[fertinaz]

Hi,

I am trying to modify the standard kEps model to attain the influence of the buoyancy related turbulence.

I followed a few different methods however all seemed to fail.

1- Using readGravitationalAcceleration.H :
--> FOAM FATAL ERROR:
request for dictionary gravitationalProperties from objectRegistry region0 failed
available objects of type dictionary are
4
(
RASProperties
fvSchemes
fvSolution
transportProperties
)

2 - Reading from transportProperties:
--> FOAM FATAL ERROR:
LHS and RHS of + have different dimensions

The solver works fine with the standard kEps so I don't think that I have to change the solver or B.C's.

3- Creating a file called "g" and reading via lookupObject<uniformDimensionedVectorField>("g") :
Unknow type uniformDimensionedVectorField

4- Linking as a field by lookupObject<volVectorField>("g") :
gives an error during the runTime since g is a uniformDimensionedVectorField

I guess one other way would be to use a hard-coded vector but I don't want to do that. Any help is appreciated.

OF version: 1.6.x
OS: CentOS 5

Thanks a lot,
Fatih.

[Fabf]

Facing the same problem. Did you find a solution?

I prefer to add

#include "UniformDimensionedField.H"

in the Header-file and call "g" by

 const uniformDimensionedVectorField& g_ = db().lookupObject<uniformDimensionedVectorField>("g");

But I get an Error that uniformDimensionedVectorField is not a type. I use OF 2.3.

[alexeym]

Hi,

You should include another file

#include "UniformDimensionedFields.H"

to have uniformDimensionedVectorField. Or declate your g_ as

UniformDimensionedField<vector>

if you insist on including just UniformDimensionedField.H.

And if you are adding gravitation to turbulence model:

http://www.cfd-online.com/Forums/ope...nce-model.html
http://openfoamwiki.net/index.php/Co...EpsilonViollet

[Fabf]

Hi Alexey,

thanks for your quick response.

I guess you meant

#include "uniformDimensionedFields.H"

This works fine fine for including the lib. However, I get for

const uniformDimensionedVectorField& g_ = db().lookupObject<uniformDimensionedVectorField>("g");

the following error:

kEpsilonBuoyant/kEpsilonBuoyant.C: In Elementfunktion »virtual void Foam::compressible::RASModels::kEpsilonBuoyant::correct()«:
kEpsilonBuoyant/kEpsilonBuoyant.C:324:47: Fehler: Referenz auf »db« ist mehrdeutig
/opt/openfoam230/src/OpenFOAM/lnInclude/IOobject.H:250:35: Fehler: Kandidaten sind: const Foam::objectRegistry& Foam::IOobject::db() const
/opt/openfoam230/src/OpenFOAM/lnInclude/IOobject.H:250:35: Fehler:                  const Foam::objectRegistry& Foam::IOobject::db() const
kEpsilonBuoyant/kEpsilonBuoyant.C:324:94: Fehler: expected primary-expression before »>« token

Means db is ambiguous. I copied that formulation from the mentioned kEpsilonViolett.

[alexeym]

Yes, you are right about header name.

Well, kEpsilonViollet was developed for 1.7, guess that time RASModel was a little bit simpler. Right now it is a child of turbulenceModel and IOobject. Each of parents has db method.

So you can either create g_ property of your class and initialize it in constructor with something like:

    g_
    (
        IOobject
        (
            "g",
            runTime_.constant(),
            mesh_,
            IOobject::MUST_READ_IF_MODIFIED,
            IOobject::NO_WRITE
        )
    )

or use constant reference to fvMesh from turbulenceModel (there db ambiguity was resolved):

const uniformDimensionedVectorField& g_ = mesh_.thisDb().lookupObject<uniformDimensionedVectorField>("g");

[Fabf]

Model runs. Thank you a lot!

To sum it up: Inculding gravity acceleration in turbulence models by adding in the .H-file:

#include "uniformDimensionedFields.H"

and in the .C-File:

const uniformDimensionedVectorField& g_ = mesh_.thisDb().lookupObject<uniformDimensionedVectorField>("g");

[Bogha]

what is uniformdimensioned vector field and why is it used in terms of g?