The calculation fails in the attached model, and I cannot find the error.
Is it possible to generate a better and more efficient mesh than the one in the attached model?
Thanks in advance for the help.
A.
Definitely. Use shells whenever possible for thin-walled parts or at least hex/wedge elements. Meshing with the latter has some requirements since they can be created only via revolution, extrusion, sweep or using the transfinite Gmsh algorithm that needs subvolumes with 5/6 faces (having 3/4 edges each). Alternatively, you can use the Thicken Shell Mesh tool. So try extracting midsurfaces from these long thin-walled parts in your CAD software and meshing them with shells first. If you encounter any CalculiX issues with 2D elements, you can always thicken them and use solids.
Apart from that, if you want to get your analysis to run, even just to see what happens in it (maybe there’s some modeling mistake), make it linear (replace contacts with tie constraints), run a frequency step to check the connections and then a linear static step to see if the results make any physical sense. Still, you will need to fix the mesh to get reasonably accurate results.
And if you get errors such as “zero coefficient on the dependent side of an equation” then there might be some overconstraint in your model, likely with tie constraints. Check and correct them as explained here: [Solved] Why does increasing the size of parts lead to an error? - #2 by FEAnalyst
Just a quick example for one of the parts:
Shell profile Agazzotti.pmx (1.5 MB)
I can explain in detail how to prepare it in FreeCAD.
Thanks for the reply.
I created the model using solid elements to better handle contact between the different bodies—partly because CalculiX expands shells into solids anyway, so it seemed pointless to model them as shells (which require proper offset management). Am I mistaken? The model includes bolts connecting the thin-walled profiles, and these bolts were modeled as solids. If I convert the profiles to shells but keep the bolts as solids—in order to evaluate bolt stresses—would the calculation still be reliable?
I ran a frequency analysis using the solid profiles, but the calculation failed.
I also tried creating a compound part combining the thin-walled elements and the bolts (excluding the bearing plates) to ensure mesh congruency at the nodes where they meet, but the meshing failed.
I’ll try using shell elements for the profiles and solid elements for the bolts, and I’ll keep you posted.
Solids can be fin, but not if you use tetrahedrons for this kind of long thin-walled geometry. You would need hex/wedge elements and you can get those by extruding shells.
It should be ok, but you can start with shells and thicken them to get solids as discussed above.
Might be due to overconstraint if you get errors as stated above.
Compounding may fail for more complex geometries. You could try merging parts in CAD software too, but you would still end up with poor quality tetra mesh.