Analysis using ASDAbsorbingBoundary3D

[kolozvari]

Thank you for your response.

But your input (time series assigned to the absorbing element) should be the velocity associated with the acceleration you want.

Yes, I have applied velocity history that correspond to sinusoidal acceleration with magnitude of 1.0 m/s2.

If the material properties (G, Poisson, and rho) of your absorbing boundary at the bottom match the ones of the soil model, you should have exactly the input you want.

This is interesting. Why does a material property of the absorbing boundary affect the acceleration applied at the bottom of the soil? That means that there should be some kind of relationship between the input and the output, but per the previous quote, it is just a velocity and acceleration, without considering properties of the boundary at the bottom. Maybe I am missing something. Also, please see the explanation about the model at the bottom.

In this case, since you are applying the input as a boundary traction (your input velocity transformed to boundary traction by the ASDAbsorbingElement) the accelerations will be absolute, that's why you should see your acceleration at the base and not zero.

OK, so just to triple check. When using absorbing boundary at the bottom to apply ground motions by applying tractions via velocity, you get absolute accelerations as output. Please confirm.

If your share your model here I will check what's wrong.

Thank you so much. Attached is the same model as the big domain (240m x 240m), but I reduced it only to 2mx2m because of the runtime (big model takes an entire day on 25 cores). I checked and the results are identical between to big domain model and the small domain model, which is good news meaning that absorbing boundaries work the same way for both models. If you can find a mistake in the small model, it should work for the big model as well.

Please note the following regarding the model attached: it has two materials for absorbing boundary at the bottom: a) same as absorbing boundary on the sides, and b) the one called "bedrock", which is stiffer and corresponds to rock at the base of the domain. Interestingly, input motion at the bottom of the soil column is not the same when I change between these two materials assigned to the base absorbing boundary element. (see attached picture).

It would be great if you can figure out what is the issue. I spent a lot of time playing with this. I just trying to apply 5Hz sinusoidal motion to the soil and compare it with theoretical solution.

Looking forward to hearing from you. Thank you!

[STKO Team]

Yes, I have applied velocity history that corresponds to sinusoidal acceleration with a magnitude of 1.0 m/s2

What you input for velocity is not exactly the derivative of a sin acceleration of 5 Hz frequency. In fact, the initial slope of your velocity should grow slowly, instead, in your case, the initial slope is not 0, so it generates that strange peak at the beginning.
Use this:

Code: Select all

acc = amplitude*sin(time*2*pi*frequency);
vel = -amplitude*cos(2*pi*frequency*time)./(2*pi*frequency);

This is interesting. Why does a material property of the absorbing boundary affect the acceleration applied at the bottom of the soil? That means that there should be some kind of relationship between the input and the output, but per the previous quote, it is just a velocity and acceleration, without considering properties of the boundary at the bottom. Maybe I am missing something. Also, please see the explanation about the model at the bottom.

You input a velocity, and the absorbing boundary converts it into an acceleration using the shear wave velocity (Vs = sqrt(G/rho)) and the mass density. If you use different material properties in the absorbing boundary and soil elements this won't work.

OK, so just to triple check. When using absorbing boundary at the bottom to apply ground motions by applying tractions via velocity, you get absolute accelerations as output. Please confirm.

Yes, absolute accelerations

Please note the following regarding the model attached: it has two materials for absorbing boundary at the bottom: a) same as absorbing boundary on the sides, and b) the one called "bedrock", which is stiffer and corresponds to rock at the base of the domain. Interestingly, input motion at the bottom of the soil column is not the same when I change between these two materials assigned to the base absorbing boundary element. (see attached picture).

If you want to simulate the presence of bed rock, model a piece of it, and below that, use the absorbing boundaries matching those values. You have to follow one rule: the absorbing boundary you apply on a face of a soil domain should have the same material properties of that soil domain.
In our webinar about absorbing elements I also made an example with a layer of bedrock (it's like a multi.-layer soil column)


Regarding the strange behavior you see at the base

1. If you fix the input velocity with the correct derivative of the sinusoidal function, you will see that the initial wave at the bottom has a maximum of 1, as you would expect
2. Now you will notice that after 2 waves the following waves are smaller. This is perfectly normal:
   Once the first waves hit the top free surface, they are reflected back towards the bottom, but due to a time shift based on the height of the soil column, they will sum/subtract to the new waves that are "going in" from the input time series.
   You can verify this, randomly changing the height of the column: the higher it is, the more waves with a correct peak of 1 you will see.

[kolozvari]

Thank you very much for looking into this and for clarification. I will keep this in mind moving forward.

[STKO Team]

You're welcome

[kolozvari]

OK, I am ready to start adding structure on top of the soil domain. I remember seeing your video about this, but I wasn't sure which one would be the best example. I have a mat foundation on top of the soil domain. Can you please point me to an similar example that shows how to add a mat foundation on top of the soil and model soil-foundation interaction correctly?

Thank you very much!

[Clarabella]

There are a few webinars also showing the structure, please check our webinar page.
There are also a few topics on our forum, I think this could be interesting for you for example:
https://asdeasoft.net/forum/viewtopic.php?f=33&t=2175

If you intend to model just the mat in interaction with the soil you mainly have two options:
1) Embed the mat at the top of the soil. The foundation will be in full contact with the soil
2) Use the implex contact if you like also to evaluate the rocking behavior

Regards

[kolozvari]

Hello,

I must apologize, but I have to ask the same question again as I still don't understand where the discrepancy is coming from.

In my model I have 240mx240m elastic soil domain, 30 meters thick soil (Vs = 200 m/s) with 0.5 meter very stiff rock layer at the base (Vs = 5000 m/s) - model is attached. When I apply the harmonic motion of 3Hz with amplitude of 1.0 m/s2 (I input the velocity in the AB element), what soil is actually seeing at the base layer is acceleration of amplitude of 2.0 m/s2 (see figure below - figure also gives the parameters of the rock layer also used in AB elements). I am pretty sure I converted acceleration to velocity correctly and that my input parameters are correct, and I still can't figure out why is my acceleration at the base of the soil not the one that corresponds to input velocity.

Can you please let me know your thoughts? I would really appreciate if we can get to the bottom of this.

Thank you,

[STKO Team]

It makes sense because you are measuring the acceleration at the interface between the bedrock and the soil.
When the wave passes the interface between 2 different materials, it gets amplified, and part of it reflected back.
Keep in mind that at the free surface (E = 0) you will see an amplification of 2.

So ideally you should see:
1 at the base of the bedrock
almost 2 at the interface between the bedrock and the soil (because the soil stiffness is negligible wrt the bedrock stiffness)
4 st the top free surface

Of course, you won't see exactly those values for some reasons:

• The bedrock layer is too thin, even smaller than the wavelength of your input. So while the wave is still entering, it already got reflected from the bedrock-soil interface. So you will see almost the identical response (2) also at the base of the bedrock
• You are using multiple waves, so the input gets added to the waves coming back. It's hard to do a benchmark in this way.
• You have damping.

If you want to understand how it works in the case of 2 layers (bedrock and soil), you should use a simple wavelet (so you have only 3 waves coming in, and when they will come back there are no other waves, so it's easy to read).

Also, you have to make sure that each layer is larger than the wavelength of your input.

As an example, download the files from webinar #24
Implicit-Explicit Contact Element Applied Examples: soil-foundation interaction and RC structures
use the file in webinar_contact_implex_14_10_2021\absorbing\T05_abs_3d_2_layers

You should see an output like this (as you can see the base is exactly 1g amplitude of ricker wavelet as per input, and at the interface and at the top you can see amplifications)

multilayer.png (61.03 KiB) Viewed 1699 times

[kolozvari]

Hello, I am doing SSI analysis of a tall building. I applied the ground motion in the SSI model by first converting the record acceleration to velocity and then divided by 2.0 to get the correct input (we discussed this before). I was plotting acceleration response at the bottom of the soil domain and compared them to the original input (see below). As you can see, the spectral response matches pretty well for periods larger than 1.5 seconds. However, for periods smaller than 1.0 seconds, it seems that the spectral acceleration response at the bottom of the soil domain (top of the absorbing boundary) is reduced by approximately 30%. It seems like something in the model "damps out" the higher frequencies of the ground motion.

At first I suspected that my mesh is too large, so I tried mesh size sensitivity (you can see the current mesh in the screenshot) and it didnt make much of a difference. However, I am still not sure if I should be trying even smaller mesh and if there is any recommendations about the mesh size, if the mesh is the issue at the first place.

I was wondering if you can provide me with your insight into this issue and an advice on how to resolve it. Is there anything else that I should be trying besides the mesh size?

Looking forward to hearing from you. Thank you.

[STKO Team]

At first I suspected that my mesh is too large, so I tried mesh size sensitivity (you can see the current mesh in the screenshot) and it didnt make much of a difference. However, I am still not sure if I should be trying even smaller mesh and if there is any recommendations about the mesh size, if the mesh is the issue at the first place.

The mesh can be one of the reasons.
Of course, you cannot expect to capture extremely high frequencies well, due to the constraint on the mesh size:
critical mesh size <= max_wave_length / 8 (or 10).
That is: critical mesh size <= Vs/fmax/8 (it means: at least 8 elements per wave-length)

If you are sure about the above-mentioned constraint, check what else can damp those higher-frequencies:
are you using rayleigh damping?
are you using a transient integrator with numerical damping?