[oscar0522]

I'm doing a simulation using bouyantBossinesqSimpleFoam and I'm triying to get the wall heat flux but it shows me an error and this one says "Unable to find compressible turbulence model" so the question is how do I get the wall heat flux on a incompressible simulation using OpenFOAM v2006.




Thank you.

[Yann]

Hi Oscar,


I have another question for you: what is the command giving you the error you have posted?


Yann

[oscar0522]

Originally Posted by Yann

Hi Oscar,


I have another question for you: what is the command giving you the error you have posted?


Yann

I'm trying to do the postprocess. The command is "buoyantBoussinesqSimpleFoam -postProcess -func wallHeatFlux".



This is the code that I have on controlDict.


functions
{

wallHeatFlux1
{
// Mandatory entries (unmodifiable)
type wallHeatFlux;
libs (fieldFunctionObjects);

// Optional entries (runtime modifiable)
patches (bottom); // (wall1 "(wall2|wall3)");
qr qr;

// Optional (inherited) entries

}

}


The exact error is:


--> FOAM FATAL ERROR:
Unable to find compressible turbulence model in the database

From virtual bool Foam::functionObjects::wallHeatFlux::execute()
in file wallHeatFlux/wallHeatFlux.C at line 241.

FOAM exiting

[Yann]

Hi Oscar,

Sorry, I read your initial post too fast and missed the fact your were using an incompressible solver. The wallHeatFlux function works only with compressible solvers and this is why it doesn't work with buoyantBoussinesq solvers.

You need to use buoyantSimpleFoam to be able to use the wallHeatFlux function. You should be able to select "Boussinesq" as the equation of state in the thermophysicalProperties file in order to run something equivalent to buoyantBoussinesqSimpleFoam.

Another way around is to use a modified version of the wallHeatFlux function in order to make it compatible with incompressible solvers. I know wyldckat made it long time ago but I am not sure it will be compatible with OpenFOAM-v2006.

Have a look here:
https://openfoamwiki.net/index.php/C...Incompressible
postProcess -func wallHeatFlux in openFoam 6


I hope this helps,
Yann