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

Newton-Raphson Residues

When doing non-linear analysis, it is good practice to indicate you would like to save the Newton-Raphson Residuals before the analysis is started. It can go a long way in troubleshooting when/if the solution doesn't converge later. You may do so by specifying how many youngest residuals you wish to keep. I personally like to keep 3 to see if it is consistent. Also, increase "Identify Element Violations" toggle to 1 to locate any mangled elements.


Number of Residuals & Identify Distorted Elements

ANSYS now spends a bit of time & resource saving the residuals as it solves each iteration (see below). If you specify only 3 (as suggested above), only the youngest 3 residuals are saved with successive overwriting of the older files. The process is highlighted in the output file below:

file.out showing when residual files are saved

If later ANSYS spouts out colorful language disguised as WARNING or ERROR, you would then see the following objects under Solution Information:

Pointers on why it doesn't converge

The nd001_* are a selection of elements that are distorted. They are sometimes referred to as "Error in Element Formulation". In addition, the 3 Newton-Raphson Residual contour plots highlights the last three iteration's out of balanced forces that are causing difficulties in convergence.

Now What?
These "hot spots" highlighted by the Newton-Raphson Residuals are the causing difficulty for convergence. Tweaking the mesh here may offer some relief. Or decrease the Normal Stiffness Factor of the contact in question to 0.01 if resultant penetration is allowed. Decreasing the initial step size may help. Making those few elements linear could be an option if that approximation is acceptable.

Troubleshooting non-converging solutions can be tough. Hopefully by identifying the offending nodes with the above method, this will help debugging the analysis easier. 

Comments

Post a Comment