asdeasoft.net

Dear STKO team,

I hope you’re doing well.

Could you please tell me how to model a contact surface for rocking? I’m modeling a three-dimensional rigid body with a pure rocking response under earthquakes.

When I perform the analysis using a node-to-node link, there is no issue. However, since I do want to include “more than one point of rocking,” I want to model a surface. I checked your past webinars, and if I understand well, I can use a node-to-element link (please check the SS01.png attached).

In addition, I have used contactASDimplex where the orientation type “from element” is selected (please see the ss SS02.png attached). Despite those steps, the analysis is not converging (see the SS03.png attached).

Could you please help me to create the surface and corresponding link to the solid correctly? Please, find attached the modell that I'm using.

All the best,
Salvador

Hi Stko Team,

Could you please help me with this?

All the best,
Salvador

I need some more info.
From the image I see 4 points fixed to the ground, but you said you want to make the whole bottom surface of the solid to be in contact... but with what? with the ground? or only with those 4 points?

Hi STKO team,

Thank you so much for your quick reply! Yes, I do want to modell that the bottom surface of the solid to be in contact with the ground!

All the best,
Salvador

So you need to:

1. Create a surface which is exactly equal to the bottom of the solid (you can use the Extract command)
2. Make sure this new surface has the same mesh of the bottom of the solid
3. This new surface does not need any ElementProperty: it will generate only nodes, not elements
4. Fix this new surface in all translational DOFs
5. Make a node-node interaction between this new surface (master) and the bottom of the solid (slave) (normal vector = +Z)
6. Add a contact to it

Hi STKO team,

Thank you so much. I have followed the procedure and it seems fine. However, since I'm trying to increase the meshing, the computing time increases a lot. So, I would like to divide the analysisis into different partitions.

Could you please check my file and tell me the correct configuration to run my model in different partitions?

All the best,
Salvador

Try this: Changes:

• Partitioned your model in the mesh tab
• Parallel Numberer + Mumps in all analyses
• Removed eigen: it doesn't work in partitioned analyses
• Used Transformation constraint handler: you don't have overlapping MP constraints so you don't really need Penalty
• Removed the "-distirbuted" flag in the contact. The stiffness you gave is already a penalty value compared to the typical stiffness of your model (1.0e6). Distirbuted makes sense if you are modeling a soft cohesive zone with real elastic moduli.
• I used IMPLEX in the contact as after the first rotation in your dynamic analysis, your model starts to jump and it makes it hard for the implicit algo to converge

Hi!!!

Thank you so much for this. I have been trying but it keeps the error. Could you please guide me?

Best,
Sal

It's because I made it partitioned for parallel computing. Use OpenSeesMP

Hi!

thank you so much! I see that everything works perfect now!

All the best,
Salva