AUTODYN User Manual Version 12.1

AUTODYN® User Manual Version 12.1
Release 12.1
November 2009
ANSYS, Inc.
Southpointe
275 Technology Drive
Canonsburg, PA 15317
ansysinfo@ansys.com
http://www.ansys.com
(T) 724-746-3304
(F) 724-514-9494
ANSYS, Inc. is
certified to ISO
9001:2008.
AUTODYN User Manual
Copyright and Trademark Information
© 2009 SAS IP, Inc. All rights reserved. Unauthorized use, distribution, or
duplication is prohibited.
ANSYS, ANSYS Workbench, AUTODYN, CFX, FLUENT and any and all ANSYS,
Inc. brand, product, service and feature names, logos and slogans are registered
trademarks or trademarks of ANSYS, Inc. or its subsidiaries located in the United
States or other countries. ICEM CFD is a trademark used by ANSYS, Inc. under
license. All other brand, product, service and feature names or trademarks are the
property of their respective owners.
Disclaimer Notice
THIS ANSYS SOFTWARE PRODUCT AND PROGRAM DOCUMENTATION
INCLUDE TRADE SECRETS AND ARE CONFIDENTIAL AND PROPRIETARY
PRODUCTS OF ANSYS, INC., ITS SUBSIDIARIES, OR LICENSORS. The
software products and documentation are furnished by ANSYS, Inc., its subsidiaries,
or affiliates under a software license agreement that contains provisions concerning
non-disclosure, copying, length and nature of use, compliance with exporting laws,
warranties, disclaimers, limitations of liability, and remedies, and other provisions.
The software products and documentation may be used, disclosed, transferred, or
copied only in accordance with the terms and conditions of that software license
agreement.
ANSYS, Inc. is certified to ISO 9001:2008
U.S. Government Rights
For U.S. Government users, except as specifically granted by the ANSYS, Inc.
software license agreement, the use, duplication, or disclosure by the United States
Government is subject to restrictions stated in the ANSYS, Inc. software license
agreement and FAR 12.212 (for non DOD licenses).
Third Party Software
See the legal information in the product help files for the complete Legal Notice for
ANSYS proprietary software and third-party software. If you are unable to access
the Legal Notice, please contact ANSYS, Inc.
Published in the U.S.A.
ii
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Table of Contents
AUTODYN User Manual ............................................................................................ 1
Overview ................................................................................................................. 1
Overview ................................................................................................................. 1
Overview - Tool Bar ............................................................................................ 3
Overview - Navigation Bar .................................................................................. 5
Overview - Dialog Panel and Dialog Windows .................................................... 7
Overview - Command Line Panel...................................................................... 12
Overview - Undock Command Line................................................................... 16
Overview - Command File Window ................................................................... 18
Overview - Message Panel ............................................................................... 20
Overview - HTML review windows .................................................................... 21
Overview - File names ...................................................................................... 22
Overview - On-Line help ................................................................................... 23
Overview - Supported Operating Systems and Compilers ................................ 24
Overview - Initialization Settings ....................................................................... 25
Slide Viewer ...................................................................................................... 30
Overview - AUTODYN in Workbench ................................................................ 35
Overview - AUTODYN solver options in Workbench ......................................... 44
Pull-down Menus .................................................................................................. 45
Pull-down Menus ...................................................................................................... 45
File .................................................................................................................... 47
Pull-Down Menu-File ......................................................................................... 47
Pull-down Menu - File - New.......................................................................... 50
Manage Folders............................................................................................. 53
Pull-down Menu - File - Manage Folders .......................................................... 53
Manage Folders - New Folder ........................................................................... 54
Pull-down Menu - File - Save As ................................................................... 55
PullDown Menus - File - SaveProject ............................................................ 56
Pull-down Menu - File - Save As Version ...................................................... 57
PullDownMenus - File - Export To Version .................................................... 58
Pull-down Menu - File - Export PostScript ..................................................... 59
Pull-down Menu - File - Export VRML ........................................................... 66
Import ................................................................................................................ 68
Pull-down Menu - Import ................................................................................... 68
Pull-down Menu - Import - TrueGrid .............................................................. 70
Pull-down Menu - Import - ICEM ................................................................... 74
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
iii
AUTODYN User Manual
Pull-down Menu - Import - LS-DYNA ............................................................. 76
Pull-down Menu - Import - Nastran ................................................................ 80
Pull Down Menus - Import - Convert IJK to Unstructured .............................. 83
Setup................................................................................................................. 84
Pull-down Menu - Setup .................................................................................... 84
Pull-down Menu - Setup - Description ........................................................... 86
Pull-down Menu - Setup - Symmetry ............................................................. 88
Execution .......................................................................................................... 89
Pull-down Menu - Execution ............................................................................. 89
Pull-down Menu - Execute - Batch Runner .................................................... 90
View .................................................................................................................. 92
Pull-down Menu - View ..................................................................................... 92
Pull-down Menu - View - Slideshow - Setup .................................................. 94
Pull-down Menu - View - Performance Profiler .............................................. 96
Options.............................................................................................................. 98
Pull-down Menu - Options ................................................................................. 98
Pull-down Menu - Options - Interactivity ........................................................ 99
Pull-down Menu - Options - Clipping Planes ............................................... 100
Pull-down Menu - Options - Default Settings ............................................... 101
Pull-down Menu - Options - Pause License ................................................. 102
Pull-down Menu - Options - Create User-Subroutine Project ...................... 103
Pull-down Menu - Help .................................................................................... 104
Plots.................................................................................................................... 105
Plots.................................................................................................................... 105
Plots - Select Contour Variable ....................................................................... 107
Plots - View range and slices (Structured) ...................................................... 108
View range and slices (SPH/Unstructured) ..................................................... 109
Settings............................................................................................................... 110
Settings............................................................................................................... 110
Settings - Display ............................................................................................ 112
Settings - Grid ................................................................................................. 119
Settings - Legend ............................................................................................ 120
Settings - Node/Element Numbers .................................................................. 122
Materials ......................................................................................................... 123
Settings - Materials ......................................................................................... 123
Settings - Materials - Modify Material Color ................................................. 125
Contour ........................................................................................................... 126
iv
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Settings - Contour ........................................................................................... 126
Settings - Contour - Profile Plot ................................................................... 129
Settings - Velocity vector ................................................................................. 131
Settings - Gauge point .................................................................................... 133
Settings - Boundary......................................................................................... 135
Settings - Joins................................................................................................ 136
Settings - Axes ................................................................................................ 137
Settings - Detonation....................................................................................... 139
Settings - Eroded Nodes ................................................................................. 140
Settings - Unused Regions ............................................................................. 141
Settings - Polygons ......................................................................................... 143
Settings - Beam Sections ................................................................................ 144
Settings - Shell Thickness ............................................................................... 149
Settings - Material Direction ............................................................................ 150
Settings - Marker ............................................................................................. 152
Settings - Shell Normal ................................................................................... 155
Settings-Part Highlights ................................................................................... 156
History ................................................................................................................ 158
History ................................................................................................................ 158
History - Single Variable Plot .......................................................................... 161
History - Reduce ............................................................................................. 163
History Write Text Output ................................................................................ 164
Multiple Variable Plot ...................................................................................... 165
History - Multiple Variable Plot ........................................................................ 165
History - Multiple Variable Plot - Set All Plots .............................................. 167
History - Multiple Variable Plot - Modify Selected Plot ................................. 169
History - Min/Max......................................................................................... 171
History - Set Scales ..................................................................................... 172
History - Set Plot Styles ............................................................................... 174
History - Set Legend Position ...................................................................... 176
History - Load .............................................................................................. 177
Slides .................................................................................................................. 179
View Slides (Slide Viewer) .................................................................................. 183
Materials ............................................................................................................. 188
Materials ............................................................................................................. 188
Materials - New / Modify .................................................................................. 190
Materials - Copy .............................................................................................. 195
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
v
AUTODYN User Manual
Materials - Delete ............................................................................................ 196
Materials - Load .............................................................................................. 197
Initial Conditions ................................................................................................. 199
Initial Conditions ................................................................................................. 199
Initial Conditions - New/Modify ........................................................................ 201
Initial Explicit Model Initialization ..................................................................... 204
Initial Conditions - Delete ................................................................................ 207
Boundaries ......................................................................................................... 208
Boundaries ......................................................................................................... 208
Boundaries - New / Modify .............................................................................. 209
Boundaries - Delete ........................................................................................ 211
Parts ................................................................................................................... 212
Parts ................................................................................................................... 212
New ................................................................................................................. 218
Parts - New ..................................................................................................... 218
Parts - New - Select Predef (2D) ................................................................. 221
Parts - New - Select Predef (3D) ................................................................. 229
Parts - New - Select Predef (3D Shell) ........................................................ 238
Parts - New - Define Zoning (2D) ................................................................ 241
Parts - New - Define Zoning (3D) ................................................................ 251
Parts - New - Define Zoning (3D Shell) ....................................................... 261
Parts - New - Fill Part (2D) ..................................................................................... 265
Parts - New - Fill Part .................................................................................. 267
Parts - New - Fill Part (Shell) ....................................................................... 270
Parts - Copy .................................................................................................... 272
Parts - Delete .................................................................................................. 273
Parts - IJK Range ............................................................................................ 274
Parts - Activation ............................................................................................. 275
Parts - Rename ............................................................................................... 276
Parts - Print ..................................................................................................... 277
Parts-Pack(Fill)................................................................................................ 278
Zoning ............................................................................................................. 279
Parts - Zoning.................................................................................................. 279
Parts - Zoning - Box..................................................................................... 282
Parts - Zoning - Cylinder .............................................................................. 284
Parts - Zoning - Sphere ............................................................................... 286
Parts - Zoning - Ogive ................................................................................. 288
vi
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Zoning - Quad .................................................................................. 290
Parts - Zoning - Hex .................................................................................... 292
Parts - Zoning - Frag/Bric (page 1) .............................................................. 294
Parts - Zoning - Frag/Bric (page 2) ......................................................................... 296
Parts - Zoning - Transition ........................................................................... 298
Parts - Zoning - Node .................................................................................. 299
Parts - Zoning - Line .................................................................................... 300
Parts - Zoning - Surface .............................................................................. 302
Parts - Zoning - Volume ............................................................................... 304
Parts - Zoning - Translate ............................................................................ 306
Parts - Zoning - Rotate ................................................................................ 307
Parts - Zoning - Scale .................................................................................. 308
Parts - Zoning - Copy .................................................................................. 309
Parts - Zoning - Delete ................................................................................ 310
Parts - Zoning - Save ................................................................................... 311
Parts - Zoning - Restore .............................................................................. 312
Parts - Zoning - Refine ................................................................................ 313
Parts-Zoning-Fill Block ................................................................................ 315
Parts-Zoning-Fill Block .................................................................................... 315
Parts-Zoning-Fill Block-Implicit .................................................................... 316
Parts-Zoning-Fill Block-Explicit .................................................................... 318
Fill ................................................................................................................... 320
Parts - Fill ........................................................................................................ 320
Parts - Fill - Block ........................................................................................ 322
Parts - Fill - I / J / K Plane ............................................................................ 324
Parts - Fill - Node......................................................................................... 326
Parts - Fill - Unused ..................................................................................... 328
Composite ................................................................................................... 329
Parts - Fill - Composite ................................................................................ 329
Parts - Fill - Multi-Fill .................................................................................... 333
Parts - Fill - Datafile ..................................................................................... 335
Parts - Fill - Part Fill ................................................................................................ 340
Parts - Fill - Block Remap ............................................................................ 342
Boundary......................................................................................................... 347
Parts - Boundary ............................................................................................. 347
Parts - Boundary - Block .............................................................................. 348
Parts - Boundary - I / J / K Plane ................................................................. 349
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
vii
AUTODYN User Manual
Parts - Boundary - Node .............................................................................. 350
Parts - Boundary - Clear .............................................................................. 351
Parts - Boundary - Apply Interactively ......................................................... 352
Parts - Boundary - Clear Interactively .......................................................... 353
Gauges ........................................................................................................... 354
Parts - Gauges ................................................................................................ 354
Parts - Gauges - Add ................................................................................... 356
Parts - Gauges - Move ................................................................................ 357
Parts - Gauges - Delete ............................................................................... 358
Parts - Gauges - Add Unstructured ............................................................. 359
Parts - Gauges - Move Unstructured ........................................................... 360
Parts - Gauges - Delete Unstructured ......................................................... 361
Solvers ............................................................................................................ 362
Parts - Solvers (Structured) ............................................................................. 362
Parts - Solvers (Structured) - Type .............................................................. 363
Parts - Solvers (Structured) - Solution (2D Shells) ...................................... 364
Parts - Solvers (Structured) - Solution (3D Shells) ...................................... 365
Parts - Solvers (Structured) - Solutions (Beams) ......................................... 366
Parts - Solvers (Structured) - Solution (3D Euler-FCT)................................ 367
Parts - Solvers (Structured) - Solution (2D SPH) ......................................... 368
Parts - Solvers (Structured) - Solution (3D SPH) ......................................... 370
Parts - Solvers (Structured) - Dezone-(2D & 3D Euler) ............................... 372
Parts-Solver (Structured) - Dezone (2D & 3D Lagrange/ALE) ..................... 373
Parts - Solvers (Structured) - Jetting ........................................................... 375
Parts - Solvers (Unstructured) - Solid .......................................................... 377
Parts - Solvers (Unstructured) - Shell .......................................................... 380
Parts - Solvers (Unstructured) - Beam ......................................................... 382
Motions ........................................................................................................... 384
Parts - Motions ................................................................................................ 384
Parts - Motions - Block ................................................................................ 385
Parts - Motions - I / J / K Plane .................................................................... 386
Parts - Motions - Node ................................................................................. 387
Parts - Motions - Modify ............................................................................... 388
Geometry ........................................................................................................ 389
Parts-Geometry - SPH .................................................................................... 389
Parts - Geometry - New/Modify ................................................................... 391
Parts-Geometry-Copy .................................................................................. 394
viii
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts-Geometry-Import Part ........................................................................ 395
Parts-Geometry-Translate ........................................................................... 398
Parts-Geometry-Rotate ............................................................................... 399
Components ....................................................................................................... 400
Components ....................................................................................................... 400
Components - New ......................................................................................... 402
Components - Modify ...................................................................................... 404
Components - Delete ...................................................................................... 406
Components - Material .................................................................................... 407
Components - Velocity .................................................................................... 408
Components - Initial Conditions ...................................................................... 409
Components - Apply Boundary ....................................................................... 410
Components - Clear Boundary ........................................................................ 411
Components - Translate .................................................................................. 412
Components - Rotate ...................................................................................... 413
Components - Scale........................................................................................ 414
Components - Copy ........................................................................................ 415
Groups ................................................................................................................ 416
Groups ................................................................................................................ 416
Groups - New .................................................................................................. 427
Groups - Rename............................................................................................ 428
Groups - Copy ................................................................................................. 429
Groups - Delete ............................................................................................... 430
Groups - Apply ................................................................................................ 431
Groups - Clear................................................................................................. 432
Groups - Material ............................................................................................ 433
Groups-Velocity ...................................................................................................... 434
Groups - Initial Condition ................................................................................. 435
Groups-Translate ............................................................................................ 437
Groups-Rotate................................................................................................. 438
Groups-Scale .................................................................................................. 439
Joins ................................................................................................................... 440
Joins ................................................................................................................... 440
Joins - Join ...................................................................................................... 446
Joins - Unjoin .................................................................................................. 448
Joins - Matrix ................................................................................................... 449
Merge Joined Nodes ....................................................................................... 450
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
ix
AUTODYN User Manual
Bonded Face Connections .............................................................................. 451
Interactions ......................................................................................................... 454
Interactions ......................................................................................................... 454
Lagrange/Lagrange ......................................................................................... 455
Interactions - Lagrange / Lagrange ................................................................. 455
Lagrange/Lagrange Introduction.................................................................. 457
Interactions - Lagrange / Lagrange - Create ................................................ 461
Interactions - Lagrange / Lagrange - Add .................................................... 462
Interactions - Lagrange / Lagrange - Remove ............................................. 464
Interactions - Lagrange / Lagrange - Matrix ................................................. 466
Interactions - Lagrange / Lagrange - Range ................................................ 468
Interactions - Lagrange / Lagrange - Friction ............................................... 469
Lagrange/Lagrange - 2D Gap Contact Options ........................................... 472
Interactions-Lagrange/Lagrange-2D Trajectory Contact Options ................ 476
Interactions-Lagrange/Lagrange-3D Gap Contact Options ......................... 480
Interactions-Lagrange/Lagrange-3D Trajectory Contact Options ................ 487
Euler/Lagrange (2D)........................................................................................ 494
Interactions - Euler / Lagrange (2D) ................................................................ 494
Interactions - Euler / Lagrange Introduction ................................................. 499
Interactions - Euler/Lagrange (2D) - New Polygon ...................................... 502
Interactions - Euler/Lagrange (2D) - Velocity ............................................... 503
Interactions - Euler/Lagrange (2D) - Porosity .............................................. 504
Interactions - Euler/Lagrange (2D) - New Interaction .................................. 505
Euler/Lagrange (3D)........................................................................................ 506
Interactions - Euler - Lagrange (3D) ................................................................ 506
Interactions - Euler / Lagrange (3D) - Select ............................................... 508
Interactions - Euler / Lagrange (3D) - Thickness ......................................... 510
Interactions - Euler / Lagrange (3D) - Joins ................................................. 512
Interactions - Euler / Lagrange (3D) - Weak Coupling ................................. 514
Detonation (2D) .................................................................................................. 517
Detonation (2D) ...................................................................................................... 517
Detonation (2D) - Point ................................................................................... 519
Detonation (2D) - Line ..................................................................................... 521
Detonation (2D) - Circle .................................................................................. 523
Detonation (2D) - Manual ................................................................................ 525
Detonation (3D) .................................................................................................. 526
Detonation (3D) .................................................................................................. 526
x
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Detonation (3D) - Point ................................................................................... 528
Detonation (3D) - Plane .................................................................................. 530
Detonation (3D) - Cylinder .............................................................................. 532
Detonation (3D) - Sphere ................................................................................ 534
Detonation (3D) - Manual ................................................................................ 536
Parallel................................................................................................................ 537
Parallel................................................................................................................ 537
Parallel - Add / Modify ..................................................................................... 540
Parallel - Copy................................................................................................. 542
Parallel - Sub-domains .................................................................................... 543
Parallel - Task Assignment ............................................................................. 545
Parallel Automatic Decomposition................................................................... 549
Automatic decomposition of Euler-FCT parts .................................................. 551
Parallel - Decomposition of beam parts .......................................................... 555
Output ................................................................................................................. 557
Output .................................................................................................................... 557
Output-Part Summary Variables ..................................................................... 564
Outputs-Results Files ...................................................................................... 567
User Variables .................................................................................................... 571
User Variables .................................................................................................... 571
User Variables - Add/Modify ........................................................................... 572
Controls .............................................................................................................. 574
Controls .............................................................................................................. 574
Controls-Mass scaling ..................................................................................... 584
Controls - Global Erosion ................................................................................ 587
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
xi
AUTODYN User Manual
AUTODYN User Manual
Overview
Overview
ANSYS AUTODYN is an explicit analysis tool for modeling nonlinear dynamics of
solids, fluids, gas, and their interaction, and forms part of the ANSYS Workbench
suite.
ANSYS AUTODYN provides a user-friendly graphical user interface (GUI),
combining pre-processor, solver and post-processor in the same windows
environment. A single executable performs simulations in both two and three
dimensions.
The GUI is laid out with buttons running horizontally along the top and vertically
down the left hand side of the main window. The horizontal group of buttons is
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
1
AUTODYN User Manual
referred to as the Tool Bar and the vertical group as the Navigation Bar. The Tool
Bar and Navigation Bar offer quick access to options also available through the Pulldown Menus.
The main window is composed of a number of Panels (View, Dialog, Message and
Command Line).
2
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Overview - Tool Bar
The Tool Bar (and the Navigation Bar) provides shortcuts to options available in the
pull-down menus.
The Tool Bar buttons and their use are described below.
Create a new model (this functionality is only available when AUTODYN is
started up outside ANSYS Workbench)
Open an existing model (this functionality is only available when AUTODYN is
started up outside ANSYS Workbench)
Save current model to current filename (this functionality is only available
when AUTODYN is started up outside ANSYS Workbench)
Open a results file
Open a settings file
Save current plot view parameters to a settings file
Print
Transform object – default to on
Transform light source
Rotate model
Translate model
Zoom function
Set view – brings up new window so that exact view can be set
Reset model
Fit model to view panel
Examine model
Profile window
Toggle wireframe mode (on/off)
Perspective on/off
Hardware acceleration on/off
Setup slide show
Create image of current view
Record slideshow
Create textslide
Show/hide Navigation Bar
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
3
AUTODYN User Manual
Manual/Automatic refresh
Refresh screen
Stop all plotting
4
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Overview - Navigation Bar
The Navigation Bar contains two groups of buttons.
The top group of buttons (View) let you control what you see in the View Panel.
From here you can access and modify plot settings, view history plots, and create or
view slide shows / animations :
The lower group of buttons (Setup) let you access dialog panels to set up your
model. Starting at the top button (Materials) and working down to the Run button,
you can build your model in the most efficient and logical way :
The Problem Setup section explains this procedure in detail:
The Run button at the foot of the bar is used to run (execute) problems :
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
5
AUTODYN User Manual
6
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Overview - Dialog Panel and Dialog Windows
When you select an option from the Navigation Bar, dialog for that option appears in
the Dialog panel :
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
7
AUTODYN User Manual
8
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
The Dialog panel generally contains input fields and buttons that access further input
options. Pressing a button in the dialog panel will display further dialog either within
the dialog panel or in a new Dialog Window that is opened :
At the bottom of all Dialog Windows there are three buttons.
The button with a question mark provides help on the current windows function.
The two other buttons are
(Cancel) and
(OK). Pressing the Cancel
button will close the window, without applying any of the changes that you made
within it. The OK button closes the window and applies your changes.
In certain cases, an Apply button will be present. This provides the ability to apply
any changes made within the window without closing the window.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
9
AUTODYN User Manual
In the dialog panel or dialog windows, input data that is required for a task to
complete is marked
(above). When you enter an appropriate value, the mark
changes to
(below). The OK button will remain inactive until you provide
appropriate values for all required fields :
10
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
11
AUTODYN User Manual
Overview - Command Line Panel
The command language will provide the user with the capability to
Record operations made in the GUI
Modify/Playback/repeat operations
Load operations previously saved to file
Setup models using the command language
This feature has Beta status and must be activated by the user by adding the
following lines above the Additional User Title option in the autodyn.ini file:
command_line_on
1
By activating this flag you accept that this is a Beta option and therefore may not be
as stable or robust as expected in a general release version.
The command line is initially inactive until a model is either loaded or created. To the
right of the message line there are 2 buttons in addition to the Message window
button that are related to the command line.
12
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Commands can be typed directly into the command line with multiple commands
being concatenated by using a ';' between the commands, i.e. PARTS:;TARGET to
select a part named TARGET. Useful/help information is output to the
Message/Output window. Note however that the command language is more easily
used when the command window is undocked from the main user interface.
The command line creates two command files:
1. autodyn.adc - this is located in the directory C:\Documents and
Settings\username\Local Settings\Temp and is overwritten every time a new
AUTODYN session is started.
2. ident.adc - this file is created every time a new model is created. If the model
is subsequently modified in a different AUTODYN session the new commands
are appended to this file. Therefore the ident.adc should contain all
commands that have been executed on the model since it was first created.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
13
AUTODYN User Manual
A typical series of commands will look similar to that shown below:
PARTS:
target
@ZONING
#OPERATION TYPE
= Zoning
#ZONING
= Predef
#PREDEF GEOMETRY = Box
X Origin
= 0.0000000E+00
Y Origin
= 0.0000000E+00
Z Origin
= 0.0000000E+00
DX
= 10.00000
DY
= 10.00000
DZ
= 10.00000
#GRADING I
= NO
#GRADING J
= NO
#GRADING K
= NO
@DO
@FILL
#OPERATION TYPE
= Fill
#FILL BY INDEX
= Block
I min
=
1
I max
=
11
J min
=
1
J max
=
11
K min
=
1
K max
=
11
#FILL WITH INITIAL CONDITION SET? = No
#FILL MATERIAL
= AL 2024
Density
= 2.785000
Int. Energy
= 0.0000000E+00
X Velocity
= 0.0000000E+00
Y Velocity
= 0.0000000E+00
Z Velocity
= 0.0000000E+00
#RADIAL VELOCITY = No
#ANGULAR VELOCITY = No
@DO
The 'PARTS:' command word is the name of the current command structure. (When
other parts of the interface are covered by the command line, each of the buttons on
the Navigation panel will be a command structure, i.e. Materials, Boundaries etc.)
The name of the part currently selected is then given, in this case it is called 'target'.
In this example the command being executed is a zoning command followed by a fill
command- @ indicates a command. To see the current list of available commands
'@?' can be typed at any time.
A # denotes an option. In the above example, #zoning allows you to choose from the
list of zoning options. Typing '?#' will give you the list of options – for zoning the
options are shown below:
For the example given here predef is chosen as the option. The predef zoning
option has a sub-option '#PREDEF GEOMETRY' which allows the user to choose
the predef they want to zone. In this simple example the box predef is chosen and
the required parameters have been set.
14
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
When all the parameters have been set the '@DO' command is issued which
executes the command.
The easiest way to use the command line and become familiar with the command
structure is to use the user interface to zone and fill parts as usual. The commands
will then be recorded and can then be edited and played back as described above.
Also, as can be seen in the picture above some guidance is given in the history
window for the syntax used to set options and parameters etc. should you choose to
type in the commands directly.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
15
AUTODYN User Manual
Overview - Undock Command Line
Press this button to detach the command line panel from the main user interface and
open it in a separate dialog window. If this window is then closed, the Command Line
docks back into the main user interface.
16
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
When the command line is detached from the main UI the command dialog panel
contains three separate lists. The 'Command History' is shown on the left hand side
and contains all valid commands executed in the current session. Multiple
commands can be selected from this list to be replayed. The Message/Output panel
is shown at the bottom. This provides the user with help if they request it and gives
any error messages when invalid commands are performed.
The 'Commands to be processed:' list behaves the same as the command line when
docked into the main UI but is much more user friendly and allows multiple lines to
be input before pressing the process button. Any commands selected from the
History list are copied into the 'commands to be processed:' panel and can then be
edited before being processed.
The example above shows how you can replay a zoning operation. In this case the
DZ parameter is modified before the command is re-processed.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
17
AUTODYN User Manual
Overview - Command File Window
The command file window allows you to open an existing AUTODYN command file
using the 'File' button.
The commands can be executed/modified in a number of ways. Select all or a
number of the commands and press the process button. Alternatively, if you want to
modify the commands before execution, simply select the required commands. The
commands are then copied to either the single command line or the 'Commands to
be processed:' list (if the command line is not docked to the main UI). The
commands can then be modified before execution by either pressing return on the
single command line or the process button in the Command line panel.
18
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
If the 'Run on Load' option is selected the commands in the selected file can
automatically be run on loading the file, or alternatively the user is given the option to
interactively step through the commands.
If stepping through the command file the user is shown the next command before
processing it. If at any stage 'No' is selected AUTODYN stops reading the file.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
19
AUTODYN User Manual
Overview - Message Panel
The message panel shows a variety of messages during problem setup, execution
and viewing.
Clicking the M box at the top right corner of the message panel will open a scrollable
window showing all the messages displayed during your session.
20
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Overview - HTML review windows
While working on a model, you may want a summary of particular data such as
material properties, detonation point or gauge point locations. These are created as
an HTML document and displayed in a browser window. You can easily insert these
documents into reports and publications.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
21
AUTODYN User Manual
Overview - File names
AUTODYN file names have the underlying format of Name_information.extension.
Examples:
A cycle zero Save file would be named myfilename_0.ad
The Save file for cycle 12500 would be named myfilename_12500.ad.
22
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Overview - On-Line help
The documentation and help pages for AUTODYN have been merged into a single
context sensitive HTML documentation system.
All documents are accessible from the AUTODYN graphics user interface.
Pressing
browser.
(Help) bring up context sensitive help pages in your default web
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
23
AUTODYN User Manual
Overview - Supported Operating Systems and Compilers
The following operating systems are supported at release 12.0 of ANSYS
AUTODYN.
System
Windows XP Pro, 32
bit
Windows Vista, 32 bit
Windows XP Pro,
64bit
Windows Vista, 64bit
RedHat EL 4 (Update
5)
SUSE 10
C++
Microsoft Visual
Studio
C++ .NET 2005
Microsoft Visual
Studio
C++ .NET 2005
Fortran
Intel Fortran
10.1
Intel Fortran
10.1
Intel Fortran
10.1
Intel Fortran
10.1
32 Bit Linux
RedHat Enterprise Linux AS release 4 (Update 5)
64 Bit Linux (x86-64)
SUSE Professional 10
64 Bit Linux (Itanium II)
RedHat Enterprise Linux AS release 4 (Update 5)
Third Party Software Requirements for Parallel
System
Parallel Environment
Windows XP Pro, 32 bit
Windows Vista, 32 bit
Windows XP Pro, 64 bit
Windows Vista, 64 bit
RedHat EL 4 (Update 5)
SUSE 10
WMPI 1.6.1
WMPI 2.4.2
HP-MPI*
HP-MPI*
*See Chapter 1.1 (Prerequisites for Running Distributed ANSYS) of the "Configuring
Distributed ANSYS" section of the Installation and Licensing Documentation for the
version of HP-MPI that is supplied as part of the installation.
24
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Overview - Initialization Settings
AUTODYN is installed with a pre-configured file called autodyn.ini, which is in the
users Application Data directory, in the sub folder Ansys\v120\AUTODYN. This is
the contents of the file after installation :
AUTODYN_initialization_file
application_window_width
1000
application_window_height
700
message_window_visibility
0
manual_refresh_default
0
background_color
1
hardware_acceleration
1
reset_plot_flags
0
plot_wireframe
0
plot_perspective
0
model_interactivity_default
0
graded_background
1
OpenGL_for_slides
1
remove_joined_faces
0
open_new_browser_window
1
enable_beep
0
mouse_option_rotate
2
keyboard_option_rotate
0
mouse_option_zoom
3
keyboard_option_zoom
0
mouse_option_translate
2
keyboard_option_translate
2
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
25
AUTODYN User Manual
mouse_option_toolbar
1
keyboard_option_toolbar
0
mouse_option_examine
1
keyboard_option_examine
3
mouse_option_boxzoom
3
keyboard_option_boxzoom
2
use_prepost_only
0
additional_user_title
You can alter the contents of this file to customize the startup of AUTODYN.
You can use any text editor to make your changes (e.g. Notepad or MS Word).
You can set the following parameters in this file.
Application window width
This sets the width of the AUTODYN application window at startup.
Application window height
This sets the height of the AUTODYN application window at startup.
Message window visibility
This switch sets the visibility of the message window on startup.
0
1
Message window hidden
Message window visible
Manual refresh default
This switch sets manual refresh on or off. For large models you may want to have
full control on the refreshing of the plot window.
0
1
Manual refresh off
Manual refresh on
Background color
This switch sets the color of the background for the View Panel on startup.
26
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
0 Black background
1 White background
Plot wireframe
This switch sets the wireframe plotting option on or off on startup.
0
1
Plot wireframe off
Plot wireframe on
Plot perspective
This switch sets the perspective plotting option on or off on startup.
0
1
Plot perspective off
Plot perspective on
Hardware acceleration
This switch sets hardware graphics acceleration on or off on startup.
0
1
Hardware graphics acceleration off
Hardware graphics acceleration on
Model Interactivity default
This switch sets the default model interaction setting for the toolbar mouse/keyboard
combination on startup.
1
2
3
Translate model
Rotate model
Zoom in/out
Reset plot flags
This switch sets reset plot flags on or off.
If this flag is on, when you load a new model (or a different cycle of the current
model) the plot settings for all Parts will be reset to default values (e.g. default view,
material locations, etc.).
If this flag is off, when you load a new model (or a different cycle of the current
model) with a model already present, the plot settings (grid, material location,
material status, contour) for the current model are migrated to the new model for
each Part with the same name.
0
1
Reset plot flags off
Reset plot flags on
Graded background
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
27
AUTODYN User Manual
This switch sets graded background on or off. If this switch is on a graded
background color is used. If this switch is off a solid black or white color is used
depending on Background color setting.
0
1
Graded background off
Graded background on
OpenGL for Slide creation
This switch sets OpenGL for Slide creation on or off. Using OpenGL during the
creation of slides can cause problems for some graphics cards. If you experience
any problems creating slides with this switch turned on, try turning it off.
0
1
OpenGL off for slide creation
OpenGL on for slide creation
Browser Options
By default, when AUTODYN opens an html document (either for the on-line help, or
for the summary reviews), the page will be displayed in any browser that is currently
open. By setting this flag to 1, a browser will be opened to display the information.
This option may not work for all browsers.
Warning Sound Options
This option lets you enable or disable the warning beep
Mouse and Keyboard options
These options let you set the mouse and keyboard combinations for interaction.
Each action type has a keyboard and an associated mouse option. A default will be
used if any are not defined.
Mouse
0
Not used
1
Left Mouse Button
2
Middle Mouse Button
3
Right Mouse Button
Keyboard
0
None
1
Shift
2
Control
3
Alt
Mouse Option Rotate & Keyboard Option
Rotate
Mouse Option Zoon & Keyboard Option
Zoom
28
Rotate mouse and keyboard
combination
Zoom mouse and keyboard
combination
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Mouse Option Translate & Keyboard
Translate mouse and keyboard
Option Translate
combination
Mouse Option Toolbar & Keyboard Option
Toolbar mouse and keyboard
Toolbar
combination
This is the default combination for the interaction type selected on the toolbar
Mouse Option Examine & Keyboard Option
Examine mouse and keyboard
Examine
combination
Mouse Option Boxzoom and Keyboard
Box zoom mouse and keyboard
Option Boxzoom
combination
PrePost license usage
By default this switch is set to zero and AUTODYN will start up using a solver
license. When the switch is set to zero AUTODYN will start up using a PrePost
license only.
Additional user title
This option lets you add additional information below the top left hand corner of the
View Panel.
You can enter up to 256 characters. The Additional User Title should always be the
last option in the file.
Command Line Options
This feature has Beta status and can be activated by the user by adding the
following lines above the Additional User Title option in the autodyn.ini file:
command_line_on
1
By activating this flag you accept that this is a Beta option and therefore may not be
as stable or robust as expected in a general release version.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
29
AUTODYN User Manual
Slide Viewer
The View Slides option on the Navigation Bar starts the Slide Viewer (it can also be
run independently of AUTODYN).
The Viewer lets you load and view GIF and GFA animations.
Components of the Viewer's user interface :
View Window
This is where your animations are shown.
Pull-down Menus
30
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
File
This pull-down menu lets you load single GIF and GFA animation files for
playback, and exit the program.
Sequence
This pull-down menu lets you playback multiple GIF animations using
sequence files.
A sequence file contains a list of GIF animations you want to view
consecutively.
All the animations in a sequence file must be in the same directory as the
sequence file.
New Sequence File
This option opens a new sequence file.
Open Sequence File
This option opens an existing sequence file.
Edit Sequence
This option lets you insert and delete animations in the current sequence
file.
The following dialog window appears when you select this option :
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
31
AUTODYN User Manual
Sequence list
The box at the top of this dialog contains a list of the animations
currently included in the sequence, together with their time delay
(how long the first slide in the sequence is shown, in seconds).
Insert
Press this button to insert another animation immediately after the
selected animation.
Delete
Press this button to delete the selected animation.
Delay
Enter a time delay in this field (in seconds). When you Insert an
animation, this time delay is applied.
You can create and edit sequence files manually if you wish. Sequence
files must have a .seq extension and use the following format
Format
Example
The number of animations 3
in the sequence
32
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
0.0 anim.gif
Default frame delay in
seconds + <space> + file
name
Default frame delay in
seconds + <space> + file
name
1.2
another.gif
1.6
yetanother.gif
Default frame delay in
seconds + <space> + file
name
etc.
Save As
This option saves the current sequence file (.seq)
Control
This pull-down menu provides the same functions that are available in the
Control Bar.
Control Bar
This bar lets you control the playing of the GIF or GFA animation you have loaded.
Pressing a button on this bar performs the following actions (you can type the
corresponding Hotkey as an alternative to pressing the a button).
Button
Hotkey Action
Go to the first frame of the
b
animation
r
Go back one frame
x
Play (from the current frame)
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
33
AUTODYN User Manual
p
s
a
e
Pause (at the current frame).
This is a toggle button.
Stop (at the current frame)
Advance one frame
Go to the last frame of the
animation
View Bar
This bar only appears when you have loaded a GFA animation.
The buttons on this bar let you control how you view your GFA animation and work in
the same way as the corresponding icons in the AUTODYN Tool Bar
Rotate view
Translate view
Zoom in or out
Set view (brings up a window that allows you to set an exact view)
Reset view (to the initial view)
Turn perspective on or off (toggle)
Frames Slider
This slider lets you move quickly to any frame in the animation(s).
Speed Slider
This slider lets you adjust the playback speed for animations.
Loop
Check this box if you want the animation(s) to automatically start again from the first
frame when the last frame is reached.
34
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Overview - AUTODYN in Workbench
An overview of how to access AUTODYN in Workbench at release 12 is provided
below. Full guidance on how to use Workbench at release 12 is provided in the online help system of Workbench.
A new paradigm for managing simulations is used with the ANSYS Workbench GUI
at release 12. The ANSYS Workbench GUI now consists primarily of a Toolbox
region, Project Schematic, Toolbar, and menu bar. Depending on the analysis type
and/or application or workspace, you may also see other windows, tables, charts, etc
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
35
AUTODYN User Manual
One way to work in ANSYS Workbench is to drag an item such as a component or
analysis system from the Toolbox to the Project Schematic or to double-click on an
item to initiate the default action. You can also use the context menus, accessible
from a right-mouse click, for additional options. You will view your analysis systems
-- the components that make up your analysis -- in the Project Schematic including
all connections and links between the systems. The individual applications in which
you work will display separately from the ANSYS Workbench GUI, but the results of
the actions you take in the applications may be reflected in the Project Schematic.
Full details of how to use ANSYS Workbench are provided in "Workbench Help"
section of the Workbench on-line help system.
An ANSYS AUTODYN product license should enable three primary systems in the
Toolbox of the Workbench GUI.
AUTODYN System
The AUTODYN system is located in the Component Systems toolbox of the
Workbench GUI. This system allows you to start-up the traditional ANSYS
AUTODYN application and includes pre-processing, solve and post-processing
options for all AUTODYN solvers.
To start-up the AUTODYN application simply insert an AUTODYN system into
the project schematic. Then double click the Setup cell.
The AUTODYN application will start-up and you can setup, solve, post-process
models in the familiar AUTODYN user interface. The default start up mode will
be the generation of a new model. The start up mode can be changed by rightmouse click the Setup cell after which you can select:
36
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
New Model - default
Import Model - open existing
AUTODYN Save file
Select user executable - defines
where a user customized version of
AUTODYN resides
Duplicate - makes a copy of the
model file
Transfer Data From - Model data from
either the Mesh system or the Explicit
Dynamics system are imported into
AUTODYN
After selection of the desired Setup cell setting double clicking the Setup cell
again will start up AUTODYN in the required mode.
Notes:
Model Name: The database for an AUTODYN model will now always
be admodel_0.ad. The project name is the now unique identifier for all
databases (see below).
2D/3D symmetry: By default, the AUTODYN application assumes you
are performing a 3D simulation in the default unit set (mm, mg, ms).
To define 2D axial or planar symmetry, use the Setup, Symmetry
option in the toolbar after start-up of the AUTODYN application.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
37
AUTODYN User Manual
Saving a project: To save a model, the recommended approach is to
save the Workbench project either from within the AUTODYN
application (File, Save Project) or from the project page of Workbench.
This ensures all data used in the AUTODYN Simulation is saved to
disk.
Exporting an AUTODYN database: The AUTODYN database (restart
file) can be exported to a file (independent of the Workbench project)
using the File, Export options in the AUTODYN application.
Please refer to the "Component Systems, AUTODYN" section of the
Workbench On-line help for further details on the operations and properties
available for an AUTODYN system.
Explicit Dynamics (ANSYS) system
The Explicit Dynamics (ANSYS) system is located in the "Analysis Systems"
toolbox of the Workbench GUI. This system allows you to completely setup,
solve and post-process an explicit dynamics simulation with the ANSYS
Mechanical Workbench user environment. At release 12, this user interface
fully supports the 3D Finite Element features of ANSYS AUTODYN
(unstructured Lagrange solvers, isotropic inert materials and linear orthotropic
materials).
The system contains a number of unique features for explicit dynamic
simulation inside Workbench:
Unidirectional and bidirectional links to CAD geometry
Links to Design Modeler
38
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Advanced meshing capabilities tailored for Explicit analysis
Mesh independent loading and boundary conditions
Fully parameterized engineering data, geometry, initial conditions,
loads, boundary conditions
Automated "What If" analysis capability
Links to design exploration tools
The full capabilities of the ANSYS Explicit Dynamics system are described in
the online help for the Mechanical analysis systems in Workbench.
Models setup in the ANSYS Explicit Dynamics system can be persistently
linked to an AUTODYN system to transfer material data, mesh, connections,
loads and constraints, analysis settings etc... into ANSYS AUTODYN.
For modeling complex geometries in ANSYS AUTODYN, we recommend you
define the FE components of the model in an ANSYS Explicit Dynamics
system then transfer the model setup to the AUTODYN system and add on
your Euler-SPH regions and explicit FSI/Coupling as required.
Mesh system
The Mesh system is located in the Component Systems toolbox of the
Workbench GUI. This system allows you to link to your model geometry and
generate a mesh. The mesh can then be transferred to an AUTODYN system
for subsequent analysis.
This system allows you to use a similar workflow that was available at release
11 to link AUTODYN models to CAD/geometry and meshing tools. However
with Version 12 the link is not persistent anymore, which means that with every
update of the workflow system the definitions made in AUTODYN (material
filling, boundary condition assignment, etc.) are lost and have to be re-applied.
Therefore at release 12, we recommend using the ANSYS Explicit Dynamics
system to link to CAD/geometry and generate a mesh for use in AUTODYN
where loads, constraints and material assignments are maintained after any
change to the geometry or mesh.
Linking different systems
If the mesh/geometry of the application to be solved in AUTODYN cannot be made
with the simple model building tools available in the AUTODYN application, we
recommend the following approaches to build the AUTODYN model.
ANSYS Explicit Dynamics => AUTODYN
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
39
AUTODYN User Manual
The recommended approach for bringing Lagrangian FE based models with complex
geometries into AUTODYN is to start off with an ANSYS Explicit Dynamics system.
Define material data using the Engineering Data application
Link directly to CAD Geometry or use DesignModeler to generate geometry
directly or adapt CAD geometry for simulation purposes
Mesh the geometry and define connections (Contact, Joins, Spotwelds)
Optionally:
Assign initial velocities to components
Apply loads and constraints directly to the geometry
Define solution controls and outputs
Solve and Post process results
To transfer the model from an ANSYS Explicit Dynamics system to the AUTODYN
application, link the Setup cell of the ANSYS Explicit Dynamics system to the Setup
cell of the AUTODYN system. Open the AUTODYN application by double click on
the AUTODYN system Setup cell. All relevant model information defined in
Engineering Data, Geometry, Model and Setup components of an ANSYS Explicit
Dynamics system are transferred into the AUTODYN application.
Once in the AUTODYN application, you can complete the model setup (for example,
add Euler and SPH regions) then solve in the AUTODYN application.
The link generated between the AUTODYN and ANSYS Explicit Dynamics system is
persistent. You can make changes to the model defined in the ANSYS Explicit
Dynamics system, update the ANSYS Explicit Dynamics system Setup cell, then
update the AUTODYN system Setup cell. The latest model definition will be
transferred into the AUTODYN model while retaining additional features present only
in the AUTODYN application. This makes it very easy to make changes to model.
40
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Notes:
Changes made to the model in the AUTODYN application are NOT
transferred back to the ANSYS Explicit Dynamics system. The link is one
way.
To avoid overwriting changes you make in the AUTODYN application, we
recommend that if a portion of the model is defined in the ANSYS Explicit
Dynamics system (for example and initial velocity) then only make changes to
this in the ANSYS Explicit Dynamics system. Transfer to the AUTODYN
model using the update procedure described above.
Local co-ordinate systems defined and used in the ANSYS Explicit Dynamics
system are transferred through to the AUTODYN application however they
cannot be reviewed or modified in AUTODYN.
Displacement boundary conditions defined in the ANSYS Explicit Dynamics
system are converted to equivalent velocity boundary conditions in the
AUTODYN application.
Loading defined in tabular form in the ANSYS Explicit Dynamics system
cannot be edited or reviewed in the AUTODYN application. The data is
transferred and used in the AUTODYN simulation.
Spot weld breaking criteria defined in the ANSYS Explicit Dynamics system
will be converted from a stress to a force criterion
Meshing => AUTODYN
If you only want to transfer a Mesh (of complex geometry) into AUTODYN then this
can be achieved (as in release 11.0) using a Mesh system. Start by inserting a
Mesh system from the Components toolbox.
Link directly to CAD Geometry or use DesignModeler to generate geometry
directly or adapt CAD geometry for simulation purposes
Mesh the geometry
Create Named Selections
To transfer a mesh from the Mesh to the AUTODYN application, link the Mesh cell of
the Mesh system to the Setup cell of the AUTODYN system. Open the AUTODYN
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
41
AUTODYN User Manual
application by double clicking on the AUTODYN system Setup cell. The mesh and
Named selections will be transferred to AUTODYN.
With Version 12 the link generated between the AUTODYN and Mesh system is not
persistent anymore. This means that with every update of the workflow system the
definitions made in AUTODYN (material filling, boundary condition assignment, etc)
are lost and have to be re-applied.
Therefore at release 12, we recommend using the ANSYS Explicit Dynamics system
to link to CAD/geometry and generate a mesh for use in AUTODYN, where loads,
constraints and material assignments are maintained after any change to the
geometry or mesh.
Notes:
Connections defined in the Mesh system will not be transferred to the
AUTODYN application.
Material assignments, Boundary Conditions and Loads defined in the
AUTODYN application will be lost during the update and will have to be reapplied.
FEModeler
Legacy and third party FE model data can be imported into the FEModeler system in
Component toolbox. This data can be transferred into AUTODYN via a Mesh
system or an ANSYS Explicit Dynamics system.
Note: Direct transfer of data from the FEModeler application into AUTODYN is not
possible at release 12.
Data Transferred by linking different systems to AUTODYN
Node Coordinates
The nodal coordinates are transferred.
Mesh Elements
The mesh elements are transferred, noting that Pyramid elements are not supported
within AUTODYN, so these are converted into two tetrahedra.
Body Definitions
The definitions of bodies in the Workbench are imported as Parts in AUTODYN.
In addition, for Meshing, Simulation and Finite Element Model Objects, the following
are transferred.
Parts Definitions
42
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
The definitions of parts (both multi body parts and single body parts) are shown as
Components in AUTODYN.
Named Selection
The named selections are represented as Groups in AUTODYN. Note that the face
named selection is transferred as a face group; all other named selections are
transferred as node groups.
Unit Setup
All models are transferred to AUTODYN in units of mm, mg, ms.
Material Associations
Each Body (AUTODYN Part) transferred is assigned a separate material.
Shell thickness
Shell parts will be assigned with the thickness as defined in the Workbench object.
An initial condition will be created for each part.
Beam Cross-Sections and Orientations
The beam cross sections associated to elements and their orientations are
transferred and applied correspondingly.
In order to update the model in AUTODYN to that in the currently selected project
page item, use the 'Update Model from Workbench' option, found in the Import menu
or on the toolbar. This function will update the parts that are in AUTODYN to reflect
the mesh in Workbench. If a part contains a single material then the updated parts
will be refilled with any materials and initial conditions that are associated. New
parts are added to the model as appropriate, deleted parts should be manually
removed from the AUTODYN model.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
43
AUTODYN User Manual
Overview - AUTODYN solver options in Workbench
There are a number of AUTODYN solver options, which may be changed by rightmouse click the Setup cell of the AUTODYN system.
Precision
Note that by default, the single precision version of AUTODYN will be used. To run
in double precision, from the ANSYS Workbench project schematic, right click the
Setup cell of the AUTODYN system and select Properties after which the Properties
window will pop up where you can select what type of executable you want to run.
User Executable Location
By default, Workbench will start the standard AUTODYN executable. You may also
choose an executable created with a user-subroutine. To run your own user
executable from the project schematic, right click the Setup cell of the AUTODYN
system and left click Select user executable, after which you will be asked for the
user executable name and locaton.
44
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Pull-down Menus
Pull-down Menus
Pull-down menus let you access all the features and dialog panels/windows in
AUTODYN.
Most options can also be accessed through buttons on the Tool Bar and Navigation
Bar.
Options that are only accessible through pull-down menus are shown below in red.
Options that only are available when AUTODYN is started outside the Workbench
environment are shown below in green.
File
Import
Setup
Execution
View
Options
Help
New
from TrueGrid
(.zon)
Description
Run
Interactively
Plots
Interactivity
Contents
Plot Settings
Clipping
Planes
About
Open
Symmetry
Open
Results
File
from ICEMCFD
(.geo)
Material
from LS-DYNA
(.k)
Initial
Conditions
from
MSC.NASTRAN
bdr (.dat)
Boundary
Convert IJK to
unstructured
Components
Batch
Runner
History
Graphs
Slideshow
Save
Save
Project
Save As
Save As
Version
Parts
Default
Settings
Performance
Profiler
Pause
License
Create
UserSubroutine
Project
Groups
Joins
Export to
Version
Interactions
Manage
Folders
Detonation
Parallel
Save
settings
Controls
Load
settings
Output
User
Variables
Print
Export
PostScript
Export
VRML
Save
Formatted
Export
Formatted
Open
Formatted
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
45
AUTODYN User Manual
Import
Formatted
46
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
File
Pull-Down Menu-File
This pull-down menu lets you perform file operations.
New
Lets you create a new model
Open
Lets you open (load) an existing model saved in a binary file.
Open Results Files
Lets you open an existing results file. For more details of results files, see the
section Outputs - Results Files.
Save
Lets you save the current model using the current Ident for the filename to a binary
file.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
47
AUTODYN User Manual
Save Project
Lets you save the Workbench project and ensures that the AUTODYN analysis
model and all Workbench related data is saved to disk.
Save As
Lets you save the current model using a new Ident for the filename.
Save As Version
Lets you save the current model in a format supported by a previous version.
Export to Version
Lets you save the current model outside the Workbench project in a format
supported by a previous version.
Manage Folders
Lets you manage your project folders.
Save settings
Lets you save the settings for the current plot in a settings file.
Load settings
Lets you load and apply plot settings from a saved settings file.
Print
Lets you output data for the current plot to a printer.
Export PostScript
Lets you output data for the current plot to a PostScript file.
Export VRML
Lets you output data for the current plot to a VRML file.
Save Formatted
Lets you save the current model using the current Ident for the filename to a
formatted (ascii) file.
Export Formatted
Lets you save the current model to a formatted (ascii) file.
48
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Open Formatted
Lets you open (load) an existing model saved in a formatted (ascii) file.
Import Formatted
Lets you open (load) an existing model saved in a formatted (ascii) file.
Close AUTODYN
Lets you exit AUTODYN.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
49
AUTODYN User Manual
Pull-down Menu - File - New
This menu is only available when AUTODYN is started outside Workbench.
This window lets you start the creation of a new model.
Folder
This box shows you the folder where files for the model will be kept.
Press the Browse button to select a different folder.
Press the Folder List button to select a folder from your current list of folders or
manage your folder list
Ident
Enter an Ident for your model in this field.
The ident you choose is used to identify all the files created for your model.
e.g. If your Ident is MyImpactProblem, then the cycles zero Save file for the
problem will be named MyImpactProblem_0.ad.
50
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Heading
Enter a heading for your model in this field.
Headings appear in plots and other output for your model.
Description
Enter a more detailed description of your model here if you want.
Symmetry
Select the dimension (2D or 3D) and symmetry you want to use for your model.
In 2D you must choose either Axial or Planar symmetry
In 3D you do not need to choose a symmetry, but you can optionally select X, Y
and/or Z symmetry.
(e.g. if you select X symmetry, then the plane X=0 is assumed to be a symmetry
plane).
Units
Select the units of length, mass and time you want to use for your model.
The default units (mm,mg,ms) will give good results, with small rounding errors, for
most models.
US Customary Units
US customary units have been added to units options when creating a new model.
These are
Length unit (inch or foot)
Mass unit (pound)
These units can be written in short as "in", "ft", and "lb". One of the three time units
can be used in conjunction with the US customary units: microsecond, millisecond,
or second.
Note they cannot be used together with Metric Units. For example, you cannot use
inch for length unit and kilogram for the mass unit.
The following table shows the unit for each type of physical variables in the US
customary system:
Length
Mass
in, lb,
s
in
lb
in, lb,
ms
in
lb
in, lb,
s
in
lb
ft, lb,
s
ft
lb
ft, lb,
ms
ft
lb
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
ft, lb,
s
ft
lb
51
AUTODYN User Manual
Time
Temperature
Density
Inertia
Volume
Force
Pressure
Impulse
Velocity
Work
Strain Rate
Energy
Energy/Unit
Mass
Energy/Unit
Volume
Fracture
Energy
Fracture
Toughness
Squared
Specific Head
Capacity
Thermal
Conductivity
s
K
lb.s2/in4
lb.s2.in
in3
lb
psi
lb.s
in/s
lb.in
1/s
lb.in
in2/s2
ms
K
lb.ms2/in4
lb.ms2.in
in3
lb
psi
lb.ms
in/ms
lb.in
1/ms
lb.in
in2/ms2
s
K
lb. s2/in4
lb. s2.in
in3
lb
psi
lb. s
in/ s
lb.in
1/ s
lb.in
in2/ s2
s
K
lb.s2/ft4
lb.s2.ft
ft3
lb
psf
lb.s
ft/s
lb.ft
1/s
lb.ft
ft2/s2
ms
K
lb.ms2/ft4
lb.ms2.ft
ft3
lb
psf
lb.ms
ft/ms
lb.ft
1/ms
lb.ft
ft2/ms2
s
K
lb. s2/ft4
lb. s2.ft
ft3
lb
psf
lb. s
ft/ s
lb.ft
1/ s
lb.ft
ft2/ s2
lb/in2
lb/in2
lb/in2
lb/ft2
lb/ft2
lb/ft2
lb/in
lb/in
lb/in
lb/ft
lb/ft
lb/ft
lb2/in2
lb2/in2
lb2/in2
lb2/ft2
lb2/ft2
lb2/ft2
in2/s2.K
in2/ms2.K
in2/ s2.K
ft2/s2.K
ft2/ms2.K
ft2/ s2.K
lb.s/K
lb.ms/K
lb. s/K
lb.s/K
lb.ms/K
lb. s/K
Micron Unit System
A new micron ( m) length system has been introduced. This can be used in
conjunction with a mass unit of picogram (pg) and time unit of microsecond or
millisecond.
52
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Manage Folders
Pull-down Menu - File - Manage Folders
This menu is only available when AUTODYN is started outside Workbench
This window lets you manage a list of the folders containing your AUTODYN models.
You can add and delete folders from this list as your projects change.
Folder List
The scroll box contains a list of the current folders you have selected. For each
folder you see its alias (if defined) followed by its full path name in parentheses.
Double clicking on any folder in this list selects it as the directory for your current
model.
Select / Create Folder
Press this button to add another folder to your list (using a browser). After selecting
the directory for the folder, you can optionally specify an alias for the folder.
Remove Folder from list
Press this button to remove the selected folder from your list.
View Folder Contents
Press this button to view the model files in the selected folder.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
53
AUTODYN User Manual
Manage Folders - New Folder
This window lets you define an optional alias name for a folder.
Enter the alias name in the field provided.
If you leave this field blank, the full folder name will be used to reference the folder.
54
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Pull-down Menu - File - Save As
This menu is only available when AUTODYN is started outside Workbench
This window lets you save the current model under a new Ident.
Folder
This field shows the current folder in which model files are saved.
Browse
Press this button to browse to a new folder for saving model files.
Folder List
Press this button to select a folder from your folder list for saving model files and/or
manage your folder list.
Ident
Enter the new Ident you want to use for saving model data.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
55
AUTODYN User Manual
PullDown Menus - File - SaveProject
This option brings up the Workbench project page and allows you to save the current
Workbench project and ensures that the AUTODYN analysis model and all
Workbench related data is saved to disk.
Save in
This field shows the current folder in which the Workbench project tree is saved and
the user can select a different folder if required.
File Name
The user defined project name.
56
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Pull-down Menu - File - Save As Version
This menu is only available when AUTODYN is started outside Workbench.
This option lets you to "Save" an AUTODYN save file in the format supported by
previous versions. The formats available are listed and the chosen format should be
selected from the list.
As features and options available in the current version, but not in the version
selected, will be lost, we recommend that you always choose a new filename when
using this option.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
57
AUTODYN User Manual
PullDownMenus - File - Export To Version
This option lets you "Save" an AUTODYN save file in the format supported by
previous versions. The formats available are listed and the chosen format should be
selected from the list.
As features and options available in the current version, but not in the version
selected, will be lost, we recommend that you always choose a new filename when
using this option.
58
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Pull-down Menu - File - Export PostScript
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
59
AUTODYN User Manual
This window lets you output the current plot to a PostScript file.
60
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
PS file
Enter the name of the PostScript file in this field (use the Browse button to navigate
to a directory/file if you wish).
Dynamic
Check this box if you want a new PostScript file to be output each time the input view
is rendered. Otherwise, you must explicitly request a new file by pressing the Write
PostScript button.
Write PostScript
If Dynamic is not checked, press this button to generation of a PostScript output file.
Color Mode
This pull-down menu lets you select the color format used in the output file.
Color
Each color is specified as an RGB triple in the output file. The output file can be
rendered in color on a color printer, or in greyscale on a monochrome printer.
Greyscale
Each color is converted to a single intensity value. The output file can only be
rendered in greyscale, on color or monochrome printer. Greyscale files will be
smaller than those written with full color information.
Background Mode
This pull-down menu lets you select how the background of the scene will be
rendered.
White
Force the scene to be rendered on a white background. This typically means
that the printer does not apply any color or shading to the background.
Black
Force the scene to be rendered on a black background.
Keep
Use the view background color specified in the AVS/Express viewer, as the
PostScript background color.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
61
AUTODYN User Manual
Orientation
This pull-down menu lets you select the page layout.
Landscape
The x-axis of the scene device coordinates is oriented along the longer side of
the paper.
Portrait
he x-axis of the scene device coordinates is oriented along the shorter side of
the paper.
Size
This pull-down menu lets you select the paper size for the output.
EPS (user)
Encapsulated PostScript format, where you can specify the dimensions of the
output, and the resulting file can be embedded in other documents. You must
set the width, height and margin in the fields provided if you select this option.
A (letter)
Standard US letter paper size (280mm x 216mm)
B
Ledger paper size (432mm x 280mm).
A4
Standard European A4 paper size (297mm x 210mm).
A3
A3 paper size (420mm x 297mm).
A0
A0 paper size (1189mm x 841mm).
Width, Height, Margin
Use these fields to specify the width and height and margin of EPS size output if this
option is selected.
62
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Color Subdivision
This pull-down menu lets you select how the color is interpolated for polylines and
surfaces, in 2D and 3D, with per-vertex color or lighting of 3D surfaces. When
subdivision is enabled (Precompute or Postcompute), the subdivision proceeds
until a color tolerance is reached. This adaptive method gives the best quality results
without subdividing primitives with small color gradients.
None (flat)
No color interpolation is performed. The output polyline and triangle primitives
are drawn with constant color per-segment, or per-facet. Incoming vertex
colors are averaged to produce the segment or facet color, where necessary.
Precompute
The OutputVPS module subdivides line segments and triangles that have pervertex color from data mapping, or as the result of lighting 3D surfaces. The
subdivision generates many smaller primitives with linearly interpolated color.
Precomputing the subdivision increases the output file size, and the subdivision
cannot be changed during printing.
Postcompute
Special interpolation macros are written to the output file, together with the
color tolerance parameter. Primitives are written with color per-vertex
information in the PostScript output. The subdivision is made at print time, in
the PostScript processor. This gives high quality output, with small file size, at
the expense of slower printing. The color tolerance parameter can be edited by
hand to change the color resolution after the file has been generated.
Color tolerance
Use this field to specify the absolute difference in color space, for the color
subdivision algorithms: Precompute and Postcompute. In Postcompute mode, the
color tolerance is written to the output file. In precompute mode it is used by the
OutputVPS module to subdivide the line segments and triangle facets which have
per-vertex color. This real value must be in the range 0.0 to 1.0. Smaller values
signify a finer subdivision. Values close to zero will force a very large number of
primitives to be generated, either precomputed in the output file (large file, slow
printing), or postcomputed internally within the printer (slow printing). A value of 1.0
will not cause any subdivision to occur, even when it is enabled by the subdivision
flag. The color tolerance user interface is not displayed for color subdivision None.
Depth Sort Algorithm
Select the depth sort algorithm you want to use from the pull-down menu.
Default
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
63
AUTODYN User Manual
A simple sort by the minimum z coordinate of each primitive object. While this
is well suited for many applications, it can result in visual artifacts in complex
scenes.
NNS
The Newell and Sancha hidden surface removal algorithm. When a possible
visual artifact is detected, the algorithm first tries to interchange the conflicting
primitives. If there is still a conflict (consider the case of intersecting triangles),
then one of the primitives is split along the
line(s) of intersection.
Gamma Correction
This pull-down menu lets you select how final colors are modified to take account of
non-linear effects in the printing device, or perhaps to match the non-linear effects of
the same scene displayed on a raster monitor.
None
No gamma correction is performed. Color values are assumed to behave
linearly.
Precompute
The OutputVPS module modifies all color values (gray, red, green, blue),
before writing the values to the file. Thus precomputed gamma correction is
applied after precomputed color subdivision, but before postcomputed color
subdivision. This means that postcomputed linear interpolation may not give
the expected appearance. Precomputed gamma marginally slows file
generation, but does not affect file size. The precomputed gamma factor
cannot be changed after the file has been generated.
Postcompute (default)
The gamma exponent is written to the output file, and an exponential function
is set for color transfer in the printer. Each rendered color is then gamma
corrected at print time. Postcomputing the gamma correction only increases
the file size by a few bytes, but it will slow down printing. The gamma factor
can be edited by hand after the file has been generated.
Gamma exponent
Use this field to specify the gamma factor to be applied to color components, either
precomputed in the output file, or postcomputed by the printer during printing. The
gamma factor is an exponential factor applied to each color component
independently (gray, red, green, blue). Its value must be greater than 0.0. A value of
1.0 leaves color unchanged, values between 0.0 and 1.0 darken the colors, and
values greater than 1.0 lighten (desaturate) the colors. The default value is 1.8
64
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Numerical Precision
Float Precision
Use this field to specify the floating point precision used to write real values to
the output file. The values include spatial coordinates and transformations, but
not colors. The value must be in the range 1 to 8. The default value is 4
Color Precision
Use this field to specify the floating point precision used to write color values to
the output file. The color values can be gray, red, green or blue. The value
must be in the range 1 to 8.The default value is 2
Alpha Threshold
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
65
AUTODYN User Manual
Pull-down Menu - File - Export VRML
This window lets you output the current plot to a VRML file.
VRML file
Enter the name of the VRML file in this field (use the Browse button to navigate to a
directory/file if you wish).
Protocol
Select the VRML protocol you want to use to write the output file.
VRML1
A clear text ASCII encoding of the VRML 1.0c standard (29 January 1996).
VRML2
66
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
A clear text UTF8 encoding of the VRML 2.0 standard, ISO/IEC CD 14772 (4
August 1996).
Float Precision
Use this field to specify the floating point precision when real values are written to
the output file. The values include spatial coordinates, normal vectors, texture
coordinates, material coefficients, and transformations, but not colors. The value
must be in the range 1 to 8. The default value is 4.
Color Precision
Use this field to specify the floating point precision when real values are written to
the output file. The values include diffuse material colors, emissive material colors,
and light colors. The value must be in the range 1 to 8. The default value is 2.
Indent format
Check this box if you want the file to be written with indented nesting of VRML
nodes. Indentation improves legibility, but increases the size of the output file.
Suppress Normals
Check this box if you do not want normals to be written to the VRML.
Dynamic
Check this box if you want a new VRML file to be output each time the input view is
rendered. Otherwise, you must explicitly request a new file by pressing the Write
VRML button.
Write VRML
When the dynamic switch is FALSE, this one-shot parameter triggers the generation
of a VRML output file. When the dynamic switch is TRUE, the user interface for this
parameter is removed.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
67
AUTODYN User Manual
Import
Pull-down Menu - Import
This pull-down menu lets you import grid data from other programs.
from TrueGrid (.zon)
Lets you import block zoning data from TrueGrid.
from ICEM (.geo)
Lets you import block zoning data from ICEM-CFD.
from LS-DYNA (.k)
Lets you import .k files from LS-DYNA.
from MSC.NASTRAN bdf (.dat)
Lets you import .bdf files from Nastran.
Convert IJK to Unstructured
Lets you convert existing IJK structured Parts to Unstructured Parts.
68
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
69
AUTODYN User Manual
Pull-down Menu - Import - TrueGrid
This window lets you import grid data from TrueGrid.
Navigate to the TrueGrid zoning file you want to import (.zon) and press
to open the following window.
Blocks
The TrueGrid zoning file contains one or more blocks of nodes (imported as Parts).
These are displayed in the scrolling box at the top of the window.
If Import selected parts is checked, you can select one or more blocks.
Import all Parts
70
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Check this option if you want to import all the blocks as Parts.
Import selected Parts
Check this option if you want to import selected blocks as Parts. Select the blocks
you want to import in the top box.
Select solver type
Select the solver type you want to assign to the imported Parts.
Press
to import the Parts.
Parts are imported with their block name. You can change these block names later in
the Parts panel.
TrueGrid zoning file format
There are two formats of TrueGrid zoning files supported by AUTODYN - implicit and
explicit. The two formats are illustrated below by an example which generates a
single cell cubic part (IMAX=2, JMAX=2, KMAX=2) called SUB1 with corners
(0.0,0.0,0.0) and (1.0,1.0,1,0) and a four cell cuboid part (IMAX=2, JMAX=2,
KMAX=3) called SUB2 with corners (2.0,2.0,2.0) and (3.0,3.0,4.0).
The implicit form of this data would be as follows:
IMPLICIT
SUB1
121212
0.0 0.0 0.0
0.0 0.0 1.0
0.0 1.0 0.0
0.0 1.0 1.0
1.0 0.0 0.0
1.0 0.0 1.0
1.0 1.0 0.0
1.0 1.0 1.0
SUB2
121213
2.0 2.0 2.0
2.0 2.0 3.0
2.0 2.0 4.0
2.0 3.0 3.0
2.0 3.0 4.0
3.0 2.0 2.0
Indicates implicit input is to follow
Name of the part for which data follows
The (I,J,K) range for the data I=1, 2, J=1,2, K=1,2
(x,y,z) coordinates for node with index (1,1,1)
(x,y,z) coordinates for node with index (1,1,2)
(x,y,z) coordinates for node with index (1,2,1)
(x,y,z) coordinates for node with index (1,2,2)
(x,y,z) coordinates for node with index (2,1,1)
(x,y,z) coordinates for node with index (2,1,2)
(x,y,z) coordinates for node with index (2,2,1)
(x,y,z) coordinates for node with index (2,2,2)
Name of the part for which data follows
The (I, J, K) range for the data I=J, 2, J=1, 2,
K=1, 3
(x,y,z) coordinates for node with index (1,1,1)
(x,y,z) coordinates for node with index (1,1,2)
(x,y,z) coordinates for node with index (1,1,3)
(x,y,z) coordinates for node with index (1,2,1)
(x,y,z) coordinates for node with index (1.2,2)
(x,y,z) coordinates for node with index (2,1,1)
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
71
AUTODYN User Manual
3.0 2.0 3.0
3.0 2.0 4.0
3.0 3.0 2.0
3.0 3.0 3.0
3.0 3.0 4.0
END
(x,y,z) coordinates for node with index (2,1,2)
(x,y,z) coordinates for node with index (2,1,3)
(x,y,z) coordinates for node with index (2,2,1)
(x,y,z) coordinates for node with index (2.2,2)
(x,y,z) coordinates for node with index (2,2,3)
The explicit form of this data would be as follows:
EXPLICIT
SUB1
1 1 1 0.0 0.0 0.0
1 1 2 0.0 0.0 1.0
1 2 1 0.0 1.0 0.0
1 2 2 0.0 1.0 1.0
2 1 1 1.0 0.0 0.0
2 1 2 1.0 0.0 1.0
2 2 1 1.0 1.0 0.0
2 2 2 1.0 1.0 1.0
SUB2
1 1 1 2.0 2.0 2.0
1 1 2 2.0 2.0 3.0
1 1 3 2.0 2.0 4.0
1 2 1 2.0 3.0 2.0
1 2 2 2.0 3.0 3.0
1 2 3 2.0 3.0 4.0
2 1 1 3.0 2.0 2.0
2 1 2 3.0 2.0 3.0
2 1 3 3.0 2.0 4.0
2 2 1 3.0 3.0 2.0
2 2 2 3.0 3.0 3.0
2 2 3 3.0 3.0 4.0
STOP
Indicates explicit input is to follow
Name of the part for which data follows
(x,y,z) coordinates for (1,1,1)
(x,y,z) coordinates for (1,1,2)
(x,y,z) coordinates for (1,2,1)
(x,y,z) coordinates for (1,2,2)
(x,y,z) coordinates for (2,1,1)
(x,y,z) coordinates for (2,1,2)
(x,y,z) coordinates for (2,2,1)
(x,y,z) coordinates for (2,2,2)
Name of the part for which data follows
(x,y,z) coordinates for (1,1,1)
(x,y,z) coordinates for (1,1,2)
(x,y,z) coordinates for (1,1,3)
(x,y,z) coordinates for (1,2,1)
(x,y,z) coordinates for (1.2,2)
(x,y,z) coordinates for (1,2,3)
(x,y,z) coordinates for (2.1,1)
(x,y,z) coordinates for (2,1,2)
(x,y,z) coordinates for (2,1,3)
(x,y,z) coordinates for (2,2,1)
(x,y,z) coordinates for (2.2,2)
(x,y,z) coordinates for (2,2,3)
Indicates end of all data
With the explicit format, it is not necessary to define coordinates for a complete block
of nodes in index space, and the order in which nodes are defined is unimportant.
When this option is used for a specific block of nodes in index space, the
"indent.zon" file is scanned and only those nodes defined in this file and within the
specified part and block to be initialized will be assigned coordinate values. Thus,
standard zoning options could be used to define the bulk of the grid and the "User"
option called to redefine the coordinates of a few isolated nodes.
Before reading in an explicit zoning file, the parts must already be created. The file
can then be read in using the Import button on the Parts Zoning panel.
72
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
The above example is for 3D. For 2D models the format is the same except of
course there is no K index or Z coordinates.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
73
AUTODYN User Manual
Pull-down Menu - Import - ICEM
This window lets you import grid data from ICEM-CFD.
Navigate to the ICEM-CFD zoning file you want to import (.geo) and press
to open the following window.
Domains
The ICEM-CFD zoning file contains one or more domains of nodes (imported as
Parts). These are displayed in the scrolling box at the top of the window.
If Import selected parts is checked, you can select one or more domains.
Import all Parts
74
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Check this option if you want to import all the domains as Parts.
Import selected Parts
Check this option if you want to import selected domains as Parts. Select the
domains you want to import in the top box.
Select solver type
Select the solver type you want to assign to the imported Parts.
Press
to import the Parts.
Parts are imported with their domain name. You can change these domain names
later in the Parts panel..
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
75
AUTODYN User Manual
Pull-down Menu - Import - LS-DYNA
Import Options
After browsing for an LS-DYNA keyword file, select import options in this dialog.
Retain LS-DYNA part definitions
Select this option to name the important parts from definitions within the LS-DYNA
file. Otherwise, generic names are automatically generated for the parts.
Merge duplicate materials
Select this option to merge duplicate materials
Check Shell orientation
Select this option to check for inconsistent or non-manifold shell meshes. If the
mesh is inconsistent and manifold, you should re-orient the mesh to have consistent
normals.
LS-DYNA Keyword File Format
Both formatted and free formatted (comma delimited) LS-DYNA keyword files can be
imported into AUTODYN. The standard used is based on version 970 of LS-DYNA.
The primary use of the LS-DYNA reader is to allow you to define a mesh to be used
with the unstructured solvers. In addition, other information regarding material
definitions, boundary conditions and initial conditions can be imported and stored in
AUTODYN.
76
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
An overview of the information, which can be imported into AUTODYN from an LSDYNA keyword file is given below.
Mesh
The mesh, represented as nodal positions and element connectivity, is read into
AUTODYN and sorted to produce Parts and Components. A Part is a collection of
connected elements of the same classification e.g. volume elements, shell elements
and beam elements. A Component is a collection of all connected elements
regardless of their topology. By default, the defined Parts in AUTODYN will not
necessarily be equivalent to those defined in the LS-DYNA keyword file.
An option to retain the Part definitions in the LS-DYNA file is also available.
Materials
Each element defined in the keyword file will have an associated material definition.
Corresponding materials will be automatically generated during the import of the
keyword file into AUTODYN. In general (except for the materials identified below),
the actual material parameters will not be read into AUTODYN and you should
ensure that all materials are properly defined after the import.
At present, a subset of the material definitions and parameters are automatically
read into AUTODYN. These include materials of type rigid, elastic, piecewise linear
plasticity and spring elastic material models.
Initial and Boundary Conditions
Fixed and prescribed boundary conditions are imported from the LS-DYNA keyword
file into AUTODYN. These are converted into the equivalent AUTODYN boundary
conditions including parameters, where possible.
Initial velocities defined on nodes and sets of nodes in the keyword file are read into
AUTODYN and converted into Initial Conditions. The initial condition is also
automatically applied to the identified nodes.
Shell and Beam Sections
Shell sections defined in the keyword file are automatically transformed into
AUTODYN initial conditions. The local direction for layered shells is not currently
translated.
Beam cross-sections and directions are read from the keyword file and these and the
relevant data are converted to be compatible with beam types used in AUTODYN.
Keyword Compatibility
The current capabilities of the AUTODYN import capability for LS-DYNA (.k) keyword
files is summarized below:
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
77
AUTODYN User Manual
Keyword
*BOUNDARY_SPC_NODE
*BOUNDARY_SPC_SET
*DEFINE_CURVE
*ELEMENT_SOLID
*ELEMENT_SHELL
*ELEMENT_BEAM
*INITIAL_VELOCITY
*INITIAL_VELOCITY_NODE
*INITIAL_VELOCITY
_GENERATION
*MAT_PIECEWISE_LINEAR
_PLASTICITY
*MAT_ELASTIC
*MAT_RIGID
*MAT_SPRING_ELASTIC
*NODE
*PART
*SECTION_BEAM
*SECTION_SHELL
*SET_NODE_LIST
*SET_PART_LIST
*SET_SHELL_LIST
*SET_BEAM
*SET_DESCRETE
*SET_SOLID
*SET_TSHELL
*SET_NODE_LIST_GENERATE
*SET_PART_LIST_GENERATE
*SET_SHELL_LIST_GENERATE
*SET_BEAM_GENERATE
*SET_DISCRETE_GENERATE
*SET_SOLID_GENERATE
78
Compatibility
Translational velocities only.
DORFX, DORFY, DORFZ not
recognized
Translational velocities only.
DORFX, DORFY, DORFZ not
recognized
Full
Full
Full
Full
BOXID and IRIGID are not
recognized
Translational velocities only.
VXR, VYR and VZR are not
recognized.
Translational velocities only.
OMEGA, XC, YC, ZC, NX, NY,
NZ and PHASE not recognized.
Full
Full
Full
Full
Full
Full
Beam types 1-5 supported.
QR/IRID, SCOOR, NSM,
NSLOC, NTLOC and IRR are not
recognized.
Shell thickness at first node is
read in and set a shell thickness
in initial condition.
Full
Full
Full
Full
Full
Full
Full
Full
Full
Full
Full
Full
Full
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
*SET_TSHELL_GENERATE
Full
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
79
AUTODYN User Manual
Pull-down Menu - Import - Nastran
Import Options
After browsing a NASTRAN input file, select import options in this dialog.
Convert Properties to AUTODYN parts
Select this option to name the imported parts from definitions within the NASTRAN
file. Otherwise, generic names are automatically generated for the parts.
Merge duplicate materials
Select this option to merge duplicate materials.
Check shell orientation is consistent
Select this option to check for inconsistent or non-manifold shell meshes. If the
mesh is inconsistent and manifold, you should re-orient the mesh to have consistent
normals.
Input File Format
AUTODYN can import MSC.NASTRAN™ input files in both free and fixed format. In
free format, the entries can appear anywhere on the line and are separated by
commas. With fixed format, a field must be located in a set part of the line. The
fixed format field can be small (8 characters) or large (16 characters).
In addition to the MSC.NASTRAN™ bulk data input, AUTODYN can recognize the
expanded input data set for explicit transient dynamics, as given by MSC.DYTRAN™
version 4.7.
80
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
The primary use of the MSC.NASTRAN™ reader is to allow you to define a mesh to
be used with the unstructured solvers. In addition, other information regarding
material definitions, boundary conditions and initial conditions can be imported and
stored in AUTODYN.
An overview of the information, which can be imported into AUTODYN from an
MSC.NASTRAN™ bulk data file is given below.
Mesh
The mesh, represented as nodal positions and element connectivity, is read into
AUTODYN and sorted to produce Parts and Components. A part is a collection of
connected elements of the same classification e.g. volume elements, shell elements
and beam elements. A component is a collection of all connected elements
regardless of their topology.
Materials
Each element, imported from the bulk data file will have the material name as
defined on the property field for the element (PSOLID, PSHELL). Corresponding
materials will be automatically generated during the import of the keyword file into
AUTODYN. In general (except for the materials identified below), the actual material
parameters will not be read into AUTODYN and you should ensure that all materials
are properly defined after the import.
At present, a subset of the material definitions and parameters are automatically
read into AUTODYN. These include materials of type rigid, elastic, piecewise linear
plasticity and spring elastic material models.
Initial and Boundary Conditions
Every element property is translated into an Initial Condition in AUTODYN and
allocated to the appropriate elements.
Fixed and prescribed boundary conditions are imported from the bulk data file into
AUTODYN. These are converted into the equivalent AUTODYN boundary
conditions including parameters, where possible.
Initial velocities defined on nodes and sets of nodes in the bulk data file are read into
AUTODYN and converted into Initial Conditions. The initial condition is also
automatically applied to the identified nodes.
Bulk Data Compatibility
The current capabilities of the AUTODYN import capability for MSC.NASTRAN™
bulk data files is summarized below:
Keyword
BEGIN BULKDATA
CBAR
Compatibility
Full
Only grid numbers to define local x-
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
81
AUTODYN User Manual
CBEAM
CHEXA
CPENTA
CQUAD4
CTETRA
CTRIA3
JOIN
FORCE
GRID
PBAR
PBEAM
PBEAM1
PCOMP
PLOAD
PSHELL
PSHELL1
PSOLID
SET1
SPC
SPC1
TABLED1
TLOAD1
y plane
Only grid numbers to define local xy plane
Full
Full
No material direction
Full
No material direction
Full
Full
No coordinate system; no SPC
Full
Only constant cross-section
Only as PBEAM
Full
Full
No thickness
Up to field 7
Full
Full 1
Full
No ranges
Full
Only FORCE
Any keyword not mentioned in the table above will be ignored.
82
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Pull Down Menus - Import - Convert IJK to Unstructured
Existing structured (IJK) Parts using the Lagrange, Shell and Beam solvers can be
converted into Unstructured Parts via the Import, Convert IJK Part to Unstructured
option. The mesh, material, boundary conditions and initial conditions will be
transferred to the new Part.
This feature lets you convert existing models to the new solvers to take advantage of
the reduced memory requirements and increased speed of solution.
During the conversion, you will be presented with the options
Delete converted IJK regions
This option deletes the structured IJK Parts that have been converted to
unstructured solvers after the conversion process.
Merge connected IJK Parts into single Unstructured Part
Complex geometries defined using the structured (IJK) solvers tend to be made up
of a large number of relatively simple Parts that are joined together (for example a
mesh imported from ICEM-CFD .geo file). By default, the conversion process will
merge connected IJK Parts into a single Part. This simplifies the model and can also
improve performance because there will be fewer Joins in the model. For some
applications, you may not wish to merge the IJK Parts in this way. De-selecting this
option will result in no change in the Parts defined in the model.
Merge joined IJK nodes into single unstructured node
By default, all joined nodes are merged into a single unstructured node during the
conversion process. In some cases, for example if you have pinned joins, you may
not wish to do this.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
83
AUTODYN User Manual
Setup
Pull-down Menu - Setup
This pull-down menu lets you set up models. Most of these options are accessible
through the Navigation Bar.
Description
Lets you modify the description of your model.
Symmetry
Lets you change the symmetry settings for your problem.
Material
Lets you define and modify materials.
Initial Conditions
Lets you define and modify Initial Condition Sets
.
Boundary
Lets you define and modify Boundary Conditions.
Parts
84
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Lets you define and modify Parts
Components
Lets you define and modify Components
Groups
Lets you define and modify Groups
Joins
Lets you define joins.
Interactions
Lets you define interactions
Detonation
Lets you define detonation points.
Parallel
Lets you set up your parallel processing environment and prepare your model for
parallel processing.
Controls
Lets you set various controls for your model such as run limits, timestep controls,
damping constants, cutoffs and gravitational forces.
Output
Lets you select the output you want from your model.
User Variables
Lets you initialize any grid variables you want to use in your user subroutines.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
85
AUTODYN User Manual
Pull-down Menu - Setup - Description
This window lets you modify the description of your model.
Ident
This field lets you change the ident for your model.
The ident you choose is used to identify all the files created for your model.
e.g. If your Ident is MyImpactProblem, then the cycles zero Save file for the
problem will be named MyImpactProblem_0.ad.
Heading
This field lets you change the heading for your model.
Headings appear in plots and other output for your model.
Description
This field lets you enter or change a detailed description of your model.
Units
86
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
This field lets you change the units of length, mass and time you want to use for your
model.
The default units (mm,mg,ms) will give good results, with small rounding errors, for
most models.
Changing the units here WILL NOT result in any scaling of data previously entered.
It only effects the units displayed in output and data conversions performed when
reading / writing data to / from material libraries.
Current Cycle
This field displays the current cycle number.
Current Time
This field lets you change the current time.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
87
AUTODYN User Manual
Pull-down Menu - Setup - Symmetry
AUTODYN started up in Workbench
AUTODYN started up outside from ANSYS Workbench
2D Window
3D Window
This window lets you change the symmetry used in you model.
88
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Execution
Pull-down Menu - Execution
This pull-down menu lets you execute your calculation.
Run Interactively
Lets you execute you problem interactively. This is the same as pressing
on the Navigation bar.
Batch Runner
Lets you run one or more of your models in batch mode (i.e. without graphics).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
89
AUTODYN User Manual
Pull-down Menu - Execute - Batch Runner
This Window lets you set up and run single or multiple Jobs (calculations) in batch
mode (without graphics).
Job List
This box lists all current jobs ( Save files to be loaded and executed) and shows their
status.
Add Job
Press this button to add a job to the list. A window opens to let you browse to the
Save file you want to load and execute.
Delete Selected Job(s)
Select one or more Jobs in the Job List and press this button to delete them from the
Job List.
Load Job(s) from File
90
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Press this button to load jobs saved in a file (.bat) into the Job List.
Save Job List to File
Press this button to save all the jobs in the current Job List to a file (.bat).
Run
Press this button to run the jobs in your Job List.
Jobs run sequentially in the Job List.
While running, the window displays information on which jobs have completed, which
job is currently executing and which are waiting in line to execute. The status of the
executing job is also displayed at the foot of the window.
Stop
Press this button to stop running jobs in the Job List.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
91
AUTODYN User Manual
View
Pull-down Menu - View
This pull-down menu lets you customize your view (what you see in the View panel).
Most of these options are accessible through the Navigation Bar.
Plots
Lets you set up what you want to see in the View panel.
Plot Settings
Lets you change settings for the various plot types that control how you view your
model.
You can change settings for the following plot types:
Display
Grid
Materials
Contour
92
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Velocity Vector
Gauge Point
Boundary
Joins
Axes
Detonation
History Graphs
Lets you view histories of Gauge points and Material, Part and Energy summaries.
Slideshow
Lets you create and organize slideshows (animations)
Performance Profiler
Brings up a performance profiler that lets you monitor your calculation.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
93
AUTODYN User Manual
Pull-down Menu - View - Slideshow - Setup
This window lets you set parameters for creating a slideshow.
Directory
Press
next to the Directory box to browse to the directory in which you want to
save your slideshow.
Slideshow prefix
Enter a slideshow prefix in this field or check Use current model name to use the
current Ident as the slideshow prefix.
This prefix is used for all image files created for the slideshow.
Next slide number
Enter a number for the next slide to be created or check Automatic numbering if
you want AUTODYN to automatically assign numbers to slides.
Image type
94
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Use this pull-down menu to select the image type you want to use to create your
slides (gif, jpeg, tiff or gfa).
Use OpenGL
Check this box if you want to use OpenGL to create your slides. This can
significantly improve the plotting of SPH objects.
Fix Slide size
Select this toggle to fix the size of slides created. Specify the width and height of the
image in pixels. If the toggle is not selected, the slides created are to be the size of
the graphics window.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
95
AUTODYN User Manual
Pull-down Menu - View - Performance Profiler
This window provides a Performance Profiler that lets you visually monitor the load
balancing performance of parallel simulations.
To take full advantage of this option, you must create an empty file profile.cfg in the
directory where the AUTODYN model resides.
If you do this, the following type of output will be displayed in the scrolling box at the
foot of the window:
Cycle/Time
Cycle/Time
Cycle/Time
Cycle/Time
Cycle/Time
Cycle/Time
Cycle/Time
Cycle/Time
Cycle/Time
Cycle/Time
Cycle/Time
Cycle/Time
Cycle/Time
Cycle/Time
Cycle/Time
96
1
2
3
4
5
6
7
8
9
10
11
12
13
14
15
/
/
/
/
/
/
/
/
/
/
/
/
/
/
/
1.637809225157053E-4 clock time (msec) 32856 (update)
3.439399411878227E-4 clock time (msec) 17030
5.421148660224775E-4 clock time (msec) 17056
7.601072880654561E-4 clock time (msec) 17029
9.998989575100770E-4 clock time (msec) 17054
1.263669799616239E-3 clock time (msec) 17016
1.553817732221804E-3 clock time (msec) 17081
1.872980465005591E-3 clock time (msec) 16994
2.224059478677190E-3 clock time (msec) 17116
2.610246402086324E-3 clock time (msec) 17024
3.035052027043786E-3 clock time (msec) 17075
3.502338224625149E-3 clock time (msec) 17070
4.016353053105620E-3 clock time (msec) 17053
4.581769376689206E-3 clock time (msec) 17019
5.203727346111727E-3 clock time (msec) 17070
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Cycle/Time
Cycle/Time
Cycle/Time
Cycle/Time
Cycle/Time
16
17
18
19
20
/
/
/
/
/
5.887881127305133E-3 clock time (msec) 17011
6.640450302929377E-3 clock time (msec) 17085
7.468276414058693E-3 clock time (msec) 34853 (update)
8.378885156037852E-3 clock time (msec) 17017
9.380554793925532E-3 clock time (msec) 17098
Each line gives the cycle number, the cycle time, and the wall clock time that the
calculation used to compute the cycle (in milliseconds). If the line ends with
"(update)", this indicates that work unit information for the interaction logic was
updated on that cycle. Such cycles usually take longer to compute.
The profiler also shows you visually how well balanced your calculation is. In the
example shown above, Balance is a measure of the relative CPU time spent on
each task for each cycle in the simulation. So a balance of 1.0 for each task is the
ideal / most efficient goal. A balance of less than 1.0 means that a task is under
utilized (does not have enough work to do). A balance of greater than 1.0 means that
a task is over utilized (has too much work to do).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
97
AUTODYN User Manual
Options
Pull-down Menu - Options
This pull-down menu lets you set various GUI options.
Interactivity
Lets you set how the mouse and keyboard is used for the Tool Bar operations that
manipulate images in the view panel.
Clipping Planes
Lets you set clipping planes for your plot.
Default Settings
Lets you change the default settings used to start up AUTODYN.
Pause License
Lets you temporarily pause the license and free it for another AUTODYN instance.
Create User-Subroutine Project
Lets you install the AUTODYN project to create your own version of AUTODYN by
using user-subroutines.
98
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Pull-down Menu - Options - Interactivity
This window lets you change how the mouse and keyboard is used for the Tool Bar
operations that manipulate images in the view panel.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
99
AUTODYN User Manual
Pull-down Menu - Options - Clipping Planes
This window lets you set clipping planes for your plot.
If you zoom in close to, or into a grid, the image will not look good if you include
everything in your view. The default values for the clipping planes usually improve
such plots considerably, but there may be times when you want to use other values.
Front
Use this field to set the distance of the front clipping plane from the viewpoint. Any
part of the grid nearer to the viewpoint than this plane will not be plotted.
Back
Use this field to set the distance of the back clipping plane from the viewpoint. Any
part of the grid further away from the viewpoint than this plane will not be plotted.
100
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Pull-down Menu - Options - Default Settings
This dialog lets you to define the default settings for the AUTODYN GUI. These
settings are stored in an ASCII file "autodyn.ini" and are used to initialize various
aspects of the GUI and rendering options, each time you start AUTODYN.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
101
AUTODYN User Manual
Pull-down Menu - Options - Pause License
If you are working with a project in Workbench which contains an AUTODYN system
linked to an ANSYS Explicit Dynamics system you will not be able to open and work
in both applications simultaneously in shared licensing mode or when the license
server only has one solver license available. For example, if you want to generate a
new mesh in the meshing application then you will need to close the AUTODYN
application to release the license for the meshing application to use.
As an alternative the user can leave the AUTODYN application open, but release the
license for another application to use. While the license is released, the AUTODYN
user interface will be locked.
After selection of the Pause option the license is released, and the AUTODYN user
interface will be locked. To continue the AUTODYN application the user can select
Retry to try to obtain the license again. The Close App option will exit the AUTODYN
application without saving any data.
For more information on licensing please review the ANSYS, Inc. Licensing Guide.
102
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Pull-down Menu - Options - Create User-Subroutine Project
When AUTODYN version 12 is run for the first time by the logged on user,
AUTODYN will perform a few additional initialization steps to create user specific
settings.
In previous version you also would have been prompted for a location for usersubroutine files which would have been created after the initial step. This step is no
longer performed and the generation of the user-subroutine project is now available
as a user action from within AUTODYN from the Options Menu instead.
After selection of the location for the user-subroutines AUTODYN will install the user
subroutine project in a sub-directory with name AUTODYN user_subroutines.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
103
AUTODYN User Manual
Pull-down Menu - Help
This pull-down menu provides general help for AUTODYN (Contents), and provides
information about the current version (About).
104
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Plots
Plots
This panel lets you set up what you want to see in the View panel.
Cycle
This pull-down menu lets you choose which cycle you want to view for the current
model (Ident).
Select part(s)
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
105
AUTODYN User Manual
This box lists the Parts in the model. Operations performed in the Plots panel will
only be applied to the Part(s) you select
Fill type
These options let you select the basic fill type you want to view. Select only one fill
type.
Additional components
This option let you view additional components in your plot. Check the boxes
alongside the additional components you want to include (any number can be
selected).
Contour Variable
This button is only active if a Contour Fill type is selected. Press this button to
change the variable to be contoured.
View Range
This button is only active if a single Part is selected. Press this button to limit the IJK
range that is plotted for the Part.
Mirror
Check a box to mirror the image in the associated axis.
All Fill types and Additional components have default Settings. You can quickly
access and change these settings by pressing the
button to the right of these
options. Doing so will bring up a dialog window containing the settings available for
the associated option.
The Settings button on the Navigation bar gives you access to all these settings.
106
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Plots - Select Contour Variable
This dialog lets you select the variable you want to contour.
Select the variable from the left hand list.
For multi-material variables (those at the top of the left hand list), you must also
select a material (or "All") from the right hand list.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
107
AUTODYN User Manual
Plots - View range and slices (Structured)
This dialog window lets you set the view range and slices to be used to display a
structured part of your model.
Part:
The part that you are defining a view range and slices for is shown here, together
with its index range.
View Range
This box lets you define the I, J and K range you want to see for this Part.
Slices
Instead of a solid view of your Part, you can request to see only slices (planes)
through the part for any of the three indices.
Check the box next to an index for which you wish to create slices and define the
planes for which you want to see these slices.
If no boxes are checked, a solid plot using the view range will be shown.
Reset
This button resets the View Range and Slices to their default values.
Apply
Pressing this button applies the current settings.
108
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
View range and slices (SPH/Unstructured)
Limit XYZ plot range?
Select this option to truncate plotting of unstructured and SPH parts. Any
unstructured elements or SPH nodes that fall outside the view range specified will be
eliminated from the plot.
View Range
Specify the maximum and minimum X, Y and Z coordinates to be plotted for
unstructured and SPH parts. These limits are not set on a per part basis, and so
setting limits will truncate the plotting for all unstructured and SPH parts in the model.
Reset range for new model?
If this option is selected, when a new model is opened, the view range will be reset
to show the full model. If this option is not selected, the view range you have
selected will be maintained.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
109
AUTODYN User Manual
Settings
Settings
Selecting Settings on the Navigation Bar displays the Plot Type Settings panel.
This panel lets you change settings for the various plot types that control how you
view your model.
At the top of this panel, a pull-down menu lets you to select the plot type whose
settings you wish to change :
You can change settings for the following plot types:
Display
Grid
Materials
Contour
Velocity Vector
Gauge Point
Boundary
Joins
Axes
Detonation
These settings can also be changed by pressing
panel.
next to the option in the Plots
The following additional settings can also be changed by pressing
option under Additional Components in the Plots panel.
Eroded Nodes
Unused Regions
Polygons (2D only)
Beam sections
Shell thickness
110
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
next to the
AUTODYN User Manual
Legend
Profile
Mat. direction
Marker
Shell normals
Node/Element
Part Highlight
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
111
AUTODYN User Manual
Settings - Display
This panel lets you set the following general options :
Deformation Magnification :
This option lets you view magnified grid deformations. Input the magnification you
want to use (1.0 gives no magnification).
Surface rendering of large 3D models :
3D models using hexahedral elements (e.g. Lagrange or Euler) are usually rendered
using all the elements. Check this box to render models using only external faces.
This makes the process much quicker. This option cannot be used for all plots (e.g.
plots with opacity applied).
Standard shell layer to plot :
This option lets you set the layer that is plotted for standard shells (e.g. in contour
plots, material status plots etc.)
Composite shell layer to plot :
This option lets you set the layer that is plotted for composite shells (e.g. in contour
plots, material status plots etc.)
112
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Background
This option lets you set the background color for the view panel.
Graded Shading
This option lets you control the color, including color grading, for the background of
the View panel.
You may select a color to be used for each of the four corners of the display by
pressing the buttons
The selected (Default) colors shown here will produce the following background
SPH Particles
Controls for the display of SPH particles are only shown when the model contains
SPH parts. In this section, the controls for displaying the points with anti-aliasing
and illuminated points are accessible. In addition, control of particle display size and
amount of fade for outliers can be set.
The figures below compare plots with and without the illuminated points option
active.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
113
AUTODYN User Manual
SPH representation without
Illuminated Points
SPH representation with
Illuminated Points
The fade outliers slider gives you the ability to fade in and out of view the sph
particles which exist outside of the range set in the contour panel (when using the
truncate facility), this facility is only available when illuminated points are displayed.
Advanced Image Shading and Lighting Options
As set of advanced shading and lighting options are available
Using a combination of the above options, metallic looking surfaces can be
rendered, for example
Shading type
The shading type can now be selected as either flat or Gouraud. For flat shading
every point on a face is given the same intensity. For Gouraud shading, the mesh is
114
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
shaded so as to give the appearance of curved surfaces. The intensity for each
point is interpolated from the normal of the face vertices.
Flat shading
Gouraud shading
Lighting Control
The advanced lighting control lets you specify up to 4 different light sources and also
to control the direction and form of each light source.
The following options are available:
Current light source
This allows you to select the current light source to be interactively transformed, after
selecting the "Transform Light" button on the toolbar.
Light source toggles
You can choose the number of light sources required (up to a maximum of 4).
Light source type
You can select between directional, bi-directional, spot or point light sources.
Examples of these are shown in the figure below.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
115
AUTODYN User Manual
Directional Light Source
Bi-Directional Light Source
Spot Light Source
Point Light Source
Show light sources
The direction and position of the light sources is shown on screen by white arrows
(switch the background color to black). Examples are shown in the figure below
(from left to right) for bi-directional light source, spot light source, point light source
and directional light.
Ambient, Diffusive and Specular Light Coefficients
The ambient light coefficient controls the amount of background lighting. Ambient
light is non-directional, affecting all parts of all surfaces equally.
116
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
No lighting
Ambient lighting only
Diffuse light reflectance controls the proportion of the available non-ambient light that
the object reflects equally in all directions. Non-ambient light emanates from the
directional and point light sources.
Specular highlights of a particular color and brightness are created when the
direction of incoming light (from a directional or point light source) is "sufficiently
close" to the viewing direction. The specular reflection coefficient determines the
brightness of such highlights.
Diffusive light only
Specular light only
The specular exponent determines what "sufficiently close" means. The greater the
sharpness, the smaller (more focused) the size of the specular highlight.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
117
AUTODYN User Manual
High specular exponent
118
Low specular exponent
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Settings - Grid
This panel lets you set the following options for grid plots (some options are not
present for 2D models) :
Grid lines :
These options let you view grids with or without grid lines (or with just the outline of
the grids displayed).
Colored grid lines :
Check this box to display grid lines in color (otherwise they are displayed in black).
Hidden line removal + allow examine :
Check this box to view grids with hidden line removal. The Examine feature is only
available if hidden line removal is chosen
Opacity :
This slider lets you set the opacity for your view. It is only functional if hidden line
removal is selected. An opacity of 1.0 means you cannot see inside a grid. An
opacity of 0.0 is equivalent to turning hidden line removal off (i.e. you can see
everything inside the grid).
Enable zoning plot :
By default you will only see the parts of a grid that are filled with material. Check this
box to see all zoning, including unused elements.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
119
AUTODYN User Manual
Settings - Legend
This window lets you set the plot legends you want to display in the View panel.
Color triad
Check this box to show a colored triad in the lower left corner of the View panel
(otherwise the triad is monochrome).
The axes are color-coded as follows :
Red
X
Green Y
Blue
Z
Filename visible
Check this box if you want the filename (ident) of you model to be visible in the
bottom left corner of the View panel.
Heading visible
Check this box if you want the heading of your model to be visible in the bottom right
corner of the View panel.
User heading
Check this box if you want to override the heading of you model with an alternative
(user) heading. Enter the user heading in the field provided.
Font size
120
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Enter the size of the font used in the graphics window for the legend, scale and user
heading.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
121
AUTODYN User Manual
Settings - Node/Element Numbers
This window lets you change settings for plotting node/element numbers
Plot type
Choose to plot numbers for nodes or elements.
Node/Element limit
The maximum number of node or element numbers to be plotted. For larger models
this number may be increased which can result in a slower graphic refresh.
Plot labels for group
Select this option to plot node or element numbers for a particular group. If this
option is not selected, node/element numbers are shown for all plotted parts.
Group list
If the "Plot labels for group"
Plot labels for SPH
Select this option to include SPH particles in the node or element plot.
122
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Materials
Settings - Materials
This panel lets you set the following options for material plots:
Grid lines :
These options let you view grids with or without grid lines (or with just the outline of
the grids displayed) and the color in which the grid lines or outline are displayed.
Pressing this icon lets you set colors for each material using the Modify Material
Color dialog window.
Smooth multi-materials
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
123
AUTODYN User Manual
Check this box to show smooth multi-material interfaces
Material visibility
Check the boxes for materials you want to be visible in the view.
Fragment plot
Check this box to view a fragment plot. Fragment plots only show elements that
contain material that has not failed.
Pressing the Output fragment analysis button causes fragment data to be output to
a file.
The fragment output post processing option is now available for all solvers, including
the unstructured solvers.
Simulation of fragmentation of a grenade modeled using unstructured tet elements
Cracked plot
Check this box to view a cracked material plot. A cracked material plot shows all
elements that contain material with damage above the specified Damage level.
Opacity
This slider lets you set the opacity for your view. An opacity of 1.0 means you cannot
see inside the grid. An opacity of 0.0 is equivalent to turning hidden line removal off
(i.e. you can see everything inside the grid).
124
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Settings - Materials - Modify Material Color
This dialog lets you modify a material color.
1) Select the material whose color you wish set from the list (top left).
2) Choose the dial mode you wish to use to set the color.
HSV - Hue, Saturation, Value
RGB - Red, Green, Blue
3) Use the three dials at the bottom of the window to set the color.
As you turn the dials, the top right window displays the color that will be used.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
125
AUTODYN User Manual
Contour
Settings - Contour
126
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
This panel lets you set the following options for contour plots (some options are not
present for 2D models:
Contour variable
Press this button to open the Select Contour Variable dialog window, allowing you
to choose the variable you want to contour.
Profile window
Check this box to open the Profile Plot dialog window, allowing you to compose and
display a profile plot.
Smoothing
Check this box if you want smoothed contour plots. All elements have a single
centered value for each variable. If you do not smooth a contour plot each element
will be color-coded for the value the variable has in that element. If you smooth a
contour plot, then the centered values are interpolated in space to provide smoothly
varying values.
Isosurface
Check this box to view a 3D isosurface plot of the contour variable. You are
prompted for the value to be used for the plot.
Min/Max Value
Check this box to open a window that displays the minimum and maximum values
for the contoured variable.
Grey scales
Check this box to view contour plots using grey scales instead of color.
Lines
Check this box to view contour plots with colored lines instead of colored fills.
Number of contours
This slider lets you select the number of contours you want to use for your plot.
Grid lines
These options let you view grids with or without grid lines (or with just the outline of
the grids displayed) and the color in which the gridlines or outline are displayed.
Contour scales
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
127
AUTODYN User Manual
Usually you should let the maximum and minimum values between which contours
are plotted be set automatically using the data in the model. However, you may
override these settings in the Contour scales box. For example, if a maximum value
is entered which is lower than the highest value present in the model, a red area will
appear corresponding to all values above the maximum that has been set. Selecting
Fix scales lets you fix the current maximum and minimum values. This is particularly
useful when you want to generate a slideshow from multiple cycles of a single
model. The red area may be removed by selecting Truncate.
Opacity :
This slider lets you set the opacity for your view. An opacity of 1.0 means you cannot
see inside the grid. An opacity of 0.0 is equivalent to turning hidden line removal off
(i.e. you can see everything inside the grid).
Slice Plane Plot
The "Slice Plane" feature is a visual tool to take a section through a model at an
arbitrary angle. Results values, as selected under the contour option, are contoured
on the selected slice through the model.
We recommend that you use the slice box feature in conjunction with the Opacity
feature of the Contour plot to obtain best results.
Example slice plane plot showing the damage inside a concrete target
128
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Settings - Contour - Profile Plot
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
129
AUTODYN User Manual
This dialog window lets you compose and display a profile plot of a chosen variable
along some defined line.
Define the Line along which the variable is profiled
Specify the end points for the line along which the variable is profiled.
You can do this by specifying the coordinates for the start point and end point of the
line (lower left)
Alternatively, in 2D, you can select this line interactively in the View Panel using the
mouse (hold shift and use the right mouse button to drag a line across your model).
Change Variable
Press this button to change the variable you want to profile.
Smoothing
Check this box if you want to see a smoothed profile plot.
Line Color
Use this pull-down menu to select the line color for your profile plot
Write textfile (uhs)
Press this button to write digital history data for the current plot to a text file. The text
file has an extension .uhs and is Microsoft Excel compatible.
Examine
Use the Left Mouse Button to select a point on the graph. The corresponding x and
y values are displayed in the Examine panel.
130
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Settings - Velocity vector
This panel lets you set the following options for velocity vector plots:
Vector Length Scale
This slider lets you set the scale factor of the arrows that are drawn for this plot type.
You can alternatively type in a scale factor in the box below the slider. You can also
fix this scale factor so that all plots use the same scale. The range for this factor is
calculated from the maximum velocity and the physical dimensions of your model.
Arrow Type
This option lets you choose the type of arrows that are plotted. Solid arrows take
longer to plot than line arrows (the default).
Vector scales
AUTODYN chooses vector scales automatically using the maximum and minimum
velocities in the model. You can override these scales and set your own minimum
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
131
AUTODYN User Manual
and maximum scale values in this box. You can also fix these scales for all plots
(useful when creating slideshows).
Surface vectors only
Check this box if you only want to plot vectors on material surfaces. This can speed
up plotting significantly, but is not always what you need, particularly if your plot uses
opacity.
Vector density
This option lets you reduce the number of velocity vectors plotted, which can speed
up plotting significantly. The option only applies to Lagrange and ALE parts. You
specify the reduction factor for each grid index (I,J and K).
132
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Settings - Gauge point
This panel lets you set the following options for gauge point plots:
Select gauge points
These options let you select all gauge points, all gauge points associated with a part
or individually by number. For the last two cases additional dialog prompts you for
the part names or gauge numbers as required.
Marker scale
Each gauge point is represented by a marker. This slider lets you set the marker
size.
Text labels
Check this box to label each marker with its corresponding gauge number.
Text size
This defines the text size used for the label
Label bounds
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
133
AUTODYN User Manual
Check this box to put a bounding box around each label.
Label offset
Check this box to set your own offset position for labels
Leading line
Check this box if you want to show lines joining each marker to its label
Radial offset
Check this box if you want to use radial label offsets instead of linear offsets
X / Y / Z offset
These sliders let you adjust the label offset distance in the X, Y and Z directions.
134
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Settings - Boundary
This panel lets you set the following options for viewing boundary conditions :
Boundary Condition
This pull-down menu lets you choose the boundary condition you want to view.
Marker scale
This slider lets you choose the size of the marker used to show where nodal
boundary conditions have been applied.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
135
AUTODYN User Manual
Settings - Joins
This panel lets you set the following options for viewing boundary conditions :
Marker scale
This slider lets you choose the size of the marker used to show joined nodes.
Joins to plot
These options let you choose the type of joins you wish to plot (pinned, rigid or all
joins)
136
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Settings - Axes
Axes are automatically chosen to fit the minimum / maximum range of your model.
This dialog lets you define your own axes.
Fix axes size
Check this box to define your own axes.
Axis Dimensions
Set the min / max range for each of your axes.
Reset
This button resets the min / max ranges to those automatically set from your model
dimensions.
Intervals
Set the number of intervals you want displayed on each of your axes.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
137
AUTODYN User Manual
with your own. It is possible for the user to fix the size of the axes in the axes
settings panel.
To reset the axes size to the default, use the Reset button. The number of intervals
on the axis can also be controlled.
Number of decimal places
Enter the number of decimal places to be displayed for the axes.
Label offset
Set the label offset to control the distance between the axes and the labels.
138
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Settings - Detonation
This panel lets you set the following options for viewing detonation points :
Marker scale
This slider lets you choose the size of the marker used to show detonation points.
Resolution
This slider lets you choose the marker resolution.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
139
AUTODYN User Manual
Settings - Eroded Nodes
This window lets you set the node size for plotting eroded nodes.
Enter an integer number. The higher the number, the larger the node.
140
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Settings - Unused Regions
This window lets you set options for the plotting of unused regions.
Gridlines
Select whether you want to plot the outline or grid for unused zones and whether the
outline/grid is drawn in black or white.
Plot contours
Check this box if you want the contour variable contoured on unused faces (for
contour plots). Otherwise the face is displayed in grey.
Opacity :
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
141
AUTODYN User Manual
This slider lets you set the opacity for unused regions. An opacity of 1.0 means you
cannot see inside the region. An opacity of 0.0 is equivalent to turning hidden line
removal off (i.e. you can see everything inside the region).
142
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Settings - Polygons
This window lets you turn on the plotting of polygons (used in 2D Euler-Lagrange
coupling).
Check the box to turn outline plotting on.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
143
AUTODYN User Manual
Settings - Beam Sections
This window lets you control the plotting of beams.
144
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Circular Beam Plot Settings
Select the number of facets to be plotted for each circular cross-section beam.
Spring Plot Settings
Select the Plot Springs toggle to enable the spring plot.
Scale
Select this option to normalize each plotted spring with the length of the spring
element.
Fixed Length
Select this option to display each plotted spring as a fixed size.
Length Scale Factor
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
145
AUTODYN User Manual
The Length Scale Factor is only used together with the scale option. If a length
scale factor of one is chosen, each spring will be displayed as the same length as
the element.
Fixed Length
If the fixed length option has been selected, specify the length of each plotted spring
in this field.
Radius to Length Ratio
Set the radius to length ratio of each plotted spring in this field.
Number of revolutions
Set the number of revolutions for each plotted spring in this field.
Resolution
Set the number of lines used to represent each plotted spring in this field.
Damper Plot Settings
Select the Plot Damper toggle to enable the damper plot.
146
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Scale
Select this option to normalize each plotted damper with the length of the damper
element.
Fixed Length
Select this option to display each plotted damper as a fixed size.
Length Scale Factor
The Length Scale Factor is only used together with the scale option. If a length
scale factor of one is chosen, each damper will be displayed as half the length as the
element.
Fixed Length
If the fixed length option has been selected, specify the length of each plotted
damper in this field.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
147
AUTODYN User Manual
Radius to Length Ratio
Set the radius to length ratio of each plotted damper in this field.
Resolution
Set the number of lines used to represent each plotted damper in this field.
148
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Settings - Shell Thickness
This window lets you select the thickness you want to use for rendering shells.
You can use either the true shell thickness or the artificial thickness that is used for
coupling shells to Euler.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
149
AUTODYN User Manual
Settings - Material Direction
This window lets you change settings for plotting material directions.
Material direction length scale
Use this slider to vary the length of the lines displaying the local axes.
Fix length scale
Check this box to fix the local axes length scale.
Line thickness
Use this slider to vary the thickness of the lines displaying the local axes.
Show Direction 1
150
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Check this box to display the local axis for direction 1.
Show Direction 2
Check this box to display the local axis for direction 2.
Show Direction 3
Check this box to display the local axis for direction 3
For large models containing mainly volume elements, you will get better results by
selecting the Settings, Display, Surface rendering option.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
151
AUTODYN User Manual
Settings - Marker
The Marker Plot lets you highlight a particular position, node or element of interest.
152
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Specify Marker Position
Choose to specify the marker position either by XYZ coordinates or by specifying a
part and I/J/K values for a node or element.
XYZ coordinates
Enter the coordinates of the marker location.
Node/Element/Face
Lets you highlight a particular node, element or face of an element.
Parts List
Select the part containing the node, element or face to be highlighted.
IJK
Select the I, J, and K values for the node, element or face of interest in case the part
selected is structured.
Node Number/Element Number/Face Number
Enter the node, element for face number of interest in case the part selected is
unstructured. Depending on the selection of User No. or Internal No. the node,
element or face number displayed is the original User Number or the AUTODYN
internal number.
Text labels
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
153
AUTODYN User Manual
Check this box to label each marker
Text size
This defines the text size used for the label
Label bounds
Check this box to put a bounding box around each label.
Label offset
Check this box to set your own offset position for labels.
Leading line
Check this box if you want to show lines joining each marker to its label.
Radial offset
Check this box if you want to use radial label offsets instead of linear offsets.
X / Y / Z offset
These sliders let you adjust the label offset distance in the X, Y and Z directions.
154
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Settings - Shell Normal
This window lets you change settings for plotting shell normals.
Local Axes length scale
Use this slide to vary the length of the arrows displaying the shell direction.
Fix length scale
Check this box to fix the shell normals length scale
Include Joins
Select this toggle to show an average normal for joined nodes. If this toggle is
unselected, a normal will be shown for each of the nodes joined.
Line thickness
Use this slider to vary the thickness of the lines displaying the shell normals.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
155
AUTODYN User Manual
Settings-Part Highlights
When this option is selected, Parts selected in the plots panel will be highlighted on
the displayed model. Selecting multiple parts in the parts list will highlight all the
selected Parts.
Using <alt> + Left Mouse button you may select a part in the model view window and
make it the current part. The part selected with the mouse will be selected in either
the part list in the plots panel or parts panel. This is useful to identify parts and to
make a particular part the current part active for zoning, filling or other part
operations.
156
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
The default highlight color is golden yellow; you may alter the color and opacity of
the highlight color that is applied to selected parts using the associated options
panel.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
157
AUTODYN User Manual
History
History
This panel lets you compose and display time histories of Gauge points and
Summary variables.
When you select this panel, the history and summary data associated with the model
you are working with will be automatically loaded and the model's Ident will be
displayed in the window at the top of the panel.
Load
Press this button to load history data for other models.
Remove
158
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Press this button to remove history data for the selected model (at least one model
must remain loaded at all times).
Reduce
Press this button to reduce the amount of history data stored for a model.
History Type
Select the type of history you want to view from the following options :
Gauge Points
Material
Summaries
Part Summaries
Energy
X momentum
Y momentum
Z momentum
Jetting Analysis
Variable histories at gauge points
Mass, energy and momentum sums for
each material
Mass, energy and momentum sums for
each Part
Energy balance
X momentum balance
Y momentum balance
Z momentum balance
Jetting analysis plots (only active if model
uses Jetting)
Single Variable Plots
Press this button to compose plots of a single variable
Multiple Variable Plots
Press this button to compose plots including multiple variables
Examine
Use the Left Mouse Button to select a point on the graph. The corresponding curve
label and x and y values are displayed in the Examine panel.
Integrate
Check this box to view integrals of the variables in the current plot.
Differentiate
Check this box to view differentials of the variables in the current plot.
Min/Max
Press this button to view maximum and minimum values for the current plot.
Write textfile (uhs)
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
159
AUTODYN User Manual
Output the data from the current plot (Write UHS for current history plot) or output all
the gauge data from a history file (Write Output for all gauges and variables in
selected ident).
Set scales
AUTODYN automatically chooses scales for your plots based on minimum and
maximum values of the data. Pressing this button lets you set your own scales.
Plot Styles
Press this button to set the color, style and thickness of lines for each plot
Legend Position
Press this button to position the legend anywhere in the view.
160
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
History - Single Variable Plot
This window lets you compose a single variable plot.
Single variable plots can contain one or more plots (histories) for the same X and Y
variables.
Ident
This pull-down menu lets you select an Ident from the models you have loaded.
Y Var
This pull-down menu lets you choose the variable assigned to the Y axis.
X Var
This pull-down menu lets you choose the variable assigned to the X axis (most often
TIME).
Histories to display
From the list on the left choose as many histories as you wish to display in the plot
(use the control and shift keys in the usual way to make your selection).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
161
AUTODYN User Manual
The choices you have available for variables and histories will depend on the type of
plot you have chosen (Gauge points, Material Summaries, etc.).
162
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
History - Reduce
It is usual to save history data very frequently (the default is every cycle) in order to
capture high frequency responses.
If a calculation is run for a large number of cycles the history files can become very
large.
This window lets you reduce the size of history files by removing data for some
cycles.
Select file
In this box, select the ident of the file you wish to reduce in size.
Reduce by
Specify the reduction factor in this field.
If you specify a reduction factor of 2, data for every other cycle will be removed from
the file.
If you specify a reduction factor of 3, data for two out of every three cycles will be
removed from the file.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
163
AUTODYN User Manual
History Write Text Output
This dialog lets you output the data from the current plot (Write UHS for current
history plot) or output all the gauge data from a history file (Write Output for all
gauges and variables in selected ident).
Write UHS for current history plot
Select this option to output to a CSV (comma separated variable) file, which is
suitable for importing into Microsoft Excel the data from the currently plotted history
file.
Write Output for all gauges and variables in selected ident
Selecting an ident and variable to output, all the data for each gauge for the selected
variable and ident is written to the output file.
Output Format
Select the format for the data output, either a CSV (Comma separated variable) file
or an html file.
164
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Multiple Variable Plot
History - Multiple Variable Plot
This window lets you compose a multiple variable plot.
Multiple variable plots can contain one or more plots (histories), each with different
variables for the X and Y axes.
This window list the plots (histories) you have currently define, displaying for each
one its Ident, Gauge number, X variable and Y variable.
Below this list are four buttons :
Select
Press this button to quickly add multiple plots to the list.
Modify
Select a plot in the list and press this button to modify its settings.
Add plot
Select a plot in the list and press this button to add a new plot to the list. The initial
settings for the new plot will be the same as the selected plot, but you can modify
these values immediately in the dialog window that opens.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
165
AUTODYN User Manual
Delete plot
Press this button to delete a plot from the list.
The choices you have available for gauges and variables will depend on the type of
plot you have chosen (Gauge points, Material Summaries, etc.).
166
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
History - Multiple Variable Plot - Set All Plots
This window lets you quickly add multiple plots to a multiple variable plot list.
Select ident
This pull-down menu lets you choose an ident from the models you have loaded.
Select gauge(s)
This box lets you choose one or more gauges (use the control and shift keys in the
usual way to make your selection).
Select Y-variable(s)
This box lets you choose one or more variables for the Y axis (use the control and
shift keys in the usual way to make your selection).
Select X-variable
This pull-down menu lets you choose a variable for the X axis.
Number of selected plots:
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
167
AUTODYN User Manual
This tells you how many plots you have defined with your current selections. The
number of plots is the union of all selections in the four input regions.
168
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
History - Multiple Variable Plot - Modify Selected Plot
This window lets you set or modify parameters for a plot to be included in a multiple
variable plot.
Ident
This pull-down menu lets you choose the Ident for the plot from the models you have
loaded.
Gauge
This box lets you select the gauge to be plotted
Y Variable
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
169
AUTODYN User Manual
This pull-down menu lets you pick the Y Variable
X Variable
This pull-down menu lets you pick the X Variable
Line color
This pull-down menu lets you pick the color of the line.
Line style
This pull-down menu lets you pick the line style (solid, dashed, etc.)
Line thickness
This box lets you set the line thickness
170
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
History - Min/Max
This window displays the maximum and minimum values for each history plot shown
in the current view.
X min is the X value at which the minimum Y value occurs
Y min is the minimum Y value
X max is the X value at which the maximum Y value occurs
Y max is the maximum Y value
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
171
AUTODYN User Manual
History - Set Scales
This window lets you set your own scales for history plots.
Minimum
These fields let you set the minimum values for your X and Y scales
Maximum
These fields let you set the maximum values for your X and Y scales
Increment
These fields let you set the X and Y increments where tick marks will be placed on
the scales.
Reset X
Press this button to reset the maximum and minimum X values to those calculated
automatically by AUTODYN.
Reset Y
Press this button to reset the maximum and minimum Y values to those calculated
automatically by AUTODYN.
172
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Major Tick Lines
Check this box if you want major tick lines to extend from left to right and top to
bottom across your plot.
Major Tick Style
This pull-down menu lets you choose the line style used to drawn tick lines (solid,
dashed, etc.)
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
173
AUTODYN User Manual
History - Set Plot Styles
This window lets you set the color, style and thickness of lines for each plot
Plot Number
Plots are numbered in the order you specify them, starting at 1. The box on the left
lets you select a plot number whose style you wish to set.
Color
Select a color for the selected plot from the top two rows on the right.
Line Style
Select a line style for the selected plot from the next four rows on the right
Line Thickness
Select a line thickness for the selected plot from the bottom row on the right
User plot title
174
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Check this box if you want to supply your own title for the plot. The default title is
"History Plot"
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
175
AUTODYN User Manual
History - Set Legend Position
This window lets you place the plot legend anywhere in the view.
Use the two sliders to adjust the horizontal and vertical position of the legend until it's
where you want it.
176
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
History - Load
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
177
AUTODYN User Manual
This window lets you load history files for plotting.
History data is stored in two types of files.
.his
These files contain history data for the gauge points defined for a model.
.sum
These files contain history data for summary plots (Material Summaries,
Part Summaries, Energy, etc.)
Depending on the plot type you have chosen, this window lets you navigate your file
system to find .his or .sum files for loading.
178
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Slides
This panel lets you compose slide shows from images created using the Text Slide,
Camera (single slide) and Animation (multiple slides) buttons on the Tool Bar.
Directory
The current directory where the slides are stored and processed is shown in this
Box.
Press the Browse button below the box to change this directory.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
179
AUTODYN User Manual
After changing the directory, press the Refresh button to update the list of slides in
the slide sequence box.
Search Pattern
You can type a search pattern in this field that restricts the files you see in the slide
sequence box.
In the example above the search pattern restricts files you see to those having an
ident "ben3d1" and extension .gif .
( all .gif, .bmp, .tiff and .jpeg files are shown if the search pattern does not include
an extension)
Slide Sequence Box
The left center box shows the current slide sequence.
Initially the slide sequence will contain all the files in the current Directory that
satisfy the Search Pattern, listed in alphanumeric order.
You can use the Cut/Paste and Shuffle Up/Down buttons to remove or rearrange
files in the slide sequence.
Press the Refresh button if you want to abandon your current sequence and start
over with all files in alphanumeric order.
When you select a file in the slide sequence, the image of that file is automatically
displayed in the View panel.
Shuffle Up/Down
These buttons let you move one or more files up or down in the slide sequence.
Select the group of files you want to move (using the shift key to select more than
one file), and press the Shuffle Up or Shuffle Down button to move them
collectively one position up or down respectively.
Cut
Select one or more files in the slide sequence and press this button to remove them.
The removed files are placed on the clipboard and you can use the Paste button to
restore them at some other point in the sequence. If you use Cut a second time, the
clipboard is cleared and the newly removed files are placed on it
.
Paste
Press this button to insert all files from the clipboard after the selected file in the
slide sequence.
Slides on clipboard
180
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
This shows you how many slide files are currently on the clipboard.
Time delay
Select one or more files in the slide sequence and rotate the dial to set the time
delay you want to apply to them (a slide's time delay is the time, in seconds, for
which it is shown).
Instead of using the dial, you can alternatively type the time delay in the field below
the dial.
Loop
Check the box if you want your slide show to replay automatically.
Run
Press this button to play the current slide sequence. The entire sequence is played,
irrespective of which files are currently selected.
Stop
Press this button to stop playing the current slide sequence.
Forward / Backward
These buttons let you quickly change your selection to the preceding (Backward) or
following (Forward) file in the slide sequence.
Since this procedure automatically updates the View panel, this is a good way of
viewing your slides manually.
Extract GIF
Press this button to extract individual .gif files from an animated GIF and place them
in the current directory.
Warning!
This option removes the current slide sequence and replaces it with a sequence
containing only the newly extracted files (irrespective of the current search pattern).
Save Seq.
Press this button to store the current slide sequence in a sequence file.
Load Seq.
Press this button to load a sequence stored in a sequence file and apply it to the
current directory.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
181
AUTODYN User Manual
Warning!
If the files listed in the sequence do not exactly match those in the current directory,
results may be unpredictable.
Create GIF
Press this button to create a GIF animation from the current slide sequence.
Create AVI
Press this button to create an AVI animation from the current slide sequence.
Create MPEG
Press this button to create an MPEG animation from the current slide sequence.
Compress AVI
Check this toggle to choose compression for AVI.
In the choose compression dialog, select the type of compression to use for the
movie. The size and quality of the resulting AVI animation will depend on the
choices made in this panel.
182
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
View Slides (Slide Viewer)
The View Slides option on the Navigation Bar starts the Slide Viewer (it can also be
run independently of AUTODYN).
The Viewer lets you load and view GIF and GFA animations.
Components of the Viewer's user interface :
View Window
This is where your animations are shown.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
183
AUTODYN User Manual
Pull-down Menus
File
This pull-down menu lets you load single GIF and GFA animation files for
playback, and exit the program.
Sequence
This pull-down menu lets you playback multiple GIF animations using
sequence files.
A sequence file contains a list of GIF animations you want to view
consecutively.
All the animations in a sequence file must be in the same directory as the
sequence file.
New Sequence File
This option opens a new sequence file.
Open Sequence File
This option opens an existing sequence file.
Edit Sequence
This option lets you insert and delete animations in the current sequence
file.
The following dialog window appears when you select this option :
184
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Sequence list
The box at the top of this dialog contains a list of the animations
currently included in the sequence, together with their time delay
(how long the first slide in the sequence is shown, in seconds).
Insert
Press this button to insert another animation immediately after the
selected animation.
Delete
Press this button to delete the selected animation.
Delay
Enter a time delay in this field (in seconds). When you Insert an
animation, this time delay is applied.
You can create and edit sequence files manually if you wish. Sequence
files must have a .seq extension and use the following format
Format
Example
The number of animations 3
in the sequence
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
185
AUTODYN User Manual
0.0 anim.gif
Default frame delay in
seconds + <space> + file
name
Default frame delay in
seconds + <space> + file
name
1.2
another.gif
1.6
yetanother.gif
Default frame delay in
seconds + <space> + file
name
etc.
Save As
This option saves the current sequence file (.seq)
Control
This pull-down menu provides the same functions that are available in the
Control Bar.
Control Bar
This bar lets you control the playing of the GIF or GFA animation you have loaded.
Pressing a button on this bar performs the following actions (you can type the
corresponding Hotkey as an alternative to pressing the a button).
Button
Hotkey Action
Go to the first frame of the
b
animation
r
Go back one frame
x
186
Play (from the current frame)
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
p
s
a
e
Pause (at the current frame).
This is a toggle button.
Stop (at the current frame)
Advance one frame
Go to the last frame of the
animation
View Bar
This bar only appears when you have loaded a GFA animation.
The buttons on this bar let you control how you view your GFA animation and work in
the same way as the corresponding icons in the AUTODYN Tool Bar
Rotate view
Translate view
Zoom in or out
Set view (brings up a window that allows you to set an exact view)
Reset view (to the initial view)
Turn perspective on or off (toggle)
Frames Slider
This slider lets you move quickly to any frame in the animation(s).
Speed Slider
This slider lets you adjust the playback speed for animations.
Loop
Check this box if you want the animation(s) to automatically start again from the first
frame when the last frame is reached.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
187
AUTODYN User Manual
Materials
Materials
This panel lets you define the materials you want to use in your model.
Material List
The box at the top of this panel lists the materials you have currently defined for your
model. You can select materials in this list.
New
Press this button to define a new material.
Modify
Press this button to modify parameters for the selected material.
Copy
Press this button to copy material component data from an existing material to either
a new material or another existing material.
Delete
Press this button to delete one or more materials from your model.
Review
188
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Press this button to review the parameters for the selected material in a browser
window.
Library
The default material library is standard.mlb. This contains all the material data
provided by Century Dynamics.
Press this button if you want to change the material library to some other material
library you have obtained or created.
Load
Press this button to load materials from your current material library.
Save
Press this button to save the materials you have defined to a material library.
Current material library
This box displays the current material library you have selected.
Update Library
Press this button to update old material library files, so that they can be used with
this version of AUTODYN.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
189
AUTODYN User Manual
Materials - New / Modify
This window lets you define or modify the model components and parameters used
for a material.
190
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Name
Enter a name for your material in this field.
Reference Density
Enter the reference density (usually the initial density) for your material in this field.
EOS
This option lets you define the Equation of State you want to use for your material.
Press
next to this option to expand the dialog.
Select the Equation of State you want to use from the pull-down menu :
Then type in parameter values in the fields provided :
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
191
AUTODYN User Manual
Strength
This option lets you define the strength model you want to use for your material.
Press
next to this option to expand the dialog.
Select the strength model you want to use from the pull-down menu :
Then type in parameter values in the fields provided:
Failure
This option lets you define the failure model you want to use for your material.
Press
next to this option to expand the dialog.
Select the failure model you want to use from the pull-down menu :
Then type in parameter values in the fields provided :
192
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Erosion
This option lets you define the erosion model you want to use for your material.
Press
next to this option to expand the dialog.
Select the erosion model you want to use from the pull-down menu :
Then type in the parameter values in the fields provided :
Cutoffs
This option lets you change the cutoffs for your material.
It is best to use the default values for these cutoff if you are using the default units
(mm,mg,ms).
Press
want.
next to this option to expand the dialog and change whatever cutoffs you
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
193
AUTODYN User Manual
Material Reference
Press
next to this option to expand the dialog and type in a reference for your
material in the field provided.
194
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Materials - Copy
This window lets you copy component data from an existing material to either a new
material or another existing material.
Select material to copy from
Select the material you want to copy from this pull-down menu.
Select data components to copy
Check the box alongside the components you want to include in the copy process.
Copy to
Choose to copy the data to a new material or an existing material.
If you copy to a new material, components not copied will be set to the default state.
If you copy to an existing material, components not copied will retain their existing
state.
New material name
If you choose to copy to a new material, enter your name for the new material in this
field.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
195
AUTODYN User Manual
Materials - Delete
This window lets you delete materials from your model.
Select the material(s) you want to delete and press
.
If the material you want to delete has been assigned to one or more Parts, you will
be asked to confirm that it's OK to remove the material from the Part(s) :
Elements that have their material removed become Unused.
196
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Materials - Load
This window lets you load materials from the current Material Library.
The available materials are listed in a vertical scroll box. For each material four
columns provide its material name, Equation of State, Strength Model and Failure
Model.
Press the button at the top of each column to sort materials alphanumerically in that
column.
Using the control and shift keys as necessary, you can select one or more materials.
Press
to load the selected materials into your model.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
197
AUTODYN User Manual
Press
198
to delete the selected materials from the library.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Initial Conditions
Initial Conditions
This panel lets you create Initial Condition Sets that can be used in Fill operations
for Parts.
You do not have to use an Initial Condition Set to fill a Part, but there is a major
advantage in using one.
Any subsequent changes you make to an Initial Condition Set are automatically
applied to the Parts that have been filled using that Initial Condition Set.
This means you don't have to refill the Parts (this is currently not true for Euler
Parts).
Initial Condition Set List
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
199
AUTODYN User Manual
The box at the top of this panel lists the Initial Condition Sets you have currently
defined for your model. You can select an Initial Condition Set in this list.
New
Press this button to define a new Initial Condition Set.
Modify
Press this button to modify the selected Initial Condition Set.
Delete
Press this button to delete one or more Initial Condition Sets from your model.
Review
Press this button to review the parameters for the selected Initial Condition Set in a
browser window.
Implicit-Explicit Model Initialization
Activate
Select this option to initialize an AUTODYN analysis model using the results of an
ANSYS Mechanical implicit analysis.
Results File
Select the ANSYS .rst results file to be used to initialize the AUTODYN analyses.
Transfer Type
Select the initialization method; either the Displacement Only or the Material State
option as described below.
Results Time
The result time from the ANSYS Mechanical implicit analysis at which to extract
results from the .rst file.
Timestep factor
(Note that this option is only applicable for the Displacement Only method.) The
initial timestep from the AUTODYN solution is multiplied by the timestep factor. The
resulting time (PVELTM) is used together with the nodal displacements from the
ANSYS Mechanical analysis to calculate constant nodal velocities. These nodal
velocities are applied to the AUTODYN model over PVELTM in order to initialize the
AUTODYN nodes to the correct positions.
200
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Initial Conditions - New/Modify
This window lets you define a new Initial Condition Set.
Name
Enter your name for the Initial Condition Set in this field
Velocity Only
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
201
AUTODYN User Manual
Select this option if you want your Initial Condition Set to only include velocities (top
left window).
Include Material
Select this option if you want your Initial Condition Set to include velocities and a
material and its associated variables (top right window)
Material
Use this pull-down menu to select the material you want to assign to the Initial
Condition Set.
Material variables
Enter the appropriate values for the material density and internal energy to be used
with this initial condition.
In addition, if the initial condition is to be used with a shell element, the element
thickness can be specified. Note that this must be used for the unstructured solvers.
Translational Velocity
Specify the global x, y and z velocity associated with the initial condition.
Radial Velocity
This option lets you define an initial velocity of fixed magnitude. The direction of the
velocity will be defined by the radial position of each node from the original (0.,0.,0.).
Spherical and cylindrical symmetry options are available.
Angular Velocity (3D only)
An angular velocity can be specified in addition to translational velocity in
AUTODYN-3D.
The angular velocity is defined in radians / time and the axis of rotation is defined
through the direction cosines of a vector passing through a point in space.
202
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
During the Fill of a Part, the angular velocity and spin axis are used to calculate the
resultant x, y and z velocity at each node. These are then added to any specified
translational velocities.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
203
AUTODYN User Manual
Initial Explicit Model Initialization
AUTODYN explicit analysis can be initialized (or pre-stressed) with the results from
either a linear static structural, non-linear static structural or transient dynamic
ANSYS Mechanical implicit analysis. Note that this feature requires the ANSYS
results to be saved to a .rst file.
It is assumed that the same mesh is always used in both the implicit and explicit
analyses; otherwise results will not be mapped onto the explicit mesh correctly. Note
that quadratic elements may be used in the implicit model. In this case results for
the corner nodes and average results for the element will be applied to the explicit
mesh.
The user is advised to check the autodyn.log file shortly after starting the AUTODYN
analysis as any errors occurring during the implicit results transfer will be echoed to
this file.
Activate
Initialization of an explicit analysis under implicit analysis results can be selected
using the Activate option under Initialize using ANSYS Mechanical results.
The menu shown above is used to configure the transfer of data from the ANSYS
Mechanical to the AUTODYN solution and in which manner AUTODYN will be
initialized.
Results File
Select the ANSYS .rst results file to be used to initialize the AUTODYN analysis.
Transfer Type
Either the Displacement Only or the Material State option as described below.
Transfer Type options are available to define what analysis results need to be
transferred from the ANSYS implicit analysis to initialize the AUTODYN analysis:
1. Displacement Only
204
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Nodal displacements from an ANSYS linear static solution are used to initialize
the AUTODYN nodal positions. These displacements are converted to
constant nodal velocities and applied for a pre-defined time in order to obtain
the required displaced co-ordinates. During this time elements stress/strains
are calculated as normal by AUTODYN. Once the displaced nodal positions
are achieved all nodal velocities are set to 0 and the solution is completely
initialized.
This option is applicable to unstructured solids (hexahedral and
tetrahedral), shells and beams
This option is only applicable to results from a linear, static structural
analysis.
Linear elastic materials only can be used in the explicit analysis when
using the Displacement Only Option.
Note that after AUTODYN model initialization static damping
(Controls>Damping Options>Static Damping) needs to be applied to
change the AUTODYN calculation from a dynamic solution to a state of
stress equilibrium. For optimal convergence, the value chosen for the
damping constant, R, may be defined by:
R=2*timestep/T
where timestep is the expected average value of the timestep and T is the
longest period of vibration for the system being analyzed.
2. Material State
Nodal displacements and element stresses, strains, plastic strains and
velocities from an ANSYS solution are used to initialize an AUTODYN analysis
at cycle 0.
The AUTODYN solution is therefore completely initialized at the start of the
analysis.
This option is only applicable to unstructured solid elements (hexahedra
and tetrahedral)
This option is applicable to results from a linear static structural, non-linear
static structural or transient dynamic Mechanical system.
The following materials can be used in the AUTODYN solution with the
Material State Option. Equations of State (linear, hyperelastic). Strength
Models (elastic, von-Mises Johnson-Cook, piecewise, Zerilli Armstrong,
Steinberg Guinan, Cowper Symonds, hyperelastic, bilinear isotropic
hardening).
Note that static damping can also be applied by using a static damping
constant, but this may not be required.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
205
AUTODYN User Manual
Results Time
The result time from the ANSYS Mechanical implicit analysis at which to extract
results from the .rst file. For a linear static solution this will always be 1.0. For a
nonlinear or transient dynamic solution this time will correspond to a result time from
the ANSYS Mechanical analysis.
Timestep factor
(Note that this option is only applicable for the Displacement Only method.) The
initial timestep from the AUTODYN solution is multiplied by the timestep factor. The
resulting time (PVELTM) is used together with the nodal displacements from the
ANSYS Mechanical analysis to calculate constant nodal velocities. These nodal
velocities are applied to the AUTODYN model over PVELTM in order to initialize the
AUTODYN nodes to the correct positions.
206
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Initial Conditions - Delete
This window lets you delete Initial Condition Sets from your model.
Select the Initial Condition Set(s) you want to delete and press
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
.
207
AUTODYN User Manual
Boundaries
Boundaries
This panel lets you create Boundary Conditions that can be applied to Parts.
Boundary Condition List
The box at the top of this panel lists the Boundary Conditions you have currently
defined for your model. You can select a Boundary Condition in this list.
New
Press this button to define a new Boundary Condition.
Modify
Press this button to modify the selected Boundary Condition.
Delete
Press this button to delete one or more Boundary Conditions from your model.
Review
Press this button to review the parameters for all Boundary Conditions in a browser
window.
208
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Boundaries - New / Modify
This window lets you define a new boundary condition.
Name
Enter your name for the boundary condition in this field.
Type
Select the type of boundary condition you want to use from this pull-down menu :
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
209
AUTODYN User Manual
Sub Option
Select the sub-option you want to use from this pull-down menu :
Parameters
Enter values for any parameters associated with your selection in the fields provided
(e.g. Constant Z Velocity).
210
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Boundaries - Delete
This window lets you delete Boundary Conditions from your model.
Select the Boundary Condition(s) you want to delete and press
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
.
211
AUTODYN User Manual
Parts
Parts
In AUTODYN, you build your model in Parts. There are two concepts for node,
element and part data storage and processing available.
Structured Parts
For structured parts in AUTODYN, all information relating to the mesh and the
elements in the mesh is stored and processed using the concept of I, J and K lines
(IJK-space). This means that for an element whose quantities are stored at position
(I, J, K), the nodes belonging to that element are automatically defined in IJK space
as (I-1, J,K), (I, J-1,K), (I-1, J-1,K),.....(see the figure below).
Typical Connectivity for IJK-based Element in AUTODYN
The element connectivity is therefore implicitly defined by the structure within the I, J,
K indexing. Information relating to each point in IJK space is also stored in this
structure. Furthermore, in this structured approach, the node and element storage
and processing is directly linked to the Parts in the model.
Each structured Part is a grid (or group of SPH nodes) that a particular solver
operates on.
AUTODYN offers many tools for the generation of structured Parts as will be
described below.
Unstructured Parts
For unstructured parts an alternative "Unstructured" approach to storing and
processing information relating to the mesh is used for the solvers: The basic
entities needed in the simulation are the Nodes, Elements, Faces Joints etc. In this
scheme, these are stored in unique and independent global "Entity" lists, where an
entity is a node, element, face, join etc. Connectivity between entities is determined
by cross-referencing to the appropriate global entity list. The data associated with
212
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
each entity is also stored in a manner most efficient for solving the equations and
does not need to follow a set structure/order.
A global list of all elements relating to unstructured Parts is maintained. Each
element is given a unique identifying number from one to total number of elements.
Each element also has a user element number associated with it for the purposes of
model manipulation and user identification.
Each element will have a list of variables associated with it the number and type of
variables depending on the type of element (for example a hexahedral element
containing an orthotropic material or a triangular shell with a rigid material).
Each element has three numbering systems for its connecting nodes (see figure)
A local isoparametric number; used to loop over the nodes of an element in
the correct order and solved the physical equations. Each element with the
same topology has the same numbering system.
An internal node number; the physical properties of each node are referenced
via the global node lists. A connectivity table is used to cross-reference the
local node number to an entry in the physical node list.
A user node number; a number assigned by the user to define the element
Example Element and Node Numbering
For the unstructured solvers in AUTODYN, Parts are simply used to allow easy
grouping and manipulation of various regions of the model. They are not related to
the actual data storage for the elements and nodes, as in IJK-based Parts.
The default definition of a Part currently used for the unstructured solvers is: "A Part
is a list of elements of the same classification (volume, shell, beam) that are
connected together via the connectivity table of the elements"
Note that within each Part, all elements must be of the same class (volume, shell or
beam), but not necessarily the topology. For example a shell Part may contain a
mixture of quadrilateral and triangular elements. Nodes are only related to Parts
through the element connectivity. Nodes can therefore exist in multiple Parts, for
example if the same node is connected to a beam and shell element.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
213
AUTODYN User Manual
AUTODYN doesn't offer any capability of generating unstructured elements and
Parts manual. Unstructured elements and Parts can be generated in ANSYS
Workbench and transferred to AUTODYN.
Furthermore unstructured models in MSC.Nastran or LS-Dyna format can also be
imported directly into AUTODYN.
The following 3D Lagrangian unstructured element types are supported:
Volume elements
o 8 noded hexahedral elements
o 6 noded pentahedral elements (to be used as transition elements)
o 4 noded tetrahedral elements
Shell elements
o 4 noded quad elements
o 3 noded tria elements (to be used as transition elements)
Beam elements
o 2 noded beam elements
The following 2D Lagrangian unstructured element types are supported:
Volume elements
o 4 noded quadrilateral volume elements
o 3 noded triangular volume elements
Note:
1. The 2D Lagrangian unstructured element types have Beta status and
therefore may not be as stable or robust as expected in a general release
version.
2. A 2D or 3D analysis involving unstructured parts with only rigid materials may
result in unphysical results, because rigid bodies do not have a minimum time
step associated with them and therefore too large displacements may occur
from cycle to cycle and contact can be missed. For this type of analysis the
user needs to manually define a small time step for the analysis.
This panel lets you create structured Parts and modify the structured and
unstructured Parts of your model.
Part List
214
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
The box at the top of this panel lists the Parts you have currently defined for your
model. You can select a Part in this list.
The size of the structured parts is displayed in terms of maximum I, J and K of the
part (see Part Euler above). Structured SPH parts are displayed in terms of the total
number of SPH nodes, because SPH parts don't use elements.
For unstructured parts the size of part is displayed as the total number of elements
(see Parts PROJECTILE and TARGET above).
New
Press this button to create a new structured part.
Load
Press this button to load a structured Part from a Part Library.
This option is not available for unstructured Parts because for these types of Parts
the ANSYS Workbench project data storage can be used as a part library.
Copy
Press this button to copy an existing Part to a new Part. This is valid for both
structured as well as unstructured Parts.
Save
Press this button to save structured Parts to a Part Library. This option is not
available for unstructured Parts because for these types of Parts the ANSYS
Workbench project data storage can be used as a part library.
Delete
Press this button to delete a structured/unstructured Part.
The remaining dialog in this panel depends on the Solver used by the selected Part.
All Structured Solvers except SPH
SPH Solver
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
215
AUTODYN User Manual
Unstructured Solvers
Zoning
Press this button to zone a structured Part.
Unstructured Parts cannot be generated; an unstructured Part can only be
translated, rotated or scaled.
Fill
Press this button to fill a part with materials and initial conditions.
Geometry (Zoning)
Press this button to define geometric objects for SPH Parts
Pack (Fill)
Press this button to pack geometric objects with SPH nodes.
Boundary
Press this button to apply boundary conditions to a Part.
Gauges
Press this button to assign gauges to a part.
Motions
Press this button to assign motion constraints to a structured ALE Part.
Solver
Press this button to select solver options for a Part.
IJK Range
Press this button to modify the IJK range for a structured Part
Activation
Press this button to set activation / deactivation times for a structured Part.
For unstructured Parts activation / deactivation time cannot be set (they are always
activated).
Rename
Press this button to rename a Part.
Print
216
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Press this button to set print ranges for a Part.
This option is not available for unstructured Parts.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
217
AUTODYN User Manual
New
Parts - New
218
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
This window lets you create a new structured Part.
Part Name
Enter your name for the Part in this field.
Solver
Select the Solver you want to use for the Part.
Definition
You can select to define your Part manually or using the Part Wizard (the Part
Wizard cannot be used for SPH or Beam Solvers, so these options are not displayed
for these solvers)
Manual
If you choose this option, fields appear for you to specify the maximum I, J and
K range for your Part (left window above).
After pressing
you return to the Parts panel where you can define your
Part manually using the Zoning and Fill buttons.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
219
AUTODYN User Manual
Part Wizard
If you choose this option, you advance through three more dialog windows that
guide you through the complete definition of your part, using one of a number
of pre-defined geometries (Predefs).
The first dialog window lets you choose the Predef you want to use.
The second dialog window lets you define your zoning.
The third dialog window lets you fill your part.
Press
to advance through the dialog windows, then press
the last window to create your Part.
220
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
in
AUTODYN User Manual
Parts - New - Select Predef (2D)
This window lets you select the Predef you want to use for the 2D Part you are
creating.
Press one of the five buttons at the top of this window to select your Predef :
Box
This predef is a box with its axes parallel to the X and Y axes.
Origin
Enter the X and Y coordinates of the lower corner of the box in the fields
provided.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
221
AUTODYN User Manual
Box Dimensions
Enter the dimensions of the box (DX, DY) in the fields provided
Circle
This predef is a circle.
Section
Choose the section you want to generate (Whole, Half or Quarter). This should
match any symmetry planes you have defined for your model.
Solid or Hollow
Choose either a solid or hollow cylinder.
222
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
If you choose a hollow cylinder, you will have to specify inner and outer radii for
the cylinder.
Origin
Enter the X and Y coordinates for the center of your circle in the fields
provided.
Outer Radius
Enter the outer radius of your circle.
Rotation
Enter the rotation (in degrees) of your circle relative to the X-axis.
Ogive
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
223
AUTODYN User Manual
This predef is an ogive with its axes parallel to the X and Y axes.
Section
Choose the section you want to generate (Whole or Half). This should match
any symmetry planes you have defined for your model.
Solid or Hollow
Choose either a solid or hollow ogive.
If you choose a hollow ogive, you will have to specify inner and outer radii for
the ogive.
Origin
Enter the X and Y coordinates for the center of your ogive in the fields
provided.
End Radius
Enter the end radius of your ogive in this field.
Ogive Radius
Enter your ogive radius in this field.
Principal Direction
Select the direction of the principal axis for your ogive from the pull-down menu
Wedge
224
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
This predef is a wedge with its lower edge lying on the X-axis. The wedge
angle is automatically set by AUTODYN.
This predef is useful for running 1D cylindrical or spherical symmetric problems
in 2D.
Minimum radius
Enter the minimum radius of the wedge (this cannot be zero).
Maximum radius
Enter the maximum radius of the wedge.
Rhombus
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
225
AUTODYN User Manual
This predef is a rhombus with its diagonals parallel to the X and Y axes.
Section
Choose the section you want to generate (Whole, Half or Quarter). This should
match any symmetry planes you have defined for your model.
Origin
Enter the X and Y coordinates for the center of your ogive in the fields
provided.
Width
Enter the width of the rhombus.
Height
226
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Enter the height of the rhombus.
Quad
Coordinates X1, Y1:
Enter coordinates of the first point of the quad.
Coordinates X2, Y2:
Enter coordinates of the second point of the quad.
Coordinates X3, Y3:
Enter coordinates of the third point of the quad.
Coordinates X4, Y4:
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
227
AUTODYN User Manual
Enter coordinates of the fourth point of the quad.
228
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - New - Select Predef (3D)
This window lets you select the Predef you want to use for the 3D Part you are
creating.
Press one of the six buttons at the top of this window to select your Predef :
Box
This predef is a box with its axes parallel to the X, Y and Z axes.
Origin
Enter the X, Y and Z coordinates of the lower corner of the box in the fields
provided.
Box Dimensions
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
229
AUTODYN User Manual
Enter the dimensions of the box (DX, DY, DZ) in the fields provided
Cylinder
This predef is a cylinder with its axis parallel to the Z axis.
Section
Choose the section you want to generate (Whole, Half or Quarter). This should
match any symmetry planes you have defined for your model.
Solid or Hollow
Choose either a solid or hollow cylinder.
230
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
If you choose a hollow cylinder, you will have to specify inner and outer radii for
the cylinder.
Origin
Enter the X, Y and Z coordinates for the center of the starting surface of your
cylinder in the fields provided.
Start Radius / End Radius
You can specify different radii for the starting and end faces of your cylinder.
For a regular cylinder (constant radius), set the starting radius equal to the end
radius.
Length
Enter the length of your cylinder in this field.
Start Surface / End surface
The starting and end surfaces of your cylinder can be flat, concave or convex.
If you select a concave or convex surface, you will have to specify its radius of
curvature.
Ogive
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
231
AUTODYN User Manual
This predef is an ogive with its axis parallel to the Z axis.
Section
Choose the section you want to generate (Whole, Half or Quarter). This should
match any symmetry planes you have defined for your model.
Solid or Hollow
Choose either a solid or hollow ogive.
If you choose a hollow ogive, you will have to specify inner and outer radii for
the ogive.
Origin
232
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Enter the X, Y and Z coordinates for the center of your ogive in the fields
provided.
End Radius
Enter the end radius of your ogive in this field.
Ogive Radius
Enter your ogive radius in this field.
Sphere
This predef is a sphere.
Section
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
233
AUTODYN User Manual
Choose the section you want to generate (Whole, Half, Quarter or Eighth). This
should match any symmetry planes you have defined for your model.
Solid or Hollow
Choose either a solid or hollow sphere.
If you choose a hollow sphere, you will have to specify inner and outer radii for
the sphere.
Origin
Enter the X, Y and Z coordinates for the center of the sphere in the fields
provided.
Radius
Enter the radius of the sphere in this field.
Hex
234
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Select Node to Edit
Use the arrow buttons to select each of the 8 nodes in turn.
Coordinates
Enter the X, Y and Z coordinates of the node.
Frag/Brick
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
235
AUTODYN User Manual
The fragment/brick wall is built with its axes parallel to the X, Y and Z axes.
The X direction runs the length of the wall.
The Y direction runs the height of the wall.
The Z direction runs through the thickness of the wall.
Number of fragments/bricks
Use these fields to set the number of fragments/bricks in the X, Y and Z
directions.
Length of each fragment/brick
Use these fields to set the length of a single brick/fragment in the X, Y and Z
directions.
Mortar size between each fragment/brick
Use these fields to set the mortar size (or gap) between fragments/bricks.
236
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Mortar included in dimension?
Check this box if you want the mortar size to be included in the length of each
brick/fragment.
Offset ratio
Set the offset ratio for the fragments/bricks in this field.
This is how the bricks are staggered along the length of the wall.
e.g. if the offset is 0.5 (the default), the bricks will be staggered halfway across
each other as shown in the above figure.
Fragment/brick symmetric about X=0?
Check this box if you want the wall to be symmetric about X=0.
Enter the required dimensions for your predef and press
next dialog window (Define Zoning).
to advance to the
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
237
AUTODYN User Manual
Parts - New - Select Predef (3D Shell)
This window lets you select the Predef you want to use for the Shell Part you are
creating.
Press one of the two buttons at the top of this window to select your Predef :
Plane
This predef is a plane perpendicular to the X Y or Z axis.
Plane Orientation
Select the orientation of the plane (e.g. XY-plane is a plane perpendicular to
the Z axis).
238
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Origin
Enter the X, Y and Z coordinates of the lower corner of the plane in the fields
provided.
Box Dimensions
Enter the dimensions of the box (DX, DY, DZ) in the fields provided
Cylinder
This predef is a cylinder with its axis parallel to the Z axis.
Section
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
239
AUTODYN User Manual
Choose the section you want to generate (Whole, Half or Quarter). This should
match any symmetry planes you have defined for your model.
Origin
Enter the X, Y and Z coordinates for the center of the starting surface of your
cylinder in the fields provided.
Start Radius / End Radius
You can specify different radii for the starting and end faces of your cylinder.
For a regular cylinder (constant radius), set the starting radius equal to the end
radius.
Length
Enter the length of your cylinder in this field.
240
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - New - Define Zoning (2D)
This window lets you Define the zoning for your 2D Part.
Box
No Grading
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
241
AUTODYN User Manual
Grading in X and Y
Cells
Enter the number of cells (elements) you want to use in the I and J directions in
fields provided. The corresponding number of nodes and elements required for
your part will be displayed below.
Grade zoning
Check the boxes if you want to grade your zoning in any direction.
If you choose this option you can specify a range of cells which have a fixed
size. The remaining cells will be smoothly graded to fit the overall dimension of
the box you specified in the previous window.
Fixed size
Enter the dimension you want to use for the fixed size cells in this field.
242
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Times
Enter the number of fixed size cells you want to use in this field.
Position
Specify where you want to place the fixed size cells relative to the full
I/J/K range.
Centered - at the center of the full I/J range
Lower
- at the lower end of the I/J range
Upper
- at the upper end of the I/J range
e.g. ten fixed size cells centered :
e.g. twelve fixed size cells at the lower end :
e.g. eight fixed size cells at the upper end :
Circle
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
243
AUTODYN User Manual
Mesh Type
Select a Type 1 or Type 2 mesh for your circle.
Type 1
Type 2
The type 1 mesh is more efficient in using elements, but some elements are
not very rectangular (which can reduce the accuracy of your solution).
All the elements of a type 2 mesh are reasonably rectangular, but about a
quarter of the elements generated for this mesh are unused.
244
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Cells across radius
Enter the number of cells (elements) you want to use across the radius of your
circle in this field.
Number of elements
Displayed below the input fields is the index space that will be used for your
Part and the number of nodes and elements required.
Ogive
Mesh Type
Select a Type 1 or Type 2 mesh for your ogive.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
245
AUTODYN User Manual
Type 1
Type 2
The type 1 mesh is more efficient in using elements, but some elements are
not very rectangular (which can reduce the accuracy of your solution).
All the elements of a type 2 mesh are reasonably rectangular, but some of the
elements generated for this mesh are unused.
Cells across radius
Enter the number of cells (elements) you want to use across the radius of your
ogive in this field.
Number of elements
Displayed below the input fields is the index space that will be used for your
Part and the number of nodes and elements required.
Wedge
246
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Cells across radius
Enter the number of cells (elements) you want to use across the radius of your
wedge in this field.
Number of elements
Displayed below the first input field is the index space that will be used for your
Part and the number of nodes and elements required.
Grade zoning
Check this box if you want to grade your zoning.
If you choose this option you can specify a range of cells which have a fixed
size. The remaining cells will be smoothly graded to fit the overall dimension of
the box you specified in the previous window.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
247
AUTODYN User Manual
Increment
Enter the dimension you want to use for the fixed size cells in this field.
Times
Enter the number of fixed size cells you want to use in this field.
Rhombus
Cells across quarter
Enter the number of cells (elements) you want to generate across a quarter of
the rhombus.
Number of elements
248
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Displayed below the input field is the index space that will be used for your Part
and the number of nodes and elements required.
Quad
Cells in I/J direction
Enter the number of cells (elements) you want to use in the I and J directions in
fields provided. The corresponding number of nodes and elements required for
your part will be displayed below.
Automatic
Select this option if you want the internal nodes to be spaced equipotentially.
IJ-Straight
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
249
AUTODYN User Manual
Select this option if you want the nodes along each I and J line to be equally
spaced along a straight line
Geometric Ratios
Input geometric ratios in the fields provided if you want to grade the zoning
instead of generating equally spaced nodes.
250
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - New - Define Zoning (3D)
This window lets you Define the zoning for your 3D Part.
Box
Cells
Enter the number of cells (elements) you want to use in the I, J and K
directions in fields provided. The corresponding number of nodes and elements
required for your part will be displayed below.
Grade zoning
Check the boxes if you want to grade your zoning in any direction.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
251
AUTODYN User Manual
If you choose this option you can specify a range of cells which have a fixed
size. The remaining cells will be smoothly graded to fit the overall dimension of
the box you specified in the previous window.
Fixed size
Enter the dimension you want to use for the fixed size cells in this field.
Times
Enter the number of fixed size cells you want to use in this field.
Position
Specify where you want to place the fixed size cells relative to the full
I/J/K range.
Centered - at the center of the full I/J/K range
Lower
- at the lower end of the I/J/K range
Upper
- at the upper end of the I/J/K range
e.g. ten fixed size cells centered :
e.g. twelve fixed size cells at the lower end :
e.g. eight fixed size cells at the upper end :
Cylinder
252
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Mesh Type
Select a Type 1 or Type 2 mesh for your cylinder.
Type 1
Type 2
The type 1 mesh is more efficient in using elements, but some elements are
not very rectangular (which can reduce the accuracy of your solution).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
253
AUTODYN User Manual
All the elements of a type 2 mesh are reasonably rectangular, but about a
quarter of the elements generated for this mesh are unused.
Cells across radius
Enter the number of cells (elements) you want to use across the radius of your
cylinder in this field.
Cells along length
Enter the number of cells (elements) you want to use along the length of your
cylinder in this field.
Number of elements
Displayed below the above input fields are the index space that will be used for
your Part and the number of nodes and elements required.
Grade zoning along length
Check this box if you want to grade the zoning along the length of your cylinder
(you will be asked to specify a starting increment to use).
Ogive
254
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Mesh Type
Select a Type 1 or Type 2 mesh for your ogive.
Type 1
Type 2
The type 1 mesh is more efficient in using elements, but some elements are
not very rectangular (which can reduce the accuracy of your solution).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
255
AUTODYN User Manual
All the elements of a type 2 mesh are reasonably rectangular, but some of the
elements generated for this mesh are unused.
Cells across radius
Enter the number of cells (elements) you want to use across the radius of your
ogive in this field.
Number of elements
Displayed below the input fields is the index space that will be used for your
Part and the number of nodes and elements required.
Sphere
Mesh Type
256
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Select a Type 1 or Type 2 mesh for your sphere.
Type 1
Type 2
The type 1 mesh is more efficient in using elements, but some elements are
not very rectangular (which can reduce the accuracy of your solution).
All the elements of a type 2 mesh are reasonably rectangular, but some of the
elements generated for this mesh are unused.
Cells across radius
Enter the number of cells (elements) you want to use across the radius of your
sphere in this field.
Number of elements
Displayed below the input fields is the index space that will be used for your
Part and the number of nodes and elements required.
Hex
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
257
AUTODYN User Manual
Cells in I/J/K direction
Enter the number of cells (elements) you want to use in the I, J and K
directions in fields provided. The corresponding number of nodes and
elements required for your part will be displayed below.
Automatic
Select this option if you want the internal nodes to be spaced equipotentially.
IJK-Straight
Select this option if you want the nodes along each I, J and K line to be equally
spaced along a straight line.
Geometric Ratios
258
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Input geometric ratios in the fields provided if you want to grade the zoning
instead of generating equally spaced nodes.
Frag/Brick
Number of elements in each fragment/brick
Use these fields to set the number of elements per fragment/brick in the X, Y
and Z directions.
Fill mortar with unused?
Check this box if you do not want the mortar to be represented as a material.
If you check this box, no elements will be generated for the mortar
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
259
AUTODYN User Manual
If you do not check this box, elements will be generated for the mortar (if the
mortar thickness is small compared to the dimension of the brick elements, the
time step is likely to be reduced significantly).
260
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - New - Define Zoning (3D Shell)
This window lets you Define the zoning for your Shell Part.
Plane
Cells
Enter the number of cells (elements) you want to use in the X, Y, Z directions in
fields provided. The corresponding number of nodes and elements required for
your part will be displayed below.
Grade zoning
Check the boxes if you want to grade your zoning in any direction.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
261
AUTODYN User Manual
If you choose this option you can specify a range of cells which have a fixed
size. The remaining cells will be smoothly graded to fit the overall dimension of
the box you specified in the previous window.
Fixed size
Enter the dimension you want to use for the fixed size cells in this field.
Times
Enter the number of fixed size cells you want to use in this field.
Position
Specify where you want to place the fixed size cells relative to the full
I/J/K range.
Centered - at the center of the full I/J/K range
Lower
- at the lower end of the I/J/K range
Upper
- at the upper end of the I/J/K range
e.g. ten fixed size cells centered :
e.g. twelve fixed size cells at the lower end :
e.g. eight fixed size cells at the upper end :
Cylinder
262
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Cells about circumference
Enter the number of cells (elements) you want to use about the circumference
of your cylinder in this field.
Cells along length
Enter the number of cells (elements) you want to use along the length of your
cylinder in this field.
Number of elements
Displayed below the above two input fields is the index space that will be used
for your Part and the number of nodes and elements required.
Grade zoning along length
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
263
AUTODYN User Manual
Check this box if you want to grade the zoning along the length of your cylinder
(you will be asked to specify a starting increment to use).
264
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - New - Fill Part (2D)
This window lets you fill the part you are creating.
Fill Part
Check this box if you want the Part Wizard to fill your Part.
The Part Wizard lets you fill your entire Part with a single material and initial values.
If you want to fill your part with multiple materials or initial conditions, this can be
done by pressing the Fill button after completing the Part Wizard.
Fill with Initial Condition Set
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
265
AUTODYN User Manual
Check this box if you want to fill your Part using an Initial Condition Set.
The advantage of filling a Part using an Initial Condition Set is that if you later
change one or more parameters in the set, you do not have to refill your Part.
Use the pull-down menu to select the Initial Condition Set you want to use.
You can define new Initial Condition Sets by pressing the Init.Cond. button on the
Navigation Bar or by pressing
next to the option in this window.
Material
If you do not want to use an Initial Condition Set, select the material you want to use
to fill your Part from this Pull-down menu.
You can define new materials by pressing the Materials button on the Navigation
Bar or by pressing
next to the option in this window.
Parameters
If you do not want to use an Initial Condition Set, enter parameter values for your fill
in the fields provided (Density, Energy, Velocity).
266
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - New - Fill Part
This window lets you fill the part you are creating.
Fill Part
Check this box if you want the Part Wizard to fill your Part.
The Part Wizard lets you fill your entire Part with a single material and initial values.
If you want to fill your part with multiple materials or initial conditions, this can be
done by pressing the Fill button after completing the Part Wizard.
Fill with Initial Condition Set
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
267
AUTODYN User Manual
Check this box if you want to fill your Part using an Initial Condition Set.
The advantage of filling a Part using an Initial Condition Set is that if you later
change one or more parameters in the set, you do not have to refill your Part.
Use the pull-down menu to select the Initial Condition Set you want to use.
You can define new Initial Condition Sets by pressing the Init.Cond. button on the
Navigation Bar or by pressing
next to the option in this window.
Material
If you do not want to use an Initial Condition Set, select the material you want to use
to fill your Part from this Pull-down menu.
You can define new materials by pressing the Materials button on the Navigation
Bar or by pressing
next to the option in this window.
Parameters
If you do not want to use an Initial Condition Set, enter parameter values for your fill
in the fields provided (Density, Energy, Velocity).
Frag/Brick
268
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Enter the material data for the brick and mortar materials
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
269
AUTODYN User Manual
Parts - New - Fill Part (Shell)
This window lets you fill the shell part you are creating.
Fill Part
Check this box if you want the Part Wizard to fill your Part.
The Part Wizard lets you fill your entire Part with a single material and initial values.
If you want to fill your part with multiple materials or initial conditions, this can be
done by pressing the Fill button after completing the Part Wizard.
Fill with Initial Condition Set
Check this box if you want to fill your Part using an Initial Condition Set.
270
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
The advantage of filling a Part using an Initial Condition Set is that if you later
change one or more parameters in the set, you do not have to refill your Part.
Use the pull-down menu to select the Initial Condition Set you want to use.
You can define new Initial Condition Sets by pressing the Init.Cond. button on the
Navigation Bar or by pressing
next to the option in this window.
Material
If you do not want to use an Initial Condition Set, select the material you want to use
to fill your Part from this Pull-down menu.
You can define new materials by pressing the Materials button on the Navigation
Bar or by pressing
next to the option in this window.
Parameters
If you do not want to use an Initial Condition Set, enter parameter values for your fill
in the fields provided (Shell Thickness, Velocity).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
271
AUTODYN User Manual
Parts - Copy
This window lets you copy an existing Part to a new Part.
Part List
This box lists all the existing Parts in your model. Select the part you want to copy
from this list.
New Part Name
Enter the name of your new Part in this field.
Pressing
272
creates your new part.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Delete
This window lets you delete Parts from your model.
Select the Part(s) you want to delete and press
.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
273
AUTODYN User Manual
Parts - IJK Range
This window lets you modify the IJK range of a structured Part.
Enter new IJK ranges for the Part in the fields provided.
If you cut a range, the corresponding elements are deleted from the Part.
If you extend a range, new (unused) elements are added to the Part.
Use zero or negative indices to add I, J or K lines to the lower end of ranges.
e.g. changing the I-range above to run From I = -4 To I = 12, will add 5 I-lines at the
lower end of the Part and 3 I-lines at the upper end of the Part. The new I-range will
then run from 1 to 17 (with the original I-lines moved to I=5 through I=14)
274
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Activation
This window lets you set the activation and deactivation times for a structured Part.
Activation / Deactivation times cannot be set for unstructured Parts. The default
values ensure the Part is active for the entire calculation.
Activation Time
Enter the activation time for the Part in this field. The Part will not be computed until
this activation time is reached.
Deactivation Time
Enter the deactivation time for the Part in this field. The Part will not be computed
after this deactivation time is reached.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
275
AUTODYN User Manual
Parts - Rename
This window lets you rename a Part.
Type the new name for the Part in the field provided.
276
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Print
This window lets you set the index range of a structured Part you want to use for grid
data written to the print file (.prt) for this Part.
You can set the frequency at which this data is written (by cycle or times) in the
Output panel (press Output on the Navigation Bar).
Index Range
Specify the index range for print data for this Part in the fields provided.
Print order
Use this pull-down menu to set the order in which data will be printed.
e.g. IKJ means J will vary faster than K and K will vary faster than I.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
277
AUTODYN User Manual
Parts-Pack(Fill)
When SPH parts are selected in the parts menu, pressing the "Pack (Fill)" button
displays the following panel in the lower region of the parts menu.
This panel allows you to fill SPH objects with SPH nodes.
Pack Selected Object(s)
Press this button to pack the selected objects with SPH nodes. You will be
prompted for the fill material, the SPH node size and velocity to use for the packing
operation.
Delete All SPH
Press this button to delete all SPH nodes in your model.
Delete Nodes in Object
Press this to delete the SPH nodes in the selected SPH objects.
Delete in XY Box
Press this to delete the SPH nodes in a box defined by the XYZ coordinates of the
origin and the size of the box in the X, Y and Z directions.
Delete Single Node
Press this to delete a single SPH node, by specifying its local IJK index. You can
use the Examine option to interactively select SPH nodes, and determine their index.
278
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Zoning
Parts - Zoning
Pressing the Zoning button in the Parts panel displays the following dialog in the
lower region of the panel :
2D-Structured
3D-Structured
2D & 3D-Unstructured
This dialog lets you define the zoning (grid coordinates) for the selected Part.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
279
AUTODYN User Manual
For 2D & 3D unstructured Parts the geometry and meshing cannot be defined. The
only option for unstructured Parts is the Transformation option, like translation,
rotation or scaling.
Plot zoning
Standard plotting will only show elements that contain material, not unused
elements.
Checking this box shows all elements, including unused elements.
Zoning for IJK range:
These fields let you specify the IJK range you want zoning operations to act on. The
default values are for the entire Part.
Predef Geometries
Box
Press this button to zone a box.
Cylinder
Press this button to zone a cylinder.
Sphere
Press this button to zone a sphere.
Ogive
Press this button to zone an ogive.
Frag/Bric
Press this button to zone a fragment / brick wall.
Transition
Press this button to zone a grid transition
Import
Press this button to import zoning from an external file (.zon)
User
Press this button to generate zoning from a user subroutine.
Fill Block
Press this button to zone and fill an Euler-FCT grid using data from an external
file.
Manual Zoning
These options let you build a grid by specifying nodes and generating lines, surfaces
and 3D volumes.
280
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Press
to reveal the following buttons :
Node
Press this button to define the coordinates of a node.
Line
Press this button to generate coordinates along a line in index space.
Surface
Press this button to generate the coordinates of an index plane.
Volume
Press this button to define the coordinates within the current IJK Range.
Transformations
These options let you translate, rotate and scale your zoning.
Press
to reveal the following buttons :
Translate
Press this button to translate zoning
Rotate
Press this button to rotate zoning
Scale
Press this button to scale zoning
Operations
These options let you perform various operations on your zoning.
Press
to reveal the following buttons :
Copy
Press this button to copy zoning from an existing Part to the current Part.
Delete
Press this button to delete zoning.
Save
Press this button to temporarily save your zoning.
Restore
Press this button to restore zoning you have temporarily saved.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
281
AUTODYN User Manual
Parts - Zoning - Box
This window lets you generate a box with its axes parallel to the X, Y and Z axes.
Origin
Enter the X, Y and Z coordinates of the lower corner of the box in the fields provided.
Box Dimensions
Enter the dimensions of the box (DX, DY, DZ) in the fields provided
Grade zoning
Check the boxes if you want to grade your zoning in any direction.
If you choose this option you can specify a range of cells which have a fixed size.
The remaining cells will be smoothly graded to fit the box dimensions.
Fixed size
282
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Enter the dimension you want to use for the fixed size cells in this field.
Times
Enter the number of fixed size cells you want to use in this field.
Position
Specify where you want to place the fixed size cells relative to the full I/J/K
range.
Centered - at the center of the full I/J/K range
Lower
- at the lower end of the I/J/K range
Upper
- at the upper end of the I/J/K range
e.g. ten fixed size cells centered :
e.g. twelve fixed size cells at the lower end :
e.g. eight fixed size cells at the upper end :
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
283
AUTODYN User Manual
Parts - Zoning - Cylinder
This window lets you generate a cylinder with its axis parallel to the Z axis.
Section
Choose the section you want to generate (Whole, Half or Quarter). This should
match any symmetry planes you have defined for your model.
Solid or Hollow
Choose either a solid or hollow cylinder.
If you choose a hollow cylinder, you will have to specify inner and outer radii for the
cylinder.
Origin
Enter the X, Y and Z coordinates for the center of the starting surface of your
cylinder in the fields provided.
284
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Start Radius / End Radius
You can specify different radii for the starting and end faces of your cylinder. For a
regular cylinder (constant radius), set the starting radius equal to the end radius.
Length
Enter the length of your cylinder in this field.
Grade zoning along axis
Check this box if you want to grade the zoning along the length of your cylinder (you
will asked to specify a geometric ratio to use).
Start Surface / End surface
The starting and end surfaces of your cylinder can be flat, concave or convex.
If you select a concave or convex surface, you will have to specify its radius of
curvature.
Mesh Type
Select a Type 1 or Type 2 mesh for your cylinder.
Type 1
Type 2
The type 1 mesh is more efficient in using elements, but some elements are not very
rectangular (which can reduce the accuracy of your solution).
All the elements of a type 2 mesh are reasonably rectangular, but about a quarter of
the elements generated for this mesh are unused.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
285
AUTODYN User Manual
Parts - Zoning - Sphere
This window lets you generate a sphere.
Section
Choose the section you want to generate (Whole, Half, Quarter or Eighth). This
should match any symmetry planes you have defined for your model.
Solid or Hollow
Choose either a solid or hollow sphere.
If you choose a hollow sphere, you will have to specify inner and outer radii for the
sphere.
Origin
Enter the X, Y and Z coordinates for the center of the sphere in the fields provided.
Radius
286
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Enter the radius of the sphere in this field.
Mesh Type
Select a Type 1 or Type 2 mesh for your sphere.
Type 1
Type 2
The type 1 mesh is more efficient in using elements, but some elements are not very
rectangular (which can reduce the accuracy of your solution).
All the elements of a type 2 mesh are reasonably rectangular, but some of the
elements generated for this mesh are unused.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
287
AUTODYN User Manual
Parts - Zoning - Ogive
This window lets you generate an ogive with its axis parallel to the Z axis.
Section
Choose the section you want to generate (Whole, Half or Quarter). This should
match any symmetry planes you have defined for your model.
Solid or Hollow
Choose either a solid or hollow ogive.
If you choose a hollow ogive, you will have to specify inner and outer radii for the
ogive.
Origin
Enter the X, Y and Z coordinates for the center of your ogive in the fields provided.
End Radius
288
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Enter the end radius of your ogive in this field.
Ogive Radius
Enter your ogive radius in this field.
Mesh Type
Select a Type 1 or Type 2 mesh for your ogive.
Type 1
Type 2
The type 1 mesh is more efficient in using elements, but some elements are not very
rectangular (which can reduce the accuracy of your solution).
All the elements of a type 2 mesh are reasonably rectangular, but some of the
elements generated for this mesh are unused.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
289
AUTODYN User Manual
Parts - Zoning - Quad
Coordinates X1, Y1:
Enter coordinates of the first point of the quad.
Coordinates X2, Y2:
Enter coordinates of the second point of the quad.
Coordinates X3, Y3:
Enter coordinates of the third point of the quad.
Coordinates X4, Y4:
Enter coordinates of the fourth point of the quad.
Cells in I/J direction
290
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Enter the number of cells (elements) you want to use in the I and J directions in
fields provided. The corresponding number of nodes and elements required for
your part will be displayed below.
Automatic
Select this option if you want the internal nodes to be spaced equipotentially.
IJ-Straight
Select this option if you want the nodes along each I and J line to be equally
spaced along a straight line
Geometric Ratios
Input geometric ratios in the fields provided if you want to grade the zoning
instead of generating equally spaced nodes.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
291
AUTODYN User Manual
Parts - Zoning - Hex
Select Node to Edit
Use the arrow buttons to select each of the 8 nodes in turn.
Coordinates
Enter the X, Y and Z coordinates of the node.
Cells in I/J/K direction
Enter the number of cells (elements) you want to use in the I, J and K
directions in fields provided. The corresponding number of nodes and
elements required for your part will be displayed below.
Automatic
Select this option if you want the internal nodes to be spaced equipotentially.
IJK-Straight
292
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Select this option if you want the nodes along each I, J and K line to be equally
spaced along a straight line.
Geometric Ratios
Input geometric ratios in the fields provided if you want to grade the zoning
instead of generating equally spaced nodes.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
293
AUTODYN User Manual
Parts - Zoning - Frag/Bric (page 1)
Two dialog windows let you build a fragment or brick wall.
This first window lets you generate the zoning.
The fragment/brick wall is built with its axes parallel to the X, Y and Z axes.
The X direction runs the length of the wall.
The Y direction runs the height of the wall.
The Z direction runs through the thickness of the wall.
Number of fragments/bricks
Use these fields to set the number of fragments/bricks in the X, Y and Z directions.
Length of each fragment/brick
294
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Use these fields to set the length of a single brick/fragment in the X, Y and Z
directions.
Mortar size between each fragment/brick
Use these fields to set the mortar size (or gap) between fragments/bricks.
Mortar included in dimension?
Check this box if you want the mortar size to be included in the length of each
brick/fragment.
Number of elements in each fragment/brick
Use these fields to set the number of elements per fragment/brick in the X, Y and Z
directions.
Offset ratio
Set the offset ratio for the fragments/bricks in this field.
This is how the bricks are staggered along the length of the wall.
e.g. if the offset is 0.5 (the default), the bricks will be staggered halfway across each
other as shown in the above figure.
Fragment/brick symmetric about X=0?
Check this box if you want the wall to be symmetric about X=0.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
295
AUTODYN User Manual
Parts - Zoning - Frag/Bric (page 2)
Two dialog windows let you build a fragment or brick wall.
This second window lets you fill the wall grid with materials and initial conditions.
Fill mortar with unused?
Check this box if you do not want the mortar to be represented as a material.
If you check this box, no elements will be generated for the mortar.
If you do not check this box, elements will be generated for the mortar (If the mortar
thickness is small compared to the dimension of the brick elements, the time step is
likely to be reduced significantly).
Fill with Initial Condition Set
Check this box if you want to fill your wall Part using an Initial Condition Set.
296
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
The advantage of filling a Part using an Initial Condition Set is that if you later
change one or more parameters in the set, you do not have to refill your Part.
Use the pull-down menu to select the Initial Condition Set you want to use.
You can define new Initial Condition Sets by pressing the Init.Cond. button on the
Navigation Bar or by pressing
next to the option in this window.
Material
If you do not want to use an Initial Condition Set, select the material you want to use
to fill your Part from this Pull-down menu.
You can define new materials by pressing the Materials button on the Navigation
Bar or by pressing
next to the option in this window.
Parameters
If you do not want to use an Initial Condition Set, enter parameter values for your fill
in the fields provided (Density, Energy, Velocity).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
297
AUTODYN User Manual
Parts - Zoning - Transition
This window lets you create a transition at any surface of the block you are zoning.
Transitions along:
Specify at which of the six surfaces of the block you want your transition to be
created, by selecting and I, J or K-plane and whether it is the corresponding lower or
upper surface of the block.
Transition orientation:
Select the orientation of the transition.
Transition Types
The image above shows you the two transition types you can use, namely a 4-2
transition and a 3-1 transition. To use a particular type, the index range in the
direction of the transition orientation must be a multiple of 4 or 3 respectively.
A message will tell if a valid transition type exists for the boundary you have defined.
If more than one type is valid, you will be asked to choose the transition type you
want to use.
298
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Zoning - Node
This window lets you specify the coordinates of a single node.
Node I/J/K:
Enter the I, J and K index to select the node you want to specify coordinates for in
this field.
Old Coordinates
The current (old) coordinates of the selected node are displayed for your information.
New Coordinates
Enter the new coordinates for the selected node in these fields.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
299
AUTODYN User Manual
Parts - Zoning - Line
This window lets you generate nodes along a line in index space from its two end
points. If either of its two end nodes has not been defined, you are asked to input the
coordinates
of
the
node.
I/J/K-varies
Select the index direction of the line you want to generate. The line will be generated
across the IJK range in the selected direction.
All
Select this option if you want to generate nodes for all 12 edges of the IJK range you
have specified.
Geometric Ratios
Input geometric ratios in the fields provided if you want to grade the zoning instead of
generating equally spaced nodes.
Line
Select this option if you want to generate the nodes along a straight line.
Arc
300
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Select this option if you want to generate the nodes along the arc of a circle (you will
be asked to specify the center of the circle).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
301
AUTODYN User Manual
Parts - Zoning - Surface
This window lets you zone a surface of the IJK region you selected (i.e. an index
plane with I, J or K constant) from nodes already defined along its four edges.
I/J/K-constant
Select whether you want to zone a surface with a constant I, J or K index.
All
Select this option if you want to zone all six outer surfaces of the IJK range you
have selected.
The dialog window will then look like this:
302
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Index (not for All)
Select the I, J or K index for the surface.
I/J/K-straight (not for All)
Select one of these options if you want surface nodes to be generated along straight
I, J or K lines.
Plane
Select this option if you want surface nodes to be generated equipotentially in a
plane.
Sphere
Select this option if you want surface nodes to be generated equipotentially on the
surface of a sphere (you will be asked to specify the center of the sphere).
Geometric Ratios
Set geometric ratios in the fields provided if you want to grade the zoning instead of
equally spacing the nodes.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
303
AUTODYN User Manual
Parts - Zoning - Volume
This window lets you zone the interior volume of the IJK region you selected from
nodes already defined on its six faces.
IJ-straight
Select this option if you want to generate the interior volume so that nodes with the
same (I,J) indices lie equally spaced along a straight line
JK-straight
Select this option if you want to generate the interior volume so that nodes with the
same (J,K) indices lie equally spaced along a straight line
IK-straight
Select this option if you want to generate the interior volume so that nodes with the
same (I,K) indices lie equally spaced along a straight line
Autozone
Select this option if you want to generate the interior volume so that all nodes are
spaced equipotentially.
Geometric Ratio
304
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Enter a geometric ratio in this field if you want to grade the zoning instead of equally
spacing the nodes.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
305
AUTODYN User Manual
Parts - Zoning - Translate
This window lets you translate nodes in XYZ space.
Current IJK Range
Select this option to apply the translation to all nodes in the current IJK Range.
Selected Parts
Select this option to apply the translation to all nodes of selected Parts. A box lets
you select one or more Parts.
X/Y/Z distance
Input the X, Y and Z components of the translation in these fields.
306
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Zoning - Rotate
This window lets you rotate nodes about an axis in XYZ space.
Current IJK Range
Select this option to apply the rotation to all nodes in the current IJK Range.
Selected Parts
Select this option to apply the rotation to all nodes of selected Parts. A box lets you
select one or more Parts.
Rotation
Input the rotation angle in degrees.
X/Y/Z-axis
Specify the axis about which the nodes will be rotated.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
307
AUTODYN User Manual
Parts - Zoning - Scale
This window lets you scale nodes relative to an origin in XYZ space.
Current IJK Range
Select this option to apply the rotation to all nodes in the current IJK Range.
Selected Parts
Select this option to apply the rotation to all nodes of selected Parts. A box lets you
select one or more Parts.
Origin
Input the X, Y and Z coordinates of the origin for the scaling.
Scale Factors
Input the X, Y and Z scale factors.
308
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Zoning - Copy
This window lets you copy zoning from an existing Part to the current IJK Range
Pick part to copy
Select the Part you want copy zoning from in this box.
Lower I/J/K index
Specify the lower I, J and K indices of the block you want to copy from in these
fields.
A block starting at these lower indices will be copied to the current IJK Range.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
309
AUTODYN User Manual
Parts - Zoning - Delete
This window lets you delete the zoning in a Part.
Parts List
In the top box, select the Part in which you want to delete some zoning.
Index Range
Specify the index range of the nodes whose zoning you want to delete.
The coordinates of all nodes in the index range will be set to Undefined (the default
state).
310
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Zoning - Save
This window lets you temporarily save the zoning for one or more Parts.
This is a useful option if you are about to do some detailed zoning changes and want
to ensure you can return to your original zoning if you make a mistake.
Pressing the Restore button in the Parts-Zoning panel lets you restore the saved
zoning.
Select the Parts whose zoning you want to save and press
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
311
AUTODYN User Manual
Parts - Zoning - Restore
This window lets you restore zoning you have temporarily saved for one or more
Parts.(pressing the Save button in the Parts-Zoning panel lets you temporarily save
zoning for one or more Parts).
Select the Parts whose zoning you want to restore and press
312
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Zoning - Refine
This window lets you refine structured Lagrange, ALE, Euler-Godunov and EulerFCT parts. However, the part must satisfy the following requirements in order to
utilize this new refining facility:
The part must be a 'box' type object.
The X, Y and Z coordinates of the grid nodes must increase with the I, J and
K indices respectively.
I/J/K Factor
Enter the Refine Factor for the I/J/K index, i.e., number of the new cells created from
an original single cell in that direction.
The refining algorithms are by default applied to all cells within a part. In order to limit
the range of cells within a part that undergo refinement the user can select an
appropriate IJK-RANGE first. In addition it should be noted that the following
limitations apply to the refinement of Euler and ALE parts.
For simplicity with multi-material Euler-Godunov grids, the material volume
fraction of an original cell is assigned to all the new cells created from that
original cell. Thus the material interface on the new grid may not be exactly the
same as that on the original grid.
For ALE grids, the original motion constraint of the ALE nodes is not retained
during the refining procedure. The motion constraint for all the new nodes is set
to Lagrange, even if the constraint of the original node is, for example,
Equipotential. The user will therefore need to re-define the motion constraints for
ALE parts following the refining process.
The cell index for time history gauge points is also updated during the refinement.
Furthermore, the mass is always conserved between the original and refined parts.
However, the momentum and kinetic energy in Lagrange and ALE parts may not be
conserved exactly because the mesh refinement modifies the nodal masses and
thus affects the momentum and kinetic energy calculation. For Euler-Godunov and
Euler-FCT parts, since the cell mass is used to calculate both the kinetic energy and
momentums, refinement does not affect the calculation. The kinetic energy and
momentums should therefore always be conserved.
An example of the refinement of a Lagrangian part is shown below. Note that the
refinement factors IFACT, JFACT and KFACT have been set to 1, 2 and 3
respectively.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
313
AUTODYN User Manual
(a) Before refinement
314
(b) After refinement
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts-Zoning-Fill Block
Parts-Zoning-Fill Block
This window lets you import complicated zoning and fill information, such as a city
centre consisting of many buildings of different size. The option is only available for
Euler-FCT parts.
After browsing for an input file (extension .blk), select the format of the external data.
Implicit format – AUTODYN reads the fill flag of Euler-FCT cells in a certain
predefined sequence. The fill flags of ALL the cells in the input region must therefore
be defined in the data file.
Explicit format – AUTODYN reads the cell index together with its fill flag. Hence, only
the buildings (unused) cells and the cells with target points need to be included in the
data file.
The external file imported into AUTODYN using the Fill Block option should have the
extension .blk, for example block0.blk. Note that this file name is not necessarily the
same as the ident of the AUTODYN model that is being pre-processed.
The Fill Block command also permits extra air space to be created beyond the input
region. For example, to allow a pressure wave to propagate over the tallest building
in the model and interact with the buildings behind, Fill Block can be used to create
additional air space above the building.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
315
AUTODYN User Manual
Parts-Zoning-Fill Block-Implicit
IMPLICIT
Fill type
IMAX, JMAX, KMAX
Maximum I, J, K indices of input region
XMIN, YMIN, ZMIN
Minimum
co-ordinates
of
input
(corresponding to the node at I=J=K=1
DX, DY, DZ
X, Y, Z zone dimensions for input region
XRAT, YRAT, ZRAT
Ratios used to extend grid beyond the original input
region. For example, if XMAX is the maximum Xcoordinate of the input region and XRAT=0.5, the
generated grid would be extended to XMAX + 0.5
(XMAX-XMIN) in the X-direction, with geometric
zoning being used automatically for cells above
XMAX. The maximum I index of the part will be
larger than the IMAX defined in the data file, hence
extra elements are created to include the extended
air space
SIE
Unit-dependent specific internal energy for the air
(2.068x105 is usually OK for the mm/mg/ms units)
IFILL
Fill flag of each cell in input region (K varying faster
than J, J varying faster than I. Input 20 cells per
line of data
IFILL= 0 Fill cell with unused
IFILL= 1 Fill cell with air
IFILL= 2 Fill cell with air and target point
region
An example of a .blk file using the implicit format is shown below. Note that the IFILL
flag has to be defined for all elements in the part. The resulting filled Euler-FCT grid
is shown in Figure 2.2.1.
IMPLICIT
6 6 6
0.0000E+00
0.1000E+03
0.4400E+00
2.0680E+05
1
1
1
1
1
1
0
0
0
2
1
1
1
1
1
1
1
1
1
1
1
316
0.0000E+00
0.1000E+03
0.4400E+00
1
1
0
1
1
1
1
1
1
0
1
1
1
1
1
1
0
1
1
1
1
1
0
1
1
1
0.0000E+00
0.1000E+03
0.4400E+00
1
1
0
1
1
1
1
1
0
1
1
1
1
1
0
1
1
1
1
1
0
1
1
1
1
1
0
1
1
1
1
1
0
1
1
1
1
1
0
1
1
1
1
1
0
1
1
1
1
1
0
1
1
1
1
1
0
1
1
1
1
1
0
1
1
1
1
1
0
1
1
1
1
2
0
1
1
1
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
317
AUTODYN User Manual
Parts-Zoning-Fill Block-Explicit
EXPLICIT
Fill type
IMAX, JMAX, KMAX
Maximum I, J, K indices of input region
XMIN, YMIN, ZMIN
Minimum
co-ordinates
of
input
(corresponding to the node at I=J=K=1
DX, DY, DZ
X, Y, Z zone dimensions for input region
XRAT, YRAT, ZRAT
Ratios used to extend grid beyond the original input
region. For example, if XMAX is the maximum Xcoordinate of the input region and XRAT=0.5, the
generated grid would be extended to XMAX + 0.5
(XMAX-XMIN) in the X-direction, with geometric
zoning being used automatically for cells above
XMAX. The maximum I index of the part will be
larger than the IMAX defined in the data file, hence
extra elements are created to include the extended
air space
SIE
Unit-dependent specific internal energy for the air
(2.068x105 is usually OK for the mm/mg/ms units)
I, J, K, IFILL
I, J and K index of the cell and its fill flag. One cell
per line of input
region
IFILL = 0 Fill cell with unused
IFILL = 1 Fill cell with air (default)
IFILL = 2 Fill cell with air and target point
An example of a .blk file using the explicit format is shown below. Note that only
elements with an IFILL flag of 0 or 2 need to be defined. The default of 1 is assumed
for all other cells. The resulting filled Euler-FCT grid is shown in Figure 2.2.2.
EXPLICIT
11 11 11
0.0000E+00
0.1000E+03
0.5000E+00
2.0680E+05
6
6
2
0
6
6
3
0
6
6
4
0
6
6
5
0
6
6
6
0
6
6
7
0
6
6
8
0
318
0.0000E+00
0.1000E+03
0.5000E+00
0.0000E+00
0.1000E+03
0.5000E+00
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
6
6
9
0
6
6
10
0
6
6
11
0
5
6
2
2
5
6
3
2
5
6
4
2
5
6
6
2
5
6
7
2
5
6
8
2
5
6
9
2
5
6
10
2
5
6
11
2
END
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
319
AUTODYN User Manual
Fill
Parts - Fill
Pressing the Fill button in the Parts panel displays the following dialog in the lower
region of the panel :
Structured
Unstructured
This dialog lets you fill the selected Part with materials and initial conditions.
The only option available for unstructured parts is to fill the whole part. When an
unstructured parts only needs to be filled partially, the Group option can be used to
create a selected group of elements which then can be filled with materials or initial
conditions.
Fill by Index Space
Block
Press this button to fill a block in index space.
I/J/K Plane
Press this button to fill a plane in index space.
Node
Press this button to fill a node.
Unused
Press this button to fill a block in index space with unused elements.
Composite
Press this button to fill a composite shell.
Fill Multiple Parts
320
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Multi-Fill
Press this button to quickly fill multiple Parts.
Additional Fill Options
Datafile
Press this button to read or write a datafile for General Remapping.
Part Fill
Press this button to fill an Euler Part from using Lagrange or Fill Parts.
Block Remap
Press this button to read or write a datafile for Fast Block Remapping.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
321
AUTODYN User Manual
Parts - Fill - Block
This window lets you fill a index block within the current Part.
Select I, J and K range to Fill
Input the I, J and K range that you want to fill in the fields provided.
Fill with Initial Condition Set
Check this box if you want to fill the block using an Initial Condition Set.
The advantage of filling a Part using an Initial Condition Set is that if you later
change one or more parameters in the set, you do not have to refill your Part.
Use the pull-down menu to select the Initial Condition Set you want to use.
You can define new Initial Condition Sets by pressing the Init.Cond. button on the
Navigation Bar or by pressing
next to the option in this window.
Material
322
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
If you do not want to use an Initial Condition Set, select the material you want to use
to fill your Part from this Pull-down menu.
You can define new materials by pressing the Materials button on the Navigation
Bar or by pressing
next to the option in this window.
Parameters
If you do not want to use an Initial Condition Set, enter parameter values for your fill
in the fields provided (Density, Energy, Velocity).
Radial Velocity
Enter the radial velocity and choose between spherical or cylindrical symmetry. For
cylindrical symmetry the direction of the cylinder axis must also be specified.
Axial Velocity
Enter the axial velocity and select the origin and direction of the axis.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
323
AUTODYN User Manual
Parts - Fill - I / J / K Plane
This window lets you fill a I, J or K plane of the current Part with initial conditions.
The example shown is for filling a I plane (input for the other planes is similar).
Select range to Fill
Enter the I index for the plane you want to fill and the J and K range to fill in this
plane.
Fill with Initial Condition Set
Check this box if you want to fill the plane using an Initial Condition Set.
The advantage of filling a Part using an Initial Condition Set is that if you later
change one or more parameters in the set, you do not have to refill your Part.
Use the pull-down menu to select the Initial Condition Set you want to use.
You can define new Initial Condition Sets by pressing the Init.Cond. button on the
Navigation Bar or by pressing
324
next to the option in this window.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Material
Since you are only filling a plane, no material fill is done, only initial conditions for
nodes are set (i.e. velocities)
Parameters
If you do not want to use an Initial Condition Set, enter parameter values for your fill
in the fields provided (Velocity only).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
325
AUTODYN User Manual
Parts - Fill - Node
This window lets you fill a I, J or K plane of the current Part with initial conditions.
The example shows is for filling a I plane (input for the other planes is similar).
Select the node to Fill
Enter the I, J and K indices for the node you want to fill.
Fill with Initial Condition Set
Check this box if you want to fill the node using an Initial Condition Set.
The advantage of filling a Part using an Initial Condition Set is that if you later
change one or more parameters in the set, you do not have to refill your Part.
Use the pull-down menu to select the Initial Condition Set you want to use.
You can define new Initial Condition Sets by pressing the Init.Cond. button on the
Navigation Bar or by pressing
next to the option in this window.
Material
326
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Since you are only filling a node, no material fill is done, only initial conditions for the
node are set (i.e. velocities)
Parameters
If you do not want to use an Initial Condition Set, enter parameter values for your fill
in the fields provided (Velocity only).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
327
AUTODYN User Manual
Parts - Fill - Unused
This window lets you fill a block in index space with Unused elements (previous
materials occupying the elements are removed).
Enter the index range of the block you want to fill and press
328
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Composite
Parts - Fill - Composite
This window lets you define a shell as a composite shell, consisting of a number of
different layers. The composite allows efficient modeling of thin composite materials
which are subjected to structural, rather than shock type loading.
New
Press this button to create a new shell layer definition.
Modify
Press this button to modify an existing shell layer definition.
Delete
Press this button to delete an existing shell layer definition.
Review
Press this button to review the existing shell layer definition.
Range
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
329
AUTODYN User Manual
Enter the J and K range of the shell to apply the selected layer definition.
Velocity
Enter the initial velocity of the shell.
330
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Fill - Composite - New
This window lets you create an existing layer definition.
Number of Layers
Select the number of layers for the composite layer definition.
Layer definition name
Enter a name for the layer definition.
Material
Select the material for each material layer.
Direction
For orthotropic materials, enter a material direction in degrees.
Thickness
Enter the thickness for each material layer.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
331
AUTODYN User Manual
Parts - Fill - Composite - Modify
This window lets you modify an existing layer definition.
Number of Layers
Select the number of layers for the composite layer definition.
Layer definition name
Enter a name for the layer definition.
Material
Select the material for each material layer.
Direction
For orthotropic materials, enter a material direction in degrees.
Thickness
Enter the thickness for each material layer.
332
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Fill - Multi-Fill
This window lets you quickly fill multiple Parts. Each selected Part must be filled in its
entirety.
Fill Parts
The top box displays a list of Parts that you can select to fill.
Below this box is a pull-down menu that lets you choose the type of Parts from which
you want to make your selection (you can only fill Parts of the same type at the same
time).
Fill with Initial Condition Set
Check this box if you want to fill the Parts using an Initial Condition Set.
The advantage of filling a Part using an Initial Condition Set is that if you later
change one or more parameters in the set, you do not have to refill your Part.
Use the pull-down menu to select the Initial Condition Set you want to use.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
333
AUTODYN User Manual
You can define new Initial Condition Sets by pressing the Init.Cond. button on the
Navigation Bar or by pressing
next to the option in this window.
Material
If you do not want to use an Initial Condition Set, select the material you want to use
to fill your Part from this Pull-down menu.
You can define new materials by pressing the Materials button on the Navigation
Bar or by pressing
next to the option in this window.
Parameters
If you do not want to use an Initial Condition Set, enter parameter values for your fill
in the fields provided (Density, Energy, Velocity).
334
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Fill - Datafile
This window lets you write fill data to or from datafiles (.fil)
These data files are commonly used for remapping solutions from 1D Wedge, 2D
axysymmetric and 3D models into other 2D / 3D models. The figure below illustrates
the remap operations available in AUTODYN
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
335
AUTODYN User Manual
The AUTODYN-2D remap (data) file writing capability includes all state
variables including the stress tensor etc. You retain the existing option to only
write hydrodynamic data if you wish to keep the size of the remap files to a
minimum.
The AUTODYN-2D remap (data) file import capability allows 2D to 2D remapping of
all
state
variables
including
the
stress
tensor
etc.
The AUTODYN-3D remap (data) file import capability includes all state
variables
including
the
stress
tensor
etc.
In AUTODYN-3D an approximate remap into single material ALE and
Lagrange solvers has also been included, that is cells are filled with the
material with the largest volume fraction. If this happens to be void material
then
the
element
is
set
to
unused.
When reading remap data files, the origin of the remap can be user defined in
both AUTODYN-2D and 3D. Furthermore, in AUTODYN-3D the axis of
symmetry for the remap can be aligned with either the X(I), Y(J) or Z(K)
direction. This reduces the existing constraint that the X-axis needed to be
consistent between the 2D and 3D models whilst keeping the geometry
calculation
simple.
Note that all remap data files created in older versions of the software can still
be read into the latest version AUTODYN, although they will only contain
hydrodynamic
material
data.
336
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
The results of the remapping of the Johnson-Holmquist material model cannot
be guaranteed to be accurate when the material is damaged considerably,
since voids are artificially closed during remapping. The user should therefore
take care to check results carefully when using the Johnson-Holmquist
material model in the remapping procedure.
Write Datafile
Select this option if you want to write fill data for the current Part to a .fil file.
Read Datafile
Select this option if you want to read fill data for the current Part from a previously
written .fil file.
Filename
Enter the file name in this field (do not append .fil)
An example of a shaped charge analysis is shown in the below. The formation of the
shaped charge jet is first modeled using the multi-material Euler solver in
AUTODYN-2D, as shown below. A remap data file is created at the desired wrapup
time.
Formation of shape charge jet in AUTODYN-2D
The analysis can then be continued using AUTODYN-3D. In this example a
Lagrange part is first created and zoned in order that the part will completely enclose
the volume occupied by the shaped charge jet. At this stage the part is not filled and
all cells are left as unused. Note that it is recommended that cell sizes are chosen
such that at least 4 filled elements will exist across the radius of the shaped charge
jet. These cell sizes can be determined by examining the geometry at the wrapup
cycle of the AUTODYN-2D analysis.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
337
AUTODYN User Manual
In AUTODYN-3D the results from the 2D multi-material Euler analysis are remapped
into the empty 3D Lagrangian part. The Lagrangian cells that contain more than 50%
material following the remap are set as used cells. The profile of the Lagrangian jet
will therefore not exactly match that of the 2D case, although accuracy can be
enhanced by using the greatest level of refinement that computation time constraints
will allow. Note that the constitutive state variables and velocities for the used cells
are also remapped into the 3D analysis. An example of the tip of a shaped charge jet
following the remap procedure described above is shown below.
Lagrangian jet following remap into AUTODYN-3D
The 3D Lagrangian part can then be translated or rotated and used in several
analyses including normal and oblique impacts onto several different targets. The
following figures show an example in which a Lagrangian target has been introduced
into the analysis and the penetration of the jet into the target has been simulated.
Note that erosion models were included for both the jet and target materials.
338
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
(a)
Normal impact onto Lagrangian target in AUTODYN-3D
(a) initial configuration,(b) shape charge penetrates target
(b)
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
339
AUTODYN User Manual
Parts - Fill - Part Fill
This window lets you fill an Euler Part by mapping the materials and initial conditions
of an existing structured Lagrange or Fill Part or unstructured volume-element parts
into the Euler Part.
Select Part to fill into current Part
In this box, select the Lagrange or Fill Part you want to use to fill your current Euler
Part.
Material to be replaced
Select the material to be replaced during the fill operation (this information is only
used if Euler cells contain multiple materials).
340
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Mesh of Projectile and Target
Multi-material mesh filled with
Unstructured Part
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
341
AUTODYN User Manual
Parts - Fill - Block Remap
This window lets you write fill data to or from datafiles (.fil) for performing fast block
remaps.
The standard remapping scheme for 3D to 3D Euler-FCT is very useful in blast
modeling but in certain circumstances can take a very long time to search for the
cells in the remapping range, especially if the part size is very large, for example
more than 2 million cells.
The "fast block" remapping command maps several cells from a fine mesh of a small
space into a single cell in a relatively coarse mesh of a large space, directly without
searching for the remapping range. Thus the efficiency of the remapping process
has been improved dramatically.
The fast block remapping procedure is applicable to Euler-FCT parts only. The
scheme allows unused cells in the remapping region. However, cover fractions are
not considered in the remapping calculations so block remapping should not be
applied to any region of the part where Euler-FCT/Lagrange or Euler-FCT/Shell
coupling takes place.
Write Datafile
Select this option if you want to write fill data for the current Part to a .fil file.
Read Datafile
342
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Select this option if you want to read fill data for the current Part from a previously
written .fil file.
Filename
Enter the file name in this field (do not append .fil)
Typical steps that will be undertaken when using Block Remapping for blast
problems are as follows:
1. Load the original building data file.
2. Modify the part so it only contains a small area of the explosive and the
surrounding buildings.
3.
Refine the mesh, then remap 1D or 2D data to the refined part.
4. Save the file and start calculation.
5. At the wrapup cycle (when the explosive wave approaches the boundary of the
refined part), output the blast field to a remap file.
6. Load the original building data file again.
7. Modify the part so it contains a larger area.
8. Refine the mesh.
9. Read the remap file.
10. Save the file and continue running.
11. Repeat 5-10 as necessary.
An example of an analysis of a blast in a city centre that was performed using the
block remapping facility is shown below. The city centre is represented using an
Euler-FCT mesh with unused regions to represent buildings as shown below. Note
that the original zoning and fill operations for this model were set up using the new
block fill command.
(a) side view
(b) plan view
Layout of original Euler-FCT part representing city centre
To perform the initial expansion of the blast the central section of the grid, as shown
below in figure a, is taken and refined by a factor of 4 as shown in figure b.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
343
AUTODYN User Manual
(a) unrefined
(b) refined by factor of 4x4x4
Central section of part (Range I=21-31, J=11-21, K=1-21)
The analysis of the detonation of the spherical charge is initially performed using a
1D wedge analysis which is then remapped into the refined grid as shown below.
The expansion of the blast wave in the central region of the city is then performed
using the refined 3D Euler-FCT grid until the wave front reaches the boundaries of
the refined region as shown in figure b. At this point the results for this analysis are
written to a block remap data file named BLKRP1.
(a)
(b)
(a) initial blast remap from 1D wedge data
(b) blast wave reaches boundary of refined region
Expansion of blast in refined central region
Following the creation of the remap data file BLKRP1 the original model is
subsequently reloaded and a larger region of the Euler-FCT part is analyzed as
shown below in figure a. This section is refined by a factor of 2 in all directions to
give the resulting mesh shown in figure b.
344
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
(a) unrefined
(b) refined by factor of 2x2x2
Larger central section of part (Range I=11-41, J=6-26, K=1-41)
The results stored in file BLKRP1 are then remapped into the refined grid to give the
initial conditions for the second phase of the analysis as shown below in figure a.
The propagation of the blast wave can then continue until again the wave front
approaches the boundaries of the refined region as shown in figure b. At this stage a
further block remap data file is written named BLKRP2.
(a)
(b)
(a) initial blast remap from BLKRP1
(b) blast wave approaches boundary of refined region
Expansion of blast in large refined region
The final stage of the analysis can be performed using the full model. This model is
reloaded and the results stored in file BLKRP2 are remapped into the entire EulerFCT part to give the initial conditions for the final phase of the analysis as shown
below in figure a. The propagation of the blast wave can then be tracked though the
remainder of the city centre as shown in figure b.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
345
AUTODYN User Manual
(a)
(b)
(a) second blast remap from BLKRP2
(b) blast wave propagates through city centre
Expansion of blast in full Euler-FCT part
346
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Boundary
Parts - Boundary
Pressing the Boundary button in the Parts panel displays the following dialog in the
lower region of the panel :
Structured
Unstructured
This dialog lets you apply boundary conditions to the selected Part.
Block
Press this button to apply a boundary condition to a block in index space.
I/J/K Plane
Press this button to apply a boundary condition to a plane in index space.
Node
Press this button to apply a boundary condition to a node.
Clear
Press this button to clear previously applied boundary conditions.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
347
AUTODYN User Manual
Parts - Boundary - Block
This window lets you apply a boundary condition to a block in index space of the
current structured Part.
For an unstructured Part the boundary condition will be applied to all nodes,
elements or faces of a Part.
IJK range for boundary
Enter the IJK range of the block in the fields provided.
Boundary
Select the boundary condition you want to apply from this pull-down menu.
You can define Boundary Conditions by pressing the Boundaries button in the
Navigation Bar, or you can press
next to the pull-down menu.
348
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Boundary - I / J / K Plane
This window lets you apply a Boundary Condition to a I, J or K plane of the current
Part.
The example shown is for applying a Boundary Condition to a I plane (input for the
other planes is similar).
IJK range for boundary
Enter the I plane and the J and K range in the fields provided.
Boundary
Select the boundary condition you want to apply from this pull-down menu.
You can define Boundary Conditions by pressing the Boundaries button in the
Navigation Bar, or you can press
next to the pull-down menu.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
349
AUTODYN User Manual
Parts - Boundary - Node
This window lets you apply a Boundary Condition to a node.
IJK range for boundary
Enter the I, J and K index for the node in the fields provided.
Boundary
Select the boundary condition you want to apply from this pull-down menu.
You can define Boundary Conditions by pressing the Boundaries button in the
Navigation Bar, or you can press
next to the pull-down menu.
350
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Boundary - Clear
This window lets you clear a Boundary Condition from the current Part.
This operation does not delete the definition of the Boundary Condition, so you can
re-apply it later.
Select the boundary condition you want to clear from the pull-down menu and press
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
351
AUTODYN User Manual
Parts - Boundary - Apply Interactively
This window lets you apply a boundary condition interactively by creating a 2D
polygon in the graphics display. The boundary condition is applied to any nodes or
faces that lie within the 2D polygon.
Boundary
Select the boundary condition you want to apply from this pull-down menu.
You can define Boundary Conditions by pressing the Boundaries button in the
navigation bar, or you can press
next to the pull-down menu.
Close the window with the
button, to enter the polygon definition stage.
Select the polygon points using the Alt key together with the left mouse button. To
delete the last polygon, use the Shift button together with the left mouse button. To
complete the polygon, use the Control and left mouse button.
After completing the polygon, the selected nodes or faces are displayed. Press the
button to accept this selection, and apply the boundary condition. At any stage,
the
button may be used to cancel the process.
352
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Boundary - Clear Interactively
This window lets you clear a boundary condition interactively by creating a 2D
polygon in the graphics display. The boundary condition is removed from any nodes
or faces that lie within the 2D polygon.
Boundary
Select the boundary condition you want to clear from this pull-down menu.
Close the window with the
button, to enter the polygon definition stage.
Select the polygon using the Alt key together with the left mouse button. To delete
the last polygon point, use the Shift button together with the left mouse button. To
complete the polygon, use the Control and left mouse button.
After completing the polygon, the selected nodes or faces are displayed. Press the
button to accept this selection, and clear the boundary condition. At any stage,
the
button may be used to cancel the process.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
353
AUTODYN User Manual
Gauges
Parts - Gauges
Pressing the Gauges button in the Parts panel displays the following dialog in the
lower region of the panel :
This dialog lets you define gauge points in the current Part.
Add
Press this button to add one or more gauge points.
Move
Press this button to relocate a gauge point.
Delete
Press this button to delete one or more gauge points.
Review
Press this button to review all your gauge points in a window.
Plot gauge points
Check this box to see the location of you gauge points in the view panel.
354
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Interactive Selection
Use the mouse to interactively select Elements or Nodes where you wish to place
your gauge points by switching on Interactive Gauge points in the Gauges Panel.
The IJK indices or XYZ position of the selected element/node will be displayed, as
they are selected.
Gauges added via this method will also be cached until cleared by selecting the
Undo button, or the Gauges Panel is closed.
When adding Gauges via this method the part containing the Element or Node
selected becomes the selected Part in the Parts panel.
The interactive selection of Gauge Points is not available in examine mode, and the
panel will not be visible if this is the case.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
355
AUTODYN User Manual
Parts - Gauges - Add
This window lets you add gauges to your model.
A gauge is a location where time histories of selected variables are recorded during
a calculation.
Point / Array / Block
Select whether you want to define a single gauge (Point), a 2D array of gauges
(Array) or a 3D block of gauges (Block).
Fixed / Moving
Select whether you want the gauge(s) to be fixed in space or move with the flow (as
if imbedded in the material).
XYZ / IJK Space
Select whether you want to specify your gauge locations in real space (XYZ) or index
space (IJK)
Depending on your selections, the remaining fields will ask you to specify the (X,Y,Z)
coordinates of your gauges or the (I,J,K) indices of the elements in which your
gauges are to be placed.
356
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Gauges - Move
This window lets you relocate one gauge point.
Gauge Number
Enter the number of the gauge you want to relocate in this field (gauges are
assigned numbers in the order in which you define them).
XYZ / IJK Space
Select whether you want to specify your gauge locations in real space (XYZ) or index
space (IJK)
New Position
Enter the (X,Y,Z) coordinates or (I,J,K) indices for the new position of the gauge.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
357
AUTODYN User Manual
Parts - Gauges - Delete
This window lets you delete one or more gauges.
Enter the range of the gauge numbers you want to delete and press
358
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Gauges - Add Unstructured
This window lets you add gauges to an unstructured part.
A gauge is a location where time histories of selected variables are recorded during
a calculation.
Point/Array
Select whether you want to define a single gauge (Point) or a 2D array of gauges
(Array)
Element/Node
Select whether you want to associate gauge points with element or nodes.
Coordinates
The remaining fields will ask you to specify the (X, Y, Z) coordinates of your gauges.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
359
AUTODYN User Manual
Parts - Gauges - Move Unstructured
This window lets you relocate one gauge point.
Gauge Number
Enter the number of the gauge you want to relocate in this field (gauges are
assigned numbers in the order in which you define them).
Element/Node
Select whether you want to associate gauge points with element or nodes.
New Position
Enter the (X, Y, Z) coordinates for the new position of the gauge.
360
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Gauges - Delete Unstructured
This window lets you delete one or more gauges.
Enter the range of the gauge numbers you want to delete and press
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
361
AUTODYN User Manual
Solvers
Parts - Solvers (Structured)
Pressing the Solvers button in the Parts panel displays the following dialog for
structured Parts in the lower region of the panel :
This dialog lets change some solver settings for the current Part.
Type
Press this button to change the type of solver used.
Solution
Press this button to change the solution type associated with some solvers.
Dezone
Press this button to perform dezoning for 2D Lagrange and Euler solvers and for 3D
Lagrange, ALE and Euler solvers.
Jetting
Press this button to add the Jetting option to a 2D shell (see the Jetting Tutorial for
details).
362
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Solvers (Structured) - Type
This window lets you change the type of solver assigned to the current Part.
You can only change to a solver compatible with the current solver used for the Part.
Current solver type
This line shows you the current solver type.
New solver type
A list of the solver types compatible with the current solver type (if any), is shown.
Select the solver type you want to use from this list.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
363
AUTODYN User Manual
Parts - Solvers (Structured) - Solution (2D Shells)
This window lets you set solution options for 2D shell Parts.
Type of Solution
Select whether you want to compute a membrane solution or a solution with full
bending moments.
Shell material location
Shell segments have no geometrical thickness, so this option lets you select the
location of the shell material relative to its geometric position.
Left
Material is located to the left of the shell as you progress from the
first node to the last node.
Center Material is located equally on either side of the shell (i.e. from -h/2 to
h/2, where h is the thickness).
Right
Material is located to the right of the shell as you progress from the
first node to the last node.
364
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Solvers (Structured) - Solution (3D Shells)
This window lets you set solution options for 3D shell Parts.
Type of Solution
Select whether you want to compute a membrane solution or a solution with full
bending moments integrating over 2 or 3 sublayers.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
365
AUTODYN User Manual
Parts - Solvers (Structured) - Solutions (Beams)
This window lets you set solution options for Beam Parts.
Type of Solution
Select whether you want to compute a truss solution or a solution with full bending
moments.
Time-step safety factor
Enter the safety factor you want to apply to the time-step calculation. The default
value usually ensures stability of your calculation.
366
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Solvers (Structured) - Solution (3D Euler-FCT)
This window lets you set solution options for 3D Euler-FCT Parts.
Energy Based Velocity Limit
Specify whether or not you want to use an energy based velocity limit for Euler-FCT
computations.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
367
AUTODYN User Manual
Parts - Solvers (Structured) - Solution (2D SPH)
This window lets you set solution options for 2D SPH Parts.
Quadratic viscosity
Enter the coefficient of quadratic viscosity you want to use for SPH computations.
Linear viscosity
Enter the coefficient of linear viscosity you want to use for SPH computations.
Smoothing Length
Specify whether you want to use a constant or variable smoothing length. Using a
variable smoothing length is not recommended for most calculations.
Interface treatment
Specify if you want to use Impact/Separation calculations for the treatment of
interfaces between different SPH regions.
Density Calculation
368
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Specify whether you want to calculate densities using a continuity equation or
kernal sum method.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
369
AUTODYN User Manual
Parts - Solvers (Structured) - Solution (3D SPH)
This window lets you set solution options for 3D SPH Parts. The default settings are
the recommended settings.
Quadratic viscosity
Enter the coefficient of quadratic viscosity you want to use for SPH computations.
Linear viscosity
Enter the coefficient of linear viscosity you want to use for SPH computations.
Smoothing Length
Specify whether you want to use a constant or variable smoothing length. Using a
variable smoothing length is not recommended for most calculations.
Interface treatment
Specify if you want to use Impact/Separation calculations for the treatment of
interfaces between different SPH regions.
Density Calculation
370
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Specify whether you want to calculate densities using a continuity equation or
kernal sum method.
Work Unit Options
Work Unit Size
Enter the work unit size (as a multiple of the smoothing length) you want to use
for SPH calculations. The value you enter here can significantly affect the
efficiency of SPH calculations.
Buffer Zone Size
Enter the buffer zone size (as a multiple of the smoothing length) you want to
use for SPH calculations. The value you enter here can significantly affect the
efficiency of SPH calculations.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
371
AUTODYN User Manual
Parts - Solvers (Structured) - Dezone-(2D & 3D Euler)
This window lets you dezone a 2D or 3D Euler (Ideal gas) or Euler (Multi-material)
Part.
Dezoning involves combining a number of cells in a fine grid into single cells of a
courser grid.
I-factor
Enter the number of cells in the I direction you want to combine into a single cell.
This total number of cells in the I direction (IMAX-1) must be exactly divisible by this
number.
J-factor
Enter the number of cells in the J direction you want to combine into a single cell.
This total number of cells in the J direction (JMAX-1) must be exactly divisible by this
number.
Update grid size?
Select Yes if you want the IJ index range of the Part to be reduced automatically to
reflect the dezone. If you select No, the index range will remain unchanged, with the
higher indexed cells becoming unused.
K-factor (3D only):
Enter the number of cells in the K direction you want to combine into a single cell.
This total number of cells in the K direction (KMAX-1) must be exactly divisible by
this number.
372
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts-Solver (Structured) - Dezone (2D & 3D Lagrange/ALE)
This window lets you dezone a 2D or 3D Lagrange or ALE Part.
Dezoning involves combining a number of cells in a fine grid into single cells of a
courser grid.
I-factor
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
373
AUTODYN User Manual
Enter the number of cells in the I direction you want to combine into a single cell.
This total number of cells in the I direction (IMAX-1) must be exactly divisible by this
number.
J-factor
Enter the number of cells in the J direction you want to combine into a single cell.
This total number of cells in the J direction (JMAX-1) must be exactly divisible by
this number.
K-factor
Enter the number of cells in the K direction you want to combine into a single cell.
This total number of cells in the K direction (KMAX-1) must be exactly divisible by
this number.
Dezone Range
In these six fields, enter the range over which the dezone should be performed.
374
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Solvers (Structured) - Jetting
This window lets you set up jetting options for a 2D Shell Part.
These options let you perform shaped charge jetting analyses in which the liner is
modeled as a shell Part and the jet characteristics are computed semi-empirically.
The Jetting Tutorial describes these options in detail.
Jetting options:
The top of this window shows the shell nodes you have defined to be jetting nodes.
Stop when jetting is done?
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
375
AUTODYN User Manual
Select whether or not you want to stop the calculation once all the jetting nodes have
jetted. If you select no, the calculation will continue until the wrapup cycle or time you
have set is reached.
Define / Redefine
Press this button to set the shell nodes you want to be jetting nodes. The following
window will appear.
Enter the range of shell nodes you want to be jetting nodes.
Clear
Press this button to clear (undefine) all current jetting nodes.
376
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Solvers (Unstructured) - Solid
Pressing the Solvers button in the Parts panel displays the following dialog for
unstructured Solid Parts in the lower region of the panel :
Hex Integration
The unstructured, 8 noded, constant strain, hexahedral element is available in two
forms.
Finite volume formulation with exact volume integration (Wilkins 1974)
(Default)
Finite element formulation using approximate Gaussian quadrature
(Hallquist 1976)
The finite volume formulation is the default option and recommended for most
applications involving large deformation or warped meshes. This formulation is the
same as that used in the Structured (IJK) Lagrange solver.
The finite element formulation is included as a solver option and provides efficiency
improvements over the above. However, the accuracy of the element is reduced for
warped elements.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
377
AUTODYN User Manual
Example performance comparison for the three Hex solvers now available in
AUTODYN
Hex Hourglass Control
Hourglass control for the Unstructured Hex solvers is provided in two forms
AD standard
Flanagan-Belytschko
The "AD Standard" option is the default option and works well for most applications.
This is the most efficient option in terms of memory and speed. A default viscous
damping coefficient of 0.1 is recommended.
The "Flanagan-Belytschko" form of hourglass control is available as an option since
the AD standard form may not perform well under large rigid body rotations. The
Flanagan-Belytschko form of hourglass control is invariant under rotation hence
overcomes this problem. Both viscous and stiffness based control is available. The
default is stiffness based control with a coefficient of 0.1.
Tet Pressure Interaction
The Unstructured Tet element is available in two forms
Standard constant pressure (SCP) Tet
Average nodal pressure (ANP) Tet, (Burton 1996)
The SCP tetrahedral element is a basic, constant strain element and can be
used with all the standard AUTODYN material models including erosion.
Explosive burn logic is also available. The element is intended as a "filler"
element in meshes dominated by hexahedral elements. The element is known
to exhibit locking behavior under both bending and constant volumetric
straining (i.e. plastic flow). If possible the element should therefore not be used
in such cases.
The ANP tetrahedral element is an extension of the advanced tetrahedral
element (Burton 1996) and can be used as a majority element in the mesh.
The ANP tetrahedral overcomes problems of volumetric locking, which occur
with the SCP tetrahedral element. However, the ANP tetrahedral element is
still susceptible to shear locking in bending dominated problems. You should
therefore be careful to verify their results in such cases.
For meshes containing a majority of tetrahedral elements, the ANP option is
recommended.
378
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Material Modeling Options Available with ANP-Tet Elements
Equations of State
Linear
Polynomial
Shock
Porous
Compaction
P alpha
Rigid
Hyperelastic
Strength Models
Elastic
Viscoelastic
Von Mises
Johnson Cook
Piecewise JC
Zerilli Armstrong
Steinberg Guinan
Drucker-Prager
Johnson-Holmquist
RHT Concrete
MO Granular
Hyperelastic
Failure Models
Hydro (Pmin)
Plastic Strain
Principal Stress
Principal Stress
Principal Stress/
Johnson-Holmquist
RHT Concrete
Grady Spall Model
Johnson Cook
Crack Softening
Parts containing ANP tetrahedral elements should only be filled with a single
material. Multiple materials can be represented in a single body by creating
multiple parts and joining them together.
Note that a hexahedral mesh will generally provide more efficient results than a
tetrahedral mesh hence we only recommend the use of predominantly
tetrahedral mesh models for convenience of mesh generation.
Comparison of SCP and ANP Tet Elements for an impact (Taylor test) involving large amounts
of plastic deformation. The ANP-Tet fives results comparable with experiments.
1) Burton A.J., "Explicit, Large Strain, Dynamic Finite Element Analysis with Applications to
Human Body Impact Problems", PhD Thesis, University of Wales, December 1996.
2) Bonet J, Burton A.J. "A simple averaged nodal pressure tetrahedral element for
incompressible and nearly incompressible dynamic explicit applications". Communications in
Numerical Methods in Engineering 1998; 14, 437-449.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
379
AUTODYN User Manual
Parts - Solvers (Unstructured) - Shell
Number of sublayers
Specify the number of through thickness integration points for an isotropic shell. The
default of 3 is suitable for many applications however this number can be increased
if better resolution of through thickness plastic deformation/flow is required.
The following advanced options are also available. Note these are not intended for
general use.
Shear correction factor
The transverse shear in the element formulation is taken as constant over the
thickness. The correction factor accounts for the replacement of the true parabolic
variation through the thickness by a uniform transverse shear stress. We do not
recommend that you change the default value.
BCW warp correction
The Belytschko-Lin-Tsay element formulation becomes inaccurate if the elements
are warped. To overcome this short-coming, the element formulation has a
correction for the element warp included. We recommend that this correction is
turned on.
Thickness Update
380
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
By default the thickness of a shell element is stored and updated at the nodes of the
element. An alternative, slightly more efficient, option to store and update the
thickness at the element is also provided.
Inertia Update
The principal axes of rotary inertia for shell elements are by default re-calculated
each cycle. Alternatively there is an option to rotate the axes, rather than recompute each cycle. This later option is more efficient however can lead to
instabilities, especially in single precision.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
381
AUTODYN User Manual
Parts - Solvers (Unstructured) - Beam
Solution type
The response of a beam element to an applied load includes, by default, the effects
of bending moments. This option lets you reduce the beam formulation to that of a
truss, in which only axial and torsional effects are considered.
Timestep safety factor
Beam elements require a timestep safety factor that is less than the standard global
factor defined under Controls, Timestep. A default value of 0.5 is used and should
work for most applications. If problems are encountered with the stability of the
beam elements, reducing this factor down to 0.1 is acceptable.
Volume element reinforcement
This option allows reinforcing bars, modeled with beam elements to be tied (bonded)
to the volume of a solid element, without the restriction that the nodes of the beams
and volume elements initially need to reside at the same physical location. The
bonded beam nodes are constrained to stay at the same initial parametric location
within the volume element during element deformation. Typical applications involve
reinforced concrete or reinforced rubber structures like tires and hoses.
At start-up, AUTODYN will determine the parametric positions of all nodes of beam
Parts, selected as reinforcement (Parts, Solver), within volume elements (hex, tet,
penta) in the model. The nodes are tied to the parametric co-ordinate of the volume
element until the element erodes.
382
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
On erosion of the volume element, the beam node bonding constraint is removed
and becomes a free beam node.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
383
AUTODYN User Manual
Motions
Parts - Motions
Pressing the Motions button in the Parts panel displays the following dialog in the
lower region of the panel for structured Parts:
This dialog lets you apply motion constraints to an ALE Part.
Block
Press this button to apply motion constraints to an IJK block of nodes.
I/J/K Plane
Press this button to apply motion constraints to an II, J or K plane of nodes.
Node
Press this button to apply a motion constraint to a single node.
Modify (ALE Settings)
Press this button to change various ALE settings.
Select motion for plotting
Select the motion constraint you want to plot in this scrolling box. All nodes with the
selected motion constraint will be highlighted in the plot.
384
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Motions - Block
This window lets you apply an ALE motion constraint to a block of nodes in IJK
space.
Select Block
Enter the IJK range for the block to which you want to apply the motion constraint in
the fields provided.
Select motion
Select the motion constraint you want to apply from the list provided.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
385
AUTODYN User Manual
Parts - Motions - I / J / K Plane
This window lets you apply an ALE motion constraint to a plane of nodes in IJK
space.
The example shown is for applying a motion constraint to an I plane (input for the
other planes is similar).
Select Plane
Enter the I index for the plane and the (J,K) range for the nodes to which you want to
apply the motion constraint in the fields provided.
Select motion
Select the motion constraint you want to apply from the list provided.
386
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Motions - Node
This window lets you apply an ALE motion constraint to a node in IJK space.
Select Node
Enter the (I,J,K) indices for the node to which you want to apply the motion constraint
in the fields provided.
Select motion
Select the motion constraint you want to apply from the list provided.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
387
AUTODYN User Manual
Parts - Motions - Modify
This window lets you change ALE settings.
Spacing
Enter the geometric ratios for spacing of I, J and K lines in the fields provided. These
are only used for certain motion constraints.
Frequency
Cycle Frequency
Enter how often (in cycles) you want ALE rezoning to be performed.
Iterations per cycle
Enter how many iterations you want the ALE solver to perform in converging to
the spacing you have requested. This is used for all motion constraints except
Fixed (Euler).
Relaxation coefficient
Enter the relaxation coefficient you want to use for the ALE rezoning.
A value of 1.0 will move each node exactly to the location required for its
motion constraint.
A value of 0.5 will move each node 50% of the distance towards the location
required for its motion constraint.
388
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Geometry
Parts-Geometry - SPH
When SPH parts are selected in the parts menu, pressing the "Geometry (Zoning)"
button displays the following panel in the lower region of the parts menu.
This panel allows you to define the geometry for SPH objects.
Select Object(s)
All defined SPH objects are shown in the Select Object(s) list. Select a single object
to Modify, Copy or Delete, or select one or more objects to Transform.
Create/Modify Predef Objects
New
Press this button to define a new SPH object.
Modify
Press this button to modify an existing SPH object. This button is only active if
a single SPH object is selected. You cannot modify objects created by
conversion from a part (using the import objects - part button).
Copy
Press this button to create a copy of the selected SPH object. This button is
only active is a single SPH object is selected.
Delete
Press this button to delete the selected SPH object. This button is only active
if a single SPH object is selected
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
389
AUTODYN User Manual
Import Objects
Part
Press this button to covert an existing part (structured or unstructured) into an
SPH object. This operation is useful for creating complex SPH objects.
Transformations
Translate
Press this button to translate the currently selected objects.
Rotate
Press this button to rotate the currently selected objects.
390
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts - Geometry - New/Modify
There are three types of Geometry Predef objects you can use - Box, Cylinder and
Sphere. These are described below.
Box
Define the box by entering the XYZ coordinates of the origin, and the size in each of
its three directions. The orientation of the box is defined by a principal direction
vector and a rotation about this vector. When the box is defined, a wire-frame
representation is shown on the screen, together with an arrow displaying the
principal vector direction.
Cylinder
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
391
AUTODYN User Manual
You may define either a whole, half or quarter cylinder by selecting the appropriate
option. To define the cylinder, first enter the XYZ coordinates of the start of the
cylinder axis. You are then prompted for the start and end radius of the cylinder. If
you wish to define a hollow cylinder, enter inner radii for the start and end of the
cylinder. Otherwise, to define a solid cylinder leave these two values as zero.
You may also define a cylinder, which is elliptical in cross-section. To do this you
must provide extra radii information. This is indicated on the figure on the left hand
side of the window.
The orientation of the cylinder is defined by a principal direction vector, which
corresponds to the axis of the cylinder and a rotation about this vector. When the
cylinder is defined, a wire-frame representation is shown on the screen, together with
an arrow displaying the principal vector direction.
Sphere
392
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
You may define either a whole, half, quarter or eighth sphere by selecting the
appropriate option. To define the sphere, enter XYZ coordinates of the sphere origin
and an outer radius. You may specify a hollow sphere by entering an inner radius.
The orientation of the sphere is defined by a principal direction vector and a rotation
about this vector. When the sphere is defined, a wire-frame representation is shown
on the screen, together with an arrow displaying the principal vector direction.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
393
AUTODYN User Manual
Parts-Geometry-Copy
This window lets you create a copy of the currently selected SPH object. Enter the
name of the new SPH object, and also an offset in the X, Y and Z direction.
394
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts-Geometry-Import Part
The parts list contains all structured Lagrange or unstructured volume parts in your
model. Select one or more of these parts to create an object that can then be
packed with SPH particles. You must enter a name for the new object to be created.
The images below show an example of a model with a projectile impacting a target.
The target modeled with tetrahedral volume elements in the first image has been
converted to an SPH object and packed with SPH nodes. This is shown in the
second image.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
395
AUTODYN User Manual
396
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
397
AUTODYN User Manual
Parts-Geometry-Translate
Enter the distance in the X, Y and Z direction to translate the currently selected part
or parts.
398
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parts-Geometry-Rotate
Specify the angle (in degrees) defining the rotation about the selected axis (either X,
Y or Z).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
399
AUTODYN User Manual
Components
Components
A Component is a group of structured and unstructured Parts to which you can
collectively apply operations.
This panel lets you define Components and use them to perform various operations.
Component List
The top box displays a list of the Components you have defined. You can select a
Component in this list.
New
Press this button to create a new Component.
Modify
Press this button to modify an existing Component.
Delete
Press this button to delete a Component.
400
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Review
Press this button to review existing Components.
Fill
Material
Press this button to fill all Parts of the selected Component with a material.
Velocity
Press this button to assign a velocity to all Parts of the selected Component.
Initial Conditions
Press this button to assign initial conditions to all Parts of the selected
Component.
Boundary
Apply Boundary
Press this button to apply a boundary condition to the selected Component.
Clear Boundary
Press this button to clear a boundary condition from the selected Component
with a material.
Transformations
Translate
Press this button to translate all Parts of the selected Component.
Rotate
Press this button to rotate all Parts of the selected Component.
Scale
Press this button to scale all Parts of the selected Component.
Operations
Copy
Press this button to copy the selected Component.
Note that unstructured Parts cannot be copied.
Delete
Press this button delete all Parts of the selected Component.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
401
AUTODYN User Manual
Components - New
This window lets you create a new Component.
Name
Enter the name of your Component in this field.
All Parts
This box initially shows a list of all the Parts in your model. You can select one or
more Parts in this list.
Component Parts
This box (initially empty) shows a list of the Parts you have chosen for your
Component.
Add
402
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Select one or more Parts in the left box and press this button to add the selected
Parts to your Component.
The Parts will be removed from the list in the left box and added to the list in the right
box, as shown in the following example:
Remove
Select one or more Parts in the right box and press this button to remove the
selected Parts to your Component.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
403
AUTODYN User Manual
Components - Modify
This window lets you modify a Component.
Name
Change the name of your Component in this field.
All Parts
This box shows a list of all the Parts in your model not currently in your Component.
You can select one or more Parts in this list.
Component Parts
This box shows a list of the Parts you have chosen for your Component. You can
select one or more Parts in this list.
Add
404
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Select one or more Parts in the left box and press this button to add the selected
Parts to your Component. The Parts will be removed from the list in the left box and
added to the list in the right box.
Remove
Select one or more Parts in the right box and press this button to remove the
selected Parts to your Component. The Parts will be removed from the list in the
right box and added to the list in the left box.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
405
AUTODYN User Manual
Components - Delete
This window lets you delete one or more components.
Select the components you want to delete in the list and press
406
.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Components - Material
This window lets you fill all Parts of the selected Component with a material.
Material
Select the material you want to use to fill your Component from this Pull-down menu.
You can define new materials by pressing the Materials button on the Navigation
Bar or by pressing
next to the option in this window.
Material Parameters
Enter material parameter values for your fill in the fields provided (Density, Energy).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
407
AUTODYN User Manual
Components - Velocity
This window lets you assign a velocity to all Parts of the selected Component.
Enter the velocity components in the fields provided and press
408
.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Components - Initial Conditions
This window lets you assign initial conditions from an Initial Condition Set to all Parts
of the selected Component.
Fill with Initial Condition Set
Check this box to fill the Component using an Initial Condition Set.
The advantage of filling Parts using an Initial Condition Set is that if you later change
one or more parameters in the set, you do not have to refill your Part.
Use the pull-down menu to select the Initial Condition Set you want to use.
You can define new Initial Condition Sets by pressing the Init.Cond. button on the
Navigation Bar or by pressing
next to the option in this window.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
409
AUTODYN User Manual
Components - Apply Boundary
This window lets you apply a boundary condition to a Component.
Boundary
Select the boundary condition you want to apply from this pull-down menu.
You can define Boundary Conditions by pressing the Boundaries button in the
Navigation bar, or you can press
next to the pull-down menu.
410
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Components - Clear Boundary
This window lets you clear a Boundary Condition from the current Component.
This operation does not delete the definition of the Boundary Condition, so you can
re-apply it later.
Select the boundary condition you want to clear from the pull-down menu and press
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
411
AUTODYN User Manual
Components - Translate
This window lets you translate all Parts of the selected Component in XYZ space.
X/Y/Z distance
Input the X, Y and Z components of the translation in these fields.
412
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Components - Rotate
This window lets you rotate all Parts of the selected Component about an axis in
XYZ space.
Rotation
Input the rotation angle in degrees.
X/Y/Z-axis
Use this pull-down menu to specify the axis about which the Component will be
rotated.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
413
AUTODYN User Manual
Components - Scale
This window lets you scale all Parts of the selected Component in XYZ space.
Origin
Input the X, Y and Z coordinates of the origin for the scaling.
Scale Factors
Input the X, Y and Z scale factors.
414
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Components - Copy
This window lets you copy the selected Component to a new Component.
During the copy operation a new copy of each structured part in the Component is
generated.
Unstructured Parts cannot be copied and therefore will not be present in the copy of
the Component.
Enter your name for the new Component and press
.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
415
AUTODYN User Manual
Groups
Groups
Introduction
The Group option allows the user to group an arbitrary (independent of Part and
Component) selection of nodes faces or elements on which operations can
subsequently be performed.
An interactive method of selecting groups of nodes, faces or elements is available.
The selection is made by drawing a 2D polygon on the screen around the region of
interest, as shown in the figure below.
416
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Any nodes, faces or elements that are enclosed by the polygon are highlighted, and
the user is prompted to accept the selection of nodes or faces. These are then
added to the current group.
For face groups, an alternative surface selection method exists. The selection is
made by interactively picking a face element in the graphics window. Any faces that
are joined to the selected face and have a normal angle between the two faces of
less than a user specified value are then added to the group.
For example, selecting an element on the side of a cube would add all faces on that
side of the cube. By setting the surface angle cut-off to a sufficiently large value,
curved surfaces may also be selected, as shown in the example below, where the
curved surface of the projectile has been added to a group.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
417
AUTODYN User Manual
Once a group is defined, a number of operations can be performed, depending on
the type of group.
Groups
418
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
A Group is a selection of nodes, faces or elements to which you can perform
operations, such as applying boundaries, filling.
This panel lets you define Groups and use them to perform various operations.
Group List
The top box displays a list of the Groups you have defined, together with their type
(node, face or element) and the group size. You can select a Group in this list.
New
Press this button to create a new Group.
Rename
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
419
AUTODYN User Manual
Press this button to rename an existing Group.
Delete
Press this button to delete a Group
Review
Press this button to review existing Groups.
Groups Definition
Polygon Add
Press this button to interactively define a polygon; any nodes, faces or
elements that lie within the 2D polygon are added to the selected Group.
Select the polygon points using the Alt key together with the left mouse button.
To delete the last polygon point, use the Shift button together with the left
mouse button. To complete the polygon, use the Control and left mouse
button.
After completing the polygon, the selected nodes or faces are displayed. Press
the
button to accept this selection, and add to the current Group. At any
stage, the
button may be used to cancel the process.
Note that the Polygon Add option is not available (greyed-out) when you have
zoomed into the model using the rubber-band option using <Ctrl>+Left mouse
button.
To be able to use the Polygon Add option you should use the zoom option,
available from the Tool Bar of AUTODYN.
Polygon Remove
Press this button to interactively define a polygon; any nodes, faces or
elements that lie within the 2D polygon are removed from the selected Group.
Select the polygon points using the Alt key together with the left mouse button.
To delete the last polygon point, use the Shift button together with the left
mouse button. To complete the polygon, use the Control and left mouse
button.
After completing the polygon, the selected nodes or faces are displayed. Press
the
button to accept this selection, and add to the current Group. At any
stage, the
button may be used to cancel the process.
Note that the Polygon Remove option is not available (greyed-out) when you
have zoomed into the model using the rubber-band zoom option using
<Ctrl>+Left mouse button.
420
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
To be able to use the Polygon Remove option you should use the zoom option,
available from the Tool Bar of AUTODYN.
Surface Add
Press this button to choose a surface and add its nodes, faces or elements to
the selected Group.
Select a face using Alt and the left mouse button. Any faces that are joined to
the selected face and have a normal angle between the two faces of less than
a value you specify are then added to the group. For example, selecting an
element on the side of a cube would add all faces on that side of the cube. By
setting the surface angle cut-off to a sufficiently large value, curved surfaces
may also be selected.
After selecting a face, the corresponding surface is highlighted in the graphics
window. Press the
button to accept this selection or continue adding
further surfaces with the Alt and left mouse button. At any stage, the
button may be used to cancel the process.
Surface Remove
Press this button to choose a surface and remove its nodes, faces or elements
to the selected Group.
Select a face using Alt and the left mouse button. Any faces that are joined to
the selected face and have a normal angle between the two faces of less than
a value you specify are then removed from the group. For example, selecting
an element on the side of a cube would remove all faces on that side of the
cube. By setting the surface angle cut-off to a sufficiently large value, curved
surfaces may also be selected.
After selecting a face, the corresponding surface is highlighted in the graphics
window. Press the
button to accept this selection, or continue removing
further surfaces with the Alt and left mouse button. At any stage, the
button may be used to cancel the process.
Surface Angle Cut-Off
Enter a cut-off angle (in degrees). Only faces with an angle between the
normal and a neighbor face's normal of less than this value will be included in a
surface selection.
Apply Boundary to Group
Apply
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
421
AUTODYN User Manual
Press this button to apply a boundary condition to a node or face Group.
Clear
Press this button to remove a boundary condition from a node or face Group.
Fill Element Group
Material
Press this button to fill the selected element Group with a material.
Velocity
Press this button to assign a velocity to the selected element Group.
Initial Conditions
Press this button to assign initial conditions to the selected element Groups.
Transform group zoning
Translate
Press this button to rotate the current group
Rotate
Press this button to rotate the current group
Scale
Press this button to scale the current group
Group Operations
Four operations are available for element groups.
Delete Elements
422
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Use this option to delete all elements within a selected Group. Select the Group
containing the elements to delete and select OK. The elements will be deleted from
the model.
Define Element Group
Delete Elements in Group
Example use of Delete Elements Group Operation
Split Nodes
Use this option to split nodes across material boundaries within a selected group.
AUTODYN will search through all elements in the selected group and identify nodes
that are connected to elements (through the connectivity table) with different
materials. Each node connected to more than one material will be replicated by the
number of connected materials, while retaining the same physical location. The
connectivity of each associated element will be updated.
The option is useful for generating a sliding interface between two materials and
enforcing a conforming mesh (coincident nodes) between the material interface at
the start of the simulation.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
423
AUTODYN User Manual
Form Multi-body Part in Design Modeler
Generate Conformal Mesh in Meshing
(with single node at material interface)
Create Element Group in AUTODYN.
Split nodes across material interface.
Nodes are duplicated at material interface to
allow sliding contact.
Example use of Split nodes to create conformal sliding interface
Merge Nodes
424
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Use this option to merge coincident (joined) unstructured nodes into a single
unstructured node. This option is similar to using the "Merged joined nodes" option
on the Join panel; with this option only the nodes that are part of the node group will
be merged.
This option will increase the robustness in many applications involving joins.
Create Node Group in AUTODYN.
Merge duplicate nodes.
Duplicate nodes are merged into single nodes.
Example use of Merge nodes to remove joins.
Reverse Shell Normals
Use this option to reverse the shell element normal of a selected group of shell
elements.
This option has to be used when not all element normals of a shell part point in the
same direction and Euler-Lagrange coupling is used with thickened shells.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
425
AUTODYN User Manual
Single part with normals differently directed
Thickened shell provides incorrect coupling
surface
Create element group in AUTODYN Reverse
normals
Thickened shell provides correct coupling
surface
426
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Groups - New
This window lets you create a Group
Group Name
Enter the Group name in this field
Group Type
Select either a node, face or element Group type.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
427
AUTODYN User Manual
Groups - Rename
This window lets you rename an existing Group.
Group Name
Enter the new Group name in this field.
428
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Groups - Copy
This window lets you create a copy of an existing Group.
Group List
Select the Group that you wish to duplicate
Group Name
Enter the new name for the copied Group
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
429
AUTODYN User Manual
Groups - Delete
This window lets you delete one or more Groups.
Select the Groups you want to delete in the list and press
430
.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Groups - Apply
This window lets you apply a boundary condition to a Group. The type of Group and
type of boundary condition must be consistent, i.e. you can only apply a nodal
boundary condition to a node Group, and a face boundary condition to a face Group.
Group List
Select the Group you wish to apply the boundary condition to.
Boundary
Select the boundary condition to be applied to the Group.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
431
AUTODYN User Manual
Groups - Clear
This window lets you clear a boundary condition to a Group. The type of Group and
type of boundary condition must be consistent, i.e. you can only clear a nodal
boundary condition from a node Group, and a face boundary condition from a face
Group.
Group List
Select the Group you wish to clear from the boundary condition to.
Boundary
Select the boundary condition to be cleared from the Group.
432
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Groups - Material
This window lets you fill the selected element Group with a material.
Material
Select the material you want to use to fill your Group from this Pull-down menu.
You can define new materials by press the Materials button on the Navigation Bar or
by pressing
next to the option in this window.
Material Parameters
Enter material parameter values for your fill in the fields provided (Density, Energy).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
433
AUTODYN User Manual
Groups-Velocity
This window lets you assign a velocity to the selected element Group.
Enter the velocity components in the fields provided and press
434
.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Groups - Initial Condition
This window lets you assign initial conditions from an Initial Condition Set to the
selected element Group.
Fill with Initial Condition Set
Check this box to fill the Group using an Initial Condition Set.
The advantage of filling using an Initial Condition Set is that if you later change one
or more parameters in the set, you do not have to refill.
Use the pull-down menu to select the Initial Condition Set you want to use.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
435
AUTODYN User Manual
You can define new Initial Condition Sets by pressing the Init.Cond. button on the
Navigation Bar or by pressing
436
next to the option in this window.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Groups-Translate
This window lets you translate all nodes associated with the current group in XYZ
space.
X/Y/Z distance
Input the X, Y and Z components of the translation in these fields.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
437
AUTODYN User Manual
Groups-Rotate
This window lets you rotate all nodes associated with the current group about an axis
in XYZ space.
Rotation
Input the rotation angle in degrees.
X/Y/Z-axis
Specify the axis about which the nodes will be rotated.
438
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Groups-Scale
This window lets you scale all nodes associated with the current group relative to an
origin in XYZ space.
Origin
Input the X, Y and Z coordinates of the origin for the scaling.
Scale Factors
Input the X, Y and Z scale factors.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
439
AUTODYN User Manual
Joins
Joins
440
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
2D Window
3D Window
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
441
AUTODYN User Manual
This panel lets you join Parts of your model.
If two Parts are joined, AUTODYN automatically finds and joins all coincident nodes
in the two parts.
When unstructured Parts are joined the coincident nodes can be merged into a
single unstructured node. This option will increase the robustness in many
applications involving joins.
Using the Bonded Face Connections option allows the nodes of an unstructured Part
to be bonded to a face of another unstructured Part. Bonded contact alleviates the
requirement that for joining purposes two nodes need to reside at the same physical
location. The nodes that are to be bonded to a face may have an offset with respect
to the face and the offset is a user-defined maximum physical normal distance of a
node from a face which can be bonded together.
Join
Press this button to join Parts.
Join All
Press this button to join all Parts.
Unjoin
Press this button to unjoin Parts.
Unjoin All
Press this button to unjoin all Parts.
Matrix
Press this button to defined join Parts using a matrix.
Review
Press this button to review which Parts are currently joined.
Join tolerance
Enter the tolerance you want AUTODYN to use in determining which nodes should
be joined. Press the Set button to set this tolerance.
The default value for the join tolerance will take care of small round-off differences in
node location and will give good results. The tolerance should not artificially be
increased to try to join nodes with a clear offset with respect to each other.
Merge joined nodes
442
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Select this option to merge joined unstructured nodes into a single unstructured
node.
Plot Joined Nodes
Check this box to plot a symbol at every joined node.
Plot Joined Parts
Check this box to show which Parts are joined to a selected Part (a box appears to
let you select a Part).
Remove joined faces from plot
Selecting this option results in continuous contours across joined faces and also
removed joined faces from other types of plots.
Improved Rendering Across Joined Nodes
There is now an option to remove joined faces from rendered images under the
Joins, Settings option. Selecting this option results in continuous contours across
joined faces and also removed joined faces from other types of plots.
Contour plot including joined faces
Contour plot with "remove joined faces" set
Material plot using opacity
Material plot using opacity with "remove
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
443
AUTODYN User Manual
joined faces" set.
Bonded Face Connections
Bonded contact allows the nodes of an unstructured Part to be bonded to a face of
another unstructured Part. Bonded contact alleviates the requirement that for joining
purposes two nodes need to reside at the same physical location. The nodes that
are to be bonded to a face may have an offset with respect to the face and the offset
is a user-defined maximum physical normal distance of a node from a face which
can be bonded together.
Bonded face connections can fail and break upon a user-defined stress criterion.
Spot Welds
Spot welds generated in an ANSYS Explicit Dynamics systems are transferred to the
AUTODYN system as beam elements filled with a rigid material.
Spot welds utilise the multi-body rigid material option where each spot weld acts as
an individual rigid boy.
Spot welds can be defined as breakable by force:
Normal force limit: maximum normal force that can be sustained by the weld
Shear force limit: maximum shear force that can be sustained by the weld.
Failure of the spot weld occurs when:
where f and f are normal and shear interface forces, S and S are the maximum
allowed normal and shear force limits and expn and exps are user defined
exponential coefficients. The normal interface force f is nonzero for tensile values
only.
Note that spot welds cannot be generated directly inside an AUTODYN system. Spot
welds should be defined in an ANSYS Explicit Dynamics system and automatically
transferred to a linked AYTODYN system.
For each spot weld connections a multiple beam rigid body is automatically
generated for each spot weld in the ANSYS Explicit Dynamics system in order to
guarantee the transfer of bending over the spot weld.
444
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
After failure of the spot weld the spot weld rigid body will be removed from the
analysis model as can be seen above.
Within an ANSYS Explicit Dynamics system an effective area can be input for spot
welds, thus the breakable criteria can be defined in terms of stress. This stress is
converted to force when transferred into AUTODYN.
Spot welds of zero length are permitted. However, if such spot welds are defined as
breakable the above failure is modified since local normal and shear directions
cannot be defined. A modified criterion using global forces is used instead:
where dfx, dfy and dfz are the global force differences across the spot weld.
Notes:
1. A spot weld is equivalent to a rigid body and as such multiple nodal boundary
conditions cannot be applied to spot welds.
2. Currently analysis models containing spot welds cannot be run in parallel.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
445
AUTODYN User Manual
Joins - Join
This window lets you join Parts.
This method of joining Parts works well no matter how many Parts you have in your
model.
If you only have a few Parts, you may prefer to use a Matrix to choose the Parts you
want to join.
Select Part(s)
This box lists all the Parts in your model. Select one or more Parts in this list.
Select Part(s) to join to the above list
This box also lists all the Parts in your model. Select one or more Parts in this list.
Apply
446
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Press this button to join all Parts selected in the top window with all Parts selected in
the lower window.
You can apply the above procedure as many times as you wish without exiting this
window. Every time you press Apply, the specified Parts are joined.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
447
AUTODYN User Manual
Joins - Unjoin
This window lets you unjoin Parts.
This method of unjoining Parts works well no matter how many Parts you have in
your model.
If you only have a few Parts, you may prefer to use a Matrix to choose the Parts you
join (or unjoin)
Select Part(s)
This box lists all the Parts in your model. Select one or more Parts in this list.
Select Part(s) to unjoin to the above list
This box also lists all the Parts in your model. Select one or more Parts in this list.
Press
to unjoin all Parts selected in the top window with all Parts selected in the
lower window.
448
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Joins - Matrix
This window lets you choose the Parts you want to join by checking boxes in a
matrix.
If you have a large number of Parts, you may find it easy to join / unjoin Parts using
the Join / Unjoin options in the Joins dialog panel.
The matrix shown in this panel list the Parts of your model vertically and horizontally.
This matrix is symmetrical, so only the diagonal and lower part of the matrix is
shown.
Check a box to join the two associated Parts.
The Remove buttons let you quickly uncheck the boxes for each row of the matrix.
Press
to apply the changes you make to the matrix.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
449
AUTODYN User Manual
Merge Joined Nodes
The option of merging joined unstructured
nodes will merge the (multiple) joined nodes
that reside at the same physical location in
the model into one single unstructured
node.
Since trajectory contact does not allow the
use of joined unstructured nodes in the
contact, the merge option can be used to
remove joins from the model. Bonded
connections are recommended over node to
node joins for unstructured models.
450
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Bonded Face Connections
Bonded contact allows the nodes of an unstructured Part to be bonded to a face of
another unstructured Part. Bonded contact alleviates the requirement that for joining
purposes two nodes need to reside at the same physical location. The nodes that
are to be bonded to a face may have an offset with respect to the face and the offset
is a user-defined maximum physical normal distance of a node from a face which
can be bonded together.
During the analysis the nodes are kept at the same relative position on the face to
which they are bonded.
Bonds are allowed to fail and break upon a user-defined criterion.
Name
Enter a name for the bonded face connection set.
Maximum Offset
The automatic search algorithm for bonded regions will bond a node to the first face
found within the specified offset distance. To ensure nodes are bonded to the
nearest face, the value of the offset distance should be defined to be as small as
possible.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
451
AUTODYN User Manual
Breakable
By default the bonded face connection will not be breakable. When the option
Stress criteria is selected the bonded connection will fail and break upon a userdefined stress failure criterion:
By stress:
o Normal stress limit: maximum normal stress that can be sustained at
the bond
o Shear stress limit: maximum shear stress that can be sustained at the
bond
Failure of the bond occurs when:
where σn and σs are normal and shear stress at the bond Sn and Ss are the maximum
allowed normal and shear stress limits and expn and exps are user defined
exponential coefficients. The normal stress at the bond σn is nonzero for tensile
values only.
Selection method
Bonded joins can be generated in AUTODYN on a part basis as well as on a
(multiple) face group basis.
Bonded Connections can also be defined in an Explicit Dynamic system and
automatically transferred into a linked AUTODYN system.
Notes
The element variable BOND_STATUS is used to record how many nodes are
actively bonded to the faces of an element. This variable can be contoured to
verify that bonds are correctly defined. If a bond fails during the simulation
the bond status will show a reduction in the number of active bonds. When an
element has no remaining bonds the value of BOND-STATUS is set to -1.0.
452
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Bonded contact is only available with trajectory contact.
Bonded contact is available for unstructured volume, shell and beam
elements.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
453
AUTODYN User Manual
Interactions
Interactions
The Interactions dialog panel lets you define interactions between the various Parts
of your model.
Buttons at the top of this panel let you choose which type of interaction you want to
set up:
Lagrange/Lagrange
Press this button to set up impact / slide interactions between Lagrangian Parts
(Parts using a Lagrange, Shell, Beam or SPH solver).
Euler/Lagrange
Press this button to set up coupling between Lagrangian Parts and Eulerian Parts.
454
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Lagrange/Lagrange
Interactions - Lagrange / Lagrange
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
455
AUTODYN User Manual
2D
3D
This panel lets you set up interactions between Lagrangian Parts (Parts using a
Lagrange, Shell, Beam or SPH solver).
456
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Lagrange/Lagrange Introduction
AUTODYN offers 2 types of Lagrange/Lagrange interaction (contact) methods.
Gap contact
In this contact method each surface segment is surrounded by a contact detection
zone. The dimensions of this contact zone is called Gap size. This means that
initially the outside surfaces of the parts in the contact should be separated by the
gap distance.
Any nodes entering the contact detection zone of a surface segment are repelled by
a force normal to the segment surface and proportional to the depth of penetration of
the node into the contact detection zone.
The interaction conserves linear and angular momentum.
To assure a stable interaction process the gap contact algorithm uses a timestep
restriction such that during 1 computational time step a surface node cannot travel
more than 20% into the contact detection zone.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
457
AUTODYN User Manual
where δ is the gap size and V the velocity of the penetrating node.
The gap contact is available for all structured as well as unstructured Lagrange
Parts, with exception for 2D unstructured Parts.
Trajectory contact
The Trajectory contact algorithm is available for all 3D Unstructured solvers,
including SPH, and has three main potential benefits over the Gap based contact
algorithm.
There is no requirement to specify a contact detection zone or leave a
physical gap between Parts at the start of a simulation. This makes model
generation for complex 3D geometries significantly easier.
There is no constraint on the timestep due to contact. The algorithm detects
node to fact contact by tracking the trajectory of the nodes and faces over
time. The removal of the timestep constraint on contact can give very
significant performance improvements.
The algorithm is energy conserving, in addition to momentum conserving.
The trajectory of nodes and faces included in frictional or frictionless contact are
tracked during the computational cycle. If the trajectory of a node and a face
intersects during the cycle a contact even is detected.
458
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
If a contact event is detected the node involved in the contact will be pushed back
towards the true contact position during the computational cycle.
There are two methods available:
1. Penalty
If a contact event is detected, a local penalty force is calculated to push the
node back to the face. Equal and opposite forces are calculated on the nodes
of the face in order to conserve linear and angular momentum. The applied
penalty force will push the node back towards the true contact position during
the cycle. However, it will take several cycles to satisfy the contact condition.
Kinetic energy is not necessarily conserved. The conservation of energy can
be tracked using the energy time history.
2. Decomposition Response (DCR)
All contacts that take place at the same point in time are first detected. The
response of the system to these contact events is then calculated to conserve
momentum and energy. During this process, forces are calculated to ensure
that the resulting position of the nodes and faces does not result in further
penetration at that point in time. The decomposition response algorithm is
more impulsive (in a given computational cycle) than the penalty method. This
can give rise to large hourglass energies and energy errors.
The trajectory contact can handle multiple contact of a node with different faces of a
contact surface during a computational timestep.
Current Limitations
The trajectory contact option cannot currently be used in parallel simulations.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
459
AUTODYN User Manual
The trajectory contact option cannot be used in combination with joined
unstructured parts. To circumvent this limitation the option to merge all joined
unstructured nodes can be used.
Interaction of SPH nodes, accounting for their full natural thickness/size is
currently not available.
The decomposition response algorithm cannot currently be used in
combination with bonded contact regions. The formulation will automatically
switch to the Penalty method if bonded regions are present in the model.
460
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Interactions - Lagrange / Lagrange - Create
This window lets you create a gap between structured Parts automatically. This
option doesn't work for unstructured parts and therefore unstructured Parts will not
appear in the window.
Gaps are created by reducing the size of surface elements of the selected Parts, so
there will be small changes in the mass of the Parts that are modified.
You may prefer to manually inset gaps using the Translate and / or Scale options in
the Zoning panel (no mass will be lost).
The box in this window lists all Parts involved in interactions.
Select the Part(s) you want to adjust while creating the gaps and press
AUTODYN to automatically create the gaps.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
for
461
AUTODYN User Manual
Interactions - Lagrange / Lagrange - Add
This window lets you add interactions between one or more Parts.
This method of adding interactions works well no matter how many Parts you have in
your model.
If you only have a few Parts, you may prefer to use a Matrix to choose the
interactions.
Select Part(s)
This box lists all Parts involved in interactions. Select one or more Parts in this list.
Select Part(s) to interact with the above list
462
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
This box also lists all Parts involved in interactions. Select one or more Parts in this
list.
Press
to set all Parts selected in the top window to interact with all Parts
selected in the lower window.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
463
AUTODYN User Manual
Interactions - Lagrange / Lagrange - Remove
This window lets you remove interactions between one or more Parts.
This method of removing interactions works well no matter how many Parts you have
in your model.
If you only have a few Parts, you may prefer to use a Matrix to add or remove
interactions.
Select Part(s)
This box lists all Parts involved in interactions. Select one or more Parts in this list.
Select Part(s) to interact with the above list
464
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
This box also lists all Parts involved in interactions. Select one or more Parts in this
list.
Press
to remove interaction between all Parts selected in the top window and
all Parts selected in the lower window.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
465
AUTODYN User Manual
Interactions - Lagrange / Lagrange - Matrix
When the model doesn't contain more than 25 parts, this window lets you choose
which Parts you want to interact by checking boxes in a matrix.
When a model contains more than 25 Parts the matrix option is not available and will
be greyed-out.
If you have a large number of Parts, you may find it easy to set interactions using the
Add / Remove options in the Interactions dialog panel.
The matrix shown in this panel list the Parts of your model vertically and horizontally.
This matrix is symmetrical, so only the diagonal and lower part of the matrix is
shown.
466
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Check a box if you want the two associated Parts to interact.
The Remove buttons let you quickly uncheck the boxes for each row of the matrix.
Press
to apply the changes you make to the matrix.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
467
AUTODYN User Manual
Interactions - Lagrange / Lagrange - Range
This window is only available for Gap contact and lets you set the index range of a
structured Part that will be checked for interactions. For unstructured parts this
option is not available.
For Trajectory contact and for unstructured parts the Interaction by Group option can
be used instead to only select a region of a Part for interaction.
Select Part
Select the Part for which you want to set the index range for interactions in this box.
Interaction Range
Enter the index range that you want to be checked for interaction.
468
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Interactions - Lagrange / Lagrange - Friction
This window is available for Gap contact and lets you set static friction coefficients
between two Parts.
Select Part 1
Select the first of the two Parts you want to set the friction coefficient between in this
box.
Select Part 2
Select the second of the two Parts you want to set the friction coefficient between in
this box.
Friction Coefficient
Enter the friction coefficient you want to use.
Press
to set the friction coefficient between the two selected Parts.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
469
AUTODYN User Manual
You can apply this procedure as many times as you like to set coefficients between
other Parts without exiting the window.
This window is available for Trajectory contact and lets you define static and
dynamic friction between two Parts.
Select Part 1
Select the first of the two Parts you want to set the friction coefficient between in this
box.
Select Part 2
Select the second of the two Parts you want to set the friction coefficient between in
this box.
Friction Coefficient
A non-zero value for the Static Friction coefficient will activate Coulomb type friction
between bodies (F=μR).
470
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
A non-zero value for the Dynamic Friction coefficient and the Dynamic friction decay
constant will activate the use of dynamic friction where an effective friction
coefficient, μ, is used which is given by:
where
μs = static
μd = dynamic coefficient of friction
β = exponential decay coefficient
v = relative sliding velocity at point of contact
Press
to set the friction coefficient between the two selected Parts.
You can apply this procedure as many times as you like to set coefficients between
other Parts without exiting the window.
Note that friction is not available for Interaction defined by Group.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
471
AUTODYN User Manual
Lagrange/Lagrange - 2D Gap Contact Options
Type - External Gap
When a 2D model contains structured elements only, the 2D gap contact must be
used to define Lagrange/Lagrange interactions.
472
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
An analysis model that contains a mix of structured (IJK) Lagrangian Parts and
unstructured Lagrangian Parts can currently not be run with Gap contact and also
not with Trajectory contact.
To be able to use Trajectory contact the analysis model must contain unstructured
Lagrangian volume Parts only. Similar, to be able to use Gap contact the analysis
model must contain structured Lagrangian Parts only.
Interaction Gap
A gap is required for the interaction logic. The size of this gap must be in the range
1/10 to 1/2 the dimension of the smallest element face of Parts involved in
interactions.
For most models you should set the gap size close to the smallest allowed value
(Parts using a Lagrange or Shell Solver).
Gap size
Enter a value for the Gap size in this field or press Calculate to have
AUTODYN set it for you.
Gap Type
Select whether you want to use an internal or external gap.
The external gap is strongly recommended because calculations using this
option are more robust and more efficient. However, this option does require
that interacting Parts are separated by the gap size at the start of your
calculation.
Quick check
Check this box to use a fast calculation for the interaction time-step using only
the maximum velocity in your problem. You should only check this box if you
know that your maximum velocities will always be in impact regions.
Calculate
Press this button to have AUTODYN automatically calculate the Gap size for
you. The Gap size will be set to 1/10 the dimension of the smallest element
face of Parts involved in interactions.
Check
Press this button to check that the Gap size is valid and that all Parts involved
in interactions are separated by the Gap size.
Erosion
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
473
AUTODYN User Manual
Retain inertia of eroded nodes
Check this box if you want to retain the inertial of eroded nodes (otherwise
eroded nodes are removed from the model).
Prevent erosion of degenerate elements
Check this box if you want the interaction calculation to be used to stop
elements from becoming degenerate. This option only works for Lagrange
volume elements.
Warning! Activating this option can lead to unphysical results, particularly if a
large Gap size is used.
Interaction by Part
Add
Press this button to set interactions between Parts.
Add All
Press this button to set all Parts to interact with each other.
Remove
Press this button to remove interactions between Parts.
Remove All
Press this button to remove all interactions between Parts.
Matrix
Press this buttons to set interactions using a Part matrix.
Range
Press this button to set the index range of each Part that will be checked for
interactions.
Friction
Press this button to set static friction coefficients between different Parts.
Review
Press this button to review all your interaction settings.
474
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Self Interaction
If the self-interaction option is switched on the contact detection algorithm will also
check for external nodes of a part contacting with faces of the same part in addition
to other parts. This is the most robust contact setting since all possible external
contacts should be detected.
Interaction Timestep
AUTODYN automatically calculates an Interaction Timestep based on the Gap size
and the maximum velocity of the Parts involved in interactions.
Safety Factor
Enter the safety factor you want to use to calculate the Interaction Timestep in
this field.
You cannot enter a value greater than the default value (0.2).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
475
AUTODYN User Manual
Interactions-Lagrange/Lagrange-2D Trajectory Contact Options
Type Trajectory
When a 2D model contains unstructured Lagrangian volume elements the 2D
trajectory must be used to define Lagrange/Lagrange Interactions.
An analysis model that contains a mix of structured (IJK) Lagrangian Parts and
unstructured Lagrangian Parts can currently not be run with Trajectory contact and
also not with Gap contact.
476
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
To be able to use Trajectory contact the analysis model must contain unstructured
Lagrangian volume Parts only. Similar, to be able to use Gap contact the analysis
model must contain structured Lagrangian Parts only.
Method
Method in which a contacting node is pushed back to the true contact position during
the computational cycle.
There are two methods available:
1. None
No contact defined
2. Penalty
If a contact event is detected, a local penalty force is calculated to push the
node back to the face. Equal and opposite forces are calculated on the nodes
of the face in order to conserve linear and angular momentum. The applied
penalty force will push the node back towards the true contact position during
the cycle. However, it will take several cycles to satisfy the contact condition.
Kinetic energy is not necessarily conserved. The conservation of energy can
be tracked using the energy time history.
3. Decomposition Response (DCR)
All contacts that take place at the same point in time are first detected. The
response of the system to these contact events is then calculated to conserve
momentum and energy. During this process forces are calculated to ensure
that the resulting position of the nodes and faces does not result in further
penetration at that point in time. The decomposition response algorithm is
more impulsive (in a given computational cycle) than the penalty method. This
can give rise to large hourglass energies and energy errors.
Retain inertia of eroded nodes
Check this box if you want to retain the inertial of eroded nodes (otherwise
eroded nodes are removed from the model).
Interaction by Part
Add
Press this button to set interactions between Parts.
Add All
Press this button to set all Parts to interact with each other.
Remove
Press this button to remove interactions between Parts.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
477
AUTODYN User Manual
Remove All
Press this button to remove all interactions between Parts.
Matrix
Press this button to set interactions using a Part matrix.
Friction
Press this button to define static and dynamic friction between different Parts.
Review
Press this button to review all your interaction settings.
User defined friction
Aside from the friction definition through the Interaction by Part method described
above there is also a user defined friction option available through the use of a usersubroutine called EXFRICTION2D.
Self Interaction
If the self-interaction option is switched on the contact detection algorithm will also
check for external nodes of a part contacting with faces of the same part in addition
to other parts. This is the most robust contact setting since all possible external
contacts should be detected.
Self-interaction Tol
The self-interaction option enables automatic erosion when an element
deforms such that one of its nodes comes within a specified distance of one of
its faces. This option will prevent that volume elements become degenerated.
478
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
The specified distance is calculated using the Self-interaction Tol. value which
is a factor in the range 0.1 to 05. This factor is multiplied by the smallest
characteristic dimension of the elements in the mesh to give a physical
dimension.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
479
AUTODYN User Manual
Interactions-Lagrange/Lagrange-3D Gap Contact Options
Interaction Gap (External Gap options)
The External Gap contact algorithm is implemented for all Lagrange, ALE, shell,
beam and unstructured solvers.
480
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
A gap is required for the interaction logic. The size of this gap must be in the range
1/10 to 1/2 the dimension of the smallest element face of Parts involved in
interactions.
There are two contact algorithms available in 3D, External Gap and Trajectory
For most models you should set the gap size close to the smallest allowed value
(1/10 the dimension of the smallest element face).
Gap size
Enter a value for the Gap size in this field or press Calculate to have
AUTODYN set it for you.
Calculate
Press this button to have AUTODYN automatically calculate the Gap size for
you. The Gap size will be set to 1/10 the dimension of the smallest element
face of Parts involved in interactions.
Create
All interacting Parts in you model must be separated by at least the Gap size.
Press this button to automatically insert the required gap between Parts.
You may want to insert gaps manually using the Translate and / or Scale
options in the zoning Panel Zoning panel.
Check
Press this button to check that the Gap size is valid and that all Parts involved
in interactions are separated by the Gap size.
Include edge on edge impacts
Check this box if you want the interaction calculation to include testing for edge
on edge impacts (significantly more computing is required if you check this
box).
Work unit size
Select the size of work unit to be used for interactions.
Average - The work unit size is based on the average cell dimension
Smallest - The work unit size is based on the smallest element dimension
Largest - The work unit size is based on the largest element dimension
Erosion
Retain inertia of eroded nodes
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
481
AUTODYN User Manual
Check this box if you want to retain the inertial of eroded nodes (otherwise
eroded nodes are removed from the model).
Prevent erosion of degenerate elements
Check this box if you want the interaction calculation to be used to stop
elements from becoming degenerate. This option only works for Lagrange
volume elements.
Warning! Activating this option can lead to unphysical results, particularly if a
large Gap size is used.
Erode over penetrated faces
Check this box if you want elements with over penetrated faces to be eroded.
You should only check this box if you know this option is required to
successfully complete your calculation.
Interaction by Part
Add
Press this button to set interactions between Parts.
Add All
Press this button to set all Parts to interact with each other.
Remove
Press this button to remove interactions between Parts.
Remove All
Press this button to remove all interactions between Parts.
Matrix
Press this buttons to set interactions using a Part matrix.
Range
Press this button to set the index range of each Part that will be checked for
interactions.
Friction
Press this button to set static friction coefficients between different Parts.
482
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Review
Press this button to review all your interaction settings.
Self interaction of Parts
Check this box if you want Parts to interact with themselves (i.e. test for self-impact).
Interaction by Group
In many calculations, the contact region may be relatively small in comparison to the
entire model, and as the interactions calculation is numerically intensive, it would be
beneficial if the scope of its work were limited to this smaller area. The Group
Contact option allows the user to select a set of face groups to describe the extent of
the interactions in unstructured models.
Select the "Specify Group Contacts by Group" toggle and press Select, to open the
"Select Groups to include in Contact" dialog, and use the Add/Remove button to
specify which face groups are to be included in the contact calculations.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
483
AUTODYN User Manual
During execution, any faces eroded will be removed from the group, and any new
faces uncovered will be added to a group named "Uncovered faces". Unstructured
Beams and SPH can also be included as a node group to participate in contact.
484
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Note that Group Contact is additive to Part contact. Selecting a Part for contact
results in all external faces in the Part being checked for contact. Group contact
should be used to add additional external faces from Parts that have been excluded
from contact in the Part interaction matrix.
Group contact is only available to faces of unstructured Parts and doesn't include
friction.
Interaction Timestep
AUTODYN automatically calculates an Interaction Timestep based on the Gap size
and the maximum velocity of the Parts involved in interactions.
Safety Factor
Enter the safety factor you want to use to calculate the Interaction Timestep in
this field.
You cannot enter a value greater than the default value (0.2).
Limiting Velocity
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
485
AUTODYN User Manual
Enter the maximum velocity you want to use for calculating the Interaction
Timestep
in this field.
This option is useful if you have large velocities controlling the timestep that
are not involved in interactions.
The default limiting velocity is larger than any velocity your model should
encounter.
486
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Interactions-Lagrange/Lagrange-3D Trajectory Contact Options
Interaction Trajectory (Trajectory options)
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
487
AUTODYN User Manual
The Trajectory contact algorithm is implemented for all unstructured Lagrangian
solvers and SPH.
Method
Method in which a contacting node is pushed back to the true contact position during
the computational cycle.
There are three methods available:
1. None
No contact defined
2. Penalty
If a contact event is detected, a local penalty force is calculated to push the
node back to the face. Equal and opposite forces are calculated on the nodes
of the face in order to conserve linear and angular momentum. The applied
penalty force will push the node back towards the true contact position during
the cycle. However, it will take several cycles to satisfy the contact condition.
Kinetic energy is not necessarily conserved. The conservation of energy can
be tracked using the energy time history.
3. Decomposition Response (DCR)
All contacts that take place at the same point in time are first detected. The
response of the system to these contact events is then calculated to conserve
momentum and energy. During this process, forces are calculated to ensure
that the resulting position of the nodes and faces does not result in further
penetration at that point in time. The decomposition response algorithm is
more impulsive (in a given computational cycle) than the penalty method. This
can give rise to large hourglass energies and energy errors.
Shell thickness factor
The value of the factor has to be taken between 0.0 and 1.0 and determines the
amount of the shell thickness that is taken into account as the interaction distance.
A factor of 1.0 takes the full shell thickness into account, which means that the
contact surface is positioned at half the shell thickness on both sides of the shell mid
plane.
A factor of 0.0 means that the shell has no contact thickness and the contact surface
is positioned at the shell mid plane.
Note that for shell node on shell face impacts, the node is always located at the midsurface of the shell.
Initial Penetrations
Check
488
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
On clicking this button, AUTODYN will search the model for initial penetrations
of nodes into surfaces. If any penetrating nodes/surfaces are found, a new
Group will be created so that they can be identified/displayed using the Groups
panel. Nodes that initially penetrate surfaces will be "missed" by the contact
algorithm.
Fix
When this option is selected the initially penetrated nodes are set back to the
closest contact surface and no initial penetrations are present at the start of the
analysis.
This option is meant for situations where small initial penetrations occur (for
example because of round-off) and should be used with care because the
analysis model geometry is changed.
Note that it may not be possible to remove all initial penetrations with this
algorithm. Features are available in the DesignModeler and Meshing
application to prevent initial penetrations occurring.
Undo
This option will restore the geometry of the analysis model before the initial
penetrations were fixed.
It is recommended that the fixed initial penetrations are checked before the
model is modified further otherwise it may not be possible to undo the last fix
operation.
Erosion
Retain inertia of eroded nodes
Check this box if you want to retain the inertial of eroded nodes (otherwise
eroded nodes are removed from the model).
Interaction by Part
Add
Press this button to set interaction between Parts.
Add All
Press this button to set all Parts to interact with each other.
Remove
Press this button to remove interaction between Parts.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
489
AUTODYN User Manual
Remove All
Press this button to remove all interactions between Parts.
Matrix
Press this button to set interactions using a Part matrix.
Range
Press this buttons to set the index range of each Part that will be checked for
interactions.
Friction
Press this button to define static and dynamic friction between different Parts.
Review
Press this button to review all your interaction settings.
User defined friction
Aside from the friction definition through the interaction by Part method described
above there is also a user defined friction option available through the use of a usersubroutine called EXFRICTION.
Self Interaction
If the self-interaction option is switched on the contact detection algorithm will also
check for external nodes of a part contacting with faces of the same part in addition
to other parts. This is the most robust contact setting since all possible external
contacts should be detected.
Self-interaction Tol.
490
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
The self-interaction option enables automatic erosion when an element
deforms such that one of its nodes comes within a specified distance of one of
its faces. This option will prevent volume elements becoming degenerate.
The specified distance is calculated using the Self-interaction Tol. value which
is a factor in the range 0.1 to 0.5. This factor is multiplied by the smallest
characteristic dimension of the elements in the mesh to give a physical
dimension.
Interaction by Group
In many calculations, the contact region may be relatively small in comparison to the
entire model, and as the interactions calculation is numerically intensive, it would be
beneficial if the scope of its work were limited to this smaller area. The Group
Contact option allows the user to select a set of face groups to describe the extent of
the interactions in unstructured models.
Select the "Specify Group Contacts by Group" toggle and press Select, to open the
"Select Groups to include in Contact" dialog, and use the Add/Remove button to
specify which face groups are to be included in the contact calculations.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
491
AUTODYN User Manual
During execution, any faces eroded will be removed from the group, and any new
faces uncovered will be added to a group named "Uncovered faces". Unstructured
Beams and SPH can also be included as a node group to participate in contact.
492
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Note that Group Contact is additive to Part contact. Selecting a Part for contact
results in all external faces in that Part being checked for contact. Group contact
should be used to add additional external faces from Parts that have been excluded
from contact in the Part interaction matrix.
Group contact is only applicable to faces of unstructured Parts and doesn't include
friction.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
493
AUTODYN User Manual
Euler/Lagrange (2D)
Interactions - Euler / Lagrange (2D)
This panel lets you set up interactions (coupling) between 2D Lagrange Parts and
Euler Parts.
Select Euler/Lagrange Coupling Type
Select the type of coupling you want to muse for Euler/Lagrange interactions.
None
Do not compute any Euler/Lagrange coupling
Automatic Let AUTODYN set up coupling automatically.
Polygons
Set up interactions manually using Polygons.
Automatic coupling is recommended if you want all Lagrange Parts to interact with
all Euler Parts and you have no Shell Parts.
If you want more control in defining which Parts should be coupled or have Shell
Parts that you want to couple to Euler, use Polygon coupling.
Erosion can be used with automatic coupling, but not with Polygon coupling.
If you select Polygon coupling, further input dialog is presented :
494
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
To set up an Euler/Lagrange interaction using Polygons, you must first generate one
or more Polygons and attach the polygon points to nodes on the surface of the
Lagrange Parts that you want to interact with Euler.
Then you must specify which Polygons you want to couple with which Euler Parts.
This dialog lets you generate your Polygons and set up coupling between your
Polygons and the Euler Parts in your model.
Polygons
Select Polygon
This box lists all the Polygons you have created. You can select a Polygon in
this list.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
495
AUTODYN User Manual
Select active part
This box lists all the Parts that can be coupled to Polygons (i.e. all Lagrange,
ALE and Shell Parts). You can select a Part in this list.
New
Press this button to create a new Polygon.
Delete
Press this button to delete the selected Polygon
Velocity
Press this button to apply a velocity to the selected node.
Porosity
Press this button to set porosity for the selected Polygon.
Add First Point (only visible when no points are defined)
Use this option to generate the first point for the selected Polygon (use shift +
right mouse button to place the point)
Select Point
Use this option to select a point of the selected Polygon (use shift + right
mouse button to select the point)
Add Point After
Use this option to add a point after the selected polygon point (use shift + right
mouse button to place the point)
If you place the added point close to a node on the surface of the selected
active Part, the point will automatically be attached to that node.
If you immediately follow this by placing a second point close to another
surface node of the same selected active Part, multiple points will be generated
attached to all surface nodes between the two placed nodes in an anticlockwise direction.
Insert Point Before
Use this option to insert a point before the selected polygon point (use shift +
right mouse button to place the point)
496
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
If you place the inserted point close to a node on the surface of the selected
active Part, the point will automatically be attached to that node.
If you immediately follow this by placing a second point close to another
surface node of the same selected active Part, multiple points will be generated
attached to all surface nodes between the two placed nodes in an anticlockwise direction.
Move Point
Use this option to move the selected polygon point to a new location (use shift
+ right mouse button to place the point at its new location)
Delete Point(s)
Use this option to delete one or more polygon points. The first point to be
deleted is the selected polygon point. Use shift + right mouse button to
select the last point to be deleted. All points from the selected point to last point
inclusive will be deleted.
X/Y Coordinates
These fields display the coordinates of the selected polygon point. You can
change the location of this point by entering new values in these fields.
Example
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
497
AUTODYN User Manual
Add first point
Add point after
(Single point not attached to grid)
(Multiple points generated
Add point after
(Single point attached to grid)
anti-clockwise around grid)
The selected polygon node is always shown in red.
The last point of Polygon is automatically connected to first point to close
the Polygon.
Coupling
Name / Polygon / Euler Part
These boxes list the interaction sets you have defined for Polygon coupling.
Name
The name of the interaction set.
Polygon The Polygon that is coupled to an Euler Part.
Euler Part The Euler Part that the Polygon is coupled to.
You can select a set in this list
New
Press this button to add a new interaction set.
Delete
Press this button to delete the selected interaction set.
498
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Interactions - Euler / Lagrange Introduction
The Euler/Lagrange interaction (Fluid-Structure Interaction) in AUTODYN couples
the Eulerian domain to the Lagrangian structural domain.
This coupling algorithm in AUTODYN finds the intersection between the external
faces of the interacting structures and the cells and faces of the Euler grids. These
intersection calculations give an exact calculation (within numerical precision) of the
covered fraction of the Euler cells and faces, as shown in the left hand figure below.
These properties are used in the 3D Euler solvers for coupled simulations.
The coupling can be chosen to be fully automatic (2D/3D) or by means of polygons
(2D).
Polygon coupling
This coupling technique is available in 2D to set up an Euler/Lagrange interaction
where one or more Polygons are defined and the polygon points are manually
attached to nodes on the surface of the Lagrange Parts that interact with Euler. All
structured Lagrangian element types can be coupled to Euler using polygons.
Unstructured parts cannot be coupled to Euler using polygons; in that case the
automatic coupling needs to be used.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
499
AUTODYN User Manual
Automatic coupling
This coupling technique is available in 2D as well as in 3D. AUTODYN will
automatically setup the Euler/Lagrange interactions and the only thing the user has
to define is which parts interact with Euler. Automatically all outside surface
segments of all selected Lagrangian parts are generated and coupled to Euler.
In 2D the automatic coupling is only available for structured and unstructured
Lagrangian volume elements.
In 3D the automatic coupling is available for structured and unstructured Lagrangian
volume and shell elements. For shell elements an artificial thickening of the shell
parts is used.
Automatic generation of outside surface
Artificial shell thickening for coupling
Coupling and Erosion
Erosion in combination with Euler/Lagrange coupling can be used for automatic
coupling in 2D as well as 3D.
500
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
When elements that are connected to the coupling surface are eroded the coupling
surface automatically will be updated for the new uncovered Lagrangian element
faces.
Example simulation of fragmenting ring using Euler-Lagrange Coupling and requiring
automated update of coupling surfaces during the simulation
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
501
AUTODYN User Manual
Interactions - Euler/Lagrange (2D) - New Polygon
This window lets you create a new Polygon for Euler/Lagrange coupling.
Enter the name you want to use for your new polygon in the field provided and press
.
Once you have created your Polygon, you can add points and attached these points
to Lagrange nodes using options in the Dialog panel.
502
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Interactions - Euler/Lagrange (2D) - Velocity
This window lets you attach a velocity boundary condition the selected polygon.
All polygon points not attached to a Part will use this velocity.
Select the boundary condition you want to use from the list and press
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
.
503
AUTODYN User Manual
Interactions - Euler/Lagrange (2D) - Porosity
This window lets you set porosity for your Polygon.
By default, a Polygon completely covers the Euler Parts it is coupled to.
Setting porosity greater than zero allows partial flow in the Euler Parts under the
Polygon.
Enter a porosity factor between 0.0 and 1.0.
504
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Interactions - Euler/Lagrange (2D) - New Interaction
This window lets you define a new interaction set for Polygon coupling.
Enter name of new interaction
Enter the name you want to use for the new interaction set in this field.
Select a Polygon and Euler Part.
Select the Polygon in the left box that you want to be coupled to the Euler Part you
select in the right box.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
505
AUTODYN User Manual
Euler/Lagrange (3D)
Interactions - Euler - Lagrange (3D)
This panel lets you set up interactions (coupling) between 3D Lagrange Parts and
Euler Parts.
Coupling Type
Select the coupling type you want to use.
None
- no coupling is defined
Rigid
- Fill Parts are used to define rigid boundaries for Euler.
Fully Coupled
- Lagrange Parts interact with Euler Parts dynamically.
Weak Coupling - A fast method for having Lagrange and Euler Parts interact
dynamically.
Cover fraction limit
Enter the cover fraction limit in this field. This is used to determine when a partially
covered Euler cell is blended to a neighbor.
Euler subcycling
506
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Select whether you want Euler subcycling On or Off
Euler/shell interactions
Select
Press this button to select the Lagrangian Parts you want to couple to Euler.
Thickness
Press this button to specify the shell thickness you want to use for the coupling
calculation.
Joins
Press this button to specify which shells are to be joined for the coupling
calculation.
Review
Press this button to review your Euler-Shell interactions.
Weak coupling settings
Browse for weak coupling data file.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
507
AUTODYN User Manual
Interactions - Euler / Lagrange (3D) - Select
This window lets you select the Lagrangian Parts you want to couple to Euler.
Parts coupled to Euler-FCT
This box shows you the current Parts that are coupled to Euler.
Select parts to add/remove
This box shows all the Parts that can be coupled to Euler. You can select one or
more Parts in this list.
Add
Press this button to add the selected Parts to be coupled with Euler.
Add all
Press this button to add all the Parts to be coupled with Euler.
Remove
Press this button to remove the selected Parts from being coupled with Euler.
Remove all
Press this button to remove all Parts from being coupled with Euler.
508
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Review
Press this button to add review all coupling with Euler.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
509
AUTODYN User Manual
Interactions - Euler / Lagrange (3D) - Thickness
As well as being able to couple volume element solvers, it is also possible in
AUTODYN to couple shell solvers. For a shell solver, the parts do not have any
geometric through thickness dimension, and as such cannot cover any volume in the
Euler mesh. Therefore, each shell part needs to be artificially thickened by the user.
Select Part
This list contains all the shell parts in the model that are selected for coupling with
Euler. If you select a part, the coupling thickness and direction of the thickening for
that part is shown below.
Coupling Thickness
This shows the coupling thickness for the selected part. To modify the coupling
thickness, enter the new value, and press the Apply button. For the coupling
methodology to function correctly, the artificial thickness of a shell must be at least
twice the dimension of the largest cell size in the surrounding Euler grid.
Direction
This shows the direction the shell is thickened in for the selected part. To modify the
thickening direction, select the desired direction, and press the Apply button.
The coupling thickness can be applied on both sides of the midplane of the shell
(Centred) or applied to one side of the shell, where Positive is in the direction of the
normal of the shell.
510
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Review
If you select the review button, an html summary is opened that displays which shell
parts have been included in the Euler coupling, the thickness and direction for these
shell parts, and also the thickened shell joined matrix.
You can also view the thickened shells by switching on "Shell thickness" in the Plots
panel, and choosing "Artificial Shell Coupling Thickness" in the Shell Thickness
Settings panel.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
511
AUTODYN User Manual
Interactions - Euler / Lagrange (3D) - Joins
To ensure that volumes of joined thickened shells do not overlap as the shells
deform, the thickening algorithm needs some information on which shell parts should
be considered joined when computing the outward normals for shell nodes in the
thickening geometry calculations. By default all thickened shell parts are set as
joined for the coupling calculation. If this is not appropriate, for example for a Tjunction between two shell parts, you should remove the joins for the coupling
calculation. It is important to note that these join settings are only used in the
coupling calculation and do not affect the structural joins.
This is illustrated in the figure below. On the left, the two shell parts are joined for
thickening calculations, and the resulting thickened shells define a closed volume.
On the right, the two shell parts are not joined for thickening calculations, and the
shell overlap is not satisfactory for coupling.
Select Part
512
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
This list shows all the shell parts that are coupled in Euler. When a part is selected
in this list, all parts joined to it are displayed in the "Included parts for normal
calculation" list.
Included parts for normal calculation
This list shows all shell parts that are joined to the shell part selected in "Select Part"
Select part(s) to add/remove from normal calculation
These two fields are used to add or remove parts from the normal calculation. For
example, a model has shell parts "hull#1", "hull#2" and "composite", as shown in the
image of the window at the top of the page. To include the normals between the first
two parts, select "hull#1" in the left hand list, "hull#2" in the right hand list, and press
the apply button.
Review
If you select the review button, an html summary is opened that displays which shell
parts have been included in the Euler coupling, the thickness and direction for these
shell parts, and also the thickened shell joined matrix, that shows which shells are
included in the normal calculation.
You can also view the thickened shells by switching on "Shell thickness" in the Plots
panel, and choosing "Artificial Shell Coupling Thickness" in the Shell Thickness
Settings panel.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
513
AUTODYN User Manual
Interactions - Euler / Lagrange (3D) - Weak Coupling
Introduction
Within AUTODYN-3D, there is a facility for the application of a pressure field in 3D
space to Lagrange type parts as a boundary condition. The pressures in 3D space
are contained in a sequence of Field files, the format of which is described below.
Also included is an additional feature that allows the user to create these fields
when using either the FCT or the Euler processors. Weak Lagrange Coupling can
be seen as equivalent to the current FCT - Lagrange couple but without the feedback
from the Lagrange type parts back into the FCT part. This weak coupling assumes
that any deflections in the Lagrange model are small, and should only be used in
such cases.
The current implementation only considers the possibility of mapping pressure data,
and applies this to the Lagrange boundary surfaces as nodal forces. The pressures
will be applied to all wetted surfaces of Lagrange type subgrids within the volume
described by the pressure files. The advantage over the current LCT-Lagrange
coupling is that multiple Lagrange calculations can be carried out on one FCT
calculation, thus saving analysis time. Also, some speedup would be expected over
a normal coupled solution for a single FCT and then Lagrange calculation.
Creating the Field files
The Field files are created as a field edit when an FCT or Euler type simulation is
being carried out. The user should press Output on the navigation bar and open the
Field output part of the dialog panel. Under this menu there are three options,
namely Cycles, Times and Set_part. The cycle and time options work in the
traditional manner of all edits in AUTODYN and allow the user to select the
frequency of the Field file output. The third menu, set_part, allows the user to select
which part the pressure data will be taken from, and the I, J and K range. The file
format only allows one block of data to be written. If this information is not given by
the user then the entire range of the first ECT or Euler part found will be written to
the Field file. A geometry data field is only produced when a problem is started or
restarted, and this cycle coincides with a field edit.
Using the Weak Interactions
The coupling option Weak Coupling is included under the Euler Lagrange
interaction tab after Interaction is selected from the navigation bar. The EulerLagrange/Shell interactions need to be set to chose which Lagrange type part are
included in the coupling, and how shells interact. Under the weak coupling settings,
the Ambient Pressure should be entered. This pressure is removed from the Field
file pressure, i.e.
Also the Field file set need to be selected by using the file browser to select the first
in the required set.
514
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Notes on the Mapping
AUTODYN-3D interpolates linearly in time the pressure data from two Field files, the
current time of the simulation being in-between the times of the fields. When a field
file is read into the solver a mapping is created. This is a lookup table for each cell
face in the Lagrange model that is activated pointing to a cell in the pressure field. If
a geometry data field is not present in the Field file then the existing mapping from
the previous field is used. The mapping is always created using the initial
coordinates (i.e. at time equal to zero) of the Lagrange type parts. The interpolation
in space is the same as for the current FCT-Lagrange interactions; the nearest cells
centre to the face centre is used.
Field file format (.ADF FILES)
The ADF (AUTODYN FIELD) file format contains field information on a regular
structured rectangular grid. Scalar data is cell centred. The naming convention of
the files is
IDENT_####.ADF
FORMAT:'(A,A1,I4.4,A4)'
Where #### is an increasing integer number, starting at 0001.
Record 1
FILEID (CH*256)
Record 2
NCYCLE, TIME, NTU,
NMU, NLU
Record 3
NI,NJ, NK
Record 3+(NS1)*2
Record 4+(NS1)*2
Record (LAST)
ITEM_NAME (CH*256)
The data attached to the
item
"END OF SCALAR FILE"
Character string which can be
used to identify the file
NTU is the time unit (1:μs
2:ms, 3:s)
NMU is the mass unit (1:mg
2:g, 3:kg)
NLU is the length unit (1:mm,
2:cm, 3:m)
Maximum number of nodes in
each of the three directions
Name of the item to follow, i.e.
GEOMETRY or PRESSURE
Item specific - See below
The data attached to the items are
GEOMETRY
XC (1:NI)
YC (1:NJ)
ZC (1:NK)
X positions, inline with the I axis
Y positions, inline with the J axis
Z positions, inline with the K axis
PN(1:NI-1, 1:NJ-1, 1:NK-1)
Pressure of each cell. I varies fastest
A geometry data record is only needed if the geometry has changed. The presence
of this field enforces a new mapping. Therefore, if the geometry is only present in
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
515
AUTODYN User Manual
the first field, then the mapping is only done at the beginning of the calculation. On
the other hand, if the geometry is present in every file, then a remapping is done
every time a new flow file is read. If a file does contain a geometry data record then
AUTODYN expects that it will occur before the pressure record. A pressure record
must exist in all files.
Errors, Warning and other Outputs
Errors encountered during the mapping cause a generic error, stop the current
simulation. A summary of the error is written to the message window. The following
table summarizes the error codes.
Too many scaler files
File does not exist
Expecting geometry
data
No pressure data
Error in reading file
1
10000 + file
counter
20000 + file
counter
30000 + file
counter
40000 + file
counter
Errors and Warnings in the Field File writing routines will not stop the calculation, but
will write to the message window an appropriate message.
516
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Detonation (2D)
Detonation (2D)
This window lets you set the locations where explosives will be detonated /
deflagrated.
Detonations / Deflagrations
The box at the top of the window shows you a list of the current detonations /
deflagrations you have defined. You can select from this list.
Point
Press this button to define a detonation point.
Line
Press this button to define a line of detonation.
Circle
Press this button to define a detonation circle (planar symmetry).
Sphere
Press this button to define a detonation sphere (axial symmetry).
Manual
Press this button to manually define initiation times for blocks of elements.
Delete
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
517
AUTODYN User Manual
Press this button to delete the selected detonation definition
Review
Press this button to review information for all detonation definitions.
Path
Select whether you want detonation times to be calculated using direct or indirect
paths.
Direct Path : Detonation times are computed from straight line paths from
detonation points. This is the most accurate method, but is only valid if the
straight line paths are through the explosive material.
Indirect Path : Detonation times are calculated from shortest paths through
explosive material. Paths are automatically computed around inert materials
(e.g. wave shapers).
Plot detonation points
Check this box if you want to see the location of detonation points in the view panel.
518
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Detonation (2D) - Point
This window lets you define a detonation point.
X/Y Coordinates.
Enter the X/Y/Z coordinates of the detonation point in these fields.
Compute Initiation Time?
Select whether you want to specify a detonation time, or have it computed by
AUTODYN.
If selected, AUTODYN will compute the detonation time using paths through the
explosive from other detonation points.
You must specify the initiation time for at least one detonation point, plane, cylinder
or sphere.
Initiation Time
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
519
AUTODYN User Manual
Enter the initiation time in field (unless you chose to have it computed).
Limit range of application?
Check this box if you want to limit the range of application of the detonation point
(extra dialog is presented).
Range will Include / Exclude region.
For each Part, you can specify an index range that is used to limit the range of
application of the detonation point.
Select whether you want the index range to specify the included region or the
excluded region.
Part list
This window lists all the Parts in your model. Select a Part in this window to limit its
range of application.
IJ range
Enter the IJ range you want to use to limit the range of application of the detonation
point in the fields provided.
520
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Detonation (2D) - Line
This window lets you define a line of detonation.
X/Y Coordinate.
Enter the X and Y coordinates for the two end points of the line.
Initiation Time
Enter the initiation time in field (unless you chose to have it computed).
Limit range of application?
Check this box if you want to limit the range of application of the detonation point
(extra dialog is presented).
Range will Include / Exclude region.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
521
AUTODYN User Manual
For each Part, you can specify an index range that is used to limit the range of
application of the detonation point.
Select whether you want the index range to specify the included region or the
excluded region.
Part list
This window lists all the Parts in your model. Select a Part in this window to limit its
range of application.
IJ range
Enter the IJ range you want to use to limit the range of application of the detonation
point in the fields provided.
522
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Detonation (2D) - Circle
This window lets you define a detonation circle (detonation propagates radially
inward and outward from the surface of the circle).
Center (X,Y)
Enter the X and Y coordinates of the center of your circle in the fields provided.
Radius
Enter the radius of your circle in this field.
Initiation Time
Enter the initiation time in field (unless you chose to have it computed).
Limit range of application?
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
523
AUTODYN User Manual
Check this box if you want to limit the range of application of the detonation point
(extra dialog is presented).
Range will Include / Exclude region.
For each Part, you can specify an index range that is used to limit the range of
application of the detonation point.
Select whether you want the index range to specify the included region or the
excluded region.
Part list
This window lists all the Parts in your model. Select a Part in this window to limit its
range of application.
IJ range
Enter the IJ range you want to use to limit the range of application of the detonation
point in the fields provided
524
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Detonation (2D) - Manual
This window lets you manually define initiation times for blocks of elements.
Part List
The top box lists all the Parts in your model. Select the Part you want to define
initiation time for in this list.
IJ range
Specify the IJ range for a the block of elements to which you want to apply an
initiation time.
Initiation time
Enter the initiation time that will be applied to all elements in the block in this field.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
525
AUTODYN User Manual
Detonation (3D)
Detonation (3D)
This window lets you set the locations where explosives will be detonated /
deflagrated.
Detonations / Deflagrations
The box at the top of the window shows you a list of the current detonations /
deflagrations you have defined. You can select from this list.
Point
Press this button to define a detonation point.
Plane
Press this button to define a detonation plane.
Cylinder
Press this button to define a detonation cylinder.
Sphere
Press this button to define a detonation sphere.
Manual
Press this button to manually define initiation times for blocks of elements..
526
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Delete
Press this button to delete the selected detonation definition
Review
Press this button to review information for all detonation definitions.
Path
Select whether you want detonation times to be calculated using direct or indirect
paths.
Direct Path : Detonation times are computed from straight line paths from
detonation points. This is the most accurate method, but is only valid if the
straight line paths are through the explosive material.
Indirect Path : Detonation times are calculated from shortest paths through
explosive material. Paths are automatically computed around inert materials
(e.g. wave shapers).
Plot detonation points
Check this box if you want to see the location of detonation points in the view panel.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
527
AUTODYN User Manual
Detonation (3D) - Point
This window lets you define a detonation point.
X/Y/Z Coordinates.
Enter the X/Y/Z coordinates of the detonation point in these fields.
Compute Initiation Time?
Select whether you want to specify a detonation time, or have it computed by
AUTODYN.
If selected, AUTODYN will compute the detonation time using paths through the
explosive from other detonation points.
You must specify the initiation time for at least one detonation point, plane, cylinder
or sphere.
Initiation Time
528
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Enter the initiation time in field (unless you chose to have it computed).
Limit range of application?
Check this box if you want to limit the range of application of the detonation point
(extra dialog is presented).
Range will Include / Exclude region.
For each Part, you can specify an index range that is used to limit the range of
application of the detonation point.
Select whether you want the index range to specify the included region or the
excluded region.
Part list
This window lists all the Parts in your model. Select a Part in this window to limit its
range of application.
IJK range
Enter the IJK range you want to use to limit the range of application of the detonation
point in the fields provided.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
529
AUTODYN User Manual
Detonation (3D) - Plane
This window lets you define a detonation plane.
Plane
Select whether you want to define an X, Y or Z detonation plane.
X/Y/Z Coordinate.
Enter the X, Y or Z coordinate of the plane in this field.
Initiation Time
Enter the initiation time in field (unless you chose to have it computed).
Limit range of application?
Check this box if you want to limit the range of application of the detonation point
(extra dialog is presented).
530
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Range will Include / Exclude region.
For each Part, you can specify an index range that is used to limit the range of
application of the detonation point.
Select whether you want the index range to specify the included region or the
excluded region.
Part list
This window lists all the Parts in your model. Select a Part in this window to limit its
range of application.
IJK range
Enter the IJK range you want to use to limit the range of application of the detonation
point in the fields provided.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
531
AUTODYN User Manual
Detonation (3D) - Cylinder
This window lets you define a detonation cylinder (detonation propagates radially
inward and outward from the surface of the cylinder).
Axis
Select the axis (X, Y or Z) to which the axis of symmetry of your cylinder will be
parallel.
Radius
Enter the radius of your cylinder in this field.
Center Coordinates.
Enter the two coordinates for the center of your cylinder in the fields provided.
Initiation Time
532
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Enter the initiation time in field (unless you chose to have it computed).
Limit range of application?
Check this box if you want to limit the range of application of the detonation point
(extra dialog is presented).
Range will Include / Exclude region.
For each Part, you can specify an index range that is used to limit the range of
application of the detonation point.
Select whether you want the index range to specify the included region or the
excluded region.
Part list
This window lists all the Parts in your model. Select a Part in this window to limit its
range of application.
IJK range
Enter the IJK range you want to use to limit the range of application of the detonation
point in the fields provided.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
533
AUTODYN User Manual
Detonation (3D) - Sphere
This window lets you define a detonation sphere (detonation propagates radially
inward and outward from the surface of the sphere).
Center Coordinates.
Enter the coordinates for the center of your sphere in the fields provided.
Radius
Enter the radius of your sphere in this field.
Initiation Time
Enter the initiation time in field (unless you chose to have it computed).
Limit range of application?
534
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Check this box if you want to limit the range of application of the detonation point
(extra dialog is presented).
Range will Include / Exclude region.
For each Part, you can specify an index range that is used to limit the range of
application of the detonation point.
Select whether you want the index range to specify the included region or the
excluded region.
Part list
This window lists all the Parts in your model. Select a Part in this window to limit its
range of application.
IJK range
Enter the IJK range you want to use to limit the range of application of the detonation
point in the fields provided.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
535
AUTODYN User Manual
Detonation (3D) - Manual
This window lets you manually define initiation times for blocks of elements.
Part List
The top box lists all the Parts in your model. Select the Part you want to define
initiation time for in this list.
IJK range
Specify the IJK range for a block of elements to which you want to apply an initiation
time.
Initiation time
Enter the initiation time that will be applied to all elements in the block in this field.
536
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parallel
Parallel
This panel lets you set up your model for parallel processing For more additional
information about setting up a parallel analysis see also the AUTODYN Parallel
Processing Tutorial Version 12.0.
Manual (Structured Parts)
The structured Lagrangian solver is decomposed along its grid lines. These provide
an easy and obvious method to decompose any structured Parts whilst maximizing
the load balancing and minimizing the communication.
Activate parallel processing
Check this box to activate parallel processing. If this box is checked, your model will
be executed in parallel when you press
Host Configuration Sets
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
537
AUTODYN User Manual
This input lets you configure the hardware you want to use for parallel processing by
defining one or more Host Configuration Sets.
These configuration sets are saved independently of your model. Any sets you
create will automatically be available for other models you have set up.
The box at the top shows the name of the current Host Configuration Set. The pulldown menu for this box lets you change the current Host Configuration Set to any
other Set you have defined.
Add
Press this button to define a new Host Configuration Set.
Modify
Press this button to modify the current Host Configuration Set.
Copy
Press this button to copy an existing Host Configuration Set to a new Host
Configuration Set.
Delete
Press this button to delete the current Host Configuration Set.
Decomposition Sets
This input lets you define the domain decompositions you want to use for parallel
processing by defining one or more Decomposition Sets.
Unlike Host Configuration Sets, Decomposition Sets are specific to your model.
The box at the top shows the name of the current Host Decomposition Set. The pulldown menu for this box lets you change the current Decomposition Set to any other
Set you have defined.
Add
Press this button to define a new Decomposition Set. Enter the name of your
new Decomposition Set in the Selected decomposition field.
Delete
Press this button to delete the current Decomposition Set.
Subdomains
538
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Press this button to decompose the Parts of your model into sub-domains
(SPH parts are decomposed automatically).
Task Assignments
Press this button to assign the sub-domains to Tasks performed on each CPU.
Automatic (Unstructured Parts)
The automatic domain decomposition for unstructured parts is conducted using a
recursive bisection method. This takes into account the geometric location of
elements, the element type and the element density.
Set Decomposition
Press this button to select the parts to be included in decomposition.
Plot parallel decomposition
Press this button to see the domain decomposition and task assignments for
the current Decomposition Set.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
539
AUTODYN User Manual
Parallel - Add / Modify
This window lets you create a new Host Configuration or modify an existing Host
Configuration Set
Configuration Set
If you are creating a new Host Configuration Set, enter its name in this field.
If you are modifying an existing Host Configuration Set, the name of the current
configuration set is displayed in this field.
540
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
List of Hosts
The large box lists all the Host machines currently included in this Host Configuration
Set. You can select a host in this list.
Add Host
Press this button to add a host to this Host Configuration Set (the Host Data fields
are cleared to let you input data for the new host).
Delete
Press this button to delete the selected host from this Host Configuration Set.
Host Data
Host Name
Enter the name of the host machine in this field
Number of Tasks
Enter the number of tasks to be run on this host. If you set the number of tasks
equal to the number of CPUs, one task will automatically be run on each CPU
(this is usually the most efficient way to run parallel calculations).
Executable path
Enter the path where the AUTODYN executables are located (usually in a
shared directory).
Speed factor
If the hosts in your Host Configuration Set have different speeds, set the speed
factor for each host in this field.
If all hosts have the same speed, set all speed factors to the same value (any
value is OK).
Number of CPU
Enter the number of CPUs on the host in this field.
Memory
Enter the amount of memory on the host in this field (this information is not
currently used).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
541
AUTODYN User Manual
Parallel - Copy
This window lets you copy an existing Host Configuration Set to a new or existing
Host Configuration Set.
Select the Host Configuration Set you want to copy in the top pull-down menu.
In the lower pull-down menu, select the Host Configuration Set to which you want to
copy the data (to copy to a new Configuration Set, select <New>, then, in the
Parallel Processing panel, rename the Configuration Set to the name you want to
use).
Press
542
to perform the copy.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parallel - Sub-domains
This window lets you decompose the Parts of your model into sub-domains for
parallel processing (SPH parts are decomposed automatically).
You can decompose each grid-based Part in you model into smaller blocks, called
sub-domains, that can be assigned to different tasks (on different hosts) for
processing.
For each Part, these blocks are formed by defining planes in the I, J and K direction
where cuts are made to form the sub-domains.
Parts List
The top box lists the model Parts that you can decompose for parallel processing.
You can select a Part in this list.
Number of Sections
Enter the number of sections into which you want the selected part divided in I, J and
K directions.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
543
AUTODYN User Manual
Dividing Planes
Enter the I, J and K values for the dividing planes in the three index directions (the
default values place the dividing planes evenly through the grid).
The example above would decompose the PROJECTILE Part into 24 sub-domains
544
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parallel - Task Assignment
This window lets you assign sub-domains to Tasks performed on each CPU.
The efficiency of parallel processing is very dependent on distributing sub-domains
among the tasks so that each task has approximately the same amount of work
(computing) to do.
Automatic / Manual assignment.
If you select Automatic assignment of Sub-domains to Tasks, AUTODYN will
automatically distribute sub-domains among the tasks, using load-balancing
algorithms. You do not need to input any further data if you use this option.
If you select Manual assignment of Sub-domains to Tasks, further input dialog is
presented :
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
545
AUTODYN User Manual
Parts List
The box at the top of the window lists the Parts whose Sub-domains you need to
assign. You can select a Part in this list.
Review Assignments
Press this button to view a list of all Sub-domains and the tasks to which they are
assigned.
Balance Automatically
If you select this option, you can invoke the load-balancing algorithms use if
you had selected Automatic assignment of the Sub-domains to Tasks, to
distribute your Sub-domains over a specific number of Tasks.
Number of tasks
Enter the number of Tasks over which you want to distribute your Subdomains.
Balance Now
546
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Press this button to perform the distribution.
Manually assign to tasks
If you select this option, dialog is presented which lets you manually assign
blocks of Sub-domains to a specific Task :
Block to be assigned
In the fields provided, specify the I, J and K section range for the block of Subdomains you want to assign to a Task.
Assign to Task
Enter the Task # to which you want to assign the block of Sub-domains in this
field.
Assign Now
Press this button to assign the specified block to the specified Task.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
547
AUTODYN User Manual
This procedure can be repeated as many times as you want, to assign blocks
of Sub-domains to Tasks.
548
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parallel Automatic Decomposition
Parts to be decomposed
Select the parts to be decomposed from the list of unstructured parts (by default all
unstructured parts will be selected).
Start Task
Enter the start task.
Number of tasks
Enter the number of tasks
Decompose now
Press the Decompose Now button to automatically define the task on which each of
the elements contained in the selected Parts will be assigned.
Examples
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
549
AUTODYN User Manual
Single unstructured Part
Select Part
Start Task = 1
Number Tasks = 8
All Parts Unstructured
One rigid material
Select All Parts
Start Task = 1
Number Tasks = 1
3 Unstructured Parts
1 Euler Part (Structured)
Manual assignment
of Euler Part to Task
1
Automatic
assignment of 2
unstructured Parts
(rod and first target)
o Start Task = 2
o # Task = 2
Automatic assignment of
unstructured Part (second
target)
o Start Task = 4
o # Tasks = 1
550
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Automatic decomposition of Euler-FCT parts
The automatic decomposition algorithm has been extended to incorporate Euler-FCT
parts in addition to its present ability to handle unstructured grids.
This facilitates the decomposing of complicated Euler-FCT/Lagrange coupled
models – the user need only stipulate the number of tasks over which the model
should be assigned and AUTODYN will automatically produce a decomposition
configuration with good load balancing qualities and minimal inter-processor
communication. Furthermore, to further enhance the efficiency of coupled
calculations the subdomains of the Lagrange structure will be placed on the same
processor, so decreasing the necessary inter-processor communication.
To automatically decompose an Euler-FCT model, go to the Parallel dialog panel as
seen below, activate parallel processing and add a new decomposition set which in
this instance is called two:
Press the Set Decomposition button and all Euler-FCT parts will be shown in the
Automatic Decomposition dialog window:
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
551
AUTODYN User Manual
Input the number of tasks you want to decompose the part over and press the
Decompose Now button. In this case the number of tasks is two and the following
decomposition can be viewed:
More complicated decompositions can also be easily achieved. Here the part is
decomposed over 16 tasks:
552
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
As previously stated the new algorithm allows easy decomposition of complicated
coupled models which include Euler-FCT and unstructured Lagrange Parts. The
model below contains a brick structure in which an explosion is occurring. The brick
structure is modeled using Lagrangian parts, whilst the explosion in air is modeled
using an Euler-FCT part. Here, only part of the Euler-FCT part is shown for
illustration purposes, the Euler-FCT part extends above the brick structure.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
553
AUTODYN User Manual
The Decomposition Set window dialog will contain all of the parts and by default
they will all be highlighted:
By choosing decomposing the model over 4 tasks, the various parts can be assigned
to the available processors whilst ensuring efficient parallel computations:
If the user wishes to override this decomposition then the Euler-FCT part can still be
manually assigned as before.
554
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Parallel - Decomposition of beam parts
AUTODYN-3D simulations including beam elements can be run in parallel.
Structured Beams
For the parallel computation, each structured Beam Part is considered as a single
sub-domain and can be assigned to a specific task for the parallel simulation. Note
that individual structured Beam Parts cannot be decomposed into multiple subdomains.
Unstructured Beams
For parallel computation unstructured Beam Parts can
decomposed, similar to all other unstructured Lagrange Parts.
be
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
automatically
555
AUTODYN User Manual
Note that parallel computations including beam elements can currently run with all
join and contact options, with the exception of edge on edge contact. This later
option is likely to be available in the near future.
556
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Output
Output
Output
This window lets you set the type of output you want from your calculation.
Interrupt
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
557
AUTODYN User Manual
Set the frequency at which your calculation is interrupted (stopped) for you to plot,
review and examine.
Refresh
Set the frequency at which your plot in the view panel is refreshed.
Save
The most important type of output you will want is data written to Save files.
Cycle / Times
Select whether you want data written at a set cycle frequency or time frequency.
Start cycle / time
Enter the cycle time that you want your first Save file to be written.
End cycle / time
Enter the cycle or time that you want your last Save file to be written.
If you are not sure how long you want to run your problem, enter a large number in
this field, then you won't have to come back and change it later.
Increment
558
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Enter the frequency you wish files to be written between the start cycle / time and the
end cycle / time.
Select Variables
Press this button to select the structured or unstructured variables you want written
to the Save file.
For the structured solvers, the majority of variables is automatically selected and
cannot be de-selected. This is because the memory for these variables is always
allocated, even if the variable is not being used in a Part.
For the unstructured solvers, the full list of potential variables that can be used is
presented. Only a small number of variables are pre-selected as commonly used
variables. The selection of additional variables is up to the user and must be made
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
559
AUTODYN User Manual
prior to execution of the model (at cycle zero). Only those variables selected will be
available for output (contour, examine etc) Note that on execution, if a particular
combination of element type and material requires a variable to be saved that has
not been selected, AUTODYN will automatically add this to the list.
Also note that the unstructured solves, some of the variables are never allocated
physical memory, instead they are reconstructed from other variables that are
allocated and stored in memory. An example of this would be the absolute velocity;
this can be reconstructed from the nodal velocities hence does not require
independent storage.
A similar list is also presented under the History, Variables option.
Note that the selection of additional post-processing variables will result in higher
memory usage and file sizes. If a significant number are selected, some degradation
in runtime performance can also be expected.
Press
alongside any of the remaining output options to reveal the input fields for
that option:
Review Variables
Select this button to create an html page of structured or unstructured variables.
After selection of the Review button first a selection window appears where the type
of variable for review needs to be selected, e.g. 2D or 3D, structured or unstructured.
An html page will be created that shows a list of requested variables and their
description.
560
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Results File
Set the frequency at which results files are written out.
Select Results Variable
Press this button to select the grid variables written to the result file.
History
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
561
AUTODYN User Manual
Set the frequency at which history data is written.
Select Gauge Variables
Select this button to choose which structured and unstructured variables to write to
the history data file.
Select Part Summary Variables
Select this button to choose which part summary variables to write to the history data
file.
Capture image
Set the frequency at which automatic image captures are done.
Print
Set the frequency at which printed data is written.
562
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Print Format
Press this button to select the formatting of the information written to the print file.
Grid Variables
Press this button to select the grid variables written to the print file.
Log file
Turn the Log file on or off.
Call EXEDIT
Set the frequency at which subroutine EXEDIT is called.
Run EXEDIT now
Press this button to call the EXEDIT user subroutine
Field output
Set the frequency at which field output is written for weak coupling analyses.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
563
AUTODYN User Manual
Output-Part Summary Variables
The Part summary variable includes three sets of optional data.
Contact energy
Hourglass energy
External forces
This data is accumulated per Part and is available for review via the print file (using
the energy summary option) or as time history data (using the Part summary option).
Note that by default, these additional variables are not available for history plotting.
The variables must be activated using the Output, History, Select Part Summary
Variables option.
564
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Hourglass energy
The 2D and 3D Lagrangian volume and shell elements in AUTODYN use hourglass
control to remove zero energy modes of deformation. The forces of the hourglass
control algorithms dissipate energy in resisting the zero energy modes of
deformation.
In AUTODYN, this energy is calculated and accumulated in the element internal
energy. In version 6.1, the hourglass energy is now also accumulated independently
to the internal energy to allow users to interrogate and assess the relevance of
hourglass energy in a simulation.
Contact energy
Contact energy is accumulated on a per part basis as
In the absence of friction, the contact energies of two Parts interacting should be
equal, but opposite sign, hence have very little contribution to the energy of the
overall system. Large imbalances in contact energy are indicative of poor model
setups.
For the purpose of energy accountancy, the contact energy is added to the work
done on the system.
External forces
The resultant external forces on a Part can now be easily extracted from a simulation
by selecting the appropriate components as Part summary variables. The
components available are
X/Y/Z contact forces
External forces applied to a Part from Lag/Lag contact
X/Y/Z coupling forces
External forces applied to a Part from Euler/Lag coupling
X/Y/Z boundary forces
External forces applied to Part from all boundary conditions
X/Y/Z total external forces
The sum of all external forces acting on a Part
Note: External forces are not extracted for polygon based Euler Lagrange coupling in
2D
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
565
AUTODYN User Manual
Example mine blast simulation highlighting source of loading (blast from coupling, impulse from soil
ejecta) using new Part summary options
566
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Outputs-Results Files
The capability to output results files, which contain a reduced amount of information,
is available in AUTODYN-3D. This allows the post-processing of large simulations
on computers with limited resources. Results Files cannot be used for restarting a
problem. The frequency of the results files is independent of the SAVE files. The
control for results file output is located in the Output panel, under Results Files:
From here, the frequency of results file output and the variable to save into the file
are selected. Note that only a limited set of results variables are selected by default.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
567
AUTODYN User Manual
When a simulation is performed with the results file option switched on, a new
directory will be created in the directory where the simulation file is located. This
directory will have the name <ident>_adres. For example, the results files from a
simulation with model name ben3d1_0.ad will be stored in a sub-directory with name
ben3d1_adres.
Results files have extension adres, and the model name is appended with two
numbers:
The first number is the cycle from which the simulation began.
The second number being the current cycle number.
For example, a results file ben3d1_10_25.adres indicates that the results file
contains data at cycle 25 from the simulation ben3d1 that began at cycle 10.
Note that the start cycle for each sequence of results files is stored in a file
<ident>_<cycle>.ad_base. For example ben3d1_10.ad_base. This base file is
essential for post processing using results files and must not be deleted. The base
file contains data required for producing graphic output that for efficiency is not
repeated in each of the Results Files.
To use the results files for post-processing of a simulation, the option under the File
menu option should be
568
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Once a results file has been selected, various options within AUTODYN will be
inactive, since no model alteration is possible. The cycle drop-down menu from the
Plots panel is automatically updated to represent the cycles of results files that can
be loaded. In order to switch back to full restart files simply load in a restart (cycle)
file.
The adres directory is designed to be independent of any other files, in order to
share the results with colleagues simply transfer the directory.
Post-processing using results files is significantly more memory efficient than from a
restart file. Using results files, AUTODYN only loads the data required to generate
the requested Plots. The efficiency improvement will be problem dependant
however a 2 to 3 times increase in the size of model that can be post-processed on a
32-bit Windows system can be expected.
To use the results files to create an animation of the simulation, select the option
"Scan for results files from this ident" from the Generate Multiple Slides panel.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
569
AUTODYN User Manual
570
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
User Variables
User Variables
This panel lets you set up grid variables that you can use when programming your
own user subroutines.
User Variable List
The top box lists the user variables you have currently defined. It shows the name
you have assigned to the variable and whether or not the variable is written to restart
(Save) files, rezoned and transported (in Euler). You can select a variable in this list.
Add
Press this button to add a new user variable.
Modify
Press this button to modify the selected user variable.
Delete
Press this button to delete the selected user variable.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
571
AUTODYN User Manual
User Variables - Add/Modify
This window lets you add a new user variable or modify the selected user variable.
Select user variable
You can define up to 20 user variables. Use this pull-down menu to select the user
variable you want to define or modify.
Activate
Check this box to activate (define) the selected user variable.
User variable name
Enter the name you want to use for your user variable.
Restart
Check this box if you want the user variable to be written to the restart (Save) file.
Rezone
Check this box if you want the user variable to be included in the list of variables
that are automatically rezoned.
Transport
Check this box if you want the user variable to be included in the list of variables that
are automatically transported in Euler Parts.
Nodal Variable
For the unstructured solvers, element and nodal quantities are stored independently.
Check this box to define a user variable that is associated with a node, rather than
572
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
an element for the unstructured solvers. Note that nodal user variable data can only
be interrogated via examine and time history plots. Contour plots are not available.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
573
AUTODYN User Manual
Controls
Controls
This panel lets you define solution controls for your model.
Wrapup Criteria
These controls are the only ones visible when you open this panel for the first time.
This is because you must specify some of the parameters.
(all other control inputs have default values that are usually OK).
Cycle limit
574
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Enter the maximum number of cycles you want your problem to run (enter a
large integer if you don't want your problem to stop on a cycle limit).
Time limit
Enter the maximum time you want your problem to run (enter a large number e.g. 1.0E20 - if you don't want your problem to stop on a time limit).
Energy fraction
Enter the energy fraction you want to use to stop your problem if the energy
error gets too large. The default value of 0.05 causes you problem to stop if the
energy error exceeds 5%.
Energy reference cycle
Enter the cycle # at which you want AUTODYN to start checking for an energy
error.
Press
alongside any of the remaining options to reveal the input fields for that
option :
Timestep Options
These options control the timestep AUTODYN uses to run your problem.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
575
AUTODYN User Manual
Start time
Enter the start time for your problem.
Minimum timestep
Enter the minimum timestep you want to use.
If the timestep drops below this value, your problem will be terminated.
If you leave this field zero, the minimum timestep will be set to 1/10 of the Initial
timestep.
Maximum timestep
Enter the maximum timestep you want to use.
AUTODYN will use the minimum of this value or the computed stability
timestep.
Initial timestep
Enter the initial timestep you want to use.
If you leave this field zero, the initial timestep will be set to 1/2 the computed
stability timestep.
Safety factor
It is not wise to run problem at the stability limit, so a safety factor is applied to
the computed stability timestep.
Enter the stability factor you want to use.
The default value (0.6666) is good for all problems, but you may want to
increase this value to 0.9 in some cases to use a larger timestep (0.9 is a good
value for most Lagrangian calculations).
Method of calculating characteristics zone
Three options are available for calculating the effective zone size used in the
timestep calculation. By default, all models will use a zone size calculation
based on element diagonals. If the user wishes to obtain improved efficiency,
especially in 3D simulations, the zone size calculation can be switched to one
of two alternative options (based on either distances between opposing face
centers or closest face centers).
576
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
To obtain the optimal time step for HEX solid elements the method of
calculating the characteristic zone dimension needs to be set to Opposing
Faces option instead of the default Diagonal option.
Experience to date has shown that these options can significantly improve the
efficiency of Lagrange simulations, especially in 3D. However, in certain
circumstances when cells become highly distorted instabilities have been
observed causing the calculation to terminate with high energy errors. The
correct choice of erosion strain can reduce these problems. It is therefore
recommended that users only utilize either of these non-default zone_size
options if efficiency is critical.
Automatic Mass Scaling
Mass scaling is an artificial (numerical) mechanism for increasing the CFL
(Courant-Friedrichs-Lewy) timestep of individual elements that govern the
maximum allowed timestep of explicit transient dynamic solutions in
AUTODYN. Increasing the timestep has the obvious benefit of reducing the
number of cycles required to run a simulation to a given point in time.
Educated use of this option can therefore result in significant improvements in
efficiency.
Damping Options
These options control the magnitude of damping applied to your problem.
The default values are best for most problems.
Be very careful if you increase these values, they can significantly change your
solution.
Quadratic viscosity
Enter the coefficient of quadratic viscosity you want to apply to shocks
(compression waves).
Linear viscosity
Enter the coefficient of linear viscosity you want to apply to shocks
(compression waves).
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
577
AUTODYN User Manual
Linear viscosity in expansion
Choose whether you also want to apply the linear viscosity in expansion.
Hourglass damping
Enter the coefficient of hourglass damping that you want to apply to Lagrangian
elements.
Static damping
A static damping constant may be specified which changes the AUTODYN
calculation from a dynamic solution to a relaxation iteration converging to a
state of stress equilibrium. For optimal convergence, the value chosen for the
constant, R, may be defined by:
R=2*timestep/T
where timestep is the expected average value of the timestep and T is longest
period of vibration for the system being analyzed.
Solver Options
Method for Lagrange/ALE density update
The element density can be updated each cycle using one of two methods;
incrementally from the change in volume relative to the last cycle or
recalculated based on the current mass and volume of the element. If the
incremental change in volume over a cycle is small, it can be more accurate to
use the incremental approach rather than the total approach to updating the
density. This especially applies to the single precision version of AUTODYN.
Hence the options are:
Automatic
- AUTODYN decides whether it needs to do an incremental
update or not based on the change in volume.
Incremental
578
- Force AUTODYN to always use the incremental update.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Total
- Force AUTODYN to always recalculate the density.
Method for Euler Strain rate calculation
For multi-material Euler there are two methods to compute strain rates.
Weighted. For multi-material Euler analysis, involving materials with strength,
strain rates need to be calculated to compute the increment in strain from cycle
to cycle. The strain rates are derived from the velocity gradients, which are
obtained by an element surface integration of the velocity. Using the Weighted
option the face velocity that is used in the integration is a density weighted
average of the element velocity on both sides of the face.
This is the default option and provides the most accurate strain rate calculation.
Averaged. With this option the face velocity used in the integration is a simple
average of the element velocity on both sides of the face and provides less
accurate results than the Weighted option. Until AUTODYN Version 6.1 the
Averaged option was the only option available, and can be used to reproduce
old results. Also models that are generated before Version 6.1 will still run
using the Averaged method.
Method for Euler pressure calculation
For multi-material Euler cells containing two or more materials, there are two
methods for calculating the resultant cell pressure:
Equilibrium
-
An iterative procedure is used for each material in a
cell to establish a single pressure consistent with the
equation of state and conditions of each material in
the cell. This method is currently only applied if there
are two materials in the cell and these materials are
defined by ideal gas, or fully burnt JWL material. If
this criterion is not met in a cell the pressure
averaging option is used.
Average
-
The resultant cell pressure is calculated from a
weighted average of the pressure of the individual
materials in the cell. The weighting algorithm takes
account of both the volume fraction of each material
and the relative stiffness of each material. This is the
default method.
Global Cutoffs
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
579
AUTODYN User Manual
These options let you set global cutoffs.
The default values are usually good if you are using the default units (mm,mg,ms).
You may want to change one or more of these defaults if you are using some other
set of units.
Minimum Velocity
Enter the minimum velocity cutoff you want to use.
If any velocity drops below this value it is set to zero.
Maximum Velocity
Enter the maximum velocity you want to use.
If any velocity rises above this value it is set to this value.
This option is sometimes useful if your problem develops high velocities, which
result in a small timestep, in regions that are not important to your solution.
Radius cutoff
Enter a value for the radius cuttoff for 2D axial models.
If a Lagrangian node is inside this radius at the start of your calculation, it is
placed on the axis of symmetry.
If a Lagrangian node is outside this radius at the start of your calculation, it will
not be allowed to come closer than this radius to the axis of symmetry as your
calculation proceeds.
SPH Cutoffs
These options let you set SPH cutoffs.
580
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
The default values are usually good if you are using the default units (mm,mg,ms).
You may want to change one or more of these defaults if you are using some other
set of units.
Limit density / Delete node
If the density of an SPH node drops below the minimum density or above the
maximum density, you have the choice of either limiting the density to the
cutoff density or deleting the node. Make your choice here.
Minimum density
Enter the minimum cutoff density for SPH nodes.
Maximum density
Enter the maximum cutoff density for SPH nodes.
Gravity
This option lets you set gravitational components for your model.
X / Y / Z acceleration
Enter the X Y and Z components of gravity in these fields.
The gravitational acceleration components will be applied to all Parts present in
the model.
Transport
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
581
AUTODYN User Manual
These options relate to the transport of material in various Solvers.
Material velocity timestep safety factor
Enter the timestep safety factor for material velocities.
In the velocity used to calculate the stability timestep is c+u, where c is the
soundspeed of the material and u is its physical velocity.
If u is of the order of or greater than c, then using c + u/f can give more stable
results, where f is the safety factor.
Euler-FCT
Select the type of transport algorithm that is used for Euler-FCT calculations
from this pull-down menu. The default setting is multi-dimensional where all
three spatial dimensions are solved simultaneously which is more efficient and
helps to maintain symmetric flow fields. The alternative is Operator Split where
each spatial dimension is solved in turn.
ALE/Euler Energy
During a computational Euler cycle mass, momentum and energy is being
transported (fluxed) from element to element. This option determines if total
energy or internal energy is being transported.
Total. This option conserves the total energy (kinetic + internal energy)
during transport. This is the most robust and accurate option and is the
default.
Internal. This option conserves the internal energy during transport. In
cases where the total energy transport doesn't provide an accurate
answer, e.g. material overheating or when the kinetic energy is
predominant, the Internal option might be chosen as an alternative.
Euler
This option determines which transport algorithm will be used for multi-material
transport.
SLIC. When material is being transported out of an element that contains
multiple materials or voids, it is necessary to use special rules to
determine the amount of each material being transported, because the
only information available for the transport algorithm is the fraction of
each material in the individual elements. In AUTODYN the Simple Lime
Interface Calculation (SLIC) method is used which uses a small number
of stereotypes of mixed material element topologies. The SLIC algorithm
is the default and works well for all multi-material Euler analysis.
582
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Updated SLIC. Isolated small parts of material smaller than an element
do not move through the mesh at the correct velocity. They tend to stop
moving while surrounding material rushes by. The Updated SLIC option
will transport these small material fractions with statistically the correct
velocity. This option should be used with care, because it can have some
undesirable side effects. It is possible for these small material fragments
to "tunnel" through other multi-material Euler objects like walls or plates
and emerge at the other side.
Global Erosion
These options define global erosion criteria for all elements in the model. The
global erosion options are only available for unstructured elements.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
583
AUTODYN User Manual
Controls-Mass scaling
Mass scaling is an artificial (numerical) mechanism for increasing the CFL (CourantFriedrichs-Levy) timestep of individual elements that govern the maximum allowed
timestep of explicit transient dynamic solutions in AUTODYN. Increasing the
timestep has the obvious benefit of reducing the number of cycles required to run a
simulation to a given point in time. Educated use of this option can therefore result
in significant improvements in efficiency.
The primary use of mass scaling is to increase the CFL timestep of a small number
of very small (or stiff) elements in the model, which otherwise would have controlled
the timestep for all elements. Using this option, AUTODYN will automatically add
artificial mass to individual elements to ensure that their CFL timestep is at least
equal to a value defined by you. Mass scaling should only be used if the increased
inertia of the scaled elements does not significantly affect the results of the
simulation.
Mass scaling can also be used to increase the CFL timestep of elements that
become highly distorted during the simulation. Extreme care should be taken to
ensure that results obtained remain physical.
Mass scaling is activated under Controls, Timestep and the input parameters are
defined as follows:
Automatic
Mass Scaling
Frequency
(cycles)
-
Activate automatic mass scaling
-
Min. CFL
timestep
Max. element
scaling
-
Max. part
scaling
-
Cycle frequency that AUTODYN will adjust the element mass
scaling. Recommended default is only at start-up (cycle 0).
Post cycle 0 adjustment will only take place for solid
elements.
Mass scaling is applied to all elements with a CFL timestep
less than the specified value
Maximum mass scaling factor that can be applied to an
element. Default is 100 (equating to 100 times original
mass). If this limit is exceeded, no more mass is added to
this element.
Maximum added mass that is allowed for an AUTODYN Part,
as a fraction of the original Part mass. Default is 0.05
(equating to 5% of the original mass. If this value is
exceeded, the simulation will terminate with an error
message.
-
Two new element variables have been introduced with the development. These
variables are automatically activated when mass scaling is selected:
TIMESTEP:
MASS.SCALE:
584
The CFL timestep for the element
The mass scale factor applied to the element.
(1.0 indicates zero added mass, 2.0 indicates 100% added
mass etc.)
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
A typical procedure to invoke mass scaling would be as follows
Activate mass scaling retaining all the default parameters
Run the simulation for 1 cycle
Plot a contour of Timestep and review the element CFL timesteps. Identify a
suitable timestep for mass scaling. The value chosen should exclude the
majority of elements from mass scaling, and especially those in regions
critical to the simulation results
Re-load cycle zero
Enter the selected Min CFL Timestep under Controls, Timestep
Run the simulation
Minimum CFL timestep = 2.0e5
Mass Scale CFL timestep =
1.0e-4
=>
Minimum CFL timestep = 1.0e4
Small number of elements are
mass scaled to maximum
factor of 5.0
Timestep increased by factor of 5, for the addition of 0.02% of the Part mass
Example application of mass scaling
Important notes and limitations:
Mass scaling will only be applied to Unstructured Elements/Parts
Mass scaling is only applied to elements filled with materials which use a
Linear or Hyperelastic equation of state
The actual timestep used in a simulation will generally be lower than the Min
CFL timestep you define
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
585
AUTODYN User Manual
A safety factor is applied to get the actual timestep (default = 2/3)
The timestep used at cycle 1 of the simulation is additionally reduced
by a factor of 2. The timestep is then allowed to increase by a
maximum of 10% per cycle.
o Large velocities can affect the timestep at cycle 0
o Other features of the code will influence the timestep, such as artificial
viscosity, blending, Gap contact.
For Beams and Tet ANP elements, the minimum CFL timestep will be increased by
using mass scaling. However, due to nodal averaging of some quantities that
influence the timestep, the actual user defined CFL timestep may not be achieved.
A summary of the contribution of mass scaling applied to the model can be obtained
through
o Plotting a contour of variable Mass Scale. This is a ratio of current
mass to original mass (with scaling).
o Review the .prt file output activated using Output, Print, Energy
Summary
o
o
586
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
AUTODYN User Manual
Controls - Global Erosion
A new global erosion option has been implemented that can be used to define global
erosion criteria for all elements in the model. The global erosion options are only
available for unstructured elements.
Three erosion criteria have been implemented and can be used in combination in an
analysis:
Global Erosion by Geometric Strain
o The user can define a single erosion strain that will be used for all
elements in the model.
 The minimum of the global erosion strain, and the local material
erosion strain (if specified) will be used to check for element
erosion.
 Global Erosion by Timestep
o The user can define a single erosion timestep that will be used for all
elements in the model.
 The maximum of the global and the local material based erosion
timestep (if specified) will be used to check for element erosion.
 Global Erosion by Failure
o The user can turn on erosion by material failure for all materials.
Using erosion by timestep will activate the element timestep variable which can be
used in post-processing.
Release 12.1 - © 2009 SAS IP, Inc. All rights reserved. – Contains proprietary and confidential information
of ANSYS, Inc and its subsidiaries and affiliates.
Published: 2009-11-5
587
Download PDF