Learning Forum

[Ines_]

Hi everyone,

I am performing an Static Analysis that consists on putting a pressure of 10 Pa on a model with hyperelastic materials and contact.

After strugging with convergence problems, I found out that there is an unstable position in my simulation because each time I run it crashes at the same point (5Pa). To give you an idea, the model of my simulation goes from one stable position to another stable position.

I took control of contact (pinball, formulation) and set Unsymmetric Newton-Raphson method and it was better but I still had convergence problems.

Then, I tried decreasing time step... and it didn't help. However, what worked was putting 5Pa on a Load Step and 5Pa more in the next Load Step. And I don't understand why.

I took care of having equivalent Time Stepping for both analysis. For example, in the 10Pa per LoadStep case I set initial step number to 10 and in the 5Pa+5Pa case I set initial step number to 5 in each Load Step: in both analysis the initial preassure was 1Pa. I did the same with the max and the min step number.

This makes me think that is not the same applying a pressure in one Load Step than applying half and half in two Load Steps in an Static Analysis and I don't understand why. Is there any logical reason for this behaviour? Does Ansys do sth different when going from one Load Step to another that doesn't do when passing from one substep from another?

Thank you very much,

Inés

[peteroznewman]

Dear In├®s You can try Transient Structural and let dynamics help your structure go through the unstable state.
Regards Peter

[Ines_]

Dear Peter,
thank you for your advice!
But I am still curious about why applying the same load in one or two Load Steps in an Static Structural Analysis is not the same.
Regards,
In├®s

[Rameez_ul_Haq]

,in order to understand that, please go through the playlist provided by ANSYS on ANSYS Learning YouTube channel, which goes as:
'Computational Resources Considerations - Ansys Innovation Course'
'Large Deformation - Ansys Innovation Course'
'Structural Nonlinearity - Ansys Innovation Course'

[peteroznewman]

Dear In├®s In a nonlinear solution involving hyperelastic materials, the best strategy is to force the solver to take many small steps. This is accomplished by setting the Minimum Substeps to a high number.
In Static Structural, under Analysis Settings, turn on Stabilization which can help structures get past an unstable deformation.

[Ines_]

Thanks for the advice!
Increasing min substeps is the strategy I followed but, is it possible that some problems don't converge even with a great number of substeps? Because that was the feeling I had in my simulation.
Bests,
In├®s

[peteroznewman]

Dear In├®s There are many reasons why a solution will fail to reach the end time. Sometimes an error occurs, such as the "highly distorted element" error. This is resolved with better element shapes. Let's exclude that from the question you ask.
There are Static Structural models where the solver fails to find equilibrium when increasing the load by a small increment. A common scenario is in structures that have a snap-through behavior. The normal load incrementing method fails, which is what you were experiencing. If the load could get past the instability, there is a statically stable configuration on the other side of the instability, but the normal algorithm can't get there. That is what turning on stabilization does, it introduces artificial forces to stabilize the structure to get it past the instability to get to the other side.
There are other technologies that can be helpful with hyperelastic materials that reduce the difficulty the solver has in finding equilibrium. One of those is called the mixed u-P element formulation. Without that, the deformation of the nodes determines the pressure in the element. That is normally fine because the material is compressible and small changes in nodal deformation creates small changes in element pressure. But hyperelastic material can be incompressible or nearly so with Poisson's ratios of 0.49 or higher. Now small changes in nodal deformation creates huge changes in element pressure, which makes find equilibrium very difficult. The mixed u-P element formulation adds a pressure degree of freedom to the element making it much easier to find a set of nodal deformations that have equilibrium. You should definitely be using this in your model.
Best regards Peter

[Ines_]

Thanks for such an amazing answer!! I wasn't aware of this tips. Thank you for the detailed explanation!