Additional drag models for the twoPhaseEulerFoam solver

From OpenFOAMWiki

1 Syamlal and O'Brien drag

1.1 Formulas

The Syamlal and O'Brien drag formula can be written as follows (according to the nomenclature used in the code):


\beta' = \frac{3 \alpha \beta \rho_b}{4 V_r^2 d_a} C_{D_s} U_r

The terminal velocity V_r can be calculated using the formula:


V_r = \frac{1}{2} \left ( A - 0.06 \texttt{Re} + \sqrt{\left( 0.06 \texttt{Re} \right)^2 + 0.12 \texttt{Re} \left( 2B - A \right) + A^2}\right)

where A = \beta^{4.14}, B =  0.8 \beta^{1.28} if \beta \leq 0.85 and B = \beta^{2.65} if \beta > 0.85.

 C_{D_s} is found using the Della Valle formulation:


C_{D_s} = \left ( 0.63 + 4.8 \sqrt{\frac{V_r}{\texttt{Re}}} \right )

with


\texttt{Re} = \frac{d_a U_r}{\nu_b}

1.2 Implementation

The Syamlal and O'Brien drag model can be implemented in OpenFOAM by dividing the \beta' <math> by the product of the two volume fractions <math> \alpha \beta to obtain K.

N.B. Every drag formulation has to be divided by the product  \alpha \beta before beeing implemented in twoPhaseEulerFoam because this product has been extracted for numerical reasons.

The code is the following.

  • SyamlalOBrien.H
 
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 1991-2004 OpenCFD Ltd.
     \\/     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 2 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, write to the Free Software Foundation,
    Inc., 59 Temple Place, Suite 330, Boston, MA 02111-1307 USA
 
Class
    SyamlalOBrien
 
Description
    Syamlal, M., Rogers, W. and O'Brien, T. J. (1993) MFIX documentation,
    Theory Guide. Technical Note DOE/METC-94/1004. Morgantown, West Virginia, 
    USA.
 
SourceFiles
    SyamlalOBrien.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef SyamlalOBrien_H
#define SyamlalOBrien_H
 
#include "dragModel.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
 
/*---------------------------------------------------------------------------*\
                           Class SyamlalOBrien Declaration
\*---------------------------------------------------------------------------*/
 
class SyamlalOBrien
:
    public dragModel
{
 
public:
    
    //- Runtime type information
    TypeName("SyamlalOBrien");
 
 
    // Constructors
 
        //- Construct from components
        SyamlalOBrien
        (
            const dictionary& interfaceDict,
            const volScalarField& alpha,
            const phaseModel& phasea,
            const phaseModel& phaseb
        );
 
 
    // Destructor
 
        ~SyamlalOBrien();
 
 
    // Member Functions
 
        tmp<volScalarField> K(const volScalarField& Ur) const;
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //
  • SyamlalOBrien.C
 
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 1991-2004 OpenCFD Ltd.
     \\/     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 2 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, write to the Free Software Foundation,
    Inc., 59 Temple Place, Suite 330, Boston, MA 02111-1307 USA
 
\*---------------------------------------------------------------------------*/
 
#include "SyamlalOBrien.H"
#include "addToRunTimeSelectionTable.H"
 
// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //
 
namespace Foam
{
    defineTypeNameAndDebug(SyamlalOBrien, 0);
 
    addToRunTimeSelectionTable
    (
        dragModel,
        SyamlalOBrien,
        dictionary
    );
}
 
 
// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
 
Foam::SyamlalOBrien::SyamlalOBrien
(
    const dictionary& interfaceDict,
    const volScalarField& alpha,
    const phaseModel& phasea,
    const phaseModel& phaseb
)
:
    dragModel(interfaceDict, alpha, phasea, phaseb)
{}
 
 
// * * * * * * * * * * * * * * * * Destructor  * * * * * * * * * * * * * * * //
 
Foam::SyamlalOBrien::~SyamlalOBrien()
{}
 
 
// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
 
Foam::tmp<Foam::volScalarField> Foam::SyamlalOBrien::K
(
    const volScalarField& Ur
) const
{
    volScalarField beta = max(1.0 - alpha_, 1.0e-6);
    volScalarField A = pow(beta, 4.14);
    volScalarField B = 0.8*pow(beta, 1.28);
 
    forAll (beta, celli)
    {
	if (beta[celli] > 0.85)
        {
		B[celli] = pow(beta[celli], 2.65);
        }
    }
 
    volScalarField Re = max(Ur*phasea_.d()/phaseb_.nu(), 1.0e-3);
    volScalarField Vr = 0.5*(A - 0.06*Re + sqrt(pow(0.06*Re,2.0) + 0.12*Re*(2.0*B-A) + pow(A,2.0)));
    volScalarField Cds = pow(0.63 + 4.8*sqrt(Vr/Re),2.0);
 
    return 0.75*Cds*phaseb_.rho()*Ur/(phasea_.d()*pow(Vr,2.0));
}
 
 
// ************************************************************************* //

1.3 Compile and link

In order to use this code:

  • Add the files in a directory named SyamlalOBrien in /.../twoPhaseEulerFoam/interfacialModels/dragModels.
  • Open the /../twoPhaseEulerFoam/interfacialModels/Make file and add to it the line
 
dragModels/SyamlalOBrien/SyamlalOBrien.C
  • Use the wmake tool to rebuild twoPhaseEulerFoam

1.4 References

  1. Dalla Valle, J.M., 1948, Micromeritics, Pitman, London.
  1. Syamlal, M., The Particle-Particle Drag Term in a Multiparticle Model of Fluidization, Topical Report, DOE/MC/21353-2373, NTIS/DE87006500, National Technical Information Service, Springfield, VA, 1987.
  1. Syamlal, M., Rogers, W. and O'Brien, T. J. (1993), MFIX documentation, Theory Guide. Technical Note DOE/METC-94/1004. Morgantown, West Virginia, USA, http://www.mfix.org.


2 Gidaspow's drag (Ergun - Wen&Yu)

2.1 Formulas

The Gidaspow formulation of the drag factor uses the Ergun correlations if \beta < 0.8 :


\beta' = 150 \frac{\alpha^2 \nu_b}{\beta^2 \rho_b d_a^2} + 1.75 \frac{\rho_b \alpha}{\beta d_s} U_r

If  \beta \geq 0.8 , the Wen and Yu correlation is used:


 \beta' = \frac{3 C_{D_s} \alpha \beta \rho_b U_r}{4 d_a} \beta^{-2.65}

where  C_{D_s} = 0.44 if \texttt{Re} \geq 1000, and


C_{D_s} = \frac{24}{\texttt{Re}} \left( 1 + 0.15 \texttt{Re}^{0.687} \right)

elsewhere (\texttt{Re} < 1000).

2.2 Implementation

  • GidaspowErgunWenYu.H
 
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 1991-2004 OpenCFD Ltd.
     \\/     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 2 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, write to the Free Software Foundation,
    Inc., 59 Temple Place, Suite 330, Boston, MA 02111-1307 USA
 
Class
    GidaspowErgunWenYu
 
Description
    D. Gidaspow, Multiphase flow and fluidization, 
	Academic Press, New York, 1994.
 
SourceFiles
    GidaspowErgunWenYu.C
 
\*---------------------------------------------------------------------------*/
 
#ifndef GidaspowErgunWenYu_H
#define GidaspowErgunWenYu_H
 
#include "dragModel.H"
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
namespace Foam
{
 
/*---------------------------------------------------------------------------*\
                           Class GidaspowErgunWenYu Declaration
\*---------------------------------------------------------------------------*/
 
class GidaspowErgunWenYu
:
    public dragModel
{
 
public:
    
    //- Runtime type information
    TypeName("GidaspowErgunWenYu");
 
 
    // Constructors
 
 
        //- Construct from components
        GidaspowErgunWenYu
        (
            const dictionary& interfaceDict,
            const volScalarField& alpha,
            const phaseModel& phasea,
            const phaseModel& phaseb
        );
 
 
    // Destructor
 
        ~GidaspowErgunWenYu();
 
 
    // Member Functions
 
        tmp<volScalarField> K(const volScalarField& Ur) const;
};
 
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
} // End namespace Foam
 
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
 
#endif
 
// ************************************************************************* //
  • GidaspowErgunWenYu.C
 
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 1991-2004 OpenCFD Ltd.
     \\/     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 2 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, write to the Free Software Foundation,
    Inc., 59 Temple Place, Suite 330, Boston, MA 02111-1307 USA
 
\*---------------------------------------------------------------------------*/
 
#include "GidaspowErgunWenYu.H"
#include "addToRunTimeSelectionTable.H"
 
// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //
 
namespace Foam
{
    defineTypeNameAndDebug(GidaspowErgunWenYu, 0);
 
    addToRunTimeSelectionTable
    (
        dragModel,
        GidaspowErgunWenYu,
        dictionary
    );
}
 
 
// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //
 
// Construct from components
Foam::GidaspowErgunWenYu::GidaspowErgunWenYu
(
    const dictionary& interfaceDict,
    const volScalarField& alpha,
    const phaseModel& phasea,
    const phaseModel& phaseb
)
:
    dragModel(interfaceDict, alpha, phasea, phaseb)
{}
 
 
// * * * * * * * * * * * * * * * * Destructor  * * * * * * * * * * * * * * * //
 
Foam::GidaspowErgunWenYu::~GidaspowErgunWenYu()
{}
 
 
// * * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * //
 
Foam::tmp<Foam::volScalarField> Foam::GidaspowErgunWenYu::K
(
    const volScalarField& Ur
) const
{
    volScalarField beta = max(1.0 - alpha_, 1.0e-6);
 
    volScalarField bp = pow(beta, -2.65);
    volScalarField Re = max(Ur*phasea_.d()/phaseb_.nu(), 1.0e-3);
 
    volScalarField Cds = 24.0*(1.0 + 0.15*pow(Re, 0.687))/Re;
 
    forAll(Re, celli)
    {
        if(Re[celli] > 1000.0)
        {
            Cds[celli] = 0.44;
        }
    }
    
    // Wen and Yu (1966)
    volScalarField KWenYu = 0.75*Cds*phaseb_.rho()*Ur*bp/phasea_.d();
 
    // Ergun
    volScalarField KErgun = 150.0*alpha_*phaseb_.nu()*phaseb_.rho()
			    /(pow(beta*phasea_.d(), 2.0))
      			    + 1.75*phaseb_.rho()*Ur/(beta*phasea_.d());
 
    forAll (beta, cellj)
    {
	if (beta[cellj] <= 0.8)
        {
		KWenYu[cellj] = KErgun[cellj];
	}
    }
    
 
    return 1.0*KWenYu;
}
 
 
// ************************************************************************* //

2.3 References

  1. D. Gidaspow, Multiphase Flow and Fluidization: Continuum and Kinetic Theory Descriptions, Academic Press, New York, 1994.
  2. C. Y. Wen, Y. H. Yu, Mechanics of fluidization, Chemical Engineering Progress Symposium Series, 62:100-111, 1966.

--Alberto 03:21, 29 Aug 2005 (CEST)