hyperelastic material data in abaqus

[karabiber]

Hello there,
Currently I am trying to simulate a hyperelastic material. I have uniaxial test data from experiment. When I implement this data to Abaqus/CAE 6.7-1, and run the simulation, I have a problem since the stress and strain do not increase continously. Simulation is aborted. Could you please help me to solve this problem? Is there any way to solve this problem?
Regards,
Berkan

 

[rstupplebeen]

More information is really needed. Could you post your analysis? Do you have Nlgeom on? I hope this helps.

Rob Stupplebeen

 

[karabiber]

Hi,
Thank you very much for your reply.
Nonlinear Geometry is: On
The problem is with the uniaxial test data.
Please find the attached file.

 

[williwang]

Did you smooth the data?

Forever Young.....

 

[rstupplebeen]

At the end of this message are the error messages that you file creates. Basically the Marlow model that you are using does not like that your test data does an "S". Do you possibly have the axies switched? If not the Marlow model is not appropriate.

I suggest using Materials-Evaluate in the property manager to select an appropriate material model.

Why have you set the step time to 1000 from 1? This is an arbitrary number and everyone else that I have worked with just reduces the step size if convergence is slow.

I hope this helps.

ERRORS:
The nominal strains under the *uniaxial test data option must be arranged in ascending order

1 elements have been defined with zero hour glass stiffness. You may use *hourglass stiffness or change the element type. The elements have been identified in element set ErrElemZeroHourGlassStiffness.

Analysis Input File Processor exited with an error.

Rob Stupplebeen

 

[karabiber]

williwang: I did not smooth the data. Do you mean changing the curve data since at one point stress starts to decrease while strain is still increasing so it does not work?

Stupplebeen: Yes, that is the problem. Data is not appropriate since it has a decrease in stress. It is not increasing continously and I do not want to change the data. Is there a way to run this simulation?
about time step: after analysis, I would like to have stress-strain data. thats why I had this.

 

[rstupplebeen]

Try a different material model. I randomly tried a different one and it was solving. I killed it because your analysis required at least 1000 steps. Use the Materials-Evaluate to select an appropriate model and you should be good to go. I hope this helps.

Rob Stupplebeen

 

[karabiber]

I checked materials parameters and stability limit information. I can not choose a different material model since it is hyperelastic material.
Regarding the strain energy potentials, I can only choose Marlow since I have only one test data. Abaqus documentation does not suggest to use other potentials if I do not have different test data(like biaxial, uniaxial, volumetric etc.)

I have changed the data a little bit, arranged the strains and stresses in an ascending order (without changing the general behavior of the curve). It does not run now. Obviously, there is no problem with nominal strains right now but it does not tell what the problem is

 

[karabiber]

Ok, I think I solved the problem. When I use Marlow Strain Energy Potential, I should put two zeros at the beginning of nominal strain-stress data. Now it looks fine.
Also I changed the time step, made it only 1 seconds, and every 0.05 seconds I receive data.

Thank you very much.