[Ramsay]

Hi IHFOAM

Thanks for the reply. I will try it with the wavemaker movement data.

[Ramsay]

Hi

I have a wave with the following properties.
H=0.5m, T=2.5s, and d=1.89m.

I want to model this with streamfunction wave model with the following parameters. I was wondering if by any chance anyone could tell me whether my coefficients and specifically, wavelength are correct or not. This wave falls in the Stokes III category.

And if streamfunction is not good for this wave, which wave model other than stokes III would be good since stokes III is not available in OF.

Bjs
****
0.181309756452899
0.008431433267874
0.000005587717729
-0.000016152089885
0.000001054838091
0.000000174554714
-0.000000003598803
-0.000000001015069
0.000000000073662
0.000000000012415

Ejs
****
0.242634915782738
0.037185250575081
0.006955801517411
0.001546277506620
0.000379793065557
0.000099277594250
0.000027099701530
0.000007680913472
0.000002389932764
0.000000645484113

waveLength
****
8.887317269175051

uMean
****
3.554926907669973

[IHFOAM Team]

Book your seat now!

It is a pleasure to announce that two new IHFOAM training courses, for beginners and advanced users, will be held in Santander (Spain) on 26 and 27 November 2019.



Detailed course information can be found here:
https://ihfoam.ihcantabria.com/training/course-datails/

Both courses will solve case studies of random wave generation, impervious and porous fixed structures, floating structures and simplified mooring systems.


Regards,
IHFOAM Team


Disclaimer: This GUI and tutorials are not approved or endorsed by the ESI Group, the producer of the OpenFOAM® software and owner of the OpenFOAM® trademark.

[minh khang]

Hello IHFOAM Team and everyone.
Do you know why there is no velocity in the simulation when I use
inlet
{
type waveVelocity;
value uniform (2 0 0);
}

outlet
{
type waveVelocity;
value uniform (2 0 0);
}
Thank you.

[IHFOAM Team]

Hi David,

Originally Posted by minh khang

Hello IHFOAM Team and everyone.
Do you know why there is no velocity in the simulation when I use
inlet
{
type waveVelocity;
....

If you check the code, you will see that the waves module it is used to generate waves, not currents nor fixed velocities.
If you want to do so, you will have to use something like:

type fixedValue;
value uniform (2 0 0);

Best Regards,
IHFOAM Team

[saeed.barzegar.v]

Hello IHFOAM Team,

I am working on a project involving generating irregular (multi) directional waves and I am following the irregularMultiDirection example on OpenFOAM-v1906. For this project I have Hs=4.5m, Tp=9s, and wave direction 45deg with +-30 variation. I was wondering if you could introduce me a code/reference to generate wave matrix (i.e. wave height as a function of wave period and direction) like the one you have in the example.

Thank you so much,
Saeed

[IHFOAM Team]

Hi Saeed,

I was wondering if you could introduce me a code/reference to generate wave matrix like the one you have in the example.

You can find some information in the release notes:
https://www.openfoam.com/releases/op...conditions.php

Multi-directional irregular waves implementation is based on the theory provided by Leo H. Holthujisen in his book: "Waves in Oceanic and Coastal Waters."

Regards,
IHFOAM Team

[goodstah]

Aloha,
Was wondering if anyone out there has successfully combined the use of a wave theory boundary condition (i.e., stokes, solitary, conoidal, etc) with dynamic mesh refinement for the free surface (dynamicRefineFvMesh) for any recent version of OpenFOAM? I've been attempting to use v1906 and v1912 along with (pls correct me if I'm wrong) IHFOAM's wave generation tools and interFoam's dynamic mesh refinement tools, and am getting thrashed. A couple observations I have found are:

• Refinement works at first, but only for 1 level of max refinement. I noticed some tutorials using dynamic refinement in combination with SHM worked, but created "protected" cell sets--I don't think that's the problem, but not sure.
• Anything greater than 1 for "maxRefinement" results in a crash
• Same model runs perfectly fine when I disable dynamic meshing (e.g., I remove the dynamicMeshDict file)
• There error/crash always seems to occur at the "Updating cnoidal wave model for patch inlet" step or similarly the "Updating cnoidal wave model for patch outlet" step
• The actual error seems to be a div by 0 issue with "[3] #3 Foam::waveModel::waterLevel() const at ??:?" suggesting to me that something funky is happening with the mesh change at the wave boundary inlet or outlet

If anyone has done it successfully or has any clues as to what might be the issue, or knows what special considerations or inclusions are necessary, I would be greatly appreciative. My case folder is attached is attached along with the log file from interFoam for (1) dynamic mesh refinement, and (2) no mesh refinement.
Mahalo nui loa

case file here:
https://www.dropbox.com/s/kmdw56f8q7...t.org.zip?dl=0

[IHFOAM Team]

Hola Christopher,

Originally Posted by goodstah

anyone out there has successfully combined the use of a wave theory boundary condition with dynamic mesh refinement for the free surface

The code is not prepared (as it has been released) for handling wave generation and dynamic mesh refinement at the same time.
I hope to have some free time in the near future to fix it.

Un saludo, y gracias a ti,
IHFOAM Team

[goodstah]

Aloha señors,
Mahalo nui loa (muchos gracias) for the reply--that's what I thought might be the case. I'll try to pick my way through to a solution, but I'm not confident I'll be able to successfully pull it off. Coding is definitely not my strongest skillset. If I do by some miracle have success, I will post the solution here... Otherwise, if you folks ever happen to engineer a solution, I would definitely be very excited to test it out.
A hui hou
Chris

Originally Posted by IHFOAM Team

Hola Christopher,



The code is not prepared (as it has been released) for handling wave generation and dynamic mesh refinement at the same time.
I hope to have some free time in the near future to fix it.

Un saludo, y gracias a ti,
IHFOAM Team

[saeed.barzegar.v]

Hello IHFOAM Team,

Thank you for your reply and great job you have been doing. I would like to report two bugs in the IFHOAM (waves) sections of OF-v1906 and OF-v1912.

First, as I understand and from my knowledge, for any directional wave generation (i.e. not perpendicular to the generation line), the number of paddles in the generation line must be greater than 1. However, in your irregularMultiDirection tutorial, nPaddle=1 which wouldn't give the proper results. I've attached an example (Case_01*) of that tutorial with an extended domain (to have a better observation of the wave propagation) and nPaddle=50. I wasn't sure about the nPaddle in the absorption boundary and any suggestion on that will be appreciated.

Second and the important one, when I wanted to have two wave generation lines (one line parallel to x axis, and the other one parallel to y axis), I noticed that my simulations got crashed even with regular waves. After trying different cases and digging up every single lines in the wave codes and my model setup, I noticed that something is wrong when I wanted to generate waves perpendicular/directional to y axis although everything was fine when it was perpendicular/directional to x axis. The piece of information on my log file (e.g. Transformation from local to global system: (-0 1 -0 -1 -0 -0 -0 -0 1)) gave me the idea that my model was generating waves going in the opposite direction (i.e. going outwards instead of coming inside the domain). This issue relies on a typo in the waveModel.C code (src/waveModels/waveModel/waveModel.C, lines 67:69). These two lines are:

// Rotation from global<->local about global origin
Rlg_ = tensor(x, y, z);
Rgl_ = Rlg_.T();

Which should be changed to below in order to fix the problem.

// Rotation from global<->local about global origin
Rgl_ = tensor(x, y, z);
Rlg_ = Rgl_.T();

I’ve attached a case (Case_02) with two generation lines for propagation of a directional wave (i.e. 30 deg) which did not work (crashed) with the original code, but worked perfectly with the modified code. Please let me know if you have any questions.

Please take care during this challenging time,
Cheers,
Saeed Barzegar

Case_01_irregularMultiDirection_Tutorial_Extended_3D.zip

Case_02.zip

Case_02.jpg

[IHFOAM Team]

Hi Saeed Barzegar,
Thank you very much for your feedback.

for any directional wave generation (i.e. not perpendicular to the generation line), the number of paddles in the generation line must be greater than 1.

Numerically you can generate just with one single wavepaddle, but if you are going to absorb at the same time, it is better to divide the domain into several wavepaddles to better absorb in each of them.

I wasn't sure about the nPaddle in the absorption boundary and any suggestion on that will be appreciated.

If you put more wavepaddles the numerical wave absorption will be better, but of course, it will take more time.

Second and the important one, when I wanted to have two wave generation lines (one line parallel to x axis, and the other one parallel to y axis), I noticed that my simulations got crashed even with regular waves.

The code (as it is in the official release) it is just prepared to generate and absorbe waves along the X axis. Modifications can be made very easily to generate or absorbe olong the Y axis.



Best Regards,
IHFOAM Team

[zivatar]

Hi everyone,

Does anybody know where could I find detailed description about the porosity handling in the IHFoam solver? I'd like to try using the solver for calculating free surface flow of non-newtonian fluids in heterogenous porous zone, and I would like to set the
a, b, and c parameters properly in the porosityDict file for my case.
Can anyone help? Everything is appreciated!

Thank You,
Tivadar

[IHFOAM Team]

Hi Tivadar,

Does anybody know where could I find detailed description about the porosity handling in the IHFoam solver?

Please, take a look to this great paper:
Modeling the Interaction of Water Waves with Porous Coastal Structures
(https://ascelibrary.org/doi/10.1061/...3-5460.0000361)

It is a review of the state of art by Professor Iñigo Losada.

Regards,
IHFOAM Team

[zivatar]

Thank You for the information,

Kind Regards,
Tivadar

[Jekke123456789]

Hi IHFOAM,

I am modelling a wave flume with a berm, I would like to do is in three steps.
1. Current only
2. Waves only
3. Combined waves and current
The basics are a rectangular blockmesh, with a stl file adde of a berm with the use of SnapyHexMesh. I have some problems in these steps, is it possible to help me?

1.
The first case with only currents, I want a current of 0.49 m/s in the water. I did that by using two inlets, the water at 0.75 m and that only water has a velocity of 0.49. (Other suggestons are welcome.)

The problem is that the water level is decreasing, this causes problems at the inlet. See figures in attachement. Here are the boundary conditions:

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{

    inlet1
    {
        type            fixedValue;
        value           uniform 1;
    }

    inlet2
    {
        type            fixedValue;
        value           uniform 0;
    }


    outlet
    {
        type            zeroGradient;
    }

    ground
    {
        type            zeroGradient;
    }

    sides
    {
        type            empty;
    }


    top
    {
        type            inletOutlet;
        inletValue      uniform 0;
        value           uniform 0;
    }
}

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1812                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    inlet1
    {
        type            fixedFluxPressure;
        value           uniform 0;
    }

    inlet2
    {
        type            fixedFluxPressure;
        value           uniform 0;
    }

    outlet
    {
        type            zeroGradient;   
       // value           uniform 0;
    }
    ground
    {
        type            fixedFluxPressure;
        value           uniform 0;
    }

    sides
    {
        type            empty;
    }

    top
    {
        type            totalPressure;
        p0              uniform 0;
    }
}
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1812                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "0";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{

    inlet1
    {
        type            fixedValue; //noslip  //waveVelocity
        value           uniform (0.49 0 0);
    }

    inlet2
    {
        type            fixedValue; //noslip  //empty
        value           uniform (0 0 0);
    }

    outlet
    {
        type            inletOutlet;
        inletValue      uniform (0 0 0);
        value           $internalField;
    }

    ground
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

    sides
    {
        type            empty;
    }


    top
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }
}

2.
The second case is waves, I want to do JONSWAP irregular waves with a specific H_s and T_p, is there any way how these could be implemented.
What are the orther possibilities for irregular waves.

3.
Is there anyway how the two can combined in one simulation using interFoam? I couldn't find any tutorial about this case.

Thanks in advance,
Jente

[goodstah]

Aloha,
Firstly, I'm hoping that everyone out there is safe and healthy, particularly you folks in Spain where I heard that the pandemic is very serious right now. Please stay safe...
Secondly, following up on previous question regarding combining automatic mesh refinement with mesh motion for a Wavemaker--I'd like to report some minimal progress. Following the instructions from Andreas Nygren at http://www.tfd.chalmers.se/~hani/kur...esentation.pdf, I was able to successfully combine the dynamicMotionSolverFvMesh and dynamicRefineFvMesh classes to create a new dynamicMotionSolverRefineFvMesh class. Using OFv1912, I was able to use their steps to compile the new dynamicMotionSolverRefineFvMesh.so library. Getting excited that it appears to work, I tried it with the Wavemaker (piston) tutorial, and no longer get the FPE from earlier. Yay. But now, after one timestep, I see a new fatal error after solving cellDisplacements:

Courant Number mean: 0.000257913 max: 0.0490584
Interface Courant Number mean: 0 max: 0
deltaT = 0.00723982
Time = 0.0131222

PIMPLE: iteration 1
Point displacement BC on patch leftwall
Displacement Paddles_leftwall => 1(0.000168196)
GAMG:  Solving for cellDisplacementx, Initial residual = 0.724213, Final residual = 2.32352e-17, No Iterations 1
GAMG:  Solving for cellDisplacementy, Initial residual = 0.989217, Final residual = 5.11691e-06, No Iterations 8
GAMG:  Solving for cellDisplacementz, Initial residual = 6.89954e-14, Final residual = 6.89954e-14, No Iterations 0
[1] [0] 
[0] 
[0] --> FOAM FATAL ERROR: 
[0] Size of newPoints 18505 does not correspond to current mesh points size 29979
[0] 
[0]     From function virtual Foam::tmp<Foam::Field<double> > Foam::polyMesh::movePoints(const pointField&)
[0]     in file meshes/polyMesh/polyMesh.C at line 1120.
[0] 
FOAM parallel run exiting
[0]

Just wanted to ask before getting lost in the code if this error looks familiar to anyone? Any insights greatly appreciated.
I can provide the case after cleaning proprietary geometry if interested.
Mahalo

Originally Posted by IHFOAM Team

Hola Christopher,



The code is not prepared (as it has been released) for handling wave generation and dynamic mesh refinement at the same time.
I hope to have some free time in the near future to fix it.

Un saludo, y gracias a ti,
IHFOAM Team

[goodstah]

Just realized I forgot to post the code, in case anyone else cares to give it a go...
Again, the original code was taken from work by Tobias Holzmann and another member QED (Combining mesh motion and refinement) where I replaced the solidBodyMotionFunction with dynamicMotionSolverFvMesh to allow the piston motion of the wavemaker.
It compiles and functions using the wave maker flume tutorial (OF v1912) but crashes after 1st timestep, with the points count error generated by polyMesh.C described above. I tinkered with it for days but no luck. Please feel free to give it a whirl...

[IHFOAM Team]

Hi Jente,

I am modelling a wave flume with a berm, I would like to do is in three steps.
1. Current only
2. Waves only
3. Combined waves and current

Yes, it can be done with OpenFOAM but we have not released it yet. We have fully validated waves, currents and currents+waves (same and opposite direction). We are using it for real projects, please send us a private email if you are interested in starting a potential collaboration.
Check this link for more info:
https://www.researchgate.net/publica...her_conditions

Regards,
IHFOAM Team

[saeed.barzegar.v]

Hi Jente,

Originally Posted by Jekke123456789

Hi IHFOAM,

I am modelling a wave flume with a berm, I would like to do is in three steps.
1. Current only
2. Waves only
3. Combined waves and current
The basics are a rectangular blockmesh, with a stl file adde of a berm with the use of SnapyHexMesh. I have some problems in these steps, is it possible to help me?

For the first step, I had a similar case (a sea current in a domain) but for a three-phase flow problem (current passing the domain interacting with gas injection at the bottom of the sea (look at attached fig1)). The problem you are having is probably because of the boundary conditions you are using. I've attached mine and you can give it a shot.


For the step two and irregular waves, you need to provide all information (H, T, phase, and direction) of all wave components in your irregular wave. You have more control over your inputs in this way comparing to using the JONSWAP shortcut and providing just Hm0 and Tp (specially the input for phase difference is important when you want to do some validation studies). You can write a small code and create those components.


For the step three, I didn't have time to do this by myself and I am still waiting for IHFOAM/OpenFOAM to make it available in their new release (really appreciate their effort and significant works). However, if you need it immediately, you can have a look at Pablo's olaFlow work (https://github.com/phicau/olaFlow/tr...rrentWaveFlume).

Hope you find this post useful and please let me know if the first step works with those boundary conditions.

Cheers,
Saeed