View Full Version : ABAQUS 6.7 for silicone rubber riddon
I've been trying to simulate stretching on a silicone ribbon (25 mmx150 mmx0.8 mm). I though it would be fairly simple but I quickly realised that hyperelastic materials had nothing to do with the more conventional ones.
On ABAQUS/CAE, I used a 2D planar model with one fixed end and the tension is applied on the other. I created a hyperelastic material with test data. I’m now very confused with the choice of my mathematical model (strain energy potential) which would allow me to obtain reasonable results. I read on the web that for silicone, Yeoh would be acceptable and I was able to complete my job analysis without any error messages but I realised that the elongation I got was about 30% out of my experimental results. I also noticed that if I slightly change my meshing, I still get error and the message file always say the same thing: ***NOTE: THE RATE OF CONVERGENCE IS VERY SLOW. CONVERGENCE IS JUDGED UNLIKELY. ***ERROR: TOO MANY ATTEMPTS MADE FOR THIS INCREMENT.
Here are my main concerns:
1. Do I choose a mathematical model according to the material I use or depending of the application? Which one would be appropriated for my situation?
2. Do you have any recommendation for the mesh? (Here’s what I use now: CPE4RH: A 4-node bilinear plane strain quadrilateral, hybrid, constant pressure, reduced integration, hourglass control.)
Thank you very much for your help,
1. I recommend that you select a material model based on the material.
2. The CPE4RH elements are typically good.
I suspect that your problem is related to the material parameters that are used in the Yeoh-model. An improper selection of material parameters can make the material model unstable at larger strains. Another possible problem could be related to hourglassing. You might want to switch to CPE4H elements to eliminate issues related to hourglassing.
Thank you very much for your help, I'll try that this morning ;)
I’ve been working on my simulation this morning and I still faced some issues. As you recommended me, I gave a try with a CPE4H mesh to eliminate hourglassing and the model didn’t converge and showed the same error message as usual (***NOTE: THE RATE OF CONVERGENCE IS VERY SLOW…). I switch back to CPE4RH.
a. I consulted the information given in the “ABAQUS Analysis User’s manual” (17.5.1) and they recommend the Marlow model when only uniaxial data is available. What do you think about this? Do you believe Yeoh is still a better model for my situation?
b. I always end up to be able to converge with my analysis (Yeoh or Marlow) but the result I get is always 30% off the track. Do you think it’s the best ABAQUS can do? (I hope not)
c. What does the option hourglass do? I looked in the information provided and it was not enough to help me understand.
I joined the file of my Yeoh model if anyone wants to have a look at it. If somebody sees anything wrong with it I would be more than happy to know it.
It is good to hear that you at lest got some results. If you post a graph of the experimental stress-strain data I can provide some comments about how accurate you are likely to get with a hyperelastic model.
There is nothing wrong with the Marlow model. You can use it instead of the Yeoh model if you like.
Hourglass stiffness is required when you use reduced integration point elements (eg CPE4RH). In somewhat simplified terms: the reduced integration elements run faster but can undergo a specific type of (hourglass looking) deformation without even any applied strain. To overcome this problem you need to specify an "hourglass stiffness".
First, thank you very much for your help; I am very impressed with the efficiency of this forum. You are very helpful!
I think I found what was wrong with my model.
When I did the experimental data, I used a silicone ribbon on which I applied tension at one end. I applied a charge, and I measured the stretching, then I applied some more weight, I measured again. And so on.
When I did it at first, I did not know that actually, I was working with a silicone which wasn't made to support large extension strain, so the material got probably "worn" and "softer". And after the test, I could definitely stretch it way more than if I had applied that same load with a new ribbon which had never been used. That might explain why the stretching I measured was about 30% longer than what ABAQUS says.
We decided to switch material and we'll go with a natural rubber of a duro 40. We noticed that it had characteristics that suit better to our needs. I'll measure my nominal stress and strain again but I'll try with a new ribbon for each try... I'll see if the results given by ABAQUS are closer to mine.
If it works with a ribbon, then I will try with a circular diaphragm… I go one step at the time to make sure I control well the simulation.
Dear Dr. Bergstrom,
I am still working on my stretched ribbon simulation. Last week, I collected new experimental data but I switched material: I’m now working with some natural rubber ribbon. As I mentioned in my last post, I decided to take only one measure by sample. I took about 10 different measures.
I am still working with the Marlow model. Once the material was defined, I also specified the mesh I would use: CPE4RH. For a tension of 0.0553 MPa, I tried different number of elements and I determined that for 1000 elements, I get a converging solution. For more than that, the solution wasn’t more accurate so I thought that mesh was good enough. This mesh worked also well for 0.1010 MPa and 0.1344 MPa. When I tried with 0.1678 MPa and higher, it stopped working. I tried to modify my mesh type, element quantity and to change my model to Yeoh: nothing worked. Is this normal that one mesh works for one loading and not for another slightly bigger? This problem occurred with the simulation of a 1213 mm long ribbon, it worked without error messages for the shorter ribbon simulations (100 mm, 50 mm). (See attachment)
One last question: On the graph showing the stress and strain resulting from the simulations, we can see the 3 simulations are superposed but are offset from the experimental results provided to Abaqus. I though it might have something to do with true vs nominal strain/stress. I read on the documentation “Getting started with Abaqus” that platic simulation used true strain/stress is used…but hyperelastic definitely requires and gives nominal values, right? Am I right to expect my experimental data curve provided to my material definition to be superposed by the resulting one? I think so… What could make this offset between the simulation and experimental curves?
I hope my questions are not too hard to understand.
Thanks again for your help!
Internally Abaqus is using true stress and strain for the calculations. The interface to the hyperelastic features are mostly written in terms of engineering stress and strain. You can convert between the two by assuming incompressible behavior.
The experimental data and the model predictions should overlap relatively OK. I am not sure why that is not the case for you :(
And would you have an idea why my simulation for the 1213mm ribbon works for low tension values and doesn't for higher loads? I thought one mesh configuration would work for every loads.
This work is a part of my master project and nobody in my department is used to work with large deformation. It looks so simple at first sight but that is giving me good headache.
If you have any recommandations, that would me more than welcome.
Powered by vBulletin® Version 4.2.0 Copyright © 2013 vBulletin Solutions, Inc. All rights reserved.