[rsaintlege]

Hello,

I'm new on this forum and OpenFOAM so I hope that I'm posting at the right place and that I'll be clear enough.

So, I found this boundary condition 'externalWallHeatFluxTemperature' that seems perfect for my case. But I would like to impose a sinusoidal heat flux and I don't manage to write it down. The best I managed to get was a time-varying external temperature like this (and that works well) but that does not correspond perfectly to the reality of the problem:

    upperFace
    {

        type            externalWallHeatFluxTemperature;
        mode            coefficient;

        Ta		           	 
	{
          type             sine;
          frequency        0.1;
          amplitude        4;
          scale            1;
          level            293;
      	}
	h		uniform	50;
        thicknessLayers (0.002);
        kappaLayers     (0.16);
        kappaMethod     fluidThermo;
        value           $internalField;
    }

Unfortunately, when I try to do the same with the heat flux I get this error:

--> FOAM FATAL IO ERROR: 
Attempt to return dictionary entry as a primitive

file: /home/romain/OpenFOAM/romain-7/run/pipe_v5.3/0/T.boundaryField.lowerFace.q from line 52 to line 56.

    From function virtual Foam::ITstream& Foam::dictionaryEntry::stream() const
    in file db/dictionary/dictionaryEntry/dictionaryEntry.C at line 83.

FOAM aborting

Hoping someone can help me figure out this problem.

[rsaintlege]

Nobody?

I think it's just a question of syntax but I can't figure it out.
There is probably only one word missing to allow OpenFOAM to understand that the flux needs to be time-varying and I can't find it...

[HPE]

The error report is related to `lowerFace`'s `q`, rather than the `upperFace` reported above.

[rsaintlege]

Originally Posted by HPE

The error report is related to `lowerFace`'s `q`, rather than the `upperFace` reported above.

Thank you for your reply. Yes, they both have the same BC, it was just a test on one of them to get the error in order to post it on the forum.

That's what I try to run (the range of q is not coherent but that's not the problem) and I precise that I get the same error for the two other modes (power and flux):

    upperFace
    {

        type            externalWallHeatFluxTemperature;

        mode            flux;

        q		           	 
	{
          type             sine;
          frequency        0.1;
          amplitude        4;
          scale            1;  
          level            293;  
        }
        thicknessLayers (0.002);
        kappaLayers     (0.16);

        kappaMethod     fluidThermo;

        value           $internalField;
    }

It seems that OpenFOAM doesn't want to interpret heat flux as a time-varying parameter.

[Bloerb]

That is because it is not programmed to do so.


externalWallHeatFluxTemperatureFvPatchScalarField. H:

scalar Q_; //- Heat flux [W/m^2] 
scalarField q_;  //- Heat transfer coefficient [W/m^2K]
scalarField h_; //- Ambient temperature [K] 
autoPtr<Function1<scalar>> Ta_; //- Heat power [W]

As you can see only Ta is defined as a Function1 (the thing that lets you choose between time varying table sin cos and polynomial definitions for its value). q and h are however allowed to vary in space (scalarField). Rather than time they change in space. For the power mode Q is only a scalar. So only one fixed value.
You can take the boundary condition, rename it, and compile a new boundary condition. Add an additional Function1 entry and simply multiply that with the q field, which you'll define as 1. Or e.g change Q from scalar to Function1. Something like this with additional changes in the .C file:

autoPtr<Function1<scalar>> yourValue_;

[rsaintlege]

Oh ok I see, it's more difficult than I thought. I have never done this before but I will try what you propose.
Thanks a lot for your help!

[hamdani]

Hi

Did you succeed to compile the new BC?

If yes, please let me know the step-by-step what you did. It would be very helpful.