|
[Sponsors] |
![]() |
![]() |
#1 |
Member
Join Date: Oct 2015
Posts: 63
Rep Power: 10 ![]() |
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: Code:
/*--------------------------------*- 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; // ************************************************************************* // Code:
/*--------------------------------*- 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 {} // ************************************************************************* // Scram_1 |
|
![]() |
![]() |
![]() |
![]() |
#2 |
New Member
Joseph Urich
Join Date: Mar 2009
Location: Pittsburgh, PA
Posts: 21
Rep Power: 17 ![]() |
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. |
|
![]() |
![]() |
![]() |
![]() |
#3 |
Member
Join Date: Oct 2015
Posts: 63
Rep Power: 10 ![]() |
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 |
|
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Stability and Realibility of microfluidic droplets storage in tube or storage coil | devalvyas | System Analysis | 0 | February 2, 2016 11:49 |
[Workbench] Simulate flow through filter with micron sized pores | FreeFall79 | ANSYS Meshing & Geometry | 1 | September 23, 2015 05:05 |
separation of water droplets from vapour using MPPIC Foam | arkadu | OpenFOAM Running, Solving & CFD | 1 | December 16, 2014 02:00 |
reactingFoam wedge handling wrong U | dhondupant | OpenFOAM Bugs | 1 | December 9, 2010 07:34 |
Number of Droplets per Cell | viv05 | OpenFOAM | 2 | August 11, 2009 02:35 |