[lukasfischer]

I think at the moment i am using what you call constant velocity, i specify the boundary condition of U at the inlet via timeVaryingUniformFixedValue and a time series file in OF-1.5.

inlet
{
type timeVaryingUniformFixedValue;
fileName "time-series";
outOfBounds warn;
value uniform (0 0 0);
}

and a file "time-series" of this form:

(
(0 (0 0 0))
(0.05 (0.0499947918294 0 0))
(0.1 (0.0999583385414 0 0))
(0.15 (0.149859414545 0 0))
(0.2 (0.199666833294 0 0))
.
.
.

)

[matteoL]

Hello,
i got one question and one answer:

answer:
as inlet BC for wave generation you can use this great library :
http://openfoamwiki.net/index.php/Contrib_groovyBC
(there is even a wavetank example)

question:
what about the non reflective BC?has anyone developed a version of wavetrasmissive BC for the interfoam solver?(the one implementd os for compressible gas if i am correct..)


if not, Niels and kevin, is your sponge BC available? I presume it would work perfectly as well...

Thank you very much,
ciao
matteo

[ngj]

Hi Matteo

Unfortunately there are still some issues and verification on my present implementation which needs to be carried out, thus my implementation is not mature for release. As soon as it is, I will submit through the OF-extend's svn. However non-reflective inlet and outlet boundaries are implemented and easily to extend to different wave theories.
I will make sure to post a note.

Best regards,

Niels

[gtampier]

Hi all,
I have a actually a new question/thread but I think it passes perfectly to the title of this thread: I think many of you (including me) has been successful modeling (harmonic) water waves with the groovyBC quite well: does anyone have experience validating these waves with analytical results?
After dealing with grid quality problems and wave reflection at the outflow I have managed to get quite good results for a 2nd order Stokes wave. My problem appears when I do the same for a wave + inlet velocity (moving observer -> encounter freq.). The wave amplitude and the wave shape doesn't match anymore with analytical results, and the wave profile looks quite ugly. I've been trying different settings, but without success until now. Does anyone have had similar experiences?
btw, the wave reflection problem mentioned in previous tasks can be eliminated very easily "numerically", by making an extreme coarse grid at the outflow region. It's not an elegant solution, but it works for me ;-)
Best Regards,

Gonzalo

[lostin4ever]

Hi all,

I have simulated tank3dsloshing using interDymfoam. For having a clear picture of comparison of theoretical and simulation results I am using natural mode frequency of tank. As far as surface mode are concern I am getting very perfect match with theoretical result for lower frequencies.

But in case of tank3d sloshing there should be mode in both the direction ( direction along which table is vibrating(width) and along length. In the simulations results along the width are perfectly ok but there is no mode shape along the length of the tank ( I have done the experiment on vibration shake table and the modes were there. ) Can anyone tell how I can correct this? Another thing is the amplitude are not as high as they should in resonance case.

For 3D tank the mode frequency is calculated by
mode frequency f is calculated as..
omega = 2*pi*f
omega = sqrt (gktanh(kh))
k = pi*sqrt((2m/W)^2+(2n/L)^2)
m and n are the natural mode along the width and length.
h is water level height in tank . in my case it is 6cm.

problem specifications :
Rectangular tank 35X50X40 cm
translation vibration for table given along 50 cm length
freq. is applied corresponding 3 mode along 50cm and 3rd mode along 35 cm ..
m =3 and n=3 in above equation.

I will send the files and simulation video if someone want to see. Here i am not able to share those due to size limit of forum.

Thanks

[m.afshar]

Hello everyone

I have just used the groovyBC to simulate a 2D wave tank on OF 1.6.x. I acted upon the instructions in "http://openfoamwiki.net/index.php/Contrib_groovyBC" and I managed to compile, mesh and set the fields.
Unfortunately interFoam crashes some time after the run and reports following lines on the terminal.
Could anyone please kindly give me his/her opinion and recommendations on this?

Regards
Amini Afshar

GAMG: Solving for p, Initial residual = 0.00018406464, Final residual = 2.4874203e-06, No Iterations 1
GAMG: Solving for p, Initial residual = 3.8566011e-06, Final residual = 1.1349343e-07, No Iterations 3
GAMGPCG: Solving for p, Initial residual = 3.9084748e-07, Final residual = 4.6119893e-09, No Iterations 7
time step continuity errors : sum local = 4.0037774e-08, global = -4.0260771e-09, cumulative = 4.0826213e-07
ExecutionTime = 7.7 s ClockTime = 7 s

Courant Number mean: 0.015971948 max: 0.47595885
deltaT = 0.01
Time = 0.69

MULES: Solving for alpha1
Liquid phase volume fraction = 0.47207799 Min(alpha1) = -0.028818711 Max(alpha1) = 1.0000086
MULES: Solving for alpha1
Liquid phase volume fraction = 0.47189442 Min(alpha1) = -0.043882922 Max(alpha1) = 1.0000086
MULES: Solving for alpha1
Liquid phase volume fraction = 0.47171085 Min(alpha1) = -0.058956843 Max(alpha1) = 1.0000087
GAMG: Solving for p, Initial residual = 0.00018071337, Final residual = 7.8103561e-06, No Iterations 1
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/mostafa/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/mostafa/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted:
#3 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::Field<double> const&, Foam::Field<double> const&, Foam::Field<double> const&) const in "/home/mostafa/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#4 Foam::GAMGSolver::scalingFactor(Foam::Field<double >&, Foam::lduMatrix const&, Foam::Field<double>&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/home/mostafa/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#5 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/home/mostafa/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#6 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/home/mostafa/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libOpenFOAM.so"
#7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/home/mostafa/OpenFOAM/OpenFOAM-1.6.x/lib/linuxGccDPOpt/libfiniteVolume.so"
#8 main in "/home/mostafa/OpenFOAM/OpenFOAM-1.6.x/applications/bin/linuxGccDPOpt/interFoam"
#9 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#10 _start at /build/buildd/eglibc-2.10.1/csu/../sysdeps/i386/elf/start.S:122
Floating point exception

[gtampier]

Hi Amini,
I would recommend you to take a look of your latest saved time step with paraFoam and check if everything looks "physically correct". If yes, post your fvSchemes and fvSolution here and I'll take a look of it. Specially your min alpha1 looks a little strange: it should be 0 or a value near to it within numerical errors, your value seems to me a little strange.
Regards,
Gonzalo

[m.afshar]

Thanks a lot Gonzalo Tampier

I looked at paraFoam and it seems that everything up to the crash moment is normal. At least a wave like motion for a while can be distinguished in it.
I brought some change to the setting before the run since there were some complaints regarding the syntax in OF 1.6. Like gamma to alpha and dynamic pressure pd to p. Also I changed the original syntax for matrix preconditioner in fvsolution to have interFoam running. Here come fvsolution and fvscheme files:

Regards
Mostafa Amini Afshar



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

solvers
{
pcorr PCG
{
preconditioner
{
preconditioner GAMG;
tolerance 1e-3;
relTol 0;

smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
nBottomSweeps 2;

cacheAgglomeration false;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
};

tolerance 1e-4;
relTol 0;
maxIter 100;
};

p GAMG
{
tolerance 1e-8;
relTol 0.05;

smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
nFinestSweeps 2;

cacheAgglomeration false;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
};

pFinal PCG
{
preconditioner
{
preconditioner GAMG;
tolerance 1e-8;
relTol 0;

nVcycles 2;

smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
nFinestSweeps 2;

cacheAgglomeration false;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
};

tolerance 1e-8;
relTol 0;
maxIter 20;
};

U smoothSolver
{
smoother GaussSeidel;
tolerance 1e-6;
relTol 0;
nSweeps 1;
};

k PBiCG
{
preconditioner DILU;
tolerance 1e-08;
relTol 0;
};
B PBiCG
{
preconditioner DILU;
tolerance 1e-08;
relTol 0;
};
nuTilda PBiCG
{
preconditioner DILU;
tolerance 1e-08;
relTol 0;
};
}

PISO
{
momentumPredictor no;
nCorrectors 3;
nNonOrthogonalCorrectors 0;
nAlphaCorr 1;
nAlphaSubCycles 3;
cAlpha 1;
pRefCell 0;
pRefValue 0;
pRefProbe
{
fields (p);
probeLocations ((0.51 0.51 0.51));
};
}

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









and




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

ddtSchemes
{
default Euler;
}

gradSchemes
{
default Gauss linear;
grad(U) Gauss linear;
grad(alpha) Gauss linear;
}

divSchemes
{
div(rho*phi,U) Gauss limitedLinearV 0;
div(phi,alpha) Gauss vanLeer01;
div(phirb,alpha) Gauss interfaceCompression;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
pcorr;
alpha1;
}

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

[elliot_hfx]

Hi Amini,

I met similar problem as yours, I changed the settings in fvSolution which is from setting in sloshing tutorial case, it run to 9 seconds, and then it crashed. I am just wondering how can I set the parameters in the file fvSolution. I will be very appreciate anyone who can give me some suggestions. Thanks.


Best regards,

Elliot

[m.afshar]

Hi Elliot

I managed to fix the problem by lowering max Courant Number and max deltaT" in controlDict.

Regards
Amini Afshar

[elliot_hfx]

Hi Amini,

Did you fix the problem by lowering the max Courant NO. and max deltaT? I tried to do this, it runs to a longer time, but it crashed at last. Thanks.

Best regards,

Elliot

[m.afshar]

Hello

Yes I did and It toke longer time. Just to inform you that I was running a 2D wave tank using GroovyBC and its computational requirements may be different than sloshing case.

Cheers
Amini Afshar

[elliot_hfx]

Hi,

Thanks for your message. I will try it again.

Best regards,

Elliot

[vrosaless]

Hello

I made a test for the wavetank using groovyBC with OpenFoam 1.7.0.

I downloaded groovuWaveTank.tgz

I found a first problem and fix it with bison

Then I got an error message:

-------------------------------------------------------------
--> FOAM FATAL IO ERROR:
cannot open file

file: /home/vrosaless/OpenFOAM/vrosaless-1.7.0/run/multiphase/interFoam/ras/groovyWaveTank/0/p_rgh at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 61.

FOAM exiting
------------------------------------------------------------

From another post in CDF online I try setFields but it doesn't work. Further in that disscution they emntion something about "reconstruct" but I don't get the idea how to fix the problem in the wave Tank case.

Thanks for any help

Victor

[elliot_hfx]

file: /home/vrosaless/OpenFOAM/vrosaless-1.7.0/run/multiphase/interFoam/ras/groovyWaveTank/0/p_rgh at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 61.


Did you have the file "p_rgh" in the directory "0"?

[vrosaless]

no I don't have p_rgh

in the 0 foulder I got:

pd
gamma.org
gamma.gz
U.gz

Victor

[elliot_hfx]

I think you need to modify the pd to p_rgh, gamma to alpha1, and then try and see

[vrosaless]

So far...

In fact I was running an old version of wave Tank. The most recently for OF 1.6 is updated with the variables needed.

From that there is an error concerning a variable maxAlphaCo:
I updated controlDict
MaxAlphaCo 0.9;

Then I update fvschemes
fluxRequired
{
default no;
p_rgh;
pcorr;
alpha;
}

It's now running...

Victor

[nuovodna]

Hi, i downloaded and ran groovyBc wave tank case in 1.7.0 but i have a problem: the level of water goes up along z direction and it stops his level near to atmosphere patch. Is it the correct behaviour ??

I attach the case ready to run

http://dl.dropbox.com/u/3617688/groo...Tank170.tar.gz

[yannH]

hi nuovocha,

I look quickly at your files, why did you put zeroGradient for boundary condition of your pressure p ? I think you should write ''type buoyantPressure;'' like it was in previous versions.

best regards,

Yann