Mesh Sensitivity for pile-soil interaction

[[email protected]]

Dear STKO team,

I've been working with the beamContact3D element for pile modelling for a while now. I got to the final stage of my modelling, so I ran a mesh sensitivity analysis to optimize the size/accuracy of my model. However, I noticed a divergence of lateral displacements when I increase the horizontal (parallel to the pile) mesh density. I am not sure what may be causing this. I'm attaching the model and a figure that compares the results for two different densities. (note, I have tested much denser meshes as well and the lateral displacements keep growing with denser meshes)

D6L20_FIN_DenseLat.rar

(745.79 KiB) Downloaded 255 times

To my understanding the beamContact element acts as an interface element and the slip between the pile and the soil interface concentrates in this element, hence the model's accuracy should not be strongly dependent on the density of the soil mesh around the pile. Of course a refinement is necessary and increased displacements are to be expected due to a denser horizontal mesh when using a non-linear soil constitutive model, however a strongly divergent behavior should not occur normally.
The model uses PIMY material and std brick elements for soil and a fiber cross section with displacement beam-column element for the pile. The analysis is transient with a 2s sine wave force+moment loading. I have purposefully left the soil inside the pile zone, as my pile in this model is a pipe pile with soil plug.
Perhaps the interaction between the soil plug and the exterior soil is causing this phenomenon? Is someone familiar with this mesh sensitivity issue? What is the solution to this divergence issue? Any advice would be appreciated.

Thank you very much for all the help I can get in advance!
Bence

Sensitivity.png (571.52 KiB) Viewed 5332 times

[STKO Team]

Dear Bence,

You are right in saying that upon mesh refinement you should converge to a unique result.

However, keep in mind that if you refine only the horizontal direction, your Hexa elements will increase their aspect ratio. Since you are using a biased mesh (finer near the circle) your elements close to the hole are also skewed.
So while you refine your mesh, you also increase their distortion (mostly aspect ratio, but also skew distortion for elements near the hole).
With standard isoparametric elements, this deteriorates considerably the element response.

The model you posted seems different from the one you are describing here (column mesh is different, and there is still the element removal).

However, I would suggest you do a step-by-step approach to identify the source of the issue:

1. Try a quasi-static analysis with a linear time series, to see if there is a problem with the transient integrator or inertia effects (if it fixes your problem, you have to look at alternative transient integrators or check for critical time steps)
2. Try elastic material, to see whether the mesh distortion causes problems to the plastic material, or also to the elastic one (if it fixes your problem, then probably the error comes from the plastic material, and the poor prediction coming from a distorted element)
3. If none of the above works, probably it's all about excessive mesh distortion. If this is the case, let me know and I will show you how to use a newly developed boundary conditions that will allow you to minimize this mesh distortion

[[email protected]]

Thank you very much for the prompt reply. I'll run the tests and report back!

[STKO Team]

You are welcome, keep us posted!

[[email protected]]

Dear STKO team,

An important addition to the original problem is that the original model was drastically over estimating displacements even for coarse mesh (meters of displacement while it should be in centimeters order).
I have run the elastic analysis. Which does not have this divergence issues with increased mesh density. I tried to run static non-linear analyses as well, but I couldn't stabilize the model, so I only got up to about 0.4 load factor. However, this result seems to be in line with the elastic results (displacements slightly larger at the same load factor but still in the order of centimeters).
In conclusion I believe the issue has a duality. The degenerate mesh results in larger errors and higher concentrated stresses around the pile (as you mentioned this may stem from some issue with the integrator) and due to this issue the non-linear soil model exaggerates the deformations, as the constitutive model does not have a length scale and tends to infinite deformations with increasing stress localization.

I am attaching the correct original model (last time I attached a different one as you mentioned) as well as the static and the elastic ones.

Thank you for the help!
Bence

[[email protected]]

Dear STKO,

I've seen you postponed the E-learning webinar for the implicit-explicit contact element to October. I was wondering if the element is available for a try prior to the webinar and whether there is a paper published on it, so I can implement the element into my models. The current beam contact element available is very unstable so I'd like to give the new element a try.

Thanks,
Bence

[STKO Team]

Regarding your previous post,
Try this:

D6L20_FIN_DenseLat.zip

(1.53 MiB) Downloaded 257 times

I used integrator = TRBF2 and I changed the geometry adding a circle around the hole, so that you can increase the mesh size there, without using the bias mesh (which is causing mesh distortion).
Try it and see if the response is any better.
Keep in mind that if the plastic material is going into a high plastic state it makes sense to have large displacements.

Regarding the Webinar, the zeroLengthImplexContact is already available in version 2.0.3. But we need to create a custom Python script that allows you to automatically create an offset from the beam so that it acts like the BeamContact.

If you want to just test it you can do it and if you have issues, let us know

[[email protected]]

Thank you very much for the help. I will try the new geometry.

The TRBDF2 integrator was not able to handle the original mesh either, I tried it last week. Hopefully simply changing the mesh quality will overcome this issue as the two suggested integrators for the contact element (TRBDF2, and Newmark with increased numerical damping) were all resulting in divergence with increased mesh density.

Just for some further tests in case the new geometry does not solve the issue, how can I determine critical time steps for the system? You mentioned this may be an issue as well.

Bence

[[email protected]]

Dear STKO,

I have tried the new mesh configuration with the TRBDF2 integrator. I am getting the same divergent results as before. Considering that the elastic model was working well I presume there is some incompatibility with the PIMY material model and the contact element. I am not sure how to move forward from here as without the non-linear soil or the contact I can not proceed with the simulations. What alternatives would you suggest?

Thank you for the help in advance!
Bence

[STKO Team]

Ok so the mesh distortion is not the main issue. let's try a couple of things.

I don't think there is a "direct interaction" between the contact and the material model itself.

First, try to look at the stress-strain results (export chart data) in some of the elements near the contact. Probably by looking at the stress-strain result you will find some issues in the constitutive model.

If the stress-strain looks reasonable, let's try to see if there is an issue with the dynamic analysis. Try to convert your analysis into a static one. If the results are ok, probably there is some instability in the dynamic analysis (in this case we will see it later)