Pile-soil Interaction Convergence

[STKO Team]

Could you please post the file that gives you the issue of non-zero displacements at the pile-toe?
It seems strange so I would like to understand why it happens

[[email protected]]

Yes. I've attached the model that replicates the InitialStateAnalysis Off issue.

I would also like to mention here as an FYI for other users that in order for the Initial State Wrapper (and non-linenar soil) to work with the BeamContact3Dp elements initial contact has to be assumed or else during the reset of displacements the model gets unstable or divergent.

During the day I figured out that the singular matrix results from using a fiber cross section with steel material instead of an elastic section. OpenSees can not create the contact between the soil and the contact elements. However, I was not able to fix the singularity issue just yet. My initial guess is that the issue may come from the meshing of the fiber cross section. I will try either refining the fiber mesh or increase the tolerance on the contact elements.

Thank you for the help! Looking forward to your tips and suggestions.

Bence

[[email protected]]

I would also like to mention here as an FYI for other users that in order for the Initial State Wrapper (and non-linenar soil) to work with the BeamContact3Dp elements initial contact has to be assumed or else during the reset of displacements the model gets unstable or divergent.

Sorry, I must specify here that this is only for the case when you install the pile first and excavate later. If excavation is finished before the installation of the pile there are no issues and following the webinar on the matter will guarantee you correct results even with non-linear soil. (Perhaps with fiber cross section as well if we solve the singularity issue here )

[STKO Team]

Dear Bence, you did a very good model!
Here is a working version of your model:

PSI_4step_remove_forSTKO2.zip

(642.24 KiB) Downloaded 218 times

there are only a few changes I had to do:

• Resetting the displacement to 0 with the InitialStateAnalysis ON/OFF works only with solid elements (2D or 3D), but not with beams or contact elements. So I had to move the InitialStateAnalsys OFF just before you added the Pile+Contact. This solves the majority of the issues you had with convergence.
• The fiber section seems to work. I included a fiber section. Probably you had singularities either because you did not input GJ. If you leave it at 0 (Default) your beam will have no torsional stiffness, hence the singularity. Another problem I found was in the plastic material. You were using a hardening ratio of 1.3, making the post-yield stiffness larger than the elastic one, and this is not physical.
• Your last stage is set to Transient. I don't think you wanted to do a dynamic analysis so I changed to static. Keep in mind that even if your load history is cyclic, it can be done in Static analysis. Dynamic does not mean cyclic, Dynamic has only to do with inertia effects. If instead, you want to consider inertia effects, go back to Transient, but do not forget to add beam mass, and make sure your time duration and dt are properly set. In your case the total duration was 1 second, so very fast for the type of load you applied.

I noticed that you successfully managed to perform an incremental excavation process using multiple removeModelSubset objects. This is fine, but sometimes it can be quite annoying when you have to remove a lot of parts. If you have some experience with Python, you can write an ad-hoc AnalasysStep, similar to the removeModelSubset, which can perform the excavation incrementally based on the current time step.

[[email protected]]

Dear STKO Team,

Thank you a lot for the final tunes on the model! I changed the analysis back to transient as it is important for my end goals with this model. I also added a top mass&load to simulate the superstructure's inertia and weight however, the mass of pile was actually applied via the disp.based.beam element already. I also moved the plastic gravity analysis into the InitialStateAnalysis portion of the simulation.

Now it works well however, I have a few concerns on the final model that I've set up. I have attached the model, if you run it and check the results there are a few conspicuous things. I also attached images if you don't have time to run the model.

First there is an upheave of the soil at the pile toe during the cyclic loading. The pile actually displaces vertically upward quite considerably. This does not seem to be physically correct. What may be the issue here? Did I mess up some material parameter again?

Upheave.png (228.05 KiB) Viewed 4172 times

Second, in the stress field I see some chaotic distributions and sudden variations between each time step (dt>=0.001s) in the soil elements surrounding the pile . This chaotic stress "flickering" only starts at the first de-loading cycle. Upon the first loading the stresses behave as expected, and they are continuously distributed. I also see some minor vibrations of the soil element edges (when looking at displacements) during and after the first unloading. The contact elements are not completely stable and they make the soil elements surrounding them "wiggle" even though the general displacements and behavior of the system is indeed correct. I assume this accurs due to the algorithm that evaluates whether the pile is in contact with the soil or not, but upon un-loading&re-loading it seems that the algorithm is struggling to decide the contact condition each time step. This is best seen when the results are animated, nevertheless here is an image of shear stresses during the first loading and the first unloading next to each other.

Correct_StressVSconspicuous_Stress.png (289.68 KiB) Viewed 4172 times

I am not sure what to make of this two phenomena, if any of you guys on the forum or at STKO have a sense of what might be going wrong please express your ideas.

If you have some experience with Python, you can write an ad-hoc AnalasysStep, similar to the removeModelSubset, which can perform the excavation incrementally based on the current time step.

PS. I just started getting into python last week, I guess I have a project to work towards now!

Thank you in advance for all the kind help!
Bence

[STKO Team]

First there is an upheave of the soil at the pile toe during the cyclic loading

Actually, I noticed this behavior even during the excavation process!
So to understand what was causing the problem, I removed the Pile and Contact, and I removed the last stage, that is, only until the excavation is finished.
I considered 3 different scenarios:

1. PressureIndependMultiYield - updated to plastic
2. PressureIndependMultiYield - kept elastic (I commented out the updateMaterialStage 1)
3. ElasticIsotropic (I used the E and nu derived from your Bulk and Shear modulus)

These are the outputs at the end of the excavation. Scenarios 2 and 3 are equal, which means that the model is working fine in the elastic range because it produces the same results as the equivalent elastic material.
So I think the issue is in your material parameters for the plasticity part. I would suggest double-checking those values.
If you think they are right, try to understand what is causing that volumetric expansion... to much dilatancy? but it seems strange because I don't think your model is going to much into nonlinear stage.
Try to investigate whether this behavior is physically correct or not. Then you can move to the dynamic last analysis-

PLASTICITY.png (405.91 KiB) Viewed 4170 times

[[email protected]]

I have noticed it in excavation too. It seemed reasonable to me as, the unloading of the toe region is significant. (120m3 soil removed+60m3 water surcharge) Hence, after producing large stresses in that area during the elastic static analysis I do expect considerable plastic deformation when I switch tonplastic state.

But during the pile lateral loading it didn't make much sense to me, as there isn't any significant unloading of the vertical forces/stresses, so I don't think the soil should upheave as much as it did during the dynamic phase.

I will look around for some answers and try to adjust the soil parameters.

In the meantime do you have any comments on the second issue related to the spurious stress development (after unloading of the lateral forces)?

Thanks a lot!
Bence

[STKO Team]

I think it's in part related to the plasticity issue. I tried to run it with an elastic material and I don't see those huge oscillations.
I do see some small oscillations in shear stress upon load reversal, But I think it's normal. First try to record accelerations to make sure your dynamic analysis is set correctly (correct time step, some damping...). If you see accelerations growing without control, it means that you need to refine your mesh or your time step.

[[email protected]]

Thank you a lot for the advice. I'll run some tests and do some research on this.

[STKO Team]

You are welcome, let us know how it goes!
STKO Team