Sean Harvey
Ansys Employee

Hello Sarvesh,

Let me clarify.

I modeled your material using those constants on a simple cube.

I push into the cube, so what should we see in the simulation?  You expect it would squish down right?  But look what it does.  The cube stretched.  This is non-physical for the silicone material.

Look at the paper you provided and we see the stress - stretch behavior.

But look at the curves in the engineering data.  They show a negative relationship between stress and strain.

This is where your problem lies.  You have the incorrect material response.

Now you may ask why?  Is it the units or typo?  While that is a common error, it is related to the slide below.

The Ogden model in Ansys has a slightly different construct using the variable. That paper has the constants for Abaqus.  The equations are identical, only that what is that mu is different.  To compute mu in Ansys, set the first term ui/ai = 2ui'/ai   Let ui' be the value from Abaqus, now you solve for ui (which is mu for Ansys) and you will get ui = 2ui'/ai.

I have done this and this is the modified material data

Notice with positive stress we have positive stretch (strain).  This is physical behavior for the silicone material.

Alternatively, you can input the material data provided from the charts, being very careful to convert to engineering stress and strain, not true stress and stretch. Then you would curve fit using the curve fit tools in engineering data. My colleague already provided lessons on how to do that.

I suggest you try the values I have provided to see if you start to get physical behavior.  I leave it to you to double-check my inputs.

I also suggest you take the hyperelastic free course which would have helped you identify that you have a non-physical stress-strain response.  But the mistake you have here is an easy one to make. It can be easily assumed that if Ansys and Abaqus have Ogden, then the mu and alpha are the same.  Unfortunately, the forms are slightly different.  Now you know :)

Please circle back and let me know if you start to get the actuator to deform more as expected.

Regards,

Sean