Hello, I have written code that is intended to be used to transform stress/strain/force data for QUAD8/TRIA6 to a specified system. The code to evaluate the element system for CQUAD8 and CTRIA6 is based on the description in the User's Guide. I thought I would use the OMID bulk data parameter to have NASTRAN output data for QUAD8/TRIA6 in a specified material system which I could use to check my code. However, the values I calculate are quite a bit different from the NASTRAN output (using OMID). At this point, I am not sure if there is a problem with my code or if the output as printed using OMID is not suitable for comparison with transformed output as calculated by my code. If anyone has any thoughts on this, I would appreciate your input. Thanks, Larry
I am not aware of any problems with OMID. However you should keep in mind that OMID only outputs the stress results written to the F06 file in the material CS. If you are looking at stresses from the OP2 file, their output does not change with OMID.
Hello Mark, That was my understanding... hence I wrote a perl script to extract the data from the f06 to make testing easier (and for visualization). I was wondering if perhaps the OMID output was evaluated at the integration points and then transformed to the material system (and perhaps then extrapolated to the grids). I expect this would in general give different results compared to evaluating the values at the grids and then transforming to the material system. Do you know if something like this could be the case? Thanks for your reply. Larry
NXN computes stress at the gauss points and then extrapolates it to the grid points in element CS. If OMID is present, it takes the stress at the grid points and transforms to material CS.
Have you tried simple test cases with square elements where you make the material x axis correspond to the element y axis? This should easily show if NXN is doing the OMID transformation right and if your perl script has a problem .... or the reverse.
Hello Mark, I did some testing yesterday... limited to square elements. Everything works fine if the mid side nodes fall on the line segment between the appropriate corner nodes. However, if I move the nodes off the segments, things don't look so good. I have attached a PNG of an element I have been looking at to see if I can find the problem. The dark line segments show the orientation of the element system as I calculate it. It looks reasonable to me based on the description in the Users Guide. It dawned on me (perhaps wrongly?) that by comparing the difference between the principal stress angle calculated for the results in the element system versus material system, I could determine the angle between the element and material system (as calculated by NASTRAN). For node 26 (the lower left node), I calculated a difference of 28.7 degrees (between the 2 NASTRAN runs). In the analysis, the material system (X) axis is at +12.5 degrees relative to the global X. This implies that the element system local X (at node 26) as calculated by NASTRAN is -16.2 degrees ( my calculation of the element local X puts it at ~ +2.0 degrees). For what it's worth, I use the Serendipity shape functions to evaluate the system. Thanks for any thoughts you might have. Larry