Additional drag models for the twoPhaseEulerFoam solver

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

Dalla Valle, J.M., 1948, Micromeritics, Pitman, London.

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.

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

D. Gidaspow, Multiphase Flow and Fluidization: Continuum and Kinetic Theory Descriptions, Academic Press, New York, 1994.
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)