INCOmpressible Element formulation leading to unexpected results

[kiakarim]

Dear all,

recently we created an input file containing a simple shear experiment. We would like the material to behave incompressible and would therefore expect a homogeneous stress distribution throughout our domain. However, whilst using the inco element option very weird results are obtained. The input file as well as an image describing the weird result can be found in the attachments.

Best regards,
Kian Karimian

[Prof. S. Govindjee]

(1) For your boundary conditions, you will not get a homogeneous stress distribution.  To get that you will need additional boundary conditions.

That said,

(2) There is however an error in ver86.  I tried your problem in ver85 and it worked fine but with ver86 the results are clearly incorrect.

We will have a look and get back to you.

[Edit: ver85 does not have this element.  the error is in opti as noted below.]

[Prof. R.L. Taylor]

The error appears to be in the profile optimization.  The Lagrange variables are not treated.  The bug will be addressed later -- can you try the solution without profile optimization. 

[kiakarim]

Thank you Prof. Taylor and Prof. Govindjee!
Out of pure interest: What would be the adequate choice of boundary conditions for simple shear?

[Prof. S. Govindjee]

The proper boundary conditions need to match the displacement or traction at every (boundary) dof, so it depends on your model.  In particular, you left the vertical sides free and that is in general incorrect.  One option is to use horizontal rollers with imposed horizontal motion.  The front and back faces, usually, can be left free, but that choice is model dependent.

Put another way, take your desired displacement field, stick it into the governing equations, and then compute possible boundary conditions (displacement or traction), also check that body forces are not needed.

[Prof. R.L. Taylor]

With enough constraints to prevent rigid body motion

[Prof. S. Govindjee]

Here is an interim working option to use the incompressible element with optimization of the profile of the equations.

1. Create your input file with the OPTI command followed by the OUTMesh command.  This will produce an input file Inco.opt.
2. You can now use the input file Inco.opt (without any added OPTI commands) and it will use an optimized profile.

I tested this workflow with version 8.6 and it seems to produce the correct results.