Good to know, I stick to Pardiso because it’s the default solver in PrePoMax and has less issues (e.g. with eigenvalue analyses).
Nothing specific, I just tried it a few times in different cases and it didn’t work well. It seems to be an equivalent of lagrange multipliers contact in Abaqus which is not recommended in most cases due to convergence difficulties and longer calculations. It’s more accurate than penalty contact though.
I have played with different values for contact stiffness. See previous pictures. This setup gives the best solution; the graph of insertion shows the most realistic graph of the insertion force.
The amount of allowed penetration is not clear.
Running with “HARD” setting for surface behavior shows this :
*WARNING reading *SURFACE BEHAVIOR: K must
be strictly positive
the following default will be used: 1125000.0000000000
the user is advised to analyze the results
carefully
I have reduced the mesh size of EON.
Runned with 2 steps with Pardiso Solver with hard surface behavior.
This looks ok.
Still lot of penetration
Now to do simulation with friction.
What penetration depth do you have in this simulation?
Same simulation, but now with friction.
Error at time step 0.6s
*ERROR: too many cutbacks
best solution and residuals are in the frd file
Process elapsed time: 1104.364 s
the value is 0.7mm(negative) or 0.8mm maybe, i lost my model files.
Here are the files. With and without friction.
Can you tell me what to do to get it done with friction?
Whether it’s frictional or frictionless contact, you still have large penetration. This has to be resolved by adding a small fillet to the edge od the PCB part, further refining the mesh locally (possibly, in a smaller region) or changing the contact settings.
Is there a optimum ratio between cells of the slave and master mesh to have less penetration?
Not really, but here the problem is more specific. You have a sharp corner, and it’s hard for the solver to properly establish contact between that edge and the rounded surface of the clip. In Abaqus, you could use a separate node-to-surface pair for that. Here, it might be best to just add a fillet to that sharp corner (and refine it properly). Adding more fillets is what helped resolve the issue with snap fit analysis described in the referenced CalculiX forum thread.
Thanks. I will do that
I have made a new model. Reduced the mesh size of the EON and added a radius on the edge of the copper-plated hole in the PCB.
Only the material of the EON has plastic properties. The copper only has linear properties to see if the simulation will run.
The simulation runs up to 1.3s of the 2s
Like to run with copper with plastic properties too, but that results in an ERROR.
EON_10103550_FEA_001_06-P.pmx (6.6 MB)
Question: How do I TIE the copper to the PCB inthe right way?
I am not entirely sure about the exact properties of the Copper-PCB interface. However, regarding the tie definition, I would suggest using a compound part with distinct material assignments. Please see the attached images for reference.
Regarding initial penetration and inspection of the load path be aware that ccx could be relaxing the contact stiffness to help for convergence and only at the end of the timestep it is increased to it’s requested value. For problems like this it could completely change the reaction and contact pressure response during the insertion and later withdrawal.
A workaround could be to a dummy step: Snap-fit contact snagging problem - #20 by SergioP - CalculiX (official versions are on www.calculix.de, the official GitHub repository is at https://github.com/Dhondtguido/CalculiX).
Thanks. I will try this.
If you choose HARD, then it relaxes, but I haven’t seen it when linear with defined stiffness was selected in the monitor output.
But further down the insertion, you see the deformation, and it seems then their the relaxation takes place.
I have re-modeld the pcb with the copper bushing with smaller mesh.
Also made the displacemant of the contact insertion very small.
I think that you have to make the step displacement smaller or equal to the mesh size of the slave to get it running.
The copper bushing and the contact are both materials with plastic properties.
It runs now well until a depth of 0.165mm then it .
divergence allowed: residual force too large
divergence; the increment size is decreased to 9.765625e-06
the increment is reattempted
to be continued
