Abaqus FEA convergence issue

[teja781]

Hello all,

I have been trying to figure out why an abaqus simulation involving uniaxial tension test of a hyperelastic material (ogden model) is failing. The error in the *.msg file is

***NOTE: THE SOLUTION APPEARS TO BE DIVERGING. CONVERGENCE IS JUDGED UNLIKELY.
***ERROR: TOO MANY ATTEMPTS MADE FOR THIS INCREMENT

I am attaching the msg file here and willing to provide any other additional information.

Any help is greatly appreciated

Regards

 

[csk62]

Can you attach your input file and/or cae file?

 

[teja781]

Thanks for the reply. Here it is.

Regards

 

[csk62]

Have you tried using other similar constitutive material models to see if you can get at least get convergence? Maybe Mooney-Rivlin?

 

[teja781]

Yes. Also one term ogden and Neo-hookean. None of them give any convergence issues. Its only with two term that I am facing this problem.

Regards

 

[csk62]

Hmm... based on this information this may be a material modelling issue, I think I would recommend posting this on PolymerFEM or the likes.
You might get lucky here with some guys experienced in hyperelasticity, but from a metals guy like me, I think this is the extent of help I can offer.

 

[IceBreakerSours]

Where did you get your constants from? Literature? Or, did you fit your material law to some experimental data? Try the material constants on a homogeneous uniaxial deformation on 1 element.

This is going to be a lot more than you are looking for but this subject interests me and I hope this gives you some background:

Ideally, if one wishes to have complete understanding of this business, one should write a symbolic math script and do a nonlinear curve fitting to get their material constants, verify Abaqus results against the results from the script, and only then go to the next step. It is known that for bounds have to be set on the material constants for the material to be physically reasonable (due to inequalities such as Coleman-Noll and Baker-Ericksen). Baker-Ericksen does not hold for anisotropic materials. The downside of Coleman-Noll inequality is that it is unreasonable under large deformation but this is the best commercial codes will offer, if at all.

Additionally, using the deformation gradient for a simple deformation, check if the elasticity tensor (C_ijkl) is positive definite (i.e., the energy is a bowl in 3D Euclidean space), full rank (rows/columns are linearly independent), and well-conditioned (condition number should not be too high) over the entire range of deformation. You may then try to impose non-trivial deformations and see how the model is doing. All of this may be done in a symbolic math script.

If the simulation in an FE solver still gives issues, then the problem *may* have to do with the implementation. And, if that is the concern, you can always try to use some other code (freely available or otherwise).

If you are interested in this subject, you may wish to look up Neff and Schroeder's (relatively) work on polyconvex strain energy density functions.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083

 

[teja781]

I am trying to fit the two term ogden model to experimental data. I have an optimization script that generates a lot of parameter sets for which the reaction force is generated using the abaqus simulation and compared to the experimental data. The optimization script is trying to zone in on the global minimum of this value. I am in fact trying to come up with reasonable bounds for the parameters to be tried in.

But I digress, for some of the parameter sets (about 1/3rd) the abaqus simulations are failing. I have taken out all the values for which the simulation is failing and applied the Drucker-stability condition to it. Roughly half of them failed the Drucker stability condition so those can be eliminated. I have posted the input file from one such case where the parameter set passes the Drucker stability condition. I am not sure if I can come with an exhaustive list of conditions to be checked so that the parameters will make physical sense. I am going to check the strain energy density function next.

I posted this here to get some extra eyeballs to look at the input file and may be someone can spot something fundamentally wrong/silly in my input file that I am just not able to see.

Regards

 

[IceBreakerSours]

You are assuming pure incompressibility, which is an additional constraint on the DOFs of the nodes. You might want to allow some compressibility (particularly because there is no confinement being modeled). In fact, try to vary K_0/mu_0 (10,100,1000,10000) and see what effect it has on your simulation. Check the Abaqus Analyis User's Guide for more.

*********************************************************
Are you new to this forum? If so, please read these FAQs:

http://www.eng-tips.com/faqs.cfm?fid=376

http://www.eng-tips.com/faqs.cfm?fid=1083