[IHFOAM] The IHFOAM Thread

IHFOAM Team · December 19, 2018, 04:00

Hi Ramsay,

Quote:

Originally Posted by Ramsay

Does anyone have any recommendation on how to get the free surface elevation of solitary waves in OpenFOAM 1806.

If you want to place some free surface gauges, please, look at the tutorials, for example ~/tutorials/multiphase/interFoam/laminar/waveExampleSolitary, and check the /system/controlDict:

Code:

functions
{
    line
    {
        type            sets;
        libs            ("libsampling.so");
        enabled         true;
        writeControl    writeTime;
        writeInterval   1;

        interpolationScheme cellPoint;
        setFormat       raw;
        sets
        (
            line1
            {
                type    uniform;
                axis    distance;
                start   ( 1.0 0.01 0.0 );
                end     ( 1.0 0.01 1.5 );
                nPoints 1001;
            }
            line2
            {
                type    uniform;
                axis    distance;
                start   ( 2.0 0.01 0.0 );
                end     ( 2.0 0.01 1.5 );
                nPoints 1001;
            }
            line3
            {
                type    uniform;
                axis    distance;
                start   ( 3.0 0.01 0.0 );
                end     ( 3.0 0.01 1.5 );
                nPoints 1001;
            }
            line4
            {
                type    uniform;
                axis    distance;
                start   ( 5.0 0.01 0.0 );
                end     ( 5.0 0.01 1.5 );
                nPoints 1001;
            }
            line5
            {
                type    uniform;
                axis    distance;
                start   ( 7.5 0.01 0.0 );
                end     ( 7.5 0.01 1.5 );
                nPoints 1001;
            }

            line6
            {
                type    uniform;
                axis    distance;
                start   ( 9.0 0.01 0.0 );
                end     ( 9.0 0.01 1.5 );
                nPoints 1001;
            }
        );

        fixedLocations  false;
        fields
        (
            U alpha.water
        );
    }
}

If you want to get and stl file with the whole free surface elevation, please add to your system/controlDict:

Code:

functions
{
    freeSurface
    {
        type surfaces;
        functionObjectLibs
        (
            "libsampling.so"
        );
        writeControl outputTime;
        outputInterval 1;
        surfaceFormat stl;
        interpolationScheme cellPoint;
        surfaces
        (
            topFreeSurface
            {
                type isoSurface;
                isoField alpha.water;
                isoValue 0.5;
                interpolate true;
            }
        );
        fields
        (
            alpha.water
        );
    }
}

Regards,
IHFOAM Team

Ramsay · December 21, 2018, 01:04

Thanks for your help.

I am also using your first method as:

Code:

functions
{
  line
      {
          type            sets;
          libs            ("libsampling.so");
          enabled         true;
          writeControl    writeTime;
          writeInterval   1;

          interpolationScheme cellPoint;
          setFormat       raw;
          sets
          (
            line1
            {
              type    uniform;
              axis    distance;
              start   ( 1.0 0.01 0.0 );
              end     ( 1.0 0.01 2.4 );
              nPoints 2401;
            }
            line2
            {
              type    uniform;
              axis    distance;
              start   ( 100.0 0.01 0.0 );
              end     ( 100.0 0.01 2.4 );
              nPoints 2401;
            }
          );

          fixedLocations  false;
          fields
          (
            alpha.water
          );
      }
}

with write times equal to 0.05 s and then I use the following matlab code to get the free surface elevation.

Code:

clear;
clc;
k=0;
end_time=20; %s
for i=0.05:0.05:end_time
    k=k+1;
    folderName_Up='/Users/line/';
    folderName=num2str(i);
    fileName_1=[folderName_Up folderName '/line1_alpha.water.xy'];
    fileName_2=[folderName_Up folderName '/line2_alpha.water.xy'];
    load(fileName_1);
    load(fileName_2);
    y=line1_alpha_water(:,1);
    alpha_1=line1_alpha_water(:,2);
    alpha_2=line2_alpha_water(:,2);
    [alpha_1, index_1]=unique(alpha_1);
    [alpha_2, index_2]=unique(alpha_2);
    y_profile_1(k,1)=interp1(alpha_1,y(index_1),0.5);
    y_profile_2(k,1)=interp1(alpha_2,y(index_2),0.5);
    time_matrix(k,1)=i;
end

However, this is for a smooth free surface. I am wondering what should we do if the surface is turbulent and there are some water particles in the air so that this method may not work since we may have alpha.water=0.5 in more than one place along the line.

Ramsay · February 21, 2019, 23:09

Hi, I am trying to create a model with 2 concurrent wave types (e.g. solitary and stokes I or II) as well as a current with a specified speed. Does anybody know how I can set two wave models in constant/waveProperties? I tried many ways but not successful :/.

thanks

IHFOAM Team · February 22, 2019, 03:52

Hi Ramsay,

Quote:

Originally Posted by Ramsay

Does anybody know how I can set two wave models in constant/waveProperties? I tried many ways but not successful :/.
thanks

You can not generate a mix of two theories in the same patch. And the generation of both wave and current has not been released yet.
(sorry for the bad news ...)

Regards,
IHFOAM Team

romainping · March 4, 2019, 10:27

Hi,
I am trying to use the IHFoam wave generation/absorption model to generate regular waves in deep water (H=4m, T=12s, h=180m).
I use OF v1712. However I see some reflection at the outlet where I defined a shallowWaterAbsorption condition.
Have you developed an absorption condition for deep water waves ?
Thanks for the help.

Best Regards,

Romain

IHFOAM Team · March 5, 2019, 05:10

Hi Romain,

Quote:

Have you developed an absorption condition for deep water waves ?

Yes, we have indeed, but we are not planning to make a public release yet.

Right now, we are working in several topics (all related) and the idea is to make a major release in the near future.

Best Regards,
IHFOAM TEAM.

Ramsay · March 20, 2019, 10:33

Hi,

Would you please write a post upon the structure of your codes? For example how does the model get the wave height and wave period from /constants/waveproperties and uses that in wave generation models and so. I am trying to expand your models, adding new features, but the structure of the codes are very interconnected and complicated.

Thanks

IHFOAM Team · March 20, 2019, 13:14

Hi Ramsay,

Please, open any of the wave types that have been already released (stokesI for example, and look into the code. In: ~/OpenFOAM/OpenFOAM-v1812/src/waveModels/waveGenerationModels/derived), open StokesIWaveModel.C.

Then, open as well waveModel.C (in ~/OpenFOAM/OpenFOAM-v1812/src/waveModels).

You should be able to understand how everything works, as the names of the classes and methods are very self-explanatory.

Best Regards,
IHFOAM Team.

cresendo · May 1, 2019, 21:46

Hi,
I am studying the case "wavestokes" in v1806.But i cant find any clear explanations about "ramptTime".
Can u help with that?

Best
Chen

IHFOAM Team · May 2, 2019, 08:20

Hi Chen,

The rampTime defined in the waveProperties dictionary is a parameter needed damp the first waves in the beginning of the simulation (as it is normally done in the laboratory).
As a general rule that might not always work, I recommend you to set it to twice the period (T).

Best Regards,
IHFOAM Team.

cresendo · May 2, 2019, 10:06

Hi,
Thanks for ur reply! And recently I am trying to achieve the motion using oversetmesh in wave case.But it seems that i met some problems.So I want to ask if it can be done in v1812?

best
Chen

IHFOAM Team · May 2, 2019, 12:16

Hi Chen,

Quote:

Originally Posted by cresendo

.So I want to ask if it can be done in v1812?

Yes, it can be done very easily.

Actually, we will be given a short course in the 3rd Iberian meeting of OpenFOAM® technology users (1 & 12 June, 2019 Porto - Portugal) about that:
https://foam-iberia.eu/files/barajasgCourse.pdf

Regards,
IHFOAM Team.

Ramsay · May 30, 2019, 11:53

Hi IHFOAM,

Thanks for your reply to my previous posts. I had a question about the outlet boundary condition for velocity.

HTML Code:

    inlet
    {
        type            waveVelocity;
        value           uniform (0 0 0);
    }

    outlet
    {
        type            waveVelocity;
        value           uniform (0 0 0);
    }

My question is that while we know the velocity at the inlet, we do not have a clue about the velocity at the outlet. Is this velocity related to the wave absorption at the outlet?

Moreover in your paper "Realistic wave generation and active wave absorption for Navier–Stokes models Application to OpenFOAM" you have mentioned that "This is to choose a number of paddles (user-defined vertical slices of patch, which resemble the individual paddles of a wavemaker) near the edges only capable of extracting water according to Eq. (11). " Could you please expand a little bit more on this and explain how can we choose the right number of paddles?

Thanks

Ramsay · June 4, 2019, 18:11

Hi IHFOAM,

I had a question about the stream function wave model:

I have modeled a stream function wave with the following input data:

T=4s, H=1m, L=8.21, h=0.4m, and the following coefficients

Ej Bj
0.049691442881364 0.036310005909239
0.014968548105525 0.021538513895102
0.005002182491150 0.010791628806089
0.001677417735919 0.005029455790592
0.000547097964529 0.002287538909920
0.000169170370929 0.001040624806039
0.000047948729438 0.000481608940598
0.000011605596599 0.000233336356172
0.000001854392051 0.000129217434153
0.000000025910920 0.000050382974278

This wave model falls within the Cnoidal wave model. I used these numbers for an analytic as well as a numerical stream function wave model. Moreover, I also did a numerical Cnoidal wave model analysis and compared these three results as shown below.

https://ibb.co/jG8Qd8B

While there is a good match between the analytic stream function and numerical cnoidal wave models, the numerical stream function wave model has a phase shift. I have the same problem with the other configurations, as well. I was wondering if you could help me with this issue. I appreciate your help and recommendations on this.

IHFOAM Team · June 18, 2019, 12:30

Quote:

Could you please expand a little bit more on this and explain how can we choose the right number of paddles?

Please, take a look to the work of Schaffer and Kllopman (2000).

https://ascelibrary.org/doi/10.1061/...26%3A2%2888%29

You must divide your patch into wave paddles of same width to have better results, but there are numerical limitations. Please, take into a account, that if you increase the number of wave paddles you increase the computational time too.

Best Regards,
IHFOAM Team

IHFOAM Team · June 18, 2019, 12:32

Quote:

Actually, we will be given a short course in the 3rd Iberian meeting of OpenFOAM® technology users (1 & 12 June, 2019 Porto - Portugal) .

You can find all the documents about the course (and much more) in the IHFOAM web page:
http://ihfoam.ihcantabria.com/source-code/tutorials/

Best Regards,
IHFOAM Team

IHFOAM Team · June 18, 2019, 12:42

Quote:

This wave model falls within the Cnoidal wave model.

Hi Ramsay,

Please use any of the theories under its correct range of application. There is no point in using the stream function wave theory when you should be using the cnoidal wave theory (as you have shown in your results)

Please, check as well your wave parameters: (T=4s, H=1m, L=8.21, h=0.4m), they do not seem to be correct.

Best Regards,
IHFOAM Team.

Ramsay · June 18, 2019, 15:16

Quote:

Originally Posted by IHFOAM Team

Hi Ramsay,

Please use any of the theories under its correct range of application. There is no point in using the stream function wave theory when you should be using the cnoidal wave theory (as you have shown in your results)

Please, check as well your wave parameters: (T=4s, H=1m, L=8.21, h=0.4m), they do not seem to be correct.

Best Regards,
IHFOAM Team.

Hi IHFOAM,

Your response is highly appreciated.
Actually that is a typo and wave should be (T=4s, h=0.4m, L=8.21, H=0.1m).

Thanks

ChiaraViola · June 25, 2019, 09:39

Hi IHFOAM.
I'm new to openfoam and I would to like to learn to use it for coastal engineering problem. I tried to start directly with the ihfoam GUI but without any background knowledge of openfoam it was impossible to me because I wasn't able to understand my mistakes.
So now I'm working on interfoam and i'm trying to add a dike to the tutorial of StokesV. My wish is to simulate irregular waves but for the moment I want to start with easy things and update my case step by step.
I hope to be in the right part of the forum since I have a lot of problem about running interfoam (I also tried to use Stokes I theory), if not I'm really sorry.
My simulation problem is try to generate regular waves propagating toward an impermeable dike with a promenade and a storm wall and I would like to have information about the water level in some points and see if I will have overtopping. My geometry is scaled according to a wave flume experiment and my aim is reproduce it.
I added the geometry with snappyHexMesh and I had problems with the 2D nature so I had to modify the BCs of the lateral faces (front and back) from the tutorial (empty) and extend my obstacle over the boundaries of the blockMesh.

condition for U

Code:

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


internalField   uniform (0 0 0);

boundaryField
{
    inlet
    {
        type            waveVelocity;
        value           uniform (0 0 0);
    }
    outlet
    {
        type            waveVelocity;
        value           uniform (0 0 0);
    }
    ground
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    top
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }
    front
    {
        type            slip;
    }
    back
    {
        type            slip;
    }
    section_B2
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
}

condition for p_rgh

Code:

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

internalField   uniform 0;

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

    outlet
    {
        type            fixedFluxPressure;
        value           uniform 0;
    }

    ground
    {
        type            fixedFluxPressure;
        value           uniform 0;
    }

    front
    {
        type            fixedFluxPressure;
	value           uniform 0;
    }

    back
    {
        type            fixedFluxPressure;
	value           uniform 0;
    }

    top
    {
        type            totalPressure;
        p0              uniform 0;
    }

section_B2
    {
        type            fixedFluxPressure;
        value           uniform 0;
    }

}

condition for alpha.water

Code:

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    inlet
    {
        type            waveAlpha;
        value           uniform 0;
    }

    outlet
    {
        type            zeroGradient;
    }

    ground
    {
        type            zeroGradient;
    }

    front
    {
        type           zeroGradient;
    }

    back
    {
        type            zeroGradient;
    }

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

section_B2
{
        type            zeroGradient;
    }

}

When I run interFoam my problem is that the Courant number after few days of simulation blows up at e+135 (like also the cumulative error) and deltaT becomes very small (e-146).

last steps of log file:

Code:

PIMPLE: iteration 1
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144586  Min(alpha.water) = -5.35741e-06  Max(alpha.water) = 1.05469
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144586  Min(alpha.water) = -1.40226e-08  Max(alpha.water) = 1.05467
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144585  Min(alpha.water) = -1.27883e-08  Max(alpha.water) = 1.05464
Updating StokesV wave model for patch inlet
Updating shallowWaterAbsorption wave model for patch outlet
DICPCG:  Solving for p_rgh, Initial residual = 0.0110179, Final residual = 0.000120469, No Iterations 5
DICPCG:  Solving for p_rgh, Initial residual = 0.000120677, Final residual = 1.15472e-05, No Iterations 15
time step continuity errors : sum local = 2.8992e-06, global = 2.1739e-09, cumulative = 0.000126839
DICPCG:  Solving for p_rgh, Initial residual = 1.22061e-05, Final residual = 1.16741e-06, No Iterations 43
DICPCG:  Solving for p_rgh, Initial residual = 1.1674e-06, Final residual = 8.35719e-07, No Iterations 5
time step continuity errors : sum local = 2.0981e-07, global = 2.58869e-09, cumulative = 0.000126842
DICPCG:  Solving for p_rgh, Initial residual = 1.02409e-06, Final residual = 4.87693e-07, No Iterations 5
GAMG:  Solving for p_rgh, Initial residual = 4.87693e-07, Final residual = 5.78942e-09, No Iterations 5
time step continuity errors : sum local = 1.45345e-09, global = -2.36671e-10, cumulative = 0.000126841
PIMPLE: iteration 2
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144586  Min(alpha.water) = -0.00138511  Max(alpha.water) = 1.05469
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144586  Min(alpha.water) = -0.00131392  Max(alpha.water) = 1.05466
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144585  Min(alpha.water) = -0.00124639  Max(alpha.water) = 1.05463
Updating StokesV wave model for patch inlet
DICPCG:  Solving for p_rgh, Initial residual = 0.000291126, Final residual = 2.79373e-06, No Iterations 5
DICPCG:  Solving for p_rgh, Initial residual = 2.79331e-06, Final residual = 7.36053e-07, No Iterations 5
time step continuity errors : sum local = 1.84598e-07, global = -3.46771e-10, cumulative = 0.000126841
DICPCG:  Solving for p_rgh, Initial residual = 9.25743e-07, Final residual = 4.5891e-07, No Iterations 5
DICPCG:  Solving for p_rgh, Initial residual = 4.5891e-07, Final residual = 3.24245e-07, No Iterations 5
time step continuity errors : sum local = 8.13187e-08, global = -5.43872e-10, cumulative = 0.000126841
DICPCG:  Solving for p_rgh, Initial residual = 3.32579e-07, Final residual = 1.97878e-07, No Iterations 5
GAMG:  Solving for p_rgh, Initial residual = 1.97878e-07, Final residual = 1.17233e-09, No Iterations 5
time step continuity errors : sum local = 2.94013e-10, global = -1.04298e-10, cumulative = 0.00012684
PIMPLE: converged in 2 iterations
ExecutionTime = 92080.4 s  ClockTime = 92127 s

Courant Number mean: 0.0062403 max: 0.504923
Interface Courant Number mean: 0.000302312 max: 0.403648
deltaT = 0.000915501
Time = 12.13

PIMPLE: iteration 1
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144585  Min(alpha.water) = -6.22537e-06  Max(alpha.water) = 1.0546
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144585  Min(alpha.water) = -4.22846e-08  Max(alpha.water) = 1.05458
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144584  Min(alpha.water) = -3.80532e-08  Max(alpha.water) = 1.05455
Updating StokesV wave model for patch inlet
Updating shallowWaterAbsorption wave model for patch outlet
DICPCG:  Solving for p_rgh, Initial residual = 0.0109772, Final residual = 0.000120993, No Iterations 5
DICPCG:  Solving for p_rgh, Initial residual = 0.000121207, Final residual = 1.09356e-05, No Iterations 15
time step continuity errors : sum local = 2.74231e-06, global = 2.31784e-09, cumulative = 0.000126843
DICPCG:  Solving for p_rgh, Initial residual = 1.16013e-05, Final residual = 1.15908e-06, No Iterations 43
DICPCG:  Solving for p_rgh, Initial residual = 1.15907e-06, Final residual = 8.5041e-07, No Iterations 5
time step continuity errors : sum local = 2.13239e-07, global = 2.77346e-09, cumulative = 0.000126846
DICPCG:  Solving for p_rgh, Initial residual = 1.02343e-06, Final residual = 4.93126e-07, No Iterations 5
GAMG:  Solving for p_rgh, Initial residual = 4.93126e-07, Final residual = 5.70577e-09, No Iterations 5
time step continuity errors : sum local = 1.43071e-09, global = -2.31627e-10, cumulative = 0.000126845
PIMPLE: iteration 2
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144585  Min(alpha.water) = -0.0017968  Max(alpha.water) = 1.0546
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144585  Min(alpha.water) = -0.00170086  Max(alpha.water) = 1.05457
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144584  Min(alpha.water) = -0.00161004  Max(alpha.water) = 1.05453
Updating StokesV wave model for patch inlet
DICPCG:  Solving for p_rgh, Initial residual = 0.000323175, Final residual = 9.54125e-06, No Iterations 9
DICPCG:  Solving for p_rgh, Initial residual = 9.53947e-06, Final residual = 9.32001e-07, No Iterations 16
time step continuity errors : sum local = 2.33577e-07, global = -3.29532e-10, cumulative = 0.000126845
DICPCG:  Solving for p_rgh, Initial residual = 1.09139e-06, Final residual = 4.62161e-07, No Iterations 5
DICPCG:  Solving for p_rgh, Initial residual = 4.62161e-07, Final residual = 6.44307e-07, No Iterations 5
time step continuity errors : sum local = 1.61475e-07, global = -3.33242e-10, cumulative = 0.000126845
DICPCG:  Solving for p_rgh, Initial residual = 6.60649e-07, Final residual = 3.59502e-07, No Iterations 5
GAMG:  Solving for p_rgh, Initial residual = 3.59503e-07, Final residual = 1.07345e+136, No Iterations 50
time step continuity errors : sum local = 2.69028e+135, global = -6.34714e+124, cumulative = -6.34714e+124
PIMPLE: converged in 2 iterations
ExecutionTime = 92110.6 s  ClockTime = 92157 s

Courant Number mean: 4.56044e+135 max: 9.79846e+141
Interface Courant Number mean: 3.28203e+134 max: 1.47078e+141
deltaT = 4.67165e-146
Time = 12.13

PIMPLE: iteration 1
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144584  Min(alpha.water) = -0.000136131  Max(alpha.water) = 1.05453
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144584  Min(alpha.water) = -4.49755e-06  Max(alpha.water) = 1.05453
Updating StokesV wave model for patch inlet
MULES: Solving for alpha.water
Phase-1 volume fraction = 0.144584  Min(alpha.water) = -4.47453e-06  Max(alpha.water) = 1.05453
Updating StokesV wave model for patch inlet
Updating shallowWaterAbsorption wave model for patch outlet

And I also have this error:

Code:

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigFpe::sigHandler(int) at ??:?
#2  ? in /lib/x86_64-linux-gnu/libc.so.6
#3  double Foam::sumProd<double>(Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
#4  Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#5  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) at ??:?
#6  Foam::fvMatrix<double>::solveSegregatedOrCoupled(Foam::dictionary const&) at ??:?
#7  Foam::fvMesh::solve(Foam::fvMatrix<double>&, Foam::dictionary const&) const at ??:?
#8  ? in ~/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/bin/interFoam
#9  __libc_start_main in /lib/x86_64-linux-gnu/libc.so.6
#10  ? in ~/OpenFOAM/OpenFOAM-v1812/platforms/linux64GccDPInt32Opt/bin/interFoam

I searched on the forum and if I understood well is related to wrong boundary conditions or mathematical problem, but from the checkMesh everything seemed OK.

Can someone please help me and say what is my mistake? How I can add my dike to the interfoam tutorial and finish my run without errors, so I can start facing to irregular waves simulation?
I have no idea why I have a lot of problems with this geometry in SHM and with the boundary conditions, if someone can explain me what is wrong and give me a clue would be helpful and very appreciated.

Best regards,
Chiara

I also provide some files in order to give more information for a really wished help

IHFOAM Team · July 1, 2019, 05:12

Hi Chiara,

Quote:

I also provide some files in order to give more information for a really wished help

Can you add a snapshot of the last time step simulated?

Best Regards,
IHFOAM Team

February 21, 2019, 23:09	two concurrent waves and a current	#263
Ramsay New Member Join Date: Oct 2018 Posts: 17 Rep Power: 8	Hi, I am trying to create a model with 2 concurrent wave types (e.g. solitary and stokes I or II) as well as a current with a specified speed. Does anybody know how I can set two wave models in constant/waveProperties? I tried many ways but not successful :/. thanks

March 4, 2019, 10:27	Deep Water waves	#265
romainping New Member Romain Ping Join Date: Feb 2019 Posts: 3 Rep Power: 7	Hi, I am trying to use the IHFoam wave generation/absorption model to generate regular waves in deep water (H=4m, T=12s, h=180m). I use OF v1712. However I see some reflection at the outlet where I defined a shallowWaterAbsorption condition. Have you developed an absorption condition for deep water waves ? Thanks for the help. Best Regards, Romain

March 20, 2019, 13:14		#268
IHFOAM Team Senior Member IHFOAM The Environmental Hydraulics Institute "IHCantabria" Join Date: Sep 2017 Location: Santander (Spain) Posts: 120 Rep Power: 9	Hi Ramsay, Please, open any of the wave types that have been already released (stokesI for example, and look into the code. In: ~/OpenFOAM/OpenFOAM-v1812/src/waveModels/waveGenerationModels/derived), open StokesIWaveModel.C. Then, open as well waveModel.C (in ~/OpenFOAM/OpenFOAM-v1812/src/waveModels). You should be able to understand how everything works, as the names of the classes and methods are very self-explanatory. Best Regards, IHFOAM Team. __________________ http://ihfoam.ihcantabria.com/

May 2, 2019, 08:20		#270
IHFOAM Team Senior Member IHFOAM The Environmental Hydraulics Institute "IHCantabria" Join Date: Sep 2017 Location: Santander (Spain) Posts: 120 Rep Power: 9	Hi Chen, The rampTime defined in the waveProperties dictionary is a parameter needed damp the first waves in the beginning of the simulation (as it is normally done in the laboratory). As a general rule that might not always work, I recommend you to set it to twice the period (T). Best Regards, IHFOAM Team. Richal Sun likes this. __________________ http://ihfoam.ihcantabria.com/

May 30, 2019, 11:53		#273
Ramsay New Member Join Date: Oct 2018 Posts: 17 Rep Power: 8	Hi IHFOAM, Thanks for your reply to my previous posts. I had a question about the outlet boundary condition for velocity. HTML Code: inlet { type waveVelocity; value uniform (0 0 0); } outlet { type waveVelocity; value uniform (0 0 0); } My question is that while we know the velocity at the inlet, we do not have a clue about the velocity at the outlet. Is this velocity related to the wave absorption at the outlet? Moreover in your paper "Realistic wave generation and active wave absorption for Navier–Stokes models Application to OpenFOAM" you have mentioned that "This is to choose a number of paddles (user-defined vertical slices of patch, which resemble the individual paddles of a wavemaker) near the edges only capable of extracting water according to Eq. (11). " Could you please expand a little bit more on this and explain how can we choose the right number of paddles? Thanks

March 20, 2019, 10:33		#267
Ramsay New Member Join Date: Oct 2018 Posts: 17 Rep Power: 8	Hi, Would you please write a post upon the structure of your codes? For example how does the model get the wave height and wave period from /constants/waveproperties and uses that in wave generation models and so. I am trying to expand your models, adding new features, but the structure of the codes are very interconnected and complicated. Thanks

May 1, 2019, 21:46		#269
cresendo New Member Chen Join Date: Feb 2019 Posts: 5 Rep Power: 7	Hi, I am studying the case "wavestokes" in v1806.But i cant find any clear explanations about "ramptTime". Can u help with that? Best Chen

May 2, 2019, 10:06		#271
cresendo New Member Chen Join Date: Feb 2019 Posts: 5 Rep Power: 7	Hi, Thanks for ur reply! And recently I am trying to achieve the motion using oversetmesh in wave case.But it seems that i met some problems.So I want to ask if it can be done in v1812? best Chen

June 4, 2019, 18:11		#274
Ramsay New Member Join Date: Oct 2018 Posts: 17 Rep Power: 8	Hi IHFOAM, I had a question about the stream function wave model: I have modeled a stream function wave with the following input data: T=4s, H=1m, L=8.21, h=0.4m, and the following coefficients Ej Bj 0.049691442881364 0.036310005909239 0.014968548105525 0.021538513895102 0.005002182491150 0.010791628806089 0.001677417735919 0.005029455790592 0.000547097964529 0.002287538909920 0.000169170370929 0.001040624806039 0.000047948729438 0.000481608940598 0.000011605596599 0.000233336356172 0.000001854392051 0.000129217434153 0.000000025910920 0.000050382974278 This wave model falls within the Cnoidal wave model. I used these numbers for an analytic as well as a numerical stream function wave model. Moreover, I also did a numerical Cnoidal wave model analysis and compared these three results as shown below. https://ibb.co/jG8Qd8B While there is a good match between the analytic stream function and numerical cnoidal wave models, the numerical stream function wave model has a phase shift. I have the same problem with the other configurations, as well. I was wondering if you could help me with this issue. I appreciate your help and recommendations on this. Last edited by Ramsay; June 4, 2019 at 22:10.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Divergence detected in AMG solver: k when udf loaded	google9002	Fluent UDF and Scheme Programming	3	November 8, 2019 00:34
udf problem	jane	Fluent UDF and Scheme Programming	37	February 20, 2018 05:17
UDF velocity profile	willroca	Fluent UDF and Scheme Programming	2	January 10, 2016 04:13
Error messages	atg	enGrid	7	August 30, 2013 12:16
Phase locked average in run time	panara	OpenFOAM	2	February 20, 2008 15:37