[arsalan.dryi]

Hi Foamers,

I'm doing a 3D simulation of two and three bubble rising using a modified interFoam solver and I need to center position, velocity and surface area of the bubbles.

For a single bubble rising I used swak4Foam expressions for example for center position in Y as follows :

    bubbleCentreY
    {
        type swakExpression;
        valueType internalField;
        verbose true;
    variables (
    "Vol= sum (alpha1 < 0.5 ? vol() : 0);"
    "VolY= sum (alpha1 < 0.5 ? pos().y*vol() : 0);"    
    );        
    expression "VolY/Vol";
        accumulations (
        min        
        );

     
    }

Is there a way to compute these for two or three bubbles in this manner?

Thanks in advance,
Best Regards,
Arsalan.

[arsalan.dryi]

Does anybody have an idea?

Any help and comment will be greatly appreciated.

Regards,
Arsalan.

[arsalan.dryi]

I still didn't solve this problem, does anyone have an idea?!

Thanks in advance,
Regards.

[x86_64leon]

Hi Arsalan

Did you solve this problem of tracking more than one bubble and computing the center of mass, velocity, surface, volume ... etc of each of the bubbles ?

Regards

[Taataa]

One way is to use a multiphase flow solver like multiphaseInterFoam and for each bubble use a different name but same physical parameters. This way you can track each phase using the method OP mentioned or use this function that I have written for a wedge mesh which works in parallel as well:

functions
{
  riseVelocity
  {
    libs            ("libutilityFunctionObjects.so");
    
    type coded;
    
    name riseVelocity;
    
    codeExecute
    #{
        const volScalarField& alpha =
            mesh().lookupObject<volScalarField>("alpha.water");
        const volVectorField& U =
            mesh().lookupObject<volVectorField>("U");
        const volVectorField& centers = mesh().C();
        const scalarField& vols = mesh().V();
        
        const objectRegistry& db = mesh().thisDb();
        scalar ts = db.time().value();
        const dictionary& transportProperties =
            db.lookupObject<IOdictionary>
            (
                "transportProperties"
            );

        dictionary alpha2
        (
            transportProperties.subDict("air")
        );
        
        dimensionedScalar rhoBubble
        (
            "rhoBubble",
            dimDensity,
            alpha2.lookup("rho")
        );
        
        // threshold for interface
        scalar th = 0.5;
        // water level in the well
        scalar ht = 0.3;
        // sum of mass
        scalar sumMass = 0;
        // sum of volume
        scalar sumVol = 0;
        // sum of y by mass
        scalar sumX = 0;
        scalar sumY = 0;
        // sum of Uy by volume
        scalar sumUY = 0;
        //volume of liquid in well
        scalar vl = 0;
        
        forAll(centers, I)
        {
            if ( alpha[I] < th && centers[I].y() < ht )
            {
                //Mass center
                sumY    += (1 - alpha[I])*rhoBubble.value()*vols[I]*centers[I].y();
                sumX    += (1 - alpha[I])*rhoBubble.value()*vols[I]*centers[I].x();
                sumMass += (1 - alpha[I])*rhoBubble.value()*vols[I];
	              
	        //Rising Velocity
                sumUY   += (1 - alpha[I])*vols[I]*U[I].y();
                sumVol  += (1 - alpha[I])*vols[I];
            } else if ( centers[I].y() < ht ) {
                vl += alpha[I]*vols[I];
            }
        }
        
        reduce(sumY, sumOp<scalar>());
        reduce(sumX, sumOp<scalar>());
        reduce(sumMass, sumOp<scalar>());
        reduce(sumUY, sumOp<scalar>());
        reduce(sumVol, sumOp<scalar>());
        reduce(vl, sumOp<scalar>());
        
        // center of gravity
        scalar cgX = sumX/max(sumMass, SMALL);
        scalar cgY = sumY/max(sumMass, SMALL);
        
        // rising velocity
        scalar vr = sumUY/max(sumVol, SMALL);
        
        const volScalarField& p =
            mesh().lookupObject<volScalarField>("p");
        const faceList& ff = mesh().faces();
        const pointField& pp = mesh().points();
        // Pressure inside the bubble
        scalar pBubble = 0;
        
        forAll(centers, I)
        {
            const cell& cc = mesh().cells()[I];
            labelList pLabels(cc.labels(ff));
            pointField pLocal(pLabels.size(), vector::zero);

            forAll (pLabels, J)
            {
                pLocal[J] = pp[pLabels[J]];
            }
            
            if
            (
              sign(Foam::max(pLocal& vector(1,0,0)) - cgX) == 1 &&
              sign(cgX - Foam::min(pLocal& vector(1,0,0))) == 1 &&
              sign(Foam::max(pLocal& vector(0,1,0)) - cgY) == 1 &&
              sign(cgY - Foam::min(pLocal& vector(0,1,0))) == 1
            )
            {
                pBubble = mag(p[I]);
                break;
            }
        }
        reduce(pBubble, sumOp<scalar>());
        
        if (Pstream::master())
        {
            const fileName& outputFile = "plots/riseUCG";
            OFstream os
            (
                outputFile,
                IOstream::ASCII,
                IOstream::currentVersion,
                IOstream::UNCOMPRESSED,
                true
            );
            
            scalar tot = 360.0/5.0;
            Info<< "Writing rising velocity, CG, "
                << "volume of bubble, volume of liquid "
                << "and pressure inside the bubble for current time" << endl;
            os  << ts << "  " << vr << "  " << cgX  << "  " << cgY 
                << "  " << sumVol*tot << "  " << vl*tot << "  " << pBubble << endl;
        }
    #};
  }
}

It can easily be extended to multiphase e.g. for each phase add a new lookup, say alpha1 for alpha.water, alpha2 for alpha.air1 etc..

[piu58]

I solved this problem by a small external program which analyses the alpha value for each cell. It is very easy to calculate the values you need form that.

[arsalan.dryi]

Originally Posted by Taataa

One way is to use a multiphase flow solver like multiphaseInterFoam and for each bubble use a different name but same physical parameters. This way you can track each phase using the method OP mentioned or use this function that I have written for a wedge mesh which works in parallel as well:

functions
{
  riseVelocity
  {
    libs            ("libutilityFunctionObjects.so");
    
    type coded;
    
    name riseVelocity;
    
    codeExecute
    #{
        const volScalarField& alpha =
            mesh().lookupObject<volScalarField>("alpha.water");
        const volVectorField& U =
            mesh().lookupObject<volVectorField>("U");
        const volVectorField& centers = mesh().C();
        const scalarField& vols = mesh().V();
        
        const objectRegistry& db = mesh().thisDb();
        scalar ts = db.time().value();
        const dictionary& transportProperties =
            db.lookupObject<IOdictionary>
            (
                "transportProperties"
            );

        dictionary alpha2
        (
            transportProperties.subDict("air")
        );
        
        dimensionedScalar rhoBubble
        (
            "rhoBubble",
            dimDensity,
            alpha2.lookup("rho")
        );
        
        // threshold for interface
        scalar th = 0.5;
        // water level in the well
        scalar ht = 0.3;
        // sum of mass
        scalar sumMass = 0;
        // sum of volume
        scalar sumVol = 0;
        // sum of y by mass
        scalar sumX = 0;
        scalar sumY = 0;
        // sum of Uy by volume
        scalar sumUY = 0;
        //volume of liquid in well
        scalar vl = 0;
        
        forAll(centers, I)
        {
            if ( alpha[I] < th && centers[I].y() < ht )
            {
                //Mass center
                sumY    += (1 - alpha[I])*rhoBubble.value()*vols[I]*centers[I].y();
                sumX    += (1 - alpha[I])*rhoBubble.value()*vols[I]*centers[I].x();
                sumMass += (1 - alpha[I])*rhoBubble.value()*vols[I];
	              
	        //Rising Velocity
                sumUY   += (1 - alpha[I])*vols[I]*U[I].y();
                sumVol  += (1 - alpha[I])*vols[I];
            } else if ( centers[I].y() < ht ) {
                vl += alpha[I]*vols[I];
            }
        }
        
        reduce(sumY, sumOp<scalar>());
        reduce(sumX, sumOp<scalar>());
        reduce(sumMass, sumOp<scalar>());
        reduce(sumUY, sumOp<scalar>());
        reduce(sumVol, sumOp<scalar>());
        reduce(vl, sumOp<scalar>());
        
        // center of gravity
        scalar cgX = sumX/max(sumMass, SMALL);
        scalar cgY = sumY/max(sumMass, SMALL);
        
        // rising velocity
        scalar vr = sumUY/max(sumVol, SMALL);
        
        const volScalarField& p =
            mesh().lookupObject<volScalarField>("p");
        const faceList& ff = mesh().faces();
        const pointField& pp = mesh().points();
        // Pressure inside the bubble
        scalar pBubble = 0;
        
        forAll(centers, I)
        {
            const cell& cc = mesh().cells()[I];
            labelList pLabels(cc.labels(ff));
            pointField pLocal(pLabels.size(), vector::zero);

            forAll (pLabels, J)
            {
                pLocal[J] = pp[pLabels[J]];
            }
            
            if
            (
              sign(Foam::max(pLocal& vector(1,0,0)) - cgX) == 1 &&
              sign(cgX - Foam::min(pLocal& vector(1,0,0))) == 1 &&
              sign(Foam::max(pLocal& vector(0,1,0)) - cgY) == 1 &&
              sign(cgY - Foam::min(pLocal& vector(0,1,0))) == 1
            )
            {
                pBubble = mag(p[I]);
                break;
            }
        }
        reduce(pBubble, sumOp<scalar>());
        
        if (Pstream::master())
        {
            const fileName& outputFile = "plots/riseUCG";
            OFstream os
            (
                outputFile,
                IOstream::ASCII,
                IOstream::currentVersion,
                IOstream::UNCOMPRESSED,
                true
            );
            
            scalar tot = 360.0/5.0;
            Info<< "Writing rising velocity, CG, "
                << "volume of bubble, volume of liquid "
                << "and pressure inside the bubble for current time" << endl;
            os  << ts << "  " << vr << "  " << cgX  << "  " << cgY 
                << "  " << sumVol*tot << "  " << vl*tot << "  " << pBubble << endl;
        }
    #};
  }
}

It can easily be extended to multiphase e.g. for each phase add a new lookup, say alpha1 for alpha.water, alpha2 for alpha.air1 etc..

Multiphase solvers need a surface tension between each two different phases and the results can be completely wrong especially when bubbles get close to each other, for example in bubbles coalescence.

[arsalan.dryi]

Originally Posted by piu58

I solved this problem by a small external program which analyses the alpha value for each cell. It is very easy to calculate the values you need form that.

Could you explain more about that, please? And also post your written code here if possible.
Thanks.

[piu58]

Originally Posted by arsalan.dryi

Could you explain more about that, please? And also post your written code here if possible.
Thanks.

That is quite easy. You go row wise through the alpha field, calculate the x and y coordinates according the setting of your region. If the alpha value is below a limiting value ( I used 0.2 for discriminating air / water), you add the x and y coordinates to get finally the average of them. This average should be close to the center of mass.

I don't believe that my C program is of any use for you. It is tailored to my setting and comments are in German.

[Taataa]

Originally Posted by arsalan.dryi

Multiphase solvers need a surface tension between each two different phases and the results can be completely wrong especially when bubbles get close to each other, for example in bubbles coalescence.

Oh, I didn't know interFoam is not a multiphase solver!

[farzadmech]

Dear Arslan
Have you added these lines to controlDict? what other lines have you added? which library have you added in the libs section?
for exmample;

libs (
    "libgroovyBC.so"
) ;

Thanks,
Farzad

Originally Posted by arsalan.dryi

Hi Foamers,

I'm doing a 3D simulation of two and three bubble rising using a modified interFoam solver and I need to center position, velocity and surface area of the bubbles.

For a single bubble rising I used swak4Foam expressions for example for center position in Y as follows :

    bubbleCentreY
    {
        type swakExpression;
        valueType internalField;
        verbose true;
    variables (
    "Vol= sum (alpha1 < 0.5 ? vol() : 0);"
    "VolY= sum (alpha1 < 0.5 ? pos().y*vol() : 0);"    
    );        
    expression "VolY/Vol";
        accumulations (
        min        
        );

     
    }

Is there a way to compute these for two or three bubbles in this manner?

Thanks in advance,
Best Regards,
Arsalan.