Soil Structure Interface Modeling

[kolozvari]

Hello, can you please point me to some material regarding Soil-Structure Interface Modeling? I would like to model SSI in such a way to allow the soil and structure elements to move independently.

Thank you!

[STKO Team]

By "to allow the soil and structure elements to move independently" do you mean that you don't want the structure to be "tied" to the soil (EqualDOF style), but rather use some sort of interaction as a contact?

[Lucy2012]

You can use the implex contact we implemented in OpenSees and define the friction. It is the perfect way if you want to model rocking or a general contact.
Regards

[kolozvari]

Yes that os what I meant. Is there any examples or YouTube videos on how to use the implex contact?

Thank you

[STKO Team]

Yes, our webinar #24:

Implicit-Explicit Contact Element Applied Examples: soil-foundation interaction and RC structures

This is the YT video:
https://www.youtube.com/watch?v=tXA5guozrFU

[kolozvari]

Thank you for this resource. A few quick questions.

1) is there any reference for the implex element? If yes, please provide it to me. If not, can you please give me a couple of sentence description so I can better understand how it works. What does "implicit-explicit" referring to?
2) when creating an interaction between two solid elements (I am using brick elements), do I select elements to be master and slave? They have a common surface, so I guess that would be the only options. Please clarify.
3) if I have a foundation and a soil, which one will be master and which one slave? I am guessing foundation is a master element and soil is slave, but it would be great if you can confirm.
4) Can you please provide any recommendations about Kn, Kt, and mu coefficients?

Looking forward to hearing from you. Thank you!

[STKO Team]

1) is there any reference for the implex element? If yes, please provide it to me. If not, can you please give me a couple of sentence description so I can better understand how it works. What does "implicit-explicit" referring to?

This is the OpenSees (short) documentation
https://opensees.github.io/OpenSeesDocu ... mplex.html
In that documentation there is a link to a wrong reference paper (we have to fix it).
This is the reference paper you can use to better understand what IMPL-EX means. Other than this, it is a simple penalty-based coulomb-frictional-contact
https://www.researchgate.net/profile/Al ... oblems.pdf

2) when creating an interaction between two solid elements (I am using brick elements), do I select elements to be master and slave? They have a common surface, so I guess that would be the only options. Please clarify.

In contact problems there is always the issue of what is slave and what is master. The rule is: The coarser mesh is the master.
In the webinar I also explain what interaction type (node-to-node or node-to-element) you have to use based on different scenarios.

3) if I have a foundation and a soil, which one will be master and which one slave? I am guessing foundation is a master element and soil is slave, but it would be great if you can confirm.

Same as above, the coarser mesh is the master

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.

[kolozvari]

Thank you very much for a quick response.

My only issue now is how to actually physically do this in STKO. Here are few more follow up questions.

1. Regarding master/slave geometries, both mesh for the foundation and the soil are of the same size, so I am still not sure which one should be master or slave. I guess it doesn't really matter at this time. Since my structure is a simple MDOF stick model and I using the structure to be the master geometry when creating node-to-solid links to connect the stick to the foundation block. Following the same analogy, I would probably start with treating foundation block to be master geometry when creating interface with the soil. Please provide some thoughts.

2. In my case both foundation block and surrounding soil are modeled with brick elements (everything has rectangular geometry - no funny angles). In my understanding, this contact is between two surfaces. Therefore, I would need to create interaction between the two "touching" faces of the foundation and soil brick elements. However, since I created the entire model using "sweep" command, it appears that there is only one face that is shared between the foundation and soil elements. So, when I want to create an interaction, I cannot select two faces (one master for foundation and the other slave for the soil) since there is only one common face for the two elements. This is where I am stuck right now. Please let me know how can I overcome this issue.

3. In your videos, you are showing interactions together with the mesh. I am not sure how to do this. When I work with my model, everything is just in the "geometry" view and I don't see the mesh. Please let me know.

Thank you very much!

[STKO Team]

1. Regarding master/slave geometries, both mesh for the foundation and the soil are of the same size, so I am still not sure which one should be master or slave. I guess it doesn't really matter at this time. Since my structure is a simple MDOF stick model and I using the structure to be the master geometry when creating node-to-solid links to connect the stick to the foundation block. Following the same analogy, I would probably start with treating foundation block to be master geometry when creating an interface with the soil. Please provide some thoughts.

If both geometries have the same mesh, their nodes should share the same position. In this case you can use a node-to-node interaction.
In this case, it doesn't matter who is the master. However, there is one rule:
The contact normal vector MUST go from the master to the slave (see the documentation). In this case, a node-to-node interaction has default local axes that coincide with the global axes, so the default contact vector is [0;0;1] (i.e. +Z direction).
In this way, the bottom surface should be the master.
If you want to make the top surface the master, then you need to create a LocalAxes (and assign it to the interaction) with a local Z vector pointing to the negative global Z-axis.

2. In my case both foundation block and surrounding soil are modeled with brick elements (everything has rectangular geometry - no funny angles). In my understanding, this contact is between two surfaces. Therefore, I would need to create interaction between the two "touching" faces of the foundation and soil brick elements. However, since I created the entire model using "sweep" command, it appears that there is only one face that is shared between the foundation and soil elements. So, when I want to create an interaction, I cannot select two faces (one master for foundation and the other slave for the soil) since there is only one common face for the two elements. This is where I am stuck right now. Please let me know how can I overcome this issue

In this case, you need to split the two parts which are in contact, so that they become two separated geometries. To do this, a) select the Sweeped Solid, b) Use the Explode command (this will explode your sweep in all separated solid pieces), c) if necessary join all the pieces for the soil and foundation blocks with the Merge command, to create only 2 geometries

3. In your videos, you are showing interactions together with the mesh. I am not sure how to do this. When I work with my model, everything is just in the "geometry" view and I don't see the mesh. Please let me know.

To view the mesh, you need to go to the Mesh tab in the Ribbon Bar

[kolozvari]

Thank you once again for a very quick response!

I understand what you are saying regarding exploding/merging the model. However, I ran into another set of issues.

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?

Please advise. Thank you very much!