[rod_petrone]

Hello,


I was trying to understand turbulence models implementation in OpenFOAM 6. Nevertheless, in linearViscousStress. H, it is used a parent class called BasicTurbulenceModel, which is the class template parameter too.

I have not been able to find BasicTurbulenceModel declaration and definition. Does someone know where it is in OpenFOAM? Or is it a declaration way that i am not familarizied with?




Codes:


linearViscousStress.H:

#ifndef linearViscousStress_H
#define linearViscousStress_H

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

namespace Foam
{

/*---------------------------------------------------------------------------*\
                           Class linearViscousStress Declaration
\*---------------------------------------------------------------------------*/

template<class BasicTurbulenceModel>
class linearViscousStress
:
    public BasicTurbulenceModel
{

public:

    typedef typename BasicTurbulenceModel::alphaField alphaField;
    typedef typename BasicTurbulenceModel::rhoField rhoField;
    typedef typename BasicTurbulenceModel::transportModel transportModel;


    // Constructors

        //- Construct from components
        linearViscousStress
        (
            const word& modelName,
            const alphaField& alpha,
            const rhoField& rho,
            const volVectorField& U,
            const surfaceScalarField& alphaRhoPhi,
            const surfaceScalarField& phi,
            const transportModel& transport,
            const word& propertiesName
        );


    //- Destructor
    virtual ~linearViscousStress()
    {}


    // Member Functions

        //- Re-read model coefficients if they have changed
        virtual bool read() = 0;

        //- Return the effective stress tensor
        virtual tmp<volSymmTensorField> devRhoReff() const;

        //- Return the source term for the momentum equation
        virtual tmp<fvVectorMatrix> divDevRhoReff(volVectorField& U) const;

        //- Return the source term for the momentum equation
        virtual tmp<fvVectorMatrix> divDevRhoReff
        (
            const volScalarField& rho,
            volVectorField& U
        ) const;

        //- Solve the turbulence equations and correct the turbulence viscosity
        virtual void correct() = 0;
};


// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

} // End namespace Foam

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#ifdef NoRepository
    #include "linearViscousStress.C"
#endif

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#endif

linearViscousStress.C:

#include "linearViscousStress.H"
#include "fvc.H"
#include "fvm.H"

// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //

template<class BasicTurbulenceModel>
Foam::linearViscousStress<BasicTurbulenceModel>::linearViscousStress
(
    const word& modelName,
    const alphaField& alpha,
    const rhoField& rho,
    const volVectorField& U,
    const surfaceScalarField& alphaRhoPhi,
    const surfaceScalarField& phi,
    const transportModel& transport,
    const word& propertiesName
)
:
    BasicTurbulenceModel
    (
        modelName,
        alpha,
        rho,
        U,
        alphaRhoPhi,
        phi,
        transport,
        propertiesName
    )
{}


// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //

template<class BasicTurbulenceModel>
bool Foam::linearViscousStress<BasicTurbulenceModel>::read()
{
    return BasicTurbulenceModel::read();
}


template<class BasicTurbulenceModel>
Foam::tmp<Foam::volSymmTensorField>
Foam::linearViscousStress<BasicTurbulenceModel>::devRhoReff() const
{
    return tmp<volSymmTensorField>
    (
        new volSymmTensorField
        (
            IOobject
            (
                IOobject::groupName("devRhoReff", this->alphaRhoPhi_.group()),
                this->runTime_.timeName(),
                this->mesh_,
                IOobject::NO_READ,
                IOobject::NO_WRITE
            ),
            (-(this->alpha_*this->rho_*this->nuEff()))
           *dev(twoSymm(fvc::grad(this->U_)))
        )
    );
}


template<class BasicTurbulenceModel>
Foam::tmp<Foam::fvVectorMatrix>
Foam::linearViscousStress<BasicTurbulenceModel>::divDevRhoReff
(
    volVectorField& U
) const
{
    return
    (
      - fvc::div((this->alpha_*this->rho_*this->nuEff())*dev2(T(fvc::grad(U))))
      - fvm::laplacian(this->alpha_*this->rho_*this->nuEff(), U)
    );
}


template<class BasicTurbulenceModel>
Foam::tmp<Foam::fvVectorMatrix>
Foam::linearViscousStress<BasicTurbulenceModel>::divDevRhoReff
(
    const volScalarField& rho,
    volVectorField& U
) const
{
    return
    (
      - fvc::div((this->alpha_*rho*this->nuEff())*dev2(T(fvc::grad(U))))
      - fvm::laplacian(this->alpha_*rho*this->nuEff(), U)
    );
}


template<class BasicTurbulenceModel>
void Foam::linearViscousStress<BasicTurbulenceModel>::correct()
{
    BasicTurbulenceModel::correct();
}


// ************************************************************************* //

[GerhardHolzinger]

There is no class named BasicTurbulenceModel, it is a template parameter from which some classes are also derived from. In order to make sense of this, get familiar with the C++ concepts of object orientation, inheritace and templates.

In OpenFOAM's hierarchy of turbulence models, there are two basic categories of turbulence models: incompressible and compressible ones.

Thus, OpenFOAM derives from the base-class of all turbulence models turbulenceModel two classes: incompressibleTurbulenceModel and compressibleTurbulenceModel.

These two classes are then used as template parameter to build the model-trees for incompressible and compressible turbulence models.

Unfortunately, the organisation of the turbulence model classes is not easy to get to understand, and it is also not easy to explain, at least for me. However, it is a brilliant way to avoid the code duplication that was there before. Download the sources of any OpenFOAM version prior to 3.0, and expore the content of $FOAM_SRC/turbulenceModels. Easier to grasp, yet lots of duplicated code.

[zhangyan]

You can find the compressible part here: https://openfoam.top/en/turb/
Sorry for that the language is Chinese.
But the UML is clear:

[rod_petrone]

Hi Gerhard,



I am familiar with many of this C++ concepts of object orientation, inheritace and templates, what i have not understand it was the template parameter used as a parent class, i haven't seen this before. But i think i was able to understand now. At the same time, BasicTurbulenceModel is a parameter, this parameter becomes the parent class of linearViscousStress class.



OpenFOAM version prior to 3.0 i understand the turbulence models class, because i had to implement turbulence models in OpenFOAM 2.3 to my master thesis.


Thank you for the answer.


Best regards,


Rodrigo Petrone