heat flux with chtMultiRegionFoam
 

Hi,

I would like to know how integrate the heat flux option between a solid and a fluid region using chtMultiRegionFoam. I tried with this:

"Solid_to_.*"
{
type compressible::turbulentHeatFluxTemperature;
heatSource flux;
q uniform 200;
alphaEff alphaEff;
Cp Cp;
value uniform 300;
}
Or

"Solid_to_.*"
{
type compressible::turbulentHeatFluxTemperature;
heatSource flux 1000;
q uniform 200;
kappaName none;
kappa solidThermo 0;
value uniform 300;
}

But, I obtained this error :

--> FOAM FATAL ERROR:

lookup of thermophysicalProperties from objectRegistry domain0 successful
but it is not a solidThermo, it is a heRhoThermo<pureMixture<const<hConst<perfectGas<sp ecie>>,sensibleEnthalpy>>>

From function objectRegistry::lookupObject<Type>(const word&) const
in file /opt/OpenFOAM/OpenFOAM-2.3.x/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 181.

FOAM aborting

Someone can help me please ?

Thank you
Lucie

Hi,

that error is related with the thermophysicalProperties dictionary, located on the constant folder (one for each region). Check the tutorials to see the differences when it's a solid or fluid region. https://github.com/OpenFOAM/OpenFOAM...tiRegionHeater

To allow exchange of energy between regions I usually use this boundary type: compressible::turbulentTemperatureCoupledBaffleMix ed
https://github.com/OpenFOAM/OpenFOAM.../bottomWater/T

Hope it helps :p

Thanks. But with compressible::turbulentTemperatureCoupledBaffleMix ed, I can't have a heat flux as parameter, it is only the temperature at the interface.
For my case, I would like to have a heat flux in enter [W/m²] and I don't know the boundary condition which allows that !

Do you have an idea?

Thank you

Lucie

Having an imposed heat flux on a interface solid/fluid doesn't make sense to me. If it was a external wall, the boundary "externalWallHeatFluxTemperature" should do the work.

Anyway, as the error you mentioned it's not related with the boundary, try the one you were using (compressible::turbulentHeatFluxTemperature, I've never use it).

Oh yeah my mistake ! This boundary condition was for an external wall so I tried externalWallHeatFluxTemperature and it seems working. Thank you for your help !

I have another question ! By imposing an heat flux for an external boundary, all the other boundaries are coupled with the fluid or another solid and the boundaries conditions in the interface are: compressible::turbulentTemperatureCoupledBaffleMix ed;

Do you know if it is possible to not imposed the temperature in the baffle because it is what I want to calculate !

Thank you so much
Lucie

You define the initial value on the compressible::turbulentTemperatureCoupledBaffleMix ed, it will change accordingly as the simulation develops.

If you fix the temperature in the coupled patch why do you need to do a cht calculation? f the boundary wall temperature is known you can essentially solve the regions separately and do not need to couple them. You can however fix the gradient between the two.

You could check out the fvOptions for coupled patches
interRegionHeatTransferModel
- variableHeatTransfer
- tabulatedHeatTransfer
- constantHeatTransfer
interRegionExplicitPorositySource