Soil Structure Interface Modeling

[BuuNguyen]

4) Can you please provide any recommendations about Kn, Kt, and mu coefficients?
Kn and Kt are penalty coefficients, so there is the typical rule:
It should be a number large enough to enforce the constraint (Kn for non-penetration, Kt for stick condition), but not too large to avoid numerical problems.
As usual, estimate the typical stiffness (Ktyp) of your problem (E*L for solid elements, EA/L for trusses, and so on...).
Then evaluate the order or magnitude: OOM = round(log10(Ktyp))
Now the penalty coefficient should be P = 10^X
where is X > OOM.
2 or 3 orders of magnitude is enough (so X = OOM + 2). At most use X = OOM+8. Why 8? because double-floating-points numbers have 16 significant digits, so OOM+8 means something in between accuracy of the constraint and numerical stability
Regarding mu, it is the friction coefficient (i.e. the tangent of the friction angle). You can find online typical friction coefficients based on the two materials in contact.

The suggestion to define Kn and Kt is similar to K (penalty constraint)?
I remember I have read a post in the forum which said that Kn=(10~100)E_min, Kt=(10~100)G_min.
Which one should be more accurate?
Thank you
Buu

[STKO Team]

After I exploded the model and merged it back so I have two geometries (superstructure with foundation block and surrounding soil domain), it seems that all solid elements in the soil domain turned into a number of faces (not solids anymore). Also, all assignments to solid elements of the soil domain got unassigned. Please see the screenshot below.

How do I fix this? Do I need to somehow manually create solid elements or is there any other more efficient way? Do I just add faces on the solid elements (red shading in the screenshot) where the interaction with the foundation block should occur and merge? Does a collection of faces automatically becomes a solid?

It should not happen.

If you have a comp-solid (a geometry made of multiple solids) and you explode it, it will become a list of simple solids.
If you explode a solid, it will become a shell (i.e. the set of faces that are boundaries of the solid).

Probably you exploded it twice...
Anyway, if you send me your model I will have a look

[kolozvari]

Thank you for your help. You were right, I must have exploded the model twice. I re-did it and it seems to be fine now in terms of geometries. However, when I try to run the model, the analysis fails even for gravity. I would really appreciate if you could take a look at the model and let me know why do you think this is happening (see attached model).

Few notes about the model:
1) Selection set "Soil only" includes soil elements and absorbing boundary elements. These are all merged as one geometry per previous discussion.
2) Selection set "Structure only" includes all elements of the superstructure, all merged as two geometries with beam-to-solid interaction.
3) Contact interactions and elements are assigned at the interface of the two geometries mentioned above. I created separate interaction/elements for each face of the interaction surface and they are labeled by the orientation of the unit normal (x+, x-, etc.).
4) The model runs perfectly fine before implementing interactions.

Can you please take a look at/clarify the following:
1) Are the contact interactions assigned correctly? I had a lot of issues actually performing this task and I am not sure if the interaction is actually assigned to both faces of the contact surfaces. When I show only the "Structure only" selection set, I cannot see the dots that represent contact interaction, but when I show "Soil only " selection set, I can see it. Maybe this is just a visualization issue, and it would be great if you can confirm if this is done correctly.
2) Can you please take a look at properties of the implex elements (they should all have the same parameters)? In particular, am I using the correct orientation type given the 5 faces of the contact interaction? Please advise.
3) Can you please check the analysis settings for gravity and time history? Maybe the analysis is crashing because implex is working only with a particular analysis settings.

Looking forward to hearing from you.

Thank you very much!

[STKO Team]

1) Are the contact interactions assigned correctly? I had a lot of issues actually performing this task and I am not sure if the interaction is actually assigned to both faces of the contact surfaces. When I show only the "Structure only" selection set, I cannot see the dots that represent contact interaction, but when I show "Soil only " selection set, I can see it. Maybe this is just a visualization issue, and it would be great if you can confirm if this is done correctly.

The visualization of the dots of the interaction has nothing to do with the selections sets. The fact that you see them in only one selection set is because you added it to that selection set...
Anyway, your interactions are fine, but you need to follow some rules:

• You have chosen Node-to-Node interaction. This is fine if the meshes at the two sides of the contact are compatible so that each node of the slave face has a node of the master face at the same location. This is the case in your model. OK
• You have chosen (in zeroLengthContactASDimplex) OrientationType = FromLocalAxes. But you did not assign any local axes to the interactions. The default local axes for the interaction correspond to the global axes. This is fine only if the contact normal (Master -> Slave) points to the global Z direction. In your case instead you have to define a local axes for each one of your interactions. WRONG

In the modified file I created the necessary local axes for your interactions, following the contact normals, because in your case, you used the faces of the foundation as master, and the faces of the soil as slave.
Note that you can create the local axes manually from STKO. But for simplicity I created a small python script to generate them automatically from a user input (a list of contact normal vectors and a list of names for each local axis). It can be useful for you in new models.

contact normals.png (280.91 KiB) Viewed 5158 times

2) Can you please take a look at properties of the implex elements (they should all have the same parameters)? In particular, am I using the correct orientation type given the 5 faces of the contact interaction? Please advise.

The parameters seem fine. Since they are all the same, you can use just 1 element property for all your contact interactions. This is what I did in the modified file.

3) Can you please check the analysis settings for gravity and time history? Maybe the analysis is crashing because implex is working only with a particular analysis settings.

Your model was singular for the wrong definition of the contact normals, but above all, because your foundation solid has a node in the middle of the top face (probably a result of a wrong boolean operation).
This extra node makes the solid invalid. This node will not belong to any element, thus the singularity.
I recreated the soil correctly.

INVALID_COMP-SOLID.png (71.51 KiB) Viewed 5158 times

[kolozvari]

Thank you very much! I really appreciate it. I am still learning to model different features in STKO and this is super useful. Thanks again.

Regards,

[kolozvari]

Can you please remove the two file you uploaded? I would like to keep the files confidential and not available to the public. Thank you.

[STKO Team]

Can you please remove the two file you uploaded? I would like to keep the files confidential and not available to the public. Thank you.

Done

Thank you very much! I really appreciate it. I am still learning to model different features in STKO and this is super useful. Thanks again.

You're welcome

[kolozvari]

Hello again. I have ran the model and I have a question about the results. Screenshot below shows the acceleration at the top of the foundation for the case when foundation and soil are fully connected (left) and when interaction with between the foundation and soil is modeled with implex contact element (right). As you can see, there is some very high-frequency response of the foundation when using implex. What do you think where is this coming from? Is it related to very high values of penalty coefficients?

I would appreciate if you can provide your opinion. Thank you.

[STKO Team]

It can be due to some of these things:

1. The IMPL-EX method requires small time steps due to the Explicit part of the integration (In the next OpenSees and STKO releases we will have an automatic check of the time step for this). To make sure this is not the source of the issue, either try to use the Implicit integration, or reduce the time step
2. The penalty values can create problems if they are too high. Start by estimating the stiffness of the soil mesh using K=E*H, where H is the mesh size. Take the Order of magnitude oom = round(log10(K)). Now do some sensistivity check. Run analyses using penalty = 10^(oom + X), where X ranges from at least 1, to at most 8.
3. If none of the above is the source of the issue, then probably it is not an issue at all. It might be intrinsic to the pounding of the contact surfaces...
4. If they are very high frequency noise, try using another integration scheme with numerical damping, such as HHT with alpha >= 0.67 (max numerical damping) and alpha <= 1.0 (no numerical damping as in newmark)

[kolozvari]

Thank you very much for your replies. I have a few follow up questions:

1. The IMPL-EX method requires small time steps due to the Explicit part of the integration (In the next OpenSees and STKO releases we will have an automatic check of the time step for this). To make sure this is not the source of the issue, either try to use the Implicit integration, or reduce the time step

Can you explain how to do this? Is this just unchecking the Implex box in the zerolengthcontactASDImplex settings or are you referring to global analysis settings? Regarding time step, I cannot see that I specified the time step anywhere. Should I just increase the numInr in analysis settings?

Thank you