12. Refine volume 1 using plane xplane depth 1
647
Trelis 15.0 User Documentation
Hex Sheet Drawing
Since refinement of hex meshes generally occurs by inserting hex sheets, tools have been provided to draw a specified
sheet or group of sheets.
This command draws a sheet of hexes that is defined by the edge or node pair.
Draw Sheet {Edge <id> |Node <id_1> <id_2>}[Mesh [List]] [Color <color_name>] [Gradient]
The following command draws the three sheets that intersect to define the given hex. These sheets are drawn green,
yellow, and red. To draw a specific sheet, list its color in the command.
Draw Sheet Hex <id> [Green][Yellow][Red][Mesh [List]] [Gradient]
The 'gradient' keyword for both commands draws the sheet in gradient shading according to the distance between
opposite hex faces that are parallel to the sheet.
The 'mesh' keyword will draw the hexes in the hex sheet. If the 'list' keyword is also given, the ids of the hexes in the
sheet will be listed.
Local Refinement of Triangles and Edges
Local refinement of triangles and edges is available. When refining triangles a node is inserted at the enter of the triangle
and three new triangles are connected to this node. The original triangle is deleted.
To refine triangles with local refinement
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Tri.
Click on the Refine action button.
Select Local Triangle Refinement from the drop-down menu.
Enter the appropriate value for Triangles to Refine. This can also be done using the Pick Widget function.
Click Apply.
Refine Local Tri <tri_id_list>
When refining an edge, a node splits the original edge between two triangles and four new triangles are created and
connected to the new node.
To refine an edge with local refinement
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Tri.
Click on the Refine action button.
Select Local Edge Refinement from the drop-down menu.
Enter the appropriate value for Edge to Refine. This can also be done using the Pick Widget function.
Click Apply.
Refine Local Edge <edge_id>
When refining a tet edge, the tet edge is split by a node and then all tets attached to the original edge are split into two
through a triangle that goes through the new node. All other adjacent nodes and edges are unmodified by the operation.
Note that on the interior of the mesh tet edges are not represented explicitly so the command takes two nodes as input to
define the edge. The command to refine a tet edge is:
Refine Tet_edge Node <node1_id> <node2_id>
648
Mesh Refinement
'N' Tets Through the Thickness Refinement
Trelis provides a capability to guarantee a user-specified number of tets through the thickness. This functionality is
intended to work on an existing tet mesh using mesh refinement. The user specifies the geometry or mesh defining the
thin region and also the number of desired tets through the thickness and the refinement algorithm will run until it meets
this criteria. The number of tets through the thickness in this context is interpreted as the number of mesh edges through
the thickness and the algorithm will continue to do refinement until there are no mesh edge paths through the thin region
that contain fewer mesh edges than the number specified by the user. The command for doing this is:
Refine min_through_thickness <val> source {surface|node|tri|nodeset|sideset|block} <id_range> target
{surface|node|tri|nodeset|sideset|block} <id_range> [anisotropic] [single_iteration] [dont_fill_in_gaps]
The various options are described below.
anisotropic: When this option is specified in the command the algorithm will only attempt to refine the edges that go
roughly normal to the source and target entities. This will give an anisotropic result. The meshes on the source and target
will generally not be affected when this option is used. When this option is not specified the refinement algorithm will be
isotropic in nature and will propagate much more. However, it will tend to have better transitioning from the refined region
to the non-refined regions.
dont_fill_in_gaps: When this option is specified in the command the algorithm will NOT try to grow the regions that will
be refined. When the regions are grown it helps to avoid leaving small pockets of mesh that are not refined (splotchiness).
This has effect only on isotropic refinement (when the anisotropic option is NOT used).
single_iteration: When this option is specified in the command the algorithm will only run for one iteration even if the
min_through_thickness criteria is not met.
Below is an example using the following commands:
refine min_through_thickness 4 source surf 1 target surf 2 anisotropic
refine min_through_thickness 4 source surf 7 target surf 13 3 14 anisotropic
Surfaces 1 and 2 are the two surfaces on opposite sides of the thin region in the green volume and surfaces 7 13 3 14 are
the surfaces on opposite sides of the thin region in the yellow volume.
649
Trelis 15.0 User Documentation
Before N through the thickness refinement
After N through the thickness refinement
Measuring the Number of Tets through the Thickness
The ability to check the number of tets through the thickness is given with the following command:
Quality Surface <surf1_id><surf2_id> num_thru_thickness
Parallel Refinement
Global mesh refinement can be used to increase global mesh density with a single command. If an extremely large mesh
is desired, one approach is to generate a coarse mesh with the desired relative mesh gradations, and then perform global
mesh refinement to scale the number of elements up across the model. Depending on the amount of refinement
requested, this can exceed the memory limits of Trelis running on a single processor. Global parallel mesh refinement
allows refinement to go beyond the memory limits of a single processor. The resulting mesh size is only limited by the
number of processors you have available to perform the refinement.
To use global mesh refinement
1.
2.
3.
4.
5.
6.
650
On the Command Panel, click on Mesh.
Click on Volume, Surface, Hex, Tet, Quad or Tri.
Select the Refine action button.
Select Global Parallel Refinement from the drop-down menu.
Enter the appropriate settings.
Click Apply.
Mesh Refinement
Refine Parallel [Fileroot <'root filename'>] [Overwrite] [No_geom] [No_execute] [Processors <int>]
[Numsplit <int>] [Version <'Sierra version'>]
This command causes Trelis to write two files to disk. First, Trelis writes an Exodus file named <root filename>.in.e which
contains the mesh elements in the current Trelis session. Second, Trelis writes an OpenNURBS 3dm file
http://www.opennurbs.org. named .3dm, which contains a definition of the geometry from the current Trelis Session. The
Fileroot argument specifies the full path and root of the files that will be written. Additional blocks are written to the
Exodus file to correspond to the geometry entities in the 3dm file. The Overwrite argument specifies if existing files on
disk with the same names should be overwritten or not.
When the mesh is refined in STK_Adapt, the new nodes created during refinement will be projected to the geometry
definitions from the OpenNURBS file. If the No_geom argument is specified, only the Exodus file is written, and new
nodes will be placed by evaluating the shape functions of the elements being evaluated.
The exported Exodus and OpenNURBS files are prepared specifically for input into the Sierra STK_Adapt program. By
default, Trelis spawns STK_Adapt in the background after exporting the files. If the No_execute argument is specified,
the Trelis command exports the files, but does not spawn STK_Adapt. The user can then move those files to a large
parallel machine to perform the STK_Adapt refinement.
If No_execute is not specified, then Trelis will spawn Sierra STK_Adapt in the background to perform the refinement. The
Processors argument specifies the number of processors to use for the STK_Adapt run. The Numsplit argument
specifies how many times the global refinement should be performed. If Numsplit = 1, then each element edge is split
into 2 sub-edges. If Numsplit = 2, then each element is split into 4 sub-edges, etc. The optional Version argument allows
the user to specify which version of STK_Adapt should be run. Possible values for Version include ‘head’, ‘4.22.0’, etc.
Refine parallel command creates groups to visualize the association between mesh entities (edge, tri, and quads ) and
geometric entities (curves & surfaces). There are three types of groups that exist for each mesh entity type edge, tri, and
quad. First group contains unique 1-1 map between mesh entity and geometric entity. Note that issuing "Debug 212"
command before calling the refine parallel command, will create separate group for each geometric entity containing
unique mesh entities. Next group contains mesh entities that point to multiple geometric entities. And the final group
contains mesh entities not associated with any geometric entity.
After the Refine Parallel command finishes, the mesh in Trelis does not change, normally because the resulting mesh
would be too big to store in Trelis on a single processor. Instead, the refined mesh is written to disk in a series of Exodus
files, one per processor, using the Fileroot argument as the root of the Exodus file names. For example, if Fileroot is
‘somemesh’ and Processors is 8, STK_Adapt will write out eight Exodus files named somemesh.e.8.0, somemesh.e.8.1,
…, somemesh.e.8.7. These files can be kept distributed for an analysis run, or united using the Sierra EPU command. In
this example, Trelis would have written out a file called somemesh.in.e, which contains all of the sideset, nodeset, and
block definitions defined in the Trelis session. All of these sidesets, nodesets and blocks are transferred to the refined
exodus files (somemesh.e.8.0, etc.) for use in the subsequent analysis. The somemesh.e.* files will also contain several
other blocks which correspond to geometric entities defined in somemesh.3dm to enable the mesh to be refined to the
CAD geometry, and should be ignored by downstream applications.
Sierra STK_Adapt must be in the PATH on the computer Trelis is running on. If Sierra STK_Adapt cannot be found, Trelis
returns an error and no refinement is performed. Information on how to download and build Sierra STK_Adapt can be
found at http://trilinos.sandia.gov/packages/stk/.
651
Mesh Pillowing
Mesh pillowing is a mesh refinement technique that inserts a layer or 'pillow' of elements around the boundary of an
enclosed mesh. It can be used to improve mesh quality while preserving the outer boundary of the selected element set.
Mesh Pillowing can be used to quickly perform a number of meshing tasks, such as inserting a uniform boundary layer a
specified distance from an outer boundary, or inserting a ring of elements around a hole.
Figure 1: A single hex before (a) and after (b) a pillow operation. The far right (c) depicts a pillow operation with
the front surface designated as a 'through' surface.
During a typical pillow operation, the user selects a set of elements, called a 'shrink set', to define what elements will be
operated on. All elements on the outer boundary of the shrink set are then shrunk towards the center of the set. New
elements are then created to fill the gap between the original boundary and the shrunk boundary. The newly created
elements form the pillow around the selected shrink set. Figure 1a and 1b show an example of a pillow operation
performed on a single hex. Geometry surfaces, or mesh element faces can be specified as through surfaces for the
pillowing operation. This means that the pillow will extend through the selected surfaces, and no new elements will be
created along them. Figure 1c shows the effect of pillowing a single hex with one surface selected as a through surface.
In some cases a shrink set may not be valid due to the geometry of a specific region. As the exterior nodes of the shrink
set move towards the middle they must be able to maintain appropriate geometric associations. Nodes on vertices must
move along curves, nodes on curves must move along surfaces. If there are multiple curves or surfaces along which an
exterior node might travel, then the ownership is ambiguous and the pillowing will fail.
Using the optional distance keyword with a specified value allows manual control of the distance that each boundary
element is shrunk towards the center of the shrink set. If no distance value is specified, an appropriate value is calculated
for each element. If a distance value is specified, all newly created nodes will have their position fixed by default. This
allows the user to smooth the mesh without altering the node positions of the newly created hexes. If the optional
unfix_nodes keyword is used, this default behavior is changed, and any smooth operations will alter the newly created
node locations. By default, a smooth operation is automatically performed following any pillow operation unless the
optional no_smooth keyword is used.
Similar analogous commands are available for creating a pillow around a set of two dimensional faces.
To use mesh pillowing
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh.
Click on Volume, Surface, Curve, Vertex, Hex or Quad.
Click on the Refine action button.
Select Pillowing from the drop-down menu.
Enter the appropriate value for the selected ID. This can also be done using the Pick Widget function.
Enter in any other appropriate settings.
Click Apply.
Pillow Hex <ids> [ Through { [Surface <ids>][Face <ids>][Tri <ids>] } ] [ Distance <value> ] [
Unfix_nodes ] [ No_smooth ]
653
Trelis 15.0 User Documentation
Pillow Face <ids> [ Through Curve <ids> ] [ Distance <value> ] [ Unfix_nodes ] [No_smooth]
Figure 2: Example model using pillow operations to create ordered nodes a specified distance around the
boundary of a mesh.
654
Mesh Coarsening
Hexahedral Coarsening
Trelis provides a limited number of options for coarsening hexahedral meshes. The options currently available for hex
coarsening rely on the hex sheet extraction process described in Mesh Refinement page. Removing a sheet from a
hexahedral mesh essentially means that a complete layer of hexes will be removed and the adjacent layers expanded to
take its place.
Extracting a Single Hex Sheet
The following command can be used to extract a single hex sheet.
Extract sheet { Edge <id> | Node <id_1> <id_2> }
The edge or node pair are used to define the sheet that will be extracted. Figure 3 below shows an example of extracting
a hex sheet. In this example the hex sheet is specified by the node pair highlighted in the images. Note that the entire
layer of hexes between the highlighted nodes has been removed and the neighboring layers have been expanded to take
its place.
Figure 3. Example of Hex Sheet Extraction
Note: Also see the Mesh Refinement section for a description of hex sheet drawing.
Extracting multiple sheets along a curve
Another option for extracting hex sheets can be done by specifying a curve at which to perform the sheet extraction
operations. In this case, multiple layers of hexes can be removed by specifying a curve perpendicular to the hex layers.
The command for coarsening perpendicular to a curve is as follows:
Coarsen Mesh Curve <id> Factor <value> [NO_SMOOTH|smooth]
Coarsen Mesh Curve <id> Remove {<num_edges>|edge <id_ranges>} [NO_SMOOTH|smooth]
655
Trelis 15.0 User Documentation
Figure 4. Coarsening a mesh by extracting sheets perpendicular to a curve
The first option uses the Factor argument. The factor argument controls how much larger the edges will be on the curve.
For example, Figure 4 shows the coarsen mesh curve command used with a factor of 2. In this case, the command
attempts to make the mesh edges approximately twice the length relative to their original length along the curve.
The second option uses the Remove argument. With this option, a specified number of layers may be removed from the
mesh. This may be accomplished by indicating an exact number, or by providing a list of edge IDs that correspond to the
layers that will be removed.
The NO_SMOOTH|smooth option allows the user to improve the element quality after the sheet extraction process by
smoothing the remaining nodes. The default for both of these commands is to not smooth. Smoothing may also be
accomplished after sheet extraction by using the smooth volume command.
Uniform hex coarsening
By applying the coarsen mesh curve command multiple times to curves that are orthogonal in the model, the effect of
uniform coarsening of the mesh may be achieved.
656
Node and Nodeset Repositioning
A capability to reposition nodesets and individual nodes is provided. This capability will retain all the current connectivity of
the nodes involved, but it cannot guarantee that the new locations of the moved nodes do not form intersections with
previously existing mesh or geometry. This capability is provided to allow the user maximum control over the mesh model
being constructed, and by giving this control the user can possible create mesh that is self-intersecting. The user should
be careful that the nodes being relocated will not form such intersections.
The user can reposition nodes appearing in the same nodeset using the NodeSet Move command. Moves can be
specified using either a relative displacement or an absolute position. The command to reposition nodes in a nodeset is:
Nodeset <nodeset_list> Move <delta_x> <delta_y> <delta_z>
The first form of the command specifies a relative movement of the nodes by the specified distances and the second form
of the command specifies absolute movement to the specified position. The third form of the command specifies a
displacement with respect to a specified surface normal.
Individual nodes can be repositioned using the Node Move command. Moves are specified as relative displacements.
To move a node
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Node.
Click on the Move Node action button.
Select Move XYZ from the drop-down menu.
Enter the appropriate value for Node ID(s). This can also be done using the Pick Widget function.
Enter the appropriate values for Delta X, Delta Y and Delta Z or manually move the node by dragging it to the
desired location.
Click Apply.
Note: The constrain to geometry option can be turned off to move the node outside of the geometry.
Node <range> Move <delta_x> <delta_y> <delta_z>
Node <range> Move {[X <val>] [Y <val>] [Z <val>]}
To move normal to surface
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Node.
Click on the Move Node action button.
Select Normal to Surface from the drop-down menu.
Enter the appropriate value for Node ID(s) and Surface ID. This can also be done using the Pick Widget
function.
Enter the appropriate values for Distance.
Click Apply.
Node <range> Move Normal to Surface <id> distance <val>
Nodes can also be repositioned using a location or direction specification. See Location, Direction, and Axis Specification
for details on the location and direction specification. The command syntax is:
Node <range> Move Location <options>
Node <range> Move Direction <options>
See also Transforming Mesh Coordinates.
657
Trelis 15.0 User Documentation
658
Collapsing Mesh Edges
Trelis currently offers several options for modifying an existing finite element mesh. In addition to providing for coarsening
and refining of hexahedral and triangle meshes, Trelis can also reposition nodes by smoothing or by moving individual
nodes.
The collapse edge command is also provided for making small modifications to an existing triangle mesh.
Meshedit Collapse Edge <id>
This command will collapse the two triangles associated with the given edge, effectively removing the triangles from the
mesh. This command only works on surface meshes, and only with triangles. If volumetric elements, or quads, are
attached to the edge, the command does nothing to the mesh.
659
Align Mesh
At times it is desirable to have identical meshes on two different surfaces or curves. The align mesh command will attempt
to assign correspondence between nodes on surfaces or curves and move the nodes on one surface or curve to match
the configuration on the other. The command syntax is:
Align Mesh Surface <id> [CloseTo] Surface <id> [Tolerance <tol>]
Align Mesh Curve <id> [CloseTo] Curve <id> [Tolerance <tol>]
These two commands align the mesh on the first entity with that of the second entity. This means that nodes on the first
entity will be moved to the closest location possible to their corresponding nodes on the second entity. This is done
without regard to mesh quality, so it is possible to invert elements with this command.
Align Mesh Node <id> [CloseTo] Node <id> [Tolerance <tol>]
This command aligns the first node with the second node, within the limits of the geometric entities that own the nodes.
This is also done without respect for element quality.
And example of this is given as follows:
brick x 10
volume 1 copy move 11
surface all except 10 6 vis off
transparent
graphics perspective off
at 5.552503 3.832384 0.134127
from 34.651051 3.640138 -0.193121
up 0.006514 0.999945 -0.008172 mesh surface all
surface 6 smooth scheme randomize free
smooth surface 6
node 432 move 0 0 -0.2
align mesh node 944 node 432
node 432 move 0 0 0.4
align mesh curve 23 closeto curve 12
align mesh surf 10 closeto surf 6
661
Creating and Merging Mesh Elements
The following forms of the create and merge commands operate on meshed entities only. They allow low-level editing of
meshes to make minor corrections to a mostly correct mesh. They are not designed for major modifications to existing
meshes. Because Trelis' display routines were not designed with these type of operations in mind, these commands may
cause the current display of the affected entities to take an unexpected form. An appropriate drawing command can be
used to return the display to the desired view.
The delete commands for deleting individual elements are still under development, but they may be used after setting a
developer flag.
Creating Mesh Elements
The create command uses existing mesh nodes to create new mesh entities.
Creating Hex and Tet Elements
To create hex and tet elements using existing mesh nodes
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh.
Click on Hex or Tet.
Click on the Create action button.
Enter the appropriate value for each Node ID.
Enter the appropriate value for Volume ID. This can also be done using the Pick Widget function.
Click Apply.
Create {Hex|Tet} Node <range> [Owner Volume <id>]
Using the nodes specified, this form of the command creates a new hex or tet that will be owned by the specified volume.
For a hex, 8 nodes are required. The order in which the nodes are specified is very important. They should describe two
opposing faces of the hex; the normal of the first face should point into the hex and the normal of the second face should
point out of the hex. For example, to create the hex shown in Figure 1 below, the following command would be entered:
create hex node 1,2,3,4,5,6,7,8 owner volume 1
663
Trelis 15.0 User Documentation
Figure 1. Node Numbering for the Create Hex command
To create a tet, 4 nodes are specified. The base is specified as a tri with the normal point toward the fourth node using the
right hand rule. To create the tet shown in Figure 2, the following command would be entered:
create tet node 1,2,3,4 owner volume 1
Figure 2. Node ordering for Create Tet Command
664
Creating and Merging Mesh Elements
Creating Wedge Elements
Create Wedge Node <range> [Owner Volume <id>]
To create a wedge, 6 nodes are specified. The base is specified as a tri with the normal pointing inward using the right
hand rule. To create the wedge shown in Figure 3, the following command would be entered:
create wedge node 1,2,3,4,5,6 owner volume 1
Figure 3. Node ordering for Create Wedge Command
Note: The wedge command is still under development. To enable this feature, use the developer command features by
issuing the command Set Developer Commands On.
Creating Face and Tri Elements
To create quad and tri elements using existing mesh nodes
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh.
Click on Quad or Tri.
Click on the Create action button.
Select Single Element from the drop-down menu.
Enter the appropriate value for each Node ID.
Enter the appropriate value for Volume ID. This can also be done using the Pick Widget function.
Click Apply.
665
Trelis 15.0 User Documentation
Create {Face|Tri} Node <range> [Owner {Volume|Surface} <id>]
The next form of the command creates a face or tri that will be owned by the specified volume or surface. Four nodes are
specified for a face, three nodes for a tri. The nodes should be specified in the order needed to produce a face or tri with
the normal in the desired direction using the right hand rule.
Creating Edge Elements
To create edge elements using existing mesh nodes
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh.
Click on Edge.
Click on the Create action button.
Select Single Element from the drop-down menu.
Enter the appropriate value for each Node ID.
Enter the appropriate value for Volume ID. This can also be done using the Pick Widget function.
Click Apply.
Create Edge Node <range> [Owner {Volume|Surface|Curve} <id>]
This form of the command creates an edge that will be owned by the specified volume, surface, or curve. Two nodes must
be specified; order is unimportant.
Creating Nodes
To create a node by specifying the location
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Node.
Click on the Create action button.
Specify the X, Y and Z Coordinates.
Choose a Node Owner by selecting Volume, Surface, Curve or Vertex from the Node Owner drop-down
menu.
Enter the appropriate value for the selected Node Owner. This can also be done using the Pick Widget
function.
Click Apply.
Create Node Location <x> <y> <z> Owner {Volume|Surface|Curve|Vertex} <id>
The last form of the command creates a node at the specified location that will be owned by the specified volume, surface,
curve, or vertex. The location is specified by three absolute values that represent the position of the node in 3D space.
Merging Nodes
The merge node command is used to join two mesh entities one node at a time. It should be used with care because
merging nodes of different meshed entities may have unpredictable results. The syntax is:
Merge Node <id1> <id2>
The merge node command replaces the node specified as id1 with the node id2. The command is equivalent to deleting
node id1 and creating node id2 in the same location. The resultant merged node takes on the characteristics of the
replaced node such as position and owner. This may include some or all of the higher level mesh entities related to the
merged node.
Caution should be taken when using the merge node command because other commands involving the related meshed
entities may not work properly following the merge.
666
Creating and Merging Mesh Elements
667
Cleaning Up a Tetrahedral Mesh
An alternative to the remesh command for tetrahedral meshes is the cleanup command. For this command the existing
mesh is validated and "optimized" by the tetmesher, instead of being deleted.
To cleanup a tetrahedral volume mesh
1.
2.
3.
4.
On the Command Panel, click on Mesh and then Volume.
Click on the Tet Cleanup action button.
Enter the appropriate value for Volume ID(s). This can also be done using the Pick Widget function.
Click Apply.
Cleanup {Volume|Block} <id_range>
A second variation of the Cleanup command allows remeshing of tetrahedra that are either part of a free mesh (not owned
by a volume) or are a subset of the tetrahedra in the volume. The command is:
To remesh tetrahedra
1.
2.
3.
4.
On the Command Panel, click on Mesh and then Tet.
Click on the Tet Cleanup action button.
Enter the appropriate value for Tet ID(s). This can also be done using the Pick Widget function.
Click Apply.
Cleanup Tet <id_range> [Free]
For example, the command
cleanup tet all free
will gather all tetrahedra in a free mesh or single volume, generate a triangle boundary surface, and "optimize" the mesh,
ignoring any volume or blocks. Without the optional free keyword, the tets will be processed volume by volume or block by
block retaining the boundary between adjacent volumes or blocks.
Also, the command
cleanup tet 200 to 300
will gather the tetrahedra in the range [200, 300], generate a triangle boundary surface, and "optimize" the mesh. If the
tetrahedra in the range are disjointed, i.e., multiple, independent sets, this operation may fail. It is best to specify a
contiguous set of elements.
Note: Trelis will issue an error if the tetrahedra are owned by more than one volume or mesh container.
669
Mesh Validity
After a mesh is generated, it is checked to ensure that the mesh has valid connectivity. If an invalid mesh is formed, then
Trelis automatically deletes it. This default behavior can be changed with the following command:
Set Keep Invalid Mesh [on|off]
The current behavior can be viewed with the following command:
List Keep Invalid Mesh
The Jacobian quality metric is also computed automatically to check quality after a mesh is generated. If the quality is
poor, a warning is printed to the terminal.
671
Geometry Adaptive Sizing Function (Skeleton
Sizing)
The Geometry Adaptive Sizing Function, also referred to as the Skeleton Sizing Function (Quadros 2005; Quadros
2004; Quadros 2004(2)), automatically generates a mesh sizing function based upon geometric properties of the model.
This sizing scheme attempts to create a sizing function that allows unstructured meshing schemes to generate a mesh
with the following properties:
•
•
•
The sizes of the mesh elements vary smoothly throughout the mesh
The mesh elements resolve the geometry to a sufficient degree
The mesh elements do not over-resolve the geometry.
The geometry adaptive sizing function can be used to create sizing information for surfaces, solids, and assemblies.
This sizing function uses geometric properties to influence mesh size. The scheme calculates or estimates:
•
•
•
•
•
3D-proximity (thickness though the volume)
2D-proximity (thickness across a surface)
1D-proximity (curve length)
Surface curvature
Curve curvature.
These properties are then used to calculate a sizing function throughout the geometric entity (or entities). Regions of
relatively high complexity will have a fine mesh size, while regions of relatively low complexity will have a coarse mesh
size. For example, generally, a high-curvature region on a surface will have a finer mesh size than a low-curvature region
on that surface
673
Trelis 15.0 User Documentation
Figure 1: Overview of Computational Framework
Figure 2: Skeleton Sizing Function example in the GUI
674
Geometry Adaptive Sizing Function (Skeleton Sizing)
Skeleton Sizing Behaviors
Skeleton sizing can be specified on single or multiple surface(s)/volume(s) at a time from the GUI (Meshing Control Panel)
or the command-line. The following describes how specifying sizing on entities can change skeleton sizing’s behavior:
Single surfaces/volumes – If skeleton sizing is applied to surfaces/volumes one at a time, each entity’s sizing is not
influenced by the others. On the command-line, issue a separate command for each entity. In the GUI, specify only one
surface or volume before selecting “Apply Size”.
Multiple surfaces – If skeleton sizing is applied on multiple surfaces together, then geometric features of a particular
surface may affect its neighboring surfaces.
Multiple volumes (assembly sizing) – Skeleton sizing can be applied to assembly models so that geometric features of a
volume may influence its neighbors. Volumes should first be imprinted and merged before they are specified together for
skeleton sizing.
Command Line Syntax
Skeleton sizing on surfaces:
Surface <surface_id_range> Sizing Function Skeleton
{[scale <1 to 10 = 7>] [time_accuracy_level <1 to 3 = 2>]
[min_depth <3 to 8 = 5>] [max_depth <4 to 9 = 7>] [facet_extract_ang <1 to 30 = 10>]
[min_num_layers_2d < 1 to N = 1>] [min_num_layers_1d < 1 to N = 1>]
[max_span_ang_surf <5.0 to 75.0 = 45.0 degrees>]
[max_span_ang_curve <5.0 to 75.0 = 45.0 degrees>]
[min_size <float>] [max_size <float>] [max_gradient <float=1.5>]}
Skeleton sizing on volumes:
Volume <range> Sizing Function Skeleton
{[scale <1 to 10 = 7>] [time_accuracy_level <1 to 3 = 2>]
[min_depth <3 to 8 = 5>] [max_depth <4 to 9 = 7>] [facet_extract_ang <1 to 30 = 10>]
[min_num_layers_3d < 1 to N = 1>] [min_num_layers_2d < 1 to N = 1>]
[min_num_layers_1d < 1 to N = 1>]
[max_span_ang_surf <5.0 to 75.0 = 45.0 degrees>]
[max_span_ang_curve <5.0 to 75.0 = 45.0 degrees>]
[min_size <float>] [max_size <float>] [max_gradient <float=1.5>]}
The options are explained below:
Basic Arguments
•
•
•
max_size (default=auto): The value for max_size is calculated automatically by default. Users can specify any
positive real number based on the dimensions of the model to control the max size of the elements. If the
skeleton sizing function creates large elements, than this argument can be used to control the maximum
element size.
min_size(default=auto): The value for min_size is calculated automatically by default. Users can specify any
positive real number based on dimension of the model to specify the minimum size of the elements.
max_gradient (1.0 to 3.0, default 1.5): The transition in element size is controlled using this parameter. Larger
values of max_gradient result in fewer elements, but also lead to more abrupt transitions in size and possibly
poorer quality elements.
Scaling and Accuracy Arguments:
•
scale (1 to 10, default 7): The overall size of the elements is controlled by this argument. A coarser mesh can
be generated by increasing the value of scale up to 10.0. To get a finer mesh, decrease the value of the scale
(minimum value = 1).
675
Trelis 15.0 User Documentation
•
time_accuracy_level (1 to 3, default 2): This controls the computational time and accuracy level by adjusting
various internal parameters of the skeleton sizing function. Users should try levels in increasing order. Level 1
takes the shortest time to compute the skeleton sizing function and Level 3 takes the longest time to compute
the skeleton sizing function. However, Level 1 is less accurate than Level 2 and Level 3.
Advanced Arguments
Lattice Arguments:
The skeleton sizing function is generated and stored on a background octree grid whose cells are subdivided based on
the graphics facets of the model. The level of subdivision of the background grid affects how well the sizing function
captures the geometric complexity of features. Reasonable defaults have been selected for the following two refinement
(subdivision) parameters, but these may be overridden for use with simple (decrease parameters) or more complex
(increase parameters) models.
•
•
•
min_depth (default auto): min_depth controls the maximum cell dimension of the background octree grid. The
higher the value of min_depth, the smaller the dimension of the maximum-sized cell. Computational time
increases with increasing min_depth. By default the min_depth is calculated based on the geometric complexity
of the input model and mesh size specified on sub-entities.
max_depth (default auto): max_depth controls the minimum cell dimension. If the object contains very fine
features then increasing the value of max_depth is suggested. The maximum depth has been limited to 9. By
default the max_depth is calculated based on the geometric complexity of the input model and mesh size
specified on sub-entities.
facet_extract_ang (default 10 degree): facet_extract_ang is used to control the faceted representation of
NURBS model. This option gives control of the accuracy of a faceted approximation of the model used to
compute the adaptive sizing. For models with high curvature regions, decreasing the tolerance will give a better
approximation of the geometry and avoid the creation of random dense meshes. Note that increasing this angle
too much can generate invalid facets over curved regions, while decreasing the angle too much can cause
signficant slowdowns in sizing calculations.
Source Entity Arguments
•
•
•
•
•
min_num_layers_3d (Any value greater than 1, default 1): This parameter ensures that a minimum specified
number of layers exist across the thickness of the volume. This parameter could be useful in generating
meshes for mold flow simulation.
min_num_layers_2d (Any value greater than 1, default 1): This parameter ensures that a minimum specified
number of layers exist across the thickness of a surface.
min_num_layers_1d (Any positive integer value, default 1): This ensures that any curve contains a minimum
specified number of intervals.
max_span_ang_curve (Range 5.0 to 75.0, default 45.0): Maximum spanning angle is a parameter that controls
the mesh size at curved regions of curves. It is defined as the angle subtended by the normals at the end nodes
of the mesh edge in the curved region of a curve. When a finer mesh is needed at curved regions of curves,
then max_span_ang_curve should be decreased.
max_span_ang_surf (Range 5.0 to 75.0, default 45.0 deg): Maximum spanning angle is a parameter that
controls the mesh size at curved regions of surfaces. It is the angle subtended by the normals at the end nodes
of the mesh edge in a curved region of a surface. When a finer mesh is needed at curved regions of surfaces,
then max_span_ang_surf should be decreased.
Note: These arguments override the basic arguments. For example, time accuracy level 1 internally sets min_depth = 4
and max_depth = 6, and when min_depth is set to 4 and max_depth is set to 7 in the advanced options (recommended
for models with fine features), then advanced options override the basic options. In the command-line, to override the
depths set by a time_accuracy_level, specify min_depth and max_depth after it.
Skeleton with Other Sizing Controls
Skeleton sizing function produces a smooth sizing function when called with other sizing controls available in Trelis.
Skeleton sizing function behaves as SOFT firmness level. Skeleton sizing function always respects interval count
specified on the curves. Skeleton sizing function respects interval size on curves and surfaces only if it is specified after
calling the skeleton sizing function.
676
Geometry Adaptive Sizing Function (Skeleton Sizing)
Figure 3: Skeleton sizing function with other sizing controls
Limitations
•
•
•
Currently, the skeleton sizing function is primarily intended for use with ACIS models. Skeleton sizing may be
used on facet-based models (STL, facet, and MBG format) models, but results are not guaranteed. Sizing
function generation with other geometry engines in Trelis is not guaranteed or supported in Trelis 10.1.
The skeleton sizing function has mainly been tested with trimesh and tetmesh schemes. In general, structured
or semi-structured meshing schemes do not have enough flexibility to utilize the skeleton sizing function. It is
recommended that the skeleton sizing be used only with unstructured meshing schemes. However, if using
skeleton sizing in conjunction with the pave scheme for surfaces, decreasing the max_gradient and scale
arguments is suggested.
For sizing function generation of assemblies in Trelis 10.1, at least time_accuracy_level 2 is generally
recommended. This helps ensure that the geometric complexity of small features is captured. For example,
“volume all sizing function skeleton time_accuracy_level 2”
677
Bias Sizing Function
Syntax:
Surface <id> Sizing Function Type Bias Start Curve <id_range>
{Finish Curve <id_range>| Factor <val>}
Synopsis:
The Bias sizing function for surfaces is similar to biasing curves. Indeed, setting a bias sizing function for a surface will
bias the boundary curves, as well as control paving to follow the bias inside the surface. You first specify the size of a
couple of bounding curves (the start curves), then specify the bias sizing function for the surface.
Discussion:
Recall that for biasing curves, you specify the start and end vertex. For the bias sizing function, you specify the start
curves, from which to bias away. The sizes of these curves should already be set before setting the surface sizing
function since their average size is taken to be the starting size (almost). If the start curve sizes change, then you should
set the surface sizing function again.
You can either supply a geometric factor, or the set of finish curves whose sizes you want to match at that distance. A
geometric factor. It automatically sizes and biases or dualbiases the non-start curves, including any finish curves. These
curves need not be perpendicular to the starting curves. The interval count and scheme are soft-set, so they won't be
changed if they are already hard-set. If the size of the start curves or finish curves are changed, then the sizing function
command should be re-issued.
The sizing function value at a point is defined in terms of the straight-line distance from the point to the closest starting
curve. So, it works best if all the starting curves have the same size, and the surface is relatively flat. But, starting curves
need not be parallel to one another. Similarly, the non-start curves need not have any particular orientation wrt the start
curves.
The bias sizing function was designed to easily set the sizes of a sequence of adjoining surfaces: assign a size to the
curve you want to bias away from, then set the bias sizing function of the first surface, with its finish curves being the start
curve of the second surface, etc. See the last example below.
Examples:
Here are some example journal files and resulting pictures:
# bias_sz_fn_demo.jou
brick x 100 y 10 z 10
color vol 1 red
surface 1 scheme pave
surface all except 1 visibility off
# label curve interval
# graph text 2
display
# mesh 1
curve 4 size 2
surface 1 sizing function type bias start curve 4 factor 1.3
mesh surface 1
# see figure 1
Figure 1. Surface with bias sizing function factor > 1.
679
Trelis 15.0 User Documentation
# mesh 2
delete mesh
surface 1 sizing function type bias start curve 4 factor {1/1.1}
mesh surface 1
# see figure 2
Figure 2. Surface with bias sizing function factor < 1
# mesh 3
reset
cyl rad 6 z 1
cyl rad 4 z 1
sub 2 from 1
section body 1 yplane
section body 1 xplane
surf all except 19 vis off
color vol 1 red
display
# finish curve mesh
surf 19 scheme qtri base scheme pave
surface 19 size 0.7
curve 26 size 0.07
surface 19 sizing function type bias start curve 26 finish curve 25
mesh surface 19
pause
# see figure 3
680
Bias Sizing Function
Figure 3. Surface with bias sizing function start and finish curve. Scheme qtri, base scheme pave.
# dual bias mesh
delete mesh
curve 25 26 size 0.02
curve 25 26 scheme equal
surface 19 sizing function type bias start curve 26 25 factor 1.3
mesh surface 19
zoom curve 12
pause
# see figure 4
681
Trelis 15.0 User Documentation
Figure 4. Close up of surface with dual bias sizing function start and finish curve. Scheme qtri, base scheme
pave.
# funny face
reset
prism sides 5 z 1 radius 1
cylinder radius 0.1 z 1
body 2 move -0.4 0 0
subtract 2 from 1
cylinder radius 0.1 z 1
body 3 move 0.2 0 0
subtract 3 from 1
prism sides 6 radius 0.2 z 1
body 4 move 0 -0.4 0
subtract 4 from 1
surface all except 34 visibility off
color vol 1 red
display
surface 34 scheme pave
curve 23 19 size 0.01
surface 34 sizing function type bias start curve 19 23 factor 1.3
mesh surface 34
# see figure 5
682
Bias Sizing Function
Figure 5. Bias away from two round holes.
# bias surface chain
reset
cylinder radius 1 z 1
cylinder radius 0.2 z 1
cylinder radius 0.4 z 1
cylinder radius 0.8 z 1
imprint body all
delete body 2 3 4
section body 1 xplane
section body 1 yplane
surface all except 42 43 44 45 vis off
color volume 1 red
surface all scheme pave
curve 55 interval 36
surface 43 sizing function type bias start curve 55 factor 1.3
surface 44 sizing function type bias start curve 57 factor 1.3
# curve 57 had its size determined by a prior bias sizing function
surface 45 sizing function type bias start curve 58 factor 1.3
surface 42 sizing function type bias start curve 55 factor 1.3
mesh surface 42 43 44 45
display
highlight curve in surface 42 43 44 45
# see figure 6
683
Trelis 15.0 User Documentation
Figure 6. A chain of biased surfaces. Only one curve's intervals were explicitly set.
684
Constant Sizing Function
To use the constant sizing function
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Mesh.
Click on Volume or Surface.
Click on the Intervals action button.
Select Sizing Function from the drop-down menu.
Enter the appropriate value for Select Volumes or Select Surfaces. This can also be done using the Pick
Widget function.
Select Constant from the Sizing Functions menu.
Enter in any other appropriate settings.
Click Apply and then Mesh.
Surface <id> Sizing Function [Type] Constant
Volume <id> Sizing Function [Type] Constant
Synopsis:
The Constant sizing function specifies that a constant element size be used over the interior of the surface or volume.
The value used as the constant size is the interval size that has been set for the entity. For example, the following
commands will cause the mesh size to be smaller on the interior than on the surface's bounding curves.
reset
brick x 10
surface 1 scheme pave
curve in surface 1 interval 5
surface 1 size 0.5
surface 1 sizing function constant
mesh surface 1
685
Trelis 15.0 User Documentation
Figure 1. Constant Sizing Function
686
Curvature Sizing Function
The Curvature sizing function determines element size based on the curvature evaluation of a surface at the current
location. Two surface curvature values (taken perpendicular to each other) are compared at the location of interest, and
the largest is used as the sizing function for the mesh. Figure 1 shows a solid with a highly deformed surface which
displays rapid change of surface curvature at several locations.
Figure 1. NURB solid with high surface curvature change
Figure 2 depicts a normal paved mesh of this surface using a common size on all bounding curves and no sizing function
in the interior. The total number of quadrilateral shell elements for this case is 1988. Figure 3 shows a mesh which was
generated with the curvature sizing function option. The mesh is graded denser in the regions of quickly changing
curvature, such as at the tops of the hills and at the bottom of the valley. Due to the intense interrogation of the underlying
geometric modeler which the curvature method relies on, this option can be very computationally expensive.
Figure 2. NURB mesh with no interior sizing function
Figure 3. NURB mesh with curvature sizing function
687
Linear Sizing Function
The Linear class of sizing functions determines element size based on a weighted average of edge lengths for mesh
edges bounding the surface being meshed. There are several variants of this class of sizing function. The Linear function
bases edge length at a location on the lengths of edges bounding the surface weighted by their inverse distance from the
current location. The result of this weighting is a more gradual change in mesh density during a transition between dense
and coarse mesh. Figure 1 shows the same NURB surface mesh but with intervals of 34 on two curves and intervals of 16
on the remaining two bounding curves and no sizing function. It can be observed that the mesh progresses more rapidly
inward from the coarser meshed curves, which locates the transition region much closer to the finer meshed curves. To
combat this, the Linear function weights the sizing of new elements such that these transitions occur slower. Figure 2
displays two views of the same NURB geometry with the same bounding curve mesh density using the linear sizing
function.
Figure 1. NURB mesh with no sizing function, 34 by 16 density
689
Trelis 15.0 User Documentation
Figure 2. NURB mesh with linear sizing function, 34 by 16 density
690
Interval Sizing Function
The Interval sizing function is similar to the Linear function, but bases edge length at a location on the squared lengths of
edges bounding the surface weighted by their inverse distance from the current location. An example is shown below.
Figure 1. NURB mesh with interval sizing function, 34 by 16 density
691
Inverse Sizing Function
The Inverse sizing function is also similar to the Linear function, but this method bases edge length at a location on the
inverse lengths of edges bounding the surface weighted by their inverse distance from the current location (see Figure 1).
The difference between the three linear sizing functions (Linear, Interval, Inverse) is sometimes subtle, but is driven by the
geometry being meshed since the influence of these functions is strongly controlled by the number, positioning, and mesh
density of the bounding curves relative to the interior surface area.
Figure 1. NURB mesh with inverse sizing function, 34 by 16 density
693
Exodus II-based Field Function
The ability to specify the size of elements based on a general field function is also available in Trelis. With this capability,
the desired element size can be determined using a field variable read from a time-dependent variable in an Exodus II file.
Both quadrilateral and triangle elements are supported for surfaces, but only tetrahedral elements are supported for
volumes at this time.
A field function is a time-dependent variable in an Exodus II file. Either node-based or element-based variables may be
used. Currently, field functions are imported from element and node-based Exodus II data. The mesh block containing the
corresponding elements must be imported along with the field function data.
Exodus variable-based adaptive meshing is accomplished in Trelis in several steps:
1.
2.
3.
4.
5.
Surface mesh scheme set to Pave or TriAdvance, and/or volume mesh scheme set to Tetmesh. Bounding
curve mesh schemes can also optionally be set to Stride (see comments below.)
An Exodus mesh and time-dependent variable for that mesh is read into Trelis.
The mesh and variable data are associated to geometry.
The Exodus variable is normalized to give localized size measures, and the surface/volume sizing function type
is designated.
Geometry is meshed
Importing a field function and associating it with its geometry, and normalizing that function are done in two separate steps
to allow renormalization. The following command is used to read in a field function and its associated mesh:
Import Sizing Function '<exodusII_filename>' Block <block_id> Variable `<variable_name>' Time
<time_val> [Deformed]
where block_id is the element block to be read, variable_name is the Exodus time-dependent variable name (either
element-based or nodal-based),and time_val is the problem time at which the data is to be read. The Deformed keyword
indicates whether deformation has been accounted for on the new model (for information on creating deformed 2D
geometry from EXODUSII data, see Importing 2D EXODUSII Files) and needs to be accounted for in the sizing function
data. When this command is given, the nodes and elements for that element block are read in and associated to geometry
already initialized in Trelis.
Note that when a sizing function is read in, the mesh is stored in an ExodusMesh object for the corresponding geometry,
and therefore the geometry is not considered meshed. Also note that if deformation is not being modeled, the geometry to
which the mesh is being associated must be in the same state as it was when that mesh was written (see Importing a
Mesh for more details on importing meshes).
Once the field function has been read in and assigned to geometry, it can be normalized before being used to generate a
mesh. The normalization parameters are specified in the same command that is used to specify the sizing function type
for the surface or volume.
To use the exodus II-based field function
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Mesh.
Click on Volume or Surface.
Click on the Intervals action button.
Select Sizing Function from the drop-down menu.
Enter the appropriate value for Select Volumes or Select Surfaces. This can also be done using the Pick
Widget function.
Select Exodus from the Sizing Functions menu.
Enter in the appropriate settings for Min Size and Max Size.
Click Apply and then Mesh.
Surface <id> Sizing Function Type Exodus [Min <min_val> Max <max_val>]
Volume <id> Sizing Function Type Exodus [Min <min_val> Max <max_val>]
695
Trelis 15.0 User Documentation
If normalization parameters are specified, the field function will be normalized so that its range falls between the minimum
and maximum values input. Subsequent normalizations operate on the normalized data and not on the original data. If an
element-based variable is used for the sizing function, each node is assigned a sizing function that is the average of
variables on all elements connected to that node. Nodal variables are used directly.
After the sizing function normalization, the geometry may be meshed using the normal meshing command.
For example, the left image in Figure 1 depicts a plastic strain metric which was generated by PRONTO-3D [Taylor, 89] a
transient solid dynamics solver, and recorded into an ExodusII data file. When the file is read back into Trelis, the paving
algorithm is driven by the function values at the original node locations, resulting in an adaptively generated mesh
[Attaway, 93]. The right image in Figure 1 depicts the resulting mesh from this plastic strain objective function.
Figure 1. Plastic strain metric and the adaptively generated mesh
Curve Meshing with Exodus II - based Field Functions
In addition to the capability to adaptively mesh surface using a field function, curves may also be meshed separately using
the Exodus II information. The Stride scheme for meshing curves is used for this purpose. If the user does not specify a
mesh scheme for the curve, Trelis will default to scheme Stride when the Exodus sizing function is used for surfaces and
volumes defined by that curve.
696
Importing Exodus II Files
•
•
•
Importing a Free Mesh without Geometry
Importing a Free Mesh onto Existing Geometry
Creating Mesh-based Geometry on Import
To import meshes from an Exodus II format file
1.
2.
3.
4.
5.
6.
Select File and then Import.
Select the file to be imported.
Select Exodus from the Files of type drop-down menu.
Click Open. A new window will appear.
Optionally select any appropriate specifications from this window.
Click Finish.
Import Mesh '<exodusII_filename>' [Block <block_ids>] [Unique Genesis IDs] [Shell] No_Geom
[group_name '<free_mesh_group_name>']]
Import Mesh '<exodusII_filename>' [Block <block_ids>] [Unique Genesis IDs] [Shell]
[{Group|Body|Volume|Surface|Curve|Vertex} <id_range> | Preview]
Import Mesh Geometry '<exodusII_filename>' [Block <id_range>|ALL] [Start_id <id>] [Use
[NODESET|no_nodeset] [SIDESET|no_sideset] [Feature_Angle <angle>]
[LINEAR|Gradient|Quadratic|Spline] [Deformed {Time <time>|Step <step>|Last} [Scale <value>] ]
[MERGE|No_Merge] [Export_facets <1|2|3>] [Merge_nodes <tolerance>]
Related Commands:
Import Mesh Geometry (options)
Import Free Mesh (2D)
Delete Mesh Preview
Export [ Genesis | Mesh ] '<filename>'
List Import Mesh NodeSet Associativity
List [Export Mesh] NodeSet Associativity
[Set] Import Mesh NodeSet Associativity [ON|off]
[Set] [Export Mesh] NodeSet Associativity [on|OFF]
Transforming Mesh Coordinates
Set Import Mesh [Vertex] [Curve] [Surface] Tolerance <distance>
Set Import Mesh NodeSet Order [On|Off]
List Import Mesh NodeSet Order
Importing a Free Mesh Without Geometry
The command to import a free mesh from an Exodus II format file without mesh-based geometry is:
Import Mesh '<exodusII_filename>' [Block <block_ids>] [Unique Genesis IDs] [Shell] No_Geom
[group_name '<free_mesh_group_name>']]
697
Trelis 15.0 User Documentation
When a free Exodus II mesh is imported into Trelis, it contains no geometric or topological information. Previously, the
user could either associate that mesh with existing geometry, or build mesh-based geometry to fit the mesh. A third
option, as of Trelis 11.1, allows the user to retain the disassociated mesh as a free mesh inside Trelis.
A free mesh may be modified as described in the Free Mesh section of the documentation. This includes limited access to
smoothing, renumbering, transformations, refinement, mesh quality, and other mesh centric operations.
When an Exodus II File is imported as a free mesh, Trelis will automatically create a group called "free_elements" to
contain the free mesh elements.
Note: The Import Mesh [No_Geom] command is not to be confused with the Import Free Mesh command which applies
only to 2D Exodus II Files.The term "Free Mesh" in both places of the documentation refers to the same thing - a mesh
without geometry. However, in the case of all other import mesh commands, the imported free mesh ends up associated
with geometry. The Import Mesh [No_Geom] is the only way to import a free mesh that remains disassociated from
geometry.
Importing a Mesh Onto Existing Geometry
The command to import a free mesh from an Exodus II format file and associate it with existing geometry is:
Import Mesh '<exodusII_filename>' [Block <block_ids>] [Unique Genesis IDs] [Shell]
[{Group|Body|Volume|Surface|Curve|Vertex} <id_range> | Preview]
The user can import a mesh from an Exodus II file and associate the mesh with matching geometry. The resulting mesh
may then be manipulated normally. For example, the mesh may be smoothed or portions of it deleted and remeshed. The
user can save their work by exporting the geometry and mesh, and then restore the geometry and mesh later. In some
cases, saving and restoring can be faster or more reliable than replaying journal files.
Saving and importing a mesh may be useful for teams working on creating a conforming mesh of a large assembly so that
they can pass information to one another. For example, a team member can export the mesh on the surfaces between
two parts, and another team member import the mesh for use on an adjoining part of the assembly.
As of Trelis version 7.0, any higher order elements, block definitions, nodesets, and sidesets are retained on import.
Importing a Mesh with Nodeset Associativity
Meshes can be imported into Trelis that contain nodeset associativity data used for defining finite element boundary
conditions. If an exported Trelis mesh is going to be imported back onto the same geometry, then before exporting the
user should issue the following command:
set export mesh nodeset associativity on
This causes extra nodeset data to be written, which associates every node to a geometric entity, resulting in an import
which is more reliable. When importing, if the user does not want to use the nodeset associativity data that exists in a file,
then before importing the following command should be used:
set import mesh nodeset associativity off
The user may wish to turn geometry associativity off if, for example, the geometry is no longer identical as a result of
curves being composited, or Trelis names changed due to a ACIS version changes.
Importing a Mesh onto Modified Geometry
Although there are some exceptions, Trelis requires that the mesh be imported onto the same geometry from which it was
exported.
Since merge information is not stored with the ACIS representation, care should be taken that the geometry is merged the
same way on export and import of the mesh. If not, importing the mesh one block at a time in successive commands may
increase the chance of a successful import, at the cost of more memory and time.
698
Importing Exodus II Files
Between exporting and importing a mesh, the geometry may be modified slightly by compositing entities. Mesh import will,
however not be successful if entities are partitioned or a body is webcut. In some cases mesh import may be successful
on modified geometry if the new vertices match up exactly with nodes of the mesh, and the new curves match up exactly
with edge chains of the mesh. Unless this criteria is met, associating the mesh with the geometry will be unsuccessful.
Mesh Import Tolerance
To change the tolerance with which imported mesh must line up with geometry issue the command:
Set Import Mesh [Vertex] [Curve] [Surface] Tolerance <distance>
Specifying a Portion of the Mesh to be Imported
The Block option in the Import Mesh command indicates that only the specified element block should be imported from
the Exodus II file. In the same manner, the Volume and other geometry options provide a way to import the nodes and
element on the indicated geometry. If neither a block nor a geometry entity is specified, then the entire mesh file is read.
If a block is specified without specifying a geometry entity, associativity or proximity is used to determine which volume
the block elements should be associated with. If a block and a volume are specified, the block elements are associated
with the specified volume, provided they actually match. If a volume is specified without a block, associativity data is
used to find a block corresponding to the given volume.
Unique Genesis IDs and Shell Options
The Unique Genesis IDs option is used to preserve ids in the genesis file in the case that id overlap exists when importing
into Trelis. This can occur when importing into an active session where Trelis ids have already been assigned.
The Shell Option is used as a flag to alert the program that there are shell elements in the file. Shell elements can not
always be detected by the import program, and this ensures that the shell elements will be included in the model.
Nodeset Ordering
If the Import mesh NodeSet Order flag is on, the nodesets will be read in a manner which allows them to be associated
with existing geometry. This means the nodesets are assumed to be in ascending order. If the flag is set to false, the
goemetry nodesets in imported mesh files are assumed to be in random order. This value is on by default, and should not
need to be changed by the user.
Creating Mesh-Based Geometry on Import
Trelis' mesh generation tools require an underlying geometry representation. In most cases, the ACIS solid modeling
engine, compiled with Trelis, is used to represent the geometry. However, in some cases, an ACIS representation is not
available, and a previously developed finite element mesh is the only available representation of the model. In order to
utilize Trelis' mesh generation tools, the import mesh geometry command provides an option for creating geometry
directly from the finite element mesh.
The import mesh geometry command will create a new volume for every block defined in the Exodus II file. It will also
create curves, surfaces and vertices at appropriate locations on the model based on dihedral angles (also called feature
angles) and assigned nodesets and/or sidesets. The mesh used to construct the geometry will be owned by the new
geometric entities. This means that the mesh can be deleted, remeshed, or smoothed using any of Trelis' meshing tools
by simply using the new geometry definition. Trelis will assign appropriate intervals to the new curves as well as
determine an acceptable meshing scheme for surfaces and volumes.
The command to import a finite element mesh from an ExodusII format file and generate geometry from the mesh is:
Import Mesh Geometry '<exodusII_filename>'
[Block <id_range>|ALL] [Start_id <id>] [Use [NODESET|no_nodeset] [SIDESET|no_sideset]
[Feature_Angle <angle>] [LINEAR|Gradient|Quadratic|Spline] [Deformed {Time <time>|Step
<step>|Last} [Scale <value>] ] [MERGE|No_Merge] [Export_facets <1|2|3>] [Merge_nodes
<tolerance>]
699
Trelis 15.0 User Documentation
File Name
Type the name of file to import in single quotation marks. The file must reside in the current directory. For information on
changing the current directory, see Trelis environment commands. To list all the files in the current directory, type ls at the
command prompt.
Blocks
Use this option to select the specific blocks to be imported from the Exodus II file. If no blocks are entered, then all blocks
will be read and imported from the file. Standard ID parsing can also be used in this argument to select a range of blocks.
For example "1 to 5" or "1, 5 to 10 except 6".
Each unique block selected to be imported will define a new body in the geometric model. Figure 1 shows a simple
example of the geometry generated from the 3D finite element mesh.
Figure 1. Example of mesh based geometry (right) created from a finite element mesh (left)
Blocks may be composed of 1D, 2D or 3D elements. For blocks composed of 2D elements (i.e. QUAD4, SHELL etc.), a
sheet body will be created. One dimensional elements (i.e.. BEAM, TRUSS, etc.) will define curves. Where a block may
be composed of more than one disconnected sets of elements, one body will be created for each continuous region of
elements assigned to the same block. Where possible, the ID of the new body will be the same as the block ID. Since IDs
must be unique, if a body ID is already in use, the next available ID will automatically assigned by the program.
Start ID
Use this option to specify an alternate ID value for imported entities. The specified value will be used as the starting ID for
BOTH nodes and mesh elements. The new IDs will be assigned consecutively from the starting value. If the new ID
values for any of the imported entities would conflict with existing IDs, the command does not abort but moves the starting
ID for all element types to the same useable starting ID value.
Nodesets/Sidesets
Use the nodeset and sideset options to use any nodeset and sideset information in the Exodus II file in constructing
geometry. Recall that nodesets and sidesets are generic boundary condition data assigned to nodes, edges or faces of
the finite elements. It is useful to group mesh entities belonging to unique boundary conditions into geometric entities. This
permits the user to remesh a particular region of the model without having to reassign boundary conditions.
If the nodeset and sideset arguments are given, geometric entities will be generated for each unique set of nodes, edges
or element faces assigned to a nodeset or sideset. The default is to use any nodeset and sideset information available in
the file. Figure 2 shows an example of how nodeset and sideset information might be used to generate geometry.
700
Importing Exodus II Files
Figure 2. Example of geometry created from mesh entities assigned to nodesets (3) and sidesets (1 and 2).
Upon import, nodesets and sidesets are automatically created with the appropriate geometric entities assigned to them.
The IDs of the new geometric entities, if generated from boundary condition data, will be the same as the nodeset and
sideset IDs. Where doing so would conflict with existing geometric IDs, the program will automatically select the next
available ID.
Feature Angle
Use this option to specify the angle at which surfaces will be split by a curve or where curves will be split by a vertex. 180
degrees will generate a surface for every element face, while 0 degrees will define a single, unbroken surface from the
shell of the mesh. The default angle is 135 degrees.
Figure 3. Example use of Feature Angle
Figure 3 shows an example of the use of different feature angles. On the left is a simple two-element hex mesh.
Specifying a feature angle greater than 120 degrees would create the geometry in the center image. Using a feature angle
less than 120 degrees and greater than 90 degrees would define the geometry on the right.
Smooth Curves and Surfaces
This argument allows the option of using a higher-order approximation of the surface when remeshing/refining the
resulting geometry. Default is to use the original mesh faces themselves as the curve and surface geometry
representation. If the finite element model to be imported is to represent geometry with curved surfaces, it may be useful
to select this option. If selected, it will use a 4th order B-Spline approximation to the surface [Walton,96]. Figure 4 shows
the effect of the smooth curve and surface option.
701
Trelis 15.0 User Documentation
Figure 4. Effect of Smooth Curve and Surface Option for remeshing of mesh-based geometry
In this figure the top image is the original finite element mesh imported into Trelis. In this example both models have been
remeshed with the same element size. The difference is that the figure on the right uses the smooth curve and surface
option. While this option can improve the surface representation, it should be noted that memory requirements and
meshing times can sometimes be affected.
If importing the Exodus II file using the command line, other options for surface representations are also available.
[LINEAR|Gradient|Quadratic|Spline]
The method used from the GUI is either Linear or Spline. The Gradient and Quadratic methods are still somewhat
experimental and may not be as general purpose as the Spline representation.
Apply Deformations
This option permits the user to import time-dependant deformation information from the Exodus file. For this option, any
vector data in the Exodus II file is assumed to be deformation information. If selected, deformations will be applied to the
nodes upon import. Enter a specific time step value, integer step, or the last time available in the file. If time-dependant
data is available in the Exodus II file, selecting the down arrow in the edit field will display the available time steps in the
file. Default time is the last time step.
702
Importing Exodus II Files
Figure 5. Example of remeshing of a deformed finite element mesh
Figure 5 shows an example of using Mesh-Based Geometry for a large deformation analysis. In this case, the analysis
[Attaway et. al.,98] began and continued until mesh quality became unacceptable. At that point, the mesh was imported
into Trelis and geometry re-created from the computed deformations. The finite element mesh could then be removed,
remeshed or improved and written back to an Exodus II file. After remapping [Wellman,99] the appropriate analysis
variables back to the mesh, the analysis could then be restarted. This process was repeated multiple times until the
desired results were achieved.
Note: Care should be taken when using large deformations, as inverted elements (negative Jacobians) may produce
unpredictable results with the resulting geometric representation.
Also available is an optional scale factor. This applies the indicated scale to all deformations. Default is 1.0.
Merge
This option allows the user to either merge or not merge the resulting volumes. The default option is to merge adjacent
volumes. This results in non-manifold topology, where neighboring volumes share common surfaces. Using the no_merge
option, adjacent volumes will generate distinct/separate surfaces.
Merge Nodes
The merge_nodes option will allow the user to specify a different tolerance for merging nodes on import. The default
value is 1e-6.
Note: Care should be taken when setting import merge tolerances. Setting a tolerance too low will not merge adjacent
nodes. Setting the tolerance too high can produce undesirable results, and severely tangle the mesh.
Export Facets
[export_facets <1|2|3>]
This is primarily a debug option available only from the command line. This option will export the shell of the Exodus mesh
to an ASCII file in the form of facets. The resulting file can be imported to Trelis using the "Import Facets" command.
Export options: 1 = export only the exterior facets to file "facets.shell"; 2 = export only the interior facets between element
blocks to file "facets.inter"; 3 = export all boundary facets to file "facets.all".
703
Importing Abaqus Files
To import a mesh from an Abaqus format file
1.
2.
3.
4.
5.
6.
Select File and then Import.
Select the file to be imported.
Select Abaqus from the Files of type drop-down menu.
Click Open. A new window will appear.
Optionally select any appropriate specifications from this window.
Click Finish.
Import Abaqus [Mesh Geometry] '<input_filename>' [Feature Angle <angle>] [Nobcs]
Including the keyword Mesh Geometry will instruct Trelis to create mesh-based geometry. This will provide the user with
the ability to remesh geometric entities. If the user does not import with the Mesh Geometry flag, he will have to tell Trelis
to draw the mesh after the import is done in order to view it.
The Feature Angle is used when building the surface topology to determine when to split a surface into two surfaces. If
the angle between two neighboring element normals is less than Feature Angle, then the two elements will be placed on
separate surfaces. If the keyword Feature Angle is not supplied, the default 135 degrees is used. For a description of
importing mesh geometry see Importing Exodus II Files.
The keyword nobcs can be included if boundary conditions are not to be imported.
The Abaqus importer can import the following Abaqus file formats: flat file, part-independent, and part-dependent.
It should be noted that Trelis sometimes cannot successfully generate mesh-based geometry for complex models. If this
occurs, import the mesh without the Mesh Geometry flag, and draw the mesh to view it.
To list Abaqus cards supported by Trelis:
List Abaqus Import Cards
This command will list out all supported Abaqus cards that Trelis can interpret.
Table 1. Supported Element Types
1st Order
2nd Order
Triangle
S3
CAX3
CPE3
STRI65
CAX6
CPE6
Quadrilateral
S4
CAX4
CPE4
S8
CAX8
CPE8
Tetrahedron
C3D4
C3D10
Hexahedron
C3D8
C3D20
Line Element
B21
B31
T2D2
T3D2
SPRINGA
SPRING1
SPRING2
B22
B32
T2D3
T3D3
705
Trelis 15.0 User Documentation
See http://www.simulia.com/ for more information on the ABAQUS file format.
706
Importing I-DEAS Files
To import a mesh from an I-DEAS format file
1.
2.
3.
4.
5.
6.
Select File and then Import.
Select the file to be imported.
Select Ideas from the Files of type drop-down menu.
Click Open. A new window will appear.
Optionally select any appropriate specifications from this window.
Click Finish.
Import Ideas [Mesh Geometry] '<input_filename>' [Feature Angle <angle>] [Nobcs]
Including the keyword Mesh Geometry will instruct Trelis to create mesh-based geometry. This will provide the user with
the ability to remesh geometric entities. If the user does not import with the Mesh Geometry flag, he will have to tell Trelis
to draw the mesh after the import is done in order to view it.
The Feature Angle is used when building the surface topology to determine when to split a surface into two surfaces. If
the angle between two neighboring element normals is less than Feature Angle, then the two elements will be placed on
separate surfaces. If the keyword Feature Angle is not supplied, the default 135 degrees is used. For a description of
importing mesh geometry see Importing Exodus II Files.
The keyword nobcs can be included if boundary conditions are not to be imported.
It should be noted that Trelis sometimes cannot successfully generate mesh-based geometry for complex models. If this
occurs, import the mesh without the Mesh Geometry flag, and draw the mesh to view it.
To see more information on the I-DEAS file format, visit their website at www.siemens.com.
707
Importing Patran Files
To import a mesh from an Patran format file
1.
2.
3.
4.
5.
6.
Select File and then Import.
Select the file to be imported.
Select Patran from the Files of type drop-down menu.
Click Open. A new window will appear.
Optionally select any appropriate specifications from this window.
Click Finish.
Import Patran '<neutral_filename>'
Import Patran Mesh Geometry '<neutral_filename>' [Use [Feature_Angle <angle>]
[Linear|Gradient|Quadratic|Spline] ]
See Importing Exodus II Files for a description of the import options.
For more information on the Patran file format, see their website at www.mscsoftware.com.
709
Importing 2D Exodus Files
Trelis has a limited capability to create ACIS Geometry from 2D ExodusII finite element mesh files. (For a more general
capability, see the Import Mesh Geometry command, which will create Mesh-Based Geometry).
To import a 2D Exodus II file and create ACIS geometry:
1.
2.
3.
4.
5.
6.
Select File and then Import.
Select the file to be imported.
Select Exodus from the Files of type drop-down menu.
Click Open. A new window will appear.
Optionally specify any appropriate settings from this window.
Click Finish.
Import Free Mesh '<filename>' {Time <t> | Step <step#> | Last}
Trelis can create ACIS geometry from 2D Exodus II data files (4, 8, or 9 node QUAD or SHELL element types) that do not
have enclosed voids (holes surrounded by mesh) and which were originally generated with Trelis and exported to
ExodusII with the Nodeset Associativity option set to on. The Nodeset Associativity command records the topology of the
geometry into special nodesets which allow Trelis to reconstruct a new solid model from the mesh even after it has been
deformed. The new solid model of the deformed geometry can be remeshed with standard techniques or meshed with a
sizing function that can also be imported into Trelis from the same ExodusII file. Trelis' implementation of the paving and
triadvance algorithms can generate a mesh following a sizing function to capture a gradient of any variable (element or
nodal) present in the ExodusII file.
In order for this feature to be effective, the following commands must be issued when the mesh is exported and later
imported:
nodeset associativity on
set associativity complete on
The first command ensures that the geometry will be correctly recovered from the mesh, while the second ensures that
boundary condition and material IDs will be recovered.
711
Mesh Deletion
Meshing a complex model often involves iteration between setting mesh parameters, meshing, and checking mesh
quality. This often requires removing mesh, for only an entity or for an entity and all its lower order geometry, or
sometimes for the entire model.
The command to remove all existing mesh entities from the model is:
Delete Mesh
To delete a mesh on a specific entity
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh.
Click on Volume, Surface, Curve or Vertex.
Click on the Delete action button.
Enter in the appropriate ID for the specified entity. This can also be done using the Pick Widget function.
Click Apply.
Delete Mesh {geom_list} [Propagate]
These commands automatically cause deletion of mesh on higher dimensional entities owning the target geometry.
If the Propagate keyword is used, mesh on lower order entities is deleted as well, but only if that mesh is not used by
another higher order entity. For example, if two surfaces (surfaces 1 and 2) sharing a single curve are meshed, and the
command "delete mesh surface 1 propagate" is entered, the mesh on surface 1 is deleted, as well as the mesh on all the
curves bounding surface 1 except the curve shared by surface 2. In some cases, the capability to delete individual mesh
faces on a surface is needed. Deleting a mesh face involves closing a face by merging two mesh nodes indicated in the
input. The syntax for this command is:
Automatic Mesh Deletion
Trelis will automatically delete the mesh from a geometry that is about to be modified by a geometry modification
command. To change this behavior, so that Trelis will issue an error instead of automatically deleting the mesh, use the
following command.
Set Mesh Autodelete [ON|Off]
713
Free Meshes
A free mesh is a mesh that is not associated with any underlying geometric entities. A free mesh contains only mesh
elements (hexahedrons, triangles, edges, nodes, etc), and not volumes, surfaces, etc. Since there is no underlying
geometry, operations on free meshes are limited. The following operations can be performed on free meshes in some
capacity:
•
•
•
•
•
•
•
•
•
•
•
•
•
Creating a free mesh
Creating mesh-based geometry to fit a free mesh
Mesh merging
Mesh transformations
Mesh smoothing
Mesh quality operations
Mesh refinement
Cleaning up a free mesh
Assigning boundary conditions
Skinning a free mesh
Mesh deletion
Bottom-up element creation
Exporting a free mesh
Creating a free mesh
A free mesh can be created in three ways.
1.
2.
3.
Importing a mesh into Trelis using the Import Mesh [No_Geom] command. This option is discussed in detail in
Importing Exodus II Files.
Disassociating an existing mesh from its geometry
Creating a mesh with the geometry-tolerant mesh scheme
Disassociating a mesh from its geometry
To disassociate a mesh from existing geometry
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh and then Volume.
Click on the Create MBG action button.
Select Disassociate Mesh from the drop-down menu.
Select Volume, Surface, Curve or Vertex from the Disassociate Mesh From menu.
Enter the appropriate value for the specified entity. This can also be done using the Pick Widget function.
Click Apply.
Disassociate Mesh [From] {Volume|Surface|Curve|Vertex} <id_range>
For example:
brick x 10
mesh volume all
disassociate mesh from volume 1
delete volume 1
When a mesh is disassociated from its geometry, a group called 'disassociate elements' is created to contain the free
mesh.
715
Trelis 15.0 User Documentation
Creating Mesh-Based Geometry to fit a Free Mesh
It is possible to create underlying mesh-based geometry to own a free mesh. It is similar in functionality to the Import
Mesh Geometry command, but it does not not require the extra import/export step. So for example, a user would be able
to read in a free mesh, fix any mesh problems, and then create the mesh-based geometry without having to write the
mesh to a file first. The command syntax is:
Create Mesh Geometry {Hex|Tet|Face|Tri|Block} <range> [Feature_Angle <angle=135>] [Keep]
The command also applies to any subset of the mesh. For example, you can create mesh geometry for a group of hexes
or element blocks.
If the keep option is specified, the mesh will be duplicated so you will have two copies of the mesh: The original mesh and
the new mesh that is owned by the new MBG geometry. If the keep option is not specified, the existing mesh will be
reused, and duplicate elements will not be created. Elements will now be owned by the new MBG geometry. The
command will check for mesh ownership and will issue warning and enable the keep option if the mesh is owned. The
keep option is not specified by default.
Also note that any genesis entites defined on the free mesh will be maintained with this option. The genesis entities will
not however be transfered to the new MBG entities and will not be used as criteria for building the new MBG geometry.
Other options such as creating a spline representation and building geometry from genesis entities are not supported in
this command. Exporting the free mesh and reimporting using "import mesh geometry" may be an option if these features
are desired.
Merging a free mesh
To merge two free meshes
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh and then Node.
Click on the Equivalence Nodes action button.
Enter the appropriate value for Node ID Range. This can also be done using the Pick Widget function.
Enter the appropriate value for Tolerance.
Click Apply.
Equivalence Node <range> [Tolerance <value>]
All nodes in the given range that are within the specified tolerance will be merged. For example:
br x 10
volume 1 copy move x 10
mesh volume all
disassociate mesh from volume 1 2
delete volume 1 2
equivalence node all tolerance 0.05
## merges all nodes that are within 0.05 of each other
Free Mesh Transformation Operations
Mesh transformations for free meshes are achieved through the use of the group transformation commands, given in
Basic Group Operations. All members of a free mesh are automatically assigned to a group. These groups can then be
modified using group operations. The following command sequence illustrates how transformations might be applied to a
free mesh.
716
Free Meshes
brick x 10
mesh volume 1
disassociate mesh from volume 1
delete volume 1
group disassociated_elements move x 10
group disassociated_elements rotate 15 about x
group disassociated_elements scale 0.25
group disassociated_elements reflect 1 1 0
group 'node_group' add node 1 to 121
group node_group move z 5
##The moved nodes do not also move the attached geometry, as one might expect.
If a group is composed of mesh entities, these commands will only operate on the nodes in the group. All nodes of the
group will be moved, scaled, rotated, or reflected as specified. If there are no nodes in the group, Trelis will return an
error. Including all nodes in the group will transform the whole model. Including only a subset of nodes will transform those
nodes and their enclosed elements, but it will not transform the whole mesh.
Disassociated mesh elements cannot be copied using the Group copy commands. To create a copy they must be
exported and reimported. Alternatively, they can be associated with mesh-based geometry, and then copied using the
typical copy commands.
Extruding Mesh Elements
Mesh elements can be extruded to create new elements from existing nodes, edges, faces or triangles. A direction or
curve can be used to specify how the elements are created. The distance parameter is optional and if not specified the
length of the given direction will be used instead. Specifying a value for the layers option determines how many elements
will be created in the given distance. Twist can also be specified and requires an angle of twist and a twist axis.
To extrude mesh elements
1.
2.
3.
4.
5.
6.
7.
8.
On the Command Panel, click on Mesh.
Click on Hex, Quad, or Edge.
Click on the Create action button.
Select Extrude from the drop-down menu.
Enter the appropriate values for Face ID(s), Edge ID(s) or Node ID(s). This can also be done using the Pick
Widget function.
Enter the appropriate values for Direction. Optionally select the Direction... button to specify the direction
settings.
Optionally enter any other appropriate from the Optional Parameters menu.
Click Apply.
Create Element Extrude {Node|Edge|Face|Tri} <element_list> {Direction <options>|Along Curve
<curve_list>} [Distance <value>] [Layers <num_layers] [Twist <angle> Axis <axis_options>]
#Extrude a face in a given direction:
create node location 0 0 0
create node location 1 0 0
create node location 1 1 0
create node location 0 1 0
create face node 1 to 4
create element extrude face 1 direction 0 0 1 distance 3 layers 3
create element extrude face 1 direction 0 0 1 distance 3 layers 3 twist 90 axis direction 0 0 1 origin 0 0 0
717
Trelis 15.0 User Documentation
#Sweep face along curve
create node location 0 0 0
create node location 1 0 0
create node location 1 1 0
create node location 0 1 0
create face node 1 to 4
create vertex location position 0 0 0
create vertex location position 0 .2 1
create vertex location position 0 1 2
create vertex location position 0 3 2
create vertex location position 0 4 1
create vertex location position 0 5 0
create curve spline vertex 1 2 3 4 5
create element extrude face 1 layers 5 along curve 1
Figure 1. Extruding mesh elements along a spline
Offsetting Mesh Elements
Faces and triangle elements can be used to create hexahedral and wedge elements from an offset command. The default
offest direction is normal to the selected face. The Oppposite_normal option will use the reverse direction. The layers
parameter determines how many elements will be created in the given direction.
To use faces to create hexahedral elements from an offset command
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh and then Hex.
Click on the Create action button.
Select Offset from the drop-down menu.
Enter the appropriate value(s) for Face ID(s). This can also be done using the Pick Widget function.
Select Normal to Element or Opposite Normal.
Enter in the appropriate values for Distance and Number of Layers.
Click Apply.
Create Element Offset {Face|Tri} <element_list> [Normal_to|Opposite_normal] {Distance <value>]
[Layers <num_layers>]
718
Free Meshes
#Create wedge and hex elements from face and tri elements via offset
create node location 0 0 0
create node location 1 0 0
create node location 1 1 0
create node location 0 1 0
create node location 2 0 1
create node location 2 1 1
create node location 1 2 0
create face node 1 to 4 create face node 3 2 5 6
create tri node 7 4 3
create tri node 7 3 6
create element offset face all tri all distance 3 layers 3 opposite_normal
Revolving Mesh Elements
Elements can be created by revolving an existing element around a given axis. The Attempt_fix parameter will try to fix
any poorly formed hex elements by collapsing them into wedge elements. Angle determines the amount of rotation
around the axis. The Layers option determines how many elements will be created in the given rotation.
To revolve an element
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Mesh.
Click on Hex, Quad or Tri.
Click on the Create action button.
Select Revolve from the drop-down menu.
Enter the appropriate value(s) for Face ID(s) or Edge ID(s). This can also be done using the Pick Widget
function.
Enter in the appropriate values for Axis Options, Angle and Number of Layers.
Click Apply.
Create Element Revolve {Edge|Face|Tri} <element_list> Axis <axis_options> Angle <angle> [Layers
<num_layers>] [Attemp_fix]
#Revolve 2 faces around the Y-axis and collapse inner hexes to wedges
create node location 0 0 0
create node location 1 0 0
create node location 1 1 0
create node location 0 1 0
create node location 2 0 0
create node location 2 1 0
create face node 1 2 3 4
create face node 2 3 5 6
create element revolve face 1 2 axis direction 0 1 0 origin 0 0 0 angle 180 layers 4 attempt_hex_fix
719
Trelis 15.0 User Documentation
Figure 2. Revolving free mesh elements to create hex and wedge elements
Smoothing a free mesh
Interior nodes can be smoothed using commands such as smooth hex all, or smooth tet all in block 100. These
commands will smooth only the interior node on the elements used in the command. The nodes on the boundary will
remain unchanged. To smooth nodes on a boundary, the target smoothing option can be used. Targeted smoothing
allows the user to smooth a group of mesh elements to a surface or curve that is not their owner. Targeted smoothing is
discussed under Mesh Smoothing. The following sequence of commands illustrate the capability of smoothing a free
mesh to a target surface.
sphere rad 25
webcut vol 1 plane xplane offset 18
delete vol 2
webcut volume 1 plane yplane offset 8
webcut volume 1 plane yplane offset -8
delete vol 1 3
surf 16 copy
delete vol 4
surf 18 scheme pave
surf 18 size 2
mesh surf 18
disassociate mesh surf 18 ##Mesh and geometry overlap
refine face 1 radius 3
set developer on ## Smoothing free mesh is a developer command
smooth face all scheme laplacian
##Smoothed mesh is away from surface
smooth face all scheme laplacian target surface 18
##Smoothed mesh is aligned with surface
720
Free Meshes
Figure 3. Smoothing without a target (above) and smoothing to a target surface (below).
Mesh quality on a free mesh
The mesh quality checks for a free mesh are the same as for other geometry-based meshes. The difference is in how you
specify elements in the command. Instead of specifying volumes or surfaces you would specify groups of hexes, faces,
tris, or tets. Examples are given below:
quality hex all
quality face all scaled jacobian
quality tet 1 to 100 draw mesh
Mesh refinement on a free mesh
Refinement for a free mesh is limited to refinement of mesh elements. Refinement may be accomplished by specifying
groups of mesh elements which to refine using the regular refinement options. For boundary elements, the refinement
scheme will use averaging methods to determine node placement, in the absence of a boundary geometry to define node
placement.
Cleaning up a free mesh
A free tet mesh may be cleaned up using the Cleanup Tet command. For example
cleanup tet all
#cleans up all tets
cleanup tet 1 to 1000
#cleans up all tets in the range [1,1000]
It is best to specify contiguous sets of elements for this command.
Assigning boundary conditions
Assigning boundary conditions on free meshes can be accomplished by explicitly specifying mesh elements, by creating a
sideset or block from the skin of a group of elements, or by creating groups based on feature angle using the seed
method. Once the group is created it is easy to assign it to a nodeset or sideset.
Trelis will respect block, nodeset, and sideset data that is associated with an imported free mesh, or disassociated mesh.
The following command sequence illustrates how the group seed operation could be used for assigning boundary
conditions on free meshes.
721
Trelis 15.0 User Documentation
##Creating blocks, nodesets and sidesets on free meshes
cylinder radius 3 z 12
volume 1 size 0.5
mesh volume 1
disassociate mesh from volume 1
delete volume 1
group 'mygroup1' add seed face 752 feature_angle 45
##Groups all faces on the cylindrical surface
group 'mygroup2' add seed face 752 feature_angle 45 divergence
##Groups only faces within 45 degrees of seed face
sideset 1 group mygroup1
sideset 2 group mygroup2
block 1 hex all
draw sideset 1
draw sideset 2
draw block 1
Figure 4. Grouping faces on free meshes using the seed method. The feature angle method is used on the left
with a feature angle of 45 degrees. On the right is the result if using the divergence method.
Even though boundary conditions can be defined directly only on geometry entities, these geometry-based BCs will be
maintained on the free mesh following the disassociate command. The following command line sequence illustrates this
capability.
##Respecting blocks, nodesets and sidesets in mesh elements after disassociation
brick x 10
mesh vol 1
sideset 1 surface 1
nodeset 1 curve 1
block 1 volume 1
disassociate mesh from volume 1
draw sideset 1
draw nodeset 1
draw block 1
722
Free Meshes
Skinning a free mesh
The skin command takes a list of mesh elements and returns the triangles and faces on the boundary of that group. The
group of elements returned from the command can be assigned to either a group, sideset, or block. Free meshes can be
skinned by specifying either a list of hexahedra, a list of tetrahedra, or a list of blocks.
Deleting free mesh elements
Typically meshes are deleted by specifying owning geometry. For free meshes, the meshes cannot be deleted in this
fashion. Instead, the mesh may be deleted using the Delete mesh command. The syntax is:
Delete Mesh
This command will delete all mesh entities in the entire model. To specify groups of elements for deletion, you can use the
individual deletion commands.
To delete a mesh on a specific entity
1.
2.
3.
4.
5.
On the Command Panel, click on Mesh.
Click on Hex, Tet, Quad, Tri, Edge or Node.
Click on the Delete action button.
Enter in the appropriate ID for the specified entity. This can also be done using the Pick Widget function.
Click Apply.
Delete {Node|Hex|Tet|Face|Tri} <id_range> [No_propagate]
When deleting elements, the default behavior will be that the child mesh entities will be deleted when they become
orphaned. For example, when a hex is deleted, if its faces, edges and vertices are no longer used by adjacent hex
elements, then they will also be deleted. The no_propagate option will leave any child mesh entities regardless if they
become orphaned.
Bottom-up element creation
Bottom-up mesh element creation methods are available for free meshes. The difference between element creation
methods for free meshes versus associated meshes is that the free meshes commands do not have a command option to
associate the elements with an owning body. Otherwise the commands are identical to mesh element creation commands
for associated meshes.
To create an element with free meshes
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh.
Click on Hex, Tet, Quad, Tri or Edge.
Click on the Create action button.
Enter the desired values for the appropriate Node ID(s). This can also be done using the Pick Widget function.
If available, deselect Assign to Geometry.
Click Apply.
Create Node <x> <y> <z>
Create {Hex|Tet|Tri|Face|Edge} Node <id_range>
Exporting free meshes
Free meshes can be exported as ExodusII files. All elements belonging to any block are exported. Any elements not
belonging to a block will not be exported (i.e. Trelis will not assign default blocks).
723
Trelis 15.0 User Documentation
724
Skinning a Mesh
The Skin command takes a range of hexahedra, tetrahedra, blocks, or volumes and generates a collection of triangles or
quadrilaterals on the exterior of the volumetric elements. This is the skin mesh.
To skin a mesh
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Mesh.
Click on Volume, Hex or Tet.
Click on the Volume Skin, Hex Skin or Tet Skin action button.
Enter the appropriate value(s) for Volume ID(s), Hex ID(s) or Tet ID(s). This can also be done using the Pick
Widget function.
Select the desired settings.
Click Apply.
Skin {Block|Volume} <range> [Individual] [Nomake]
Skin {Hex|Tet|Block|Volume} <range> [Nomake]
Skin {Hex|Tet|Block|Volume} <range> [Make {Block|Sideset [<id>] |Group [<name>|<id>]}
Skin {Hex|Tet|Block|Volume} <range> {Add|Replace} {Block|Sideset [<id>] |Group [<name>|<id>]}
The Individual keyword tells Trelis to skin Blocks or Volumes, one by one independently of each other, even if they share
merged surfaces.
The Nomake keyword tells Trelis to not create any kind of grouping of the mesh faces resulting from the skinning
operation.
If the Make option and its arguments are present, then the specified object (block, sideset or group) receives the skin
mesh. The command fails if an object with the optional identifier already exists. If the object identifier is omitted, the
identifier is set to the next object of that type. The skin mesh is stored in the next available sideset if the Make option is
missing.
Another command form has two options, Add and Replace. Each option has a required, associated identifier. If the
identifier is missing or invalid, the command fails. The Add option appends the skin mesh to the object. The Replace
option removes any existing mesh from the object before adding the skin mesh.
The skin mesh will respect the merged volumes. If two adjacent volumes are merged, the skin mesh will not include the
merged surface. If the volumes are not merged, each volume will generate a separate skin surface. If volumes are not
merged, they are treated separately. The skin command will also respect any number of interior voids. All surface
elements will be oriented forward with respect to the originating volumes.
The primary use for the skin command is to generate surface meshes of quads or tris for sidesets and remeshing.
725
Element Block Specification
•
•
•
•
•
•
•
•
•
•
•
•
•
•
•
Creating Blocks
Assigning a Name or Description to an Element Block
Defining the Element Type
Default Element Blocks
Duplicate Block Elements
Assigning Attributes
Displaying Blocks
Deleting Blocks
Automatically Assigning Mesh Edges to a Block (Rebar)
Creating Spider Blocks
Creating Beam Blocks
Creating Spring Blocks
2d Elements
Mixed Element Output
Adding Materials to a Block
Element blocks are the method CUBIT uses to group related sets of elements into a single entity. Each element in an
element block must have the same basic and specific element type.
The preferred method for defining blocks is to use geometric entities such as volumes, surfaces or curves. Blocks can
also be defined using mesh entities. If a block is defined at a geometric entity, each of the elements owned by the
geometry are automatically assigned to the block. Deleting or remeshing the geometry automatically changes the set of
elements grouped into the block. If mesh entities are used to specify a block, deleting the mesh will also delete the
elements from the block.
Some important notes regarding Element Blocks are as follows:
•
•
•
•
Multiple volumes, surfaces, and curves can be contained in a single element block
A volume, surface, or curve can only be in one element block
Element Block id's are arbitrary and user-defined. They do not need to be in any contiguous sequence of
integers.
Element Blocks can be assigned a single floating point number, referred to as the block Attribute; this number is
used to represent the length or thickness of Bar and Shell elements, respectively. The attribute defaults to 1.0 if
not specified.
Creating Element Blocks
To define element blocks
1.
2.
3.
4.
5.
On the Command Panel, click on Analysis Groups and Materials and then Block.
Click on the Manage action button.
Enter the appropriate Block ID.
Specify the desired Entity Type and enter the ID(s). This can also be done using the Pick Widget function.
Click Apply.
To remove an entity type from element blocks
1.
2.
3.
4.
5.
On the Command Panel, click on Analysis Groups and Materials and then Block.
Click on the Delete action button.
Enter the appropriate Block ID.
Specify the desired Entity Type to Remove and enter the ID(s). This can also be done using the Pick Widget
function.
Click Apply.
Block <block_id> {Vertex | Curve | Surface | Volume} <range> [Remove]
727
Trelis 15.0 User Documentation
Block <block_id> {Hex|Tet|Pyramid|Face|Tri|Edge|Node} <range> [Remove]
Block <block_id> Group <range> [Remove]
The first command defines the block based on a list of geometric entities, while the second uses specific lists of mesh
entities. Since a block can only contain a single element type, usually entities of the same type are defined on the same
block. The third option provides for assigning groups of entities to a single block. This is useful, for example, when
several entities of the same type can be grouped together. The Block Group command simplifies the specification of the
block.
By using the Remove argument to the block command, the specified geometry or mesh entity can be removed from the
block definition.
When a mesh entity, or a meshed geometric entity is put into a block, it is assigned a Global Element ID which is exported
to the exodus file for tracking during analysis.
Assigning a Name or Description to an Element Block
The following commands can be used to assign a name or description to an element block. Assigning a name to a block
can be more intuitive than using traditional integer IDs, and the name and description are preserved in DART metadataenabled applications (like SIMBA). This command is also available for nodesets and sidesets.
Block<ids> Name "<new_name>"
Block<ids> Description "<description>"
Defining the Element Type
Each block must have a specific element type associated with it. To assign an element type to a block, use the following
command:
Block <block_id_range> Element Type <type>
Available element types are defined by the Exodus II file format specification (Schoof, 95). CUBIT supports the following
element types:
Nodes: SPHERE SPRING
Curves: BAR BAR2 BAR3 BEAM BEAM2 BEAM3 TRUSS TRUSS2 TRUSS3 SPRING
Surfaces: QUAD QUAD4 QUAD5 QUAD8 QUAD9 SHELL SHELL4 SHELL8 SHELL9 HEXSHELL
TRI TRI3 TRI6 TRI7 TRISHELL TRISHELL3 TRISHELL6 TRISHELL7
Volumes: HEX HEX8 HEX9 HEX20 HEX27 PYRAMID TETRA TETRA4 TETRA8 TETRA10
TETRA14
If the element type is not assigned for an element block, it will be assigned a default type depending on which type of
geometry entity is contained in the block. The default values used for element type are:
Volume: 8-node hexahedral elements (HEX8) will be generated for hex meshes. TETRA4 will be
generated for tet meshes.
Surface: 4-node shell elements (SHELL4) will be generated for quad meshes and TRISHELL3 for tri
meshes.
Curve: 2-node bar elements (BAR2) will be generated.
Node: 1-node elements (SPHERE) will be generated.
Higher order nodes are moved to curved geometry by default. To change this, use the following command:
728
Element Block Specification
set Node Constraint [ON|off|smart]
On means higher order nodes snap to curved geometry. Off means the nodes retain their positions. “smart” means
higher order nodes will only snap to geometry if they do not cause quality problems after being moved. Nodes that cannot
be moved without causing quality problems are placed at the average location of the element nodes: for edges, this
means on the line containing the edge; for 2d elements, this usually means on the plane containing the element. Several
examples of specifying various types of element blocks are given in the Appendix.
Default Element Blocks
When exporting an ExodusII file, if the user has not specified any Element Blocks, by default element blocks will be
written for any meshed volumes. This default behavior can be changed, to write surface, volume, or no meshes by default.
This option can be set using the command
Set Default Block [ON|off|Volume|Surface]
Default behavior, ON, is for the blocks to automatically be written based on their owning geometry. When the OFF setting
is used, only the mesh contained in blocks created by the user will be exported. Mesh not in an element block at export
time, will not be exported. The export will still succeed and no error will be thrown. If Volume is specified, only elements
contained in volumes will have default blocks specified. Similarly, the Surface argument indicates that only surfaces
containing elements will use default blocks.
When default blocks are used, the IDs for the resulting blocks will be defined as follows based upon the type of geometry:
Volume: The default block ID will be set to the Volume ID
Surface: The block ID will be set to 0
Curve: The block ID will be set to
Duplicate Block Elements
By default, any given element cannot be included in more than one block. However, when using the following command,
an element may be included in more than one block. Please note, since material properties are assigned to blocks, using
this command to allow duplicate block elements may result in an element being assigned to multiple materials.
Set Duplicate Block Elements {on|OFF}
Assigning Attributes to Blocks
It may be necessary to associate attributes with a specific element block. Attributes are generally integer or floating point
values that represent some physical property in the region occupied by the block, such as material properties or shell
thickness. To assign an attribute to an element block, use the following command:
Block <block_id_range> Attribute <value>
The default number of attributes of an element block is dependent on the element type of the element block. Except for
the element blocks of the element types below, all element blocks contain zero attributes by default.
Element Type
Number Default Attributes
SPHERE
1
BAR
3
729
Trelis 15.0 User Documentation
BEAM
7
TRUSS
1
SPRING
1
SHELL
1
TRISHELL
1
To assign more attributes than the number of default attributes use the following command:
Block <id_range> Attribute Count <1-20>
CUBIT will store up to 20 attributes per block. Specify the maximum number of attributes to be stored on the block with
this command. Once this command has been executed, individual attributes may be set using the following command:
Block <id_range> Attribute Index <index> <value>
The index is an integer from 1 to the maximum count specified in the Block Attribute Count command. The value may be
any valid floating point number.
Displaying Element Blocks
Blocks can be viewed individually with CUBIT by employing the following command:
Draw Block <block_id_range> [Color <color_spec>] [add] [thickness [offset [scale <val>] |
include_normal]]
For blocks that are of type SHELL and TRISHELL or one of its variants including the [thickness] keyword and parameters
will result in the blocks being color-coded by shell thickness with a corresponding color bar. Blocks can be drawn with
their specified thickness, so they visually have a thickness. This thickness can also be scaled in the draw command.
Arrows defining the shell normal direction will be displayed as well as a legend showing the thickness values.
Block colors can also be changed using the following command:
Color Block <block_id_range> {color|Default}
Deleting Element Blocks
All Nodesets, Sidesets and Blocks may be deleted from the model using the following command:
Reset Genesis
To remove only Blocks, the following may be used:
Reset Block
To remove a specific block, use:
730
Element Block Specification
Delete Block <block_id_range>
Automatically Assigning Mesh Edges to a Block (Rebar)
After a mesh has been defined within a volume, it may be useful to use the existing mesh edges as the basis for an
element block. Such an element block might be composed of bars or truss type elements that might propagate through a
solid medium such as rebar placed in reinforced concrete. Although the Block <id> Edge <range> command could be
used for this task, it would prove extremely tedious defining the individual edges to add to the block. To make this process
easier, the following command can be used:
Rebar Start <x> <y> <z> Direction <x> <y> <z> [Length <value>] Block <id> [Element Type
{bar|bar2|bar3|BEAM|beam2|beam3|truss|truss2|truss3}]
The Rebar command allows the user to specify a starting location for a set of edges and an initial direction. The program
will find the closest existing node in the mesh to Start <x> <y> <z> and begin propagating through the mesh in the
specified Direction <x> <y> <z>, adding edges to the block as it propagates through the mesh. The edge that is attached
to the last node and is within a fixed 30 degrees of the specified direction is added to the block. The Propagation of the
edges continues until either the optional Length value is reached or an edge does not meet the Direction criteria. Also
required with this command is a block ID. An Element Type can also be specified.
Similarly, you can use the following command which will use the 30 degree cone described above to gather edges from a
surface into a single block using the Cartesian x, y, and/or z vectors.
Rebar Surface <range> [x] [y] [z] Block <id> [Element Type
{bar|bar2|bar3|BEAM|beam2|beam3|truss|truss2|truss3}] [Propagate]
Diagonal and Orthogonal Rebar Blocks
Another method for generating rebar blocks include the Diagonal/Orthogonal option. This command can only be used on
surfaces that have been meshed with the mapping scheme. This command will create a block of edges from the mapped
mesh by starting in one corner and gathering edges orthogonally, or creating new edges diagonally based on the option
specified, using the parametric coordinate system dictated by the mapping scheme on the surface. The spacing option
dictates how many edges are skipped over before starting the next set of rebar edges.
Rebar Surface <range> {Diagonal|Orthogonal} [Spacing <int>] [Block <id> [Element Type
{bar|bar2|bar3|BEAM|beam2|beam3|truss}]
731
Trelis 15.0 User Documentation
CUBIT> rebar surf 1 diagonal spacing 2 block 2
CUBIT> rebar surf 1 orthogonal spacing 3 block 3
Specifying a set of nodes
A final rebar option allows the user to create or group rebar edges into a specified block using nodes. Edges are created,
or gathered, using the ordered list of nodes specified in the command.
Rebar Node <range> [Target Block <id>] [Element Type {bar|bar2|bar3|BEAM|beam2|beam3|truss}]
732
Element Block Specification
CUBIT> rebar node 113 105 97 89 81 73 65 57 49 target block 1
A related command for creating curve geometry directly from mesh edges is the Create Curve from Mesh command. See
Curve creation for more details.
Creating Spider Blocks
The block creation tool also allows the user to create a special block of bar elements that can be used as part of the
boundary specification. This command creates beam type elements directly without creating any underlying geometry.
The command for creating this type of block is:
Block <id> Joint {Vertex <id> | Node <id> }Spider {Surface|Curve|VertexFace|Tri|Node} <range>
[preview] [Element Type {bar|bar2|bar3|BEAM|beam2|beam3|truss|truss2|truss3}]
The joint node is the starting location of the bar elements and the spider location is the terminating location of the bar
elements. You can specify the terminating location as either a node, vertex, geometric surface or the face of a mesh
entity. Some analysis codes refer to these bar elements as tied contacts or rigid bar elements. They can be used to tie
models together or to enforce specific kinds of boundary conditions. For example, in the figure below a block of beam
elements is used to tie a node at the center of the circle to every node on the edge of the circle. This arrangement can be
used to enforce circularity but still allow for displacement of the entire circle. This may occur if there are additional
structures above the cylinder that are being excluded from the current finite element model. The beam elements were
created by a series of commands of the form
block 10 joint node 1 spider node 2
The preview option can be included to draw the location of the beam blocks on the screen without actually executing the
command.
When specifying vertex ids, please know the bar elements will be tied to the nodes associated with the vertex, not the
vertex itself.
733
Trelis 15.0 User Documentation
Figure 1. Beam elements created with the Spider command
Creating Beam Blocks
Properties for blocks that are beam types (beam, beam2, beam3) have additional commands to define a cross-sectional
area. The following command can be used to change the type of cross-sectional area of a beam block:
Block <id> beam_type {CIRCLE|box|rectangle|pipe|ibeam|general}
The dimensions are set by listing them after the keyword beam_dimensions:
Block <id> beam_dimensions <values>
The order in which the values need to be specified are described in the chart below.
If the solver used is to integrate over the section during the simulation, turn section_integration on using the following
command:
Block <id> section_integration {ON|off}
The beam normal vector is a vector normal to the plane of motion and tangent to the first bending axis. This vector can
be set using the following command:
Block <id> beam_normal <x><y><z>
Section Profile
Order to Specify Dimensions
Circle
Radius
Pipe
Outer radius, wall thickness
734
Element Block Specification
Rectangle
Width, height
Box
Total width, total height, thickness (right), thickness (top), thickness (left), thickness
(bottom)
I-Beam
Distance to bending axis (from bottom), total height, bottom width, top width, thickness
(bottom), thickness (top), thickness (web)
General
Area, Ixx, Ixy, Iyy, Polar moment of inertia (J)
Creating Spring Blocks
Spring blocks that will be exported to Abaqus can contain additional properties related to Abaqus springs. Users can
specify the spring type, stiffness, and DOFs associated with Abaqus springs. The spring type mapping to Abaqus
elements is in the following table.
CUBIT Block Spring Type
Abaqus Element Type
Node_to_node
SPRINGA
Node_to_node
SPRING1
Node_to_ground_fixed
SPRING2
The spring type is set using the spring_type keyword. In order to use this command, the block must already have an
element type of “SPRING.” If a DOF is associated with a spring, the spring_dof_1 keyword is used to specify the DOF
on the first node and spring_dof_2 is used to specify the DOF on the second node (SPRING2 only).
Block <id> [spring_type {NODE_TO_NODE | node_to_node_fixed_axis | node_to_ground}] [stiffness <k>]
[spring_dof_1 <n>] [spring_dof_2 <n>]
2D Elements
CUBIT is a 3d mesh generator by default. Element types, by default, are respectively TRISHELL and SHELL for triangle
and quad elements. If a 2d mesh is desired, blocks types must be explicitly set to TRI or QUAD.
Example:
create brick x 10
surface 1 scheme trimesh
mesh surface 1
block 1 surface 1
block 1 element type tri
export mesh "mymesh.exo"
Sideset 1 will be based on the TRI and QUAD elements in blocks 1 and 2, with the side numbering referring to the edges
of the triangles and quads.
Mixed Element Output
The Set Block Mixed Output command controls the behavior of blocks containing different element types when exporting
in a file format that doesn't support blocks with mixed element types. If EXPLICIT, only elements of a type matching the
element block will be exported. If DEGENERATE, all elements will be exported in one block, but tets and pyramids will be
written as degenerate hexes, and triangles will be written as degenerate quads. If OFFSET, then new element blocks will
be created separating the types. Hex and Quad blocks retain the block id, whereas tets, triangle, pyramids and wedges
get put into other blocks. The ids of the other blocks are based on the block id plus the offset for that type. Those values
are set using the offset commands.
Set Block Mixed Element Output { OffSet | Degenerate | Explicit }
735
Trelis 15.0 User Documentation
Set Block Triangle Offset <value>
Set Block Tetrahedron Offset <value>
Set Block Pyramid Offset <value>
Adding Materials to a Block
Block <id> Material <id|'name'>
If a material is assigned to an element block, the material properties will be associated with the block's elements when the
mesh is exported. If no material is assigned to a block, a default material will be used during export.
736
Nodeset and Sideset Specification
•
•
•
•
•
•
•
•
Creating Nodesets and Sidesets
Assigning Names and Descriptions to Nodesets and Sidesets
Grouping Faces on a Surface into a Sideset
Deleting Nodesets and Sidesets
Displaying Nodesets and Sidesets
Nodeset Associativity Data
Equation-Controlled Distribution Factors
Nodesets/Sidesets/Blocks Behavior with Geometric Entity Copy
Boundary conditions such as constraints and loads are applied to the finite element model using nodesets or sidesets,
also known as Genesis entities. Rather than attempting to maintain specific boundary condition information, such as load,
temperature, constraint, etc., Genesis entities are the generic vehicle for the user to set up boundary conditions on the
model. Nodes, elements and element faces are instead grouped together and assigned unique IDs. Node, element and
face IDs assigned to Genesis entities can then be written to the Exodus II mesh file. Once imported to the intended
analysis application, the nodeset and sideset IDs can be appropriately interpreted as specific physical boundary
conditions.
The preferred method for creating Genesis entities is to assign vertices, curves, surfaces or volumes to a specific nodeset
or sideset ID. Any mesh entity owned by the geometric entity in a nodeset or sideset is automatically assigned to the
same nodeset or sideset. This allows greatest flexibility in generating and updating the finite element mesh. For example,
if a surface belongs to a specific sideset, remeshing the surface will automatically delete any old faces from the sideset
and add the faces of the new mesh.
In some cases, the geometric model does not provide enough resolution to define the desired boundary conditions. In this
case, the model may be partitioned using Trelis' virtual geometry features. Where this may not be feasible, mesh entities
can also be added directly to the desired nodeset or sideset. Where individual mesh entities have been added to nodesets
or sidesets, deleting the mesh will also remove these elements from the Genesis entity. If the geometry is remeshed, the
new mesh entities must also be added once again to the nodesets or sidesets.
Nodesets can be created from groups of nodes categorized by their owning volumes, surfaces, curves or vertex.
Individual nodes may also be added to a nodeset. Nodes can belong to more than one nodeset.
Sidesets can be created from groups of element sides or faces categorized by their owning surfaces or curves or by their
individual face IDs. Element sides and faces can also belong to more than one sideset.
Creating Nodesets and Sidesets
Nodesets and Sidesets are created in Trelis by assigning the appropriate geometry or mesh entities in the model to a
nodeset or sideset ID.
To create a nodeset
1.
2.
3.
4.
5.
On the Command Panel, click on Analysis Groups and Materials and then Nodeset.
Click on the Manage action button.
Select Add from the drop-down menu.
Enter the appropriate settings.
Click Apply.
To remove a nodeset
1.
2.
3.
4.
5.
On the Command Panel, click on Analysis Groups and Materials and then Nodeset.
Click on the Delete action button.
Enter the appropriate value for Nodeset ID.
Select the Entity Type to Remove and the appropriate ID(s).
Click Apply.
Nodeset <nodeset_id> {Curve | Surface | Volume | Vertex | Node} <range> [Remove]
737
Trelis 15.0 User Documentation
To create a sideset
1.
2.
3.
4.
5.
On the Command Panel, click on Analysis Groups and Materials and then Sideset.
Click on the Manage action button.
Select Add from the drop-down menu.
Enter the appropriate settings.
Click Apply.
To remove a sideset
1.
2.
3.
4.
5.
On the Command Panel, click on Analysis Groups and Materials and then Sideset.
Click on the Delete action button.
Enter the appropriate value for Sideset ID.
Select the Entity Type to Remove and the appropriate ID(s).
Click Apply.
Sideset <sideset_id> Group <id_range> [remove]
Sideset <sideset_id> {Curve|Surface|Edge|Face|Tri} <id_range> Remove
Sideset <sideset_id> Edge <id_range> [wrt {{Tri|Face} <id_range> | all } ]
Sideset <sideset_id> Face <id_range> [wrt {Hex <id_range> | all} ]
Sideset <sideset_id> Tri <id_range> [wrt {Tet <id_range> | all} ]
Sideset <sideset_id> Surface <id_range> [wrt {{Volume|Surface} <id_range> | all} ]
[FORWARD|Reverse|Both]
Sideset <sideset_id> Curve <id_range> [wrt {Surface <id_range> | all} ]
Like element blocks, Nodesets and Sidesets are given arbitrary, user-defined ID numbers. If there are no user-defined
Nodesets or Sidesets, none are written to the Exodus II file.
With Sidesets, direction is often important. For surfaces, the direction may be specified using the Forward, Reverse, or
Both options. The Forward option will write a sideset in relation to hexes in the surface's forward volume, which is the
volume that the surface's normal points away from. The Reverse option will write a sideset in relation to hexes in the
surface's reverse volume, which is the volume that the surface's normal points into. The Both option will allow sidesets to
be written in relation to the hexes that lie in volumes on both sides of the surface. The default is Forward. The user can
additionally specify the volume from which the hexes should be taken in relation to by using the wrt Volume option.
Direction is equally important for curves in Sidesets. The wrt Surface option allows the user to indicate which surface's
faces will be included in the Sideset. The wrt All option will include all faces attached to the curve. The default is wrt All.
Useful hint:
When creating nodesets and sidesets it is often userful to use the Extended Command Line Entity Specification. Here is
an example that creates a nodeset which includes all the nodes on the exterior of the geometry:
# Create the geometry
Create brick x 10
Create cylinder height 10 radius 2
Move volume 2 z 10
# Merge the geometry
Merge volume all
# Mesh the geometry
Mesh volume all
# Create a nodeset that includes only those nodes
# located on the exterior of the geometry
Nodeset 1 surface in volume all with not is_merged
The following commands remove nodes from the nodeset that belong to a surface. Continuing from the previous example:
738
Nodeset and Sideset Specification
# Remove surface 2 from the nodeset
Nodeset 1 surface 2 remove
# Remove nodes from the nodeset
# that belong to the curves that bound surface 2
Nodeset 1 node in curve in surface 2 remove
Nodes can also be added or removed based upon their coordinates. Here is an example that removes all the nodes with a
z coordinate equal to 15. Continuing from the previous example:
# Remove the nodes with a z coordinate equal to 15
Nodeset 1 node in surface all with z_coord = 15 remove
Assigning Names and Descriptions to Nodesets and Sidesets
Nodesets and sidesets can be assigned names and descriptions. Using names and descriptions is often more intuitive
than using traditional integer IDs. When exporting a mesh as a DART artifact, names and descriptions are included in the
metadata, making them available to DART metadata-enabled applications such as SIMBA. To give a name or description
to nodeset or sideset, use one of the following commands:
{Nodeset|Sideset} <ids> Name "<new_name>"
{Nodeset|Sideset} <ids> Description "<description>"
This command can also be used to define names and descriptions for Element Blocks.
Grouping Faces on a Surface into a Sideset
To create sideset from a subset of the faces on a given surface
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Analysis Groups and Materials and then Sideset.
Click on the Manage action button.
Select Patch from the drop-down menu.
Enter the appropriate value(s) fro SideSet ID and Surface ID. This can also be done using the Pick Widget
function.
Select Define Bounding Box or Define Bounding Circle.
Enter the appropriate settings.
Click Apply.
SideSet <sideset_id> Surface <id_range> Patch Maximum <x> <y> <z> Minimum <x> <y> <z>
SideSet <sideset_id> Surface <id_range> Patch Center <x> <y> <z> Radius <value> [Filter]
[Partition]
SideSet <sideset_id> Surface <id_range> Patch Center <x> <y> <z> Outer_radius <value>
Inner_radius <value> [Filter] [Partition]
SideSet <sideset_id> Surface <id_range> Patch Cylinder <axis_specification> Radius <rad> [Filter]
[Partition]
SideSet <sideset_id> Surface <id_range> Patch Cylinder <axis_specification> Outer_radius <rad>
Inner_radius <rad> [Filter] [Partition]
These commands place only the faces meeting the specified criteria into the sideset.
•
Using the maximum and minimum options will include all faces on the surface whose centroid falls within the
axis-aligned box defined by the maximum and minimum points.
739
Trelis 15.0 User Documentation
•
•
•
•
Using the center and radius options will include all faces on the surface whose centroid falls within the sphere
defined by center and radius.
Using the center, outer_radius, and inner_radius options will include all faces on the surface whose centroid
falls within the sphere defined by center and outer_radius, but excluding those faces whose centroid falls within
the sphere defined by center and inner_radius. In other words, a face will be included if the distance between
the face and the center point is between inner_radius and outer_radius.
Using the cylinder option will include all faces whose centroid falls within a cylinder of infinite length with the
given axis and radius. The axis is specified as described in Specifying an Axis.
Using the optional inner_radius will exclude those faces whose centroid is closer to the axis than the specified
inner_radius.
Normally, these commands place the individual elements into the sideset. If the mesh on the surface is deleted, the
elements will be removed from the sideset. If the surface is then remeshed, new elements will NOT automatically be
added to the sideset. This is usually the intended behavior.
If the filter option is included, only a single connected set of elements is added to the sideset. If the shape of the surface
is such that multiple disconnected sets of elements fall within the specified spherical or cylindrical region, the filter option
will limit the faces added to the sideset to the one set closest to center.
Using the partition option changes this behavior. The partition option causes the surface to be split, based on the faces
included in the patch. The newly created patch surface will be added to the sideset instead of the individual elements. If
the mesh is deleted and a new mesh is generated, the new mesh on the patch surface will automatically be included in
the sideset, just as occurs with other geometric entities assigned to sidesets.
Note that the sideset patch commands work with both triangular and quadrilateral faces.
Grouping elements in voids and enclosures
The sideset start enclosure command creates sidesets of monotonically increasing ID numbers containing the elements
comprising the watertight skin of the input elements. When there's a 'void' in the middle of the elements, a region devoid
of elements, though still enclosed by elements, this enclosed region will also have a sideset defined on the skin of the
enclosed region.
To group elements in voids and enclosures
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Analysis Groups and Materials and then Sideset.
Click on the Manage action button.
Select Enclosure from the drop-down menu.
Enter the appropriate value for Sideset Starting ID. This can also be done using the Pick Widget function.
Select the desired Entity of Enclosure and enter the appropriate value.
Click Apply.
Sideset Start <id> Enclosure {Volume|Hex|Tet} <range>
The start id is the id of the sideset at which to start. The ID numbers will increase monotonically unless there is a
conflicting ID number. The command will add as many sidesets as there are fully continuous regions or tris or faces in the
input group. This function can be particularly helpful for calculations for radiation enclosures.
Deleting Nodesets and Sidesets
All Nodesets, Sidesets and Blocks may be deleted from the model using the following command:
Reset Genesis
To remove only nodesets or sidesets, the following may be used:
Reset Nodeset
740
Nodeset and Sideset Specification
Reset Sideset
To remove a specific nodeset or sideset, use:
Delete Nodeset <nodeset_id_range>
Delete Sideset <sideset_id_range>
Displaying Nodesets and Sidesets
To view Nodesets and Sidesets individually
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Analysis Groups and Materials.
Click on Nodeset or Sideset.
Click on the Manage action button.
Select Draw from the drop-down menu.
Enter the appropriate settings.
Click Apply.
Draw NodeSet <nodeset_id_range> [Color <color_spec>] [add]
Draw SideSet <sideset_id_range> [Color <color_spec>] [add]
To change the colors for Nodesets and Sidesets
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Analysis Groups and Materials.
Click on Nodeset or Sideset.
Click on the Manage action button.
Select Color from the drop-down menu.
Enter the appropriate settings.
Click Apply.
Color NodeSet <nodeset_id_range> {color|Default}
Color SideSet <sideset_id_range> {color|Default}
Nodeset Associativity Data
Nodesets can be used to store geometry associativity data in the Exodus II file. This data can be used to associate the
corresponding mesh to an existing geometry in a subsequent Trelis session. This functionality can be used either to
associate a previously-generated mesh with a geometry (See Importing an Exodus II File), or to associate a field function
with a geometry for adaptive surface meshing (See Adaptive Meshing).
The commands to control and list whether associativity data is written or read from an Exodus II files are the following:
List Import Mesh NodeSet Associativity
List [Export Mesh] NodeSet Associativity
List [Export Mesh] NodeSet Associativity Complete
set Import Mesh NodeSet Associativity [ON|off]
[set] [Export Mesh] NodeSet Associativity [on|OFF]
741
Trelis 15.0 User Documentation
[set] [Export Mesh] NodeSet Associativity Complete [On|OFF]
Associativity data is stored in the Exodus II file in two locations. First, a nodeset is written for each piece of geometry
(vertices, curves, etc) containing the nodes owned for that geometry. Then, the name of each geometry entity is
associated with the corresponding nodeset by writing a property name and designating the corresponding nodeset as
having that property. Nodeset numbers used for associativity nodesets are determined by adding a fixed base number
(depending on the order of the geometric entity) to the geometric entity id number. The base numbers for various orders
of geometric entities are shown in the following table. For example, nodes owned by curve number 26 would be stored in
associativity nodeset 40026.
Table 1. Nodeset ID base numbers for geometric entities
Geometric Entity
Base Nodeset ID
Vertex
50000
Curve
40000
Surface
30000
Volume
20000
Instead of storing just the nodes owned by a particular entity, nodes for lower order entities are also stored. For example,
the associativity nodeset for a surface would contain all nodes owned by that surface as well as the nodes on the
bounding curves and vertices.
Equation-Controlled Distribution Factors
By default, distribution factors on nodesets or sidesets are written with a constant value of "1" at each node. It is also
possible to vary the distribution factor for each node in a nodeset or sideset, using an equation to control the value of the
distribution factor at each node. To do so, an equation must first be defined using the command:
Create Equation "<expression>" name "<name>"
where expression is any mathematical expression which evaluates to a single number, and name is the name by which
this equation will be known. The expression is written using aprepro syntax, with a few differences from the use of
APREPRO in its usual context.
1.
2.
The expression as a whole is not wrapped in curly braces "{" and"}".
The expression may include any of the following pre-defined variables:
{x} - The x-coordinate of the current node
{y} - The y-coordinate of the current node
{z} - The z-coordinate of the current node
{n} - The Trelis ID of the current node. This is the ID of the node in Trelis, which may not be the same
as the node's ID in the Exodus II file.
For example, to define an equation which varies from -10 to 10 based on the sine of the node's x_coordinate:
Create Equation "10*sin({x})" Name "my_equation"
Once an equation has been defined, it can be applied to a nodeset or sideset:
{Nodeset|Sideset} <id> Distribution Equation "<equation_name>"
For example, to apply the equation created earlier to nodeset 10:
Nodeset 10 Distribution Equation "my_equation"
742
Nodeset and Sideset Specification
When nodeset 10 is written to an Exodus II file, "my_equation" will be evaluated once for each node in the nodeset, with
the values of {x}, {y}, {z}, and {n} set to appropriate values for the node. The result is used as the distribution factor for that
node.
Here is a complete example that writes out the distribution factors 0.0, 0.5, and 1.0 for the 3 nodes on the curve:
# Create a straight line from (0,0,0) to (1,0,0)
create vertex 0 0 0
create vertex 1 0 0
create curve vertex 1 2
# Mesh with 3 nodes
curve 1 interval 2
mesh curve 1
# Create a block and a nodeset
block 1 curve 1
nodeset 1 curve 1
# Define an equation and apply it to the nodeset
create equation "{x}" name "simple_eq"
nodeset 1 distribution equation "simple_eq"
# Write the mesh
export mesh "temp.g" overwrite
Here is another complete example that varies the distribution factors for sideset 20 from zero to 1, depending on the
node's x-coordinate. The sideset is applied to sides of HEX20 elements, so each element side has 8 different distribution
factors.
# Mesh a cube
brick x 10
mesh volume 1
# Create a block of 20-noded hexes
block 1 volume 1
block 1 element type hex20
# Apply a sideset to be used for a variable pressure
sideset 20 surface 1
# Define an equation and apply it to the sideset
create equation "({x}+5)/10" name "zero_to_one"
sideset 20 distribution equation "zero_to_one"
# Write the mesh
export mesh "temp.g" overwrite
Note that distribution equations only affect Exodus II output. Equations are currently ignored for other mesh file types.
See APREPRO in the appendix.
Nodesets/Sidesets/Blocks Behavior with Geometric Entity Copy
The below commands can be used set the behavior of nodesets/sideset/blocks when a copy command is applied on
geometric entities. The default OFF option states that the nodesets/sideset/blocks will not be copied to new geometric
entity if the original geometric entity contains nodesets/sideset/blocks. The "on" option implies that the
nodesets/sideset/blocks present in the original geometric entity will be copied to new geometric entity. The use_original
option indicates that the new geometric entities created after the copy command will have the nodesets/sidesets/blocks
present in the original geometric entities.
set copy_nodeset_on_geometry_copy [on | OFF| use_original]
set copy_sideset_on_geometry_copy [on | OFF| use_original]
set copy_block_on_geometry_copy [on | OFF| use_original]
743
Nodeset and Sideset Specification
•
•
•
•
•
•
•
•
Creating Nodesets and Sidesets
Assigning Names and Descriptions to Nodesets and Sidesets
Grouping Faces on a Surface into a Sideset
Deleting Nodesets and Sidesets
Displaying Nodesets and Sidesets
Nodeset Associativity Data
Equation-Controlled Distribution Factors
Nodesets/Sidesets/Blocks Behavior with Geometric Entity Copy
Boundary conditions such as constraints and loads are applied to the finite element model using nodesets or sidesets,
also known as Genesis entities. Rather than attempting to maintain specific boundary condition information, such as load,
temperature, constraint, etc., Genesis entities are the generic vehicle for the user to set up boundary conditions on the
model. Nodes, elements and element faces are instead grouped together and assigned unique IDs. Node, element and
face IDs assigned to Genesis entities can then be written to the Exodus II mesh file. Once imported to the intended
analysis application, the nodeset and sideset IDs can be appropriately interpreted as specific physical boundary
conditions.
The preferred method for creating Genesis entities is to assign vertices, curves, surfaces or volumes to a specific nodeset
or sideset ID. Any mesh entity owned by the geometric entity in a nodeset or sideset is automatically assigned to the
same nodeset or sideset. This allows greatest flexibility in generating and updating the finite element mesh. For example,
if a surface belongs to a specific sideset, remeshing the surface will automatically delete any old faces from the sideset
and add the faces of the new mesh.
In some cases, the geometric model does not provide enough resolution to define the desired boundary conditions. In this
case, the model may be partitioned using Trelis' virtual geometry features. Where this may not be feasible, mesh entities
can also be added directly to the desired nodeset or sideset. Where individual mesh entities have been added to nodesets
or sidesets, deleting the mesh will also remove these elements from the Genesis entity. If the geometry is remeshed, the
new mesh entities must also be added once again to the nodesets or sidesets.
Nodesets can be created from groups of nodes categorized by their owning volumes, surfaces, curves or vertex.
Individual nodes may also be added to a nodeset. Nodes can belong to more than one nodeset.
Sidesets can be created from groups of element sides or faces categorized by their owning surfaces or curves or by their
individual face IDs. Element sides and faces can also belong to more than one sideset.
Creating Nodesets and Sidesets
Nodesets and Sidesets are created in Trelis by assigning the appropriate geometry or mesh entities in the model to a
nodeset or sideset ID.
To create a nodeset
1.
2.
3.
4.
5.
On the Command Panel, click on Analysis Groups and Materials and then Nodeset.
Click on the Manage action button.
Select Add from the drop-down menu.
Enter the appropriate settings.
Click Apply.
To remove a nodeset
1.
2.
3.
4.
5.
On the Command Panel, click on Analysis Groups and Materials and then Nodeset.
Click on the Delete action button.
Enter the appropriate value for Nodeset ID.
Select the Entity Type to Remove and the appropriate ID(s).
Click Apply.
Nodeset <nodeset_id> {Curve | Surface | Volume | Vertex | Node} <range> [Remove]
745
Trelis 15.0 User Documentation
To create a sideset
1.
2.
3.
4.
5.
On the Command Panel, click on Analysis Groups and Materials and then Sideset.
Click on the Manage action button.
Select Add from the drop-down menu.
Enter the appropriate settings.
Click Apply.
To remove a sideset
1.
2.
3.
4.
5.
On the Command Panel, click on Analysis Groups and Materials and then Sideset.
Click on the Delete action button.
Enter the appropriate value for Sideset ID.
Select the Entity Type to Remove and the appropriate ID(s).
Click Apply.
Sideset <sideset_id> Group <id_range> [remove]
Sideset <sideset_id> {Curve|Surface|Edge|Face|Tri} <id_range> Remove
Sideset <sideset_id> Edge <id_range> [wrt {{Tri|Face} <id_range> | all } ]
Sideset <sideset_id> Face <id_range> [wrt {Hex <id_range> | all} ]
Sideset <sideset_id> Tri <id_range> [wrt {Tet <id_range> | all} ]
Sideset <sideset_id> Surface <id_range> [wrt {{Volume|Surface} <id_range> | all} ]
[FORWARD|Reverse|Both]
Sideset <sideset_id> Curve <id_range> [wrt {Surface <id_range> | all} ]
Like element blocks, Nodesets and Sidesets are given arbitrary, user-defined ID numbers. If there are no user-defined
Nodesets or Sidesets, none are written to the Exodus II file.
With Sidesets, direction is often important. For surfaces, the direction may be specified using the Forward, Reverse, or
Both options. The Forward option will write a sideset in relation to hexes in the surface's forward volume, which is the
volume that the surface's normal points away from. The Reverse option will write a sideset in relation to hexes in the
surface's reverse volume, which is the volume that the surface's normal points into. The Both option will allow sidesets to
be written in relation to the hexes that lie in volumes on both sides of the surface. The default is Forward. The user can
additionally specify the volume from which the hexes should be taken in relation to by using the wrt Volume option.
Direction is equally important for curves in Sidesets. The wrt Surface option allows the user to indicate which surface's
faces will be included in the Sideset. The wrt All option will include all faces attached to the curve. The default is wrt All.
Useful hint:
When creating nodesets and sidesets it is often userful to use the Extended Command Line Entity Specification. Here is
an example that creates a nodeset which includes all the nodes on the exterior of the geometry:
# Create the geometry
Create brick x 10
Create cylinder height 10 radius 2
Move volume 2 z 10
# Merge the geometry
Merge volume all
# Mesh the geometry
Mesh volume all
# Create a nodeset that includes only those nodes
# located on the exterior of the geometry
Nodeset 1 surface in volume all with not is_merged
The following commands remove nodes from the nodeset that belong to a surface. Continuing from the previous example:
746
Nodeset and Sideset Specification
# Remove surface 2 from the nodeset
Nodeset 1 surface 2 remove
# Remove nodes from the nodeset
# that belong to the curves that bound surface 2
Nodeset 1 node in curve in surface 2 remove
Nodes can also be added or removed based upon their coordinates. Here is an example that removes all the nodes with a
z coordinate equal to 15. Continuing from the previous example:
# Remove the nodes with a z coordinate equal to 15
Nodeset 1 node in surface all with z_coord = 15 remove
Assigning Names and Descriptions to Nodesets and Sidesets
Nodesets and sidesets can be assigned names and descriptions. Using names and descriptions is often more intuitive
than using traditional integer IDs. When exporting a mesh as a DART artifact, names and descriptions are included in the
metadata, making them available to DART metadata-enabled applications such as SIMBA. To give a name or description
to nodeset or sideset, use one of the following commands:
{Nodeset|Sideset} <ids> Name "<new_name>"
{Nodeset|Sideset} <ids> Description "<description>"
This command can also be used to define names and descriptions for Element Blocks.
Grouping Faces on a Surface into a Sideset
To create sideset from a subset of the faces on a given surface
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on Analysis Groups and Materials and then Sideset.
Click on the Manage action button.
Select Patch from the drop-down menu.
Enter the appropriate value(s) fro SideSet ID and Surface ID. This can also be done using the Pick Widget
function.
Select Define Bounding Box or Define Bounding Circle.
Enter the appropriate settings.
Click Apply.
SideSet <sideset_id> Surface <id_range> Patch Maximum <x> <y> <z> Minimum <x> <y> <z>
SideSet <sideset_id> Surface <id_range> Patch Center <x> <y> <z> Radius <value> [Filter]
[Partition]
SideSet <sideset_id> Surface <id_range> Patch Center <x> <y> <z> Outer_radius <value>
Inner_radius <value> [Filter] [Partition]
SideSet <sideset_id> Surface <id_range> Patch Cylinder <axis_specification> Radius <rad> [Filter]
[Partition]
SideSet <sideset_id> Surface <id_range> Patch Cylinder <axis_specification> Outer_radius <rad>
Inner_radius <rad> [Filter] [Partition]
These commands place only the faces meeting the specified criteria into the sideset.
•
Using the maximum and minimum options will include all faces on the surface whose centroid falls within the
axis-aligned box defined by the maximum and minimum points.
747
Trelis 15.0 User Documentation
•
•
•
•
Using the center and radius options will include all faces on the surface whose centroid falls within the sphere
defined by center and radius.
Using the center, outer_radius, and inner_radius options will include all faces on the surface whose centroid
falls within the sphere defined by center and outer_radius, but excluding those faces whose centroid falls within
the sphere defined by center and inner_radius. In other words, a face will be included if the distance between
the face and the center point is between inner_radius and outer_radius.
Using the cylinder option will include all faces whose centroid falls within a cylinder of infinite length with the
given axis and radius. The axis is specified as described in Specifying an Axis.
Using the optional inner_radius will exclude those faces whose centroid is closer to the axis than the specified
inner_radius.
Normally, these commands place the individual elements into the sideset. If the mesh on the surface is deleted, the
elements will be removed from the sideset. If the surface is then remeshed, new elements will NOT automatically be
added to the sideset. This is usually the intended behavior.
If the filter option is included, only a single connected set of elements is added to the sideset. If the shape of the surface
is such that multiple disconnected sets of elements fall within the specified spherical or cylindrical region, the filter option
will limit the faces added to the sideset to the one set closest to center.
Using the partition option changes this behavior. The partition option causes the surface to be split, based on the faces
included in the patch. The newly created patch surface will be added to the sideset instead of the individual elements. If
the mesh is deleted and a new mesh is generated, the new mesh on the patch surface will automatically be included in
the sideset, just as occurs with other geometric entities assigned to sidesets.
Note that the sideset patch commands work with both triangular and quadrilateral faces.
Grouping elements in voids and enclosures
The sideset start enclosure command creates sidesets of monotonically increasing ID numbers containing the elements
comprising the watertight skin of the input elements. When there's a 'void' in the middle of the elements, a region devoid
of elements, though still enclosed by elements, this enclosed region will also have a sideset defined on the skin of the
enclosed region.
To group elements in voids and enclosures
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Analysis Groups and Materials and then Sideset.
Click on the Manage action button.
Select Enclosure from the drop-down menu.
Enter the appropriate value for Sideset Starting ID. This can also be done using the Pick Widget function.
Select the desired Entity of Enclosure and enter the appropriate value.
Click Apply.
Sideset Start <id> Enclosure {Volume|Hex|Tet} <range>
The start id is the id of the sideset at which to start. The ID numbers will increase monotonically unless there is a
conflicting ID number. The command will add as many sidesets as there are fully continuous regions or tris or faces in the
input group. This function can be particularly helpful for calculations for radiation enclosures.
Deleting Nodesets and Sidesets
All Nodesets, Sidesets and Blocks may be deleted from the model using the following command:
Reset Genesis
To remove only nodesets or sidesets, the following may be used:
Reset Nodeset
748
Nodeset and Sideset Specification
Reset Sideset
To remove a specific nodeset or sideset, use:
Delete Nodeset <nodeset_id_range>
Delete Sideset <sideset_id_range>
Displaying Nodesets and Sidesets
To view Nodesets and Sidesets individually
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Analysis Groups and Materials.
Click on Nodeset or Sideset.
Click on the Manage action button.
Select Draw from the drop-down menu.
Enter the appropriate settings.
Click Apply.
Draw NodeSet <nodeset_id_range> [Color <color_spec>] [add]
Draw SideSet <sideset_id_range> [Color <color_spec>] [add]
To change the colors for Nodesets and Sidesets
1.
2.
3.
4.
5.
6.
On the Command Panel, click on Analysis Groups and Materials.
Click on Nodeset or Sideset.
Click on the Manage action button.
Select Color from the drop-down menu.
Enter the appropriate settings.
Click Apply.
Color NodeSet <nodeset_id_range> {color|Default}
Color SideSet <sideset_id_range> {color|Default}
Nodeset Associativity Data
Nodesets can be used to store geometry associativity data in the Exodus II file. This data can be used to associate the
corresponding mesh to an existing geometry in a subsequent Trelis session. This functionality can be used either to
associate a previously-generated mesh with a geometry (See Importing an Exodus II File), or to associate a field function
with a geometry for adaptive surface meshing (See Adaptive Meshing).
The commands to control and list whether associativity data is written or read from an Exodus II files are the following:
List Import Mesh NodeSet Associativity
List [Export Mesh] NodeSet Associativity
List [Export Mesh] NodeSet Associativity Complete
set Import Mesh NodeSet Associativity [ON|off]
[set] [Export Mesh] NodeSet Associativity [on|OFF]
749
Trelis 15.0 User Documentation
[set] [Export Mesh] NodeSet Associativity Complete [On|OFF]
Associativity data is stored in the Exodus II file in two locations. First, a nodeset is written for each piece of geometry
(vertices, curves, etc) containing the nodes owned for that geometry. Then, the name of each geometry entity is
associated with the corresponding nodeset by writing a property name and designating the corresponding nodeset as
having that property. Nodeset numbers used for associativity nodesets are determined by adding a fixed base number
(depending on the order of the geometric entity) to the geometric entity id number. The base numbers for various orders
of geometric entities are shown in the following table. For example, nodes owned by curve number 26 would be stored in
associativity nodeset 40026.
Table 1. Nodeset ID base numbers for geometric entities
Geometric Entity
Base Nodeset ID
Vertex
50000
Curve
40000
Surface
30000
Volume
20000
Instead of storing just the nodes owned by a particular entity, nodes for lower order entities are also stored. For example,
the associativity nodeset for a surface would contain all nodes owned by that surface as well as the nodes on the
bounding curves and vertices.
Equation-Controlled Distribution Factors
By default, distribution factors on nodesets or sidesets are written with a constant value of "1" at each node. It is also
possible to vary the distribution factor for each node in a nodeset or sideset, using an equation to control the value of the
distribution factor at each node. To do so, an equation must first be defined using the command:
Create Equation "<expression>" name "<name>"
where expression is any mathematical expression which evaluates to a single number, and name is the name by which
this equation will be known. The expression is written using aprepro syntax, with a few differences from the use of
APREPRO in its usual context.
1.
2.
The expression as a whole is not wrapped in curly braces "{" and"}".
The expression may include any of the following pre-defined variables:
{x} - The x-coordinate of the current node
{y} - The y-coordinate of the current node
{z} - The z-coordinate of the current node
{n} - The Trelis ID of the current node. This is the ID of the node in Trelis, which may not be the same
as the node's ID in the Exodus II file.
For example, to define an equation which varies from -10 to 10 based on the sine of the node's x_coordinate:
Create Equation "10*sin({x})" Name "my_equation"
Once an equation has been defined, it can be applied to a nodeset or sideset:
{Nodeset|Sideset} <id> Distribution Equation "<equation_name>"
For example, to apply the equation created earlier to nodeset 10:
Nodeset 10 Distribution Equation "my_equation"
750
Nodeset and Sideset Specification
When nodeset 10 is written to an Exodus II file, "my_equation" will be evaluated once for each node in the nodeset, with
the values of {x}, {y}, {z}, and {n} set to appropriate values for the node. The result is used as the distribution factor for that
node.
Here is a complete example that writes out the distribution factors 0.0, 0.5, and 1.0 for the 3 nodes on the curve:
# Create a straight line from (0,0,0) to (1,0,0)
create vertex 0 0 0
create vertex 1 0 0
create curve vertex 1 2
# Mesh with 3 nodes
curve 1 interval 2
mesh curve 1
# Create a block and a nodeset
block 1 curve 1
nodeset 1 curve 1
# Define an equation and apply it to the nodeset
create equation "{x}" name "simple_eq"
nodeset 1 distribution equation "simple_eq"
# Write the mesh
export mesh "temp.g" overwrite
Here is another complete example that varies the distribution factors for sideset 20 from zero to 1, depending on the
node's x-coordinate. The sideset is applied to sides of HEX20 elements, so each element side has 8 different distribution
factors.
# Mesh a cube
brick x 10
mesh volume 1
# Create a block of 20-noded hexes
block 1 volume 1
block 1 element type hex20
# Apply a sideset to be used for a variable pressure
sideset 20 surface 1
# Define an equation and apply it to the sideset
create equation "({x}+5)/10" name "zero_to_one"
sideset 20 distribution equation "zero_to_one"
# Write the mesh
export mesh "temp.g" overwrite
Note that distribution equations only affect Exodus II output. Equations are currently ignored for other mesh file types.
See APREPRO in the appendix.
Nodesets/Sidesets/Blocks Behavior with Geometric Entity Copy
The below commands can be used set the behavior of nodesets/sideset/blocks when a copy command is applied on
geometric entities. The default OFF option states that the nodesets/sideset/blocks will not be copied to new geometric
entity if the original geometric entity contains nodesets/sideset/blocks. The "on" option implies that the
nodesets/sideset/blocks present in the original geometric entity will be copied to new geometric entity. The use_original
option indicates that the new geometric entities created after the copy command will have the nodesets/sidesets/blocks
present in the original geometric entities.
set copy_nodeset_on_geometry_copy [on | OFF| use_original]
set copy_sideset_on_geometry_copy [on | OFF| use_original]
set copy_block_on_geometry_copy [on | OFF| use_original]
751
Exodus II File Specification
Exodus II Manual
The full Exodus II manual is available from the web.
Element Block Definition Examples
Multiple Element Blocks
Multiple element blocks are often used when generating a finite element mesh. For example, if the finite element model
consists of a block which has a thin shell encasing the volume mesh, the following block commands would be used:
Block 100 Volume 1
Block 100 Element Type Hex8
Block 200 Surface 1 To 6
Block 200 Element Type Shell4
Block 200 Attribute 0.01
Mesh Volume 1
Export Genesis `block.g'
This sequence of commands defines two element blocks (100 and 200). Element block 100 is composed of 8-node
hexahedral elements and element block 200 is composed of 4-node shell elements on the surface of the block. The
"thickness" of the shell elements is 0.01. The finite element code which reads the Genesis file (block.g) would refer to
these blocks using the element block IDs 100 and 200. Note that the second line and the fourth line of the example are
not required since both commands represent the default element type for the respective element blocks.
Surface Mesh Only
If a mesh containing only the surface of the block is desired, the first two lines of the example would be omitted and the
Mesh Volume 1 line would be changed to, for example
Mesh Surface 1 To 6.
Two-dimensional Mesh
Trelis also provides the capability of writing two-dimensional Genesis databases similar to FASTQ. The user must first
assign the appropriate surfaces in the model to an element block. Then a Quad* type element may be specified for the
element block. For example
Block 1 Surface 1 To 4
Block 1 Element Type Quad4
In this case, it is important for users to note that a two-dimensional Genesis database will result. In writing a twodimensional Genesis database, Trelis ignores all z-coordinate data. Therefore, the user must ensure that the Element
Block is assigned to a planar surface lying in a plane parallel to the x-y plane. Currently, the Quad* element types are the
only supported two-dimensional elements. Two-dimensional shell elements will be added in the near future if required.
753
Exodus II Model Title
Trelis will automatically generate a default title for the Genesis database. The default title has the form:
Trelis(genesis_filename): date: time
The title can be changed using the command:
Title '<title_string>'
755
Exodus Coordinate Frames
Trelis allows the user to define coordinate systems (frames) that are written to an Exodus II file. These coordinate frames
are generally used as reference coordinate systems during analysis. In Trelis, the user may define multiple exodus
coordinate frames. When created, a coordinate frame is assigned an id. Exodus coordinate frames can be created using
x-y-z coordinates, nodes or vertices with the following commands:
Exodus Create Coordinate Frame
<xval> <yval> <zval>//origin
<xval> <yval> <zval> //z-axis
<xval> <yval> <zval> //xz-plane
[tag { 'R' | 'C' | 'S' } ]
Exodus Create Coordinate Frame Node
<node_origin_id>
<node_zaxis_id>
<node_xzplane_id>
[tag { 'R' | 'C' | 'S' } ]
Exodus Create Coordinate Frame Vertex
<vertex_origin_id>
<vertex_zaxis_id>
<vertex_xzplane_id>
[tag { 'R' | 'C' | 'S' } ]
Using the 'tag' option specifies the type of coordinate frame, i.e., rectangular (R), cylindrical (C) or spherical (S). The
default coordinate frame type is rectangular. Exodus coordinate frames may also be listed and deleted using the
commands below:
List Exodus Coordinate Frame [ids] [ <frame_id>]
Delete Exodus Coordinate Frame [ids] [ <frame_id>| all]
Any exodus coordinate frames that exist at the time the exodus file is exported will be written out in the exodus file.
757
Defining Materials and Media Types
Materials can be defined in Trelis and assigned to element blocks. If an element block is exported without a material
assigned to it, a default material (with properties for common steel) will be exported for it.
Creating and modifying materials can be done two ways
1.
2.
3.
4.
5.
On the Command Panel, click on Analysis Groups and Materials and then Block.
Click on the Create Material or Modify Material action button.
Select FEA Material from the drop-down menu.
Enter in the appropriate settings.
Click Apply.
1.
2.
3.
4.
5.
6.
On the Command Panel, click on FEA BCs.
Click any option from the Entity list.
Click on the Create Material or Modify Material action button.
Select FEA Material from the drop-down menu.
Enter in the appropriate settings.
Click Apply.
Or
Create Material [id] [Name <'name'>] [Elastic_modulus <value>] [Poisson_ratio <value>]
[Shear_modulus <value>] [Density <value>] [Specific_heat <value>] [Conductivity <value>] [User
constants <value ...>] [DepVar <value>]
Modify Material <id_list|'name'|all> [Name <'name'>] [Elastic_modulus <value>] [Poisson_ratio
<value>] [Shear_modulus <value>] [Density <value>] [Specific_heat <value>] [Conductivity <value>]
[User constants <value ...>] [DepVar <value>]
To create and modify media
1.
2.
3.
4.
5.
On the Command Panel, click on CFD BCs.
Click on the Create Medium or Modify Medium action button.
Select CFD Media from the drop-down menu.
Enter the appropriate settings
Click Apply.
Create Media [id] [Name <'name'>] [Fluid|Porous|Solid]
Modify Media <id_list|'name'|all> [Name <'name'>] [Fluid|Porous|Solid]
Materials can be created with any number of the following material properties:
•
•
•
•
•
•
•
•
Elastic modulus
Poisson Ratio
Density
Specific Heat
Conductivity
Shear Modulus (must satisfy E = 2G(1+v) )
User Constants
DepVar (Only written to Abaqus file)
Media types include:
•
•
Fluid
Porous
759
Trelis 15.0 User Documentation
•
Solid
Any properties that are not initialized by the user will have a default value of 0.
Materials and media types can be listed and deleted using the following commands:
List Material <id_list|'name'|all>
Delete material <id_list|'name'|all>
List Media <id_list|'name'|all>
Delete Media <id_list|'name'|all>
Materials and media can be added to an existing block using the following command:
Block <id> Material <id|'name'>
Block <id> Media <id|'name'>
760
Boundary Condition Sets
To create boundary condition sets
1.
2.
3.
4.
5.
6.
On the Command Panel, click on FEA BCs and then Set.
Click on the Create action button.
Specify the settings for ID/Name.
Enter in the appropriate settings.
Optionally select Specify Analysis Type and/or Specify Modal Max Frequency and enter the appropriate
settings.
Click Apply.
Create bcset [id] [name <'name'>] [After bcset <id>] [{Add|Remove} {bc_type} <id-range | <with name
'name'> >] [analysistype {STATIC|heat|dynamic|modal}] [modal_max_frequency <value>]
To modify boundary condition sets
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs and then Set.
Click on the Modify action button.
Enter in the appropriate settings.
Optionally select Specify Analysis Type and enter the appropriate settings.
Click Apply.
Modify bcset {id_list|'name'|all} [name <'name'>] [After bcset <id>] [{Add|Remove} {bc_type} <id-range |
<with name 'name'> >] [analysistype {STATIC|heat|dynamic|modal}]
*** ABAQUS Parameters ***
Modify bcset {id_list|'name'|all} [max_step_increments <value>] [nonlinear_geometry
<on|OFF>][perturbation <on|OFF>][stabilize <on|OFF>] [steadystate <on|OFF>][modal_max_frequency
<value>]
Modify bcset {id_list|'name'|all} [initial_step_size <value>] [step_period <value>][min_step_size
<value>] [max_step_size <value>][min_step_temperature_change <value>]
Modify bcset {id_list|'name'|all} [mass_scaling <on|OFF>] [mass_scaling_dt
<value>][mass_scaling_factor <value>] [mass_scaling_type <'uniform'|'BELOW_MIN'|'set_equal_dt'>]
Modify bcset {id_list|'name'|all} [restart <on|OFF>][restart_overlay
<on|OFF>] [{restart_frequency|restart_num_intervals} <value>]
Modify bcset {id_list|'name'|all} [output_field <on|OFF>] [output_field_frequency <value>]
[output_history <on|OFF>] [output_history_frequency <value>]
Modify bcset {id_list|'name'|all} [el_file <on|OFF>][el_file_frequency <value>] [node_file
<on|OFF>][node_file_frequency <value>]
Modify bcset {id_list|'name'|all} [el_print <on|OFF>][el_print_frequency <value>] [node_print
<on|OFF>][node_print_frequency <value>]
*** NASTRAN Parameters ***
Modify bcset {id_list|'name'|all} {displacement_output <on|OFF> {PLOT|print|punch|punchprint} {group
<ALL|none|<id>> }}
Modify bcset {id_list|'name'|all} {oload <on|OFF> {PLOT|print|punch|punchprint} {group <ALL|none|<id>>
}}
761
Trelis 15.0 User Documentation
Modify bcset {id_list|'name'|all} {mpcforces <on|OFF> {PLOT|print|punch|punchprint} {group
<ALL|none|<id>> }}
Modify bcset {id_list|'name'|all} {spcforces <on|OFF> {PLOT|print|punch|punchprint} {group
<ALL|none|<id>> }}
Modify bcset {id_list|'name'|all} {stress <on|OFF> {PLOT|print|punch|punchprint} {group
<ALL|none|<id>> } {CENTER|cubic|sgage|corner} {VONMISES|maxs}}
Modify bcset {id_list|'name'|all} {element_strain_energy <on|OFF>
{PLOT|print|punch|punchprint} {group <ALL|none|<id>> } {AVERAGE|amplitude|peak}}
Trelis can create BC sets, which is a group of previously defined loads, restraints and contact pairs. A BCSet is used to
define a load case (analysis step) when writing out 3rd party analysis decks. A BCSet can be a static analysis set, a
thermal analysis set, a modal analysis set, or a dynamic analysis set by specifying the analysistype. The After keyword
can be used to define the order that the BCSets will be written when the model is exported.
Several solver-specific parameters can be set for a BCSet. For ABAQUS, parameters associated with *STEP, *STATIC,
*DYNAMIC, *FREQUENCY, *HEAT TRANSFER, *MASS SCALING, *RESTART, *OUTPUT, *EL FILE, *NODE FILE, *EL
PRINT, and *NODE PRINT can be modified. For Nastran, output requests can be defined for Displacement, Reaction
Loads, MPC Forces, SPC Forces, Stress, and Element Strain Energy.
762
Using Restraints
•
•
•
•
Displacement
Acceleration
Velocity
Temperature
Displacements/Accelerations/Velocities
A Trelis user has the ability to create displacement boundary conditions on most geometric entities found within Trelis.
To create a displacement
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs and then Displacement.
Click on the Create action button.
Specify the settings for ID/Name, Entity List, and Entity ID(s).
Enter any other appropriate settings.
Click Apply.
Create Displacement [id] [Name <'name'>] [{Add|On}
{Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [DOF
{All|{[1][2][3][4][5][6]}} Fix <value>] [SmallestCombine|Average|LargestCombine|OVERWRITE]
To modify a displacement
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on FEA BCs and then Displacement.
Click on the Modify action button.
Specify the settings for ID/Name.
Select Add Entities or Remove Entities.
Select an Entity from the Entity List and specify the Entity ID(s).
Enter any other appropriate settings.
Click Apply.
Modify Displacement {id_list|'name'|all} [name <'name'>] [{Add|Remove}
{Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [DOF
{All|{[1][2][3][4][5][6]}} {Fix <value>|Free}] [SmallestCombine|Average|LargestCombine|OVERWRITE]
To create an acceleration
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs and then Acceleration.
Click on the Create action button.
Specify the settings for ID/Name, Entity List, and Entity ID(s).
Enter any other appropriate settings.
Click Apply.
Create Acceleration [id] [Name <'name'>] [{Add|On}
{Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [DOF {All|{[1][2][3][4][5][6]}}
Fix <value>] [SmallestCombine|Average|LargestCombine|OVERWRITE]
To modify an acceleration
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs and then Acceleration.
Click on the Modify action button.
Specify the settings for ID/Name.
Select Add Entities or Remove Entities.
Select an Entity from the Entity List and specify the Entity ID(s).
763
Trelis 15.0 User Documentation
6.
7.
Enter any other appropriate settings.
Click Apply.
Modify Acceleration {id_list|'name'|all} [name <'name'>] [{Add|Remove}
{Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [DOF {All|{[1][2][3][4][5][6]}}
{Fix <value>|Free}] [SmallestCombine|Average|LargestCombine|OVERWRITE]
To create a velocity
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs and then Velocity.
Click on the Create action button.
Specify the settings for ID/Name, Entity List, and Entity ID(s).
Enter any other appropriate settings.
Click Apply.
Create Velocity [id] [Name <'name'>] [{Add|On}
{Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [DOF {All|{[1][2][3][4][5][6]}}
Fix <value>] [SmallestCombine|Average|LargestCombine|OVERWRITE]
To modify a velocity
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on FEA BCs and then Velocity.
Click on the Modify action button.
Specify the settings for ID/Name.
Select Add Entities or Remove Entities.
Select an Entity from the Entity List and specify the Entity ID(s).
Enter any other appropriate settings.
Click Apply.
Modify Velocity {id_list|'name'|all} [name <'name'>] [{Add|Remove}
{Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [DOF {All|{[1][2][3][4][5][6]}}
{Fix <value>|Free}] [SmallestCombine|Average|LargestCombine|OVERWRITE]
A number of required and optional keywords make the BC create displacement command one of the more complicated of
the boundary condition commands. These keywords will be examined individually in detail.
Degrees of Freedom
The dof keyword is the heart of this command. It specifies how to constrain the entity in question. The keyword is an
abbreviation for ‘degree of freedom’. Typing the optional keyword all tells Trelis that the entered command will encompass
all six degrees of freedom. The degrees of freedom (1 - 6) are defined below in Table 2.
Table 2: Trelis definitions of the six degrees of freedom.
DOF
Physical analog
1
x-translation
2
y-translation
3
z-translation
4
x-rotation
5
y-rotation
764
Using Restraints
6
z-rotation
Trelis will allow displacement commands to be applied upon between one and all six of the degrees of freedom. The
degrees of freedom do not need to be entered in any order. The command strings ‘ 1 2 3 4 5 6 ‘ ‘2 6 1 4 3 5’ and ‘all’ will
end with the same result.
Fixed or Free
The fix and free keywords tell Trelis whether an entity’s displacement defined by the dof keyword is to be enforced with a
finite value or not. If the displacement is fixed, the entity will be constrained in the pre-specified degrees of freedom. A
decimal number entered after the fix keyword will be the value of the enforced degree(s) of freedom. Trelis allows the user
to leave this value blank if the enforced displacement is to be zero, for convenience. However, entering ‘0’ is still
permitted. If a user wishes to remove a displacement from an entity, he or she should just delete it rather than trying to set
all of the degrees of freedom to free.
Displacement Combinations
The SmallestCombine, Average and LargestCombine keywords deal with displacement combinations. These keywords
only apply when a user is modifying an existing displacement boundary condition.
The SmallestCombine keyword will compare the existing displacement values with the current (residing on the command
line) displacement values. The keyword will modify the displacement to the match the displacements dictated by the
boundary condition that has the smallest absolute value. If the boundary condition with the smallest absolute value is the
existing value, the displacement boundary condition will be unchanged. If the current boundary condition has a smaller
absolute value than the existing displacement, the displacement boundary condition will be changed to incorporate the
new values.
The Average keyword will average the existing displacement values with the current (residing on the command line)
displacement values. Note that these averages are not continually updated (i.e., they are not weighted). If a user created
a displacement boundary condition and constrained a degree of freedom to 10.0 and then constrained the same degree of
freedom to 20.0 with the Average keyword, the new displacement value would be 15.0. But if a user constrained the same
degree of freedom to 30.0, while using the Average keyword, the new displacement value would be 22.5 ([15+30]/2), not
20.0 ([10+20+30]/3).
The LargestCombine keyword will compare the existing displacement values with the current (residing on the command
line) displacement values. The keyword will modify the displacement to the match the displacements dictated by the
boundary condition that has the largest absolute value. If the boundary condition with the largest absolute value is the
existing value, the displacement boundary condition will be unchanged. If the current boundary condition has a larger
absolute value than the existing displacement, the displacement boundary condition will be changed to incorporate the
new values.
When none of these keywords are specified, Trelis will combine displacements in its default mode, Overwrite. The
Overwrite keyword overwrites the entity’s previous displacement boundary condition(s) with the displacement values
specified in the command.
Temperature
Trelis can create temperature boundary conditions on most geometric and mesh entities. The temperature boundary
condition can also be applied to thin-shell elements.
To create a temperature
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs and then Temperature.
Click on the Create action button.
Specify the settings for ID/Name, Entity List, and Entity ID(s).
Optionally click on Create On Thin-Shell Elements and enter in the appropriate settings.
Click Apply.
Create Temperature [id] [Name <'name'>] [{Add|On}
{Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [Value <val>]
765
Trelis 15.0 User Documentation
Create Temperature [id] [Name <'name'>] [{Add|On}
{Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [{ Top <val>
Bottom <val> | [Middle <val>] [Gradient <val>] } ]
To modify a temperature
1.
2.
3.
4.
5.
6.
7.
On the Command Panel, click on FEA BCs and then Temperature.
Click on the Modify action button.
Specify the settings for ID/Name.
Select Add Entities or Remove Entities.
Select an Entity from the Entity List and specify the Entity ID(s).
Optionally click on Create On Thin-Shell Elements and enter in the appropriate settings.
Click Apply.
Modify Temperature {id_list|'name'|all} [name <'name'>] [{Add|Remove}
{Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [Value <val>]
Modify Temperature {id_list|'name'|all} [name <'name'>] [{Add|Remove}
{Nodeset|Volume|Surface|Curve|Vertex|Hex|Tet|Face|Tri|Edge|Node} <entity_list>] [{ Top <val>
Bottom <val> | [Middle <val>] [Gradient <val>] } ]
The value keyword defines the amplitude (temperature). The other command options are discussed below
Top, Gradient, Middle, Bottom
The above keywords are only used for thin-shell elements (i.e., 2D entities). The valid combinations are limited to: top and
bottom, middle and gradient, only gradient or only middle. It should be noted that temperature boundary conditions cannot
contain regular and thin-shell temperature values.
766
Using Loads
•
•
•
•
Force
Pressure
Heat Flux
Convection
Forces
To create a force
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs and then Force.
Click on the Create action button.
Specify the ID/Name,Force Entity and Entity ID(s).
Select or Deselect Specify Using Vector and enter the appropriate settings.
Click Apply.
Create Force [id] [Name <'name'>] [ {Add|On} {Nodeset|Surface|Curve|Vertex|Face|Tri|Edge|Node}
<entity_list>] [Force Value <val>] [Moment Value <val>] [Direction { direction_options}]
Create Force [id] [Name <'name'>] [ {Add|On} {Nodeset|Surface|Curve|Vertex|Face|Tri|Edge|Node}
<entity_list>] [ Vector <val> <val> <val> <val> <val> <val>]
To modify a force
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs and then Force.
Click on the Create action button.
Specify the ID/Name,Force Entity and Entity ID(s).
Select or Deselect Specify Using Vector and enter the appropriate settings.
Click Apply.
Modify Force {id_list|'name'|all} [Name <'name'>] [ {Add|Remove}
{Nodeset|Surface|Curve|Vertex|Face|Tri|Edge|Node} <entity_list>] [Force Value <val>] [Moment
Value <val>] [Direction { direction_options}]
Modify Force {id_list|'name'|all} [Name <'name'>] [ {Add|Remove}
{Nodeset|Surface|Curve|Vertex|Face|Tri|Edge|Node} <entity_list>] [ Vector <val> <val> <val> <val>
<val> <val>]
A Trelis user has the ability to create forces on 0D, 1D, and 2D entities. A force can be created using the direction syntax
(see Specifying Direction). If the vector keyword is used, the first three values are the force components, and the last
three values are the moment components.
The use of the force and moment keywords specify the type of load. If both a force and a moment are to be applied, first
create one of them, then modify it to add the other. Note that every instance of a force or moment keyword must have an
accompanying value keyword.
Regarding force and moment keywords, the following detail may be helpful:
A user may create a force and moment at the same time, but can only specify a direction once. If the force and moment
have the same unit vector, it will be successful. If a users wants to create a force in the direction 1,2,3 and a moment in
the direction 1,0,0, the user will have to create one, then add the other by modifying it.
Using Pressure
To create or modify a pressure
767
Trelis 15.0 User Documentation
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs and then Pressure.
Click on the Create or Modify action button.
Specify the ID/Name,Force Entity, Entity ID(s) and Magnitude Value.
Enter any other appropriate settings.
Click Apply.
Create Pressure [id] [Name <'name'>] [{Add|On} {Sideset|Surface|Curve|Face|Tri|Edge} <entity_list>]
[Magnitude <value>] [TOP|Bottom] [PRESSURE|Totalforce]
Modify Pressure {id_list|'name'|all} [Name <'name'>] [{Add|Remove}
{Sideset|Surface|Curve|Face|Tri|Edge} <entity_list>] [Magnitude <value>] [TOP|Bottom]
[PRESSURE|Totalforce]
Trelis users can create pressure boundary conditions on 1D and 2D entities. Positive surface pressures acting on solid
elements are defined as pointing into the face of the elements. Pressures are always normal to the face. For shells and
independent surfaces, a ‘left-hand-rule’ is employed. Point your left thumb at the surface in question. If the direction your
fingers curl matches the direction of ascending vertex numbering, the direction of the pressure vectors will match the
direction of your thumb.
Value
The value variable is the magnitude of the pressure boundary condition. If the user leaves this value blank, Trelis will
assign the pressure magnitude to zero (possibly a trivial case) and issue a warning. Typing a negative value will not flip
the direction of the pressure arrows on the display; instead, the pressure magnitude will be negative.
Pressure and Total Force
The pressure and totalforce keywords are used to modify the pressure boundary condition. The pressure keyword is the
default. All pressures applied with this keyword present (or with both of these keywords absent from the command string)
are pure pressures. If the user enters the totalforce keyword, the pressure magnitude is divided by the area of the surface
the pressure is acting on (or the length of the curve, for a curve pressure). In effect, the user is entering a force that is
treated and exported as a pressure.
Top and Bottom
The top keyword (default) indicates the pressure will occur on the top of a shell element. Specifying bottom will cause the
pressure to be applied to the bottom of the element.
Using Heat Flux
To create or modify a heatflux
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs and then Heatflux.
Click on the Create or Modify action button.
Specify ID/Name, Entity List and Entity ID(s).
Enter any other appropriate settings.
Click Apply.
Create Heatflux [id] [Name <'name'>] [{Add|On} {Sideset|Surface|Curve|Face|Tri|Edge} <entity_list>]
[Value <value>]
Create Heatflux [id] [Name <'name'>] [{Add|On} {Sideset|Surface|Face|Tri} <entity_list>] [Top <value>
Bottom <value>]
Modify Heatflux {id_list|'name'|All} [Name <'name'>] [{Add|Remove}
{Sideset|Surface|Curve|Face|Tri|Edge} <entity_list>] [Value <value>]
Modify Heatflux {id_list|'name'|All} [Name <'name'>] [{Add|Remove} {Sideset|Surface|Face|Tri}
<entity_list>] [Top <value> Bottom <value>]
A Trelis user may apply heat flux boundary conditions to 1D and 2D entities, including thin-shell elements.
768
Using Loads
Top and Bottom Values
Heat fluxes can be applied to thin-shell elements as well. The same rules apply to thin-shell heat fluxes as to thin-shell
temperatures: thin-shell heat fluxes can only be applied to surfaces and heat flux boundary conditions cannot contain
regular and thin-shell heat flux values (see journal below). However, thin-shell heat flux commands do not contain
gradient or middle keyword options. Only top and bottom keywords are supported.
Using Convection
To create or modify a convection
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs and then Convection.
Click on the Create or Modify action button.
Specify ID/Name, Entity List and Entity ID(s).
Enter any other appropriate settings.
Click Apply.
Create Convection [id] [Name <'name'>] [{Add|On} {Sideset|Surface|Curve|Face|Tri|Edge}
<entity_list>] [Surrounding {<value>| Top <value> Bottom <value>} Coefficient {<value>| Top <value>
Bottom <value>}]
Modify Convection [id] [Name <'name'>] [{Add|On} {Sideset|Surface|Curve|Face|Tri|Edge}
<entity_list>] [Surrounding {<value>| Top <value> Bottom <value>} Coefficient {<value>| Top <value>
Bottom <value>}]
A Trelis user can apply convection boundary conditions to 1D and 2D entities. Convection is a transport of thermal energy
that is proportional to the difference between the surface temperature and the temperature of the surroundings.
Surrounding
The surrounding keyword specifies the temperature surrounding the entity with the convection boundary condition.
Coefficient
The coefficient keyword is a convection coefficient, in units of energy per length times time times temperature (i.e.,
[energy]/([length]*[time]*[temperature]) ).
769
Using Contact Surfaces
•
•
•
Contact Region
Contact Pair
Auto-Contact Tool
The Contact Region
To define contact between two entities, Trelis requires each entity to be defined as a separate contact region. Each
region can be made up of multiple 1D or 2D entities.
To create a contact region
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs and then Contact Region.
Click on the Create action button.
Specify ID(s)/Name settings.
Select the Contact Region Entity and specify the Entity ID(s). This can also be done using the Pick Widget
function.
Click Apply.
Create Contact Region [id] [Name <'name'>] [{Add|On} {Sideset|Surface|Curve|Face|Tri|Edge}
<entity_list>]
To modify a contact region
1.
2.
3.
4.
5.
6.
On the Command Panel, click on FEA BCs and then Contact Region.
Click on the Modify action button.
Specify ID(s)/Name and optionally Change Name.
Select Add Entities or Remove Entities.
Select the Contact Region Entity and specify the Entity ID(s). This can also be done using the Pick Widget
function.
Click Apply.
Modify Contact Region {id_list|'name'|All} [Name <'name'>] [{Add|Remove}
{Sideset|Surface|Curve|Face|Tri|Edge} <entity_list>]
The Contact Pair
To create or modify a contact pair
1.
2.
3.
4.
On the Command Panel, click on FEA BCs and then Contact Pair.
Click on Create or Modify.
Enter the appropriate settings.
Click Apply.
create contact pair [id] [name <'name'>] [master contact region <id|'name'>] [slave contact region
<id|'name'>] [friction <value>] [tolerance <value>] [tied {on|OFF}] [General <on|OFF> [Exterior
<on|OFF>]]
modify contact pair {id_list|'name'|all} [name <'name'>] [master contact region <id|'name'>] [slave contact
region <id|'name'>] [friction <value>] [tolerance <value>] [tied {on|OFF}] [General <on|OFF> [Exterior
<on|OFF>]]
771
Trelis 15.0 User Documentation
A contact pair is composed of two contact regions. One region will be the ‘master’ surface, and the other will be the
‘slave.’ 2D contact regions can not be mixed with 1D contact regions. The friction coefficient can also be included. The
tolerance keyword is currently unused. Use the tied keyword to specify that the contact is to define tied contact between
the two contact regions, essentially “gluing” the parts together. Currently, this option is only available when using the
Abaqus Exporter.
The General keyword can be used to specify general (i.e. global) contact without specifying surfaces/curves to use as
contact pairs. Currently, this keyword is only valid when exporting to Abaqus. If the Exterior keyword is used with the
General keyword, then Abaqus will consider all exterior surfaces when determining contact regions. If the Exterior
keyword is omitted, then the user must provide a master contact region and/or a slave contact region.
Auto-Contact Tool
With the auto-contact tool, Trelis can search for contact pairs and automatically set up all of the necessary contact regions
and contact pairs.
Create Contact Autoselect [{Volume|Surface|Curve} <ids>] [Master Volume <id>] [Maxgap <value>]
[Curve_Contact]
The optional geometry list can be used to limit Cubit’s search to only a subset of entities. If this list is omitted, all bodies in
the model will be searched. The optional master volume keyword can be used to tell Trelis which volume should be used
as the master contact region. If this keyword is omitted, the user will not have control over which volume is the master
region. The maxgap keyword can be used to control how Trelis searches for contact regions. This value is used as the
maximum amount of gap that can exist between two surfaces and be identified as a contact region. If this keyword is
omitted, the geometry tolerance is used. The curve_contact keyword can be used to indicate the model requires curve
contact as opposed to surface contact.
772
Using Contact Surfaces
•
•
•
Contact Region
Contact Pair
Auto-Contact Tool
The Contact Region
To define contact between two entities, Trelis requires each entity to be defined as a separate contact region. Each
region can be made up of multiple 1D or 2D entities.
To create a contact region
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs and then Contact Region.
Click on the Create action button.
Specify ID(s)/Name settings.
Select the Contact Region Entity and specify the Entity ID(s). This can also be done using the Pick Widget
function.
Click Apply.
Create Contact Region [id] [Name <'name'>] [{Add|On} {Sideset|Surface|Curve|Face|Tri|Edge}
<entity_list>]
To modify a contact region
1.
2.
3.
4.
5.
6.
On the Command Panel, click on FEA BCs and then Contact Region.
Click on the Modify action button.
Specify ID(s)/Name and optionally Change Name.
Select Add Entities or Remove Entities.
Select the Contact Region Entity and specify the Entity ID(s). This can also be done using the Pick Widget
function.
Click Apply.
Modify Contact Region {id_list|'name'|All} [Name <'name'>] [{Add|Remove}
{Sideset|Surface|Curve|Face|Tri|Edge} <entity_list>]
The Contact Pair
To create or modify a contact pair
1.
2.
3.
4.
On the Command Panel, click on FEA BCs and then Contact Pair.
Click on Create or Modify.
Enter the appropriate settings.
Click Apply.
create contact pair [id] [name <'name'>] [master contact region <id|'name'>] [slave contact region
<id|'name'>] [friction <value>] [tolerance <value>] [tied {on|OFF}] [General <on|OFF> [Exterior
<on|OFF>]]
modify contact pair {id_list|'name'|all} [name <'name'>] [master contact region <id|'name'>] [slave contact
region <id|'name'>] [friction <value>] [tolerance <value>] [tied {on|OFF}] [General <on|OFF> [Exterior
<on|OFF>]]
773
Trelis 15.0 User Documentation
A contact pair is composed of two contact regions. One region will be the ‘master’ surface, and the other will be the
‘slave.’ 2D contact regions can not be mixed with 1D contact regions. The friction coefficient can also be included. The
tolerance keyword is currently unused. Use the tied keyword to specify that the contact is to define tied contact between
the two contact regions, essentially “gluing” the parts together. Currently, this option is only available when using the
Abaqus Exporter.
The General keyword can be used to specify general (i.e. global) contact without specifying surfaces/curves to use as
contact pairs. Currently, this keyword is only valid when exporting to Abaqus. If the Exterior keyword is used with the
General keyword, then Abaqus will consider all exterior surfaces when determining contact regions. If the Exterior
keyword is omitted, then the user must provide a master contact region and/or a slave contact region.
Auto-Contact Tool
With the auto-contact tool, Trelis can search for contact pairs and automatically set up all of the necessary contact regions
and contact pairs.
Create Contact Autoselect [{Volume|Surface|Curve} <ids>] [Master Volume <id>] [Maxgap <value>]
[Curve_Contact]
The optional geometry list can be used to limit Cubit’s search to only a subset of entities. If this list is omitted, all bodies in
the model will be searched. The optional master volume keyword can be used to tell Trelis which volume should be used
as the master contact region. If this keyword is omitted, the user will not have control over which volume is the master
region. The maxgap keyword can be used to control how Trelis searches for contact regions. This value is used as the
maximum amount of gap that can exist between two surfaces and be identified as a contact region. If this keyword is
omitted, the geometry tolerance is used. The curve_contact keyword can be used to indicate the model requires curve
contact as opposed to surface contact.
774
Using CFD Boundary Conditions
•
•
•
•
•
•
Inlet Velocity
Inlet Pressure
Inlet Massflow
Outlet Pressure
Farfield Pressure
Symmetry
Trelis can export models to the Fluent mesh format and supports defining the above CFD boundary conditions. Only the
region on which the BC acts can be defined in Trelis. The data associated with each boundary condition (pressure,
velocity, mass values) is not defined within Trelis and must be assigned using a CFD model editor, such as Fluent.
The following shows the commands for creating and modifying CFD boundary conditions. To delete them, use the delete
command (see Miscellaneous Commands).
Inlet Velocity
To create and modify inlet velocity
1.
2.
3.
4.
5.
On the Command Panel, click on CFD BCs.
Click on the Create or Modify action button.
Select Velocity Inlet from the drop-down menu.
Enter the appropriate settings.
Click Apply.
Create Inletvelocity [id] [name <'name'>] [{Add|On} {Surface} <entity_list>]
Modify Inletvelocity [id] [name <'name'>] [{Add|Remove} {Surface} <entity_list>]
Inlet Pressure
To create and modify inlet pressure
1.
2.
3.
4.
5.
On the Command Panel, click on CFD BCs.
Click on the Create or Modify action button.
Select Pressure Inlet from the drop-down menu.
Enter the appropriate settings.
Click Apply.
Create Inletpressure [id] [name <'name'>] [{Add|On} {Surface} <entity_list>]
Modify Inletpressure [id] [name <'name'>] [{Add|Remove} {Surface} <entity_list>]
Inlet Massflow
To create and modify inlet massflow
1.
2.
3.
4.
5.
On the Command Panel, click on CFD BCs.
Click on the Create or Modify action button.
Select Mass Flow Inlet from the drop-down menu.
Enter the appropriate settings.
Click Apply.
Create Inletmassflow [id] [name <'name'>] [{Add|On} {Surface} <entity_list>]
775
Trelis 15.0 User Documentation
Modify Inletmassflow [id] [name <'name'>] [{Add|Remove} {Surface} <entity_list>]
Outlet Pressure
To create and modify outlet pressure
1.
2.
3.
4.
5.
On the Command Panel, click on CFD BCs.
Click on the Create or Modify action button.
Select Pressure Outlet from the drop-down menu.
Enter the appropriate settings.
Click Apply.
Create Outletpressure [id] [name <'name'>] [{Add|On} {Surface} <entity_list>]
Modify Outletpressure [id] [name <'name'>] [{Add|Remove} {Surface} <entity_list>]
Farfield Pressure
To create and modify farfield pressure
1.
2.
3.
4.
5.
On the Command Panel, click on CFD BCs.
Click on the Create or Modify action button.
Select Pressure Far Field from the drop-down menu.
Enter the appropriate settings.
Click Apply.
Create Farfieldpressure [id] [name <'name'>] [{Add|On} {Surface} <entity_list>]
Modify Farfieldpressure [id] [name <'name'>] [{Add|Remove} {Surface} <entity_list>]
Symmetry
To create and modify symmetry
1.
2.
3.
4.
5.
On the Command Panel, click on CFD BCs.
Click on the Create or Modify action button.
Select Symmetry from the drop-down menu.
Enter the appropriate settings.
Click Apply.
Create Symmetry [id] [name <'name'>] [{Add|On} {Surface} <entity_list>]
Modify Symmetry [id] [name <'name'>] [{Add|Remove} {Surface} <entity_list>]
776
Miscellaneous Boundary Condition Commands
•
•
•
•
Delete
List
Draw
Highlight
Delete
The BC delete keyword combination is used to delete boundary conditions. The current list of all entities that can be
deleted using this command were shown in Table 1. Trelis currently has no ‘undo’ command to ‘undelete’ a boundary
condition deletion.
To delete a boundary condition
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs or CFD BCs.
Click on any option from the Entity menu.
Click on the Delete action button.
Enter the appropriate settings.
Click Apply.
Delete {bc_type} [<id-range>|All]
Delete Boundary Conditions
Every set (and boundary condition within them) can be deleted at once by typing delete boundary conditions. This
command will delete all boundary conditions from your model.
List
The List keyword combination is used to list boundary conditions. The current list of all entities that can be listed using
this command was shown in Table 1. Cubit’s parser can evaluate boundary conditions given the entities they act on. For
example, "List pressure in surface 1" will list all pressures that act on Surface 1.
To list boundary conditions
1.
2.
3.
4.
5.
On the Command Panel, click on FEA BCs or CFD BCs.
Click on any option from the Entity menu except Contact Pair and Set.
Click on the List action button.
Enter the appropriate settings.
Click Apply.
List {bc_type} [<id-range>]
List Boundary Conditions
Every set (and boundary condition within them) may be listed at once by typing list boundary conditions. Trelis will list
the number of sets and individual boundary conditions in your model. This command will list the total number of each type
of set and boundary condition, including boundary conditions that are not a part of a BC set.
Draw
To draw boundary conditions
1.
2.
3.
On the Command Panel, click on FEA BCs or CFD BCs.
Click on any option from the Entity menu except Contact Pair and Set.
Click on the Draw action button.
777
Trelis 15.0 User Documentation
4.
5.
6.
Select Draw.
Enter the appropriate settings.
Click Apply.
Draw {bc_type} {<id-range>|all}[Add]
The draw keyphrase allows a Trelis user to draw any type of boundary condition. This command will clear the graphics
window of every part of the model except for the selected boundary condition. Using the add keyword will permit multiple
boundary conditions to be drawn at the same time. Any combination of boundary conditions and entities that were valid for
delete and list are also valid for draw.
Highlight
To Highlight boundary conditions
1.
2.
3.
4.
5.
6.
On the Command Panel, click on FEA BCs or CFD BCs.
Click on any option from the Entity menu except Contact Pair and Set.
Click on the Draw action button.
Select Highlight.
Enter the appropriate settings.
Click Apply.
Highlight {bc_type} {<id-range>|All}
The highlight keyphrase allows a Trelis user to highlight any boundary condition. Highlighting a boundary condition will
turn it bright orange and the vectors defining it will thicken. The highlight command is similar to the draw command.
778
Exporting Sierra Files
Sierra input decks can be exported from Trelis. This capability was added in response to a need to translate
Abaqus input decks to Sierra input decks by importing the Abaqus deck into Trelis and then immediately
exporting the Sierra deck. Therefore, it is assumed that most of the input deck information has been created
outside of Trelis and that the user will not interact with it in Trelis .
The Sierra input deck writer is simply another export format and as a result it can be used for any currently
defined mesh and input deck info defined in Trelis.
The Sierra input deck exporter relies on some of the mesh-specific information that is generated when
exporting the Genesis mesh. Therefore, you should export the Genesis mesh before exporting the
Sierra input deck.
779
Defining PARAMS for NASTRAN
List Nastran Exporter Params
Set Nastran Exporter Params Add '<param_string>'
Set Nastran Exporter Params Remove '<param_string>'
Set Nastran Exporter Params Clear
Nastran uses “PARAMS” to define additional instructions and settings in its Bulk Data file. Any string can be defined as a
Nastran Exporter Param, and it will be exported to the Nastran file as “PARAM, <string>”.
781
Finite Element Model
•
•
•
•
Global Element IDs
Exodus Boundary Conditions
Non-Exodus Boundary Conditions
Exporting the Finite Element Model
This chapter describes the techniques used to complete the definition of the finite element model. The definitions of the
basic items in an Exodus database are briefly presented, followed by a description of the commands a user would
typically enter to produce a customized finite element problem description, and how to export the finite element model.
783
Exporting an Exodus II File
To export an Exodus II file
1.
2.
3.
4.
5.
6.
7.
Click File and then Export.
Select the desired location to save the file.
Enter the File Name.
Select Exodus from the Save as type drop-down menu.
Click Save. A new window will appear.
Enter the appropriate settings.
Click Finish.
Export [Genesis|Mesh] '<filename>' [dimension {2|3}] [Block <id_list>] [cubitids] [XML '<filename>']
The Genesis or Mesh arguments are optional and both indicate that an Exodus II format will be written. The filename can
be any valid filename. Where a full path is not specified, the file will be written in the current working directory.
The dimension argument is also optional. Most element types have an inherent dimensionality associated with them. For
example, a truss or beam element is inherently 2D while a hex or tetra element is 3D. Without this argument, only the x-y
location of the nodal coordinates of 2D elements are written to the Exodus II file. Using the argument dimension 3, in this
example, permits the full 3D coordinates to be written.
The optional Block argument may also be added to the Export command. Without this ar