I am performing an analysis on a damper mechanism. It consist of a Rubber material that is defined using hyper-elastic material model.
My assembly is in tilted position as can be seen from the photo.
I simplified this geomtery from 3D to 2D, just to analyse the most critical cross-section. Unfortunately the contacts did not work that well. So I extruded my 2D geometry with 1 mm thickness.
For the first trial I have turned the large displacments off and also only elastic part of steel material is defined. I have defined 100 iterations for the total time of 1 sec.
Unfortunately I face convergence issues and I can only compress till 2.97 mm from total 4.5 mm. It seems my rubber material is too soft to resist the pressing by steel.
So I would correct the tie constraints and contact (including master/slave assignment - there are specific rules: Selection master and slave in contact) first. You can play with position tolerance and adjustment settings to make sure ties work properly. Then try refining the mesh, it’s pretty coarse currently. Since there are no hybrid elements in CalculiX and volumetric locking is of concern when using hyperelastic materials, I would recommend reduced integration elements.
I remeshed the Rubber part with 1st order hexa elements, also the region with highest deformation was meshed finer. I switched master and slave contacts in such a way that master is stiffer than slave.
Regarding adjustment setting I have no idea what to do, so no changes made. I am working on it and if it gets me good results then I will update it here.
The analysis stops at similar time point but this time deformation mode is slightly better than previous
I wouldn’t use C3D8, just the reduced integration version (C3D8R) or its second-order equivalent (C3D20R).
Adjustment just puts the nodes of the slave surface (within the tolerance distance) on the master surface to remove initial gaps and penetrations. It’s not always needed and sometimes even breaks models but may improve the situation in many cases with misalignments between the meshes that are supposed to be touching.
I would also enable Nlgeom to see more realistic deformation (the strains are really large here). If the mesh still distorts too much, you may have to refine it further. Perhaps even add some small fillets to the sharp corners in the critical contact region.
That’s more general tip to avoid unrealistic results and potential convergence issues due to volumetric locking but there are independent problems with mesh distortion here.
Yeah, it may reveal even more significant (but also realistic) distortion but then you should focus on refining the mesh (and maybe also geometry as mentioned before) there. This seems to be the main cause of non-convergence and should be resolved first.
i guess about divergence issue by stress singularity at the corner, not in mesh distortion since the element (C3D8R) have hourglass controls. However, local mesh refinement at interested areas may help for both problems if existed.
Default hourglass control is not always enough to avoid hourglassing. And the distortion that causes non-convergence doesn’t necessarily have to be caused by hourglass modes. Unfortunately, there’s no artificial energy output in ccx to easily check for hourglassing.
I have 1.2 mm mesh in rest of the model and in area where I face convergence issue is meshed with 0.1 mm mesh. I am not sure how much more refinement do I need to reach the convergence. I already have reduced integration elements
I am thinking about geometry changes, by adding small fillets to check if it helps. or may be I cut the overly deformed area and remove it assuming that it will be destroyed anyways, then I will check what happens with the rest of the geometry
seen better than previously, i means refinement only needed at corner to make it less in number of element and nodes. Probably using quasi-structured quads algorithm and mesh refinement, then extrusion in PrePoMax for getting linear hexahedral element with reduced integration.
Fillets definitely may help. Such sharp edges are really bad for contact and large deformations. Such gasket-like parts should be deformed by smooth tools. You could even make them rigid for now and focus only on the rubber component.
Are you sure that the rubber is not bonded to any of the components? Looks like the rubber can be molded with the upper metal, and then assemblied with the lower and fixed with riveting the inner tubes.
In case of solving the part in work position you should work with half part to take in count the round shape, other wise you are assuming that the part is a protusion and not a revolution. About the upper rigid part, if is a sheet metal part forget of chamfers or radius, will be an straigh angle with luck, could there even some reburrs if the tooling is not well sharpned.
I had started with this but it was taking much computational time and I still had convergence problem so I first thought about solving the convergence issue in thin solid then moving to half part and then full part. I assume that if it does not work with even simple thin solid geometry then it is not going to work in half revolution too
Is this rubber really supposed to squeeze so much locally ? Isn’t it too soft ? What is the source of the hyperelastic material model data here ? It will be hard to represent such deformation even with a very fine mesh.
