turbulenceFields.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) 2013-2016 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::turbulenceFields
 
Group
    grpFieldFunctionObjects
 
Description
    Computes various turbulence-related quantities that are not typically
    output during calculations, and stores/writes them on the mesh database
    for further manipulation.
 
    Fields are stored as copies of the original, with the prefix
    "turbulenceModel:", e.g.:
 
    \verbatim
      turbulenceModel:R
    \endverbatim
 
    Operands:
    \table
      Operand           | Type             | Location
      input             | -                | -
      output file       | -                | -
      output field      | vol<Type>Field | $FOAM_CASE/<time>/<outField>
    \endtable
 
    where \c <Type>=Scalar/SymmTensor.
 
Usage
    Minimal example by using \c system/controlDict.functions:
    \verbatim
    turbulenceFields1
    {
        // Mandatory entries (unmodifiable)
        type        turbulenceFields;
        libs        (fieldFunctionObjects);
 
        // Mandatory entries (runtime modifiable)
        // Either field or fields entries
        fields      (R devRhoReff);
        field       R;
 
        // Optional (inherited) entries
        ...
    }
    \endverbatim
 
    where the entries mean:
    \table
      Property     | Description                           | Type | Req'd | Dflt
      type         | Type name: turbulenceFields           | word |  yes  | -
      libs         | Library name: fieldFunctionObjects    | word |  yes  | -
      fields       | Names of fields to store (see below)  | wordList | yes | -
      field        | Name of a field to store (see below)  | word | yes | -
    \endtable
 
    where \c fields can include:
    \verbatim
      k           | turbulent kinetic energy
      epsilon     | turbulent kinetic energy dissipation rate
      omega       | specific dissipation rate
      nuTilda     | modified turbulent viscosity
      nut         | turbulent viscosity (incompressible)
      nuEff       | effective turbulent viscosity (incompressible)
      mut         | turbulent viscosity (compressible)
      muEff       | effective turbulent viscosity (compressible)
      alphat      | turbulence thermal diffusivity (compressible)
      alphaEff    | effective turbulence thermal diffusivity (compressible)
      R           | Reynolds stress tensor
      devReff     | deviatoric part of the effective Reynolds stress
      devRhoReff  | divergence of the Reynolds stress
      L           | integral-length scale / mixing-length scale
      I           | turbulence intensity
    \endverbatim
 
    The inherited entries are elaborated in:
     - \link functionObject.H \endlink
 
    Minimal example by using the \c postProcess utility:
    \verbatim
        <solver> -postProcess -func turbulenceFields
    \endverbatim
 
See also
    - Foam::functionObject
    - Foam::functionObjects::fvMeshFunctionObject
    - ExtendedCodeGuide::functionObjects::field::turbulenceFields
 
SourceFiles
    turbulenceFields.C
    turbulenceFieldsTemplates.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef functionObjects_turbulenceFields_H
#define functionObjects_turbulenceFields_H
 
#include "fvMeshFunctionObject.H"
#include "HashSet.H"
#include "Enum.H"
#include "volFieldsFwd.H"
#include "Switch.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
namespace functionObjects
{
 
/*---------------------------------------------------------------------------*\
                      Class turbulenceFields Declaration
\*---------------------------------------------------------------------------*/
 
class turbulenceFields
:
    public fvMeshFunctionObject
{
public:
 
    // Public Enumerations
 
        //- Options for the turbulence fields (compressible)
        enum compressibleField
        {
            cfK,            
            cfEpsilon,      
            cfOmega,        
            cfNuTilda,      
            cfMut,          
            cfMuEff,        
            cfAlphat,       
            cfAlphaEff,     
            cfR,            
            cfDevRhoReff,   
            cfL,            
            cfI             
        };
 
        //- Names for compressibleField turbulence fields
        static const Enum<compressibleField> compressibleFieldNames_;
 
        //- Options for the turbulence fields (incompressible)
        enum incompressibleField
        {
            ifK,            
            ifEpsilon,      
            ifOmega,        
            ifNuTilda,      
            ifNut,          
            ifNuEff,        
            ifR,            
            ifDevReff,   
            ifL,            
            ifI             
        };
 
        //- Names for incompressibleField turbulence fields
        static const Enum<incompressibleField> incompressibleFieldNames_;
 
        //- Turbulence closure model name
        static const word modelName_;
 
protected:
 
    // Protected Data
 
        //- Fields to load
        wordHashSet fieldSet_;
 
 
    // Protected Member Functions
 
        //- Return true if compressible turbulence model is identified
        bool compressible();
 
        //- Process the turbulence field
        template<class Type>
        void processField
        (
            const word& fieldName,
            const tmp<GeometricField<Type, fvPatchField, volMesh>>& tvalue
        );
 
        //- Return omega calculated from k and epsilon
        template<class Model>
        tmp<volScalarField> omega(const Model& model) const;
 
        //- Return nuTilda calculated from k and omega
        template<class Model>
        tmp<volScalarField> nuTilda(const Model& model) const;
 
        //- Return integral length scale, L, calculated from k and epsilon
        template<class Model>
        tmp<volScalarField> L(const Model& model) const;
 
        //- Return turbulence intensity, I, calculated from k and U
        template<class Model>
        tmp<volScalarField> I(const Model& model) const;
 
 
public:
 
    //- Runtime type information
    TypeName("turbulenceFields");
 
 
    // Constructors
 
        //- Construct from Time and dictionary
        turbulenceFields
        (
            const word& name,
            const Time& runTime,
            const dictionary& dict
        );
 
        //- No copy construct
        turbulenceFields(const turbulenceFields&) = delete;
 
        //- No copy assignment
        void operator=(const turbulenceFields&) = delete;
 
 
    //- Destructor
    virtual ~turbulenceFields() = default;
 
 
    // Member Functions
 
        //- Read the controls
        virtual bool read(const dictionary&);
 
        //- Calculate turbulence fields
        virtual bool execute();
 
        //- Do nothing.
        //  The turbulence fields are registered and written automatically
        virtual bool write();
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace functionObjects
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#ifdef NoRepository
    #include "turbulenceFieldsTemplates.C"
#endif
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //