fluxSummary.H

Go to the documentation of this file.

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | www.openfoam.com
     \\/     M anipulation  |
-------------------------------------------------------------------------------
    Copyright (C) 2015 OpenFOAM Foundation
    Copyright (C) 2015-2020 OpenCFD Ltd.
-------------------------------------------------------------------------------
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::functionObjects::fluxSummary
 
Group
    grpFieldFunctionObjects
 
Description
    Computes the volumetric- or mass-flux
    information across selections of face zones.
 
    Operands:
    \table
      Operand       | Type | Location
      input         | -    | -
      output file   | dat  | $FOAM_CASE/postProcessing/<FO>/<time>/<faceN>
      output field  | -    | -
    \endtable
 
Usage
    Minimal example by using \c system/controlDict.functions:
    \verbatim
    fluxSummary1
    {
        // Mandatory entries (unmodifiable)
        type            fluxSummary;
        libs            (fieldFunctionObjects);
 
        // Mandatory entries (runtime modifiable)
        mode            cellZoneAndDirection;
        cellZoneAndDirection
        (
            (porosity (1 0 0))
        );
 
        // Optional entries  (runtime modifiable)
        phi             phi;
        scaleFactor     1.0;
        tolerance       0.8;
 
        // Optional (inherited) entries
        ...
    }
    \endverbatim
 
    where the entries mean:
    \table
      Property     | Description                        | Type | Req'd | Dflt
      type         | Type name: fluxSummary             | word |  yes  | -
      libs         | Library name: fieldFunctionObjects | word |  yes  | -
      mode         | Mode to generate faces to test     | word |  yes  | -
      phi          | Name of surface flux field         | word |  no   | phi
      scaleFactor | Factor to scale results             | scalar | no  | 1.0
      tolerance   | Tolerance for reference direction   | scalar | no  | 0.8
    \endtable
 
    Options for the \c mode entry:
    \verbatim
      faceZone
      faceZoneAndDirection
      cellZoneAndDirection
      surface
      surfaceAndDirection
    \endverbatim
 
    The inherited entries are elaborated in:
     - \link functionObject.H \endlink
     - \link writeFile.H \endlink
 
    Usage by the \c postProcess utility is not available.
 
Note
    For surface and direction, phi='U' can be used for determining the fluxes.
 
See also
    - Foam::functionObject
    - Foam::functionObjects::fvMeshFunctionObject
    - Foam::functionObjects::writeFile
    - Foam::functionObjects::timeControl
    - ExtendedCodeGuide::functionObjects::field::fluxSummary
 
SourceFiles
    fluxSummary.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef functionObjects_fluxSummary_H
#define functionObjects_fluxSummary_H
 
#include "fvMeshFunctionObject.H"
#include "writeFile.H"
#include "vector.H"
#include "DynamicList.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
 
// Forward Declarations
class dimensionSet;
 
namespace functionObjects
{
 
/*---------------------------------------------------------------------------*\
                         Class fluxSummary Declaration
\*---------------------------------------------------------------------------*/
 
class fluxSummary
:
    public fvMeshFunctionObject,
    public writeFile
{
public:
 
    // Public Enumerations
 
        //- Face mode type
        enum modeType
        {
            mdFaceZone,             
            mdFaceZoneAndDirection, 
            mdCellZoneAndDirection, 
            mdSurface,              
            mdSurfaceAndDirection   
        };
 
        //- Face mode names
        static const Enum<modeType> modeTypeNames_;
 
 
protected:
 
    // Protected Data
 
        //- Track if the surface needs an update
        bool needsUpdate_;
 
        //- Mode for face determination/to generate faces to test
        modeType mode_;
 
        //- Factor to scale results
        scalar scaleFactor_;
 
        //- Name of flux field
        word phiName_;
 
 
        // Per-faceZone/surface information
 
            //- Region (zone/surface) names
            List<word> zoneNames_;
 
            //- Region (zone/surface) directions
            List<vector> zoneDirections_;
 
            //- Face IDs
            List<labelList> faceID_;
 
            //- Face patch IDs
            List<labelList> facePatchID_;
 
            //- Face flip map signs
            List<boolList> faceFlip_;
 
            //- Output file per face zone
            PtrList<OFstream> filePtrs_;
 
 
        //- Tolerance applied when matching face normals
        scalar tolerance_;
 
 
    // Protected Member Functions
 
        //- Check if surface mode instead of zone mode
        bool isSurfaceMode() const;
 
        //- Check flowType (mass or volume)
        //  Return name on success, fatal error on failure.
        word checkFlowType
        (
            const dimensionSet& fieldDims,
            const word& fieldName
        ) const;
 
        //- Initialise for given surface name
        void initialiseSurface
        (
            const word& surfName,
            DynamicList<word>& names,
            DynamicList<vector>& dir,
            DynamicList<boolList>& faceFlip
        ) const;
 
        //- Initialise for given surface name and direction
        void initialiseSurfaceAndDirection
        (
            const word& surfName,
            const vector& refDir,
            DynamicList<word>& names,
            DynamicList<vector>& dir,
            DynamicList<boolList>& faceFlip
        ) const;
 
        //- Initialise face set from face zone
        void initialiseFaceZone
        (
            const word& faceZoneName,
            DynamicList<word>& names,
            DynamicList<vector>& dir,
            DynamicList<labelList>& faceID,
            DynamicList<labelList>& facePatchID,
            DynamicList<boolList>& faceFlip
        ) const;
 
        //- Initialise face set from face zone and direction
        void initialiseFaceZoneAndDirection
        (
            const word& faceZoneName,
            const vector& refDir,
            DynamicList<word>& names,
            DynamicList<vector>& dir,
            DynamicList<labelList>& faceID,
            DynamicList<labelList>& facePatchID,
            DynamicList<boolList>& faceFlip
        ) const;
 
        //- Initialise face set from cell zone and direction
        void initialiseCellZoneAndDirection
        (
            const word& cellZoneName,
            const vector& refDir,
            DynamicList<word>& names,
            DynamicList<vector>& dir,
            DynamicList<labelList>& faceID,
            DynamicList<labelList>& facePatchID,
            DynamicList<boolList>& faceFlip
        ) const;
 
        //- Calculate the total area for the surface or derived faceZone
        scalar totalArea(const label idx) const;
 
        //- Initialise - after read(), before write()
        bool update();
 
        //- Output file header information
        virtual void writeFileHeader
        (
            const word& zoneName,
            const scalar area,
            const vector& refDir,
            Ostream& os
        ) const;
 
        //- Specialized write for surfaces
        bool surfaceModeWrite();
 
 
public:
 
    //- Runtime type information
    TypeName("fluxSummary");
 
 
    // Constructors
 
        //- Construct from Time and dictionary
        fluxSummary
        (
            const word& name,
            const Time& runTime,
            const dictionary& dict
        );
 
        //- No copy construct
        fluxSummary(const fluxSummary&) = delete;
 
        //- No copy assignment
        void operator=(const fluxSummary&) = delete;
 
 
    //- Destructor
    virtual ~fluxSummary() = default;
 
 
    // Member Functions
 
        //- Read the field fluxSummary data
        virtual bool read(const dictionary& dict);
 
        //- Execute, currently does nothing
        virtual bool execute();
 
        //- Write the fluxSummary
        virtual bool write();
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace functionObjects
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //