basement interaction with soil

[spater]

Dear STKO team
My model simulates the interaction between the basement and the soil. I used shell unit to simulate the basement, and my model is in the attachment. The model worked fine, but when I went into post-processing to look at the results, the calculations were strange. Can you help me see what went wrong?
I am looking forward to your reply.

屏幕截图 2022-01-04 154742.png (617.78 KiB) Viewed 7217 times

[STKO Team]

There were some mistakes:

• You cannot use the Linear solver: the contact element is non-linear
• Instead of Newmark I used TRBF2, it adds some numerical damping that can be useful in case of contact
• Use some rayleigh damping
• I switched off the IMPLEX option in the contact element. The IMPLEX option improves convergence but you need smaller time steps
• After the gravity analysis I inserted a dummy dynamic analysis with very large time steps in order to relax any spurious oscillation after the gravity analysis due to contact elements

SB.zip

(675 KiB) Downloaded 2663 times

[spater]

Thank you very much!!!!!
I have two questions and one request

I switched off the IMPLEX option in the contact element. The IMPLEX option improves convergence but you need smaller time steps

• Do you mean to modify the time step here?

屏幕截图 2022-01-05 163512.png (44.87 KiB) Viewed 7201 times

• How did you define the parameters of the damping? I know the principle of Rayleigh damping, but the natural frequency of the model is not known.

屏幕截图 2022-01-05 161656.png (69.13 KiB) Viewed 7202 times

• Attached is my latest model. Every time I mesh, STKO cannot work normally, indicating that the software has no response. Can you help me find out what the problem is?

屏幕截图 2022-01-05 162514.png (745.77 KiB) Viewed 7202 times

I am looking forward to your reply. Thank you!

[STKO Team]

Do you mean to modify the time step here?

Yes

How did you define the parameters of the damping? I know the principle of Rayleigh damping, but the natural frequency of the model is not known.

In your specific file, I simply put some numbers which are somehow meaningful
If you want to be more precise you can find more information here:
https://geotechsimulation.com/2018/04/0 ... -analysis/
The first natural frequency can be estimated as:
f1 = Vs/4/H (Vs = shear wave velocity = sqrt(G/rho), and H is the hight of your soil column, 78 meters in your case)
f1 = 0.83 Hz
f2 = n*f1 (where n is the first odd integer larger than or equal to the ratio of f_input / f_1)
f_input is the main frequency of the input motion. You can compute it with the following matlab/octave script:

Code: Select all

% load velocity
vel = load('data.txt');
n = numel(vel);

% create the time vector
dt = 0.005;
time = linspace(dt, dt*n, n).';

% compute acceleration (finite differences)
acc = [0; diff(vel)./dt];

%% COMPUTE THE POWER SPECTRAL DENSITY
Nsamps = numel(acc);
fsamp = 1.0/dt;
t = (0:Nsamps-1)*dt;
% Choose FFT size and calculate spectrum
Nfft = 4096;
[Pxx,f] = pwelch(acc, gausswin(Nfft), 0.5, Nfft,fsamp);
% truncate
id = min(find(f>20))-1;
f = f(1:id);
Pxx = Pxx(1:id);
% Plot frequency spectrum
plot(f, Pxx);
ylabel('PSD');
xlabel('Frequency(Hz)');
% Get frequency estimate (spectral peak)
[~,loc] = max(Pxx);
FREQ_ESTIMATE = f(loc);
title(sprintf('Frequency estimate = %f Hz', FREQ_ESTIMATE))

f_input = 2.69 Hz
so since f_input/f1 = 3.2,
n is 5
and f2 = n*f1 = 4.16

Attached is my latest model. Every time I mesh, STKO cannot work normally, indicating that the software has no response. Can you help me find out what the problem is?

If you look at the mesh information (log) given in the STKO terminal there is a line telling you what solids could not be meshed as structured hexaedrons:

Code: Select all

Command: BuildMesh
Warning: 5 faces cannot be meshed with "structured" mesh algorithm
28994, 28996, 29001, 29261, 29263, 
Warning: 3 solids cannot be meshed with "structured" mesh algorithm
7803, 7804, 7873, 

SO I could identify them and as you can see, there are two very close vertices which make those solids not-valid for structured meshing (they have more than 4 vertical faces)
You should recreate them paying attantion to those small edges

warnin.png (162.12 KiB) Viewed 7204 times

[spater]

Thank you for replying so quickly.
I have one more question
What size should I take for my soil domain when I use the absorbing boundary?
In my model, I set the 5L、5W、78m，Where L=110m is the length of the building and W=60m is its width. If I do that, I'm going to have too many units to compute properly.
Can you give me some advice?

[STKO Team]

It's not so easy to answer as it depends on many aspects.
The X-Y size can be a multiple of the size of the building, probably 4 or 5 times...
In-depth, it depends on also on the stratigraphy that you want to capture.

[spater]

SO I could identify them and as you can see, there are two very close vertices which make those solids not-valid for structured meshing (they have more than 4 vertical faces)

3
How can you find this mistake so easy? Are there any tricks

[STKO Team]

How can you find this mistake so easy? Are there any tricks

• Read the error or warning messages. They can tell you a lot.

  Code: Select all

  Warning: 3 solids cannot be meshed with "structured" mesh algorithm
  7803, 7804, 7873,

  When a solid cannot be meshed with a structured algorithm, it means that it does not have exactly 6 faces.
  It gives you the local ID of the sub-solids of your geometry (7803, 7804, 7873 in this case)
• In the worktree, expand the node of the geometry, expand its node of solids, select the solids listed before and "select" them.
• Once they are selected you can isolate the selection (show command) or zoom to the selection or create a selection set to better understand where it is.
• Once you locate them, try to understand why they have more than 6 faces -> in this case 2 very near vertices create an extra tiny face!

check.png (58.63 KiB) Viewed 7206 times

[spater]

Dear STKO team
I modified the model, but when I calculated, there was another error.

错误1.png (39.15 KiB) Viewed 7200 times

I've been looking for a long time and I can't find any mistakes. I am very anxious to use this model now.
Can you help me fix the problem? Also, how to use this error message, I don't know where to find the problem.
I am looking forward to your reply.
Thank you very much.

[STKO Team]

The ASDAbsorbingBoundary3DAuto tries to find (Automatically) the orientation of the boundary faces. Sometimes it happens that it cannot find the correct orientation of some elements which are very distorted (though we are working on it).
In your case the distorted elements are those at the base of the soil domain coming from the diagonal cuts around the piles.

You can still make it work now with the standard ASDAbsorbingBoundary3D element. You can refere to our first webinar on Absorbing boundaries to know how to use it.

IN the meantime we will improve the "Auto" version for distorted elements