ABAQUS stent analysis failing

[ryankb]

I'm having some difficulty running a stent analysis and I'm hoping there might be some expertise here that can help me out. I just got done taking the online stent simulation tutorial from Simulia, and now I'm working to extrapolate on my own practice. I have a very simple laser-cut style 8- strut, single loope strut "stent" in 1/8 symmetry. It's nitinol, with an expand, recoil, and pressure steps. It fails about 0.73 through the expand step with time increments too small error. (general static step). I'm trying to define the nitinol with plasticity so I can overstrain it and model a good recoil behavior. My material model is as follows:

7232772.81
0.33
4403414.861
0.33
0.048987845
986.2584
65533.12968
68269.43497
0
986.2584
31662.44994
28827.94359
75637.317
0.0515
0
0
10
68312.898
0.065
90286.44508
0.06949
112303.6486
0.07449
156220.4298
0.08449
174045.6
0.09
184923.45
0.095
188549.4
0.1
190724.97
0.105
191450.16
0.11
192175.35
0.15

("units" are psi and C FWIW).
I've also tried eliminating the plasticity part and it still fails around the same time step. The max stress is only around 70 ksi, so it's still well within the material model. I've done "tricks" with nlgeom, and general solution controls I0, and Ir. I attached my cae file here.

Any thoughts why this won't converge?

 

[Dave442]

I can't check your file at the moment but It sounds like you're trying to run a balloon-expandable analysis with a self-expanding stent. Doesn't make sense.

Nitinol stents aren't expanded, Their initial shape is set through processing and heat treatment and they are allowed to expand freely in the target anatomy due to the shape memory property of nitinol.

Recoil only occurs with balloon-expandable devices when you deflate the balloon. There should be no recoil with a nitinol stent since there is no balloon.

There is an Abaqus/Standard benchmark analysis in the documentation that involves crimp and deployment of a nitinol stent. You can check that for guidance.

 

[ryankb]

In order to "shape set" a nitinol stent in ABAQUS it typically is expanded and annealed through several steps before crimp and deploy. You're right, what I'm doing is a little atypical, however it is merely the start of what I'm hoping to do. If I can't get a single expansion step to complete, then I can't get to an anneal step, then another expansion, anneal, then finally to the part of the analysis I care about which is what you already stated. I'm playing with a few different things at the same time with this, so while some of it doesn't physically make sense, from an analysis perspective the methods are good to learn.

I'll see if the documentation has something different than the test problem I was working on in the tutorial.

 

[Dave442]

I understand the shape set process - that's not what you described previously.

If you're running into problems with shape set analyses, check the message file. Have force/displacement equilibrium been achieved? If not, you might have a problem with your boundary conditions. You can check the node and direction of the largest residual to see what portion of your model is causing problems and how it might not be constrained. What happens at 0.73 through the step? Do two parts come in contact? If so you might not have fully constrained one of them.

If contact hasn't converged you can adjust your interaction properties. Softened contact can help in these analyses. Where possible, avoid edge-surface interaction on your contact surfaces.

Also, if you think it's the material model, run it with linear elastic properties and see does it converge.

 

[ryankb]

I re-read my first post - I did not describe my problem well. I was multi-tasking and trying to leave the office all at the same time, and ended up with a poor problem definition.

Contact initiates almost immediately in the expand step. It quickly expands about 50% through the step, then bogs down. I ran the same model with the material model from ABAQUS, and it did complete, but with stress values an order of magnitude higher than what is possible. Just for completeness sake, here's the ABAQUS material model:

46728
0.33
25199
0.33
0.0426
4.5
358.2
437.8
0
4.5
124.25
17.75
537.3
0.0426

I'm hesitant to condemn my material model, because the two are so very close:

But on the other hand that one seemingly simple change really messes things up. Perhaps it's highlighting an issue somewhere else?

I'm running it right now with a linear elastic only "steel" model (no plastic definition at all), and I'll see if it completes.

 

[Dave442]

With a superelastic material model non-physical stresses are observed above strains of ~6%. Are you seeing strains that high? If so, I think your expansion is too aggressive. Can you split the step into two less aggressive steps?

 

[ryankb]

The Logorithmic strain is only at 1% - far below anything where I'd expect any issues. It's almost like the model isn't handling the austinite/martensite transformation well - and the stress and strain values aren't matching well (in my material model, at 1% strain, the stress should be around 65ksi, not 73ksi like I'm getting).

 

[Dave442]

Sorry, I assumed strains were high because you said "stress values an order of magnitude higher than what is possible".

Have you tried rerunning the analysis with loosened contact constraints? What are you using for interaction properties at the moment?

 

[ryankb]

So a quick update: I ran some jobs this weekend. The ABAQUS material model does complete, but the stress values are 4,300 Mpa - obviously way too high. The material model that I developed above doesn't get much beyond 2% strain before it fails - it doesn't make sense.

 

[Dave442]

I took a look at your model and I you have two problems.

Firstly, you're using inconsistent units. Your dimensions appear to be in meters but your stresses are in PSI. For consistency the stresses should be in Pa. Alternatively, scale your parts so they are in mm and adjust your stresses so they are in MPa - I find this much easier when modelling stents. Secondly, your transformation and volumetric transformation strains are different values. When this is the case, a different flow algorithm is used and the USYMM parameter is required on the *USER MATERIAL keyword. If you try to run the analysis without this parameter included you will run into convergence problems. Your model produced non-physical results with the Abaqus material model due to inconsistent units (dimensions are in meters but stresses are in MPa). Also, you did not have convergence problems with the Abaqus material model because the transformation and volumetric transformation strains are equal values.

When I addressed these problems your model ran fine. Here is the material model I used:

*Material, name=ABQ_SUPER_ELASTIC
*Depvar
24,
*User Material, constants=15, UNSYMM
4.9868e+10, 0.33, 3.036e+10, 0.33, 0.049, 6.80001e+06, 4.52e+08, 4.7e+08
0., 6.80001e+06, 2.18e+08, 1.99e+08, 5.22e+08, 0.0515, 0.

 

[ryankb]

I've been mixing/matching so many different attempts I must have mixed my units along the way and didn't realize it! I had attempted several different models, and used several different online resources to provide information. I feel like a dunce - complete rookie mistake.

Thanks also for the catch on the volumetric strain - you described exactly what I was running into. I'll go through and double check all my units, make the edit to the material model and try again. Thanks for bearing with me Dave!

 

[Dave442]

no worries - one other thing i noticed is that you hadn't specified any normal behavior in your interaction property.

You should specify this and be aware of what properties are being used.