I’m trying to bend a flat bar. When I use plasticity, the analysis doesn’t complete. I’ve tried various methods, but I only get an elastic solution. Is it possible to obtain a result within the plastic range? A mesh size of <0.5mm disproportionately increases the calculation time. Could you please advise me on what I can change to perform the calculations for a solid? What’s blocking the solution?
BOND2.pmx (1.2 MB)
Make sure that you extrapolate plasticity so that it never reaches plastic plateau (CalculiX assumes horizontal line after the last point).
Also, isn’t the model overconstrained ? On the symmetry planes, you have all DOFs fixed. Is it supposed to be supported this way ?
16
There is no symmetry.
You should add PEEQ to output requests to see how much it yields before the analysis stops converging. If it reaches the final points of the curve, you will need to extrapolate it.
I’m still running it (0.446543 s, converging for now). It would be also good to switch to linear elements.
I would start with linear hex/wedge elements. Maybe 3-5 layers for the plate.
What is the source of this plasticity data ? I’m trying without the bottom part (or actually making it rigid and disabling contact with it) and it still doesn’t work regardless of the mesh size, element type and relaxed BCs for the plate. I also made the indenter rigid. It seems that CalculiX really doesn’t like this plasticity definition and doesn’t want to solve it even without Nlgeom.
Yeah, I switched to linear (C3D8R or C3D8I) elements for all the tests, but this plasticity (even extrapolated as shown above) seems really problematic for CalculiX.
With just these two parts (one deformable with C3D8I), it reached 0.236584 s:
And with 6 layers of C3D8R it reached 0.251416:
Perhaps it would be good to get rid of nonlinear contact entirely for now.
Here’s my current test model with several changes:
BOND2 mod.pmx (669.7 KB)
Thank you for checking
Too much deformation of 1 FEM element? Material escapes from contact?
In this case we can’t easily remove contact for debugging because it would change the way load is applied. But try limiting the contact region to a small patch on the plate - currently it spans the entire plate:
Of course, trying different contact stiffnesses also makes sense.
See this model with no contact - just pressure (of course, it can be increased to reach the desired deformation):
BOND2 mod pres.pmx (623.9 KB)
I’ve tried various contact stiffnesses without success. I’ve noticed that there’s a problem with cylinder contact. I had a similar problem with a cylinder in a hole with clearance. Only fitting the cylinder into the hole yields a result. In this case, after bending the sheet metal 90 degrees, the sheet metal suddenly loses contact and pops out. The problem is interesting because no nodes are in contact until the analysis is complete. I apologize, but I won’t be able to correct the calculations for about two weeks. Thank you very much for your time.
Maybe dividing the analysis into several stages would help. Unfortunately, I don’t know how to do that.
For cylinder in a hole, it’s important to use well adjusted and refined hex-only meshes. Without adjustment if you want to model interference fit.
Also, you can track CPRESS and COPEN to see if contact is lost.
Here, you could also try adjustment and maybe even no separation contact (Tied + low friction and slip), but it didn’t help in my tests.
Perhaps local mesh refinement in the contact region would help. But you need a partition there.
Yoi could try multiple steps: Understanding multistep analyses
It sometimes helps, but often makes it worse (due to discontinuity introduced by it). Using amplitudes to add (or remove) the load gradually might be safer.
