[ngj]

Hi Niall

It is possible to add a constant wind velocity in the air in the relaxation zones. Others using waves2Foam have tried this, however, I am unaware of their results.

Please consult the wiki, section 5.

Kind regards,

Niels

[mf.]

Hi Nils,

after a few days of interrupt using OpenFOAM now my waveTheory is running. I am using the OpenFOAM version 2.1 so I had to modify the interFoam solver on my own to get wave2Foam as it's discribed on your wiki. During this the variable DOFVERSION was to set by hand in the Make/options file of the solver. To compile a new waveTheory I had to do this again for the Make/options file of the waveTheories but I didn't. What a bad mistake.

Thank you again for helping me to localize my problem.
Marco

[ngj]

Good morning Marco,

I am a bit puzzled with your post (but congrats that it is now working):

1. waveFoam for 2.1 is supported directly without your need to do anything. I tried to compile it on my own 2.1. distribution, and everything went smoothly. If you do not have the directory waves2Foam/applications/solvers/solvers210, then you should do an update from svn.

2. I do not understand what you mean about setting OFVERSION for waveTheories. If you execute the Allwmake script in either waves2Foam or waves2Foam/src, then the OFVERSION is set automatically; thus no need to manual editing.

Kind regards,

Niels

[Sagun]

Hello Niels,

I hope you are doing well. If you might recall my previous posts, I asked you about the possibility of simulating waves in 3D around an offshore structure. To that you replied that it is indeed possible to do so and that your colleagues run such simulations on a regular basis. Now I have been trying to do the same thing for the past one week but the simulations are taking A LOT of time. I wanted to ask you if this is something normal or do I need to make any changes to my case files. My mesh has a total number of 125,526 points and I'm using a time step of 0.01s for an end time equal to 10s. I'm running these simulations on a Intel i5 Quad-Core 3.20 GHz machine with 4 GB RAM.

Thanks,
Sagun

[ngj]

Well, it sounds like a small problem with merely a 1000 time steps (are you sure it stays there this large?) Furthermore, the mesh sounds like a small of the kind, so I would not be scared at all. For 2D problems some hundred thousands are not uncommon for my simulations.

Kind regards,

Niels

[Sagun]

Well, it has been almost 4 hours now since I started the last simulation and it has only reached 1.16s as of right now. This is the kind of processing speed that I am having to face.

[ngj]

That sounds uncommonly slow, but it is hard to say anymore with such limited information.
A colleagues of mine has been running entire irregular sea-states (3 hours), and I have not heard him complain.

/Niels

[Sagun]

Any other information I can provide which can help you suggest something?

[ngj]

The full - ready to run - test case would be a nice start.

/ Niels

[Sagun]

These are my entire case files:

http://www.4shared.com/archive/XbKTs...Objecttar.html

I would be extremely grateful if you could take a look and suggest something.

Regards,
Sagun

[ngj]

Is it correct that I need to create an account to download the files? If yes, please find another way to send the files.

/ Niels

[Sagun]

Ohh I didn't know that. I realized that the file size is only 3.7 MB. So may be I can simply mail it to you?

[nima3906m]

Originally Posted by dahicke

Hi all,

I have been playing with the wave solvers for a while and am running into a problem with a dynamic mesh version using 2.1.x, though I don't think it is version related. I have a 3D wave flume that appears to work OK without floating object (a box). However, when I add the box in one case with the mass calculated to the submerged section, it slowly picks up velocity and sinks reaching over -60 m/sec. In the other case with weight less than calculated, it starts to rise until it reaches an upward velocity of over 60 m/sec. Both of these reach local high velocities that case the Courant number is over 1 and the case crashes.

I have tried turning on momentum prediction, increasing nCorrectors to 3 and nNonOrthogonalCorrectors to 2, which did not seem to change this run away z velocity.

With this new version I had to add a definition for div((muEff*dev(T(grad(U))))) which I set to Gauss linear;

Has anyone encountered this kind of velocity run away?

Dave Hickerson

Hi Dave

I just saw your thread today , was wondering if you have solved your problem or not? I have been struggling to find a solution for long time

Regards
Nima

[ngj]

Good morning Sagun,

You can find my contact on http://www.dtu.dk/Service/Telefonbog.aspx

Kind regards,

Niels

[Sagun]

Good afternoon Niels,

Please follow this link. And you don't need to create an account on this one.

https://www.yousendit.com/download/W...NEhTRTcwZXNUQw

Thanks once again,
Sagun

[ngj]

Hi Sagun

You need to use the correct wave properties. Those defined in your file are merely the standard from the waveFlume tutorial. Please run setWaveParameters. The solution you got is actually the correct one, but based on incorrect input parameters; e.g. the velocities are 200 m/s after the very first time step.

Furthermore, your wave gauges (see controlDict) are partly defined outside the computational domain - leading to segmentation fault after Time = 2 s.

Correcting your setup makes it possible to complete the simulation in the time is takes to go for a cup of coffee

Kind regards,

Niels

[Sagun]

Hello Niels,

Thank you so much for taking a look at my case files. Since there was a problem with some of the wave gauges, I removed all of them for the time being. I kept the wave parameters same as those in the waveFlume tutorial since I just wanted to experiment with simple Airy wave theory first. On running setWaveParameters, the simulation does end in about 10 mins but when I try to visualize the flow in paraView there is no flow at all. There seems to be some problem with the generation of waves at the inlet. I have looked hard at the waveProperties file of the 3Dwaves tutorial but I don't seem to be able to understand what I'm doing wrong. I believe I have not understood how to assign wave parameters (esp. direction to waves and relaxation zones) properly. I have copied my waveProperties file here. I'll be grateful if you could take another look.

timeShift 0;

seaLevel 8;

relaxationNames ( inlet outlet );

initializationName outlet;

pName pd;

inletCoeffs
{
waveType stokesFirst;
depth 8;
period 2;
direction ( 1 0 0 );
phi 0;
height 0.2;
waveNumber (1.00608 0 0);
omega 3.14159;

relaxationZone
{
relaxationScheme Spatial;
relaxationShape Rectangular;
beachType Empty;
relaxType INLET;
startX ( -40 8 0 );
endX ( -20 8 3 );
orientation ( 1 0 0 );
}
}

outletCoeffs
{
waveType potentialCurrent;
U ( 0 0 0 );
Tsoft 2;

relaxationZone
{
relaxationScheme Spatial;
relaxationShape Rectangular;
beachType Empty;
relaxType OUTLET;
startX ( 20 8 0 );
endX ( 40 8 3 );
orientation ( 1 0 0 );
}
}

Thanks,
Sagun

[ngj]

Hi Sagun

Without knowing the dimensions of your test case, it looks correct. What do you mean by no flow at all? When I ran the test with the same parameters, everything worked as it should.

1. Try to visualise the pressure field.

2. If your Courant number is not very small, then there is probably a certain flow, but you might be looking at the wrong number/data range.

3. You have a quite small wave height relative to the other spatial dimensions, so it might be hard to see.

Kind regards,

Niels

[Sagun]

Hello Niels,

Good morning. I wanted to let you know that the case finally worked. The problem was indeed with the wave height and its velocity. They were too small with respect to the other spatial dimensions. I fixed those and it worked like a charm.

Now that I have been able to generate waves around an offshore structure, could you possibly tell me how can I extract the velocity potential only on the surface of the structure? I have tried to find some info on the forums here on this topic but to no avail. It would be great if you can point me in the right direction.

Thanks for all your help.
Sagun

[ngj]

Hi Sagun,

If you want the velocity potential (irrotational), then why are you using a solution based on the Navier-Stokes equations? You already have the velocities and the pressure, wouldn't that suffice your requirements?

Kind regards,

Niels