# OpenFOAM/OpenFOAM-5.x

Switch branches/tags
Nothing to show
Fetching contributors…
Cannot retrieve contributors at this time
357 lines (283 sloc) 10.1 KB
 /*---------------------------------------------------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | \\ / A nd | Copyright (C) 2011-2016 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 . Class Foam::totalPressureFvPatchScalarField Group grpInletBoundaryConditions grpOutletBoundaryConditions Description This boundary condition provides a total pressure condition. Four variants are possible: 1. incompressible subsonic: \f[ p_p = p_0 - 0.5 |U|^2 \f] where \vartable p_p | incompressible pressure at patch [m2/s2] p_0 | incompressible total pressure [m2/s2] U | velocity \endvartable 2. compressible subsonic: \f[ p_p = p_0 - 0.5 \rho |U|^2 \f] where \vartable p_p | pressure at patch [Pa] p_0 | total pressure [Pa] \rho | density [kg/m3] U | velocity \endvartable 3. compressible transonic (\f$\gamma = 1\f$): \f[ p_p = \frac{p_0}{1 + 0.5 \psi |U|^2} \f] where \vartable p_p | pressure at patch [Pa] p_0 | total pressure [Pa] G | coefficient given by \f$\frac{\gamma}{1-\gamma}\f$ \endvartable 4. compressible supersonic (\f$\gamma > 1\f$): \f[ p_p = \frac{p_0}{(1 + 0.5 \psi G |U|^2)^{\frac{1}{G}}} \f] where \vartable p_p | pressure at patch [Pa] p_0 | total pressure [Pa] \gamma | ratio of specific heats (Cp/Cv) \psi | compressibility [m2/s2] G | coefficient given by \f$\frac{\gamma}{1-\gamma}\f$ \endvartable The modes of operation are set by the dimensions of the pressure field to which this boundary condition is applied, the \c psi entry and the value of \c gamma: \table Mode | dimensions | psi | gamma incompressible subsonic | p/rho | | compressible subsonic | p | none | compressible transonic | p | psi | 1 compressible supersonic | p | psi | > 1 \endtable Usage \table Property | Description | Required | Default value U | Velocity field name | no | U phi | Flux field name | no | phi rho | Density field name | no | rho psi | Compressibility field name | no | none gamma | (Cp/Cv) | no | 1 p0 | Total pressure | yes | \endtable Example of the boundary condition specification: \verbatim { type totalPressure; p0 uniform 1e5; } \endverbatim See also Foam::fixedValueFvPatchField SourceFiles totalPressureFvPatchScalarField.C \*---------------------------------------------------------------------------*/ #ifndef totalPressureFvPatchScalarField_H #define totalPressureFvPatchScalarField_H #include "fixedValueFvPatchFields.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // namespace Foam { /*---------------------------------------------------------------------------*\ Class totalPressureFvPatchScalarField Declaration \*---------------------------------------------------------------------------*/ class totalPressureFvPatchScalarField : public fixedValueFvPatchScalarField { // Private data //- Name of the velocity field word UName_; //- Name of the flux transporting the field word phiName_; //- Name of the density field used to normalise the mass flux // if neccessary word rhoName_; //- Name of the compressibility field used to calculate the wave speed word psiName_; //- Heat capacity ratio scalar gamma_; //- Total pressure scalarField p0_; public: //- Runtime type information TypeName("totalPressure"); // Constructors //- Construct from patch and internal field totalPressureFvPatchScalarField ( const fvPatch&, const DimensionedField& ); //- Construct from patch, internal field and dictionary totalPressureFvPatchScalarField ( const fvPatch&, const DimensionedField&, const dictionary& ); //- Construct by mapping given totalPressureFvPatchScalarField // onto a new patch totalPressureFvPatchScalarField ( const totalPressureFvPatchScalarField&, const fvPatch&, const DimensionedField&, const fvPatchFieldMapper& ); //- Construct as copy totalPressureFvPatchScalarField ( const totalPressureFvPatchScalarField& ); //- Construct and return a clone virtual tmp clone() const { return tmp ( new totalPressureFvPatchScalarField(*this) ); } //- Construct as copy setting internal field reference totalPressureFvPatchScalarField ( const totalPressureFvPatchScalarField&, const DimensionedField& ); //- Construct and return a clone setting internal field reference virtual tmp clone ( const DimensionedField& iF ) const { return tmp ( new totalPressureFvPatchScalarField(*this, iF) ); } // Member functions // Access //- Return the name of the velocity field const word& UName() const { return UName_; } //- Return reference to the name of the velocity field // to allow adjustment word& UName() { return UName_; } //- Return the name of the flux field const word& phiName() const { return phiName_; } //- Return reference to the name of the flux field // to allow adjustment word& phiName() { return phiName_; } //- Return the name of the density field const word& rhoName() const { return rhoName_; } //- Return reference to the name of the density field // to allow adjustment word& rhoName() { return rhoName_; } //- Return the name of the compressibility field const word& psiName() const { return psiName_; } //- Return reference to the name of the compressibility field // to allow adjustment word& psiName() { return psiName_; } //- Return the heat capacity ratio scalar gamma() const { return gamma_; } //- Return reference to the heat capacity ratio to allow adjustment scalar& gamma() { return gamma_; } //- Return the total pressure const scalarField& p0() const { return p0_; } //- Return reference to the total pressure to allow adjustment scalarField& p0() { return p0_; } // Mapping functions //- Map (and resize as needed) from self given a mapping object virtual void autoMap ( const fvPatchFieldMapper& ); //- Reverse map the given fvPatchField onto this fvPatchField virtual void rmap ( const fvPatchScalarField&, const labelList& ); // Evaluation functions //- Inherit updateCoeffs from fixedValueFvPatchScalarField using fixedValueFvPatchScalarField::updateCoeffs; //- Update the coefficients associated with the patch field // using the given patch total pressure and velocity fields virtual void updateCoeffs ( const scalarField& p0p, const vectorField& Up ); //- Update the coefficients associated with the patch field virtual void updateCoeffs(); //- Write virtual void write(Ostream&) const; }; // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // } // End namespace Foam // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // #endif // ************************************************************************* //