[alberto]

This one should work and run.

[maolongliu]

This is the p_rgh file now I use
//================================================== ==============
FoamFile
{
version 2.0;
format ascii;

root "";
case "";
instance "";
local "";

class volScalarField;
object p_rgh;
}

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


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

internalField uniform 0;

boundaryField
{
bottomInlet
{
type zeroGradient;
}
topInlet
{
type zeroGradient;
}
outlet
{
type fixedValue;
value uniform 0;
}
pipe
{
type zeroGradient;
}
defaultFaces
{
type empty;
}
}


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

Take care of the object name is "p_rgh", not "p", and also the dimension is different to simpleFoam.

Originally Posted by vrosaless

Hello

Can you explain more on how to fix the error "p_rgh at line 0"

I get the same error for a case to run a wave Tank. I downloaded the file twoStream.tar.gz and but I got an error like the file is corrupted

gzip: stdin: not in gzip format
tar: Child returned status 1
tar: Exiting with failure status due to previous errors
vrosaless@ubuntu:~/Downloads$ gunzip twoStream.tar.g

Any help is wellcome

Thanks

Victor

[vrosaless]

The last file it´s OK.

I' m actually using p_rgh for a wave tank in interFoam. I used your case to update the wave tank files where I found the p_rgh missing.

Thanks for your help

Victor

[phinallydone]

Hi, I'm also having the same problem trying to extract "twoStream.tar.gz". Would someone be willing to post a working version for v1.7 or as Victor requested provide some additional detail on how to fix the error "p_rgh at line 0"?

Thanks in advance!

[maolongliu]

Try this
//================================================== ==============
FoamFile
{
version 2.0;
format ascii;

root "";
case "";
instance "";
local "";

class volScalarField;
object p_rgh;
}

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


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

internalField uniform 0;

boundaryField
{
bottomInlet
{
type zeroGradient;
}
topInlet
{
type zeroGradient;
}
outlet
{
type fixedValue;
value uniform 0;
}
pipe
{
type zeroGradient;
}
defaultFaces
{
type empty;
}
}

Originally Posted by phinallydone

Hi, I'm also having the same problem trying to extract "twoStream.tar.gz". Would someone be willing to post a working version for v1.7 or as Victor requested provide some additional detail on how to fix the error "p_rgh at line 0"?

Thanks in advance!

[phinallydone]

Thanks Maolong LIU!

When I use the your suggestion I get the following

=======================
DILUPBiCG: Solving for alpha1, Initial residual = 0.00755434, Final residual = 2.4898e-08, No Iterations 2
Phase 1 volume fraction = 0.501191 Min(alpha1) = 0 Max(alpha1) = 1
DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 2.74871e-12, No Iterations 3
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 9.82467e-12, No Iterations 3


--> FOAM FATAL IO ERROR:
keyword p_rgh is undefined in dictionary "/home/hunts/Desktop/twoStream/system/fvSolution::solvers"

file: /home/hunts/Desktop/twoStream/system/fvSolution::solvers from line 22 to line 73.

From function dictionary::subDict(const word& keyword) const
in file db/dictionary/dictionary.C at line 456.

FOAM exiting
=======================

Any ideas? My apologies. I'm relatively new to OpenFOAM.

Thanks

[maolongliu]

In the fvSoluction file, and also fvSchems file, because now you solve p_rgh equation in stead of p equation, so you need change p to p_rgh.
So just change all the word "p" to "p_rgh" in both those files.

Originally Posted by phinallydone

Thanks Maolong LIU!

When I use the your suggestion I get the following

=======================
DILUPBiCG: Solving for alpha1, Initial residual = 0.00755434, Final residual = 2.4898e-08, No Iterations 2
Phase 1 volume fraction = 0.501191 Min(alpha1) = 0 Max(alpha1) = 1
DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 2.74871e-12, No Iterations 3
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 9.82467e-12, No Iterations 3


--> FOAM FATAL IO ERROR:
keyword p_rgh is undefined in dictionary "/home/hunts/Desktop/twoStream/system/fvSolution::solvers"

file: /home/hunts/Desktop/twoStream/system/fvSolution::solvers from line 22 to line 73.

From function dictionary::subDict(const word& keyword) const
in file db/dictionary/dictionary.C at line 456.

FOAM exiting
=======================

Any ideas? My apologies. I'm relatively new to OpenFOAM.

Thanks

[maolongliu]

This is my fvSolution file

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{

p_rgh
{
solver PCG;
preconditioner DIC;
tolerance 1e-8;
relTol 0;
}
p_rghFinal
{
solver PCG;
preconditioner DIC;
tolerance 1e-8;
relTol 0;
}

alpha1
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-06;
relTol 0;
}

U
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-08;
relTol 0;
}

UFinal
{
solver PBiCG;
preconditioner DILU;
tolerance 1e-08;
relTol 0;
}
}


PIMPLE
{
nOuterCorrectors 2;
nCorrectors 2;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}

Originally Posted by phinallydone

Thanks Maolong LIU!

When I use the your suggestion I get the following

=======================
DILUPBiCG: Solving for alpha1, Initial residual = 0.00755434, Final residual = 2.4898e-08, No Iterations 2
Phase 1 volume fraction = 0.501191 Min(alpha1) = 0 Max(alpha1) = 1
DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 2.74871e-12, No Iterations 3
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 9.82467e-12, No Iterations 3


--> FOAM FATAL IO ERROR:
keyword p_rgh is undefined in dictionary "/home/hunts/Desktop/twoStream/system/fvSolution::solvers"

file: /home/hunts/Desktop/twoStream/system/fvSolution::solvers from line 22 to line 73.

From function dictionary::subDict(const word& keyword) const
in file db/dictionary/dictionary.C at line 456.

FOAM exiting
=======================

Any ideas? My apologies. I'm relatively new to OpenFOAM.

Thanks

[phinallydone]

Thank you!

[balkrishna]

what does alphatab stand for ?

[mehdoo]

Originally Posted by alberto

This one should work and run.

I am looking for folder 0.org for this solver. Does anyone have it ?
please help me with this
Regards

[ziemowitzima]

0.zip
here you have.

[Amiga500]

Originally Posted by balkrishna

what does alphatab stand for ?

+1?


Dab is the diffusivity, as would be calculated using Chapman-Enskog for 2 gases...


Is alphatab some kind of multiplier on that?

[maolongliu]

alphatab = 1/Sct (the turbulent Schmidt number)

Originally Posted by Amiga500

+1?


Dab is the diffusivity, as would be calculated using Chapman-Enskog for 2 gases...


Is alphatab some kind of multiplier on that?

[Amiga500]

Originally Posted by maolongliu

alphatab = 1/Sct (the turbulent Schmidt number)

Ah. Thank you.

[alberto]

FYI, it is written in the code (createFields.H)

// Read the reciprocal of the turbulent Schmidt number
    dimensionedScalar alphatab(twoPhaseProperties.lookup("alphatab"));

[Tanay]

I'm trying to write a separate case for using twoLiquidMixingFoam in a customized form. First, I removed the variables 'p' and 'g' and 'gh' and instead operated everything in 'p_rgh'. Next, I removed 'alphatab' and now the diffusivity works solely on Dab.

In pEqn.H
{
volScalarField rAU = 1.0/UEqn.A();
surfaceScalarField rAUf = fvc::interpolate(rAU);

U = rAU*UEqn.H();
surfaceScalarField phiU
(
"phiU",
(fvc::interpolate(U) & mesh.Sf())
+ fvc::ddtPhiCorr(rAU, rho, U, phi)
);

adjustPhi(phiU, U, p_rgh);

phi = phiU ;//- ghf*fvc::snGrad(rho)*rAUf*mesh.magSf()

for(int nonOrth=0; nonOrth<=nNonOrthCorr; nonOrth++)
{
fvScalarMatrix p_rghEqn
(
fvm::laplacian(rAUf, p_rgh) == fvc::div(phi)
);

p_rghEqn.setReference(pRefCell, getRefCellValue(p_rgh, pRefCell));

p_rghEqn.solve
(
mesh.solver
(
p_rgh.select
(
finalIter
&& corr == nCorr-1
&& nonOrth == nNonOrthCorr
)
)
);

if (nonOrth == nNonOrthCorr)
{
phi -= p_rghEqn.flux();
}
}


U += rAU*fvc::reconstruct((phi - phiU)/rAUf);
U.correctBoundaryConditions();

#include "continuityErrs.H"


The problem is in the line-
fvm::laplacian(rAUf, p_rgh) == fvc::div(phi)

And the output reads-

--> FOAM FATAL IO ERROR:
keyword laplacian(interpolate((1|A(U))),p_rgh) is undefined in dictionary "/home/tanay/OpenFOAM/tanay-1.7.1/run/roughMix/system/fvSchemes::laplacianSchemes"

file: /home/tanay/OpenFOAM/tanay-1.7.1/run/roughMix/system/fvSchemes::laplacianSchemes from line 54 to line 63.

So, I tried adding this line to fvSchemes but it didn't work. Any suggestions on what's missing in fvSchemes?

Here's the fvSchemes file if anyone wishes to view it-
ddtSchemes
{
default Euler;
}

gradSchemes
{
default Gauss linear;
grad(U) Gauss linear;
grad(muEff) Gauss linear;
grad(p_rgh) Gauss linear;
}

snGradSchemes
{
default corrected;
}

divSchemes
{
default none;
div(phi,U) Gauss limitedLinearV 1;
div(phi,k) Gauss limitedLinear 1;
div(phi,epsilon) Gauss limitedLinear 1;
div(phi,R) Gauss limitedLinear 1;
div(R) Gauss linear;
div(phi,nuTilda) Gauss limitedLinear 1;
div((nuEff*dev(grad(U).T()))) Gauss linear;
div(phi,alpha1) Gauss limitedLinear 1;
div(phi) Gauss limitedLinear 1;
div(rhoPhi,U) Gauss limitedLinear 1;
div(rho*phi,U) Gauss limitedLinear 1;
}

laplacianSchemes
{
default none;
laplacian(nuEff,U) Gauss linear corrected;
laplacian((1|A(U)),p_rgh) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(DepsilonEff,epsilon) Gauss linear corrected;
laplacian(DREff,R) Gauss linear corrected;
laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
laplacian(Dab,alpha1) Gauss linear corrected;
laplacian(rAUf,p_rgh) Gauss linear corrected;
laplacian(muEff,U) Gauss linear corrected;
}

interpolationSchemes
{
default linear;
interpolate(U) linear;
}

fluxRequired
{
default no;
p_rgh ;
alpha1 yes;
}

[ziemowitzima]

Hi Tanay,

I think that you can have a problem with an extra "bracket". An error says:
laplacian(interpolate((1|A(U))),p_rgh)
so here u have : ...U))) -- triple closing )

but in your
laplacianSchemes you have :
....
laplacian((1|A(U)),p_rgh) Gauss linear corrected;
....

and: A(U)) double closing )

so it seems that you have some typo in your code.

Cheers
ZMM

[Tanay]

Yeah, thanks. That was a simple typo. Now, I'm getting a Courant number blow-up.

Courant Number mean: 21.0277 max: 258.938
deltaT = 3.37996e-06
Time = 0.0145817

#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted:
#3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so"
#4 Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<d ouble>&, Foam::Field<double> const&) const in "/opt/openfoam171/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 "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so"
#6 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so"
#7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam171/lib/linuxGccDPOpt/libfiniteVolume.so"
#8
in "/home/tanay/OpenFOAM/tanay-1.7.1/applications/bin/linuxGccDPOpt/customizedTwoLiquidMixingFoam"
#9 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#10
in "/home/tanay/OpenFOAM/tanay-1.7.1/applications/bin/linuxGccDPOpt/customizedTwoLiquidMixingFoam"
Floating point exception

Lowering the time step just prolongs the blow-up. All the fvSchemes (printed above) I've used correspond to a pimpleFoam tutorial and so they can't be too problematic. Where may be the error?

[Tanay]

Well, ziemowit, I've given up trying to make the blowing up case converge since I tried everything from reducing the time step to decreasing the velocity and increasing laminar viscosity etc. So, now I'm trying to build a new solver based on PIMPLE to simulate twoLiquidMixing. In this, I've included a file called customTwoLiquid.H for laminar mixing. It reads as-

surfaceScalarField muEff ("muEff", (alpha1*mu1 + (scalar(1)-alpha1)*mu2));
volScalarField rho ("rho", (alpha1*rho1 + (scalar(1)-alpha1)*rho2));
surfaceScalarField rhoIntoPhi ("rhoIntoPhi", rho*phi);

Now this produces a compilation error. Can you please tell me what's wrong?