Abaqus and hyperelasticity

[jimstazinsky]

I am a new abaqus user. I have done some reading of simulia provided literature/other forum posts but can't seem to solve my problem with negative eigen values when I try to run a hyperelastic analysis (my job is always aborted, and never finishes). Can anyone tell me what are the strain limits abaqus is capable of modeling accurately?

I have uniaxial data and have tried making up biaxial and planar data that I believe to be realistic. Here are the data sets. However, I can't get elongation for a simple solid rubber block (constrained from all translations and all rotations at one end and with a pressure applied to the opposite end) of more than about 10%. I am looking to get elongations of about 500% for my application.

Thank you ahead of time for any assistance or insight you can provide.

Uniaxial (strain, psi)
0 0.4 0.8 1.2 1.6 2 2.4 2.8 3.2 3.6 4 4.4 4.8 5.2 5.6 6

0 300 400 500 550 680 800 900 1080 1200 1350 1550 1680 1850 2000 2100

Biaxial (strain, psi (made up))
0 0.4 0.8 1.2 1.6 3 3.6 4.4 5.2
0 320 430 600 700 1200 1600 1900 2600

Planar (strain, psi (made up))
0 0.4 0.8 1.2 1.6 3 3.6 4.4 5.2
0 0.4 0.8 1.2 1.6 3.1 3.6 4.4 5.2

[Mr. Inventor]

Which Hyperelastic Model do you use?

I would suggest you try the Yeoh Model with only the uniaxial testdata.

I don't think there is a limit for maximum strain, but it depends on the Hyperelastic model. Try to evaluate the Materialmodel, so you can see if it is stable.

Hope this helps.

[jimstazinsky]

I was using the Neo-Hookean model (Reduced poly n=1). I tried your recommended approach with using only uniaxial and switching to Yeoh, but I still can't get above about 10% strain. :(

Both the Neo-Hookean and the Yeoh models are stable for all strains between -0.5 and 6.0.

Thanks for trying to help though. Any other suggestions will be welcomed.

[Mr. Inventor]

Which element type are you using? S3D8RH should be ok.

How much elements are you using for your rubber block?

Maybe the problem is the boundary condition or the pressure. You can try to replace the pressure with a displacment boundary.

A picture of your rubber block could help to understand the problem.

[jimstazinsky]

Mr. Inventor and everyone else,

I'm currently using C3D8RH elements. For my first analysis I used 16000 elements, seeding a prism with a square cross section in 20x20x40 (to ensure each element is a perfect cube). My second analysis, which took about 2 hours, I doubled the seed number on each end, which yielded 128,000 elements. Unfortunately, the analysis still fails to finish.

Unfortunately, I can't use a displacement instead of a pressure boundary condition, because my application is to obtain the displacement my part will see under a known pressure (not stress, so I can't do an inverse analysis).

I'm having some trouble uploading a picture, but I'll do my best to describe the model.

It is a prism with a square cross sectional area. It's bottom 10x10 (intended units inches) face is constrained from all translations and rotations. It's top 10x10 face has a uniform 150 (intended units psi) pressure acting on it so as to put the block in tension. The length of the prism/block is 20. The pressure is ramped up. Let me know if any more information is needed for clarification.

Once again, thanks for everyone's help. I would really appreciate anymore assistance/ideas as to how to solve this problem.

[Mr. Inventor]

Try to constrain only the translations and not the rotations. Maybe some elements are overconstrained.

Change the elementtype to C3D20RH, and reduce the number of elements. These elements could work better if you have problems with "Hourglassing", but they need much more time and memory.

It would be useful to see the undeformed and deformed shape of your block. You could also try to upload your .cae file, so we can see the problem for our self.

[carita]

hi jimstazinsky,

I'm dealing with hyperelasticity for the first time too!!!

Was wondering, is the nlgeom option on?

And also, did you have a look at the message file while you monitor your job? There are few parameters there you can play with...

Regards,
Carita

[jimstazinsky]

Thanks again for all of your responses!

To Mr. Inventor:
I did indeed try C3D20RH elements and removed the constraints on all rotations, leaving only the constraints on translation in any direction. Still no luck. Curiously though, when I subjected the block to a much smaller stress (150 psi) than my intended value, the analysis did run to completion when LESS elements were used. That is to say, when I seeded by 10x10x20 block by 10x10x20 seeds respectively, my analysis did not finish (see the .cae I have attempted to attach). However, when I reduced the number of seeds to 5x5x10, the job reached completion. Why is this so? Also, since this prevents me from doing a convergence study, I can't have much faith in these results. Please let me know what your thoughts are.

To Carita:
I have indeed togged nlgeom on and my warning messages under job>monitor are as follows:
Excessive distortion at a total of (some x number) integration points in solid (continuum) elements
The strains are so large that the program will not attempt the hyperelasticity calculation at (some y number) points

What are some of the parameters that you had in mind?

If anyone else would care to comment on how large of strains they have been able to produce in ABAQUS and what was their strategy in doing so, I would be much obliged.

Thanks :)

[Jorgen]

You should be able to reach >> 100% strain.

Can you attached your inp-file or cae-file?

-Jorgen

[jimstazinsky]

I'm sorry, this may be a very stupid question, but how do I attach a .cae? When I click on "attachments" paperclip, even when I filter for "all file types", I still can't see the .cae files I have in the folder.

Is there another way to attach?

[Mr. Inventor]

Valid file extensions: bmp doc gif jpe jpeg jpg pdf png psd txt zip

Zip your .cae file and try to attach it.

[jimstazinsky]

I keep getting the following error when I try to attach a 250 kb zipped up cae:
406 [IOErrorEvent type=”ioError” bubbles=false cancelable=false eventPhase=2 text=”Error #2038”]

I tried multiple browsers (IE, FireFox, and Chrome), and still can't get it to work. I don't know what the problem is, but if someone wants to look at the cae file, I could attach it in a personal email. My address is jimstazinsky@hotmail.com.

Hopefully someone can get large strains (I need to see around 500% eventually) with it and tell me what my mistake was when they get the file.

Thank you, once again, for everyone's help. I truly appreciate your assistance and having the patience to deal with my download issues :(.

[Jorgen]

There was a problem with the upload manager. I switched to a different upload approach and it appears to work now again.
Feel free to give it a try...

-Jorgen

[jimstazinsky]

Thanks Jorgen!

I think the new uploader got the job done. My simple .cae file is attached.

To reiterate my problem, I would like to get strains in the area of 500%. Obviously, my final geometry will be different (I'm sorry, but due to a pending patent and IP I can't disclose it at this time), but I figured if I can't get these types of strains on a simple block I have no hope of my real model working :).

Any ideas/feedback will be welcomed.

[Mr. Inventor]

Hi jimstazinsky,

sorry that I am a little late. I tried something with your Block:

- Added a Reference Point
- Coupling of the RP and the Rubbersurface
- Displacement Boundary Condidition on RP
- C3D8RH

The Rubberblock is 20mm long in the beginning. I get hourglassing after 48mm displacement.

I think the main problem is the pinned support.

I made a plot of the reaction Force and the displacement of the Reference Point. See the images I attached to this post.

[jimstazinsky]

Mr. Invenotr,

Thank you very much for your help. I'm terribly sorry for the extremely late response. This is definitely quite an improvement on what I was able to accomplish (in regard to highest achieved strain) before.

Another approach I tried was using Riks algorithm (instead of static, general step, use static, riks). I was able to achieve incredibly high deformations (see picture of pressurized "hyperelastic pressure vessel" (used purely for demonstration, don't worry, I'm not planning to endanger lives with this :) )).

However, now I have a new problem. I will be applying a load to my part that will put the material well into its hyperelastic region. The load, which is applied by a fluid flow, is removed after a brief period of time (2-4 seconds). If the load is not removed, the material will fail after 6 seconds or so. My questions to forums member are:

1) Is this a problem best solved with standard or explicit?

2) If fluid is creating the load, should I try to incorporate fluid cavity elements or should I simply apply the load (in the form of pressure) that results from the fluid?

3) Amateur question: Using standard or explicit, how can I model the application of the load for a specific time (3-4 seconds in my case)?

Thank you, any help would be appreciated.

[Mr. Inventor]

I would like to see the undeformed state of your demonstration model. :)

1) With "explicit dynamics" contacts and large deformations are a less problem than with Abaqus standard.

However, since explicit simulates stress wave propagation it can't handle incompressibility (poisson ratio 0.5). If you have incompressible material it will assume a poisson ratio of 0.475. Of course you can choose a poisson ratio of 0.49999 but it is not recommend to use a higher ratio than 0.495.

So the question is: Is your material nearly incompressible and is your application mostly under compression load? I would suggest you make both, standard an explicit to be sure.

2) If you know the pressure of your fluid you can use the pressure load directly. But if the pressure is unknown you should think of using fluid cavities. For example you have a water filled bottle an you squeeze it the pressure will rises while the volume remain constant.

3) You can do a multi step analysis. Here you can vary the loads and boundary conditions step by step.

[FEguru]

Regarding your initial model, the reason for the non convergence may be the solver. If you are using the default symmetric solver, try the non-symmetric solver instead. You are applying a pressure load on a face that is changing with deformation, and this causes a non-symmetric stiffness term that gets more severe as the load increases. Another possible cause is the stress singularity at the supported end.

[jimstazinsky]

Mr. Inventor, Jorgen and others,

Thanks again for everyone’s help and I’m really sorry for the incredibly late response (to Mr. Inventor), work has been unusually and unpleasantly more time consuming than the usual.

The attached zipped up .cae file is a model of a thick walled bladder made of a hyperelastic material. What I'm trying to accomplish is to define a fluid cavity with a reference point so that I could prescribe an initial pressure to this cavity (the pressure will be just atmospheric pressure) and then indicate a volumetric flow profile (which is included as the amplitude in the model) into it to see how the bladder responds to fluid being pumped into it. If I properly understood what I read (correct me if I'm wrong), I can't do this using the graphical user interface, so I have to edit keywords. However, I keep getting errors, with the most recent telling me that I'm placing *FLUID EXCHANGE TYPE into the wrong section.

Please help me understand what I'm doing wrong. Am I using the wrong keywords? Typing them in in the wrong places? Is my cavity incorrectly defined (geometry or elements) ? Is there an easier way to model the response of my material to a fluid flow?

Thanks for all the help ahead of time, and I’ll definitely be more on top of checking the forum from now on, sorry.

Best,
J

[Enticer]

Hello All,

I have actually posted this question in another thread but I'm reposting as the subject of discussion is more relevant!

This problem is more similar to the problem mentioned by Mr.Jimstazinksky at the starting point of this discussion.

I am trying to model uniaxial compression of low denisty polyurethane foam in ABAQUS. For doing this, I have carried out a uniaxial compression test of a solid foam block in Instron and with the experimental data, I have found the values of Myu1, alpha1, Myu2 and alpha2 by curve fitting in Matlab. When I tried to incorporate these values into ABAQUS and run a simulation on a same sized foam block, I'm currently facing these issues :

1. The poisson's ratio was assumed to be zero as suggested in the Polymer Foams Handbook by N.J.Mills citing couple of references who have used zero poisson's ratio for curve fitting. I'm able to run the simulation with this case, but the load at 80% of strain in experiments (10N) is achieved at 20% of strain in Simulation.

2. This made me to search for some more references as I speculated poisson's ratio for low density foams might be significant and came across the classic paper of Mr. Roderic Lakes in 1988 Science journal titled "Foam structures with a negative Poisson's ratio". A detailed study from other papers helped me in understanding that the P.R for low density polyurethane foams with density of 24Kg/cu.m varied from -0.28 at 2% compresion to -0.03 at 45% strain. As the density of the foam that I'm trying to model is around the same range, I used these values of -0.28 and -0.03 in the Nu1, Nu2 input parameters of Hyperfoam model in ABAQUS. But still, it's the same result and no improvement is obtained in the curve.

3. Alternatively, I tried using the uniaxial test data directly with the Hyperfoam model in ABAQUS and tried to evaluate the curve fit parameters, but it doesn't allow me to do that with a message indicating that it's possible only for Hyperelastic and viscoelastic models. I then tried using the Hyperelastic material model and tried to fit the curve with Ogden model, but I am obtaining a Negative Shear modulus (Myu1) value when I did so. I believe though it says Ogden fit, it has a different governing equation and wasn't sure about what the parameters D1, D2 signify. The curve fitting tool in ABAQUS unlike Matlab doesn't allow user to customize limits to which the values need to be restricted . But I was able to get some improvisation with the maximum load being achieved at 30% strain in this case.

1. Is there some improvement that I can work in my model to overcome this problem. Can anyone suggest me the correct apporach for modeling a problem like this?

2. Have anyone tried fitting the experimental data with Hyperfoam model in ABAQUS and achieved the material constants? If so, can someone suggest on where I should look on for this?

Thanks very much to whosoever in advance,
Enticer

P.S : I would like to let you know that I currently work with a coarse mesh of around 1000 nodes for saving time

[Jorgen]

It sounds like you are doing things correctly. My first reaction is that you need to experimentally test not only the uniaxial compression response, but also the volumetric compression response. A constant Poisson's ratio is not a good approximation.

I am not sure why ran into problems when trying to calibrate the hyperfoam model. You might be interested that my MCalibration (http://polymerfem.com/content.php?9-MCalibration) software can calibrate the hyperfoam model to an arbitrary set of experimental data. Send me a message if you would like a free trial license to MCalibration.

Thanks,
Jorgen