waveVelocityFvPatchVectorField.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) 2017-2019 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::waveVelocityFvPatchVectorField

Description
    This boundary condition provides a waveVelocity condition. This sets the
    velocity to that specified by a superposition of wave models. All the
    wave modelling parameters are obtained from a centrally registered
    waveSuperposition class.

    Flow reversal will occur in the event that the amplitude of the velocity
    oscillation is greater than the mean flow. This triggers special handling,
    the form of which depends on the inletOutlet flag and whether a wave
    pressure condition is being used.

    If a wave pressure condition is not being used, and inletOutlet is false,
    then this is a standard fixed value condition, with the value supplied by
    the wave model. If flow reversal occurs this state may be unstable. The
    corresponding pressure condition should be fixedFluxPressure.

    If a wave pressure condition is not being used, and inletOutlet is true or
    not specified then the proportion of the patch over which the flow is
    reversed functions in a manner similar to the flowRateOutletVelocity
    condition; i.e., the velocity is extrapolated and then scaled to match the
    required outlet flow rate. Numerically, this is still a fixedValue
    constraint on the normal velocity, just one which tends to avoid
    instability. Again, the corresponding pressure condition should be
    fixedFluxPressure.

    If a wave pressure condition is being used, then the normal velocity
    condition becomes fixedGradient on outlet faces. This gradient is
    calculated numerically by evaluating the wave model on both the patch face
    and the adjacent cell. The pressure boundary in this case should be a
    wavePressure condition. This will do the opposite; it will fix the pressure
    value on outlet faces, and the gradient otherwise.

Usage
    \table
        Property    | Description                            | Req'd? | Default
        phi         | Name of the flux field                 | no     | phi
        p           | Name of the pressure field             | no     | p
        inletOutlet | does the condition behave like inletOutlet | no | true
        ramp        | ramping function for the mean flow speed | no   | None
    \endtable

    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type        waveVelocity;
        phi         phi;
        p           p;
        inletOutlet yes;
        ramp        constant 1;
    }
    \endverbatim

See also
    Foam::waveSuperposition

SourceFiles
    waveVelocityFvPatchVectorField.C

\*---------------------------------------------------------------------------*/

#ifndef waveVelocityFvPatchVectorField_H
#define waveVelocityFvPatchVectorField_H

#include "directionMixedFvPatchFields.H"
#include "waveSuperposition.H"

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

namespace Foam
{

class fvMeshSubset;

/*---------------------------------------------------------------------------*\
                Class waveVelocityFvPatchVectorField Declaration
\*---------------------------------------------------------------------------*/

class waveVelocityFvPatchVectorField
:
    public directionMixedFvPatchVectorField
{
    // Private Data

        //- Name of the flux field
        const word phiName_;

        //- Name of the pressure field
        const word pName_;

        //- Act as an inlet/outlet patch?
        const Switch inletOutlet_;

        //- Mesh subset corresponding to the patch adjacent cells
        mutable autoPtr<fvMeshSubset> faceCellSubset_;

        //- Time index for keeping the subset up to date
        mutable label faceCellSubsetTimeIndex_;


public:

    //- Runtime type information
    TypeName("waveVelocity");


    // Constructors

        //- Construct from patch and internal field
        waveVelocityFvPatchVectorField
        (
            const fvPatch&,
            const DimensionedField<vector, volMesh>&
        );

        //- Construct from patch, internal field and dictionary
        waveVelocityFvPatchVectorField
        (
            const fvPatch&,
            const DimensionedField<vector, volMesh>&,
            const dictionary&
        );

        //- Construct by mapping given mixedTypeFvPatchField onto a new patch
        waveVelocityFvPatchVectorField
        (
            const waveVelocityFvPatchVectorField&,
            const fvPatch&,
            const DimensionedField<vector, volMesh>&,
            const fvPatchFieldMapper&
        );

        //- Copy constructor
        waveVelocityFvPatchVectorField
        (
            const waveVelocityFvPatchVectorField&
        );

        //- Construct and return a clone
        virtual tmp<fvPatchVectorField> clone() const
        {
            return tmp<fvPatchVectorField>
            (
                new waveVelocityFvPatchVectorField(*this)
            );
        }

        //- Copy constructor setting internal field reference
        waveVelocityFvPatchVectorField
        (
            const waveVelocityFvPatchVectorField&,
            const DimensionedField<vector, volMesh>&
        );

        //- Construct and return a clone setting internal field reference
        virtual tmp<fvPatchVectorField> clone
        (
            const DimensionedField<vector, volMesh>& iF
        ) const
        {
            return tmp<fvPatchVectorField>
            (
                new waveVelocityFvPatchVectorField(*this, iF)
            );
        }


    // Member Functions

        // Access

            //- Access the name of the pressure field
            const word& pName() const
            {
                return pName_;
            }

            //- Access the face-cell subset
            const fvMeshSubset& faceCellSubset() const;


        // Evaluation functions

            //- Return the current modelled velocity field on the patch faces
            tmp<vectorField> U() const;

            //- Return the current modelled velocity field in the neighbour cell
            tmp<vectorField> Un() const;

            //- Update the coefficients associated with the patch field
            virtual void updateCoeffs();


        //- Write
        virtual void write(Ostream&) const;
};


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

} // End namespace Foam

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


#endif

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