[jasouza1974]

Dear all,

I'm trying to understand how to set wave parameters in the new openFoam 5.0 wave tutorial.

Basically, I do not understand what is the speed parameter. Is it the wave velocity? Description talk about "mean flow speed", but I don't know what it means?

For example for a wave with the following parameters

wave length = 65.4 m
period = 7.5 s
height = 1 m

how can I set up the waveVelocity boundary condition?

left
{
type waveVelocity;
origin (0 0 0);
direction (1 0 0);
speed ????? (what should I put here?);
waves
(
Airy
{
length 65.4;
amplitude 0.5;
phase 0;
angle 0;
}
);
scale constant 1;
crossScale constant 1;
}

Thanks,

[JNSN]

Speed is an additional current, I.e. if you solve a ship sailing in waves with forward speed. In case you only want to have a wave without current, set speed to zero

[jasouza1974]

Thanks a lot.

[insane]

Hi, Jeferson
I'm trying to understand the parameters of waveVelocity recently, but a few parameters confused me a lot
1) scale table ((1200 1) (1800 0));
2) scale and crossScale(I have never seen before)
3) note that speed does not mean wave velocity how to set it
any advice would be great appreciated
thanks in advance

[Rasmusiwersen]

Originally Posted by jasouza1974

Dear all,

I'm trying to understand how to set wave parameters in the new openFoam 5.0 wave tutorial.

Basically, I do not understand what is the speed parameter. Is it the wave velocity? Description talk about "mean flow speed", but I don't know what it means?

For example for a wave with the following parameters

wave length = 65.4 m
period = 7.5 s

where is the period specified?? I can see where wave length and the amplitude. However, the period doesn't seem to be specified anywhere.

[Thepsy]

did you find an answer to define the period ?

[jasouza1974]

Actually, period can be obtained from the Dispersion Relationship. For a linear wave we have
sig^2 = g k tanh(k h)
sig = 2 Pi/T

k = 2 Pi/L
g -> gravity
L -> wave length
T -> wave period

[RiderCharles]

Originally Posted by insane

Hi, Jeferson
I'm trying to understand the parameters of waveVelocity recently, but a few parameters confused me a lot
1) scale table ((1200 1) (1800 0));
2) scale and crossScale(I have never seen before)
3) note that speed does not mean wave velocity how to set it
any advice would be great appreciated
thanks in advance

Hi，
I also encountered this problem.
Do you already know something about these parameters?
thanks for your sharing in advance。

[nasa55]

Originally Posted by RiderCharles

Hi，
I also encountered this problem.
Do you already know something about these parameters?
thanks for your sharing in advance。

scale table means between 1200m and 1800m (in x direction) the wave should be damped. In other owrds, up to 1200, the wave has scale factor 1 and at 1800, the scale factor is 0 (no wave).

[zyfsoton]

Originally Posted by nasa55

scale table means between 1200m and 1800m (in x direction) the wave should be damped. In other owrds, up to 1200, the wave has scale factor 1 and at 1800, the scale factor is 0 (no wave).

Hi, I am wondering if it is possible to set waves from one side of the domain e.g from the inlet boundary?

Currently, I am simulating the KCS model in calm water and waves using OpenFOAM v7.

Many thanks
Tony

[jasouza1974]

Hi, yes.


You can do it easily. I prefer to use the olaFlow (https://olaflow.github.io/) instead of interFoam.



olaFlow is kind of optimized to this kind of problems. Its compilation is also straight forward.

[nasa55]

Originally Posted by zyfsoton

Hi, I am wondering if it is possible to set waves from one side of the domain e.g from the inlet boundary?

Currently, I am simulating the KCS model in calm water and waves using OpenFOAM v7.

Many thanks
Tony

You can use funky SetField to define the boundary at the inlet.

[zyfsoton]

Originally Posted by jasouza1974

Hi, yes.


You can do it easily. I prefer to use the olaFlow (https://olaflow.github.io/) instead of interFoam.



olaFlow is kind of optimized to this kind of problems. Its compilation is also straight forward.

Hi Jeferson,

Many thanks for your reply. But I think I have to use interFoam because I have modified the solver based on interFoam. I have successfully run the KCS in calm water and Stokes2 wave. Now I am hoping to simulate the KCS in waves and use the final state of calm water as the initial state of wave condition. For example, I ran the calm water case for 50s and take the 50s state as the initial state of stokes2 wave condition, but it seems didn't add wave on from 50s. I attached some pictures of wave elevation contours for wave condition.

Since in calm water just use setFields while in wave condition have to use setWave, I think I have changed all controlDict file and waveProperities file. But it seems wave is not added on from 50s.

And I am confused about the scale table ((4 1) (12 0)) located in waveProperties, I am hoping to let wave just pass through the hull from the right handside of my domain, how should I do? Please let me know if you need more information from me.

Many thanks
Tony

[zyfsoton]

Originally Posted by nasa55

You can use funky SetField to define the boundary at the inlet.

Hi, many thanks for your reply. I use setFields for my hull in calm water and then change to setWaves in wave conditons. Do you have any tutorial or case to use think funky setField to define the boundary at the inlet?

Many thanks
Tony

[jasouza1974]

I've never been able to validate the solution (comparing to the analytical wave solution) of the wave tutorial. That's why I recommended the olaFlow.


About the restart. Did you change the boundary conditions at the 50s folder?

[zyfsoton]

Originally Posted by jasouza1974

I've never been able to validate the solution (comparing to the analytical wave solution) of the wave tutorial. That's why I recommended the olaFlow.


About the restart. Did you change the boundary conditions at the 50s folder?

Hi,

Yes, the 50s folder contains the information of alpha_water, U, p_rgh and etc of the final state of calm water. Also, I copied these variables of initial state of wave condition(alpha_water.orig, U.orig, p_rgj.orig and etc) into 50s folder. Then I do renumberMesh, setWaves, decomposePar and then interFoam. But it doesn't add wave on.

[jasouza1974]

It's a long time that I did not run this kind of problem, but i think you should not run setWaves again.


Another thing, did you decomposed the right time? -> "decomposePar -latestTime"

[zyfsoton]

Originally Posted by jasouza1974

It's a long time that I did not run this kind of problem, but i think you should not run setWaves again.


Another thing, did you decomposed the right time? -> "decomposePar -latestTime"

Many thanks, I will give it a try and keep you updated!

[zyfsoton]

Originally Posted by JNSN

Speed is an additional current, I.e. if you solve a ship sailing in waves with forward speed. In case you only want to have a wave without current, set speed to zero

Hi Jan,

nowadays I am simulating a ship in wave with forward speed. I am using openfoamv7 and the calculation conditions are as follows:

ship speed=1.588m/s, wave speed=2.602m/s, I modified the waveProperties file which is located at constant file as follows:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  7
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      waveProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

origin          (0 0 0);

direction       (-1 0 0);

speed           1.588; 

waves
(
    Stokes2
    {
        length      4.338;
        amplitude   0.038;
        phase       0;
        angle       0;
    }
);

UxMean          -2.602;

UMean           ($UxMean 0 0);

scale           table ((10 1) (20 0));


// ************************************************************************* //

But I am not sure whether this setup is right or not? Please correct me if I am wrong.

Many thanks for your help and best regards,
Tony

[JNSN]

Hi Tony, what do you mean with wave velocity?