Firstly, I was impressed to see that version 1.3.3 is a lot more stable than previously and happy to report that results correlated somewhat to other commercial software that I used to compare. Obviously there were some differences in the stress concentration regions.
Things I would have liked, but was unable to do in PrePoMax
1D elements to use as bolts
split/divided some of the surfaces in order to apply smaller boundary conditions. The issue is that unless you split a surface into separate parts in CAD, the step model does not translate the split faces into PrePoMax
I wasn’t able to apply a frictional contact between the two flanges - kept getting a negative Jacobian error (but this could have been my lack of correct usage)
Below are screenshots from other commercial software, as comparison:
Tie constraint are very good for interfaces between different types of elements. However, in some cases it’s better to use tied contact to connect shells and solids:
Hi Arnie, @arnie Could you please send a link to this model. The reason for results deviation could be that " calculix use a standard shape function for first order elements" , The commercial finite element tools add ingredients to make them stable, which are rarely documented , to these element formulations. could you please re-run the model with S8 elements and check the results again.
I can confirm the file cannot be opened in the new version of PrePoMax. I have fixed the problem in the code, and I am sharing the file saved in the development version of v2.0.3 that can also be opened in the release version 2.0.0.
Today, I would probably set it up a little differently. For example, now that you have implemented ‘Compression Only’ BC in PrePoMax, I would apply this on the bracket (wall) rather than the X-displacement = 0.
Calculix documentation says , *TIE is not allowed between shells and solids. ( Shells have rotational DOF , whereas solids have translational DOF only). Could someone advice me how to tie shell and solids with calculix?
Don’t trust this part of the documentation. It’s outdated or too restrictive because tie constraints work fine with 2D elements. You can also try tied contact.
@Matej i would like to report a Bug. Tie contacts after deletion exist in the database. also you will find that this model if exported cant be read back properly.
Hi @arnie i think the reason behind results deviation could be Ansys using NLGEOM by default. Also i believe the loads are significant enough for NLGEOM to be activated. I did try to run your model with NLGEOM on but it doesn’t seems to converge. ( I think the culprit is the Tie contact) .
update- 15th Jan
@arnie I Think results are close.(pattern is different) Could you please run the Ansys simulation with second order elements and NLGEOM off . ( however i could not converge the solution with NLGEOM on.)
After trying i can say, the model does not converge if NLgeom=ON because of the connections between rigid body constraints and shell elements. It can be seen in the picture, the simulation runs successful when fixing the lower edge, but does not converge when fixing the upper edge. (The model has no contact only tied- and rigid body constraints).
If these two flanges where made of solid elements, i am sure the nonlinear analyses would converge.
