Stress exceeds yield strength of perfectly plastic material in OptiStruct Explicit Simulation

Hello,

I did a dynamic explicit simulation in OptiStruct. I set up a perfectly plastic material using MAT1/MATS1 with H = 0 to represent perfectly plastic material.

The simulation is smooth without any error but I find out the von Mises stress of the shell elements exceeds the yield strength of the material. The yield strength I set up is 250MPa but the stress from simulation exceeds 250MPa and seems 322MPa is the yield strength..

I tried the nonlinear static analysis and the stress is limited to 250MPa. The problem only happens when dynamic explicit simulation is adopted.

Any clue or any suggestions to solve this problem? I attached the FEM file for your reference.

Thank you.

OptiStruct_Crash_Test.fem

Find more posts tagged with

English

OptiStruct

v2021.2

Accepted answers

All comments

PaulAltair

If you look at 'mid' layer stress (rather than 'max') then it is 250, I guess this is where the calculation is done for yield. Not sure if that is expected or not, but seems to be the explanation.

I will look into it further next week

Shengjia Wu

Hi Paul,

Thanks for this interesting finding. I also did the corresponding Abaqus explicit simulation. The von Mises stress is output at the top layer in Abaqus and the value is limited to 250.

Based on my study in FEM, the formulation of shell element is at the midplane but after solving the displacement field and get the strain (membrane and bending strain), the stress at mid, bottom and top can be calculated and the stress should follow the given stress-strain curve?

I am not sure how OptiStruct does the above calculation. But thank you very much for your reply and it seems a good clue to dig more..

I also attached the corresponding Abaqus .inp file if you have a chance to run it for comparison.

Abaqus_Crash_Test_Modified.inp

PaulAltair

Hi Paul,

Thanks for this interesting finding. I also did the corresponding Abaqus explicit simulation. The von Mises stress is output at the top layer in Abaqus and the value is limited to 250.

Based on my study in FEM, the formulation of shell element is at the midplane but after solving the displacement field and get the strain (membrane and bending strain), the stress at mid, bottom and top can be calculated and the stress should follow the given stress-strain curve?

I am not sure how OptiStruct does the above calculation. But thank you very much for your reply and it seems a good clue to dig more..

I also attached the corresponding Abaqus .inp file if you have a chance to run it for comparison.

This does seem to be a bug, thanks for reporting, the OS explicit solution sequence is still in beta development and this issue will be fixed in a future release.

Shengjia Wu

I conducted the same analysis in Radioss (using OptiStruct environment but use Radioss integration).

The result is almost the same as Abaqus.

So I guess OptiStruct currently has a bug to output stress in its explicit dynamic step.

The attached is the input file for Radioss using OptiStruct environment for everyone as a reference.

OptiStruct_Crash_Test_Using_EXPDYN.fem

PaulAltair

Yes, indeed, it is a confirmed bug with perfectly plastic material (output for stress only) and is fixed in development, it will be corrected in the next public release 2022.2