Learning Forum

[ting teng]

Hi, 

I have a problem in compressing an hyperelastic structure. 

The geometry of a simulation file consists of two components: two rigid plates with a fixed one and a moving one; and one hyperelastic structure between two plates.

As seen in the attached figure, the elastic structure was not able to be compressed after certain displacement of a moving rigid plate.

The error message is as following: "The solver engine was unable to converge on a solution for the nonlinear problem as constrained."

Can anyone resolve this problem?

For instance, I have tried finer mesh for a hyperelastic structure, but same error occurred.

I can share my .wbpz file through google drive, if it is needed.

Thank you for advance.

[Erik Kostson]

Hi

Ansys employees are not allowed to download a file - still we can provide some general advice:

 

Very common issue - lots on the internet about it especially about hyperel. material - so searc there.

Some material which I found could be of help.

 

Overcoming Convergence Difficulties in ANSYS Workbench Mechanical, Part I: Using Newton-Raphson Residual Information
https://www.padtinc.com/2012/10/10/overcoming-convergence-difficulties-in-ansys-workbench-mechanical-part-i-using-newton-raphson-residual-information/

Overcoming Convergence Difficulties in ANSYS Workbench Mechanical, Part II: Quick Usage of Mechanical APDL to Plot Distorted Elements
https://www.padtinc.com/2012/10/18/overcoming-convergence-difficulties-in-ansys-workbench-mechanical-part-ii-quick-usage-of-mechanical-apdl-to-plot-distorted-elements/

Nonlinear Convergence Tips
https://www.ansystips.com/2018/06/non-linear-convergence.html

1. Align nodes between contact and target if possible in the sliding direction (link)
2. Save Newton-Raphson Residuals & Identify Element Violation before analysis starts (link)
3. Use MPC for bonded contacts if needed (link).
4. Set small initial time steps. Here is my default setting for difficult problems:


The first step would thus be 1/100= 0.01s with a minimum time step of 1/1000= 0.001s. Apply this to all "Current Step Number" of interest.

5. Have similar size mesh at contacts. If not, Contact has finer mesh while Target is coarser.
6. Slice and dice geometry such that the volumes adjacent to contacts can be Hexahedron elements. 
         - Starting with pretty mesh by the contacts reduces the distortion during the analysis. 
         - Hexahedron elements are less distorted when capturing curved geometries (e.g. holes). 
7. Drop Contact Normal Stiffness Factor (i.e. FKN) to 0.01. Watch out for excessive penetration.
8. Use Contact Tool to see if any contacts are open. Pinball radius may need tweaking. 
9. Switch model to Displacement driven instead of Force driven for better stability. 
10. Avoid over-constrained model whenever possible (e.g. symmetry and bonded contacts) 
11. Move the body to be just in contact so that it doesn't 'fly' a small distance before touching. 

Also look up hyperelastic and convergence issues on the internet for more advice.

All the best

Erik

[peteroznewman]

Great post Erik!  The link for 3. MPC bonded contact is no longer valid.

[ting teng]

Thank you for kind explanation on solving nonlinear convergence issues.

Based on your advices, I aligned the contact nodes, set small initial time steps, and used MPC for bonded contacts. Also, same mesh sizes were used for all elements.

After many attempts, I obtained the best results, but yet not converged, as shown below:

(Note that I omitted bottom and top plates for convinience.)

and the latest Newton-Raphson Residual Force is as below:

The right image shows magnified view of local maximum probe. It is located at the internal edge of an elastic structure.

For this issue which is not related to the contact between different component, can you give me some clues?

Again, thank you for your kind support. 

[ting teng]

Dear all, 

So far, I used custom material for elasic structure with fitting Mooney-Rivlin 3 parameter model to experimental stress-strain curve.

However, as I changed the material of elastic structure from custome material to structural steel, which is included in basic material library in Ansys, the simulation converged, although there were any changes except material.

Then, can anyone explain about this problem?

Below is the compressed structure with structural steel as a material.

[peteroznewman]

Hyperelastic materials are more difficult to converge because they are either incompressible or nearly so. Tiny differences in nodal displacements cause large changes in the internal forces and pressure in each element causing the N-R Force Residual to bounce around, making it difficult to converge on nodal displacements that create a force equilibrium. A special element formulation has been developed to tackle this issue, called the mixed u-P element forumlation. It add an extra degree of freedom, pressure P that can be tracked to convergence separate from the nodal displacements u. This greatly improves the ability of the solver to find convergence of hyperelastic materials. The mixed u-P element formulation is turned on by inserting Keyopt,matid,6,1 using a Command Object inserted under the solid body in the Geometry branch of the Outline in Mechanical.

[ting teng]

Dear Peter, 

Thank you for your valuable advices.

I made some improvements by adjusting fitting model, but still it did not converge completely. Inserting Keyopt,matid,6,1 using Command object seems to be not effective for this case.

Here are some results, and N-R Force residual. Still max point of N-R force residual was inside the elastic structure.

I used tetragonal mesh, with its contact matched to both plates.

What would be effective for this simulation to converge more?

 

[peteroznewman]

Using smaller elements in the region of high N-R Force Residual is often required in order to achieve convergence.