[Scram_1]

Hello everyone!
I'm working on evaporation of droplets and am using reactingFOAM as the solver. The evaporation of liquid droplets works well when the initial droplet size (set in reactingCloud1Properties) is greater than or equal to 6e-7. As soon as I decrease the size to 5e-7, all the injected particles evaporate i.e. the Mass transfer phase change is equal to the mass introduced in the domain. I'm quite certain that with the BCs and initial conditions remaining the same, decreasing the size from 6e-7 to 5e-7 should not cause the droplets to flash. I've used both liquidEvaporation and liquidEvaporationBoil models to test this anomaly. In both cases, the droplets disappear as soon as they are injected into the domain. Has anyone used evaporation models for droplet sizes 6e-7 and lower? Is this a problem with how openFOAM injection / evaporation models work? I'm using patch injection of droplets into the domain if that helps in any way to solve this problem.

thermoPhysicalProperties:

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

thermoType
{
    type            heRhoThermo;
    mixture         multiComponentMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}



air
{
    specie
    {
        molWeight       28.85;
    }
    equationOfState
    {

		pRef	1e5;
    }
    thermodynamics
    {
         Cp              1004.5; 
         Hf              0;
    }
    transport
    {
        mu            1.8e-05; 
        Pr              0.7; 
    }
}

H2O
{
    specie
    {
        molWeight       18.0153;
    }
    equationOfState
    {
		pRef	1e5;
    }
    thermodynamics
    {
         Cp              4187; 
         Hf              -13423000;
    }
    transport
    {
        mu              8.9e-4; 
        Pr              7; 
    }
}

species
(
    air
    H2O

);


inertSpecie     air;

liquids
{
    H2O;
}

solids
{}

// de-activate the pressure-work term when running local time-stepping
dpdt            no;


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

reactingCloud1Properties:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  plus                                  |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      reactingCloud1Properties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solution
{
    active          true;

    transient       yes; // yes;
    calcFrequency   10;
    maxCo           0.3;

    coupled         true;
    cellValueSourceCorrection off;

    sourceTerms
    {
        resetOnStartup  false;
        schemes
        {
            rho             semiImplicit 1;
            U               semiImplicit 1;
            Yi              semiImplicit 1;
            h               semiImplicit 1;
            radiation       semiImplicit 1;
        }
    }

    interpolationSchemes
    {
        rho             cell;
        U               cellPoint;
        thermo:mu       cell;
        T               cell;
        Cp              cell;
        kappa           cell;
        p               cell;
    }

    integrationSchemes
    {
        U               analytical;//Euler;
        T               analytical;
    }
}


constantProperties
{
    rho0            1000;
    T0              310.5;
    Cp0             4100;

    constantVolume  false;
}


subModels
{
    particleForces
    {
        sphereDrag;
        gravity;
    }

    injectionModels
    {
        model1
        {
            type            patchInjection;
            parcelBasisType fixed;
			massTotal  0;
            patch           INLET;
            nParticle       10;
            parcelsPerSecond 1e9;
			SOI 0;
            duration        1e-6; // NOTE: set to 1 for steady state
            U0              (0 0 0);
            flowRateProfile constant 1;
			
        sizeDistribution
            {
                type        fixedValue;
                fixedValueDistribution
                {
                    value   5e-07;
                }
            }
        }
    }

    dispersionModel stochasticDispersionRAS;

    patchInteractionModel standardWallInteraction;

    heatTransferModel RanzMarshall;

    compositionModel singleMixtureFraction;

    phaseChangeModel myLiquidEvaporation;

    devolatilisationModel none;

    surfaceReactionModel none;

    stochasticCollisionModel none;

    surfaceFilmModel none;

    radiation       off;

    standardWallInteractionCoeffs
    {
        type            rebound;
    }

    RanzMarshallCoeffs
    {
        BirdCorrection  off;
    }

    singleMixtureFractionCoeffs
    {
        phases
        (
            gas
            {
            }
            liquid
            {
				H2O 1;
            }
            solid
            {
            }
        );
        YGasTot0        0;
        YLiquidTot0     1;
        YSolidTot0      0;
    }

    myLiquidEvaporationCoeffs
    {
        enthalpyTransfer enthalpyDifference;
        activeLiquids   ( H2O );
    }
}


cloudFunctions
{}

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

Best,
Scram_1

[jurich]

Hello Scram_1,

OpenFOAM has a lower limit on parcel mass, below which the parcel mass is transferred immediately. It is minParcelMass, and it defaults to 1E-15. That may be what causes your issue.

You can change it by adding:

minParcelMass 1e-20;

to the constantProperties dictionary.

You can see how it works in ReactingMultiphaseParcel.C, around line 344 depending on the version, search for minParcelMass.

Hope that helps.

[Scram_1]

Thanks Joseph!
That helped. I have another problem when it comes to injecting parcels. As I mentioned earlier, I use patch injection to inject parcels into the domain. Now, my time step is 1e-8 and I want to inject 1000 parcels all at once i.e. my SOI is 0 and my duration 1e-8 (The small time step is to capture certain phenomena exhibited by sub micron droplets). For this, I need to keep my parcelsPerSecond as 1e11. However, when I increase my parcelsPerSecond beyond 1e9, it crashes. Do you have any idea about this? I checked reactingMultiphaseParcel and kinematicParcel but there is no mention of this.
Thanks again!

Best,
Scram_1