[bastil]

Hello all,

I try to set-up a case in buoyantSimpleFoam using the "externalWallHeatFluxTemperature" BC. In my 0/T I have:

Cooler_wall_heat_in
{
    type            externalWallHeatFluxTemperature;
    mode          flux;
    q                uniform 1; // 1W/m2
    kappaMethod     fluidThermo;
    value           $internalField;
}

I expect to get 1W/m2 in the model. The patch has a size of 0.42m2, so I expect a total heat power of 0.42W going into the system.

I want to check this and came across the "wallHeatFlux" function object. I added the following in my system/controlDict:

wallHeatFlux
{
    type            wallHeatFlux;
    libs            ("libfieldFunctionObjects.so");
    patches     (Cooler_wall_heat_in); // (wall1 "(wall2|wall3)");
    qr          qr;

    writePrecision  8;
    writeToFile     false;
    useUserTime     true;
    region          region0;
    enabled         true;
    log             true;
    timeStart       0;
    timeEnd         1000;
    executeControl  timeStep;
    executeInterval 1;
    writeControl    timeStep;
    writeInterval   1;
}

Two questions about that:

1. I basically want the wall heat flux sum in the log. Therefore I turned "writeToFile" to false. Nevertheless, I am getting a folder for each time step containing the whole wallHeatFlux results per patch face. Why so? How to turn this off?

1. In the log-file I get the following line:
   

   min/max/integ(Cooler_wall_heat_in) = 0.770455625, 0.832415145, 0.0326535893

   min/max seems to be minimum and maximum heat flux on one face? What is integ, it is lower than min? How to get the sum of the heat flow over all faces in the given patch?

[jherb]

Originally Posted by bastil

DE]

1. I basically want the wall heat flux sum in the log. Therefore I turned "writeToFile" to false. Nevertheless, I am getting a folder for each time step containing the whole wallHeatFlux results per patch face. Why so? How to turn this off?

Have you tried adding writeField off;

Originally Posted by bastil

DE]

1. In the log-file I get the following line:
   

   min/max/integ(Cooler_wall_heat_in) = 0.770455625, 0.832415145, 0.0326535893

   min/max seems to be minimum and maximum heat flux on one face? What is integ, it is lower than min? How to get the sum of the heat flow over all faces in the given patch?

The last value should be the spacial integral of the heat flux, so the power flowing into the fluid.

[bastil]

Originally Posted by jherb

The last value should be the spacial integral of the heat flux, so the power flowing into the fluid.

Then my expectation would be 0.42W instead of the given 0.0326... Also I checked the global temperature increase and using P = cP*m*delta(T) gives me a added heat power of 0.42W. So I know case-setup is correct, but wallHeatFlux is strange.
Furthermore, how comes that min and max values are both larger than integral (=sum?).

[jherb]

Here is the source code for the wallHeatFlux function object in the current version, where the integral value is calculated: https://github.com/OpenFOAM/OpenFOAM...eatFlux.C#L266

It is in fact the integral, meaning the sum over all faces of a patch of heat flux * face area. So if your face is small enough, the integral of the heat flux = power [W] can be smaller than the miniumum of the heat flux [W/m²].

Regarding the difference between between the boundary condition and the output of the function object: You might have to compare really the source code, how both are calculating it.

By the way, as you wrote the whole heat flux field. What is the integral using paraview?

[bastil]

Thanks for the feedback so far. I checked a few things and made some progress:

1. I am using Openfoam v1906. The wallFUnction integral is the overall integral heat given in (in W). This now is reasonable and fine for me.
2. I am still getting the whole field written for all time-steps even though I have "writeField off" in my controlDict:

    wallHeatFlux_coolant
    {
        // Mandatory entries (unmodifiable)
        type            wallHeatFlux;
        libs            ("libfieldFunctionObjects.so");
        // Optional entries (runtime modifiable)
        patches         (Cooler_wall_heat_in); // (wall1 "(wall2|wall3)");
        qr          qr;
        // Optional (inherited) entries
        writePrecision  8;
        writeToFile     false;
        writeField      false;
        useUserTime     true;
        region          coolant-fluid;
        enabled         true;
        log             true;
        timeStart       0;
        timeEnd         1000;
        executeControl  timeStep;
        executeInterval 1;
        writeControl    timeStep;
        writeInterval   1;
    }

[jherb]

I looked at the source code and it seems that you can not turn off writing the field into the time directories. Also, I missed an "s" above. The options for other function objects is called writeFields.

[Yann]

Hi,

Even if you cannot turn off the field writing, you can probably play with the executeControl and writeControl parameters to have all the data in your .dat file but to write the fields only at writeTime, or at the end of the simulation.

https://www.openfoam.com/documentati...n-objects.html

Yann