soil structure interaction

[STKO Team]

Maybe you are right and in this case, the soil is not affecting the behaviour.. but if I model the springs, it does...You can see that in the plot attached. That's why I wanted to check what happens if I add another type of interaction...

Probably the properties you used for the springs were not equivalent to the properties you assigned to the Soil model. I suggest you double-check the properties of your soil. Start with an elastic material first, because, with your springs, the response was different already in the linear stage.
Once you check them, you can move to a nonlinear model. Another note: you used the PressureIndependentMultiYiled, but since it is pressure independent, it means it uses a Von-mises-like criterion. I think you should use the PressureDependent material, which instead uses a Drucker-Prager-like criterion.

Yes, I tried that. I added ZL3dcontact in the structure. However, there is a convergence problem. Two foundations seem to be collapsing in the first steps of the analysis (see image).

It happened for 2 reasons:

• your beamToSolidCoupling condition is using only the 4 corners as slave nodes, while you should use the whole top face as slave.

  

  Immagine 2021-03-17 104107.png (54.16 KiB) Viewed 7058 times

• You used EDOFs for the foundation sides, which will restrain the foundation rigid body rotation.

Here is a working copy of your file where the beamToSolidCoupling is attached to the whole top face of the foundation, and the EDOFs at the foundation level are removed (they are unphysical)

03_SOLID_01_push_6_ZLcontact.zip

(3.08 MiB) Downloaded 306 times

Immagine 2021-03-17 121822.png (120.91 KiB) Viewed 7058 times

[mmc]

Dear STKO,

Thanks always for your replies.

I have been working lately on performing several analyses. I have found out that owing to the characteristics of my structure and soil, my building's performance is not affected by the SSI effects... You were right.

I have also been working on improving the modal analyses of my buildings. I have tried to perform analyses using the code you provided me but if I include the soil, an error appears... Also, how can I add the mass of the foundation and the soil, as VolumeMass?

I also wanted to ask you if there is a way to obtain the eigen vectors already normalized in an output file. I want to process them later in Matlab... I have also seen that it is possible to apply them proportionally to the master nodes... Would it be like a customcomand defining a load pattern?

[STKO Team]

I have been working lately on performing several analyses. I have found out that owing to the characteristics of my structure and soil, my building's performance is not affected by the SSI effects... You were right.

Ok, we were expecting that.

I have also been working on improving the modal analyses of my buildings. I have tried to perform analyses using the code you provided me but if I include the soil, an error appears.

Just use Mumps, probably UmfPack is not able to handle such a huge model. With OpenSees + Mumps + 1 processor it runs well.

Also, how can I add the mass of the foundation and the soil, as VolumeMass?

Yes, Volume mass. I saw you added mass only in Z direction. In reality, mass is along all the 3 axes.

I also wanted to ask you if there is a way to obtain the eigen vectors already normalized in an output file. I want to process them later in Matlab... I have also seen that it is possible to apply them proportionally to the master nodes... Would it be like a customcomand defining a load pattern?

You can so it as I did in the TCL custom command. Unfortunately it cannot be done automatically in OpenSees

[mmc]

Hi STKO,
Thanks for your advice. You were right.
This time I am writing to you regarding the dynamic analysis of the model.
I have followed the webminar of SSI. I have included all of the steps. The model is calculating. However, the building is being deformed too much at the gravitational step. It is sinking a lot. I think that the problem is related to the fixity in the Z direction. I added it as the webminar but I think that I should also fix the X and Y direction. What do you think?
Also, I added the damping of the structure using the region command. However, I am not sure how to add the damping of the soil. Is it considered by STKO automatically? Or a way to automatically consider it? Or should I add it manually with the region command?
I added the monitor step. However, an error appears in the cmd.exe saying that it cant finde the Python file... How can I solve this error? I downloaded the latest version of OpenSees solvers.
Regards

[STKO Team]

It was sinking because you applied the "Force From Reaction" in a wrong way:

This tool adds, on each node of the selection, forces equal to the reactions.
SO it makes sense to apply this condition, ONLY on nodes whose fixities are removed during your analysis.
However, you applied this condition on the whole soil domain.
In this way it is also applying forces from reactions obtained from the kinematic constraints between soil and foundation.
Keep in mind that a reaction arise not only from SP constraints, but also from MP constraints (kinematic constraints)

Here is a working version of your model

05_SOLID1_dynamic_LK_2.zip

(6.37 MiB) Downloaded 314 times

[mmc]

Hi!
Thanks for your reply.
My bad! It is like I am always forgetting something about the modelling...
The model is working, yes. However, the displacement is minimum compared to the fixed model or the one using springs. You can see that in the plots I uploaded. In the case of the soil model, the displacement is reaching higher values than the fixed model. This is even at the beginning of the analysis. I obtained these results by adding the GM as a Uniform Excitation pattern.

So, I decided to study the solid model again. First, I added the Cv and Ch considering the properties of my soil (I used the same for all of the soil layers). Then, I converted the GM from acceleration into velocity by integrating. The acceleration is expressed in g (so, I had to multiplied it by 9.81 m/s2). Did I do it right? Hen, I added the cFactor in the definition Path to scale it to meet the response spectrum and the fundamental period of the building. I added the corresponding damping for the soil and the structure. My first question is if I should add the cFactor there or if I should add the vectors multiplied by this.

Also, I have seen in your SSI webminar that you added a scaling factor at the bottom in the loadPattern definition. This factor is used, if I am not wrong, to convert the GM into a time history horizontal force (velocity into force). I have read about it and I have seen that:

This force history is obtained by multiplying the velocity time history of the recorded ground motion by the mass density and shear wave velocity of the underlying bedrock layer and the area of the base of the model

I have seen that you multiplied it in the webminar by the acceleration and not the velocity so I just wanted to confirm that I did it right. In my case, I have 1.79Mg/m3*1250m/s*0.15g=3292. I used 0.15g because my GM is defined for that IM. (Note: this GM has been defined for a soil type B, not A (rock). That's another thing that I should change). I added this factor and I got huge values of displacement compared to the fixed or the springs' models.

I have plotted the displacement at the bottom and the control node to check if there were any reflections. I think that there arent. However, I am worried about the results at the foundation level. The plot is the same as the one corresponding to the bottom of the soil. So, I think that the damping of the soil is nor really affecting..

Do you think that those values are correct? Any thoughts?

PD: I was able to open the STKO Monitor finally. There was something weird with my Windows. It is a cool option. Also, I tried to find the FLAC manual but it is no longer available.

[STKO Team]

However, the displacement is minimum compared to the fixed model or the one using springs...
... obtained these results by adding the GM as a Uniform Excitation pattern.

Keep in mind that when you do a fixed model with uniformExcitation, the results you obtain (disp, vel, acc) are relative to the input ground motion. In fact, if you check the acceleration at the base they will be 0.
While, with an LK approach, where you apply the acceleration as a force at the base, the results are absolute, in fact, you will see that also the base of the model is moving, and the acceleration at the base is exactly the acceleration associated to your ground motion (if you did all the conversions properly).
So if you want to compare the displacements of the 2 models, you should compute the displacements relative to the rigid displacement at the bottom.

Also, I have seen in your SSI webminar that you added a scaling factor at the bottom in the loadPattern definition. This factor is used, if I am not wrong, to convert the GM into a time history horizontal force (velocity into force). I have read about it and I have seen that ...
... I have seen that you multiplied it in the webminar by the acceleration and not the velocity so I just wanted to confirm that I did it right

Yes, the scaling factors in opensees are quite confusing... in this specific case there are 2 scaling factors that you can use:

1. the cFactor in the timeSeries (call it alpha)
2. the cFactor in the loadPattern (call it beta)

If you want to use them or not, it's up to you. The only thing that matters is that the output value of the applied force at time t is exactly what you expect:
F(t) = timeSeries(t)*alpha*F_ref*beta
This means that the reference load (F_ref, i.e. the value that you applied in the FaceForce condition) is multiplied by the timeSeries at time t, multiplied by the cFactor of the timeSeries and by the cFactor of the loadPattern.

For example in my webinar, the F_ref was unit (1), the time Series was normalized such that it would have produced an acceleration of about 1, so I put the entire scale factor in beta: 0.4*g*rho*Vs, while alpha was 1.
so F(t) = timeSeries(t)*alpha*F_ref*beta = 1 * 1 * 1 * (0.4*g*rho*Vs).

Try to make sure that all the abovementioned points are clear, check your model, and let's see if there is something wrong

[mmc]

Hi. Thanks for your answer. I have a few questions.

So if you want to compare the displacements of the 2 models, you should compute the displacements relative to the rigid displacement at the bottom.

I am not sure I understand this.

Regarding the cFactors, I have considered the following:

• I added the GM in velocity in the Path. I had the acceleration in g and dt (0.005). So, before integrating, I multiplied the Acc by alpha (1.252) and 9.81 m/2. Also, I normalized de Acc by dividing it by the Maximum acceleration. I finally didnt add alpha in STKO

• I added 1 as the vector of the FaceForce. (I normalized the Acc)

• I added beta (which multiplies the timeSeries Velocity) in the LoadPattern as rho*Vs, being 2237. In the OpenSees documentation, it says that beta multiplies the timeseries velocity so I dont understand why you multiplied it by 0.4g. Also, it is said that it should be multiplied by the area of the base of the model. I assume that the command does this automatically in STKO.

I have plotted the GM multiplied by alpha and the Acc at the bottom of the soil. Both curves are more or less similar. Why do you think that they are not the same?

[STKO Team]

so I dont understand why you multiplied it by 0.4g

Because the velocity I put in the timeSeries was normalized such that it will produce an acceleration of 1g, but I wanted a lower acceleration of 0.4g... That's all. I could have done it in the timeSeries, in the cFactor of the timeSeries... as I said the only important thing is that finally you obtain what you want. I'm soory if that made confusion.. I should have added it to the timeSeries.

Also, it is said that it should be multiplied by the area of the base of the model. I assume that the command does this automatically in STKO.

In the example you are refering to, they used just 1 single dashpot at the base, where all the base nodes where connected via an equal-dof in the X direction. In that simplified case, since you have only 1 dashpot for the whole base, you need to scale it for the total area.
STKO instead allows you to insert the dashpot values per unit-area (3D) or per unit-length (2D) and it does the nodal-lumping for you based on the tributary area of the mesh node.

I have plotted the GM multiplied by alpha and the Acc at the bottom of the soil. Both curves are more or less similar. Why do you think that they are not the same?

Because the LK conditions are not exact... unfortunately they are not so precise in complex models... I would suggest to use a simple ricker wavelet (as I did in my tutorial) to make sure that everything is working as expected. then you change it with the actual ground motion

[STKO Team]

Did you complete the analysis? You should be able to see the whole model. If it says that one of the DB is inconsistent is because probably you interrupted the analysis while one of the processes was still writing