CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Programming & Development

New Viscosity Model - Best Practice for Temporary Values

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree1Likes
  • 1 Post By MaSch

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 23, 2016, 11:52
Default New Viscosity Model - Best Practice for Temporary Values
  #1
New Member
 
Join Date: Aug 2016
Posts: 4
Rep Power: 7
MaSch is on a distinguished road
Hello FOAMers,
currently I am implementing a temperature-dependant viscosity model, to be concise, the Carreau-WLF-Model, for polymer melts. It is very similiar to a Cross-WLF-model. (See equations 2.29 and 2.32 in this preview for more details: http://files.hanser.de/hanser/docs/2..._Leseprobe.pdf)

I have referred to the following materials:

http://www.cfd-online.com/Forums/ope...time-loop.html

http://www.tfd.chalmers.se/~hani/kur...nFoam%20v2.pdf

http://www.cfd-online.com/Forums/ope...mperature.html


Given the fact that the equation is - while not complex - rather long, I tried to split it up across several lines. See this snippet from GermanCarreau.C.

Code:
// * * * * * * * * * * * * Private Member Functions  * * * * * * * * * * * * //

Foam::tmp<Foam::volScalarField>
Foam::viscosityModels::GermanCarreau::calcNu() const
{
const volScalarField& Tcurrent=U_.mesh().lookupObject<volScalarField>("T");


Foam::dimensionedScalar Tsp1 = Te_+scalar(50);
Foam::dimensionedScalar termA = (scalar(8.86)*(Tmeasure_ - Tsp1)) / (scalar(101.6)+(Tmeasure_ -Tsp1));
Foam::dimensionedScalar termB = (scalar(8.86)*(Tcurrent - Tsp1)) / (scalar(101.6)+(Tcurrent -Tsp1));
Foam::dimensionedScalar alpha_shift = pow(scalar(10), (termA - termB));
Foam::dimensionedScalar eta_shifted = ( (alpha_shift*A_) / (pow (eta_shifted*scalar(1)*strainRate()*B_, C_) ));

    return (eta_shifted/rho_.value()

    );
}
This fails to compile, resulting in the following errors:

Code:
viscosityModels/GermanCarreau/GermanCarreau.C:58:82: error: conversion from ‘Foam::tmp<Foam::DimensionedField<double, Foam::volMesh> >’ to non-scalar type ‘Foam::dimensionedScalar {aka Foam::dimensioned<double>}’ requested
 Foam::dimensionedScalar termB = (scalar(8.86)*(Tcurrent.internalField() - Tsp1)) / (scalar(101.6)+(Tcurrent.internalField()  -Tsp1));
                                                                                  ^
viscosityModels/GermanCarreau/GermanCarreau.C:60:58: error: conversion from ‘Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >’ to non-scalar type ‘Foam::dimensionedScalar {aka Foam::dimensioned<double>}’ requested
 Foam::dimensionedScalar eta_shifted = ( (alpha_shift*A_) / (pow (eta_shifted*scalar(1)*strainRate()*B_, C_) ));
                                                          ^
viscosityModels/GermanCarreau/GermanCarreau.C:62:24: error: could not convert ‘Foam::operator/(const Foam::dimensioned<Type>&, const Foam::dimensioned<double>&) [with Type = double](Foam::dimensioned<double>((* &((const Foam::viscosityModels::GermanCarreau*)this)->Foam::viscosityModels::GermanCarreau::rho_.Foam::dimensioned<Type>::value<double>())))’ from ‘Foam::dimensioned<double>’ to ‘Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >’
     return (eta_shifted/rho_.value()
                        ^
viscosityModels/GermanCarreau/GermanCarreau.C: In constructor ‘Foam::viscosityModels::GermanCarreau::GermanCarreau(const Foam::word&, const Foam::dictionary&, const volVectorField&, const surfaceScalarField&)’:
viscosityModels/GermanCarreau/GermanCarreau.C:81:5: error: class ‘Foam::viscosityModels::GermanCarreau’ does not have any field named ‘GermanCarreauCoeffs_’
     GermanCarreauCoeffs_(viscosityProperties.subDict(typeName + "Coeffs")),
     ^
viscosityModels/GermanCarreau/GermanCarreau.C:82:22: error: ‘GermanCarreauCoeffs_’ was not declared in this scope
     A_("A", dimless, GermanCarreauCoeffs_),
                      ^
viscosityModels/GermanCarreau/GermanCarreau.C:83:21: error: expected ‘)’ before ‘GermanCarreauCoeffs_’
     B_("B", dimless GermanCarreauCoeffs_),
As you can see, Scalars and volScalarFields cannot be used together.

As far as I understand, the transport equation is evaluated for each point in the flow field - so how would I go about describing my temporary variables in terms of OpenFOAM data types? How would you approach such a problem?

Is my approach of compartmentalizing the equation fundamentally sound?

Can you point to a implented transport model that utilizes a very long formula in a similar manner?

Thank you very much!

Attached, you'll find GermanCarreau.C and GermanCarreau.H:

GermanCarreau.C
Code:
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011-2015 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/>.

\*---------------------------------------------------------------------------*/

#include "GermanCarreau.H"
#include "addToRunTimeSelectionTable.H"
#include "surfaceFields.H"

// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //

namespace Foam
{
namespace viscosityModels
{
    defineTypeNameAndDebug(GermanCarreau, 0);

    addToRunTimeSelectionTable
    (
        viscosityModel,
        GermanCarreau,
        dictionary
    );
}
}


// * * * * * * * * * * * * Private Member Functions  * * * * * * * * * * * * //

Foam::tmp<Foam::volScalarField>
Foam::viscosityModels::GermanCarreau::calcNu() const
{
const volScalarField& Tcurrent=U_.mesh().lookupObject<volScalarField>("T");


Foam::dimensionedScalar Tsp1 = Te_+scalar(50);
Foam::dimensionedScalar termA = (scalar(8.86)*(Tmeasure_ - Tsp1)) / (scalar(101.6)+(Tmeasure_ -Tsp1));
Foam::dimensionedScalar termB = (scalar(8.86)*(Tcurrent - Tsp1)) / (scalar(101.6)+(Tcurrent -Tsp1));
Foam::dimensionedScalar alpha_shift = pow(scalar(10), (termA - termB));
Foam::dimensionedScalar eta_shifted = ( (alpha_shift*A_) / (pow (eta_shifted*scalar(1)*strainRate()*B_, C_) ));

    return (eta_shifted/rho_.value()



    );
}


// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //

Foam::viscosityModels::GermanCarreau::GermanCarreau
(
    const word& name,
    const dictionary& viscosityProperties,
    const volVectorField& U,
    const surfaceScalarField& phi
)
:
    viscosityModel(name, viscosityProperties, U, phi),
    GermanCarreauCoeffs_(viscosityProperties.subDict(typeName + "Coeffs")),
    A_("A", dimless, GermanCarreauCoeffs_),
    B_("B", dimless GermanCarreauCoeffs_),
    C_("C", dimless, GermanCarreauCoeffs_),
    Te_(GermanCarreauCoeffs_.lookup("Te"),
    rho_("rho", dimless, GermanCarreauCoeffs_),
    Tmeasure_("Tmeasure", dimless, GermanCarreauCoeffs_),
    pFactor_("pFactor", dimless, GermanCarreauCoeffs_),



    nu_
    (
        IOobject
        (
            name,
            U_.time().timeName(),
            U_.db(),
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        calcNu()
    )
{}


// * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * * //

bool Foam::viscosityModels::GermanCarreau::read
(
    const dictionary& viscosityProperties
)
{
    viscosityModel::read(viscosityProperties);

    GermanCarreau_ = viscosityProperties.subDict(typeName + "Coeffs");

    GermanCarreauCoeffs_.lookup("A") >> A_;
    GermanCarreauCoeffs_.lookup("B") >> B_;
    GermanCarreauCoeffs_.lookup("C") >> C_;
    GermanCarreauCoeffs_.lookup("Te") >> Te_;
    GermanCarreauCoeffs_.lookup("rho") >> rho_;
    GermanCarreauCoeffs_.lookup("Tmeasure") >> Tmeasure_;
    GermanCarreauCoeffs_.lookup("pFactor") >> pFactor_;


    return true;
}


// ************************************************************************* //
GermanCarreau.H
Code:
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011 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::viscosityModels::GermanCarreau

Description
    An incompressible isothermal Carreau Three-factor viscosity model.

SourceFiles
    GermanCarreau.C

\*---------------------------------------------------------------------------*/

#ifndef GermanCarreau_H
#define GermanCarreau_H

#include "viscosityModel.H"
#include "dimensionedScalar.H"
#include "volFields.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

namespace Foam
{
namespace viscosityModels
{

/*---------------------------------------------------------------------------*\
                           Class GermanCarreau Declaration
\*---------------------------------------------------------------------------*/

class GermanCarreau
:
    public viscosityModel
{
    // Private data

        dictionary GermanCarreau_;

        dimensionedScalar A_;
        dimensionedScalar B_;
        dimensionedScalar C_;
        dimensionedScalar rho_;
        dimensionedScalar Te_;
        dimensionedScalar Tmeasure_;
        dimensionedScalar pFactor_;

        dimensionedScalar Tsp2_;
        dimensionedScalar termA_;
        dimensionedScalar termB_;
        dimensionedScalar eta_shifted_;
        dimensionedScalar alpha_shift_;

        volScalarField nu_;

    // Private Member Functions

        //- Calculate and return the laminar viscosity
        tmp<volScalarField> calcNu() const;


public:

    //- Runtime type information
    TypeName("GermanCarreau");


    // Constructors

        //- Construct from components
        GermanCarreau
        (
            const word& name,
            const dictionary& viscosityProperties,
            const volVectorField& U,
            const surfaceScalarField& phi
        );


    //- Destructor
    ~GermanCarreau()
    {}


    // Member Functions

        //- Return the laminar viscosity
        tmp<volScalarField> nu() const
        {
            return nu_;
        }

        //- Return the laminar viscosity for patch
        tmp<scalarField> nu(const label patchi) const
        {
            return nu_.boundaryField()[patchi];
        }

        //- Correct the laminar viscosity
        void correct()
        {
            nu_ = calcNu();
        }

        //- Read transportProperties dictionary
        bool read(const dictionary& viscosityProperties);
};


// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

} // End namespace viscosityModels
} // End namespace Foam

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#endif

// ************************************************************************* //
MaSch is offline   Reply With Quote

Old   August 24, 2016, 04:36
Default
  #2
Senior Member
 
Gerhard Holzinger
Join Date: Feb 2012
Location: Austria
Posts: 305
Rep Power: 24
GerhardHolzinger will become famous soon enoughGerhardHolzinger will become famous soon enough
Hello,

in Line 58 you try to compute a dimensionedScalar with a formula containing a volScalarField. This is equivalent to compute a scalar directly from a vector. You can compute the magnitude of the vector or the inner product to gain a scalar, but otherwise you won't get a scalar out of a vector. The same logic applies to scalar fields.

Code:
Foam::dimensionedScalar termB = (scalar(8.86)*(Tcurrent - Tsp1)) / (scalar(101.6)+(Tcurrent -Tsp1));
Thus, in your model the variables termB, alpha_shift and eta_shifted need to be volScalarFields, unless you do something about Tcurrent, e.g. apply spatial averaging to make a scalar from the field.
GerhardHolzinger is offline   Reply With Quote

Old   August 24, 2016, 04:54
Default
  #3
New Member
 
Join Date: Aug 2016
Posts: 4
Rep Power: 7
MaSch is on a distinguished road
First off: Thank you a lot for your very useful feedback, Gerhard.

There is - however - a simple question remaining:

As far as I understand, the viscosity model is evaluated for each point the flow channel. Otherwise, shear thinning [that is, the reduction of the kinematic viscosity nu in areas of high shear rate] could not be observed.

How would I modify
Code:
const volScalarField& Tcurrent=U_.mesh().lookupObject<volScalarField>("T");{
so that Tcurrent is not the entire volScalarField, but rather the temperature of the node for which nu is currently being calculated?

Thanks again!
MaSch is offline   Reply With Quote

Old   August 24, 2016, 05:36
Default
  #4
Senior Member
 
Gerhard Holzinger
Join Date: Feb 2012
Location: Austria
Posts: 305
Rep Power: 24
GerhardHolzinger will become famous soon enoughGerhardHolzinger will become famous soon enough
If the variables termB, alpha_shift and eta_shifted are volScalarFields, then your formula is automatically evaluated for all cells of the mesh. There is no need to change the expression for Tcurrent.
GerhardHolzinger is offline   Reply With Quote

Old   August 25, 2016, 10:18
Default
  #5
New Member
 
Join Date: Aug 2016
Posts: 4
Rep Power: 7
MaSch is on a distinguished road
Hello Foamers, in the end I did manage to make it work. I used a hack described here:

http://www.cfd-online.com/Forums/ope...tml#post595370

so I could avoid having to manually create new volScalarFields.

Also, I left out the calculation of Tstandard. Now, Ts is defined in the transportProperties file.

A short test revealed that the results are accurate to within ca. 10%, which I blame on shear heating and my godawful mesh.

Attached you'll find the compileable files GermanCarreau.C and GermanCarreau.H. However, the material model only runs with a non-isothermal solver such as the one found here: http://www.dhcae-tools.com/docs/visousHeatingSolver.pdf

I hope you'll find my results useful!

Code:
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011-2015 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/>.

\*---------------------------------------------------------------------------*/

#include "GermanCarreau.H"
#include "addToRunTimeSelectionTable.H"
#include "surfaceFields.H"

// * * * * * * * * * * * * * * Static Data Members * * * * * * * * * * * * * //

namespace Foam
{
namespace viscosityModels
{
    defineTypeNameAndDebug(GermanCarreau, 0);

    addToRunTimeSelectionTable
    (
        viscosityModel,
        GermanCarreau,
        dictionary
    );
}
}


// * * * * * * * * * * * * Private Member Functions  * * * * * * * * * * * * //

Foam::tmp<Foam::volScalarField>
Foam::viscosityModels::GermanCarreau::calcNu() const
{
const volScalarField& Tcurrent=U_.mesh().lookupObject<volScalarField>("T");

volScalarField alpha_shift =Tcurrent;            //instead of constructing a new volScalarField, we "copy" the old one            
alpha_shift *= scalar(0.0);                //we then set all values of the volScalarField to zero
alpha_shift.dimensions().reset(dimless);        //also, since T is a Value in Kelvin, we make the new Field dimensionsless

volScalarField termA =Tcurrent;
termA *= scalar(0.0);
termA.dimensions().reset(dimless);

volScalarField termB =Tcurrent;
termB *= scalar(0.0);
termB.dimensions().reset(dimless);

volScalarField Tnew =Tcurrent;
Tnew.dimensions().reset(dimless);

//alpha_shift += scalar(1.2);
//Tsp1.dimensions().reset(dimLength*dimLength/dimTime);  //turns into a kinematic viscosity

termB = (scalar(8.86)*(Tnew - Ts_)) / (scalar(101.6)+(Tnew -Ts_));
termA = (scalar(8.86)*(Tmeasure_ - Ts_)) / (scalar(101.6)+(Tmeasure_ -Ts_));
alpha_shift = pow(scalar(10), (termA - termB));


     return (nuA_*alpha_shift)/(scalar(1) + pow(alpha_shift*B_*strainRate(), C_));
    
}


// * * * * * * * * * * * * * * * * Constructors  * * * * * * * * * * * * * * //

Foam::viscosityModels::GermanCarreau::GermanCarreau
(
    const word& name,
    const dictionary& viscosityProperties,
    const volVectorField& U,
    const surfaceScalarField& phi
)
:
    viscosityModel(name, viscosityProperties, U, phi),
    GermanCarreauCoeffs_(viscosityProperties.subDict(typeName + "Coeffs")),
    nuA_("nuA", dimViscosity, GermanCarreauCoeffs_),
    B_("B", dimTime, GermanCarreauCoeffs_),
    C_("C", dimless, GermanCarreauCoeffs_),
    Ts_("Ts", dimless, GermanCarreauCoeffs_),
    Tmeasure_("Tmeasure", dimless, GermanCarreauCoeffs_),
    nu_
    (
        IOobject
        (
            name,
            U_.time().timeName(),
            U_.db(),
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        
        ),    
               calcNu()
    )
{}

// * * * * * * * * * * * * * * Member Functions  * * * * * * * * * * * * * * //

bool Foam::viscosityModels::GermanCarreau::read
(
    const dictionary& viscosityProperties
)
{
    viscosityModel::read(viscosityProperties);

    GermanCarreauCoeffs_ = viscosityProperties.subDict(typeName + "Coeffs");

    GermanCarreauCoeffs_.lookup("nuA") >> nuA_;
    GermanCarreauCoeffs_.lookup("B") >> B_;
    GermanCarreauCoeffs_.lookup("C") >> C_;
    GermanCarreauCoeffs_.lookup("Ts") >> Ts_;
    GermanCarreauCoeffs_.lookup("Tmeasure") >> Tmeasure_;



    return true;
}


// ************************************************************************* //
Code:
/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011 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::viscosityModels::GermanCarreau

Description
    An incompressible isothermal Carreau Three-factor viscosity model with WLF correction for temperatures

SourceFiles
    GermanCarreau.C

\*---------------------------------------------------------------------------*/

#ifndef GermanCarreau_H
#define GermanCarreau_H

#include "viscosityModel.H"
#include "dimensionedScalar.H"
#include "volFields.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

namespace Foam
{
namespace viscosityModels
{

/*---------------------------------------------------------------------------*\
                           Class GermanCarreau Declaration
\*---------------------------------------------------------------------------*/

class GermanCarreau
:
    public viscosityModel
{
    // Private data

        dictionary GermanCarreauCoeffs_;

        dimensionedScalar nuA_;
        dimensionedScalar B_;
        dimensionedScalar C_;
        dimensionedScalar Ts_;
        dimensionedScalar Tmeasure_;

        volScalarField nu_;



    // Private Member Functions

        //- Calculate and return the laminar viscosity
        tmp<volScalarField> calcNu() const;


public:

    //- Runtime type information
    TypeName("GermanCarreau");


    // Constructors

        //- Construct from components
        GermanCarreau
        (
            const word& name,
            const dictionary& viscosityProperties,
            const volVectorField& U,
            const surfaceScalarField& phi
        );


    //- Destructor
    ~GermanCarreau()
    {}


    // Member Functions

        //- Return the laminar viscosity
        tmp<volScalarField> nu() const
        {
            return nu_;
        }

        //- Return the laminar viscosity for patch
        tmp<scalarField> nu(const label patchi) const
        {
            return nu_.boundaryField()[patchi];
        }

        //- Correct the laminar viscosity
        void correct()
        {
            nu_ = calcNu();
        }

        //- Read transportProperties dictionary
        bool read(const dictionary& viscosityProperties);
};


// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

} // End namespace viscosityModels
} // End namespace Foam

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

#endif

// ************************************************************************* //
vanq likes this.
MaSch is offline   Reply With Quote

Old   March 6, 2018, 03:41
Default Compressible thermophysical transport model
  #6
Member
 
Alberto
Join Date: Sep 2013
Posts: 37
Rep Power: 10
malv83 is on a distinguished road
Hello everyone,

I have seen some tutorials on how to modify the (incompressible) viscosity models (Powerlaw, Casson, etc.) to make them temperature dependent.

I am trying to modify a compressible thermo physical model, such as Sutherland model (for viscosity) which depends on Pressure and Temperature, but not on the strainRate.

The strainRate() is directly available for incompressible viscosityModels, but it is not available for compressible thermo physical model, such as Sutherland.

Does any body know how to make the Sutherland model strainRate dependent? in addition to the Pressure and Temperature dependency?.

I am using OpenFoam 5.x in Windows by BlueCFD.

Thanks in advanced
malv83 is offline   Reply With Quote

Old   March 16, 2018, 04:51
Default
  #7
New Member
 
Join Date: Aug 2016
Posts: 4
Rep Power: 7
MaSch is on a distinguished road
Dear malv,

while I'm not certain that it's going to work in the compressible flow model, you might try to calculate the strain rate directly from the flow field.

See this useful thread:
StrainRate definition 141 vs 15

which eventually arrives at:
Code:
strainrate= sqrt(2) * mag(symm(fvc::grad(U)))
MaSch is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Viscosity model - Compressible flow Aurelien Thinat OpenFOAM Programming & Development 3 March 6, 2018 08:08
Adding new temperature dependent viscosity model vabishek OpenFOAM Programming & Development 3 May 15, 2016 22:05
coefficient of power-Law viscosity Model in OpenFOAM Daniel_Khazaei OpenFOAM Running, Solving & CFD 6 April 5, 2016 05:23
How to modify the viscosity model mpml OpenFOAM Running, Solving & CFD 4 October 13, 2010 08:44
Regarding Implementation of Hershel Bulkley Model in Viscosity correlation Pathak FLOW-3D 0 August 24, 2009 07:34


All times are GMT -4. The time now is 21:24.