pressureTools.H

Go to the documentation of this file.

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2012-2013 OpenFOAM Foundation
     \\/     M anipulation  | Copyright (C) 2015 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::pressureTools
 
Group
    grpUtilitiesFunctionObjects
 
Description
    This function object includes tools to manipulate the pressure into
    different forms.  These currently include:
 
    - static pressure
        \f[
            p_s = \rho p_k
        \f]
    - total pressure
        \f[
            p_T = p_{ref} + p_s + 0.5 \rho |U|^2
        \f]
    - static pressure coefficient
        \f[
            Cp_s = \frac{p_s - p_{\inf}}{0.5 \rho_{\inf} |U_{\inf}|^2}
        \f]
    - total pressure coefficient
        \f[
            Cp_T = \frac{p_T - p_{\inf}}{0.5 \rho_{\inf} |U_{\inf}|^2}
        \f]
 
    where
    \vartable
        \rho        | density [kg/m3]
        U           | velocity [m/s]
        \rho_{\inf} | freestream density [kg/m3]
        p_{\inf}    | freestream pressure [Pa]
        U_{\inf}    | freestream velocity [m/s]
        p_k         | kinematic pressure (p/rho)[m2/s2]
        p_s         | pressure [Pa]
        p_T         | total pressure [Pa]
        p_{ref}     | reference pressure level [Pa]
        Cp_{s}      | pressure coefficient
        Cp_{T}      | total pressure coefficient
    \endvartable
 
    The function object will operate on both kinematic (\f$ p_k \f$) and static
    pressure (\f$ p_s \f$) fields, and the result is written as a
    volScalarField.
 
    The modes of operation are:
    \table
        Mode                        | calcTotal | calcCoeff
        static pressure             | no        | no
        total pressure              | yes       | no
        pressure coefficient        | no        | yes
        total pressure coefficient  | yes       | yes
    \endtable
 
    Example of function object specification to calculate pressure coefficient:
    \verbatim
    pressureTools1
    {
        type        pressureTools;
        functionObjectLibs ("libutilityFunctionObjects.so");
        ...
        calcTotal   no;
        calcCoeff   yes;
    }
    \endverbatim
 
    \heading Function object usage
    \table
        Property     | Description             | Required    | Default value
        type         | type name: pressureTools| yes         |
        calcTotal    | Calculate total coefficient | yes     |
        pName        | Name of pressure field  | no          | p
        UName        | Name of velocity field  | no          | U
        rhoName      | Name of density field   | no          | rho
        pRef         | Reference pressure for total pressure | no | 0.0
        calcCoeff    | Calculate pressure coefficient | yes  |
        pInf         | Freestream pressure for coefficient calculation | no |
        UInf         | Freestream velocity for coefficient calculation | no |
        rhoInf       | Freestream density for coefficient calculation | no |
        resultName   | Name of derived pressure field | no   | auto generated
        log          | log to standard output  | no          | yes
    \endtable
 
SourceFiles
    pressureTools.C
    IOpressureTools.H
 
\*---------------------------------------------------------------------------*/
 
#ifndef pressureTools_H
#define pressureTools_H
 
#include "volFieldsFwd.H"
#include "dimensionedScalar.H"
#include "Switch.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
 
// Forward declaration of classes
class objectRegistry;
class dictionary;
class polyMesh;
class mapPolyMesh;
 
/*---------------------------------------------------------------------------*\
                        Class pressureTools Declaration
\*---------------------------------------------------------------------------*/
 
class pressureTools
{
    // Private data
 
        //- Name of this set of pressureTools objects
        word name_;
 
        //- Reference to the database
        const objectRegistry& obr_;
 
        //- On/off switch
        bool active_;
 
        //- Name of pressure field, default is "p"
        word pName_;
 
        //- Name of velocity field, default is "U"
        word UName_;
 
        //- Name of density field, default is "rho"
        word rhoName_;
 
        //- Result name
        word resultName_;
 
        //- Switch to send output to Info as well as to file
        Switch log_;
 
 
        // Total pressure calculation
 
            //- Flag to calculate total pressure
            bool calcTotal_;
 
            //- Reference pressure level
            scalar pRef_;
 
 
        // Pressure coefficient calculation
 
            //- Flag to calculate pressure coefficient
            bool calcCoeff_;
 
            //- Freestream pressure
            scalar pInf_;
 
            //- Freestream velocity
            vector UInf_;
 
            //- Freestream density
            scalar rhoInf_;
 
            //- Flag to show whether rhoInf has been initialised
            bool rhoInfInitialised_;
 
 
    // Private Member Functions
 
        //- Return the density scale
        dimensionedScalar rhoScale(const volScalarField& p) const;
 
        //- Return the density field
        tmp<volScalarField> rho(const volScalarField& p) const;
 
        //- Return the reference pressure
        dimensionedScalar pRef() const;
 
        //- Calculate and return the dynamic pressure
        tmp<volScalarField> pDyn(const volScalarField& p) const;
 
        //- Convert to coeff by applying the freestream dynamic pressure scaling
        tmp<volScalarField> convertToCoeff(const volScalarField& p) const;
 
        //- Disallow default bitwise copy construct
        pressureTools(const pressureTools&);
 
        //- Disallow default bitwise assignment
        void operator=(const pressureTools&);
 
 
public:
 
    //- Runtime type information
    TypeName("pressureTools");
 
 
    // Constructors
 
        //- Construct for given objectRegistry and dictionary.
        //  Allow the possibility to load fields from files
        pressureTools
        (
            const word& name,
            const objectRegistry&,
            const dictionary&,
            const bool loadFromFiles = false
        );
 
 
    //- Destructor
    virtual ~pressureTools();
 
 
    // Member Functions
 
        //- Return name of the set of pressureTools
        virtual const word& name() const
        {
            return name_;
        }
 
        //- Read the pressureTools data
        virtual void read(const dictionary&);
 
        //- Execute, currently does nothing
        virtual void execute();
 
        //- Execute at the final time-loop, currently does nothing
        virtual void end();
 
        //- Called when time was set at the end of the Time::operator++
        virtual void timeSet();
 
        //- Calculate the pressureTools and write
        virtual void write();
 
        //- Update for changes of mesh
        virtual void updateMesh(const mapPolyMesh&)
        {}
 
        //- Update for changes of mesh
        virtual void movePoints(const polyMesh&)
        {}
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //