It seems that PrePoMax is getting more and more attention and good reviews. The forum posts also seem to be growing by the day. I have raved about the user friendliness of the GUI since I stumbled across it a couple of years back. Matej and his team are visionaries and I am so grateful that they selflessly devote their time and effort to this software.
Anyway, since I see others posting comparisons to other commercial software, I thought I would post a simple comparison I did recently regarding modal frequencies. I used a simple 20x20x300 long beam fixed on one end with density of 7850kg/m3 and Young’s Modulus 2E5MPa.
I have captured the results in the comparison table below. It is interesting, but also a little mysterious, the differences in mode shape #5. Consequently, it is the only mode shape with a ROTATIONAL deformation pattern. The others are all translational along the X or Y axis.
Note that those are mostly not corresponding modes, I just placed them in one table and eliminated repeating frequencies. The analytical model can’t capture all the mode shapes that solid FEM model shows. Only transverse vibrations are considered in this analytical solution.
It’s puzzling because the difference in the mesh (hex vs tet in the Solids option) doesn’t affect all the other mode results, just that one.
Also, in the shells (midsurfaces) analysis I have used quads in both software.
The Abaqus results you posted have a close correlation to the Ansys results, so the Calculix mode 5 is still a little perplexing to me.
Try changing the settings in the static step. There is an option to select the solver for the linear system behind the finite element method. Pardiso requires some additional .dll files, so if you do not have them, it will not work.
I went back to the modal analysis using shell element and changed the solver to Spooles, which gave me some dubious results on some of the mode shapes (see below) - Edited after original post - this turned out to be a freak result that did not reoccur.
Further, there is also a lesser correlation on all modal frequencies with the Ansys results compared to default (PaStix) solver.
The issue with modal analyses run using PaStiX should be fixed. Here’s a quote from ccx 2.19 release notes:
Made a correction in pastix.c: PaStiX did not always give correct results in combination with *FREQUENCY. This problem has been solved. For *STATIC and *DYNAMIC calculations PaStiX is much faster than PARDISO, for *FREQUENCY calculations (i.e. all calculations which need an eigenvalue analysis in combination with ARPACK) it is significantly slower.
I would suggest using the same mesh for such tests. And also the same element type (linear, parabolic, reduced, …). Maybe there is a tool to output the Ansys mesh to a .inp file that can be read in PrePoMax.
The other thing that you might try is to increase the number of elements and see if the result changes. If it does, your mesh is not good enough.
i’m only done fast checking due to unexpected of deformation result you shown, the model may differs e.g Poisson ratio were it’s not available in problem descriptions.
also, vibration analysis in application using Ansys, Abaqus and CalculiX may have discrepancy each others even though still acceptable. as seen from an example report below,
This can sometimes happen for reasons not known to me when using the Spooles solver. There are some nodes having unphysical values. For other solver types I have not observed this behaviour before. Did somebody else observe such behaviour with other solvers?
In the beginning, I thought that PrePoMax is to blame but rerunning the same analysis solves the issue, so my conclusion is that this is a solver issue.
(see below) - Edited after original post - this turned out to be a freak result that did not reoccur.
