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

It's EALIVE! It's Alive!

To be able to EKILL and EALIVE elements is a neat trick. It allows for a dormant element that springs to life. The reactivated elements have zero strain so some people use it to simply clear it of any unwanted stresses. I have more frequently use it to turn on and off contacts.

Here's a simple example problem: A block is fixed at the bottom, the top cylinder is pushed by hand downwards until it touches the block. Because of adhesive, the two are now 'bonded' together. In the second step, the hand lets go of the cylinder, the spring which is attached to ground at the top pulls on the cylinder creating stress on both parts.

Just push down to cure glue and let go!

There are a few steps needed to get this to work.

Firstly create a snippet of the bonded contact so it could be identified later. The code is simply:
mycid = cid
mytid = tid

Secondly, create two more snippets in the Analysis tree. Snippet #1 will EKILL the contacts for the first time step. Specifying the Step Number is critical here.

Snippet #2 will EALIVE the contact elements at Step Number 2.  

Finally, there are other odds-and-ends setup similar to other nonlinear analysis. For example Large Deflection - ON, large Pinball Radius, and deactivating the 'hold down' Displacement on the second time step. Additional details can be found in the archived v18 file. Download button is on the top right.

There are other great examples of this on the web. Here are a few:
PADT's example has contacts that controls penetration.
Simutech's example is cool in e-killing elements above a certain stress level while still in /SOLU

Update: Ansys V19 has Contact EKILL and EALIVE options native in Workbench. Snippets are no longer necessary.