Thanks for your answer. I had already studied the suggested topics.
To determine the right value of K, I have done some runs with different values of K.
Also did run latch simulations with different K values. Those were ok.
Curve 10 is the curve that is right according to literature.
Calculation up to max insertion goes well, but as soon as the direction of movement reverses, the calculation gives an error. I also have played with the K factor.
It would be good to make the withdrawal less abrupt. Abaqus has so-called smooth step amplitude for that - loading and unloading is done with polynomial transitions:
Here, you can only use manual (tabular) amplitude curve definitions, though. But reducing the maximum time step and forcing more time steps for the transition may help (this is also mentioned in the referenced forum thread).
Some form of damping (contact damping or inertia in quasi-static dynamic analysis) could also help with instabilities in contact.
Sometimes you also have to change the step controls if nothing else works.
And you may have to refine the mesh of the clip too.
I have made in the past some simulations of plastic parts inserted with Abacus, but the results didn’t agree with real testing. There are a lot of uncertainties due to wide range of properties of the plastics that dependes a lot on humidity condition (suppliers gives data for wet or dry condition), and friction coefficient as well.
I had a setup with linear interaction with K=1E07 (default value when you select linear) and an insertion of 0.7 mm instead of 0.8 mm, and it finished.
Abaqus handles such cases really well because it has a few tricks up its sleeve. Namely:
general contact automatically handling all kinds of interactions, including edge-to-surface contacts (often needed in snap-fit analyses)
contact and step-wise automatic stabilizations - this very often helps overcome such convergence issues. In fact, some time ago I asked Guido if he could implement automatic stabilization for static steps, but he said it had low priority for him because they don’t use this Abaqus feature in their company (aerospace industry) - they consider it risky for the correctness of the results (even though there are ways to control it).
dynamic implicit quasi-static step - recommended for problematic static analyses; CalculiX also has dynamic implicit step but with no special settings for quasi-statics and definitely not so robust.
Abaqus also has advanced material models for polymers such as the PRF model. Still, accurate experimental data and/or good numerical (or FE-model based) calibration is needed.
Some other things you can try here are first order elements (second order ones may not work well with contact), dynamic step and further local mesh refinement. Plus step controls, as I’ve mentioned before. In the referenced CalculiX forum thread, you can see how many attempts it took to obtain a working solution.
What about the number of contact elements. Those jumps look like some contact areas are suddenly detached or too sticky?.
I’m, also experiencing issues when the amplitude reverse sign. Have you tried to split the analysis in two steps and redefine the BC that controls the withdrawal?
The problem is also that you model is computationally too large to be doing tests. I will try to build a lighter version.
Out of curiosity, I downloaded and ran the analysis from FEAnalyst to look at the details and settings, but the contact doesn’t seem to be working correctly. When displaying the true deformation, there is a large amount of penetration.
I haven’t changed anything in the OP’s setup apart from replacing amplitude with 2 steps. I already advised the OP to refine the mesh of the clip because it’s way too coarse and to adjust the contact stiffness accordingly. However, the main issue was with non-convergence on amplitude reversal and this can be solved by just switching to multistep approach.
I stick to 2.22 for now due to the new limitation with rigid bodies and shells plus some reports of slower calculations.
I prefer Pardiso too (faster and more robust).
Mortar (Lagrange multipliers) contact often fails to converge, but may indeed be a good way to obtain more accurate contact results with less penetration. I would still refine the mesh on the contact surface of the clip though.
So you simulated only the insertion ? Withdrawal should work with the 2-steps approach.
my experiences shown PaStiX is faster than Pardiso in case of large contact and plasticity.
any example models were Mortar contact fails? it’s promoted by many to be robust and accurate in contact analysis, unfortunately Abaqus and Ansys seems not have.
i’m only simple testing for contact algorithm due to times effort in computational, but probably it can work also for two steps analysis.
. I will use this with my other simulations. Will be continued.
