Soil-Pile Interaction Modeling

[kolozvari]

Hi I was wondering if you had a chance to look at the model and if you found reason for the two issues. Please let me know. Thank you..

[STKO Team]

The beamSolidCoupling is an automation that creates a mix of rigidLink (6 DOFs for the beam) and equalDOF (3 DOF for the solid). Due to this, some nodes are part of both constraints.
This is not supported by the Transformation method in OpenSees.
Everytime you have overlapping constraints, the only handler can be the Penalty

[kolozvari]

That worked. Thank you!

[kolozvari]

Hello, I have another two quick questions regarding this model.

1) I have run the analysis with and without cohesion defined in the ContactMaterial3D. However, the cohesion parameter has zero impact on the overall stiffness of the system. Is the cohesion parameter in the ContactMaterial3D somehow not compatible with the zeroLengthContactASDImplex element? Can you please let me know how can I include cohesion in the analysis?

2) Regarding the units of stiffness parameters of contact elements. My understanding is that the interface elements can be considered as a nonlinear spring between nodes. Then, units of stiffness should be [Force/Displacement]. (e.g. [N/m]). In the case that the interface elements are applied to a surface, it is considered that each spring has a stiffness proportional to its representative area associated the node where the spring is attached. In addition, the stiffness of the springs per unit area (a kind of average stiffness) are considered to be the same in the same interface element. Therefore, the stiffness of each spring is obtained by multiplying an average stiffness and a representative area of the node. Here, the unit of “Average stiffness” is [Force/Displacement/Length^2] which is equal to [Stress/Displacement]. (e.g. [Pa/m]). So, my understanding is that units of stiffness parameters (G in ContactMaterial3D and Kt in zeroLengthContactASDImplex) are N/m2/m. Can you please confirm that my understanding is correct or please correct me if I am wrong.

Thank you.

[STKO Team]

1) I have run the analysis with and without cohesion defined in the ContactMaterial3D. However, the cohesion parameter has zero impact on the overall stiffness of the system. Is the cohesion parameter in the ContactMaterial3D somehow not compatible with the zeroLengthContactASDImplex element? Can you please let me know how can I include cohesion in the analysis?

The ContactMaterial3D is not used by the zeroLengthContactASDimplex element. It does not require any material because everything is defined in the element property itself.
In the current implementation, this is a pure contact element (no cohesion or tension strength typical of cohesive/contact elements).
Anyway, we are implementing the cohesive/tensile strength in this elements in the near future.

2) Regarding the units of stiffness parameters of contact elements. My understanding is that the interface elements can be considered as a nonlinear spring between nodes. Then, units of stiffness should be [Force/Displacement]. (e.g. [N/m]). In the case that the interface elements are applied to a surface, it is considered that each spring has a stiffness proportional to its representative area associated the node where the spring is attached. In addition, the stiffness of the springs per unit area (a kind of average stiffness) are considered to be the same in the same interface element. Therefore, the stiffness of each spring is obtained by multiplying an average stiffness and a representative area of the node. Here, the unit of “Average stiffness” is [Force/Displacement/Length^2] which is equal to [Stress/Displacement]. (e.g. [Pa/m]). So, my understanding is that units of stiffness parameters (G in ContactMaterial3D and Kt in zeroLengthContactASDImplex) are N/m2/m. Can you please confirm that my understanding is correct or please correct me if I am wrong.

First, a small clarification:
There are no surface interface elements in OpenSees. Only springs (zero length elements), So their units are always force-disp.
Now in STKO we allow user to assign contact elements betweens surfaces. If you do so, you can optionally check the "distributed" option in the element property. If you select it, the stiffness you input will be multiplied by the tributary area of that node.
That being said, if it matters or not depends on what you are modelling.
If you model a pure contact (interaction between to bodies that are already separarted), it does not matter. because thew Kn and Kt should be theoretically INF. Of course, due to the penalty approach, you assign a high stiffness instead of an infinite value.
Instead, if you are modeling a cohesive zone, i.e. a layer of material that connects two separated bodies, Kn and Kt are real stiffnesses (then they will depend on the elastic moduli of the cohesive zone and its thickness which is not modelled - zero-length... ), because in that case you want to include the deformability of that finite-length cohesive zone

[kolozvari]

Hello, I have worked on expanding my model of a single pile to a model of group of 9 piles. I used the same model as previously discussed in this thread and simply copied it 9 times and made appropriate modifications of boundary conditions. I also added a pile cap that connects all piles together. You can see the geometry of the model below.

Geom.JPG (50.65 KiB) Viewed 4007 times

When I run the model it appears that contact between the soil and the piles has issues. As you can see in the figure below, the piles simply penetrate through the soil.

Capture2.JPG (95.93 KiB) Viewed 4007 times

You can also see from load-deformation curve, that this penetration is not happening linearly. The model starts with a stiff response, as it should, but then the penetration starts increasing exponentially.

Capture.JPG (24.13 KiB) Viewed 4007 times

I tried many different things, such as changing the slave vs. master geometries in the interactions, checked local axes, played with the Kn and Kt stiffnesses. Some of these attempts did impact the results, I cant seem to get a reasonable model response.

I attached the model and I would really appreciate if you could take a look. I am almost certain that the issue is with the modeling of the contact.

Looking forward to hearing from you. Thank you.

[kolozvari]

Hello, I was wondering if you had a chance to look into this. Please let me know. Thank you.

[STKO Team]

You forgot to assign local axes to your node-node side interactions.

But pay attantion: the cylindrical local axes if valid only for you first pile! the cylindrical and spherical local axes are location-dependent.
So you can either create 1 cylindrical local axes at the center of each pile (but in this case you need 1 interaction per pile),
or you can move to node-to-element interaction and use FromElement option (it will take the normal vector from the master surface).

See this example:

Group_of_Piles.zip

(1.52 MiB) Downloaded 296 times

[kolozvari]

Hello,

Thank you for your response. I have ran the model with the group of piles and the piles do not penetrate the soil anymore, so that issue is fixed. However, the overall stiffness of the systems seems smaller than expected. Upon in-depth investigation, it was observed that interactions are not connected as one would expect. Despite the fact that the locations of nodes of the pile elements and soil domain coincide, it appears that interactions are not generated between the closest nodes (see circled interactions in the screenshot below for more details). I would expect that these would show as dots, not lines. Can you please let me know how can this be fixed? The file attached in your response is the most recent one - i just increased the number of elements in vertical direction.

Capture.JPG (113.75 KiB) Viewed 3838 times

Please let me know. Thank you

[STKO Team]

That's not the issue. It's just a visual representation of the node-to-element interaction:
For each slave node, STKO searches for the sub-triangle of each quad face it touches. Then it creates a visual representation of 1 line for each of the 3 masters (of the sub-triangle master) connecting them to the slave node.

If the stiffness is not as expected try to play with the contact parameters.
Also, try to make use contact also at the bottom face of the pile cap, probably its friction with the soil can play a role