CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   How to modify kinematic viscosity "nu" within the time loop? (http://www.cfd-online.com/Forums/openfoam-solving/87674-how-modify-kinematic-viscosity-nu-within-time-loop.html)

taner April 26, 2011 08:50

How to modify kinematic viscosity "nu" within the time loop?
 
Dear all,

kinematic viscosity "nu" can be modified during the runtime by changing its value in the "transportProperties" dictionary.
Is there a simple way to change its value within the time loop?
I would like to define it as a function of time/iterations in a SIMPLE solver to improve convergence like:

while (runTime.loop())
{

if ( current_time <= some_fixed_time )
{
nu = nu_desired * ( some_fixed_time / current_time );
}
else
{
nu = nu_desired;
}

...

}

so that it reaches to the desired value after some fixed time. I would appreciate any proposal to implement it in an elegant way.

Thanks in advance
Taner.

MartinB April 26, 2011 09:41

Hi Taner,

I propose to modify one of the existing viscosity models. You can find them in OpenFOAM-xxx/src/transportModels/incompressible/viscosityModels/.

Add some new values to the constant/transportProperties file, for example nu_start, nu_desired and some_fixed_time. Read these values into your new viscosity model class and adjust the current nu in dependency of the current time step.

This approach should work directly for simpleFoam or nonNewtonianIcoFoam and every other solver that uses non newtonian material models.

Martin

MartinB April 26, 2011 14:01

Well, here is a quick implementation. I changed the algorithm a little bit so that it runs more smoothly with my test case.

First, the "constant/transportProperties" file:
Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  1.6                                  |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    format      ascii;
    class      dictionary;
    location    "constant";
    object      transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

transportModel  approachingNu;

approachingNuCoeffs
{
    nu_desired            nu_desired [ 0 2 -1 0 0 0 0 ] 1e-06;
    nu_start                  nu_start [ 0 2 -1 0 0 0 0 ] 1.0;
    some_fixed_time  some_fixed_time [ 0 0 1 0 0 0 0 ] 200;
}

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

Here is the header file "approachingNu.H", written and roughly tested for OpenFOAM-1.6-ext:
Code:

/*---------------------------------------------------------------------------*\
  =========                |
  \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox
  \\    /  O peration    |
    \\  /    A nd          | Copyright held by original author
    \\/    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., 51 Franklin St, Fifth Floor, Boston, MA 02110-1301 USA

Class
    Foam::viscosityModels::approachingNu

Description
    A material model which is approaching the desired viscosity nu_desired,
    starting from nu_start.

    A blended algorithm is:
    if (current_time < some_fixed_time_)
    {
        scalar alpha = current_time / some_fixed_time;
        return (alpha * nu_desired_ + (1 - alpha) * nu_start_);
    }
    else
    {
        return nu_desired_;
    }

    However this one behaves better in my tests:
    if (current_time < some_fixed_time_)
    {
        scalar alpha = (nu_start * 1000 / nu_desired) ^ (1/some_fixed_time)
        return (nu_start / (alpha ^ current_time)) + nu_desired;
    }
    else
    {
        return nu_desired_;
    }
   

SourceFiles
    approachingNu.C

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

#ifndef approachingNu_H
#define approachingNu_H

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

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

namespace Foam
{
namespace viscosityModels
{

/*---------------------------------------------------------------------------*\
                          Class approachingNu Declaration
\*---------------------------------------------------------------------------*/

class approachingNu
:
    public viscosityModel
{
    // Private data

        dictionary approachingNuCoeffs_;

        dimensionedScalar nu_desired_;
        dimensionedScalar nu_start_;
        dimensionedScalar some_fixed_time_;

        volScalarField nu_;


    // Private Member Functions

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


public:

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


    // Constructors

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


    // Destructor

        ~approachingNu()
        {}


    // Member Functions

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

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

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


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

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

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

#endif

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

And the "approachingNu.C" file:
Code:

/*---------------------------------------------------------------------------*\
  =========                |
  \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox
  \\    /  O peration    |
    \\  /    A nd          | Copyright held by original author
    \\/    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., 51 Franklin St, Fifth Floor, Boston, MA 02110-1301 USA

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

#include "approachingNu.H"
#include "addToRunTimeSelectionTable.H"
#include "surfaceFields.H"

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

namespace Foam
{
namespace viscosityModels
{
    defineTypeNameAndDebug(approachingNu, 0);
    addToRunTimeSelectionTable
    (
        viscosityModel,
        approachingNu,
        dictionary
    );
}
}


// * * * * * * * * * * * * Private Member Functions  * * * * * * * * * * * * //
/* this is the linear blended algorithm... however I do prefer the alternative algorithm below
Foam::tmp<Foam::volScalarField>
Foam::viscosityModels::approachingNu::calcNu() const
{
    scalar current_time((U_.time()).value());
    Info << "current_time = " << current_time << endl;
    Info << "some_fixed_time_ = " << some_fixed_time_.value() << endl;

    if (current_time < some_fixed_time_.value())
    {
        scalar alpha = current_time / some_fixed_time_.value();
        Info << "alpha = " << alpha << ", nu = " << (alpha * nu_desired_ + (1 - alpha) * nu_start_) << endl;
        return
        (
            strainRate() * dimensionedScalar("dummy",nu_desired_.dimensions()*dimTime,0.0) // dummy for adding strainRate dependend model
            + (alpha * nu_desired_ + (1 - alpha) * nu_start_)
        );
    }
    else
    {
        Info << "nu = " << nu_desired_ << endl;
        return
        (
            strainRate() * dimensionedScalar("dummy",nu_desired_.dimensions()*dimTime,0.0) // dummy for adding strainRate dependend model
            + nu_desired_
        );
    }
}
*/
Foam::tmp<Foam::volScalarField>
Foam::viscosityModels::approachingNu::calcNu() const
{
    scalar current_time((U_.time()).value());
    //Info << "current_time = " << current_time << endl;
    //Info << "some_fixed_time_ = " << some_fixed_time_.value() << endl;

    if (current_time < some_fixed_time_.value())
    {
        scalar alpha = pow((nu_start_.value()*1000/nu_desired_.value()), (1/some_fixed_time_.value()));
        //Info << "alpha = " << alpha << ", nu = " << (nu_start_ / (pow(alpha, current_time))) + nu_desired_ << endl;
        return
        (
            strainRate() * dimensionedScalar("dummy",nu_desired_.dimensions()*dimTime,0.0) // dummy for adding strainRate dependend model
            + (nu_start_ / (pow(alpha, current_time))) + nu_desired_
        );
    }
    else
    {
        //Info << "nu = " << nu_desired_ << endl;
        return
        (
            strainRate() * dimensionedScalar("dummy",nu_desired_.dimensions()*dimTime,0.0) // dummy for adding strainRate dependend model
            + nu_desired_
        );
    }
}

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

Foam::viscosityModels::approachingNu::approachingNu
(
    const word& name,
    const dictionary& viscosityProperties,
    const volVectorField& U,
    const surfaceScalarField& phi
)
:
    viscosityModel(name, viscosityProperties, U, phi),
    approachingNuCoeffs_(viscosityProperties.subDict(typeName + "Coeffs")),
    nu_desired_(approachingNuCoeffs_.lookup("nu_desired")),
    nu_start_(approachingNuCoeffs_.lookup("nu_start")),
    some_fixed_time_(approachingNuCoeffs_.lookup("some_fixed_time")),
   
    nu_
    (
        IOobject
        (
            "nu",
            U_.time().timeName(),
            U_.db(),
            IOobject::NO_READ,
            IOobject::AUTO_WRITE
        ),
        calcNu()
    )
{}


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

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

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

    approachingNuCoeffs_.lookup("nu_desired") >> nu_desired_;
    approachingNuCoeffs_.lookup("nu_start") >> nu_start_;
    approachingNuCoeffs_.lookup("some_fixed_time") >> some_fixed_time_;

    return true;
}


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

For non-Extend OpenFOAM versions it should be
Code:

tmp<volScalarField> nu() const
in line 126 instead, but I didn't test it with these versions...

Martin

taner April 28, 2011 03:51

Hi Martin,
I appreciated your quick and accurate support very much.
The model that you implemented works well for the non-extended, official OpenFOAM 1.7.1.
Best regards,
Taner.

hossein_y62 January 8, 2013 04:12

Hi every body,

I need to change the power law in the OpenFOAM-xxx/src/transportModels/incompressible/viscosityModels/ directory. How can I do that?

the default power law model defines nuMax and nuMin, as I set them to 100000 and 0 respectively, the run time will increase dramatically. I have to notice that I am using interFoam Solver.

It would be very appreciated if someone could help me,

Thanx


All times are GMT -4. The time now is 03:07.