Hello everyone,
I am running a nonlinear simulation with contacts and high plasticity deformation. I have succeeded in solving my simulations. If I re-run it again without any change, it does not solve.
I sometimes have an instability feeling that I am, once in a while lucky and get my simulation through.
Does anyone also have had this impression before? Is there something I can do to avoid it and improve my success guaranty?
Thank you
Rui
I assume that you mean that the solver fails to converge. This happens with CalculiX from time to time. It would be best to discuss it on the CalculiX forum since it’s not an issue with PrePoMax itself.
Do you at least, get the same result?
That’s my point I dont get the simulation reconverging… So, I don’t even know.
It would be smart indeed. Thank you very much for the piece of advice.
What’s the error message?. Number of iterations exceeded, to many cutbacks, Solver stops without any message …
It mostly always ended with the minimal solver increment reached (1E-06s).
I read yesterday only, that CalculiX rather work with big time periods to prevent that problem. With the specific case I mentioned, I have not had the opportunity to study the behavior over a bigger Time Period. Thus, nothing has converged better with a bigger one.
I know that corners are no friends of contacts and given that plasticity reaches 100%, it could be that of my simulation extreme. Although simple, its physics are extreme and could push the limits of the solver…
But you are descriving a different problem now.
Yesterday solved and today not or yesterday didn’t solve.
ÂżWhat do you mean by plasticity reaches 100%?
ÂżIs your problem load or displacement driven?
Sorry, I am indeed. I somehow feel they are linked.
The only 2 times, I managed to solve my simulation I could not resolve it straight away. I have since been trying to optimize my parameters / find a solution to stabilize it / to make it work and apply it with my 3-4 design iterations (consisting of a variation of a diameter only).
Plastic strain exceeds 1. I specified more points to cover the strain range as the extrapolation is constant past the plastic curve and subjects to non-convergence. It helps though but still not 100% sure.
I am working with displacement. It is easier to obtain convergence.
ÂżIs that posible? You mean 100%
ÂżWhat kind of material is it?
I remember JuanP saying "Strains should keep arround 4% so it can be called “small deformation” (from Bathe in his book). You are at a 100%. 
With so huge plastic strain you may need hybrid elements (unfortunately, they are not available in CalculiX). But it’s possible that something is wrong with the model setup. If not, you could try adding some small fillets.
I have been trying with small fillets and slightly bigger mesh on the contact and CalculiX seems consistent. I have however never used such elements even with other softwares. I will make some researches.
It is only a small portion of the component. It is an Aluminium Alloy.
Hybrid elements are available in Abaqus (on which CalculiX is based). They are recommended or even required for incompressible and nearly incompressible hyperelastic materials but can help also in cases when plastic strains reach large values (> 10%).
I’m surprissed. Is that a comercial Alluminum?
Are you talking about PEEQ being=1?
Could you please share the inp *PLASTIC values.
Yes the plastic strain , isn’t it ?
You want the actual material data ? Instead of leaving it up to calculiX to extrapolate the missing points here (such as it would in blue), I added data till up to 0.95 of plastic strain.
Thanks for sharing VIR
mmh, 
ÂżIs this a metal forming process?. I have never attained such large PEEQ. Codes are limiting me way below those values.
Indeed, the default constant yield stress extrapolation can be really problematic in many cases. Only recently (in 2022 version) linear extrapolation options was added to Abaqus. CalculiX would also benefit from such a setting.
No problem 
.
It could be indeed but in this case it is a cold assembling process similar to rivet-style.
Perhaps explicit dynamics analysis (configured to be quasi-static) would be the way to go then if it’s something involving significant nonlinearities like difficult contact conditions and large plastic strains. Explicit dynamics procedure in CalculiX is far from what Abaqus can do in this regard but it’s still worth giving a try in such cases.
Thank you both for all the input.
Unfortunately, I have no experience with explicit dynamics simulations. I am just aware that there’s a trick to run it on CalculiX. I will try to dig further into that matter & see where it takes me.
But, even with such high plastic strain the addition of the fillets on the contact corners increased considerably the stability of the simulations. Big move.
Really good typ FEA!!.
One must pay attention to corners and plasticity. If one arrives to the point where two element sides become flat (aligned) the element blows up and convergence fail.
