229 lines
7 KiB
C++
229 lines
7 KiB
C++
/*---------------------------------------------------------------------------*\
|
|
========= |
|
|
\\ / F ield | OpenFOAM: The Open Source CFD Toolbox
|
|
\\ / O peration |
|
|
\\ / A nd | Copyright (C) 2011-2017 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::flowRateInletVelocityFvPatchVectorField
|
|
|
|
Group
|
|
grpInletBoundaryConditions
|
|
|
|
Description
|
|
Velocity inlet boundary condition either correcting the extrapolated
|
|
velocity or creating a uniform velocity field normal to the patch adjusted
|
|
to match the specified flow rate
|
|
|
|
For a mass-based flux:
|
|
- the flow rate should be provided in kg/s
|
|
- if \c rho is "none" the flow rate is in m3/s
|
|
- otherwise \c rho should correspond to the name of the density field
|
|
- if the density field cannot be found in the database, the user must
|
|
specify the inlet density using the \c rhoInlet entry
|
|
|
|
For a volumetric-based flux:
|
|
- the flow rate is in m3/s
|
|
|
|
Usage
|
|
\table
|
|
Property | Description | Required | Default value
|
|
massFlowRate | mass flow rate [kg/s] | no |
|
|
volumetricFlowRate | volumetric flow rate [m3/s]| no |
|
|
rho | density field name | no | rho
|
|
rhoInlet | inlet density | no |
|
|
extrapolateProfile | Extrapolate velocity profile | no | false
|
|
\endtable
|
|
|
|
Example of the boundary condition specification for a volumetric flow rate:
|
|
\verbatim
|
|
<patchName>
|
|
{
|
|
type flowRateInletVelocity;
|
|
volumetricFlowRate 0.2;
|
|
extrapolateProfile yes;
|
|
value uniform (0 0 0);
|
|
}
|
|
\endverbatim
|
|
|
|
Example of the boundary condition specification for a mass flow rate:
|
|
\verbatim
|
|
<patchName>
|
|
{
|
|
type flowRateInletVelocity;
|
|
massFlowRate 0.2;
|
|
extrapolateProfile yes;
|
|
rho rho;
|
|
rhoInlet 1.0;
|
|
value uniform (0 0 0);
|
|
}
|
|
\endverbatim
|
|
|
|
The \c flowRate entry is a \c Function1 of time, see Foam::Function1Types.
|
|
|
|
Note
|
|
- \c rhoInlet is required for the case of a mass flow rate, where the
|
|
density field is not available at start-up
|
|
- The value is positive into the domain (as an inlet)
|
|
- May not work correctly for transonic inlets
|
|
- Strange behaviour with potentialFoam since the U equation is not solved
|
|
|
|
See also
|
|
Foam::fixedValueFvPatchField
|
|
Foam::Function1Types
|
|
Foam::flowRateOutletVelocityFvPatchVectorField
|
|
|
|
SourceFiles
|
|
flowRateInletVelocityFvPatchVectorField.C
|
|
|
|
\*---------------------------------------------------------------------------*/
|
|
|
|
#ifndef flowRateInletVelocityFvPatchVectorField_H
|
|
#define flowRateInletVelocityFvPatchVectorField_H
|
|
|
|
#include "fixedValueFvPatchFields.H"
|
|
#include "Function1.H"
|
|
|
|
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
|
|
|
|
namespace Foam
|
|
{
|
|
|
|
/*---------------------------------------------------------------------------*\
|
|
Class flowRateInletVelocityFvPatchVectorField Declaration
|
|
\*---------------------------------------------------------------------------*/
|
|
|
|
class flowRateInletVelocityFvPatchVectorField
|
|
:
|
|
public fixedValueFvPatchVectorField
|
|
{
|
|
// Private data
|
|
|
|
//- Inlet integral flow rate
|
|
autoPtr<Function1<scalar>> flowRate_;
|
|
|
|
//- Is volumetric?
|
|
bool volumetric_;
|
|
|
|
//- Name of the density field used to normalize the mass flux
|
|
word rhoName_;
|
|
|
|
//- Rho initialisation value (for start; if value not supplied)
|
|
scalar rhoInlet_;
|
|
|
|
//- Set true to extrapolate the velocity profile from the interior
|
|
Switch extrapolateProfile_;
|
|
|
|
|
|
// Private member functions
|
|
|
|
//- Update the patch values given the appropriate density type and value
|
|
template<class RhoType>
|
|
void updateValues(const RhoType& rho);
|
|
|
|
|
|
public:
|
|
|
|
//- Runtime type information
|
|
TypeName("flowRateInletVelocity");
|
|
|
|
|
|
// Constructors
|
|
|
|
//- Construct from patch and internal field
|
|
flowRateInletVelocityFvPatchVectorField
|
|
(
|
|
const fvPatch&,
|
|
const DimensionedField<vector, volMesh>&
|
|
);
|
|
|
|
//- Construct from patch, internal field and dictionary
|
|
flowRateInletVelocityFvPatchVectorField
|
|
(
|
|
const fvPatch&,
|
|
const DimensionedField<vector, volMesh>&,
|
|
const dictionary&
|
|
);
|
|
|
|
//- Construct by mapping given
|
|
// flowRateInletVelocityFvPatchVectorField
|
|
// onto a new patch
|
|
flowRateInletVelocityFvPatchVectorField
|
|
(
|
|
const flowRateInletVelocityFvPatchVectorField&,
|
|
const fvPatch&,
|
|
const DimensionedField<vector, volMesh>&,
|
|
const fvPatchFieldMapper&
|
|
);
|
|
|
|
//- Construct as copy
|
|
flowRateInletVelocityFvPatchVectorField
|
|
(
|
|
const flowRateInletVelocityFvPatchVectorField&
|
|
);
|
|
|
|
//- Construct and return a clone
|
|
virtual tmp<fvPatchVectorField> clone() const
|
|
{
|
|
return tmp<fvPatchVectorField>
|
|
(
|
|
new flowRateInletVelocityFvPatchVectorField(*this)
|
|
);
|
|
}
|
|
|
|
//- Construct as copy setting internal field reference
|
|
flowRateInletVelocityFvPatchVectorField
|
|
(
|
|
const flowRateInletVelocityFvPatchVectorField&,
|
|
const DimensionedField<vector, volMesh>&
|
|
);
|
|
|
|
//- Construct and return a clone setting internal field reference
|
|
virtual tmp<fvPatchVectorField> clone
|
|
(
|
|
const DimensionedField<vector, volMesh>& iF
|
|
) const
|
|
{
|
|
return tmp<fvPatchVectorField>
|
|
(
|
|
new flowRateInletVelocityFvPatchVectorField(*this, iF)
|
|
);
|
|
}
|
|
|
|
|
|
// Member functions
|
|
|
|
//- Update the coefficients associated with the patch field
|
|
virtual void updateCoeffs();
|
|
|
|
//- Write
|
|
virtual void write(Ostream&) const;
|
|
};
|
|
|
|
|
|
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
|
|
|
|
} // End namespace Foam
|
|
|
|
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
|
|
|
|
#endif
|
|
|
|
// ************************************************************************* //
|