-
Andrew Heather authoredAndrew Heather authored
pressure.H 10.69 KiB
/*---------------------------------------------------------------------------*\
========= |
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
\\ / O peration |
\\ / A nd | www.openfoam.com
\\/ M anipulation |
-------------------------------------------------------------------------------
Copyright (C) 2012-2016 OpenFOAM Foundation
Copyright (C) 2016-2020 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::pressure
Group
grpFieldFunctionObjects
Description
Provides several methods to convert an input pressure
field into derived forms, including:
- static pressure
\f[
p_s = p_{ref} + \rho p_k
\f]
- total pressure
\f[
p_0 = p_{ref} + p + 0.5 \rho |\vec U|^2
\f]
- isentropic pressure
\f[
p_i = p*(1 + ((\gamma-1)*M^2)/2)^{(\gamma/(\gamma - 1))}
\f]
- static pressure coefficient
\f[
Cp = \frac{p_s - p_{\inf}}{0.5 \rho_{\inf} |\vec U_{\inf}|^2}
\f]
- total pressure coefficient
\f[
Cp_0 = \frac{p_0 - p_{\inf}}{0.5 \rho_{\inf} |\vec U_{\inf}|^2}
\f]
where
\vartable
\rho | Density [kg/m3]
\vec 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 | Static pressure [Pa]
p_0 | Total pressure [Pa]
p_{ref} | Reference pressure level [Pa]
p_i | Total isentropic pressure
Cp | Pressure coefficient Cp_0 | Total pressure coefficient
\gamma | Specific heat ratio
\endvartable
The function object will operate on both kinematic (\f$ p_k \f$) and static
pressure (\f$ p \f$) fields.
Operands:
\table
Operand | Type | Location
input | volScalarField | $FOAM_CASE/\<time\>/\<inpField\>
output file | - | -
output field | volScalarField | $FOAM_CASE/\<time\>/\<outField\>
\endtable
Usage
Minimal example by using \c system/controlDict.functions:
\verbatim
pressure1
{
// Mandatory entries (unmodifiable)
type pressure;
libs (fieldFunctionObjects);
// Mandatory entries (runtime modifiable)
mode \<option\>;
// Optional entries (runtime modifiable)
p \<pName\>;
U \<UName\>;
rho <rhoName>;
rhoInf 1.0; // enabled if rho=rhoInf
pRef 0.0;
hydroStaticMode none;
g (0 -9.81 0); // enabled if hydroStaticMode != none
hRef 0.0; // enabled if hydroStaticMode != none
pInf 0.0;
UInf (1 0 0);
// Optional (inherited) entries
...
}
\endverbatim
where the entries mean:
\table
Property | Description | Type | Req'd | Dflt
type | Type name: pressure | word | yes | -
libs | Library name: fieldFunctionObjects | word | yes | -
mode | Calculation mode (see below) | word | yes | -
p | Name of the pressure field | word | no | p
U | Name of the velocity field | word | no | U
rho | Name of the density field | word | no | rho
rhoInf | Freestream density for coefficient calculation | scalar <!--
--> | conditional| -
pRef | Reference pressure for total pressure | scalar | no | 0
hydrostaticMode | Hydrostatic contributions (see below) | word | no | none
g | Gravity vector (see below) | vector | no | -
hRef | Reference height (see below) | scalar | no | -
pInf | Freestream pressure for coefficient calculation | scalar | no | -
UInf | Freestream velocity for coefficient calculation | vector | no | -
\endtable
Options for the \c mode entry:
\verbatim
static | static pressure
total | total pressure
isentropic | isentropic pressure
staticCoeff | static pressure coefficient
totalCoeff | total pressure coefficient \endverbatim
The optional \c hydrostaticMode entry provides handling for the term
\f$ \rho (\vec{g} \dot \vec{h})\f$ where options include
\verbatim
none | not included
add | add the term, e.g. to convert from p_rgh to p
subtract | subtract the term, e.g. to convert from p to p_rgh
\endverbatim
If the \c hydrostaticMode is active, values are also required for
gravity, \c g, and reference height, \c hRef. By default these will be
retrieved from the database. When these values are not available
the user must provide them, e.g.
\verbatim
g (0 -9.81 0);
hRef 0;
\endverbatim
The inherited entries are elaborated in:
- \link functionObject.H \endlink
- \link fieldExpression.H \endlink
Usage by the \c postProcess utility is not available.
See also
- Foam::functionObject
- Foam::functionObjects::fieldExpression
- Foam::functionObjects::fvMeshFunctionObject
- ExtendedCodeGuide::functionObjects::field::pressure
SourceFiles
pressure.C
\*---------------------------------------------------------------------------*/
#ifndef functionObjects_pressure_H
#define functionObjects_pressure_H
#include "fieldExpression.H"
#include "volFieldsFwd.H"
#include "dimensionedVector.H"
#include "dimensionedScalar.H"
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
namespace Foam
{
namespace functionObjects
{
/*---------------------------------------------------------------------------*\
Class pressure Declaration
\*---------------------------------------------------------------------------*/
class pressure
:
public fieldExpression
{
public:
// Public Data Types
//- Enumeration for pressure calculation mode
enum mode : unsigned
{
STATIC = (1 << 0), //!< Static pressure
TOTAL = (1 << 1), //!< Total pressure
ISENTROPIC = (1 << 2), //!< Isentropic pressure
COEFF = (1 << 3), //!< Coefficient manipulator STATIC_COEFF = (STATIC | COEFF),
TOTAL_COEFF = (TOTAL | COEFF),
};
static const Enum<mode> modeNames;
//- Enumeration for hydrostatic contributions
enum hydrostaticMode : unsigned
{
NONE = 0,
ADD,
SUBTRACT
};
static const Enum<hydrostaticMode> hydrostaticModeNames;
private:
// Private Data
//- Calculation mode
mode mode_;
//- Hydrostatic constribution mode
hydrostaticMode hydrostaticMode_;
//- Name of velocity field
word UName_;
//- Name of density field
word rhoName_;
// Total pressure calculation
//- Reference pressure level
scalar pRef_;
// Pressure coefficient calculation
//- Freestream pressure
scalar pInf_;
//- Freestream velocity
vector UInf_;
//- Freestream density
scalar rhoInf_;
//- Flag to show whether rhoInf has been initialised
bool rhoInfInitialised_;
//- p +/- rgh calculation
//- Gravity vector
mutable dimensionedVector g_;
//- Flag to show whether g has been initialised
bool gInitialised_;
//- Reference height
mutable dimensionedScalar hRef_;
//- Flag to show whether hRef has been initialised
bool hRefInitialised_;
// Private Member Functions
//- Return the name of the derived pressure field
word resultName() const;
//- Multiply the static pressure p by rhoInf if necessary and return
tmp<volScalarField> rhoScale(const volScalarField& p) const;
//- Multiply the given field by rho or rhoInf as appropriate and return
tmp<volScalarField> rhoScale
(
const volScalarField& p,
const tmp<volScalarField>& tsf
) const;
//- Add the hydrostatic contribution
void addHydrostaticContribution
(
const volScalarField& p,
volScalarField& prgh
) const;
//- Calculate and return the pressure
tmp<volScalarField> calcPressure
(
const volScalarField& p,
const tmp<volScalarField>& tp
) const;
//- Convert to coeff by applying the freestream dynamic pressure scaling
tmp<volScalarField> coeff(const tmp<volScalarField>& tp) const;
//- Calculate the derived pressure field and return true if successful
virtual bool calc();
public:
//- Runtime type information
TypeName("pressure");
// Constructors
//- Construct from Time and dictionary
pressure
(
const word& name,
const Time& runTime,
const dictionary&
);
//- No copy construct
pressure(const pressure&) = delete;
//- No copy assignment
void operator=(const pressure&) = delete;
//- Destructor
virtual ~pressure() = default;
// Member Functions
//- Read the pressure data
virtual bool read(const dictionary&);
};
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
} // End namespace functionObjects
} // End namespace Foam
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
#endif
// ************************************************************************* //