[rl3418]

Hi, I am new to OpenFOAM and I’m trying to simulate convective heat transfer between a metal wall and a fluid.

I’m using the lumpedMassWallTemperature boundary condition, which takes a heat capacity value but does not explicitly define a heat transfer coefficient. I’ve disabled conduction by setting kappa to none, yet I still observe heat transfer, which I assume is via convection. Could someone clarify how lumpedMassWallTemperature computes heat flux and whether convection is handled automatically, even without specifying a heat transfer coefficient? Thank you!

[Tobermory]

A good place to start is the code for the lumpedMassWallTemperature class (https://www.openfoam.com/documentati...8H_source.html).

The meat of the coding is in the updateCoeffs() function (like most boundary classes):

    const scalarField q(tkappa.ref()*snGrad());
    // Total heat in or out of the wall
    const scalar Q = gSum(q*magSf);
    Tp += -(Q/mass_/Cp_)*deltaT;
    refGrad() = 0.0;
    refValue() = Tp;
    valueFraction() = 1.0;

In other words, the code calculates the heat flux into the patch, from the temperature gradient normal to the patch and the kappa value, and uses this to update the lumped mass temperature for the patch. Is it conduction or convection? Depends how you interpret the imposed kappa value.

[rl3418]

Thanks for the reply. Considering that Q=-k(T_s-T_ambient)/L=h(T_ambient-T_s), I guess the thermal conductivity could be approximated by the convective heat transfer as k=h*metal_thickness.

One thing I don't understand though is what's the value of thermal conductivity used for the calculation. I guess lumpedMassWallTemperature takes in a kappa value measured in watts per meter per Kelvin (W/m·K). However, in the hot room tutorial kappa is set to none, and the heat transfer is still observed. I'm not sure what is the kappa value used in that case. (https://develop.openfoam.com/Develop...tRoom/0.orig/T)

[rl3418]

functions
{
htc
{
type heatTransferCoeff;
libs (fieldFunctionObjects);
field T;
writeControl writeTime;
writeInterval 1;
htcModel fixedReferenceTemperature;
patches (cell1 wall);
TRef 330;
}

Seems that the hot room example defined a heatTransferCoeff in controlDict. Not sure how this works.

[Tobermory]

It is a little confusing, I have to agree, but the code is working in a different way to how you imagine it. The lumpedMassWallTemperature boundary condition is simply calculating the wall patch temperature based on a lumped capacitance model for the heat trabnsfer into/out of the wall.

Let's start with the patch definition in 0/T:

    ceiling
    {
        type            lumpedMassWallTemperature;
        kappaMethod     fluidThermo;
        kappa           none;
        mass            1000;
        Cp              4100;
        value           uniform 300.0;
    }

An entry of "none" against kappa does not mean that kappa is zero (ie no heat transfer), it just means that no value is supplied ... because it isn't needed. The line above says that the kappMethod is fluidThermo. To understand what this means, look in temperatureCoupledBase.H (https://www.openfoam.com/documentati...8H_source.html), from which the lumpedMassWallTemperatureFvPatchScalarField is derived. In the header it says:

    The thermal conductivity \c kappa may be obtained by the following methods:
      - 'lookup' : lookup volScalarField (or volSymmTensorField) with name defined by 'kappa'
      - 'fluidThermo' : use fluidThermo and default compressible::turbulenceModel to calculate kappa
      - 'solidThermo' : use solidThermo kappa()
      - 'directionalSolidThermo': uses look up for volSymmTensorField for transformed kappa vector. Field name definable in 'alphaAni', named 'Anialpha' in solid solver by default
      - 'function' : kappa, alpha directly specified as Function1
      - 'phaseSystem' : used for multiphase thermos

The tutorial case uses fluidThermo, i.e. is getting the value of kappa from the turbulence model (wall function). That's why you don't need to supply it - it's calculated as part of the simulation from the turbulence etc.

The function you spotted in the controlDict is a functionObject, i.e. a postProcessing tool - check out: https://www.openfoam.com/documentati...f.html#details. This is just a tool to calculate HTCs during or after the run, based on the flux, the wall temperature ans a user supplied reference temperature. It has no effect on the solution.

Hope that helps.

[Tobermory]

Originally Posted by Tobermory

Is it conduction or convection? Depends how you interpret the imposed kappa value.

For the hot room case, with air next to the wall boundary, kappa is clearly coming from convection ... don't know what I was thinking when I wrote the above!

[rl3418]

Great, thanks for the clarification.