[mehtab]

Hi,

I tried implementing temperature boundary condition at Inlet as:

T_s = T_0 + 1/C_p(Q_f/m" - Hv)


Here is my files

boundaryField
{
    outlet
    {
        type            inletOutlet;
        inletValue      uniform 298.15;
        value           uniform 298.15;
    }
    sides
    {
        type            inletOutlet;
        inletValue      uniform 298.15;
        value           uniform 298.15;
    }
    base
    {
        type            zeroGradient;
    }
    inlet
    {
    type                          groovyBC;
    valueExpression        "T0+((1/cpi)*((Qf/m)-Hv))";
    variables                  "T0=300;m{inlet}=phi;Hv=8500;Qf{inlet}=Qr;cpi{inlet}=cp;";
    value                        300;

    }

controlDict

application     fireFoam;

startFrom       startTime;

startTime       0.0;

stopAt          endTime;

endTime         1.0;

deltaT          1.0e-2;

writeControl    adjustableRunTime;

writeInterval   0.01;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression uncompressed;

timeFormat      general;

timePrecision   6;

graphFormat     raw;

runTimeModifiable yes;

adjustTimeStep  yes;

maxCo           0.6;

maxDeltaT       0.1;

functions
{
    fieldAverage
    {
        type            fieldAverage;
        functionObjectLibs ( "libfieldFunctionObjects.so" );
        enabled         true;
        outputControl   outputTime;

        fields
        (
              U
              {
                  mean on;
                  prime2Mean on;
                  base time;
              }
          T
              {
                  mean on;
                  prime2Mean on;
                  base time;
              }
          CH4
              {
                  mean on;
                  prime2Mean on;
                  base time;
              }
          CO2
              {
                  mean on;
                  prime2Mean on;
                  base time;
              }
          H2O
              {
                  mean on;
                  prime2Mean on;
                  base time;
              }
          O2
              {
                  mean on;
                  prime2Mean on;
                  base time;
              }
        );
    }

libs (
    "libOpenFOAM.so"
    "libgroovyBC.so"
    "libgroovyStandardBCs.so"
    "libsimpleFunctionObjects.so"
    "libsimpleSwakFunctionObjects.so"
    "libswakFunctionObjects.so"
    "libswakPythonIntegration.so"
    "libswakTransportTurbFunctionPlugin.so"
) ;

I also checked my solver fireFoam createFields.H to check how Cp is being used.

createFields.H

volScalarField cp
    (
        IOobject
        (
            "cp",
            runTime.timeName(),
            mesh,
            IOobject::MUST_READ,
            IOobject::AUTO_WRITE
        ),
        thermo.Cp()
    );

I am getting this error:

swak4Foam: Setting default mesh
swak4Foam: Allocating new repository for sampledGlobalVariables
--> FOAM Warning : 
    From function ConcretePluginFunction<DriverType>::exists
    in file lnInclude/ConcretePluginFunction.C at line 121
    Constructor table of plugin functions for PatchValueExpressionDriver is not initialized


--> FOAM FATAL ERROR: 
 Parser Error for driver PatchValueExpressionDriver at "1.1-2" :"field Qr not existing or of wrong type"
"Qr"
  ^^
--| 

Context of the error:


- Driver constructed from scratch
  Evaluating expression "Qr"


    From function parsingValue
    in file lnInclude/CommonValueExpressionDriverI.H at line 1189.

FOAM exiting

What should I modify in me expressions? Have I defined cp correctly or should I change to thermo.Cp? Here Qr is totat radiative flux being calculated through radiation model. I am not able to understand the error. Please help

Thanks in advance....

[ Moderator note: moved from http://www.cfd-online.com/Forums/ope...-values-2.html ]

[mehtab]

Hi,

Is it possible to access field variables (mass flow, temperature, heat flux) in groovyBC? If yes then how?

Please help

Thanks

[wyldckat]

Greetings firefoam,

I've had your questions on my to-do list for quite sometime now and only today did I finally manage to come to it .

The first issue I'm not able to reproduce. I used the tutorial case "combustion/fireFoam/les/smallPoolFire2D" as a test case for this and tried this condition:

    inlet
    {
      type                          groovyBC;
      valueExpression            "T0+(Qf/m)";
      variables                  "T0=300;m=phi;Qf=Qr;";
      value                        300;
    }

It worked fine without any problems. For future reference, I used OpenFOAM 2.4.x and swak4Foam 0.3.2.

I'm guessing the second question is related to the same problem, therefore I would need more details in order to be able to answer better to your question, because access to the "T" field should be straight forward and the other calculations could perhaps be achieved by using what's shown here: http://www.cfd-online.com/Forums/ope...tml#post446085 - post #5.

Best regards,
Bruno

[mehtab]

Dear Bruno,

Thank you very much for looking at my problem. I also checked with OF 2.4.0 and swak4Foam 0.3.2. I took smallpoolfire3D tutorial case in OpenFoam.

First I defined my boundary condition exactly same as you and it was working fine. Then I added Cp term into my equation as below.

inlet
    {
        type                          groovyBC;
        valueExpression            "T0+1/Cp*(Qf/m)";
      	variables                  "T0=300;m=phi;Qf=Qr;";
      	value                        300;
    }

But in this case the solver does not recognise Cp as mentioned in the valueExpression and gives error.

I referred to the link provided by you : http://www.cfd-online.com/Forums/ope...tml#post446085

I have added the following piece of code into my controlDict and try to run the tutorial.

loadThermo {
    type loadPsiThermoModel;
    correctModel false;
    //        correctModel true;
    allowReload false;
    failIfModelTypeExists false;
    outputControl timeStep;
    outputInterval 1;
}

cvField {
    type expressionField;
    autowrite false;
    outputControl timeStep;
    outputInterval 1;
    expression "thermo_Cv()";
    fieldName CRRv;
}

cpField {
    type expressionField;
    autowrite false;
    outputControl timeStep;
    outputInterval 1;
    expression "thermo_Cp()";
    fieldName CRRp;
}

My error is below:

--> FOAM FATAL ERROR:
Parser Error for driver PatchValueExpressionDriver at "1.6-9" :"field CRRp not existing or of wrong type"
"T0+1/CRRp*(Qf/m)"
^^^^
-------|

Context of the error:


- From dictionary: /home/maqsood/OpenFOAM/maqsood-2.4.0/tutorials/combustion/fireFoam/les/smallPoolFire3D/0/T.boundaryField.inlet
Evaluating expression "T0+1/CRRp*(Qf/m)"


From function parsingValue
in file lnInclude/CommonValueExpressionDriverI.H at line 1189.

FOAM exiting

Please suggest where I am doing it wrong.

Thanks

[mehtab]

Dear Bruno and Ehsan,

I am facing the same problem from quite a long time. But after reading this thread, I realized that I might be missing some functions in my controlDict file.

I am attaching my controlDict file and Temperature Boundary condition file where I am using groovyBC.

PS: Bruno, I have referred to your post http://www.cfd-online.com/Forums/ope...-groovybc.html #3 and http://www.cfd-online.com/Forums/ope...-values-2.html #39. I read the full post and think that I must be missing some functions in my controlDict file That is why I am attaching it to have a look for you. Please look at the files. Your guidance will be really helpful.
My error message reads as below:

--> FOAM FATAL ERROR:
Parser Error for driver PatchValueExpressionDriver at "1.1-6" :"field thermo not existing or of wrong type"
"thermo:cp()"
^^^^^^
--|

Context of the error:


- From dictionary: /home/maqsood/OpenFOAM/maqsood-2.4.0/tutorials/combustion/fireFoam/les/smallPoolFire3D/0/T.boundaryField.inlet
Evaluating expression "thermo:cp()"


From function parsingValue
in file lnInclude/CommonValueExpressionDriverI.H at line 1189.

FOAM exiting

For the information I am using OF2.4.0 with swak4Foam0.3.2 and I am trying to solve the tutorial case of fireFoam :smallpoolfire3D.

Thanks in advance.


[ Moderator note: Moved from http://www.cfd-online.com/Forums/ope...-values-2.html ]

[wyldckat]

Quick answer: Please provide the complete "system/controlDict" file. I suspect something might be out-of-place and I can't guess what it is without seeing the full contents of the file.

[mehtab]

Dear Bruno,

Please find attached my system/controlDict file and Temperature boundary condition file where I am using groovyBC.



Thanks in advance
Maqs

[wyldckat]

Quick answer: My guess was right, you defined the function objects in the wrong place. In theory, the correct content for "controlDict" is this:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.4.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version         2.0;
    format          ascii;
    class           dictionary;
    object          controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     fireFoam;

startFrom       startTime;

startTime       0.0;

stopAt          endTime;

endTime         4.0;

deltaT          0.001;

writeControl    adjustableRunTime;

writeInterval   0.1;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression uncompressed;

timeFormat      general;

timePrecision   6;

graphFormat     raw;

runTimeModifiable yes;

adjustTimeStep  yes;

maxCo           0.6;

maxDeltaT       0.1;



libs (
    "libgroovyBC.so"
    "libsimpleFunctionObjects.so"
    "libsimpleSwakFunctionObjects.so"
    "libswakFunctionObjects.so"
    "libgroovyStandardBCs.so"
    "libswakThermoTurbFunctionPlugin.so"
);

functions
{

    loadThermo
    {
        type loadpsiThermoModel;
        correctModel false;
        //correctModel true;
        allowReload false;
        failIfModelTypeExists false;
        outputControl timeStep;
        outputInterval 1;
    }

    CvField
    {
            type expressionField;
            dimension [0 2 -2 -1 0 0 0];
            autowrite false;//false;
            outputControl timeStep;
            outputInterval 1;
            expression "thermo:Cv()";
            fieldName CRRv;
    }

    CpField
    {
            type expressionField;
            dimension [0 2 -2 -1 0 0 0];
            autowrite false;//false;
            outputControl timeStep;
            outputInterval 1;
            expression "thermo:Cp()";
            fieldName CRRp;
    }
  
}

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

It feels like you didn't take good look into the tutorial cases that OpenFOAM has got for function objects. This is also explained in the OpenFOAM User Guide, section 6.2: http://cfd.direct/openfoam/user-guide/function-objects/

[mehtab]

Dear Bruno,

Thank you very much for your support and guidance. I understood from this discussion that "loadPsiThermoModel" will provide all the fields which are defined in createField as thermo.p or thermo.T or thermo.psi etc. (mentioned in below code RoyalBlue color)

createFields.H

Info<< "Creating combustion model\n" << endl;

autoPtr<combustionModels::psiCombustionModel> combustion
(
    combustionModels::psiCombustionModel::New
    (
        mesh
    )
);

Info<< "Reading thermophysical properties\n" << endl;

psiReactionThermo& thermo = combustion->thermo();
thermo.validate(args.executable(), "h", "e");

SLGThermo slgThermo(mesh, thermo);

basicMultiComponentMixture& composition = thermo.composition();
PtrList<volScalarField>& Y = composition.Y();

const word inertSpecie(thermo.lookup("inertSpecie"));

Info<< "Creating field rho\n" << endl;
volScalarField rho
(
    IOobject
    (
        "rho",
        runTime.timeName(),
        mesh,
        IOobject::NO_READ,
        IOobject::AUTO_WRITE
    ),
    thermo.rho()
);

volScalarField& p = thermo.p();
const volScalarField& T = thermo.T();
const volScalarField& psi = thermo.psi();

However if I want to access the value of mass concentration of a particular species eg CH4 in this tutorial case for modifying velocity BC, I cannot get it from this function "loadPsiThermoModel". I think the reason is that this multicomponent specie fraction is defined in a different way as shown below.

Info<< "Creating combustion model\n" << endl;

autoPtr<combustionModels::psiCombustionModel> combustion
(
    combustionModels::psiCombustionModel::New
    (
        mesh
    )
);

Info<< "Reading thermophysical properties\n" << endl;

psiReactionThermo& thermo = combustion->thermo();
thermo.validate(args.executable(), "h", "e");

SLGThermo slgThermo(mesh, thermo);

basicMultiComponentMixture& composition = thermo.composition();
PtrList<volScalarField>& Y = composition.Y();

Is there any way to access mass concentration of a particular specie in groovyBC using swak4Foam?

CH4Field
    {
            type expressionField;
            dimension [0 0 0 0 0 0 0];
            autowrite false;//false;
            outputControl timeStep;
            outputInterval 1;
            expression "thermo_composition()";
            fieldName Ych4;
    }

I tried this but did not succeed and getting errors. I tried loading other functions as well but no success. I think I am not using the correct function to load species mass concentration.

Please suggest.

Thanks
Maqs

[wyldckat]

Quick answer: If the CH4 field is registered in memory and accessible from the outside, it will show up when you test this function object: http://openfoamwiki.net/index.php/Ti...gisteredObject

[mehtab]

Dear Bruno,

Thanks a lot for you help and suggestions. With your help, my temperature boundary condition is working now.

But I tried to implement groovyBC for velocity BC using CH4 field only and this is not running and shows error. It is not calculating the velocity in first iteration only and stops just after rho calculations.

My controlDict file looks fine now. I think the problem is in U file only while defining groovyBC. I have attached the file for your reference. Please suggest, if you point out any error or mistake in files.

Thanks
Maqs

[Scram_1]

Hi Mehtab,
Did you manage to fix your issue? If yes, then can you share your solution?
I'm facing a similar problem where my variable is not getting updated with time if I use groovyBC.

Best,
Scram_1