Case with 2 connected plates of different materials not working

Dear all,
I’m in trouble with an apparently super-silly case of two connected consecutive plates (of different material) subjected just to their weight and with an extremity which is fixed. The plates are modeled with shell elements. As you can see from the attached figures, the nodes at the plate-to-plate interface are conformal. The problem is that CCX leads to a solution that seems not to consider as attached the two plates (as you see from the super-high displacements of one of the two plates).

Hoping that some experienced user can help me fixing this case, I’m sharing all the related files here: Dropbox - CCX_Forum-2PlatesCase - Simplify your life

The inp file to be used is static.inp, that gathers data from 2Plates.inp. The mesh was obtained with gmsh starting from the provided step file.

Thanks in advance!

Connect the touching edges of these two plates with tie constraint and it should work properly.

I agree, even if the mesh is not conformal, the two parts are separated entities, use TIE or merge the nodes at the junction.

1 Like

Thanks a lot for your replies,
looks like the TIE constrain applies only to 3D elements (and in the current cases I’m using SHELL elements). Can you show me an example about how could I join the overlapping points at the plate-to-plate interface?

Indeed, the documentation says that tie constraints can be applied only to surfaces of solid elements. But somehow it worked when I used it for surfaces defined on edges of the shells in your model.

I carried out some tests and it seems that tie works fine as long as both shell parts have the same thickness.

Probably this constraint in CalculiX can’t find nodes to connect when shell parts have different thicknesses. But I’m surprised it even works for shell elements, as opposed to what is said in the documentation.

I think that it would be best to merge the nodes or, even better, create a single part, partition it (divide the surface into 2 separate regions) and apply separate section to each region:

Thanks a lot for all the contributions,
all of you spot the issue (duplicated nodes at the plate-to-plate interface).
Just to add another strategy that could be useful for other users, I found a command in GMSH allowing to merge any duplicated node in a mesh:
Coherence Mesh;

1 Like