CFD Online Discussion Forums - externalWallHeatFluxTemperature

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - externalWallHeatFluxTemperature (https://www.cfd-online.com/Forums/openfoam-solving/201976-externalwallheatfluxtemperature.html)

externalWallHeatFluxTemperature

I have modified the buoyantCavity tutorial found for buoyantSimpleFoam such that there is 1) a crossflow across the hot plate and 2) a heat flux (W/m^2) is specified. The hot plate seems to cool in the flow direction, whereas I would expect it to heat up. I have attached my modified version of the tutorial.

It could be externalWallHeatFluxTemperature is doing something different and is perhaps related to the specified ambient temperature ...

The temperature differences in my problem do not really need to account for compressibility. The only reason I have chosen buoyantSimpleFoam over buoyantBoussinesqSimpleFoam is that the former seemed to allow a wall heat flux to be specified. Any suggestions on how to specify a heat flux for the latter would be appreciated.

If you look at your velocity at your lower plate you can see that it is very fast after the inlet, then the streamlines detach slightly from the wall in the region with the higher temperature and then reattach to the hot wall.
So you have a high velocity at the hot wall behind the inlet, slower velocity in the next section, and higher velocity when the streamlines come nearer to the wall again.

If you want a fully developed flow (which should give you an increase of wall temperature along the streamwise direction):
You could either specify a developed velocity inlet profile or for incompressible flow a periodic boundary condition for the velocity (but not temperature) by adding to fvOptions:

Code:

momentumSource

{

         type            pressureGradientExplicitSource;

             active          true;

             selectionMode   all;



        pressureGradientExplicitSourceCoeffs

        {

                fieldNames  (U);

    Ubar        ( 0 0 1 );

        }

The boundary condition is in the library libcompressibleTurbulenceModels. Since it seems to retrieve its value for the thermal conductivity kappa from the thermophysical model, which is not used for incompressible flow, you would have to change this part (get it from a field by using 'lookup' for example). To get everything running would take some time.

I would recommend a fixedGradient boundary condition since your thermal conductivity should be nearly independent of the temperature for small temperature changes. Use q=-kappa*dT/dx to define a fixed temperature gradient (Be careful with the signs, I mean the direction of your flux.)