waveForcing.H

Go to the documentation of this file.

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Copyright (C) 2022-2024 OpenFOAM Foundation
     \\/     M anipulation  |
-------------------------------------------------------------------------------
License
    This file is part of OpenFOAM.
 
    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.
 
    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.
 
    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.
 
Class
    Foam::fv::waveForcing
 
Description
    This fvModel applies forcing to the liquid phase-fraction field and all
    components of the vector field to relax the fields towards those
    calculated from the current wave distribution.
 
    The force coefficient \f$\lambda\f$ should be set based on the desired level
    of forcing and the residence time the waves through the forcing zone.  For
    example, if waves moving at 2 [m/s] are travelling through a forcing zone 8
    [m] in length, then the residence time is 4 [s]. If it is deemed necessary
    to force for 5 time-scales, then \f$\lambda\f$ should be set to equal 5/(4
    [s]) = 1.2 [1/s].  If more aggressive forcing is required adjacent to the
    boundaries, which is often the case if wave boundary conditions are
    specified at outflow boundaries, the optional \c lambdaBoundary
    coefficient can be specified higher than the value of \f$\lambda\f$.
 
    Alternatively the forcing force coefficient \c lambdaCoeff can be
    specified in which case \f$\lambda\f$ is evaluated by multiplying the
    maximum wave speed by \c lambdaCoeff and dividing by the forcing region
    length.  \c lambdaBoundary is similarly evaluated from
    \c lambdaBoundaryCoeff if specified.
 
Usage
    Example usage:
    \verbatim
    waveForcing1
    {
        type            waveForcing;
 
        libs            ("libwaves.so");
 
        liquidPhase     water;
 
        // Define the line along which to apply the graduation
        origin          (600 0 0);
        direction       (-1 0 0);
 
        // // Or, define multiple lines
        // origins         ((600 0 0) (600 -300 0) (600 300 0));
        // directions      ((-1 0 0) (0 1 0) (0 -1 0));
 
        scale
        {
            type        halfCosineRamp;
            start       0;
            duration    300;
        }
 
        lambdaCoeff     2;   // Forcing coefficient
 
     // lambdaBoundaryCoeff  10;  // Optional boundary forcing coefficient
                             // Useful when wave BCs are specified at outlets
 
        // Write the forcing fields: forcing:scale, forcing:forceCoeff
        writeForceFields true;
    }
    \endverbatim
 
See also
    Foam::fv::forcing
 
SourceFiles
    waveForcing.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef waveForcing_H
#define waveForcing_H
 
#include "forcing.H"
#include "waveSuperposition.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
namespace fv
{
 
/*---------------------------------------------------------------------------*\
                      Class waveForcing Declaration
\*---------------------------------------------------------------------------*/
 
class waveForcing
:
    public forcing
{
    // Private Data
 
        scalar lambdaCoeff_;
 
        scalar lambdaBoundaryCoeff_;
 
        dimensionedScalar regionLength_;
 
        //- Reference to the waves
        const waveSuperposition& waves_;
 
        //- Name of the liquid phase
        const word liquidPhaseName_;
 
        //- Name of the liquid phase-fraction field
        const word alphaName_;
 
        //- Name of the velocity field
        const word UName_;
 
        //- Phase-fraction field calculated from the current wave form
        tmp<volScalarField::Internal> alphaWaves_;
 
        //- Velocity field calculated from the current wave form
        tmp<volVectorField::Internal> Uwaves_;
 
        //- Forcing coefficient scale field
        autoPtr<volScalarField::Internal> scale_;
 
 
    // Private Member Functions
 
        //- Non-virtual read
        void readCoeffs();
 
        //- Return the scale distribution
        virtual tmp<volScalarField::Internal> scale() const;
 
        //- Return the force coefficient
        virtual tmp<volScalarField::Internal> forceCoeff() const;
 
 
public:
 
    //- Runtime type information
    TypeName("waveForcing");
 
 
    // Constructors
 
        //- Construct from components
        waveForcing
        (
            const word& name,
            const word& modelType,
            const fvMesh& mesh,
            const dictionary& dict
        );
 
 
    //- Destructor
    virtual ~waveForcing()
    {}
 
 
    // Member Functions
 
        //- Read dictionary
        virtual bool read(const dictionary& dict);
 
 
        // Checks
 
            //- Return the list of fields for which the fvModel adds source term
            //  to the transport equation
            virtual wordList addSupFields() const;
 
 
        // Add explicit and implicit contributions
 
            //- Source term to VoF phase-fraction equation
            virtual void addSup
            (
                const volScalarField& alpha,
                fvMatrix<scalar>& eqn
            ) const;
 
            //- Source term to momentum equation
            virtual void addSup
            (
                const volScalarField& rho,
                const volVectorField& U,
                fvMatrix<vector>& eqn
            ) const;
 
 
        // Mesh changes
 
            //- Update for mesh motion
            virtual bool movePoints();
 
            //- Update topology using the given map
            virtual void topoChange(const polyTopoChangeMap&);
 
            //- Update from another mesh using the given map
            virtual void mapMesh(const polyMeshMap&);
 
            //- Redistribute or update using the given distribution map
            virtual void distribute(const polyDistributionMap&);
 
 
        //- Correct the wave forcing coefficients
        virtual void correct();
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace fv
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //