Chinmay
Subscriber

I am not an expert but going through you post I observed few points I would like to share which I learnt during initial experimental stages of Static Structural. (maybe you are familiar with most of them)
1) In Bi-linear hardening, I could not see value of tangent modulus you used but in general do not use tangent modulus of 0 MPA (perfectly plastic) which contributed in convergence issues in my case.
2) In case of high plastic strain, I usually go for 2D plain strain model as suggested by Peter (maybe try mid surface in Space Claim but make sure plane is XY and no thickness in Z-axis). This will give an idea about what you are thinking is in line with what the software understands, if it works, you can go for 3D models.
3) The metal sheet you have used is quite long for initial try, because the longer it is, the more number of nodes and elements it will have and more time it will take to solve the problem.
4) In mesh settings, right click on Mesh --> show --> Sweepable bodies, you must see that the sheet is sweepable or you might have made some mistake in above steps, add Method, select sweep then manually select contact and target faces. (I see you have used NLAD, which cannot have that mesh). Then select no of elements to 6 (in case of NLAD) or 8 otherwise.
5) The friction coefficient value is quite high for metal to metal contact is what I believe which is another possible cause for convergence issues (if it is high, try reducing it till you get some results, then maybe try to increase a bit in next tries)
6) For initial tries, try not changing advance analysis settings, program controlled are best to try (otherwise you wouldn't understand where exactly you made mistake) Like pure penalty with normal stiffness value of 0.6 and in static analysis define by "steps" instead of "time". In initial substeps I think 100, minimum substeps 100 and maximum 10000 would be fine.
7) In NLAD, the remeshing takes place around 0.35 is what I can see in Force convergence graph, so try setting NLAD as manual if possible (but then # of steps needs to be increased, maybe try this later in simulation to improve results)
8) If you want finer mesh for specific part sheet (initially), use body split (divide the sheet into 2 or more bodies) in SC at appropriate distance and give different meshing to them reducing number of nodes and elements.
9) Save as this project to other name, clear results and meshing but keep all settings you need like remote displacement etc and then try to Archive this project to .wbpz extention for smaller archive file size.
10) Right click on solution information, insert, deformation and strain plotter will help you understand problems earlier than when the problem fails completely. (Select both trackers, right click and switch them to automatic update)
If I made some mistakes in this comment, Peter will definitely teach us something new.
Thanks CK