Learning Forum

[zjuv9021]

Hi all,

A few things:

It appears with this problem that as I decrease the size of the elements, the more issues it has with "element turning inside out", so generally speaking, I've had more success with larger sized elements. Are there any thoughts as to why that may be the case?

Also: My convergence charts are a little perplexing.... It appears that I am below the criteria, but it is not successfully converging a substep for quite some time. Is there something that I'm not understanding here or some code I can enter to force this to converge if it's smaller than the criterion?

Regards,

Zach

[Sandeep Medikonda]

Zach,

 

The reason why it might show more iterations is that even though the force has convergence, the displacement or moment might not have.

Regards,
Sandeep

[peteroznewman]

To add to Sandeep's comment, you can plot the convergence for displacement instead of force and get a different plot.

[zjuv9021]

I am still quite confused, as both the displacement convergence shows similar characteristics as the force (well below the criterion), and there is NO moment convergence...

Any thoughts as to why my run may be experiencing this issue?

Regards,

Zach

[Bhargava Sista]

Zach,

For incompressible hyperelastic materials, u-P formulation is used which introduces an additional convergence criterion on volumetric compatibility, chances are that this criterion is not met (it's not plotted, you'll need to check this in the solve.out file). Usually, when an incompressible material is pushed to large deformation, the elements tend to turn inside out in the process of satisfying the volumetric compatibility.

To achieve convergence for such cases

• introduce some amount of artificial compressibility in the material property.


• loosen the convergence tolerance on volumetric compatibility. I think that the default value is 1e-5, so increase it to 1e-4 and see if that helps.


• also, check the physics of the problem. For instance, if you're modeling a foma material as incompressible material, you'll run into these issues because foams are hyperelastic but are compressible. So, modeling them as incompressible will put the material under tremendous stress and would cause issues with convergence.

[zjuv9021]

Thank you for this.
Could you please assist in what the command in ansys is to loosen the convergence tolerance?

Is it: SOLCONTROL, , , , 1E-4

[Bhargava Sista]

It's CNVTOL,COMP,,5e-3 to increase it to 5e-3 (default is 1e-3). 

[zjuv9021]

In similar fashion, if I wanted to increase the tolerance for force convergence, it would be CNVTOL,F,,8e-3 (default is 5e-3)?