pressureDirectedInletOutletVelocityFvPatchVectorField.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) 2011-2023 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::pressureDirectedInletOutletVelocityFvPatchVectorField
 
Description
    This velocity inlet/outlet boundary condition is applied to pressure
    boundaries where the pressure is specified.  A zero-gradient condition is
    applied for outflow (as defined by the flux); for inflow, the velocity
    is obtained from the flux with the specified inlet direction.
 
Usage
    \table
        Property     | Description             | Required    | Default value
        phi          | flux field name         | no          | phi
        rho          | density field name      | no          | rho
        inletDirection | inlet direction per patch face | yes |
    \endtable
 
    Example of the boundary condition specification:
    \verbatim
    <patchName>
    {
        type            pressureDirectedInletOutletVelocity;
        phi             phi;
        rho             rho;
        inletDirection  uniform (1 0 0);
        value           uniform 0;
    }
    \endverbatim
 
    Note:
        Sign conventions:
      - positive flux (out of domain): apply zero-gradient condition
      - negative flux (into of domain): derive from the flux with specified
        direction
 
See also
    Foam::mixedFvPatchVectorField
 
SourceFiles
    pressureDirectedInletOutletVelocityFvPatchVectorField.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef pressureDirectedInletOutletVelocityFvPatchVectorField_H
#define pressureDirectedInletOutletVelocityFvPatchVectorField_H
 
#include "fvPatchFields.H"
#include "mixedFvPatchFields.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
 
/*---------------------------------------------------------------------------*\
    Class pressureDirectedInletOutletVelocityFvPatchVectorField Declaration
\*---------------------------------------------------------------------------*/
 
class pressureDirectedInletOutletVelocityFvPatchVectorField
:
    public mixedFvPatchVectorField
{
    // Private Data
 
        //- Flux field name
        word phiName_;
 
        //- Density field name
        word rhoName_;
 
        //- Inlet direction
        vectorField inletDir_;
 
 
public:
 
    //- Runtime type information
    TypeName("pressureDirectedInletOutletVelocity");
 
 
    // Constructors
 
        //- Construct from patch, internal field and dictionary
        pressureDirectedInletOutletVelocityFvPatchVectorField
        (
            const fvPatch&,
            const DimensionedField<vector, volMesh>&,
            const dictionary&
        );
 
        //- Construct by mapping given
        //  pressureDirectedInletOutletVelocityFvPatchVectorField
        //  onto a new patch
        pressureDirectedInletOutletVelocityFvPatchVectorField
        (
            const pressureDirectedInletOutletVelocityFvPatchVectorField&,
            const fvPatch&,
            const DimensionedField<vector, volMesh>&,
            const fvPatchFieldMapper&
        );
 
        //- Disallow copy without setting internal field reference
        pressureDirectedInletOutletVelocityFvPatchVectorField
        (
            const pressureDirectedInletOutletVelocityFvPatchVectorField&
        ) = delete;
 
        //- Copy constructor setting internal field reference
        pressureDirectedInletOutletVelocityFvPatchVectorField
        (
            const pressureDirectedInletOutletVelocityFvPatchVectorField&,
            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 pressureDirectedInletOutletVelocityFvPatchVectorField
                (
                    *this,
                    iF
                )
            );
        }
 
 
    // Member Functions
 
        // Attributes
 
            //- Return true: this patch field is altered by assignment
            virtual bool assignable() const
            {
                return true;
            }
 
 
        // Access
 
            //- Return the name of rho
            const word& rhoName() const
            {
                return rhoName_;
            }
 
            //- Return reference to the name of rho to allow adjustment
            word& rhoName()
            {
                return rhoName_;
            }
 
            //- Return the name of phi
            const word& phiName() const
            {
                return phiName_;
            }
 
            //- Return reference to the name of phi to allow adjustment
            word& phiName()
            {
                return phiName_;
            }
 
 
        // Mapping functions
 
            //- Map the given fvPatchField onto this fvPatchField
            virtual void map
            (
                const fvPatchVectorField&,
                const fvPatchFieldMapper&
            );
 
            //- Reset the fvPatchField to the given fvPatchField
            //  Used for mesh to mesh mapping
            virtual void reset(const fvPatchVectorField&);
 
 
        //- Update the coefficients associated with the patch field
        virtual void updateCoeffs();
 
        //- Write
        virtual void write(Ostream&) const;
 
 
    // Member Operators
 
        virtual void operator=(const fvPatchField<vector>& pvf);
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //