[michaelb]

Hello Foamers,

I would like to know if there is a simple solver which could allow me to track a cloud of fluid particles ( size less : no drag & massless : no settling due to gravity) injected as a sphere of given position and diameter at t = 0 (only) with no initial velocity in an unsteady simulation.

Is there a way of doing such things with the icoLagrangianFoam solver in OpenFOAM-1.6-ext ? I couldn't figure out what would be the appropriate parameters in the kinematicCloudProperties dic file.

Actually, I need, for each saved timestep, the particles locations and their distances to wall patches.
If anybody could give me an hint on how to start here, I would be eternally thankful.

Best regards,

Michael

[BernhardGrieser]

Hi Michael,

I'm trying the same at the moment: Massless tracer particles. So far, I've only succeeded to load two particles in a cloud, and to write out their positions in an object file. Still fiddling around with the particle movement, though.
That's my code, so far:

vector position1(0.00005, 0.0001, 0.000995);
vector position2(0.00005, 0.0001, 0.001005);
label celli1 = mesh.findCell(position1);
label celli2 = mesh.findCell(position2);
Info<< "celli1 = mesh.findCell(position1) = " << celli1 << endl;
Info<< "celli2 = mesh.findCell(position2) = " << celli2 << endl;
const IDLList<passiveParticle>& particles();

passiveParticleCloud cloud(mesh, "cloud", particles);
cloud.clear();
passiveParticle* ptr1 = new passiveParticle(cloud, position1, celli1);
cloud.addParticle(ptr1);
passiveParticle* ptr2 = new passiveParticle(cloud, position2, celli2);
cloud.addParticle(ptr2);

cloud.writePositions();

Did you already solve the issue? Can somebody else help us?

Best Regards,
Bernhard

[BernhardGrieser]

one question would be, for example:

1.) How to address the cloud member function move()?

Compiling with

cloud.move();

returns the error message:

error: no matching function for call to 'Foam::passiveParticleCloud::move()'

2.) How to interpret the following warning message?

warning: the address of 'const Foam::IDLList<Foam::passiveParticle>& particles()' will always evaluate as 'true'

Cheers,
Bernhard

[francesco_capuano]

One guess for question #1: move is a member function of the base cloud class Cloud<ParticleType>, which is templated on particle type, see:

http://foam.sourceforge.net/docs/cpp...ce.html#l00181

You might try to define cloud as an object of Cloud<passiveParticle> and then try to call the move function.

Hope it helps,
Francesco

[BernhardGrieser]

Hi Francesco, thanks for the reply.

Originally Posted by francesco_capuano

You might try to define cloud as an object of Cloud<passiveParticle> and then try to call the move function.

My cloud was already defined as a passiveParticleCloud (see previous post). While instantiating, it calls the constructor of Cloud<passiveParticle>. But the member function move(TrackingData&) still cannot be called, probably because I don't know which argument it needs to be fed with. I probably address it the wrong way, since I'm not that familiar with template classes. Here's the move implementation:

template<class ParticleType>
template<class TrackingData>
void Foam::Cloud<ParticleType>::move(TrackingData& td)
{
    const globalMeshData& pData = polyMesh_.globalData();
    const labelList& processorPatches = pData.processorPatches();
    const labelList& processorPatchIndices = pData.processorPatchIndices();
    const labelList& processorPatchNeighbours =
        pData.processorPatchNeighbours();

    // Initialise the setpFraction moved for the particles
    forAllIter(typename Cloud<ParticleType>, *this, pIter)
    {
        pIter().stepFraction() = 0;
    }

    // Assume there will be particles to transfer
    bool transfered = true;

    // While there are particles to transfer
    while (transfered)
    {
        // List of lists of particles to be transfered for all the processor
        // patches
        List<IDLList<ParticleType> > transferList(processorPatches.size());

        // Loop over all particles
        forAllIter(typename Cloud<ParticleType>, *this, pIter)
        {
            ParticleType& p = pIter();

            // Move the particle
            bool keepParticle = p.move(td);

            // If the particle is to be kept
            // (i.e. it hasn't passed through an inlet or outlet)
            if (keepParticle)
            {
                // If we are running in parallel and the particle is on a
                // boundary face
                if (Pstream::parRun() && p.facei_ >= pMesh().nInternalFaces())
                {
                    label patchi = pMesh().boundaryMesh().whichPatch(p.facei_);
                    label n = processorPatchIndices[patchi];

                    // ... and the face is on a processor patch
                    // prepare it for transfer
                    if (n != -1)
                    {
                        p.prepareForParallelTransfer(patchi, td);
                        transferList[n].append(this->remove(&p));
                    }
                }
            }
            else
            {
                deleteParticle(p);
            }
        }

        if (Pstream::parRun())
        {
            // List of the numbers of particles to be transfered across the
            // processor patches
            labelList nsTransPs(transferList.size());

            forAll(transferList, i)
            {
                nsTransPs[i] = transferList[i].size();
            }

            // List of the numbers of particles to be transfered across the
            // processor patches for all the processors
            labelListList allNTrans(Pstream::nProcs());
            allNTrans[Pstream::myProcNo()] = nsTransPs;
            combineReduce(allNTrans, combineNsTransPs());

            transfered = false;

            forAll(allNTrans, i)
            {
                forAll(allNTrans[i], j)
                {
                    if (allNTrans[i][j])
                    {
                        transfered = true;
                        break;
                    }
                }
            }

            if (!transfered)
            {
                break;
            }

            forAll(transferList, i)
            {
                if (transferList[i].size())
                {
                    OPstream particleStream
                    (
                        Pstream::blocking,
                        refCast<const processorPolyPatch>
                        (
                            pMesh().boundaryMesh()[processorPatches[i]]
                        ).neighbProcNo()
                    );

                    particleStream << transferList[i];
                }
            }

            forAll(processorPatches, i)
            {
                label patchi = processorPatches[i];

                const processorPolyPatch& procPatch =
                    refCast<const processorPolyPatch>
                    (pMesh().boundaryMesh()[patchi]);

                label neighbProci =
                    procPatch.neighbProcNo() - Pstream::masterNo();

                label neighbProcPatchi = processorPatchNeighbours[patchi];

                label nRecPs = allNTrans[neighbProci][neighbProcPatchi];

                if (nRecPs)
                {
                    IPstream particleStream
                    (
                        Pstream::blocking,
                        procPatch.neighbProcNo()
                    );
                    IDLList<ParticleType> newParticles
                    (
                        particleStream,
                        typename ParticleType::iNew(*this)
                    );

                    forAllIter
                    (
                        typename Cloud<ParticleType>,
                        newParticles,
                        newpIter
                    )
                    {
                        ParticleType& newp = newpIter();
                        newp.correctAfterParallelTransfer(patchi, td);
                        addParticle(newParticles.remove(&newp));
                    }
                }
            }
        }
        else
        {
            transfered = false;
        }
    }
}

How can I interpret the TrackingData template? Since move expects its argument to be of Type TrackingData, which tracking data are valid, then?

Thanks

[francesco_capuano]

Maybe you already know it, anyway the following reference could be useful:

http://www.tfd.chalmers.se/~hani/kur...LPT_120911.pdf

Cheers,
Francesco

[michaelb]

Hi guys,

thanks for addressing the problem.
I've kept trying so far to use what is already implemented in the code and it really looks like that there are tons of material to deal with. ( Because I'm horrible at C++ coding... )
Unfortunately, I can't figure out what are meaning all the parameters available in a "kinematicCloudProperties" file.
I thought that I could specify a very low particle density leading me to a very small Stokes number therefore implying near to massless fluid particle tracking.
So until now, I've been playing around with the tutorials/lagrangian/icoLagrangianFoam/channelParticles of OpenFOAM-1.6-ext. Only three particles are injected at t=0, but are not moving unless I activate the gravity. Particles are then just settling downwards.

Here is my "kinematicCloudProperties" file :

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM Extend Project: Open Source CFD        |
|  \\    /   O peration     | Version:  1.6-ext                               |
|   \\  /    A nd           | Web:      www.extend-project.de                 |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      kinematicCloud1Properties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

active          yes;

InjectionModel  ManualInjection;

DragModel       none;

DispersionModel none;

PatchInteractionModel StandardWallInteraction;

PostProcessingModel none;

coupled         true;

cellValueSourceCorrection on;

parcelTypeId    2;

constantProperties
{
    rhoMin          rhoMin [ 1 -3 0 0 0 ] 1e-15;
    minParticleMass minParticleMass [ 1 0 0 0 0 ] 1e-15;
    rho0            rho0 [ 1 -3 0 0 0 ] 5000;
}

interpolationSchemes
{
    rho             cell;
    U               cellPoint;
    mu              cell;
}

integrationSchemes
{
    U               Euler;
}

particleForces
{
    gravity         off;
    virtualMass     off;
    pressureGradient off;
}

ManualInjectionCoeffs
{
    massTotal       massTotal [ 1 0 0 0 0 ] 0.0002;
    parcelBasisType mass;
    SOI             0;
    positionsFile   "kinematicCloudPositions";
    U0              ( 0 0 0 );
    parcelPDF
    {
        pdfType         RosinRammler;
        RosinRammlerPDF
        {
            minValue        5e-05;
            maxValue        0.0001;
            d               ( 7.5e-05 );
            n               ( 0.5 );
        }
    }
}

ConeInjectionCoeffs
{
    SOI             0.001;
    duration        0.005;
    position        ( 0.25 0.25 0.05 );
    direction       ( 0 -1 0 );
    parcelsPerSecond 10000;
    volumeFlowRate  Constant 0.01;
    Umag            Constant 50;
    thetaInner      Constant 0;
    thetaOuter      Constant 30;

    parcelPDF
    {
        pdfType         RosinRammler;
        RosinRammlerPDF
        {
            minValue        5e-05;
            maxValue        0.0001;
            d               ( 7.5e-05 );
            n               ( 0.5 );
        }
    }
}

StandardWallInteractionCoeffs
{
    type            rebound;
}

and the kinematicCloudPosition

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM Extend Project: Open Source CFD        |
|  \\    /   O peration     | Version:  1.6-ext                               |
|   \\  /    A nd           | Web:      www.extend-project.de                 |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       vectorField;
    object      kinematicCloud1Positions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
(
(0.05 0.025 0.005)
(0.05 0.05 0.005)
(0.05 0.075 0.005)
)

If nobody can give me an hint here, I think I'll just follow your way Bernhard...

Best,

Michael

[michaelb]

@Bernhard :
We might take advantage of the files associated with the pdf Francesco suggested :
http://www.tfd.chalmers.se/~hani/kur...olver_case.tgz

I'll have a look and keep you updated.

Best,

Michael

[BernhardGrieser]

Originally Posted by francesco_capuano

Maybe you already know it, anyway the following reference could be useful:

http://www.tfd.chalmers.se/~hani/kurser/OS_CFD/OF_kurs_LPT_120911.pdf

Cheers,
Francesco

Nice Didn't know that one, thanks!

Still stuck with the problem, though... I'll dive back in the code, then.

Cheers, Bernhard

[michaelb]

Hi Bernhard,

I managed to inject some particles with kinematicCloud classes in the pimpleFoam transient solver. Here's an example with around 5000 particles in a 3D lid-driven cavity. Works fine in parallel too. Tell me if you want me to share.

However, I'm still wondering about the kinematicCloudProperties file, and yet not sure whether I specified correct parameters for massless fluid particles.
The reason I'm doubting is that when I turn off the particleForces, particles aren't moving anymore. And much of the parameters are still very obscure to me.

I'm doubting whether I should start I new thread about the correct use of "kinematicCloudProperties". Would somebody be able to tell us a little bit more about it ?

Cheers,

Michael

[BernhardGrieser]

Originally Posted by michaelb

Tell me if you want me to share.

Hi Michael,

looks very promising, I'd like to have a look at your implementation, yes.

Meanwhile I succeeded in implementing my own particle tracking in a very simplistic approach. For my part, I only have a very small amount of tracer particles, so I do not take advantage of the stepwise particle tracking (stepFraction to next face, etc.) which was intended to avoid calling the mesh.findCell(position) for every particle at every timestep, from what I've understood.

Maybe you want to have a look at it:

// my solver C-file:

#include "fvCFD.H"
#include "volMesh.H"
#include "interpolationCellPoint.H"
#include "IFstream.H"
#include "OFstream.H"

int main(int argc, char *argv[])
{
    #include "setRootCase.H"
    #include "createTime.H"
    #include "createMesh.H"
    #include "createFields.H"
    #include "initContinuityErrs.H"

    // Load particle positions from dictionary

    IOdictionary particlePositionsDict
    (
        IOobject
        (
            "particlePositionsDict",
            runTime.timeName(),
            mesh,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        )
    );

    List<vector> particlePositions
    (
        particlePositionsDict.lookup("particlePositions")
    );

    // Initialize List for the interpolated particle velocity and the motion vector deltaX
    labelList particleCell(particlePositions.size());
    List<vector> Uint(particlePositions.size());
    List<vector> deltaX(particlePositions.size());

    // Initialize particleTracks
    std::fstream particleTracks;
    particleTracks.open("particleTracks",std::ios::out | std::ios::app);
    particleTracks << "#Time[s]\t\t";
    forAll(particlePositions, posI)
    {
        Info<< "    Position of particle #" << posI+1 << ": " << particlePositions[posI] << endl;
        particleTracks << "particle" << posI+1 << ".x()\t"
               << "particle" << posI+1 << ".y()\t"
               << "particle" << posI+1 << ".z()\t\t";
    }
    particleTracks << std::endl;

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

    Info<< "\nStarting time loop\n" << endl;

    while (runTime.loop())
    {
        Info<< "Time = " << runTime.timeName() << nl << endl;

        #include "readPISOControls.H"
        #include "CourantNo.H"
        
        scalar deltaT = runTime.deltaT().value();
        interpolationCellPoint<vector> UInt_(U);
        particleTracks << runTime.time().value() << "\t\t";

        forAll(particlePositions, posI)
        {
            particleCell[posI] = mesh.findCell(particlePositions[posI]);
            Uint[posI] = UInt_.interpolate(particlePositions[posI], particleCell[posI]);
            deltaX[posI] = Uint[posI]*deltaT;
            particlePositions[posI] += deltaX[posI];
            particleTracks << particlePositions[posI].x() << "\t"
                      << particlePositions[posI].y() << "\t"
                      << particlePositions[posI].z() << "\t\t";
        }

        particleTracks << std::endl;
...

Basically, I create a restartable log file for the particle positions at every timestep ("particleTracks") as well as a restartable dictionary in the respective time folder which contains the particle positions (particlePositionsDict).

The latter one looks like this:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.7.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "0";
    object      particlePositionsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

particlePositions
(
    (5e-05 0.0001 0.000993)
    (5e-05 0.0001 0.001013)
);

Best regards,
Bernhard

[michaelb]

Hello,

attached is what I've done without any guarantee .
I compiled it under OpenFOAM-2.0.1 and for some reason, it required some libraries that were buried deep into the source code.

I like your implementation since you have a total control of what you're doing. How many particles do you think you could track ? Is there a limitation implied by the format ?
Do you have any idea if this is quicker and more/less accurate than what I've done?
I would be very interested in the results if you do some comparison.

cheers,

Michael

[BernhardGrieser]

Originally Posted by michaelb

I like your implementation since you have a total control of what you're doing. How many particles do you think you could track ? Is there a limitation implied by the format ?

Hi Michael, the flaws of the simplistic approach are: nonparallel simulations only, particleTracks have to be transformed in order to be able to view them in paraview.

Thanks for your files, I'll check them.
Bernhard

[CFDUser_]

Originally Posted by francesco_capuano

Maybe you already know it, anyway the following reference could be useful:

http://www.tfd.chalmers.se/~hani/kurser/OS_CFD/OF_kurs_LPT_120911.pdf

Cheers,
Francesco

Dear Francesco,

This link is not working. May be it will be useful for me as well. Can you please re-upload.

Thanks

Regards
CFDUser_

[wyldckat]

Quick answer - The current link is this one: http://www.tfd.chalmers.se/~hani/kur...LPT_120911.pdf

[CFDUser_]

Originally Posted by wyldckat

Quick answer - The current link is this one: http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2011/OF_kurs_LPT_120911.pdf

Thanks for very quick and kind reply. Seems it will be very useful for me.

Regards
CFDUser_

[CFDUser_]

Dear All,

Can somebody post LPTVOF case files Michaelb said about?

Originally Posted by michaelb

@Bernhard :
We might take advantage of the files associated with the pdf Francesco suggested :
http://www.tfd.chalmers.se/~hani/kurser/OS_CFD/LPTVOF_solver_case.tgz

I'll have a look and keep you updated.

Best,

Michael

Thanks & Regards,
CFDUser_

[wyldckat]

Originally Posted by CFDUser_

Can somebody post LPTVOF case files Michaelb said about?

Quick answer: http://www.tfd.chalmers.se/~hani/kur...olver_case.tgz

PS: The course changes links with each new year: http://openfoamwiki.net/index.php/Ha...ource_software

[camzis]

Dear foamers,
I'm currently working with the solver "iconUncoupledKinematicParcelFoam (lagrangian)



I need to inject a different number of particles at each time step.
I'm currently using the model "patchInjection" in the file kinematicCloudProperties.
The problem is, I dont know how to make the number of particels vary.


Is there a way to force the number of particles to vary by wether providing a table (for number of particles vs. time) or as a function?


Any suggestions, ideas are very welcome.

Please, my master thesis depends on this.

[vonboett]

Hi Mamadou,
Did you find something? I am stuck at the same place. I implemented a write-out control such that I can write the particle position in a higher frequency than the fluid field variables, and I would start to implement the same for reading in from particlePosition files at predefined times- but I am shure someone has solved this before!