[Mar_Vayreda]

Good afternoon!

I'm trying to run a simple case of waves in a 2D tank, running first the FNPF model and at the end of the domain running CFD (coupling). The first simulation went well, I got the REEF3D_FNPF_State and added it to the CFD folder. Then I did the DiveMESH for the CFD and got the REEF3D_HDC_INPUT. I attached a photo of paraview where you can see the simulation done by FNPF and at the end of the domain, the mesh created by the CFD.

The problem appears when I run the mpirun command for the CFD. It only runs the first iteration and this message appears:

EMERGENCY STOP -- velocities exceeding critical value N 61

Also, I saw in this forum an example where you have to add the wave generation for the second simulation (CFD). So I added dirichlet wave generation but I don't really understand it, because it should be taking as input the output of the first simulation.

If someone can help me understand why you have to add the wave generation in the second simulation and why the emergency stop appears it would be of great help. I also attached the ctrl and control files.

Thank you!!

Screenshot from 2023-02-08 15-04-05.jpg

control_cfd.txt

ctrl_cfd.txt

ctrl_fnpf.txt

control_fnpf.txt

[valgrinda]

B 99 4 doesn't work for HDC, because no wave theory input is know prior to the simulation (at least the way it is implemented now). So please use B 99 3 (which is the one to use anyway).

Another comment: you are creating standing waves with FNPF, because your waves are too steep for AWA. So best to use B 99 1 or B 99 2 for FNPF with the HDC overlap somewhat away from the beach.

And one question: for your case, why do you use HDC? Why not generate the waves directly in CFD? I think that would be easier.

[Mar_Vayreda]

Hi Hans!

Sorry for the late reply and thank you so much for your suggestions. I tried changing with B 99 3 and also adding the relaxation zone for the CFD and the numerical beach for the FNPF and it started running. The problem is that when I visualize it with paraview, I can see that the wave is badly generated (I attached a photo and ctrl and control files). Do you have any other suggestion for why this is happening?

Answer to your question: The purpose of this test, is being able to run more complex cases in the future in a faster way, so in the CFD area is where the development would be added.

ctrl_fnfp.txt

control_fnfp.txt

control_cfd.txt

ctrl_cfd.txt

MicrosoftTeams-image.jpg

[kamath]

Unless you have surface piercing structures z_max=1.0 in control.txt for FNPF.
Also ten cells in the z-direction are sufficient.

Z-grids in FNPF need to be stretched to get a good dispersion. Check this paper by Pakozdi et al

A good start (and mostly works) is:
B 103 5
B 113 2.0
B 116 1.0

Check the tutorial files for FNPF in the folder you download from github.

In control.txt for the coupled CFD simulation:
Since you use a truncated domain in B 10, you don't need to specify this with H 21-22-23.

(And this is the cause of your "bad waves". I suspect if you check the console output, you have velocities of the order 0.000x)
You also have H 31-32 where H 32 points to a non existent location. Your FNPF simulation ended at 30s whereas you ask for decomp to 60s.
Divemesh seems to handle this without throwing an error, but you should be doing for clarity's sake atleast.

In ctrl.txt for CFD, while B 98 2 works, imo it defeats the purpose of the coupling when you hold off a part of the domain for wave generation and in addition introduce a modulated wave rather than the actual output at the coupling point.
Here I would recommend B 98 3.
Set I 241 to 20 s assuming you want to start the sim at 20 s.



control-fnpf:
C 11 6
C 12 3
C 13 3
C 14 7
C 15 21
C 16 3

B 2 1000 1 10
B 10 0.0 230.0 0.0 0.2 0.0 1.0

B 103 5
B 113 2.0
B 116 1.0


M 20 2
M 10 8


control-cfd: H 10 4, H 31 20.0 H 32 30.0

ctrl-cfd: I 241 20.0

This will work.

[Mar_Vayreda]

Thankyou so much for your answer!

Your corrections did work. I only had to add a numerical beach at the end of CFD to avoid reflection.