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

CMS Superelement Harmonic Analysis

Fig 1: Project Schematic

With the release of Mechanical 19.2, substructuring is now available for Modal & Rigid Dynamics without scripting. That just made my earlier post on CMS outdated! Note that there is still a key limitation where Generation and Expansion Pass must be performed on your local machine.

To get ahead of the game a bit, here is a way to do Harmonic Analysis extending on previous work. (Please go through that before this post). Some points of note:
  1. The method of merging the CMS and non-CMS models together into System C is the same.
  2. All files related to the superelement has to be copied over to the solver file directory as before.
  3. Modal analysis need not be performed first as the example here uses Full Method instead of Modal Superposition for simplicity. 
  4. The script expands the responses the same way as Modal Analysis does so the script will look familiar.
Additional Resources:
Example: Harmonic Response to Unbalanced Force using CMS (Link)
Example: Modal and Harmonic Analyses of an Automotive Suspension Assembly Using CMS (Link)

Command Snippet for Combined Analysis D
!!!!! Save full model
/filnam, full

!!!!! perform use pass solution
/filnam, use
! Deletes body to be replaced by cms element
cmsel, s, BODY1_CMS_PART_  ! ** part named selection for deletion **     
cmsel,u, interA_CMS_PART_  ! ** don't delete interface nodes **
edele, all
ndele, all

*get, etmax, etyp, 0, num, max
et, etmax+1, 50         ! define substructure element type 
type, etmax+1
mat, 1
se, myse                ! define substructure element

/solu                   ! uses exisitng settings

!!!!! expand the solution for viewing purposes
/clear, nostart
/filnam, myse

expass, on
seexp, myse, use        ! substructure name and the use pass jobname 
numexp, all,,, yes   ! Expand all modes

!!!!! merge results file
/clear, nostart
/filnam, full

nsubsteps = 3         ! **number of harmonic frequencies**
*do,ct, 1, nsubsteps
   file, use
   set, 1, ct
   file, myse
   append, 1, ct
   reswrite, file      ! file name for results file

Model Comparison with verification model
Fig 2: CMS Model

Fig 3: Verification Model

The results looks pretty similar for the solved frequency.

Archived Model V19+
The archived file can be found here:  Link

All posts on Superelement 
CMS Superelement Harmonic Analysis Link
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

In more recent version of Ansys Workbench, distributed file combinations defaults were changed to OFF. This needs to be corrected with appending the following commands to the Analysis A command snippet (Generation Pass).
    dmpopt, esav, yes
    dmpopt, emat, yes
    dmpopt, full, yes

Update [Jan 18, 2020]
A new post shows the same procedure in Ansys 2019 r3.


  1. Can we use CMS for electric motor modal analysis, what I try to achieve is that stator, rotor, bearing, endplates, housing are independent components, and then use CMS to get the full motor assembly modes.

    1. Yes, you should be able to branch off multiple analysis for different components.


Post a Comment