soil structure interaction

[mmc]

Thanks @clarabella.
And again, this is also weird. The pushover curves for a soft clay and a stiff clay are practically the same... (these horizontal analyses do not consider the gravity analysis as mentioned previously)

[STKO Team]

I checked your model.

I removed the EqualDOF (X and Y) for soil, they are unnecessary since you fixed Ux and Uy on the side faces.

However, the non-convergence was due to the fact that the gravity analysis was generating stresses in the soil that were quite outside its linear limit. Then, when you call the updateMaterialStage, the soil suddenly turns nonlinear, but it does not manage to bring the elastic stress onto the yield surface all at once.

What I did is to:

• move the updateMaterialStage (plastic) before the gravity analysis
• remove the body force from the SSPBrick element property, because they will be applied all at once (difficult for convergence)
• I applied the soil and foundation body forces as VolumeForce, and then I added them to the load pattern. The advantage is that they will be applied incrementally.

As you can see the vertical analysis is already nonlinear:

Immagine 2021-03-03 192452.png (10.78 KiB) Viewed 5851 times

And this is the final result:

Immagine 2021-03-03 192435.png (232.37 KiB) Viewed 5851 times

The only doubt that I have is about Py springs... I think you should use them when you don't model the soil. In your case the soil is explicitly modeled. And in fact, if you change the soil properties, but you keep the Py springs equal, probably they are governing the response (especially if they are softer than the soil).
Make sure you really need those Py Springs

Here is the file:

05_ST-INF-SOLID_3_pushXY_DISC__.zip

(4.13 MiB) Downloaded 327 times

[mmc]

Thanks for your advice.

I removed the EqualDOF (X and Y) for soil, they are unnecessary since you fixed Ux and Uy on the side faces.

Okay, thanks. I wasnt sure about that...

What I did is to:
move the updateMaterialStage (plastic) before the gravity analysis
remove the body force from the SSPBrick element property, because they will be applied all at once (difficult for convergence)
I applied the soil and foundation body forces as VolumeForce, and then I added them to the load pattern. The advantage is that they will be applied incrementally.

In the model attached, the updateMaterialStage is still after the gravity analysis... I have moved the command before the gravity analysis. I have run the analysis and my curve reaches 0.26 of displacement while in your model it reaches at least 0.38...I dont know if the convergence problem is due to this fact.

The only doubt that I have is about Py springs... I think you should use them when you don't model the soil. In your case the soil is explicitly modeled. And in fact, if you change the soil properties, but you keep the Py springs equal, probably they are governing the response (especially if they are softer than the soil).
Make sure you really need those Py Springs

I thought that this was a way to link the soil to the nodes of the walls. I am going to change them into Eqdof links. However, there is a friction contact between the walls and the soil...I havent come up with an idea to model that and it was just an initial approach. But thanks for that, you are right about this.

Have you checked what I mentioned about the similar curves that I obtained for the stiff and soft clays? Do you think that are those values real? I am gonna try to run the code in OpenSees to check that... I dont know... it seems weird to me..

Also, how did you define the pushover curve in STKO in the postprocessor window? Maybe that's another thing that I am not doing right... I thought that in displacement control analysis, the load that you apply is the pseudo time step... But I have seen that in your plot, you considered different variables (Sum(RFx) and Ux).

[STKO Team]

In the model attached, the updateMaterialStage is still after the gravity analysis...

No, it is before the analysis, it is after the loads, but before the analysis. If it is before or after the application of loads does not change anything, the only important thing is that it is before the analysis.

before.png (13.66 KiB) Viewed 5842 times

I have run the analysis and my curve reaches 0.26 of displacement while in your model it reaches at least 0.38

Actually, I stopped it at 0.38.. but it was converging fine. If your model is not converging, and you did no change on the model I sent you, make sure you are using the latest OpenSees version. I'm using the one hosted on Prof. Tarque's website (OpenSees-Solvers-3.2.2)

I thought that this was a way to link the soil to the nodes of the walls. I am going to change them into Eqdof links. However, there is a friction contact between the walls and the soil...I havent come up with an idea to model that and it was just an initial approach. But thanks for that, you are right about this.

If you change them with EDOF, then you are doing a perfect connection. If instead, you want to simulate frictional contact, you can use the zeroLengthContact element or other contact elements. In both cases, I would subdivide the soil geometry so that is is alligned with the beams that are in contact, otherwise the links will not be alligned, and won't give you accurate results.

Have you checked what I mentioned about the similar curves that I obtained for the stiff and soft clays? Do you think that are those values real? I am gonna try to run the code in OpenSees to check that... I dont know... it seems weird to me.

I did test only the material parametetrs you put in the file, however looking at the output (material.stress) of your Py zeroLength, they were fully in plastic stage... What I meant is that you can change your soil properties as you want, but if the Py spring fails, it will be the one that determines the output of the analysis.

Also, how did you define the pushover curve in STKO in the postprocessor window? Maybe that's another thing that I am not doing right... I thought that in displacement control analysis, the load that you apply is the pseudo time step... But I have seen that in your plot, you considered different variables (Sum(RFx) and Ux).

In the Displacement Control, the pseudo-time is the Load multiplier. In your case, the sum of the nodal forces at the diaphragms is 1, so yes, the load multiplier will also be equal to the total force.
I simply did it in another (equivalent) way, I extracted both the displacement at the top node, and the reaction forces (Sum operation) at all the fixed dofs.
Another nice feature is the monitor Analysis step. It basically allows you to plot something in real time while the analysis is running.
Check our webinars for that feature. A webinar where I used it, was the out of plane failure of masonry walls with micro modelling

[mmc]

Hi again.
Thanks for your answer.
My concern is now on what you mentioned here.

If you change them with EDOF, then you are doing a perfect connection. If instead, you want to simulate frictional contact, you can use the zeroLengthContact element or other contact elements. In both cases, I would subdivide the soil geometry so that is is alligned with the beams that are in contact, otherwise the links will not be alligned, and won't give you accurate results.

How should I apply the zeroLengthContact element. It is an element property but, do I have to apply any physical property? Like a material or something like that? How would you do that?
Also, I have redone the mesh so that the nodes are aligned. I knew I would have to do that eventually.
Regards

[STKO Team]

How should I apply the zeroLengthContact element. It is an element property but, do I have to apply any physical property? Like a material or something like that? How would you do that?

It really depends on what kind of contact you want to simulate.

The easiest is the unilateral (frictionless) contact. In this case, you can use a simple zero-length, whose physical properties use a uniaxial ENT (elastic no tension), where the E is quite large like a penalty parameter.

If instead, you want to simulate a real normal and frictional contact, then it's going to be a little more complicated. In this case, you can use the zeroLengthContact element (no physical property is needed).
However, your master and slave nodes must be aligned and starting at the same position. You should also pay attention to the master->slave direction. See the documentation of that element to understand what I mean

[mmc]

The easiest is the unilateral (frictionless) contact. In this case, you can use a simple zero-length, whose physical properties use a uniaxial ENT (elastic no tension), where the E is quite large like a penalty parameter.

I have used this approach in the model where I have redone the mesh... I used 1e+16 for the E, like the Penalty parameter. However, there are several convergence errors. I am not quite sure about how to add them...

What I could actually do is to add those ENT ZL elements in a 1 bay model. If I use a large value of E, the pushover curve is similar to the Eqdof curve... If I consider a smaller E, like 10000, the curve presents lower initial stiffness, leading to a worse behaviour.

If instead, you want to simulate a real normal and frictional contact, then it's going to be a little more complicated. In this case, you can use the zeroLengthContact element (no physical property is needed).
However, your master and slave nodes must be aligned and starting at the same position. You should also pay attention to the master->slave direction. See the documentation of that element to understand what I mean

I have read this other topic viewtopic.php?f=29&t=1711&p=2350&hilit=CONTACT#p2350. I am not sure if you have modified this element so that the direction can be omitted. I think that it is not available yet from your comment.

I have used ZLcontact elements in a model that is more horizontal because with Eqdof, the pushover curves considering a soft and stiff clay were similar to the fixed cuve... It was weird and that's why I wanted to try new types of interaction. They were similar even if I used a well fitted mesh. I added the ZL elements taken into account the direction, however, there are several convergence problems considering krylov. Therefore, since I am using contact elements, I used Newton with LineSearch. Turned out that the resulting curve is similar to the one I obtain with Eqdof and also similar if I consider a soft and stiff clay...

What do you think? I know that it is a lot to handle...

[mmc]

Sorry, I forgot to upload the file with the Eqdof and the different soils...

[STKO Team]

I have read this other topic viewtopic.php?f=29&t=1711&p=2350&hilit=CONTACT#p2350. I am not sure if you have modified this element so that the direction can be omitted. I think that it is not available yet from your comment.

We are in the last stages of testing this new contact element, it will be available in few days. We will let you know.

Sorry, I forgot to upload the file with the Eqdof and the different soils...

If your curves are so similiar, with soft/stiff soil springs and also with EDOF, by best guess is that the soil in your model is not relevant to the structural behavior.

Let's see what happens when using contact

[mmc]

Thanks for your reply STKO...

If your curves are so similiar, with soft/stiff soil springs and also with EDOF, by best guess is that the soil in your model is not relevant to the structural behavior.

No sorry, that's not what I meant.... The curves are similar using soft/stiff soil springs. It is something related to this issue... viewtopic.php?f=36&p=3144#p3144 I will have a look at it...

Regarding the soil modelled as continuum, similar curves are obtained if I consider the interaction with Eqdof and Krylov and ZL3dcontact element using Newton with LineSearch. Also, these curves are similar to the fixed model and if I consider a soft and stiff soil.

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...

Let's see what happens when using contact

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)... that's weird and seem a little bit random. Why those two? And why are there convergence problems if the structure has just moved 1cm?... I tried different options in the analysis but none of them resulted in normal values... I think the values of the elements are okey and the direction of application are in the positive X, Y and Z...
Any ideas?