variableHeatTransfer.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) 2011-2015 OpenFOAM Foundation
    Copyright (C) 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::fv::variableHeatTransfer
 
Group
    grpFvOptionsSources
 
Description
    Applies a variable heat transfer model depending
    on local values for inter-region heat exchanges.
 
    The area of contact between regions (area) must be provided.
    The Nu number is calculated as:
 
    \f[
        Nu = a \, \textrm{Re}^b \, \textrm{Pr}^c
    \f]
 
    and the heat transfer coefficient as:
 
    \f[
        htc = \frac{\textrm{Nu} \, K}{ds}
    \f]
 
    where
    \vartable
      htc     | Heat transfer coefficient
      Nu      | Nusselt number
      Re      | Reynolds number
      Pr      | Fluid Prandtl number
      K       | Heat conduction
      ds      | Strut diameter
      a, b, c | Model constants
    \endvartable
 
    Required fields:
    \verbatim
      AoV       | Area per unit volume of heat exchanger    [1/m]
    \endverbatim
 
Usage
    Minimal example by using \c constant/fvOptions:
    \verbatim
    variableHeatTransfer1
    {
        // Mandatory entries (unmodifiable)
        type             variableHeatTransfer;
 
        // Optional entries (runtime modifiable)
        UNbr             U;
        a                0.0;
        b                0.0;
        c                0.0;
        ds               0.0;
        Pr               0.0;
 
        // Mandatory/Optional (inherited) entries
        ...
    }
    \endverbatim
 
    where the entries mean:
    \table
      Property  | Description                     | Type  | Reqd | Dflt
      type      | Type name: variableHeatTransfer | word  | yes  | -
      UNbr      | Name of operand neighbour velocity field | word | no | U
      a         | Model constant                  | scalar | no  | 0
      b         | Model constant                  | scalar | no  | 0
      c         | Model constant                  | scalar | no  | 0
      ds        | Struct diameter                 | scalar | no  | 0
      Pr        | Fluid Prandtl number            | scalar | no  | 0
      \endtable
 
    The inherited entries are elaborated in:
     - \link interRegionHeatTransfer.H \endlink
 
Notes
  - With v2512, the denominator of the Reynolds number calculation has been
    changed from 'mut' to 'muEff'. For fully turbulent regions, there should be
    no significant difference as mut >> mu, thus muEff ~ mut. However, in
    porous/laminar regions, this change prevents the Reynolds number from
    blowing up due to very low turbulent viscosity. Instead, the classical
    laminar Reynolds number is now used in such regions.
 
SourceFiles
    variableHeatTransfer.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef variableHeatTransfer_H
#define variableHeatTransfer_H
 
#include "interRegionHeatTransferModel.H"
#include "autoPtr.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
namespace fv
{
 
/*---------------------------------------------------------------------------*\
                    Class variableHeatTransfer Declaration
\*---------------------------------------------------------------------------*/
 
class variableHeatTransfer
:
    public interRegionHeatTransferModel
{
 
    // Private Data
 
        //- Name of operand neighbour velocity field
        word UNbrName_;
 
        //- Model constants
        scalar a_;
        scalar b_;
        scalar c_;
 
        //- Strut diameter
        scalar ds_;
 
        //- Fluid Prandtl number
        scalar Pr_;
 
        //- Area per unit volume of heat exchanger
        autoPtr<volScalarField> AoV_;
 
 
public:
 
    //- Runtime type information
    TypeName("variableHeatTransfer");
 
 
    // Constructors
 
        //- Construct from dictionary
        variableHeatTransfer
        (
            const word& name,
            const word& modelType,
            const dictionary& dict,
            const fvMesh& mesh
        );
 
        //- No copy construct
        variableHeatTransfer(const variableHeatTransfer&) = delete;
 
        //- No copy assignment
        void operator=(const variableHeatTransfer&) = delete;
 
 
    //- Destructor
    virtual ~variableHeatTransfer() = default;
 
 
    // Public Functions
 
        //- Calculate the heat transfer coefficient
        virtual void calculateHtc();
 
        //- Read dictionary
        virtual bool read(const dictionary& dict);
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace fv
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //