Hyperelastic material model verification?

aman7aman7 Member Posts: 4

Hello,

I am working to model a material using Mooney-Rivlin (MR) model. I have the experimental data. I used the curve fitting tool in ansys to find the coefficients of MR model. Now I want to verify the model with simulation. I made a cylindrical sample of material and I have given it the displacement equivalent to strain in material during experiment so that it gets loaded under same strain rate. Now the Von-Mises stresses I am getting from the simulation are not matching the experimental values as I have used the same experimental data to drive its model. I think conversely it should give similar stress under similar loading. Can anybody help me in this regarding?

Answers

  • peteroznewmanpeteroznewman Posts: 11,404Member
    edited March 14

    @aman7

    Watch the ANSYS Course video on Hyperelastic curve fitting.

    It describes how to validate the material model results against the experimental data.

    The example uses a unit cube with edge length of 1 m. The model outputs the reaction force for an applied displacement on one face. Since the force acts on a face that has an area of 1 sq. m the force has the same units as Engineering Stress in Pa. Similarly, since the length of the cube is 1 m, the applied displacement is equivalent to Engineering Strain.

  • aman7aman7 Posts: 9Member

    @peteroznewman

    Thank you for your reply. The video is informative. But in mean time I get to know that hyperelastic material FEM face problems of shear and volumetric locking. I have seen some videos that suggest using reduced integration.

    I don't know how to use reduced integration?

  • peteroznewmanpeteroznewman Posts: 11,404Member

    @aman7

    Reduced Integration may be automatically selected by the solver. Read the Solution Output and look for Keyops.

    Reduced Integration is set by Keyops, often Keyop,2,1. Look in Ansys Help in the Element Library for the element used in your model.

  • aman7aman7 Posts: 9Member

    @peteroznewman

    the values of KEYOPTs is as:

    KEYOPT(2) = 0 for SOLID186 means Uniform reduced integration. How can i use other methods like selective reduced integration?

  • peteroznewmanpeteroznewman Posts: 11,404Member

    @aman7

    SOLID186 is a Quadratic element and has only two choices: Full Integration and Uniform Reduced Integration.

    Under Mesh, set the Element Order to Linear. SOLID185 has four choices for Element Technology.

    KEYOPT(2)

    Element technology:

    0 -- 

    Full integration with 

     method (default)

    1 -- 

    Uniform reduced integration with hourglass control

    2 -- 

    Enhanced strain formulation

    3 -- 

    Simplified enhanced strain formulation

Sign In or Register to comment.