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

Weld Analysis with Ansys

Figure 1: Equivalent Stress of White Paper Model

There are many software out there now that does weld analysis. Among others...
For fatigue type analysis, there are: FE-Safe (Verity Method) & Ncode (Volvo Method)
For static type analysis, there are: FEWeld & EDRMedeso

A good reference classic book is Blodgett's Design of Welded Structures. This book is a real gem. Here are two links to a short write-up by the same author et al: Welded Connections.

White Paper
Figure 2: Weaver's White Paper Comparing  FEA to Hand Calculations

I came across this really good white paper by Weaver Engineering that had a worked example comparing both hand calculation to their software along with in depth discussions. The example was detailed enough to be replicated. This is a great stepping stone when following the crawl-walk-run philosophy.

Model and Snippet Comments
A critical step in setting up the model is highlighted in Figure 3. Nodal Forces has to be computed for later post processing and "Save MAPDL db" is required for later named selection pointing. This should be done before the model is solved.

Figure 3: Key Settings

Secondly, the forces at the weld-line was extracted with the elements of the terminating member selected. As noted in the FSUM help: "Sums and prints, in each component direction for the total selected node set, the nodal force and moment contributions of the selected elements attached to the node set." To find the "effective length" of the weld associated with the extracted load, the average length was taken (see script for details).

Finally, the Workbench model takes advantage of Ansys DesignXplorer with Snippets similar to a previous post to test the sensitivity of mesh size.

Figure 4: Ansys Results with Different Mesh Density

In Figure 2 by Weaver, his peak weld force/length (fw) from hand calculation comes in at 2,390lbf/in. In this Ansys Model and associated script, it peaked at 2,775lbf/in for 10 elements along the weld line (WELDFORCE10.txt). As the number of elements is increased, so too did the force/length. It appears to be a singularity there though the good news is that if one is to use the "hot spot method", the trend is slightly under 3,000lbf/in which is in line with the White Paper's FEA model.

A better way of averaging out the forces at the end could be finessed if needed. All the best!  

Source Files
Archived Ansys Workbench File V18.2:  Link
APDL Snippet Used in Ansys Workbench: Link
Octave/Matlab Plot Script: Link


Post a Comment