[bhh]

Hi,

I am running buoyantPimpleFoam with a built-in boundary condition for heat transfer based on heat transfer coefficient (aphaWall) and outside temperature (Tinf) like this:

window
{
type wallHeatTransfer;
alphaWall uniform 1.5;
Tinf uniform 263;
value uniform 293.;
}

This work perfectly.

Now I want to impose a fixed heat flux ( eg 50 W/sq m) on a patch (radiator). How do I do this in the solver? Is there a built-in BC condition for this. I know that the solver demands boundary conditions for temperature but the enthalpy is used for solving the energy equation.

Can anybody give me a hint?

Regards
Bjorn

[mabinty]

Hi!

Check out this BC (for RAS turbulence models): src/turbulenceModels/compressible/RAS/derivedFvPatchFields/turbulentHeatFluxTemperature. It applies for the heated boundary patch as a temperature boundary condition like that:

heatedPatch
{
    type              compressible::turbulentHeatFluxTemperature;
    heatSource    power;
    q                   uniform 65.0;
    value             uniform 293.0;
}

cheers,
Aram

[bhh]

Hi Aram!

It works like a charm! Thank you very much

rgds
Bjorn

[bhh]

Hi Aram,

One thing that is unclear about the BC: is power q given in Watts or Watts per sq m for the patch in question?

rgds

Bjorn

[mabinty]

hi bjorn!

see src/turbulenceModels/compressible/RAS/derivedFvPatchFields/turbulentHeatFluxTemperature/turbulentHeatFluxTemperatureFvPatchScalarField.C lines 176 - 202. if you set

heatSource  power;

q stands for power (W); in case of

heatSource  flux;

q is taken as power density (W/m2).

cheers!
aram

[bhh]

Hi Aram,

Thanks again! This clarified the situation
rgds
Bjorn

[chandramurthy]

Dear Aram,
In the calculation of gradient() [ turbulentHeatFluxTemperatureFvPatchScalarField.C, lines 180 and 185 ], effective thermal conductivity is calculated as (Cp*alphaEff). I guess it should have been (Cp*alphaEff.Rho).

[chandramurthy]

Please read (Cp*alphaEff.Rho) as (Cp*alphaEff*Rho)

[mabinty]

hi!

alpha = a*rho = k/cp (kg/s/m) denotes the effective enthalpy (energy) diffusivity, whereas "a" (m^2/s) stands for the thermal diffusivity. hence, conductivity k = cp*alpha.

cheers,
aram

[murrdpirate]

heatedPatch
{
    type              compressible::turbulentHeatFluxTemperature;
    heatSource    power;
    q                   uniform 65.0;
    value             uniform 293.0;
}

What exactly is the temperature value for? Does it change the flux value? I implemented this bc into one of my projects, but I forgot to change the temperature and I ended up with a wall that was at a lower temperature than the internal field. Is it still transferring 65 W to the internal field?

[mabinty]

Originally Posted by murrdpirate

heatedPatch
{
    type              compressible::turbulentHeatFluxTemperature;
    heatSource    power;
    q                   uniform 65.0;
    value             uniform 293.0;
}

What exactly is the temperature value for? Does it change the flux value? I implemented this bc into one of my projects, but I forgot to change the temperature and I ended up with a wall that was at a lower temperature than the internal field. Is it still transferring 65 W to the internal field?

Hi,

value             uniform 293.0;

is used as initial value at the respective patch. To check wall heat fluxes use the "wallHeatFlux" utility.

Aram

[matthi]

Hello,

I´m relatively new in applying OpenFoam.

My question is if anyone can give me an advice where I have to search if I want to apply a heat flux to walls in case of laminar flows (solver rhoSimpleFoam). I`d like to have access to all wall cells and want to set a different heat flux for every cell according to values which I get from somewhere else (measured or calculated data).

I think an approach like using
src/turbulenceModels/compressible/RAS/derivedFvPatchFields/turbulentHeatFluxTemperature

would be right. But I can use this only for turbulent flows ?
Or do you think that I could use a RAS-code for laminar flow and replace the values Ap, Cpp, alphaEffp in such a manner that I get the desired heat flux?

Thanks in advance for any information

Matthias

[chandramurthy]

Nearest matching BC for your requirement is timeVaryingMappedFixedValue. You have to tweak around slightly to make it timeVaryingMappedFixedHeatFlux. in base class inherit fixedGradient instead fixedValue.

Originally Posted by matthi

Hello,
I`d like to have access to all wall cells and want to set a different heat flux for every cell according to values which I get from somewhere else (measured or calculated data).
Matthias

[matthi]

Hi Chandramurthy,

many thanks for your reply. I got also an other advice from Aran (see above). He wrote me, that I should govern the laminar heat flux with the temperature gradient (Fourier's law) on the respective patch (fixedGradient).
I`ll search in both ways ... but ... as I`m a beginner it will take a lot of time to succeed. If I will be successful I will post the result in the forum.

Greetings Matthias

[murrdpirate]

It appears that the turbulentHeatFluxTemperature only works for heat gains and not heat losses, is that correct? Or am I doing something wrong? I just tried making the "q" value a negative number, but I get a heat gain. Is there a way to make this work or am I stuck with temperature gradients?

[matthi]

Hi Kevin,

it should work in both ways (for positive and negative gradient). This would be physically and numerically right. Maybe, the code uses somewhere only the absolute value of and nobody tried it before, or you made something wrong. The flux is not independent from your coordinate system ! Be sure that you "think" in the right direction.

Greetings Matthias

[murrdpirate]

Matthais,

Sorry, I forgot that I never got back to you. You are correct that this BC handles negative heat transfer. At one point, I did see what appeared to be heat gain, but I think somehow my turbulence model was causing it to create pockets of heat (and a heat loss overall). Thanks for your help.

[murrdpirate]

It looks like this boundary condition has changed in ver 2.0. I now get the error "Keyword K is undefined in [my boundary condition]" Anyone know what that means?

[mabinty]

Originally Posted by murrdpirate

It looks like this boundary condition has changed in ver 2.0. I now get the error "Keyword K is undefined in [my boundary condition]" Anyone know what that means?

That means you did not specify how the conductivity fied "K" shoud be calculated. Look at the top of src/turbulenceModels/compressible/turbulenceModel/derivedFvPatchFields/turbulentHeatFluxTemperature/turbulentHeatFluxTemperatureFvPatchScalarField.H:

hotWall
        {
            type            compressible::turbulentHeatFluxTemperature;
            heatSource      flux;        // power [W]; flux [W/m2]
            q               uniform 10;  // heat power or flux
            K               basicThermo; // calculate K by alphaEff*thermo.Cp
            value           uniform 300; // initial temperature value
        }

Cheers,
Aram

[murrdpirate]

Thanks. I didn't realize there were examples in the code for these things.

Issue now is that it's saying "KName is undefined." As you showed, that's not listed in the example. I see somewhere online that it's "CHARACTER*(*) array of species names," but I don't know what that means