[Jimmy Chokshi]

Originally Posted by ziemowitzima

Hi,
Give me your email, I will send you the working case with few words of explanations.
I would attached it here, but size of the file seems to be too large (1.4MB), and I could not attached it to my reply.

best

Hi,

Can you please send this working case to chokshirl@gmail.com ?

Many thanks !!

[Jimmy Chokshi]

Hi,

Can you please send this working case to chokshirl@gmail.com ?

Many thanks !!

[HVonSch]

Hello everyone,


I had the same problem (multi-fluid-mixing flow, single phase, compressible, stationary).

I combined rhoSimpleFoam and reactingFoam to a new solver, which integrates in rhoSimpleFoam.
I called it rhoMixingSimpleFoam. It is attached to this post.


EDIT: Please keep in mind, that this solver is not well tested or validated in any way!
Also: In this solver the turbulent species transport is modelled via alphat and is thus equal to the turbulent heat fluxes. This is not always the case!



Installation:
Just copy the dir "rhoMixingSimpleFoam" to the rhoSimpleFoam-directory (/path_to_Openfoam/applications/solvers/compressible/rhoSimpleFoam/), enter it and run wmake.


Also attached is the following thermophysicalProperties which is used by this solver:

thermoType
{
    type            heRhoThermo;
    mixture         multiComponentMixture;
    transport       sutherland;
    thermo          janaf;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

inertSpecie air;

species (air CO2);

air
{
    specie
    {
        nMoles          1;
        molWeight       28.965; // (refprop)
    }
    equationOfState
    {
        pRef            1e6;
    }
    thermodynamics
    {
        Tlow            200;
        Thigh           6000;
        Tcommon         1000;
        highCpCoeffs    ( 3.08792717E+00 1.24597184E-03 -4.23718945E-07 6.74774789E-11 -3.97076972E-15 -9.95262755E+02 5.95960930E+00 );
        lowCpCoeffs     ( 3.56839620E+00 -6.78729429E-04 1.55371476E-06 -3.29937060E-12 -4.66395387E-13 -1.06234659E+03 3.71582965E+00 );
        // no source, sorry
    }
    transport
    {
        As          1.460846342e-06; // (White - Viscous Fluid Flow)
        Ts          111;
    }
}

CO2
{
    specie
    {
        nMoles          1;
        molWeight       44.01; // (refprop)
    }
    equationOfState
    {
        pRef            1e6;
    }
    thermodynamics
    {
        Tlow            200;
        Thigh           3500;
        Tcommon         1000;
        highCpCoeffs    ( 3.85746029E+00 4.41437026E-03 -2.21481404E-06 5.23490188E-10 -4.72084164E-14 -4.87591660E+04 2.27163806E+00 );
        lowCpCoeffs     ( 2.35677352E+00 8.98459677E-03 -7.12356269E-06 2.45919022E-09 -1.43699548E-13 -4.83719697E+04 9.90105222E+00 );
         //http://combustion.berkeley.edu/gri-mech/data/nasa_plnm.html
    }
    transport
    {
        As              1.503425096e-06; // (White - Viscous Fluid Flow)
        Ts              222;
    }
}

[KAMAL KHEMANI]

Originally Posted by HVonSch

Hello everyone,


I had the same problem (multi-fluid-mixing flow, single phase, compressible, stationary).


I combined rhoSimpleFoam and reactingFoam to a new solver, which integrates in rhoSimpleFoam.
I called it rhoMixingSimpleFoam. It is attached to this post.


Just copy the dir "rhoMixingSimpleFoam" to the rhoSimpleFoam-directory (/path_to_Openfoam/applications/solvers/compressible/rhoSimpleFoam/), enter it and run wmake.


Also attached is the following thermophysicalProperties which is used by this solver:

thermoType
{
    type            heRhoThermo;
    mixture         multiComponentMixture;
    transport       sutherland;
    thermo          janaf;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

inertSpecie air;

species (air CO2);

air
{
    specie
    {
        nMoles          1;
        molWeight       28.965; // (refprop)
    }
    equationOfState
    {
        pRef            1e6;
    }
    thermodynamics
    {
        Tlow            200;
        Thigh           6000;
        Tcommon         1000;
        highCpCoeffs    ( 3.08792717E+00 1.24597184E-03 -4.23718945E-07 6.74774789E-11 -3.97076972E-15 -9.95262755E+02 5.95960930E+00 );
        lowCpCoeffs     ( 3.56839620E+00 -6.78729429E-04 1.55371476E-06 -3.29937060E-12 -4.66395387E-13 -1.06234659E+03 3.71582965E+00 );
        // no source, sorry
    }
    transport
    {
        As          1.460846342e-06; // (White - Viscous Fluid Flow)
        Ts          111;
    }
}

CO2
{
    specie
    {
        nMoles          1;
        molWeight       44.01; // (refprop)
    }
    equationOfState
    {
        pRef            1e6;
    }
    thermodynamics
    {
        Tlow            200;
        Thigh           3500;
        Tcommon         1000;
        highCpCoeffs    ( 3.85746029E+00 4.41437026E-03 -2.21481404E-06 5.23490188E-10 -4.72084164E-14 -4.87591660E+04 2.27163806E+00 );
        lowCpCoeffs     ( 2.35677352E+00 8.98459677E-03 -7.12356269E-06 2.45919022E-09 -1.43699548E-13 -4.83719697E+04 9.90105222E+00 );
         //http://combustion.berkeley.edu/gri-mech/data/nasa_plnm.html
    }
    transport
    {
        As              1.503425096e-06; // (White - Viscous Fluid Flow)
        Ts              222;
    }
}

Hi HVonSch, with laminar conditions the temperature shoots up at very high value any reason for that ?

[HVonSch]

Hello Kamal,

Is the simulation fully converged?
Please provide more information about your case and the way you are using the species mixing (species, phases) to track down if the error is caused by the solver modification.


Best regards,
Hendrik

[petr.f.]

Hi Hendrik, I'm checking out your solver (nice work btw.). How do you prescribe boundary conditions for the individual species? Is it in the same way as in case of reactingFoam i.e. by individual files in constant/ dir as e.g. "air" and "CO2"?

[HVonSch]

Hello Petr,


thank you!


Yes, BCs are prescribed as in reactingFoam.


For example for CO2:

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      CO2;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    INLET
    {
        type            fixedValue;
        value           uniform 0;
    }
    OUTLET
    {
        type            inletOutlet;
        value           uniform 0;
        inletValue      uniform 0;
    }
    PLENUM_INLET
    {
        type            fixedValue;
        value           uniform 1;
    }
    PLENUM_OUTLET
    {
        type            inletOutlet;
        value           uniform 1;
        inletValue      uniform 1;
    }
    WALL
    {
        type            zeroGradient;
    }
}


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

You don't need a BC-file for the "inert species" as its fraction is just 1-sum(other species fractions).


Best,
Hendrik

[nikhil108]

Hallo Foamers,

can you suggest me a solver for, propane jet leak in to air. Right now, i am using reactingbuoyantfoam, but i want to add dynamic mesh, which is not supported by reactingFoam. any suggestions?.

cheers,
nm.