Hi, I was wondering if anyone
 

Hi,
I was wondering if anyone had an example of using the twoLiquidMixingFoam solver that they would be willing to share? The user and programer's reference don't seem to have one. I am interested in modeling some microfluidic mixers.

Cheers

Shawn Pfeil

Enjoy, http://www.cfd-onli
 

Enjoy,

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif twoStream.tgz

Hrv

I noticed in the controlDictio
 

I noticed in the controlDictionary the solver is interFoam is twoLiquidMixingFoam not used? I'm a little bit of a newbie.

Thanks,

Hi Hrv, (and others) I went t
 

Hi Hrv, (and others)
I went to run the example you sent and got the following error:

--> FOAM FATAL ERROR : gradientInternalCoeffs cannot be called for a defaultFvPatchField.
(Actual type fixedMeanValue)
You are probably trying to solve for a field with a default boundary conditions.

From function defaultFvPatchField<type>::gradientInternalCoeffs( ) const
in file fields/fvPatchFields/basicFvPatchFields/default/defaultFvPatchField.C at line 421.

FOAM exiting

I noticed that when defining the boundary conditions you used an auxilary file outside of the blockMesh dictionary. The file boundary in the polyMesh/ directory. I'm a little new to OpenFOAM and am not entirely sure how this works. If somone has the time to clue me in I would greatly appreciate it. All the examples in the programing guide appear to have b.c.'s self contained in the blockMeshDictonary. Putting them in a seperate file has obvious advantages. I suspect my problem is that I have not figured out how to tell interFoam to look for the boundary file.

Cheers,

Shawn

Aha, that's one of my new boun
 

Aha, that's one of my new boundary conditions: change it to fixedValue and all will be well.

Hrv

Hi, I still a little confused
 

Hi,
I still a little confused. Is defaultFvPatchField a boundary condition you wrote? If so where is it referenced that I need to replace with a fixedValue? I didn't see it in the .OpenFOAM-1.3/Fields directory. Or do I need to replace some of the conditions in the blockMeshDictionary with fixedValue? Sorry for all the newbie questions.

Shawn

edit 0/pd, line 42: change fix
 

edit 0/pd, line 42: change fixedMeanValue into fixedValue.

In any case, here's an updated version.

Hrv

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif twoStream.tgz

For the discussion on default b.c. please have a look through the forum - I have already explained this ad nauseum. :-)

I figured it out.
 

I figured it out.

Hi, I was wondering if their
 

Hi,
I was wondering if their is a simple way to make the viscosity in twoLiquidMixing foam a function of gamma. I am interested in mixing two newtonian liquids where the viscosity is a function of the fraction gamma. It seems like this should be fairly straightforward to code, but I wanted to ask the various c++ and OpenFoam masters before I invest the time. Also, if you could point me to the part of the code I need to tinker with that would be great.

Shawn

Hi, Dear Foamers, I update the example case using twoLiquidMixingFoam solver for OpenFOAM Version 1.6.

Enjoy,
Chiven

Hi,

I tried gunzip on the example and got out a binary file. I was expecting some directories? I just updated to OpenFOAM-1.6 and was hoping to find a good example to get up to speed.

I realized the file was a .tar.gz file and set up the example. It still gives an error. I ran blockMesh and then twoLiquidMixingFoam. The output is

Create time

Create mesh for time = 0


Reading g
Reading field p_rgh



--> FOAM FATAL IO ERROR:
cannot open file

file: /home/shp/OpenFOAM/OpenFOAM-1.6.x/tutorials/twoStream/0/p_rgh at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 62.

FOAM exiting

field p_rgh is not mentioned in any of the entries under system. What is this?

Shawn

Hi, I think you 've probably forgotten the "step" setFields

try this : blockMesh, setFields and finally twoLiquidMixingFoam

regards

Yann

Sorry, I'm using this solver too.
I use your files.
Also I use setFields, but still no p_rgh file.

Hi Hrv,

is there a version of fixedMeanValue for Openfoam 1.6 yet ?
I would be really glad to get hold of it, if possible, since i have been dealing with a problem which might be solved by your boundary condition. But I kind of dislike the thought of going back do OF 1.5...or earlier.

thx & regards

omg, never mind my stupidity, plz!

Just figured it out ... for the records, fixedMeanValue works also with OF 1.6..

you need:

files file:
The options file needs only:

in the control dict you need to add:

This is the one I modified on OpenFOAM 1.6.x.

Dear Foamers,

Does anyone of you know where I can find some informations about model being implemented in TwoLiquidMixingFoam, especially descriptions of the extra terms in NS equations ?
1. (fvc::grad(U) & fvc::grad(muEff))
2. what function reconstruct does ?

fvc::reconstruct
(
fvc::interpolate(rho)*(g & mesh.Sf())
- mesh.magSf()*fvc::snGrad(p)
),
3. Why there is "- mesh.magSf()*fvc::snGrad(p)" to calculate pressure gradient instead of:
"-fvc::grad(p)" ?

Thanks for your help !
ZM

They use flux reconstruction to introduce the pressure gradient and the buoyancy term (combined now with the introduction of p_rgh) in the momentum predictor. Due to this, the pressure gradient introduced as the contribution it gives to the flux, as argument of reconstruct().

p_rgh at line 0
 

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

This one should work and run.

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.

p_rgh
 

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

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!

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;
}
}

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

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.

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;
}

Thank you!

what does alphatab stand for ?

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

Attachment 6025
here you have.

+1?


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


Is alphatab some kind of multiplier on that?

alphatab = 1/Sct (the turbulent Schmidt number)

Ah. Thank you. :)

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

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;
}

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

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::printStack(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?

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?