Strange 2D model behavior

I am running some simple 2D models for designing seal profiles (non linear with contact). I haven’t run these in years and forgot how fast and stable they are. I hope the results are somewhat realistic as well :slight_smile: I am mostly interested in the installation and removal forces and don’t care about stresses etc.

I am using hard contact with different amounts of friction (currently at 0.05 but I don’t think it is pertinent to the question at hand). They are run from ProPoMax with the default solver, (standard nonlinear). I have tested other contact models but haven’t found anything that works better yet. These are displacement driven models which I pull reaction forces from.

As I pull the seal out (or press it back in) I see strange deformations in the edges of the part. I have adjustment turned off. Any ideas what I am doing wrong?

This model should run quasi-static, as in we don’t get dynamics as in explicit models.

1 Like

Make sure that:

  • boundary conditions allow motion only in the desired directions
  • there are no regions where the parts may get stuck in contact, also because of discretization inaccuracy
  • mesh is sufficiently refined (in this case, you may have to apply some further refinement to the critical areas due to what was mentioned above)
  • material model is correct (for seals you may need hyperelasticity)

If you can share the file, it will be much easier to help.

1 Like

Thanks, I will look into hyper-elasticity and the other suggestions (and then perhaps post the file)


1 Like

Here is the input file with some hyper elastic values I found in a paper on silicone lip seals (what I am working on) It won’t run at all, with other models it will run tiny amount but blows up in the most spectacular fashion so I am guessing I need to work on my boundary conditions. I have being working with FEA for a long time but never with polymers.

Ok lets see if this works hyper_v3.inp - Google Drive

Try analyzing half of this model and applying symmetry boundary condition to the edges of the cut. Refine the mesh in the regions where contact occurs. Sharp edges with too few elements can be the source of the problem here. Maybe use linear elasticity for now until the model converges and then add hyperelasticity.

From the inp that you updload, looks like you are working with shell elements. I have edited and extruded the shells manually to get hexas/wedges (1mm thick, only one element in thickness, and apply standard bc (lower side fixed, upper side movil Y direction from 0 to 5mm, Z simmetry on front/rear faces and contact)… and it works directly, even if I would say that the mesh in the contact area was coarse. Attached a comparation with lineal and parabolic elements, have tunned your seal material a little, but should work with some hyperelastic as well. Will try later



Those are plane strain elements.

Maybe CalculiX has some issues with contact in 2D analysis in this case. Or Mecway does some tricks.

I would avoid 2D elements for this kind of analysis. If the seal is circular you could even use axisimetric, but still I preffer to work with standard solid elements. No element expansion, no new nodes, no weird considerations. Have solved with 45 Sh. A rubber (Mooney Rivling) material and it works well also. Extraccion force was very much lower than before. You must investigate very carefully your hyperelastic coefficents. Prepomax developer has also another very usefull program (Optimax) that would allow you to identify those parameters from test data using optimization and Calculix as solver, have used in the past and works very well.

1 Like

I agree with @SergioP 's comments. Try to avoid 2D elements, you don’t want the automatic expansion to cause any issues with your contact constraints. I follow the same approach of having solid elements, simply extrude the shells 1mm thick.

if the input is identical or exactly the same so i guess some code had been changes?

expanding of plane strain to solid element with constraint is done since early previous versions of CalculiX. this should be not a problem and given a consistent result

when a face or surface being extruded to create solid manually, it most similar to plane stress conditions, not plane strain in equivalency.

also, imagine when the thickness is large enough says 1000mm or 100000mm


right, truly solid element is recommended, i have some experiences also in modeling such a *Fastener in Abaqus with shell element. an existing constraint or knot lead to conflict problems with penalty contact.

1 Like