[jango]

Dear community,

I'm currently trying to solve the cyclone case with a lower outlet using simpleReactingParcelFoam for a steady-state case with lagrangian particle tracking. As for a first step I modified the verticalChannel tutorial case to the cyclone boundaries with it's standard thermophysical model and ajusted it to my flow rate, but unfortunately it's diverging after 20 iterations throwing out the following error message:

Maximum number of iterations exceeded: 100

Checking the results, the particles get injected, and according to the log file, there's a mass flow through both outlets. I guess, that there's some error on my boundary conditions regarding the outlets, as in the verticalChannel case the particle/gas concentration is known and set to a sum of 1 at a single outlet.

In my case I have two outlets and want the solver to calculate the concentration accordingly. Does anybody know the correct settings for the outlet for this case ?

Attached to this post I'll send you my boundary settings for the initial fields, maybe that helps.

Thank you in advance,

Jan

[jango]

Unfortunately I still couldn' t spot out the error. If I run the case with the default thermophysical properties from the verticalChannel tutorial case it's still diverging. Checking out the output for pmin/pmax it can be observed, that the pressure field diverges.

When I change the material properties to my own created thermophysical properties, I get the error message, that specie- keyword is not defined (even though it is)

[kcjarvis56]

The phaseChangeModel in the reactingCloudProperties is set to liquid evaporation. Look at the air flows at the inlet along mass rates of reacting cloud are ratio'ed correctly or it will blow up quickly. You can use none for the phaseChangeModel which may help you get to a running model quick then add the evaporation model if you need it. As far as using your properties it doesn't appear you are using the right thermoType mixture for the solver. I didn't have any luck using multiComponetMixture, it needed to be reactingMixture. Also the error message regarding specie (with your own properties), since you are not using the reactingMixture (as mentioned above) it doesn't read the foamChemistryFiles files you need to put all the information in the thermophysicalProperites file.

For example:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5                                     |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

thermoType
{
    type            heRhoThermo;
    mixture         multiComponentMixture; // couldn't get to work with simpleReactingParcelFoam
    transport       const;
    thermo          hConst;
    equationOfState incompressiblePerfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

//chemistryReader foamChemistryReader;

//foamChemistryFile "$FOAM_CASE/constant/reactions";

//foamChemistryThermoFile "$FOAM_CASE/constant/thermo.incompressiblePoly";

inertSpecie     air;

liquids
{
    H2O;
}

solids
{}

species
(
    air
    H2O
);

H2O
{
    specie
    {
        nMoles          1;
        molWeight       18.0153;
        pRef            100000;
    }
    equationOfState
    {
        pRef            100000;
    }
    
    thermodynamics
    {
        Cp              4310;
        Hf              6.3225e+05;
    }
    transport
    {

        mu              1.825e-04;
        Pr              1.15;
    }
}

air
{
    specie
    {
        nMoles          1;
        molWeight   18.0153;
        pRef            100000;
    }
    equationOfState
    {
        pRef            100000;
    }

    thermodynamics
    {
//        Cp              1007;
        Cp          2396;
//        Hf              2.257e+06;
        Hf          2.7459e+06;
    }
    transport
    {
//        mu              1.41e-05;
        mu          1.399e-05;
//        Pr              1;
        Pr          1.089;
    }
}




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

Hope this helps.

[jango]

Hello Kirk,

thank you for your reply. I finally managed to run my own case by adjusting it to the proper material properties using the standard-steam tables. I also switched off the phase change modell to "none" as the only thing which is needed is the information about the particle behaviour at the wall. Unfortuntely by running different models varying the coefficients of e and mu for the wall behaviour there are no changes regarding the particle masses leaving and remaining into the vessel. It seems that this coefficients doesn't have any effect... Is there a good documentation available for the reactingCloud1Properties dict anywhre available- I've searched the web but couldn't find anything suitable.

Have a nice day,

Jan