radial force stent crimping

[AliceF]

thread799-356649

Hi to all,
I'm trying to reconstruct a numerical model of two Nitinol stents and I need information about the radial force they exibit.
I have meshed the stent frame models with C3D8R elements and I have considered the UMAT subroutine based on Auricchio and Taylor to reproduce the material properties. In addition, I have built a cylinder (SFM3D4R elements, rigid) around each stent. The diameter of the cylinder is reduced and then re-explanded. I have performed analyses with Abaqus\Explicit 6.13 and they run. Now I have a problem: I want to evaluate the radial force of the each entire stent but I don't know how it is possible to do this. Which is the best way to evaluate it? In several articles I have found force-diameter curves related to the entire model. At now I am only able to evaluate the force in a single point. Which parameters are necessary to trace during the whole simulation to reach my pourpose?
Best regards

 

[Dave442]

Hi,

You need to sum the radial reaction force at each node on your rigid surface at each increment to obtain the force response over time. You can figure out the diameter values from the starting diameter of the rigid surface and the applied displacements. Alternatively, you can simplify this task significantly by using a reference point and *Equation to control the rigid surfaces. That way, you can just plot the radial reaction force for the reference point during the analysis (no summation required).

This type of analysis would also be a lot quicker to run in Abaqus/Standard.

Good Luck,
Dave

 

[AliceF]

I have another problem: for me CF is 0 at each node. Do you have any suggestion to solve this problem?
(I have selected
penalty technique: 'Normal behavior constraint enforcement method' = default; pressure-over closure: 'Hard contact';friction formulation='Penalty'; friction coefficient=0)

Thanks,
AliceF

 

[Dave442]

You want RF (reaction force) not CF (concentrated force)

 

[IceBreakerSours]

I agree with both of Dave's suggestions - implicit solver and RF (not CF). Also, you probably meant to say VUMAT; UMAT does not work with Abaqus/Explicit. So, use the UMAT with implicit solver.

FYI: I am not sure if having a friction coefficient of zero is very accurate. Since it is likely a small number (0.01, perhaps?), you will be better off keeping it zero until you get the rest of the model set-up correctly.

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

 

[CamiS]

Hi guys,
my question is pretty similar. I'm using Abaqus/Explicit. The crimping tool in my case is octogonal in cross section. I used 3d deformable part and meshed it using SFM3D4R elements. One node on the stent is fixing it in the Z axial direction (cyl coord) and tool is crimped by inward radial displacement. Simulation seems to work fine and now I need to compute the radial force. How am I to do that? I looked at Reaction Force for the nodes on the tool, but they are far too small to what I'd expect. Any advice would be really appreciate it.

 

[Dave442]

Hi,

You need to follow the exact same instructions i gave AliceF. Sum the radial reaction force at each node on your SFM3D4R surface(s) at each increment to obtain the force response over time. Simplify this task significantly by using a reference point and *Equation.

Dave

 

[CamiS]

Sounds pretty straight forward, but I can't seem to be able to do it. If I use a Smooth amplitude for applying the displacement, I get a wave curve for the RF at each node of the crimping tool. If I sum up the absolute values of these forces at each time increment, the values are around 1 order smaller than what I would expect. If use a tabular amplitude, the RF are zero at all nodes. What I'd like to see is an increase in the RF from 0 up to a max value corresponding with the displacement applied, and then a decrease in the RF down to 0. I would like to see the hysteresis. What am I doing wrong?

 

[Dave442]

Avoid using amplitudes by running your analysis in Standard. Its a stent and a rigid surface - there's no complex contact and no need for explicit, you're just taking much longer to obtain less accurate results. Aside from that, check your material properties (units) and applied loading conditions. Check that your explicit analysis remains quasi-static and that kinetic energy is negligible throughout. Finally, check that you are not making any errors when post-processing the reaction forces.

Maybe throw up some images of your model or share your input deck if you still have problems.

 

[CamiS]

Thanks for your support, Dave. The stent is braided, the contact is pretty difficult, all researchers as far as I know have used Explicit. However, I managed to get the simulation running in both Standard and Explicit. The analysis is quasi-static as you've mentioned, I checked the kinetic energy. The material model & units are correct, because I used the same in other simulations with good results. I get similar results for displacements and stresses in both versions, and comparing the stent elongation with experiment they seem to be accurate. There must be an error somewhere related to the reaction force, I didn't figure it out yet.

 

[Dave442]

Apologies, a braided stent is a more complex contact problem. Yes sounds like it must be an issue with how you are you extracting the reaction forces - how exactly are you doing it?

 

[CamiS]

This is how the reaction force vs. time looks. It's not correct...

I requested Reaction Forces (History Output) for the crimper set (16 nodes). I added up the absolute values for each node per time increment. The time for the whole step is 1. Crimping goes from 0 to 0.5, uncrimping 0.5 to 1.

 

[Dave442]

Something is definitely not right there. Can you share an input deck or some images of your model?

 

[CamiS]

 

[CamiS]

To solve the problem in a reasonable amount of time and to be able to make iterations, I used mass scaling. I didn't do a natural frequency extraction analysis, I tried a factor of 10 initially, then picked a factor of 400. The kinetic energy looked low, but maybe not low enough. I think that's the problem, the model looks like it's oscillating.

 

[Dave442]

You are also crimping/expanding your stent over 1s which seems fast. Check that your analysis is actually quasi-static by plotting the kinetic energy versus internal energy. The kinetic energy should be <5% of the internal energy throughout the duration of the analysis. If you are seeing oscillations I expect that the kinetic energy is too high due to excessive time/mass scaling. You mentioned that you got the analysis running in standard, what do the reaction forces look like in that analysis?

 

[CamiS]

In Abaqus/Standard, the Reaction Forces for half the nodes look like in the photo:

For the other half, it's the same signature, but magnitude ~8N. The stent is not quite positioned centrally, so I suspect that's why the values are not identical.

 

[Dave442]

Have you transformed results to polar coordinate system before extracting RF1?

Definitely an issue with your explicit analysis by the looks of it.

 

[CamiS]

That might be the problem, Dave. I haven't done it. Can you point me to an Abaqus Example\Analysis guide to see how it's done?

 

[Dave442]

By default, the reaction force you output has three components (RF1, RF2 and RF3) in the three global Cartesian directions. You are only interested in the reaction force in the radial direction so you need to define a polar coordinate system, transform your data and extract the radial component.

In Viewer you can go to "Tools -> Coordinate System -> Create" to create a polar coordinate system. Then go to "Result -> Options -> Transformation -> User-Specified" and select the new polar coordinate system to transform your data. Now you just extract the RF component corresponding to the radial direction.