Nonlinear analysis - failure to converge

[CR27]

Hi,

I'm modelling the inflation of an angioplasty balloon within a stenosed artery (artery with plaque) in \Standard. I'm working with a 1/4 model enforcing symmetry boundary conditions and fixing the artery at each end. The balloon is inflated within the artery to a diameter to match that of an unstenosed artery using displacement in a cylindrical co-ordinate system. My model runs perfectly with a linear elastic properties and nlgeom off and easily shows the "squashing" of the plaque in this model.

However, I am attempting to introduce non linearity in the model and am unable to reach convergence doing so. I've attempted automatic stabilization, the addition of damping parameters, decreasing my step initial increment to 1E-6 and minimum increment to 1E-20 but it still begins to abort with excessive distortion of elements... Other things I've tried include increasing mesh density and altering boundary conditions in the model..

I am beginning to think I can't solve this problem in Abaqus/Standard but am reluctant to move to Implicit or Explicit as I am working under time constraints and am not familiar with either.

Has anyone any tips or suggestions that might help?

Thank you

 

[FEA way]

Such problem definitely should be solved with nonlinearities included. Rubber can be modeled using hyperelastic material (e.g. Mooney-Rivlin). Also include NLGEOM and what’s ecen more important - define contact. Personally I would use Explicit with General contact for that.

 

[CR27]

I already have hard penalty contact defined in the model and have attempted to apply hylerelasticity to the artery using a Mooney-Rivlen constitutive equation and nonlinear geometry. My balloon model is simply linear elastic. I'm just wondering if it's possible to solve this problem in Standard as all my attempts are producing negative eigenvalues once the balloon begins to expand.

Would there be much difficulty in moving this to explicit?

 

[FEA way]

If you have access to Knowledge Base take a look at the „Understanding Abaqus/Standard negative eigenvalue messages” article. In your case I think it’s because of highly distorted elements. Apart from increasing mesh density make sure that its quality is good. Use Verify Mesh tool for that purpose.
Also check your material properties (especially units) and try with lower load or different contact settings.

 

[Dave442]

what's the purpose of the analysis?

Is the balloon compliant, semi-compliant or non-compliant - this dictates what assumptions you can make to simplify the model.

You also said the balloon is inflated by specifying a displacement - how does that work? Surely it should be pressurized?

I've run analyses like this in the past. I had to use explicit as the balloons are folded and unwrap during inflation.

Explicit was required for the complex contact.

 

[DanStro]

Is the excessive distortion warning from the elements in the balloon, plaque,or something else? Have you tried using hybrid elements for the parts that have excessive deformations?

 

[IceBreakerSours]

Abaqus/Standard uses the implicit scheme; it sounds like what you are currently running is a static analysis (i.e., inertia is ignored). In all likelihood, you will have to resort to the explicit scheme for solving this problem.

In addition to what has been suggested/asked above, I am also curious as to the purpose of the analysis because this problem has been solved many times by various groups. In the last couple of years, Markus Geith/Marcus Wagner/..and colleagues have published some good computational work on balloon expansion of stents.

*********************************************************
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