I am a new Prepomax user.
I am looking to validate prepomax on a calculation of a thin plate (thickness 0.7411mm) in bending, subjected to gravity, supported on 2 edges and with a plane of symmetry on the other two edges.
At 2 nodes at one extremity, I block UX movements to avoid rigid body movements.
Note: I directly imported my mesh from external software via the .inp format. These are linear interpolation elements.
In my 1st case, the case of a flat plate, I am OK with the result (I compared it analytically). See “cal_prepomax_rectangle.pmx”
I get a U2 max displacement of 396.8mm.
I noticed that the default solver (pastix) gives completely wrong results (the calculation diverges it seems to me). But, with other solvers, it’s OK, for example “Pardiso”.
In my 2nd case, all conditions are identical, except the shape of the plate. This plate has a wave shape.
The problem is that I have a result that seems completely wrong to me.
In fact, the maximum deflection U2 obtained is 0.06647mm.
I use another software at my disposal (Framatome Systus, software used in the nuclear sector in France), I obtain a result close to 386 mm. Which seems much more realistic to me.
See the “cal_prepomax2.pmx” file.
Are there any limitations on calculations with shells that could explain this surprising result?
Do you see anything strange in the setup of my calculation?
Pastix does not give good results, which solver do you recommend?
For information, once this calculation works, I would like to activate nlgeom to consider large transformations.
Thank you in advance for your expertise.
Post-Edit: I can’t upload my 2 files .pmx, I have the message “Sorry, new users can not upload attachments.”
So here are some screenshots of my 1st case :
I exported the input file from cal_prepomax2.pmx and submitted it in Abaqus. The result is 384.4 mm. So your setup is correct and it seems to be an issue with CalculiX. Might be worth reporting on its forum and (if confirmed) GitHub repository.
thanks for the problem example files, quite strange for me. Since it’s related to the solver, it may need to repost and inform at CalculiX forum also,
the problem is specific to PaStiX not Spooles or Pardiso, given it is notified can be useful info for another user to warn and use with caution.
CalculiX does not have real shell elements built in. It extends them into solid elements while solving. Doing that introduces many strange behaviors in some cases.
I noticed that your mesh is linear, and linear shell elements get extruded into linear solid elements. Such elements are good enough to capture constant stress files, like in tension, but not good enough to capture variable stress field, like in bending. Can you try to prepare the mesh using parabolic finite elements and repeat the procedure?
I exported the undeformed solid mesh from your results to get the solid mesh of your problem (linear solid elements). I reapplied all boundary conditions and loads and got the following result.
since it’s look strange for me, i recreated similar case and observing. This problem in PaStiX is specific when the ratio of thickness to spans is too large or extreme. It seems it will start to fail at a ratio of greater than 1000.
below an example of 1000mm x 1000mm steel plates subject to its own gravity loads, element type is linear (S4), result in detail of every thickness reduction for clarity.
What about Pardiso ? That was the solver used by the OP when the issue occurred for the waved plate. I also tested this using Pardiso and got the same incorrect result.
