[IHFOAM] The IHFOAM Thread

mo_na · June 8, 2016, 09:47

Hi all,

I am using ihFoam (OF3.0) to simluate a wave with the following properties:

Code:

IH Wave Generation BC 
Wave theory: StokesII 
H: 0.06 
T: 1 
h: 0.775
L: 1.55536 
Direction: 0º 
Generation in: Intermediate waters. 
Relative depth (kh): 3.13076

The mesh has 24 cells/wave height and 116/wave length.

I simulated 4 different cases:
*1* laminar case with front and backside empty
*2* turbulent case with front and backside empty
*3* turbulent case with front and backside symmetryPlane (Thats actually what I need later)
*4* exactly the same as case *3* but I adjusted maxCo and maxAlphaCo both to 0.2 in the controlDict

I am attaching some plots of the 4 cases after 5, 10, 15 and 20 seconds and also my case *4* if you wanna have a look at it. None of them looks very good and I am wondering what I did wrong. To me it looks a little bit like the waves are being reflected at the outlet.

If you have any ideas, that could help, I would be really happy!

Thank you in advance!

Cheers,
Mona

agnip · June 21, 2016, 11:56

Hi,
did you use the active absorption?
in IHwavesDict, genAbs=1?

hope to be able to help you

Agnese

Quote:

Originally Posted by mo_na

Hi all,

I am using ihFoam (OF3.0) to simluate a wave with the following properties:

Code:

IH Wave Generation BC 
Wave theory: StokesII 
H: 0.06 
T: 1 
h: 0.775
L: 1.55536 
Direction: 0º 
Generation in: Intermediate waters. 
Relative depth (kh): 3.13076

The mesh has 24 cells/wave height and 116/wave length.

I simulated 4 different cases:
*1* laminar case with front and backside empty
*2* turbulent case with front and backside empty
*3* turbulent case with front and backside symmetryPlane (Thats actually what I need later)
*4* exactly the same as case *3* but I adjusted maxCo and maxAlphaCo both to 0.2 in the controlDict

I am attaching some plots of the 4 cases after 5, 10, 15 and 20 seconds and also my case *4* if you wanna have a look at it. None of them looks very good and I am wondering what I did wrong. To me it looks a little bit like the waves are being reflected at the outlet.

If you have any ideas, that could help, I would be really happy!

Thank you in advance!

Cheers,
Mona

mo_na · June 21, 2016, 12:33

Hi Agnese,

thanks for your help!
But yes I already used the active absorption. I am not quite sure why it wasn't working but I inserted a porous zone in the end of the tank now with a quite high porosity:

Code:

// Materials: clear region, porous region
a               2(0 50);
b               2(0 1.2)  ;
c               2(0 0.34);

D50             2(1 0.01);
porosity        2(1 0.95);

And this actually helps the prevent reflection. See picture "porosity" in the attachments. Here I only did laminar simulations

Now I got back to my initial setup and added turbulence again and the waves get damped quite much along the flume. I attached another plot showing the amplitude plotted over x.coordinate after 10s, 20s and 30s compared to the analytical curve. (See picture "turbulent" )
I read before on this thread, that it might be necessary to modify the k-epsilon model to avoid this effect... Does anyone have experience with that?
Or could it be that my mesh is just not good enough or I used wrong solvers, schemes etc...
I attached my 2D turbulent case also if someone wants to have a look at it.

One more thing that I don't understand yet, is why the wavelengths don't quite match the analytical solution...

I will appreciate any suggestions!
Cheers,
Mona

agnip · June 22, 2016, 05:54

which value of epsilon did you put? I m not able to see your files (I don't know why).
but, otherwise, Now I'm working on that topic at IH Cantabria, we know there are some problem with this version and the new one will be release soon, with improved wave BC.
if you want, you can write to Javier L. Lara and ask for the new version!

Quote:

Originally Posted by mo_na

Hi Agnese,

thanks for your help!
But yes I already used the active absorption. I am not quite sure why it wasn't working but I inserted a porous zone in the end of the tank now with a quite high porosity:

Code:

// Materials: clear region, porous region
a               2(0 50);
b               2(0 1.2)  ;
c               2(0 0.34);

D50             2(1 0.01);
porosity        2(1 0.95);

And this actually helps the prevent reflection. See picture "porosity" in the attachments. Here I only did laminar simulations

Now I got back to my initial setup and added turbulence again and the waves get damped quite much along the flume. I attached another plot showing the amplitude plotted over x.coordinate after 10s, 20s and 30s compared to the analytical curve. (See picture "turbulent" )
I read before on this thread, that it might be necessary to modify the k-epsilon model to avoid this effect... Does anyone have experience with that?
Or could it be that my mesh is just not good enough or I used wrong solvers, schemes etc...
I attached my 2D turbulent case also if someone wants to have a look at it.

One more thing that I don't understand yet, is why the wavelengths don't quite match the analytical solution...

I will appreciate any suggestions!
Cheers,
Mona

mo_na · June 22, 2016, 12:13

I am just gonna attach my epsilon and k files, maybe you find something strange in there:
epsilon

Code:

dimensions      [0 2 -3 0 0 0 0];

internalField   uniform 0.00003;

boundaryField
{
    bottom
    {
        type            epsilonWallFunction;
        Cmu             0.09;
        kappa           0.41;
        E               9.8;
        value           uniform 0.00003;
    }
    outlet
    {
        type            zeroGradient;
    }
    inlet
    {
        type            fixedValue;
        value           uniform 0.00003;
    }
    atmosphere
    {
        type            inletOutlet;
        inletValue      uniform 0.00003;
        value           uniform 0.00003;
    }
    middle
    {
        type            empty;
    }
    maxY
    {
        type            empty;
    }


}

k

Code:

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

internalField   uniform 0.0001;

boundaryField
{
    bottom
    {
        type            kqRWallFunction;
        value           uniform 0.0001;
    }
    outlet
    {
        type            zeroGradient;
    }
    inlet
    {
        type            fixedValue;
        value           uniform 0.0001;
    }
    atmosphere
    {
        type            inletOutlet;
        inletValue     uniform 0.0001;
        value           uniform 0.0001;
    }
    middle
    {
        type            empty;
    }
    maxY
    {
        type            empty;
    }

}

And what do you mean with "we know that problem"? The reflection issue or the problem with reduced wave height due to the use of turbulence models?
And with the new version you mean the ihFoam solver itself?

agnip · June 23, 2016, 05:12

Good morning,

everything seems to me ok, a part the k and epsilon condition on inlet: I usually put "zeroGradient" as the outlet.

Yes, the new version of IHFOAM will be released soon!

Quote:

Originally Posted by mo_na

I am just gonna attach my epsilon and k files, maybe you find something strange in there:
epsilon

Code:

dimensions      [0 2 -3 0 0 0 0];

internalField   uniform 0.00003;

boundaryField
{
    bottom
    {
        type            epsilonWallFunction;
        Cmu             0.09;
        kappa           0.41;
        E               9.8;
        value           uniform 0.00003;
    }
    outlet
    {
        type            zeroGradient;
    }
    inlet
    {
        type            fixedValue;
        value           uniform 0.00003;
    }
    atmosphere
    {
        type            inletOutlet;
        inletValue      uniform 0.00003;
        value           uniform 0.00003;
    }
    middle
    {
        type            empty;
    }
    maxY
    {
        type            empty;
    }


}

k

Code:

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

internalField   uniform 0.0001;

boundaryField
{
    bottom
    {
        type            kqRWallFunction;
        value           uniform 0.0001;
    }
    outlet
    {
        type            zeroGradient;
    }
    inlet
    {
        type            fixedValue;
        value           uniform 0.0001;
    }
    atmosphere
    {
        type            inletOutlet;
        inletValue     uniform 0.0001;
        value           uniform 0.0001;
    }
    middle
    {
        type            empty;
    }
    maxY
    {
        type            empty;
    }

}

And what do you mean with "we know that problem"? The reflection issue or the problem with reduced wave height due to the use of turbulence models?
And with the new version you mean the ihFoam solver itself?

mo_na · June 23, 2016, 05:37

Hi Agnese,

ah yes! I changed that at some point in the past and forgot to change it back to zeroGradient. I am running it again now to check if that might have caused the problem.
Thanks for your help again!

If this doesn't help I'll try to contact Javier Lara for the new version.

mo_na · June 24, 2016, 06:53

Hi Agnese (and everyone else who has good ideas

),

I changed the inlet BC to zeroGradient but the problem with the decreasing wave height remains.
I am attaching some paraView screenshots of Ux, k and epsilon after 30s. Is it normal that k and epsilon are so high on the inlet and in the airpart above the freesurface?
Do you have any ideas how to deal with the turbulence problem?
I will also attach my fvSolution and fvSchemes and U file, maybe there is something wrong there...
Or do you think I should ask Mr. Lara for the new version? Could this fix my problem?

fvSchemes:

Code:

ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    div(rhoPhi,U)  Gauss limitedLinearV 1;
    div(U)  Gauss linear;
    div((rhoPhi|interpolate(porosity)),U)  Gauss limitedLinearV 1;
    div(rhoPhiPor,UPor)  Gauss limitedLinearV 1;
    div(rhoPhi,UPor)  Gauss limitedLinearV 1;
    div(rhoPhiPor,U)   Gauss limitedLinearV 1; 
    div(phi,alpha)  Gauss vanLeer01;
    div(phirb,alpha) Gauss interfaceCompression;
    div((muEff*dev(T(grad(U))))) Gauss linear;
    div(phi,k)      Gauss upwind;
    div(phi,epsilon) Gauss upwind;
    div((phi|interpolate(porosity)),k)      Gauss upwind;
    div((phi|interpolate(porosity)),epsilon) Gauss upwind;
    div(phi,omega) Gauss upwind;
    div((phi|interpolate(porosity)),omega) Gauss upwind;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p_rgh;
    pcorr;
    alpha.water;
}

fvSolution:

Code:

solvers
{
    "alpha.water.*"
    {
        nAlphaCorr      1;
        nAlphaSubCycles 2;
        alphaOuterCorrectors yes;
        cAlpha          1;

        MULESCorr       no;
        nLimiterIter    3;

        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-8;
        relTol          0;
    }

    pcorr
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-5;
        relTol          0;
    }

    p_rgh
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-07;
        relTol          0.05;
    }

    p_rghFinal
    {
        $p_rgh;
        relTol          0;
    }

    U
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-06;
        relTol          0;
    }

    "(U|k|epsilon)"
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-06;
        relTol          0;
    }

    "(U|k|epsilon)Final"
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-08;
        relTol          0;
    }
}

PIMPLE
{
    momentumPredictor   no;
    nOuterCorrectors    1;
    nCorrectors         3;
    nNonOrthogonalCorrectors 0;
}

relaxationFactors
{
    fields
    {
    }
    equations
    {
        ".*" 1;
    }
}

U:

Code:

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

internalField   uniform (0 0 0);

boundaryField
{
    bottom
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    inlet
    {
        type            IH_Waves_InletVelocity;
        waveDictName    IHWavesDict;
        value           uniform (0 0 0);

    }
    outlet
    {
        type            IH_3D_2DAbsorption_InletVelocity;
        absorptionDir   400;
        value           uniform (0 0 0);
    }
    atmosphere
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }
    middle
    {
        type            empty;
    }
    maxY
    {
        type            empty;
    }

}

agnip · June 24, 2016, 07:26

HI!

I was re looking at your graphs, it seems it is not a generation problem (the Ihfoam is not going to do like this, also with the old version), and you have set everything regarding the generation in the right way.

Did you check the mesh? the aspect ratio between cell sizes in x and z? the difference has to be small. you can put also less cell(in the wave height 10 are enough for example).

and about the porosity area, do you use it just to absorb? if yes, you don't need it if you use the active wave absorption.
instead if you want to use the porosity zone, be sure to put it in the right zone (in the setFieldsDict). furthermore, your porosity values are very high, so you are gonna to loose a lot of energy.

Agnese

Quote:

Originally Posted by mo_na

Hi Agnese (and everyone else who has good ideas

),

I changed the inlet BC to zeroGradient but the problem with the decreasing wave height remains.
I am attaching some paraView screenshots of Ux, k and epsilon after 30s. Is it normal that k and epsilon are so high on the inlet and in the airpart above the freesurface?
Do you have any ideas how to deal with the turbulence problem?
I will also attach my fvSolution and fvSchemes and U file, maybe there is something wrong there...
Or do you think I should ask Mr. Lara for the new version? Could this fix my problem?

fvSchemes:

Code:

ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    div(rhoPhi,U)  Gauss limitedLinearV 1;
    div(U)  Gauss linear;
    div((rhoPhi|interpolate(porosity)),U)  Gauss limitedLinearV 1;
    div(rhoPhiPor,UPor)  Gauss limitedLinearV 1;
    div(rhoPhi,UPor)  Gauss limitedLinearV 1;
    div(rhoPhiPor,U)   Gauss limitedLinearV 1; 
    div(phi,alpha)  Gauss vanLeer01;
    div(phirb,alpha) Gauss interfaceCompression;
    div((muEff*dev(T(grad(U))))) Gauss linear;
    div(phi,k)      Gauss upwind;
    div(phi,epsilon) Gauss upwind;
    div((phi|interpolate(porosity)),k)      Gauss upwind;
    div((phi|interpolate(porosity)),epsilon) Gauss upwind;
    div(phi,omega) Gauss upwind;
    div((phi|interpolate(porosity)),omega) Gauss upwind;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p_rgh;
    pcorr;
    alpha.water;
}

fvSolution:

Code:

solvers
{
    "alpha.water.*"
    {
        nAlphaCorr      1;
        nAlphaSubCycles 2;
        alphaOuterCorrectors yes;
        cAlpha          1;

        MULESCorr       no;
        nLimiterIter    3;

        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-8;
        relTol          0;
    }

    pcorr
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-5;
        relTol          0;
    }

    p_rgh
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-07;
        relTol          0.05;
    }

    p_rghFinal
    {
        $p_rgh;
        relTol          0;
    }

    U
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-06;
        relTol          0;
    }

    "(U|k|epsilon)"
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-06;
        relTol          0;
    }

    "(U|k|epsilon)Final"
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-08;
        relTol          0;
    }
}

PIMPLE
{
    momentumPredictor   no;
    nOuterCorrectors    1;
    nCorrectors         3;
    nNonOrthogonalCorrectors 0;
}

relaxationFactors
{
    fields
    {
    }
    equations
    {
        ".*" 1;
    }
}

U:

Code:

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

internalField   uniform (0 0 0);

boundaryField
{
    bottom
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    inlet
    {
        type            IH_Waves_InletVelocity;
        waveDictName    IHWavesDict;
        value           uniform (0 0 0);

    }
    outlet
    {
        type            IH_3D_2DAbsorption_InletVelocity;
        absorptionDir   400;
        value           uniform (0 0 0);
    }
    atmosphere
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }
    middle
    {
        type            empty;
    }
    maxY
    {
        type            empty;
    }

}

mo_na · June 27, 2016, 10:35

Hi Agnese,

yes I use the porous medium only to prevent reflection. It seems like the active absorption is not preventing reflection completely. Still I tried again to remove it but the results get worse.

There is three plots attached:
* turbulent2D: showing the three different cases (my original, one with no porous zone and one with no porous zone and an updated mesh) after 30s
* no_porosity: showing the surface elevation after 20, 22, 24, 26, 28 and 30s with no porous zone
*porosity: showing the surface elevation after 20, 22, 24, 26, 28 and 30s with a porous zone

Regarding the mesh i was trying to follow the suggestion of the ITTC in Practical Guidelines for Ship CFD Applications:

"Use no less than 40 grid points per wavelength on the free surface.
In irregular waves use at least 20 grid points for the shortest wave length to resolve. The number of grid points per wavelength also depends on the order of accuracy of the numerical scheme so if 40 points are required for a 3 rd /4 th order method then 80 points are required for a 2 nd order scheme to obtain the same accuracy (as provided by most commercial codes).
Use no less than 20 grid points in the vertical direction where the free surface is expected."

Now I followed your advice and tried to make only cells with an aspect ratio of 1 and less cells per wave height. I picked a number of 12 cells per wave height (0.06m) so the cells are 0.005m high and wide. Unfortunately the results got even worse.

Do you have any more ideas what I could try? Can I maybe send you my case per email?

I appreciate your help very much!
Cheers,
Mona

rcarmi · July 4, 2016, 11:42

Hi,

I am not sure how to select the proper value for the k-Eps model. I see in the tutorial of breakwater the values of k and eps are set to 0.0001 but in other tutorial to 0.1
Here is what I have set so far (I have only solid boundaries which should be equivalent to plexiglass)
epsilon
internal field uniform 0.0001
bottom => type epsilonWallFunction with value 0.0001
inlet outlet => type zeroGradient
atmosphere => type inletOutlet with value 0.0001
k
internalField uniform 0.0001
bottom => type kqRWallFunction with value 0.0001
atmostphere and inlet outlet idem previous

and the kEps coeffs are left unchanged
Cmu = 0.09
C1 = 1.44
C2 = 1.92
sigmaEps =1.3

Is there a rule for the waves?

I am interested in waves for water depth of 0.15m period 0.65s and wave height 0.035m.

Thanks for any advice!

Carmi

zanis · July 13, 2016, 07:38

Dear Pablo,

I'm a new user of IHFoam and it seems great, but when I try to solve "breakwater" after "interFoam" I face with the error as follows:

file: /home/zanis/tutorials/OF300/breakwater/0/U.boundaryField.inlet from line 26 to line 28.

From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&)
in file /home/openfoam/OpenFOAM/OpenFOAM-3.0.1/src/finiteVolume/lnInclude/fvPatchFieldNew.C at line 143.

FOAM exiting

I have checked mentioned page many times, but couldn't find what the problem is.
Could you please guide me to run it correctly?

Best regards
Zahra

eb19 · July 27, 2016, 12:47

Hi Hossein,

Did you manage to simulate waves with turbulence being included in your numerical domain? I am currently facing a similar problem. With the turbulence modeling being implemented, the wave amplitudes experience reduction in time.

Could you please share your suggestion or anyone who has experience? Thanks.

Cheers
Bangun

Quote:

Originally Posted by HosseinB

Hi Pablo,

May you please further explain what numerics could be adjusted to more realistically model the waves? I am experiencing damping of waves with time and location.

What fvSchemes do you recommend for steep waves?

Cheers,
Hossein

HosseinB · August 4, 2016, 10:19

Quote:

Originally Posted by eb19

Hi Hossein,

Did you manage to simulate waves with turbulence being included in your numerical domain? I am currently facing a similar problem. With the turbulence modeling being implemented, the wave amplitudes experience reduction in time.

Could you please share your suggestion or anyone who has experience? Thanks.

Cheers
Bangun

Hi,

Since the turbulence models I used, k-epsilon, and k-omega, led to unrealistic dampings, I modelled my case as a laminar problem and results were largely compared very well with the experiment.

For a new round of my studies, I might consider the turbulence modelling.

Did you figure out how to fix this problem?

Cheers,
Hossein

HosseinB · August 4, 2016, 10:26

Hi IHFoamers,

I am modelling:

Height, H: 0.776 m
Depth, d: 1.454 m
Period, T: 2.4

Cell size info: nearly cubic: 0.03 m side length.

This wave is close to the upper limit of reality breaking limit which is H/d = 0.54.

IHFoam waves break very very badly, but it doesn't in reality (experiment). Any suggestion how to prevent numerical breaking?

This is a very challenging modelling exercise and any input is highly appreciated.

Cheers,
Hossein

eb19 · August 26, 2016, 11:51

Hi Hossein,

The standard turbulence modeling in OpenFoam for incompressible multiphase problem is unphysically dissipative in the free surface because the production term in the turbulence modeling equations contain shear strain. To remedy the problem, curls of velocity should be implemented. I haven't tried it yet. But you could find the discussions about this issue from wave2foam thread and Jacobsen's Phd thesis.

Or you could try set the k and epsilon or omega values in such a way that nut is sufficiently smaller than molecular viscosity. It significantly helps reducing the dissipation in time.

Best
Bangun

HosseinB · August 26, 2016, 11:58

Thanks a lot for sharing your knowledge here with me.

I'll see what I can do.

Cheers,
Hossein

Quote:

Originally Posted by eb19

Hi Hossein,

The standard turbulence modeling in OpenFoam for incompressible multiphase problem is unphysically dissipative in the free surface because the production term in the turbulence modeling equations contain shear strain. To remedy the problem, curls of velocity should be implemented. I haven't tried it yet. But you could find the discussions about this issue from wave2foam thread and Jacobsen's Phd thesis.

Or you could try set the k and epsilon or omega values in such a way that nut is sufficiently smaller than molecular viscosity. It significantly helps reducing the dissipation in time.

Best
Bangun

HosseinB · August 30, 2016, 15:01

Hi,

I have a time-series for the location of a paddle during a test (experiment). I'd like to input that to IH Foam. I am aware this is possible by need directions how.

Cheers,
Hossein

IHFOAM Team · September 14, 2017, 06:07

Quote:

Originally Posted by CHiller

Dear Foamers,

are there any values for porosity: a, b, c, D50 and porosity given in literature. Or any hints how I can find out which value to assume for my simulaiton or on which model it is based?

Thanks for your help.

Hi CHiller,

You can find some validation data about porosity in Pablo Higuera's Thesis:
http://ihfoam.ihcantabria.com/references/phd-thesis/

Check IH-Cantabria gitHub account to download the codes:
https://github.com/IHCantabria

Best Regards,
IHFOAM Team

Maoyanjun · September 16, 2017, 00:54

hi foamers:
I am using the WaveMaker piston type boundary in the OLAFoam to generate waves in the NWT, and I found the active absorption in the outlet is not very stable to absorb the wave.have you met this problem? and I also have a question about the wave absorption at the inlet. I got the surface elevation in time history.is it sufficient to absorb the secondary reflection? I have no idea about it. because the wave height is larger than what I set H 0.2. is it normal?

July 4, 2016, 11:42	How to select the constant values for k-Eps?	#231
rcarmi New Member Remi Carmi Join Date: Jul 2014 Posts: 15 Rep Power: 12	Hi, I am not sure how to select the proper value for the k-Eps model. I see in the tutorial of breakwater the values of k and eps are set to 0.0001 but in other tutorial to 0.1 Here is what I have set so far (I have only solid boundaries which should be equivalent to plexiglass) epsilon internal field uniform 0.0001 bottom => type epsilonWallFunction with value 0.0001 inlet outlet => type zeroGradient atmosphere => type inletOutlet with value 0.0001 k internalField uniform 0.0001 bottom => type kqRWallFunction with value 0.0001 atmostphere and inlet outlet idem previous and the kEps coeffs are left unchanged Cmu = 0.09 C1 = 1.44 C2 = 1.92 sigmaEps =1.3 Is there a rule for the waves? I am interested in waves for water depth of 0.15m period 0.65s and wave height 0.035m. Thanks for any advice! Carmi

July 13, 2016, 07:38	query	#232
zanis New Member Zahra Ashoori Join Date: Mar 2016 Location: Tehran - Iran Posts: 9 Rep Power: 10	Dear Pablo, I'm a new user of IHFoam and it seems great, but when I try to solve "breakwater" after "interFoam" I face with the error as follows: file: /home/zanis/tutorials/OF300/breakwater/0/U.boundaryField.inlet from line 26 to line 28. From function fvPatchField<Type>::New(const fvPatch&, const DimensionedField<Type, volMesh>&, const dictionary&) in file /home/openfoam/OpenFOAM/OpenFOAM-3.0.1/src/finiteVolume/lnInclude/fvPatchFieldNew.C at line 143. FOAM exiting I have checked mentioned page many times, but couldn't find what the problem is. Could you please guide me to run it correctly? Best regards Zahra

August 4, 2016, 10:26	Very close-to-breaking wave modelling	#235
HosseinB Member Join Date: Apr 2015 Posts: 42 Rep Power: 11	Hi IHFoamers, I am modelling: Height, H: 0.776 m Depth, d: 1.454 m Period, T: 2.4 Cell size info: nearly cubic: 0.03 m side length. This wave is close to the upper limit of reality breaking limit which is H/d = 0.54. IHFoam waves break very very badly, but it doesn't in reality (experiment). Any suggestion how to prevent numerical breaking? This is a very challenging modelling exercise and any input is highly appreciated. Cheers, Hossein

August 26, 2016, 11:51		#236
eb19 New Member bangun Join Date: Feb 2015 Posts: 16 Rep Power: 11	Hi Hossein, The standard turbulence modeling in OpenFoam for incompressible multiphase problem is unphysically dissipative in the free surface because the production term in the turbulence modeling equations contain shear strain. To remedy the problem, curls of velocity should be implemented. I haven't tried it yet. But you could find the discussions about this issue from wave2foam thread and Jacobsen's Phd thesis. Or you could try set the k and epsilon or omega values in such a way that nut is sufficiently smaller than molecular viscosity. It significantly helps reducing the dissipation in time. Best Bangun Maoyanjun, mo_na and Stan Zhou like this.

August 30, 2016, 15:01	Test paddle position as a function of time input by IH Foam	#238
HosseinB Member Join Date: Apr 2015 Posts: 42 Rep Power: 11	Hi, I have a time-series for the location of a paddle during a test (experiment). I'd like to input that to IH Foam. I am aware this is possible by need directions how. Cheers, Hossein

June 23, 2016, 05:37		#227
mo_na Member Mona Join Date: Mar 2016 Location: Berlin Posts: 49 Rep Power: 10	Hi Agnese, ah yes! I changed that at some point in the past and forgot to change it back to zeroGradient. I am running it again now to check if that might have caused the problem. Thanks for your help again! If this doesn't help I'll try to contact Javier Lara for the new version.

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