Skip to main content

Component Mode Synthesis(CMS) Substructure in ANSYS Workbench

Here is a basic example of how one may use CMS inside Workbench with APDL command snippets. These appropriately named superelements has the advantage of being quick to solve once the initial investment is put in. This saves time especially for multiple iteration of the same parts (condensed once with CMS) while changes are performed on a local full model part.

The archived workbench file (R18) can be downloaded here (download icon at top-right).

Original Model in ANSYS Work Bench

The model is rather simple with 3 parts. The bodies are in this case to be connected with CEINTF. The "MainBody" part will be condensed into a superelement (Craig-Bampton method) and will be used later when connected to "Leg1" and "Leg2". The system natural frequencies are then evaluated. The results are compared to the old fashion way of creating a full model for verification.

Step 1
Suppress all other bodies except for the "MainBody" which a superelement will be generated from. Create Named Selections of the surfaces which will join to "Leg1" and Leg2". In this case, named them "C1" and "C2". Add a command snippet CreateSE as follows:

fini
/filname,myse  ! name of the super element
/solu
antype,substr     ! analysis type: substructure
seopt,myse,2  ! saves mass and stiffness matrix
cmsopt,fix,12  ! Craig-Bampton, 12 modes (CRITICAL)

cmsel,s,c1  ! selects interface name selection
cmsel,a,c2  ! additional interface name selection
m,all,all  ! creates master nodes

alls
solve
fini
/eof  ! important such that it doesn't solve modal

Note that ANSYS Work Bench will complain of an Error even if everything went well. Check in the Solver File Directory to verify the file myse.sub was created. This can be done by clicking on Outline Tree > Solution, Right-Mouse-Button > Open Solver File Directory.

Step 2
Without getting out of Mechanical, suppress "MainBody" and unsuppress "Leg1" and "Leg2" bodies. Verify that there are no unintended connections created when you do this. Next, insert the command snippet below (don't forget to suppress previous SE generation snippet):

/prep7
*get,etmax,etyp,0,num,max
et,etmax+1,50              ! SuperElement Type

type,etmax+1
mat,1
se,myse                    ! Creates Super Element

!! Joins Things Together
alls
ceintf, ,all               ! Joins interfaces

/solu
alls

Running the above should solve the modes and get something like this:
Use of SE in Modal Analysis

The original superelement part was not expanded, thus hidden. This would require another step not covered here.

Verification Step
To verify the method above, all bodies are unsuppressed and command snippet needs to be configured the same as the previous CMS for connections:
/prep7
alls
ceintf, ,all ! Joins interface the same way
/solu
alls

The solved full solution should look similar to this:
Full Model Verification

The natural frequencies and mode shapes are almost the same which is what we're looking for.

Update: Expansion of CMS results discussed in new blog post.

All posts on Superelement 
Reuse CMS Superelement in Ansys Workbench with Expansion Link
Component Mode Synthesis (CMS) with Results Expansion in Ansys Workbench Link
Craig Bampton Method Overview Link
Component Mode Synthesis(CMS) Substructure in ANSYS Workbench Link

Comments

  1. Thank you very much for this great introduction. Could you please extend your tutorial with the expansion in Ansys workbench.

    ReplyDelete
    Replies
    1. http://www.ansystips.com/2018/03/component-mode-synthesis-cms-with.html

      Delete
  2. Hi,
    Is it possible to have the wbpz in an earlier version; ex: v17.
    Many thanks

    ReplyDelete
    Replies
    1. Apologies, but I don't have v17 installed so I can't recreate it there.

      Delete
  3. Could this method be applied in flexible multibody dynamics analysis?

    ReplyDelete
    Replies
    1. Yes, this method works for flexible multibody dynamic analysis.

      Delete
  4. Hi,
    Thank you very much for your tutorial regarding CMS. Could you please explain the CMS procedure for harmonic analysis too??

    ReplyDelete
    Replies
    1. Please see another post here: http://www.ansystips.com/2018/12/cms-superelement-harmonic-analysis.html

      Delete
  5. This comment has been removed by the author.

    ReplyDelete
  6. Hi,
    Thanks for a great web site. Really useful stuff in here.
    I am trying to implement the creation of super elements myself, but get the following error when running your script, modified to work with my project, from "step 1":

    The option of SUBSTR on the ANTYPE command is either not available for
    this version of ANSYS or the appropriate product was not selected for
    this session.

    Have you maybe come across this error before? I assumed this was the error you said ANSYS would give and still process the commands, but unfortunately I get no file "myse.sub" in my solver directory. It seems as the solver stops at this line, and does not process the following commands.
    I have run the same commands directly in APDL without problems, so I find it strange that Mechanical is complaining.

    I am using ANSYS Mechanical Release 19.2, with an ANSYS Academic Research license.

    Any help is greatly appreciated.
    Adrian

    ReplyDelete
    Replies
    1. This sounds strange to me as well when you can do it in Ansys Classic but not Workbench. Is it possible the license selected is different for the two modules?

      Good luck,
      Jason

      Delete
    2. Well, yes. I finally figured it out. It was licensing trouble causing it. So, for future reference, here is the fix that worked for me:

      In Workbench, go to Tools -> License Preferences.
      Then, I "moved up" my license for ANSYS Academic Associate Mechanical and CFD in all tabs, resulting in this being the license that is checked out first.
      Restarting Workbench and Mechanical session seemed to fix it, and I do now get a super element matrix, "super.sub" generated in the solver files directory.

      Delete

Post a Comment