HI
I tried to create a base plate by assigning compression-only behavior to the nodes of the plate surface in version v.1.5.4. My intention was to simulate the presence of the foundation with the behavior of the compression-only surface. The analysis fails.
Where is the error?
piastra_solid_2.pmx (1.5 MB)
You know that with concentrated force applied to a surface, each node belonging to the surface will be loaded with the specified force, right ? So the total force will be 2609 N in this case. It would be better to use the surface traction load which is independent of the mesh size.
There’s a long warning:
And, after a while, the analysis fails with the following messages:
Solution contains NaN!
PaStiX could not converge to a valid result
Job failed - no results exist.
Process elapsed time: 67.337 s
The list of warnings appears after deleting a part which contained “compression only” constraints. I wrote about it:
Looking at the file piastra_solid_2.pmx it seems to me something goes wrong when a Compression-only constraint is deleted. I will have to look into it in detail to figure out what.
Just switching from parabolic to linear elements solves the problem. Something goes wrong with 2nd order elements…
The problem was that when parabolic tetrahedral elements are used the weight factor of some of the nodes equals 0 and the gap element stiffness gets multiplied by it, making it 0. Obviously using 0 as gap element stiffness and force does not work.
I fixed it. Now the model piastra_solid_2.pmx runs without problems. I have updated the code and prepared a new version v1.5.5 dev for testing.
hi
the execution is now correct. I tried to perform the buckling analysis on the same model, but the results obtained do not seem correct, there is a gap between the vertical and horizontal plate.
Thank you for the excellent work you are doing.
https://we.tl/t-dZs1IgMYmn
It solves with tetrahedral mesh but when I convert mesh to hex (Extruded mesh) it no longer converges.
You are using tied contact, which the frequency/buckling analysis does not support. Replace it with a tied constraint.
It might be a bug, or it is only a convergence issue. The convergence could be problematic. Here, I cannot do any magic. Try changing the stiffness of the initial time increment step, and maybe try using parabolic amplitude for the load, …
It is noticeable that in the example convergence problems only occur when the lower plate is meshed with 2nd order hex-elements (4). Also the last model (5) with tied contact does not converge.
Taking advantage of this already-created topic in compression-only, I would like to ask if this is an expected behavior or not. I am using version v.1.5.2 dev.
I’m working on a model which hasn’t this kind of constraint (and also they were not created anytime during modeling), but in the input file, I see some references to compression-only keywords.
*BOUNDARY
*NSET
*ELEMENT
For me, there are absolutely no problems with these keywords since both nodes and elements are empty. But I would like to report it anyway 
.
i recreate model using the same Step files since there’s some error related to set names as observed. Quadratic hexahedral solid element seems not working properly, but linear type is ran without any issues.
some feature being used:
- rigid body and reference point for point loads
- tie constraint to connect vertical plates and base
- compression only by user defined values
p.s versions 1.5.4dev
I’ve also noticed this. It would be good if PrePoMax didn’t add this to each input file to avoid potential issues (I had some when running the analysis using standalone CalculiX) and confusion.
Please use version 1.5.5 since some bugs were fixed in it.
2 Likes
HI
I tried applying the constraint as suggested but the analysis fails.
I tried a further model by generating the horizontal and vertical plate from CAD as the only element so as not to define any constraints between the parts, even the static analysis fails. I can’t resolve the problem. I have always used ver. 1.5.5
piastra_solid_4.pmx (926.3 KB)
Please try version 1.5.5, where this internal node and element sets should not appear.
Right, they are gone there. Thanks.
1 Like
HI, I’m asking here so synt can continue with his pictures on the other post.
Subject: Only Compression support option N/mm
When the user define a Spring Stiffness of 1 N/mm how does Prepomax apply it?
-Do Prepomax build one spring on each node of the surface with Stiffness 1N/mm / nÂş of nodes as if they were working in parallel?
Does it happens the same in Spring Support option N/mm?