Mooney Rivlin hyperelastic material failure

[blckwtr]

Hi, all. I have defined a mooney rivlin material in abaqus, with a predefined set of points to elongation at break. However, I experience the material to take up more stress than what the material is capable of, based on a uniaxial stress strain curve. The stress state is triaxial, although the analysis is 2d axixymmetric. How can this be, and what is the failure mode?

 

[Dave442]

by how much do the values differ?

are you plotting integration point results or nodal results? nodal results are extrapolated from the integration points to the nodes and then averaged. is it possible your issue is caused by extrapolation error?

also, in a nonlinear analysis abaqus outputs cauchy (true stress) whereas i think hyperelastic materials are defined using nominal/engineering stress/strain. is it possible this explains your issue?

you could run a single element uniaxial tension analysis and verify tbat you get the correct output.

im not sure what you mean by "what is the failure mode"

 

[blckwtr]

How do you set the nodal or integration point as the value of interest? Anyway, I would assume that the integration points would be close to the nodal results, I don't think the gradient is extreme in my case. When it comes to hyperelastic material definition, it is true that it is defined by using nominal stress, so the stress strain values are implemented directly, contra a metal, where this must be converted. I will try to "benchmark" as you say with a known specimen, and see what I get out of it.

What I mean with failure mode. What causes the material to fail (crack)? Since I am pressing rubber together in an enclosed cavity, I can in theory compress this to infinity?! I suppose not, but how would this material fail then? By extruding through openings in this cavity, or does it disintegrate long before that... If, just to pick a random number, the element is capable of 10 MPa uniaxial stress. when performing an analysis, whether it is 2D or 3D, the uniaxial stress strain curve is used, but the elements are distorted in 3 dimensions, hence they experience a triaxial stress state. The one direction in which I compress the element would increase in compression, but the other two direction would increase in tension. Would it then fail when reaching this 10 MPa when converting it from triaxial stress state to uniaxial and acheive 10 MPa? And how would it fail, since it is enclosed in a chamber?

If i use octahedral stress equivalent, I find it to coincide with theoretical calculations...

 

[Dave442]

to see integration point results in Viewer select:
Options -> Contour and then select "Quilt" in the basic tab.

you can convert your nominal stress-strain curve to true stress-strain very quickly and compare with your abaqus output. I would also run a single element analysis to verify the hyperelastic material model is accurate under uniaxial loading before worrying about results in multi-axial loading. Abaqus can run the verification for you:

Abaqus/CAE Users Guide 12.4.7 Evaluating hyperelastic and viscoelastic material behavior.

im struggling to follow the rest of your post. Rubbers are typically incompressible, you cant compress them to infinity. If you're modelling rubber parts that see a lot of compression you should have compression test data to calibrate the material model. From that testing you should have determined how your parts fail in compression. You should also use the hybrid elements that were developed for modelling incompressible behavior.

equivalent stress/strain measures are typically used to compare the stress state in elements subjected to multi-axial loading back to a uniaxial stress-strain curve.