porousBafflePressureFvPatchField.H

Go to the documentation of this file.

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011-2015 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::porousBafflePressureFvPatchField
 
Group
    grpCoupledBoundaryConditions
 
Description
    This boundary condition provides a jump condition, using the \c cyclic
    condition as a base.
 
    The porous baffle introduces a pressure jump defined by:
 
        \f[
            \Delta p = -(D \mu U + 0.5 I \rho |U|^2 )L
        \f]
 
    where
 
    \vartable
        p      | pressure [Pa]
        \rho   | density [kg/m3]
        \mu    | laminar viscosity [Pa s]
        D      | Darcy coefficient
        I      | inertial coefficient
        L      | porous media length in the flow direction
    \endvartable
 
 
    \heading Patch usage
 
    \table
        Property     | Description             | Required    | Default value
        patchType    | underlying patch type should be \c cyclic| yes |
        phi          | flux field name         | no          | phi
        rho          | density field name      | no          | rho
        D            | Darcy coefficient       | yes         |
        I            | inertial coefficient    | yes         |
        length       | porous media length in the flow direction | yes |
        uniformJump  | applies a uniform pressure drop on the patch based on the
    \endtable
 
    Example of the boundary condition specification:
    \verbatim
    myPatch
    {
        type            porousBafflePressure;
        patchType       cyclic;
        jump            uniform 0;
        D               0.001;
        I               1000000;
        length          0.1;
        uniformJump     false;
        value           uniform 0;
    }
    \endverbatim
 
Note
     The underlying \c patchType should be set to \c cyclic
 
SourceFiles
    porousBafflePressureFvPatchField.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef porousBafflePressureFvPatchField_H
#define porousBafflePressureFvPatchField_H
 
#include "fixedJumpFvPatchField.H"
#include "DataEntry.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
 
/*---------------------------------------------------------------------------*\
                Class porousBafflePressureFvPatchField Declaration
\*---------------------------------------------------------------------------*/
 
class porousBafflePressureFvPatchField
:
    public fixedJumpFvPatchField<scalar>
{
    // Private data
 
        //- Name of flux field (default = phi)
        const word phiName_;
 
        //- Name of density field (default = rho)
        const word rhoName_;
 
        //- Darcy pressure loss coefficient
        autoPtr<DataEntry<scalar> > D_;
 
        //- Inertia pressure lost coefficient
        autoPtr<DataEntry<scalar> > I_;
 
        //- Porous media length
        scalar length_;
 
        //- Aplies uniform pressure drop
        bool uniformJump_;
 
 
public:
 
    //- Runtime type information
    TypeName("porousBafflePressure");
 
 
    // Constructors
 
        //- Construct from patch and internal field
        porousBafflePressureFvPatchField
        (
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&
        );
 
        //- Construct from patch, internal field and dictionary
        porousBafflePressureFvPatchField
        (
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const dictionary&
        );
 
        //- Construct by mapping given porousBafflePressureFvPatchField
        // onto a new patch
        porousBafflePressureFvPatchField
        (
            const porousBafflePressureFvPatchField&,
            const fvPatch&,
            const DimensionedField<scalar, volMesh>&,
            const fvPatchFieldMapper&
        );
 
        //- Construct as copy
        porousBafflePressureFvPatchField
        (
            const porousBafflePressureFvPatchField&
        );
 
        //- Construct and return a clone
        virtual tmp<fvPatchField<scalar> > clone() const
        {
            return tmp<fvPatchField<scalar> >
            (
                new porousBafflePressureFvPatchField(*this)
            );
        }
 
        //- Construct as copy setting internal field reference
        porousBafflePressureFvPatchField
        (
            const porousBafflePressureFvPatchField&,
            const DimensionedField<scalar, volMesh>&
        );
 
        //- Construct and return a clone setting internal field reference
        virtual tmp<fvPatchField<scalar> > clone
        (
            const DimensionedField<scalar, volMesh>& iF
        ) const
        {
            return tmp<fvPatchField<scalar> >
            (
                new porousBafflePressureFvPatchField(*this, iF)
            );
        }
 
 
    // Member functions
 
 
        // Evaluation functions
 
            //- Update the coefficients associated with the patch field
            virtual void updateCoeffs();
 
 
        //- Write
        virtual void write(Ostream&) const;
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //