OpenFOAM-6/src/finiteVolume/fvMesh/wallDist/patchDistMethods/advectionDiffusion/advectionDiffusionPatchDistMethod.H

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 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::patchDistMethods::advectionDiffusion

Description
    Calculation of approximate distance to nearest patch for all cells and
    boundary by solving the Eikonal equation in advection form with diffusion
    smoothing.

    References:
    \verbatim
        P.G. Tucker, C.L. Rumsey, R.E. Bartels, R.T. Biedron,
        "Transport equation based wall distance computations aimed at flows
         with time-dependent geometry",
        NASA/TM-2003-212680, December 2003.
    \endverbatim

    Example of the wallDist specification in fvSchemes:
    \verbatim
        laplacianSchemes
        {
            .
            .
            laplacian(yPsi) Gauss linear corrected;
            laplacian(yWall) Gauss linear corrected;
            .
            .
        }

        wallDist
        {
            method advectionDiffusion;

            advectionDiffusionCoeffs
            {
                method    Poisson;
                epsilon   0.1;
                tolerance 1e-3;
                maxIter   10;
            }
        }
    \endverbatim
    Also the solver specification for yWall is required in fvSolution, e.g.
    for simple cases:
    \verbatim
        yPsi
        {
            solver          PCG;
            preconditioner  DIC;
            tolerance       1e-4;
            relTol          0;
        }

        yWall
        {
            solver          PBiCG;
            preconditioner  DILU;
            tolerance       1e-4;
            relTol          0;
        }

    or for more complex cases:

        yPsi
        {
            solver          GAMG;
            smoother        GaussSeidel;
            cacheAgglomeration true;
            nCellsInCoarsestLevel 10;
            agglomerator    faceAreaPair;
            mergeLevels     1;
            tolerance       1e-4;
            relTol          0;
        }

        yWall
        {
            solver          GAMG;
            smoother        symGaussSeidel;
            cacheAgglomeration true;
            nCellsInCoarsestLevel 10;
            agglomerator    faceAreaPair;
            mergeLevels     1;
            tolerance       1e-4;
            relTol          0;
        }
    \endverbatim

SeeAlso
    Foam::patchDistMethod::meshWave
    Foam::wallDist

SourceFiles
    advectionDiffusionPatchDistMethod.C

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

#ifndef advectionDiffusionPatchDistMethod_H
#define advectionDiffusionPatchDistMethod_H

#include "patchDistMethod.H"

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

namespace Foam
{
namespace patchDistMethods
{

/*---------------------------------------------------------------------------*\
                          Class advectionDiffusion Declaration
\*---------------------------------------------------------------------------*/

class advectionDiffusion
:
    public patchDistMethod
{
    // Private Member Data

        //- Sub-dictionary of coefficients
        dictionary coeffs_;

        //- Run-time selected method to predict the distance-to-wall field
        autoPtr<patchDistMethod> pdmPredictor_;

        //- Diffusion coefficient multiplying y*laplacian(y)
        scalar epsilon_;

        //- Convergence tolerance for the iterations of the advection-diffusion
        //  equation to correct the distance-to-patch and normal-to-patch fields
        scalar tolerance_;

        //- Maximum number of iterations of the advection-diffusion equation
        //  to correct the distance-to-patch and normal-to-patch fields
        int maxIter_;


    // Private Member Functions

        //- Disallow default bitwise copy construct
        advectionDiffusion(const advectionDiffusion&);

        //- Disallow default bitwise assignment
        void operator=(const advectionDiffusion&);


public:

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


    // Constructors

        //- Construct from coefficients dictionary, mesh
        //  and fixed-value patch set
        advectionDiffusion
        (
            const dictionary& dict,
            const fvMesh& mesh,
            const labelHashSet& patchIDs
        );


    // Member Functions

        //- Correct the given distance-to-patch field
        virtual bool correct(volScalarField& y);

        //- Correct the given distance-to-patch and normal-to-patch fields
        virtual bool correct(volScalarField& y, volVectorField& n);
};


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

} // End namespace patchDistMethods
} // End namespace Foam

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

#endif

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