asdeasoft.net

Dear STKO,

I am trying to run a static SSI analysis(currently linear elastic) but only works with the linear solver algorithm.
I believe the issue is related to the interaction definition between structure and soil, or the soil transition.
I tried Newton, Newton w/ line search, and Krylov-Newton (all with adaptive time step).
I wanted to ask for your insight and recommendations to run the analysis.

Here is some context of the model.

1. The model is an embedded concrete mass where the applied loads come from machinery.
2. Soil domain is composed of 2 geometries with a transition.
3. Absorbing Boundaries are not used yet since I am trying to run a static analysis first.
4. At the moment all elements are SSP Bricks, linear elastic since I am checking the solver.


I used the 'sfsi.scd' presented in webinar #25 from Nov 4 2021 (New Element Presentation - ASDAbsorbingBoundary) as a guide for my model

Thank you very much for your help and your time. I attached the model for your reference.

It runs on my side, but it struggles to converge.

Can you try these test settings?
Lowering the Relative Error to 1.0e-5 (relative to the initial error) can be hard to achieve

Another question:
Why are you using the reset command?
It resets everything to the initial condition as if the previous analysis was never performed. Are you sure this is what you want?

Dear STKO thank you for the prompt reply.
I adjusted the tolerance for convergence. I was able to run the gravity analysis with no issues but the lateral load analysis did not go past 50%

As a follow-up:
I also noticed that when defining the 'zeroLengthContactASDimplex' my model used the Orientation 'from local axes'.
I changed it to 'From Element' as it is recommended for node-to-element links. With this change the I was able to reach 65% of the lateral load analysis.

Based on this change and the deformed shape it seems that this issue could be related to the Soil-to-block interaction.
For reference I attached a figure showing the deformed shape obtained at the last converged step using the Linear and the Krylov-Newton solver

Note: I am aware I am resetting the model after each analysis. At the moment I am trying to run each case independently but this will be corrected later on - thank you for bringing this up.

Thank you for your time. The assistance is very much appreciated.
Kind regards,
Andres R.

I changed it to 'From Element' as it is recommended for node-to-element links. With this change the I was able to reach 65% of the lateral load analysis.

This is true. When the interaction is node-to-element (for incompatible meshes) you SHOULD use "FromElement". "From Local Axes" requires the user to provide a valid Normal vector for contact. The "From Element" option is easier: STKO automatically computes the contact vector from the master element surface.
Instead, when the mesh is compatible between master and slave, and you have a node-node interaction, you can use "From Local Axes"

For reference I attached a figure showing the deformed shape obtained at the last converged step using the Linear and the Krylov-Newton solver

The Linear solver cannot be used with non-linear components (materials or contact)


Tip:
With contact problems, when you don't have a compatible mesh (as in your case), the SLAVE mesh should be finer than the MASTER mesh.
For this, I gave a fiber mesh to the BLOCK geometry and an even finer mesh to the ShearKeys. Now it runs smoothly:

Thank you very much for the feedback, the model is running now.

Regards,
Andres R

You're welcome