[NBad]

Hi everyone, I have a funny challange for you!

I'm performing a thermal simulation on a component using chtMultiregionFOAM and need to implement on a boundary surface of one of the solids a particular boundary condition, which is a heat flux which is dependent on the temperature of the surface itself.

In particular I need to apply on this patch the following boundary condition:

so that a heat flux dependent on the surface temperature is extracted from the surface itself.

I was thinking to do that with scalarCodedSource, but I don't even know from where to start, any idea??

Is it even possible to do that with the codedSource or do I need to implement from scratch a whole new boundary condition?

Thanks in advance for your replies!

[crubio.abujas]

Hi NBad,

Try with codedMixed. You didn't mention if the patch should be attached into a solid region or a fluid one, that will affect to the thermal conductivity (kappa in the code). You need the thermal conductivity because you cannot apply directly a heat flux, you need to tell a gradient of T, which is the meaningful variable, and this factor is required for conversion.

I've attached a version for a solid region. In case you want to apply it to a fluid one you may need to change the way to get the thermo property (rather use the fluid properties themselves, or use the effective ones given by the turbulent model).


Try the code and let me know if it worked for you!

    <patchName>
    {
        type            codedMixed;
        value           uniform 300;
        name            temperatureHeatFlux;
        refValue        uniform 600;       
        refGradient     uniform 0;      
        valueFraction   uniform 0;      //1 - Dirictlect ;  0 - Neumann

    code
    #{
        // Get the basic thermo properties (for solid region)
        const solidThermo& thermo =
            db().lookupObject<solidThermo>(basicThermo::dictName);


        // Get current patchi
        const label patchi = patch().index();

        // This is the temperature of current patch
        const scalarField& Tp(*this);
        
        // Constant of the equation
        const scalar C1 = 1;
        const scalar C2 = 0;

        // Calculate the values on each face of the patch
        // Note: Eq is divided by thermal conductivity to units of grad(T)
        this->refGrad() = C1*pow(Tp, 2)*pow(M_E, C2*Tp)/thermo.kappa(patchi);

        bool debug = true;  
        if (debug) {
            Info << "Evaluating temperatureHeatFlux on " << patch().name() << endl;
            Info << "temperatureHeatFlux::average(Tp)  = " << gAverage(Tp) << " K" << endl;
            Info << "temperatureHeatFlux::average(Q) = " 
                 << gAverage(this->refGrad()*thermo.kappa(patchi)) << " W/m2K"
                 << endl << endl;
        }
    #};

    codeInclude
    #{
        #include "solidThermo.H"
    #};

    codeOptions
    #{
        -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
        -I$(LIB_SRC)/thermophysicalModels/solidThermo/lnInclude \
    #};

    }

[GiaQ]

Originally Posted by crubio.abujas

Hi NBad,

Try with codedMixed. You didn't mention if the patch should be attached into a solid region or a fluid one, that will affect to the thermal conductivity (kappa in the code). You need the thermal conductivity because you cannot apply directly a heat flux, you need to tell a gradient of T, which is the meaningful variable, and this factor is required for conversion.

I've attached a version for a solid region. In case you want to apply it to a fluid one you may need to change the way to get the thermo property (rather use the fluid properties themselves, or use the effective ones given by the turbulent model).


Try the code and let me know if it worked for you!

    <patchName>
    {
        type            codedMixed;
        value           uniform 300;
        name            temperatureHeatFlux;
        refValue        uniform 600;       
        refGradient     uniform 0;      
        valueFraction   uniform 0;      //1 - Dirictlect ;  0 - Neumann

    code
    #{
        // Get the basic thermo properties (for solid region)
        const solidThermo& thermo =
            db().lookupObject<solidThermo>(basicThermo::dictName);


        // Get current patchi
        const label patchi = patch().index();

        // This is the temperature of current patch
        const scalarField& Tp(*this);
        
        // Constant of the equation
        const scalar C1 = 1;
        const scalar C2 = 0;

        // Calculate the values on each face of the patch
        // Note: Eq is divided by thermal conductivity to units of grad(T)
        this->refGrad() = C1*pow(Tp, 2)*pow(M_E, C2*Tp)/thermo.kappa(patchi);

        bool debug = true;  
        if (debug) {
            Info << "Evaluating temperatureHeatFlux on " << patch().name() << endl;
            Info << "temperatureHeatFlux::average(Tp)  = " << gAverage(Tp) << " K" << endl;
            Info << "temperatureHeatFlux::average(Q) = " 
                 << gAverage(this->refGrad()*thermo.kappa(patchi)) << " W/m2K"
                 << endl << endl;
        }
    #};

    codeInclude
    #{
        #include "solidThermo.H"
    #};

    codeOptions
    #{
        -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
        -I$(LIB_SRC)/thermophysicalModels/solidThermo/lnInclude \
    #};

    }

If I just want to use dt/dx = q/kappa, should I put the refValue = 0 ?

[crubio.abujas]

Hi Giacomo,


As soon as you use valueFraction = 0 the refValue will be ignored so it doesn't matter which value you use.


If you need further information about what means each term you can check the info in the source code.

[dhiraj kumar]

hello everyone. I have a solar receiver in which at outer surface of the receiver i have to apply non-uniform heat flux [cosine profile - q(θ) = qnet ·
cos θ(−90 ≤ θ ≤ 90)] with radiation and convection losses to ambient. can anyone give me the idea for writing the UDF for ansys fluent for this condition. thanks !

[NBad]

Originally Posted by crubio.abujas

Hi NBad,

Try with codedMixed. You didn't mention if the patch should be attached into a solid region or a fluid one, that will affect to the thermal conductivity (kappa in the code). You need the thermal conductivity because you cannot apply directly a heat flux, you need to tell a gradient of T, which is the meaningful variable, and this factor is required for conversion.

I've attached a version for a solid region. In case you want to apply it to a fluid one you may need to change the way to get the thermo property (rather use the fluid properties themselves, or use the effective ones given by the turbulent model).


Try the code and let me know if it worked for you!

    <patchName>
    {
        type            codedMixed;
        value           uniform 300;
        name            temperatureHeatFlux;
        refValue        uniform 600;       
        refGradient     uniform 0;      
        valueFraction   uniform 0;      //1 - Dirictlect ;  0 - Neumann

    code
    #{
        // Get the basic thermo properties (for solid region)
        const solidThermo& thermo =
            db().lookupObject<solidThermo>(basicThermo::dictName);


        // Get current patchi
        const label patchi = patch().index();

        // This is the temperature of current patch
        const scalarField& Tp(*this);
        
        // Constant of the equation
        const scalar C1 = 1;
        const scalar C2 = 0;

        // Calculate the values on each face of the patch
        // Note: Eq is divided by thermal conductivity to units of grad(T)
        this->refGrad() = C1*pow(Tp, 2)*pow(M_E, C2*Tp)/thermo.kappa(patchi);

        bool debug = true;  
        if (debug) {
            Info << "Evaluating temperatureHeatFlux on " << patch().name() << endl;
            Info << "temperatureHeatFlux::average(Tp)  = " << gAverage(Tp) << " K" << endl;
            Info << "temperatureHeatFlux::average(Q) = " 
                 << gAverage(this->refGrad()*thermo.kappa(patchi)) << " W/m2K"
                 << endl << endl;
        }
    #};

    codeInclude
    #{
        #include "solidThermo.H"
    #};

    codeOptions
    #{
        -I$(LIB_SRC)/thermophysicalModels/basic/lnInclude \
        -I$(LIB_SRC)/thermophysicalModels/solidThermo/lnInclude \
    #};

    }

Thank you very much crubio!



In the end I left OpenFOAM to use some other enterprise software, since I was not able to get my simulation to converge in any way, even with simpler BC and without using this variable term.



Still, thank you for your reply, it was very interesting!!


Sincerely,

Nicolò.

[NBad]

Originally Posted by dhiraj kumar

hello everyone. I have a solar receiver in which at outer surface of the receiver i have to apply non-uniform heat flux [cosine profile - q(θ) = qnet ·
cos θ(−90 ≤ θ ≤ 90)] with radiation and convection losses to ambient. can anyone give me the idea for writing the UDF for ansys fluent for this condition. thanks !

Hi dhiraj, I don't think this is the right thread to ask, here we are discussing about OpenFOAM which is a different software. You might want to post your question as a new thread in the blog so you can get proper help.

[Brodenson]

Hi folks!
I have tested this code in my example. It is compounded by two regions, one of them solid and another one a fluid. I have implemented this boundary condition in a solid region and it compiles. I haven't verified the convergence.
Regards!

[Brodenson]

Hi folks!
I have tested this code in my example. It is compounded by two regions, one of them solid and another one a fluid. I have implemented this boundary condition in a solid region and it compiles. I haven't verified the convergence.
Regards!

P/D:
the line that I added is the following:
-I$(LIB_SRC)/transportModels/compressible/lnInclude \

for ESI version v2112