Good morning All,
I’m facing some problem with a simple assembly, where I have a big disk with L-sheet attached (centre of the disk).
I apply a Constraints Tied contact to all the L-sheet to the main disk; imposing also a surface interaction:
The result of the Frequency analysis is strange, with all Rigid Body motion… it seems like that the component are not bonded to the main disk.
Where am I making the mistakes?
WBR
Marco F.
Analisi_modale_shell.pmx (7.8 MB)
Even with offsets defined, there are still some gaps between the extruded shells (you can see that in the results visualization even if you just run Check Model - make sure that Output is set to 3D, though).
Tie constraints may need non-default (higher) position tolerances. However, it’s better to disable adjustment if there are significant gaps.
But most importantly, watch out for surface sides. Fixing this makes the connections work:
Analisi_modale_shell mod.pmx (3.0 MB)
Note that for shell edges, you may actually need tied contact instead (but it’s not appropriate for frequency analyses): Tie constraint on the edges of 2D elements - Analysis issues - CalculiX (official versions are on www.calculix.de, the official GitHub repository is at https://github.com/Dhondtguido/CalculiX).
Thank you very much for your clarification; now it’s clear where I was making the mistakes.
Just to have another clarification regarding the use of a shell part: which is the difference between the use of Thicken Shell Mesh and the use of Shell Section?
WBR
Marco F.
Thicken Shell Mesh turns shell part (surface geometry, meshed with shell elements) into extruded solid part. So if you use this tool, you have to apply Solid section instead of Shell section.
So it two different procedure to handle and prepare the shell part to the calculation, am I right?
One approach is to import surface geometries and mesh them with shell elements. Internally, they are extruded to 3D solid elements by the solver anyway, but they have some advantages and are mostly the best choice for thin-walled parts.
However, if you encounter some known CalculiX bugs/limitations with 2D (shell or plane stress/strain) elements or if you want to work with solid elements for any other reason, you can use the Thicken Shell Mesh tool to obtain one or more layers of solid elements from surface geometry meshed with shell elements. Sometimes it’s used even if your parts are not thin-walled and you don’t plan to use shell elements at all because this tool is simply another (quite versatile) way to generate hexahedral meshes from quad surface meshes.
Thank you very much for the clarification 
Now it’s all clear.
WBR
Marco F.
in case of frequency analysis and tied contact type required perturbation activated to make it works, create first analysis step w/o stressed model is allowed.
Yes, contact state in perturbation steps is frozen (cannot change) from the previous general step or initial state, but I recall some issues with that in CalculiX, so I would just stick to tie constraints whenever possible.
