Abaqus/Standard 6.8-2 Job Error - Too many attempts for this increment

[maxmg]

Hi All,

I am having some trouble getting a converged solution for my hand/wrist model.

Here are some details of the model:
1) The model has 58 parts total: 29 for trabecular bone of the hand/wrist and 29 for cortical.

2) The parts representing trabecular bone are constrained to their relative cortical counterparts with tie constraints that were found using the constraint detector from the Interaction module.

3) There are contact interactions between the cortical bone parts representing joint articulations. The interactions are tangential, frictionless, and finite sliding interactions.

Problems:
1) The job analysis aborts with 'Too many attempts for this increment' error.

2) The model has 53 unconnected regions.

3) There are numerical singularities in the model.

4) Many nodes for tie constraint parts cannot be tied because they are not within the position tolerance (using computed default value).

Troubleshooting/Questions:
I have searched the Abaqus manual and other threads in this forum for tips. Here is what I have tried so far:

1) Decreased the initial increment size for the analysis step from its default value of 1 to 1E-009. Received same error 'Too many...' and other warnings.

2) Used contact controls - stabilization (default values) along with decrease in initial increment size. Received same error 'Too many...' and other warnings.

3) The 53 unconnected regions in the model are most likely due to the initial spacing between the contact pairs. From reading other threads, this problem can be solved by setting fixed displacements on the contact pairs in a first step so that they are touching at the beginning of the analysis. Then remove the fixed displacements in a subsequent step.

How do I find the amount of displacement to apply? I have a large number of contact interactions. And would this procedure introduce overclosure between contact pairs?

4) The numerical singularities will most likely disappear after I fix the unconnected regions issue.

5) How do I find the distance between tie constrained parts as to apply an adequate position tolerance?

Any help is greatly appreciated,
Max

 

[maxmg]

I forgot to mention that I have springs between the cortical bones to represent the ligaments. From what I've read in other threads, if I have springs connecting the bones that will contact then I do not need to define contact interactions for them?

 

[gwolf2]

Ouch! I have been using ABAQUS for 20 years for some fairly complex analyses involving contact. The job which you describe would still be challenging for me.

I suggest that you try just one grounded finger with three bones and two joints, then work up from there.

Good luck!

gwolf

 

[corus]

gbor is right, with so many regions in contact it might be just too much to do. For highly non-linear problems you might be better trying an explicit analysis. You don't have to worry so much about ensuring you have equilibrium then, but the down side is it'll take for ever to run. Otherwise try and simplify the problem as much as you can (no non-linear materials for example) and then introduce them back in to see where it fails. Use *contact controls, automatic tolerance too.

The initial displacement you use tends to be very small, just enough for a nudge.

corus

 

[maxmg]

Thanks for the suggestions gwolf2 and corus.

I've reduced the complexity of my model as much as I could. It still won't finish running. Stuck on the "too many increments..." error.

Would either of you be willing to take a quick look at the model and perhaps, point out the problem areas? I have uploaded the .cae file to rapidshare.

http://rapidshare.com/files/199811886/Hand_SIM4-7-2.cae.html

Max

 

[gwolf2]

I can't read CAE files and I don't have access to ABAQUS atm. You need to post a .inp file and find someone with an ABAQUS licence.

gwolf

 

[ccheric]

maxmg,

There are so many reasons who your model didn't converge...

First of all, did the analysis progress at all? (total time >0 ) If you are stuck at t=0. Then it's possible that you have some over constraint or bad BC problems.

If you get to some point in a step, then get stuck, this is much better because you know your model works. You can try:
* add contact stabilization or whole model stabilization
* up the limit on "increments" in solution control
* up the min time increment (make it like 1E-15)

You can also learn more about what's wrong by reading the "warning" tab. The error tab just tells you it crashed, warning tells you why.

See if you can find more info from "warning" or ".dat" log.

 

[maxmg]

Thanks for the suggestions ccheric. I've already tried most of them out, still get the "too many attempts..." error.

Quick question. When using the verify mesh tool (Mesh > Verify) are the default values good enough or should I change them? For instance, is an aspect ratio of 10 a good error checking parameter for the mesh? I ask because I have distorted elements when I run the analysis but the verify mesh tool doesn't catch them with the default parameters.

Max

 

[ccheric]

If your analysis can't even get a step forward (total time =0), it is possible that your model is invalid.

* quick note: did you turn on "nonlinear geometry"?

I don't know much about distorted elements. If you are mesh savvy, use mapped mesh. (you can partition your model to guide the mesh mapping) Mapped mesh generally yields the better element shapes for higher accuracy.

 

[maxmg]

Switched to Abaqus/Explicit. It works now. Thanks for your help, gwof, corus, and ccheric.

 

[gwolf2]

> Switched to Abaqus/Explicit. It works now.

Well it´s more or less bound to run because Explicit can deal with free bodies. If the loads on your model won´t balance statically, there is likely still a problem with the model.

 

[oroden01]

I have access to abaqus licenses for version 6.7 and 6.8. if you would still like someone to look at it I'll be happy to, it sounds like a very interesting problem and pretty difficult!!! Are you looking at your output files during the analysis? does it pass one time point iteration? what is the largest residual force or largest nodal displacement for the steps it does finish?