Tensile testing simulation of PTFE (teflon) - material model

[Bonias]

Hi,

I have to perform a simulation of tensile testing of PTFE(teflon). I've been given the data about the experiment (I have the stress-strain curve, Poisson's ratio, sample dimensions, strain rate). The problem is that this material is very ductile and the percent strain is equal to 246%. I work in Ansys apdl and I've been struggling with choosing the correct material model. Because I have the stress-strain curve I tried with
nonlinear -> inelastic -> rate-independent -> isotropic hardening plasticity -> Mises Plasticity -> multilinear
I just copied the points from the plot I was given (experiment data) and created the same stress-strain curve in Ansys. I know that behavior of PTFE depends on strain rate but in this case the strain rate is 0.5mm/min so I think it can be neglected at first. Anyway every time I start simulation I receive information "one or more elements have become highly distorted..." after some time. My guess is that this happens because the stress value exceeds the value from the curve (but it doesn't happen when I input true stress-strain curve). But I don't know why because the stress-strain curve becomes almost horizontal at some point (if the curve is engineering curve). My second guess is that elements' elongation is to high but have no idea how to prevent that.
Can anybody help me to solve this problem? Why I keep getting this error and what material model would be correct for Teflon in Ansys apdl? I enclosed a picture of the shape of the elements at the error step

PS I really read a lot about nonlinear simulation in Ansys, I tried so many different solution settings and it didn't help at all so the cause of the problem must be somewhere else

 

[Petr Vymlatil]

Bonias,

I am not sure which model is right for teflon, but if you can neglect strain rate, your choice is OK.
Be sure that you are using nlgeom,on (includes large-deflection or large strain effects).
I would recommend to load with displacements.
ANSYS expect TRUE stress-strain data. As far I know, ANSYS extrapolates the curve if the maximal value in your stress-strain definition is reached. So if your true stress-strain curve is monotonically increasing function it should be OK.
According my experience with plastics the high distortion errors occurs due to very high elongation of an element (in tensile test the whole elongation of the rod is concentrated at few elements which have very large elongation, similar to necking).
You could try Rezoning to eliminate distorted elements.


Petr Vymlatil (

http://www.designtec.eu)

 

[Bonias]

Thanks Petr for your answer. I didn't know that Ansys expects true stress-strain and extrapolates the curve.

Of course I use nlgeom,on and my displacement is applied in 100 steps (the analysis is transient so every step is divided into subsetps, the number of steps is rather random)

I read earlier about rezoning and I was thinking about introducing it to my simulation but the ansys help says

Rezoning is effective only when the mesh distortion is caused by a large, nonuniform deformation. Rezoning cannot help if divergence occurs for any other reason such as unstable material, unstable structures, or numerical instabilities.

where the definition of unstable material is

Most nonlinear material models, especially those employing hyperelastic materials, have their own applicable ranges. When a deformation is too large or a stress state exceeds the applicable range, the material may become unstable. The instability can manifest itself as a mesh distortion, but rezoning cannot help in such cases. While it is sometimes difficult to determine when material is unstable, you can check the strain values, stress states, and convergence patterns. A sudden convergence difficulty could mean that material is no longer stable. The program also issues a warning at the beginning of the solution indicating when hyperelastic material could be unstable, although such a warning is very preliminary and applies only to cases involving simple stress states.

so I am not sure if this could help in this case.

 

[IceBreakerSours]

Please know that: a) I do not know anything about PTFE, b) I do not know the purpose of the simulation, and c) I am not an ANSYS user!

That said, looking at some generic curves for PTFE suggests you ought to look into, at least, isotropic hyperelastic material model (neo Hooke, Mooney Rivlin, Ogden, Yeoh, etc.) and add some simple linear viscoelastic effect (Prony series) to it. On the other end of the spectrum, you may need a more advanced treatment like the Bergstrom-Boyce model. Click here for a quick overview.

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

 

[Bonias]

IceBreakerSours I thought about using hyperelastic model, but the most essential feature in my simulation is plastic deformation. As far as I know Ansys do not allow to combine hyperelastic model with plasticity. But thank you for the link. This paper seems to be very valuable!

 

[IceBreakerSours]

In the large scheme of things, it might be more financially prudent to contract the work out to a consultancy (Axel, Veryst, .. ..). Whether it makes strategic sense or not depends on the situation.

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

 

[rickfischer51]

Rather than rezoning, start with a mesh bias so that the size parallel to the load is small compared to the size transverse, so as it stretches, the elements become square, then distort so that the size parallel to the load is larger than the size transverse. Also, I think you need a much finer mesh. Also also, you might take a look at a plane element, plane strain with thickness specified.

Rick Fischer
Principal Engineer
Argonne National Laboratory