[jlobera]

Hi all,

I'm using OpenFoam to simulate the air flow through a tower with buoyantSimpleFoam solver. I have used externalWallHeatFluxTemperature BC to simulate the heat losses by convection across the tower wall.

Now I want to know the heat dissipation in every surface with convection. I have been loking for some utility but I haven’t found. I’m especially interested knowing the heat using PyFoamPlotWatcher.

Someone knows if there is any expression to include the heat in the customRegExp file? Or someone knows how to do the post-processing of the heat through a wall?

Thanks all

[zfaraday]

Hi,

what about wallHeatFlux utility provided with OF? Check it out!

Besides that you can use some function objects in your controlDict file in order to compute the same heat fluxes and plot your results with gnuplot.

Hope it helps,

Alex

[jlobera]

Thanks Alex,

I think wallHeatFlux will be a good option.

The problem with gnuplot is I can't use any expression because outside the wall there isn’t mail so I can´t use a gradient or any other expression.

If someone knows any solution it will be welcome.

Thanks;

[zfaraday]

Hi Jorge,

I'm not sure if I get your problem about using gnuplot... However, I recomend you to use the function object attached below. Copy it and paste it to your controlDict file. It computes the heat by convection at every patch of your geometry. It only works if you have swak4foam installed, I hope you have it...

functions
{
    heat_air_patches
    {
        type patchExpression;
        outputControlMode timeStep;
        outputInterval 1;
        patches (".*");
        region air;              //only if it is a multi region case
        accumulations ( sum );
        verbose true;
        aliases { alpha thermo:alpha; }
	expression "alpha*snGrad(h)*area()";
    }
}

libs (
    "libsimpleFunctionObjects.so"
    "libsimpleSwakFunctionObjects.so"
    "libswakFunctionObjects.so"
);

Hope it helps,

Alex