This document describes how to perform submodeling in ANSYS Workbench v12.1 using APDL command blocks since it is not natively supported. The process involves setting up a global model, generating its solution, creating a submodel with cut boundaries, and using command blocks to map displacements between models while solving each independently. The example demonstrates the procedure and checks results for accurate boundary mapping.

1. Submodeling using
ANSYS Workbench
v12.1
Patrick Cunningham
1/18/2011
© 2009 CAE Associates

2. Submodeling in ANSYS Workbench
 Although submodeling using the ANSYS Workbench environment is not
currently supported at release v12.1 it can be accomplished using APDL
command blocks.
 The method involves setting up the global model and the submodel in the
same Workbench project as shown here.
2

3. Submodeling in ANSYS Workbench
 The general procedure is as follows:
1. Generate the solution on the global model using the Mechanical tool.
2. Create the submodel in a separate Mechanical window and use a command
block to generate a node file
file.
3. Go back to the global model and use command blocks to perform the cut
boundary interpolation forcing Mechanical to not regenerate the solution.
4. Go to the submodel and use a command block to read the cut boundary y
displacements.
5. Generate the submodel solution.
 One advantage to using Workbench for submodeling is that both the
global model and submodel can be open during the process. The v12
license manager will share the Mechanical license with the two models.
g
3

4. Submodeling in ANSYS Workbench
 The following example problem is used to illustrate the set up in detail
detail.
Submodel region
4

5. Submodeling in ANSYS Workbench
The submodeling method for Workbench v12 1 is as follows:
v12.1
1. Bring the CAD geometry into DesignModeler and defeature the global
model as needed. For illustration purposes the cut boundaries are
included in the global geometry model (not required)
required).
5

6. Submodeling in ANSYS Workbench
2.
2 Bring the DesignModeler geometry into the Mechanical tool Set up the
tool.
model as needed (material assignment, mesh control, loads, supports,
etc.).
6

7. Submodeling in ANSYS Workbench
3.
3 Add a command block to the Solution folder with a command to copy the
ANSYS result file to a known location using the /system command:
7

8. Submodeling in ANSYS Workbench
4.
4 Generate the solution for the global model:
8

9. Submodeling in ANSYS Workbench
5.
5 Return to the Project page and duplicate the DesignModeler geometry:
RMB
9

10. Submodeling in ANSYS Workbench
6.
6 Open the duplicate geometry item and cut out the submodel (suppress or
delete the remainder).
For this case a fillet was added to the submodel geometry.
10

11. Submodeling in ANSYS Workbench
7.
7 Drag and drop a new Structural Analysis system onto the submodel
geometry. Open the new Mechanical window, mesh the geometry and
create a Named Selection consisting of the cut boundary faces.
Note: Be sure to set the active unit system consistent with the global
model.
11

12. Submodeling in ANSYS Workbench
8.
8 Add two command blocks to the Static Structural folder of the submodel:
a. 1st pass – Write Node File
Selects the nodes attached to the Named Selection surfaces and writes a
node file to a user defined location Adds a /eof command to halt the solution
location.
process.
12

13. Submodeling in ANSYS Workbench
8.
8 Submodel command blocks – continued:
a. 2nd pass – Reads a cut boundary displacement file from a known location.
13

14. Submodeling in ANSYS Workbench
9.
9 Suppress the “2nd pass – Read CBD” command block and Solve to
2d CBD
generate the node file.
RMB - Suppress
14

15. Submodeling in ANSYS Workbench
10.
10 Return to the global Mechanical model and suppress the Solution
command block that copies the original result file.
RMB > Suppress
15

16. Submodeling in ANSYS Workbench
11.
11 Add a command block to the Static Structural folder that copies the
original result file back to the solution directory. Exit the solution
processor using the finish command to stop ANSYS from resolving the
global model. Do not use /eof.
16

17. Submodeling in ANSYS Workbench
12.
12 Add a command block to the Solution folder to generate a file with global
model displacements interpolated onto the cut boundary nodes.
Note: For the sake of simplicity the CBD file is written to the same
directory as the node file and the global .rst file
rst file.
node file CBD file
17

18. Submodeling in ANSYS Workbench
13.
13 Make sure that the 1st pass command block is suppressed and that the
2nd pass command blocks (Static Structural and Solution) are active.
14. Solve.
Active
Suppressed
Active
18

19. Submodeling in ANSYS Workbench
15.
15 Return to the submodel Mechanical window Suppress the command
window.
block used to write the node file in the first pass.
16. Add a command block in the Static Structural file reads the CBD file from
the specified directory
directory.
17. Solve.
Suppress
Add
19

20. Submodeling in ANSYS Workbench
 Check the submodel results for proper mapping of the displacements If
displacements.
the cut boundaries exist in the global model this is easily accomplished.
Otherwise cut plane displays and the result probe can be used as an
approximation.
20

21. Submodeling in ANSYS Workbench
 Use the result Probe to compare the stresses at the cut boundary Good
boundary.
agreement is an indication that the boundary is far enough away from the
stress concentration.
21

22. Submodeling in ANSYS Workbench
 The example models have been provided in the ANSYS archive file
v12_submodel_example.zip.
 The file should be opened using the File > Restore utility on the v12
project page
page.
22