Indentation with two materials: convergence problems

[bra1]

I want to model an indentation. The part wich is indented by a punch is made of two materials with different yield stress. I noted that when I use the values 376 and 200 MPa for Yield Stress everything is ok. But if I choose 376 and 110 MPa the job is aborted because of convergence problems. It happens in the final part of the job.
I think It has something to do with the difference between the values. Am I right?
Does anybody know how I can solve this?

Thanks in advance,

BRA

 

[mrgoldthorpe]

It depends on what is causing the loss of convergence. I assume that the increment size is being cut back because you're not achieving either force/moment or displacement convergence. Look at your .msg file and tell us what field variable is causing this. One of my tricks in this situation is to relax the convergence tolerances (I often find that the displacement tolerance is the culprit). Another trick is to restrict the maximum size of the increments to say no more than 5% of the step size. You might find that by doing this solution takes a different 'route' and the problem goes away.
MRG

http://www.analysis.demon.co.uk

 

[bra1]

MRG,

Thanks for your attention. I looked at my .msg file and I think the error is because the displacement problems. The last increment reports this:

THE MOMENT EQUILIBRIUM EQUATIONS HAVE CONVERGED
DISP. CORRECTION TOO LARGE COMPARED TO DISP. INCREMENT

This message repeats during 5 interations and the job is aborted. I have started using abaqus few weeks ago and I'm using abaqus CAE. Could you tell me how can I relax the convergence tolerances?

Thanks in advance,

BRA

 

[harry123456]

In abaqus manual 6.4 read " Getting started with abaqus standard/keywords version" In the section for non-linearity read the non-linear skew plate example. It explains how abaqus computes the force and displacement correction. From there you can change the displacement correction factors to get convergence. Channging these factors though might not produce accurate results though I think.
harry

 

[mrgoldthorpe]

Try this. It sets a more relaxed displacement tolerance of 10%, i.e. allows corrections to the displacements of 10% compared with the actual displacements.
*CONTROLS, PARAMETERS=FIELD, FIELD=DISPLACEMENT
** R_n^alpha C_n^alpha q_0^alpha q_n^aplha R_p^alpha eps^alpha
, 0.10 , , ,
btw, does ABAQUS report nodes going in and out of contact? Also, try restricting the maximum size of the increment:
*STATIC
** init'l time period min. max.
** time of step time time
0.01 , 1.00 , 1.0E-6 , 0.05

MRG

http://www.analysis.demon.co.uk

 

[harry123456]

If it is a dynamic problem then explicit would be easier but if it is just a static one like the classic indentation problems you will have to be careful when you do explicit, try it out with standard and see if it works. Sometimes I have found that if you change one tolerance the other might fail to converge. Just a thought and may not happen in your problem.
harry