Skip to main content

Defining Ansys Superelement SUB File Manually

Photo by  James Owen  on  Unsplash A surprisingly popular blog-post written here is Exporting Stiffness Matrix from Ansys . A sensible follow up question is what can one do with the exported stiffness matrix? In a recent Xansys Forum post, a question was raised on how we can edit the stiffness matrix of a superelement and use it for our model.  An approach presented below is to first create a superelement that has the same number of DOF and nodal location that will serve as a template. An APDL script can then be written to edit the stiffness matrix entries as desired before exporting to a new superelement *.SUB file for use in future models. The self-contained script below demonstrates this.  /prep7 et ,1, 185 mp , ex, 1, 200e3 mp , prxy, 1, 0.33 w = 0.1 ! single element (note nodal locations) n , 1, w, -w, -w n , 2, w, w, -w n , 3, -w, w, -w n , 4, -w, -w, -w n , 5, w, -w, w n , 6, w, w, w n , 7, -w, w, w n , 8, -w, -w, w e , 1, 2, 3, 4, 5, 6, 7, 8 /solu antype , substr     ! analy

DesignXplorer Design Point Alternative Save

Solving for many cases with small variations using DesignXplorer is quite convenient. After setting up an initial model, a parameter could be defined in SpaceClaim or elsewhere. The solution for multiple design points are then generated as I sip on my beer (legally at home).

As shown in this YouTube Video, the output parameters are single values like natural frequency, displacements and other maximum or minimum of available solution results. Unfortunately if you are interested in more complicated items that aren't easily available through the user defined results or *GET commands, how do you capture that output parameter?

One way would be to retain all design point results for later post processing but that would be overkill especially since I'll have to go into everyone of them to extract out the information which is a pain.

Alternately, a post-processing APDL script could be written to extract out key information at each run. An example would be the mode shape of a beam. With different input parameters (e.g. length), let's export the response at the nodes on top of the beam for all runs.

Step 1
Setup the model as usual with at least one input parameter and one output parameter.

Step 2
Create Named Selection of regions of interest. This can then be later accessed via the MAPDL db to be called by the script. Note that this should be done before the first solve.

Step 3
The command snippet is added at the Solution branch to allow for /POST1 computation in extracting out the results of interest. In this case the nodal X location and the Y displacements. Two key points:
1. The file.db was made available to identify the named selection.
2. The output text file is copied over to the user file directory before Ansys DesignXplorer deletes it.

The Command Snippet could look like the following:
resume, file, db

cmsel, s, TopNodes
*get, ncount, node, 0, count
*dim, data, array, ncount, 4

*do,cto, 1, 3
set, 1, cto
nnow = 0
*do, ct, 1, ncount
nnow = ndnext(nnow)
data(ct, 1) = nx(nnow)
data(ct, cto+1) = uy(nnow)

!!! Writes data to file
! File Name
*get, timenow_test, active,, time, wall ! appends time 
timenow = chrval(timenow_test)

*dim, fname, string, 128
fname(1) = strcat('file',timenow)

! Actual File Writing
*cfopen, fname(1), txt
*vwrite, data(1,1), data(1,2), data(1,3), data(1,4)
(E20.5,'  ',E20.5,'  ',E20.5,'  ',E20.5)

!!! Copies over to User Folder
*dim, fname2, string, 120
fname2(1) = strcat(_WB_USERFILES_DIR(1), fname(1))
/copy, fname(1),txt,, fname2(1).txt

Step 4
With the exported text file in the user_file directory, the data can then be post processed in Matlab/Octave. The plots of the first three mode shapes are shown in the first figure of this post.

Files Used in this Post
Ansys Workbench R18.2 Archive File
Octave/Matlab Post Processing Script File