[balkrishna]

I faced the following difficulty.
I switch off the dispersed phase volume fraction at inlet . That is inlet alpha = uniform 0 and also the dispersed phase velocity . I keep my continuous phase velocity Ub = 0.1 m/s . Continuous properties are rho = 1000 kg/m3 , nu = 1e-06 m2/s . This means now i am studying single phase flow . I compared the results to simpleFoam results and have found a problem with the velocity plots in the plane z=0.2 on the same timestep . Specifically on the line joining (0 0.5 0.2) and (1 0.5 0.2) . Can someone help me resolve this issue ....
My blockMeshDict is as follows :

/*--------------------------------*- C++ -*----------------------------------* \
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices        
(
 (0 0 0)
 (0.25 0 0)
 (0.25 0.25 0)
 (0 0.25 0)
 (0 0.75 0)
 (0.25 0.75 0)
 (0 1 0)
 (0.25 1 0)
 (0.75 0 0)
 (0.75 0.25 0)
 (1 0 0)
 (1 0.25 0)
 (0.75 0.75 0)
 (1 0.75 0)
 (0.75 1 0)
 (1 1 0)

 (0 0 2)
 (0.25 0 2)
 (0.25 0.25 2)
 (0 0.25 2)
 (0 0.75 2)
 (0.25 0.75 2)
 (0 1 2)
 (0.25 1 2)
 (0.75 0 2)
 (0.75 0.25 2)
 (1 0 2)
 (1 0.25 2)
 (0.75 0.75 2)
 (1 0.75 2)
 (0.75 1 2)
 (1 1 2)
 
);

blocks          
(
 hex (0 1 2 3 16 17 18 19) (10 10 10) simpleGrading (1 1 1)
 hex (3 2 5 4 19 18 21 20) (10 10 10) simpleGrading (1 1 1)
 hex (4 5 7 6 20 21 23 22) (10 10 10) simpleGrading (1 1 1)
 hex (1 8 9 2 17 24 25 18) (10 10 10) simpleGrading (1 1 1)
 hex (2 9 12 5 18 25 28 21) (10 10 10) simpleGrading (1 1 1)
 hex (5 12 14 7 21 28 30 23) (10 10 10) simpleGrading (1 1 1)
 hex (8 10 11 9 24 26 27 25) (10 10 10) simpleGrading (1 1 1)
 hex (9 11 13 12 25 27 29 28) (10 10 10) simpleGrading (1 1 1)
 hex (12 13 15 14 28 29 31 30) (10 10 10) simpleGrading (1 1 1)
 );

edges           
(
);

patches         
(
 patch inlet (
	      (2 5 12 9)
	      ) 

 patch outlet (
	       (16 19 18 17)
	       (19 20 21 18)
	       (20 22 23 21)
	       (17 18 25 24)
	       (18 21 28 25)
	       (21 23 30 28)
	       (24 25 27 26)
	       (25 28 29 27)
	       (28 30 31 29)
	      
       	       )

   wall fixedWalls 
    (
     (0 16 19 3)
     (3 19 20 4)
     (4 20 22 6)
     (6 22 23 7)
     (7 23 30 14)
     (14 30 31 15)
     (15 31 29 13)
     (13 29 27 11)
     (11 27 26 10)
     (10 26 24 8)
     (8 24 17 1)
     (1 17 16 0)
     (0 3 2 1)
     (3 4 5 2)
     (4 6 7 5)
     (5 7 14 12)
     (12 14 15 13)
     (9 12 13 11)
     (8 9 11 10)
     (1 2 9 8)
     )


    
);

mergePatchPairs 
(
);

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

The velocity plots are on this page .... https://sites.google.com/site/balkrishnanitt/

[alberto]

How is the model set up in bubbleFoam? Are you using the turbulence model or performing a laminar simulation?

Best,

[balkrishna]

I am performing a laminar simulation .

[alberto]

Ignore my previous answer (removed). I generated the mesh, and run the case, noticing you have an expansion. Could you post your case setup?

[balkrishna]

Thanks for the reply ...
I was unable to place an image of the mesh in the post ... I have uploaded the image of the mesh on the link ... Sorry for the inconvienience ....

Secondly , I am not seeking convergence ... All that I am saying is if I switch off my dispersed phase , my equations reduce to those solved by simpleFoam and hence should give the same results at the same time on the same mesh .

Do clarify me if I am wrong somewhere ....

[balkrishna]

Alpha :

/*--------------------------------*- C++ -*----------------------------------* \
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      alpha;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 0 0 0 0];

internalField  uniform 0 ;
boundaryField
{
    inlet           
    {
        type            fixedValue;
        value           uniform 0;
    }

    outlet          
    {
      type            zeroGradient;
    }

    fixedWalls           
    {
        type            zeroGradient;
    }


}

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

Pressure

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 0;
boundaryField
{
    inlet
    {
        type            zeroGradient;
    }

    outlet
    {
        type            fixedValue;
        value           uniform 0;
    }

    fixedWalls
    {
        type            buoyantPressure;
        value           uniform 0;
    }

    defaultFaces
    {
        type            empty;
    }
}

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

Ub velocity of continuous phase

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      Ub;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform (0 0 0);
boundaryField
{
    inlet           
    {
        type            fixedValue;
        value           uniform (0 0 0.1);
    }

    outlet          
    {
      type            zeroGradient;
    }

    fixedWalls           
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }


}

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

Ua velocity of dispersed phase

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      Ua;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform (0 0 0) ;

boundaryField
{
    inlet           
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

    outlet          
    {
      type            zeroGradient;
    }

    fixedWalls           
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }


}

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

k

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 1e-8;

boundaryField
{
    inlet           
    {
        type            fixedValue;
        value           uniform 1e-8;
    }

    outlet          
    {
        type            inletOutlet;
        inletValue      uniform 1e-8;
        value           uniform 1e-8;
    }

    fixedWalls           
    {
        type            zeroGradient;
    }

    defaultFaces    
    {
        type            empty;
    }
}

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

epsilon

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 0.1;

boundaryField
{
    inlet           
    {
        type            fixedValue;
        value           uniform 0.1;
    }

    outlet          
    {
      type       zeroGradient;     
    }

    fixedWalls           
    {
        type            zeroGradient;
    }

    
}

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

controlDict

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     bubbleFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         2;

deltaT          0.001;

writeControl    runTime;

writeInterval   0.5;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression uncompressed;

timeFormat      general;

timePrecision   6;

runTimeModifiable yes;


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

fvSchemes

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    default         none;
    div(phia,Ua)    Gauss limitedLinearV 1;
    div(phib,Ub)    Gauss limitedLinearV 1;
    div(phib,k)     Gauss limitedLinear 1;
    div(phib,epsilon) Gauss limitedLinear 1;
    div(phi,alpha)  Gauss limitedLinear01 1;
    div((-nuEffa*grad(Ua).T())) Gauss linear;
    div((-nuEffb*grad(Ub).T())) Gauss linear;
}

laplacianSchemes
{
    default         none;
    laplacian(nuEffa,Ua) Gauss linear corrected;
    laplacian(nuEffb,Ub) Gauss linear corrected;
    laplacian((rho*(1|A(U))),p) Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p               ;
}


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

fvSolution

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-10;
        relTol          0;
    }

    Ua
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0;
    }

    Ub
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0;
    }

    alpha
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-10;
        relTol          0;
    }

    beta
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-10;
        relTol          0;
    }

    k
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0;
    }

    epsilon
    {
        solver          PBiCG;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0;
    }
}

PISO
{
    nCorrectors     2;
    nNonOrthogonalCorrectors 0;
    nAlphaCorr      2;
    correctAlpha    no;
    pRefCell        0;
    pRefValue       0;
}


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

g

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       uniformDimensionedVectorField;
    location    "constant";
    object      g;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -2 0 0 0 0];
value           ( 0 0 -9.81  );


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

RASProperties

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      RASProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

RASModel        laminar;

turbulence      off;

printCoeffs     off;


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

transportProperties

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

rhoa            rhoa [ 1 -3 0 0 0 0 0 ] 1;

rhob            rhob [ 1 -3 0 0 0 0 0 ] 1000;

nua             nua [ 0 2 -1 0 0 0 0 ] 1.6e-05;

nub             nub [ 0 2 -1 0 0 0 0 ] 1e-06;

da              da [ 0 1 0 0 0 0 0 ] 0.003;

db              db [ 0 1 0 0 0 0 0 ] 0.0001;

Cvm             Cvm [ 0 0 0 0 0 0 0 ] 0.5;

Cl              Cl [ 0 0 0 0 0 0 0 ] 0;

Ct              Ct [ 0 0 0 0 0 0 0 ] 1;


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

[alberto]

You are correct. The result should be the same.

Did you use the same numerical schemes and the same tolerances in the linear solvers also in simpleFoam?

Also, set to zero the lift (Cl), virtual mass coefficients (Cvm) and Ct (not necessary in theory, since bubbleFoam uses a formulation depending on alpha, so these term should be zero automatically).

Best,
Alberto

[balkrishna]

Will recheck on the same .... Thanks for the help ...

[balkrishna]

Yes checked it .... the schemes are the same ....

[balkrishna]

But they should not matter as alpha or the dispersed phase is 0 . Those equations are written for the dispersed phase ....

[alberto]

Yes that's correct. I was just removing everything term that makes the two equations different.

The only additional difference I see in your files is g. There is no g in simpleFoam.

Best,

[balkrishna]

inclusion of g is only going to affect the pressure contours ... not the velocity plots ...
thanks ...

[alberto]

I did not imply this is going to cause a difference in the velocity plot, just that the only physical element of difference is that one in the equations.

The difference in the two solutions is located essentially at the walls, and the rest of the profile adapts as a consequence.

At what tolerance is the solution converged? Would you share a case so I can take a look at it (I sent my email address if you cannot upload)?

Best,

[alberto]

Since I was a bit puzzled by the problem, because I did a similar validation in the past, I run a simpler case of a flow between two parallel plates.

You find the cases here: http://dl.dropbox.com/u/659842/bubbl...bleFoam.tar.gz

And as you can see in the attached picture, the velocity profiles are identical.

Best,

[balkrishna]

your test case works great . have you found any problem in my case setup ?

[alberto]

Hi,

the case you sent me stops at 2 seconds, which is not enough for the solution to reach convergence. You might want to run the case with a larger time step (0.1 for example, or a bit smaller if you want residuals to be low) until t = 1000.

Additionally, the contour plots show quite a clear influence of the mesh on the solution, mainly due to the non-uniformity and the jumps in grid size between the different blocks.

I hope this helps.

Best,

[balkrishna]

I wish to modify bubble Foam of 2 phases to n phase and add heat transfer and species mixing to it .. One stumbling block i came across was the way the alpha equation was programmed .
it consists of the following line in the header file alphaEqn.H

 word scheme("div(phi,alpha)");

    surfaceScalarField phir = phia - phib;

This means they perform the phase calculation as stated in the wiki here . How does one extend the relative flux to n phase ...

[alberto]

Silva and Lage did it and have a conference paper on this topic. Check your email :-)

[balkrishna]

thanks a lot .....

[balkrishna]

Thanks for the link .... Can i get the source code of the solver ?? The implementation of the algorithm is the tough aspect in OpenFOAM .....