[fumiya]

As you know, perturbU utility [1] can be used
to generate an initial velocity field for large eddy simulation
of channel flow. This utility is not included in the official release
version but we can substitute setExprFields utility [2] for it.
The settings of setExprFields utility are specified in system/setExprFieldsDict file.

The following code is an implementation of perturbU by setExprFields utility
for the tutorial incompressible/pimpleFoam/LES/channel395.

You can play around with the tutorial by changing its mesh resolution.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2006                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      setExprFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

expressions
(
    U
    {
        field       U;
        dimensions  [0 1 -1 0 0 0 0];

//        constants
//        {
//        }

        variables
        (
            "Retau = 395"
            "Ubar = 0.1335"
            "nu = 2e-05"
            "h = 1"
            "utau = Retau*nu/h"
            "y = (pos().y() <= h) ? pos().y() : 2.0*h - pos().y()"
            "yPlus = y*Retau/h"
            "xPlus = pos().x()*Retau/h"
            "zPlus = pos().z()*Retau/h"
            "duPlus = Ubar*0.25/utau"
            "betaPlus = 2.0*pi()/200.0"
            "sigma = 0.00055"
            "alphaPlus = 2.0*pi()/500.0"
            "epsilon = Ubar/200.0"
            "deviation = pos().x()/pos().x() + 0.4*(rand() - 0.5)"
        );

        condition
        #{
            (pos().x() > -10)
        #};

        expression
        #{
            vector
            (
                1.5*Ubar*pos().y()*(2.0*h - pos().y())
              + (utau*duPlus/2.0)*(yPlus/40.0)*exp(-sigma*sqr(yPlus) + 0.5)*cos(betaPlus*zPlus)*deviation,
                0.0,
                epsilon*sin(alphaPlus*xPlus)*yPlus*exp(-sigma*sqr(yPlus))*deviation
            )
        #};
    }
);

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

The following link is an animation:
https://twitter.com/ennovacfd/status...96828440895488

[1] https://github.com/wyldckat/perturbU
[2] https://www.openfoam.com/documentati...xprFields.html

Hope this helps,
Fumiya

[fumiya]

The setExprFields utility in OpenFOAM v2006 does not work if the entry "condition" is empty as shown below:

        condition
        #{
        #};

[ht2017]

Originally Posted by fumiya

As you know, perturbU utility [1] can be used
to generate an initial velocity field for large eddy simulation
of channel flow. This utility is not included in the official release
version but we can substitute setExprFields utility [2] for it.
The settings of setExprFields utility are specified in system/setExprFieldsDict file.

The following code is an implementation of perturbU by setExprFields utility
for the tutorial incompressible/pimpleFoam/LES/channel395.

You can play around with the tutorial by changing its mesh resolution.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2006                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      setExprFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

expressions
(
    U
    {
        field       U;
        dimensions  [0 1 -1 0 0 0 0];

//        constants
//        {
//        }

        variables
        (
            "Retau = 395"
            "Ubar = 0.1335"
            "nu = 2e-05"
            "h = 1"
            "utau = Retau*nu/h"
            "y = (pos().y() <= h) ? pos().y() : 2.0*h - pos().y()"
            "yPlus = y*Retau/h"
            "xPlus = pos().x()*Retau/h"
            "zPlus = pos().z()*Retau/h"
            "duPlus = Ubar*0.25/utau"
            "betaPlus = 2.0*pi()/200.0"
            "sigma = 0.00055"
            "alphaPlus = 2.0*pi()/500.0"
            "epsilon = Ubar/200.0"
            "deviation = pos().x()/pos().x() + 0.4*(rand() - 0.5)"
        );

        condition
        #{
            (pos().x() > -10)
        #};

        expression
        #{
            vector
            (
                1.5*Ubar*pos().y()*(2.0*h - pos().y())
              + (utau*duPlus/2.0)*(yPlus/40.0)*exp(-sigma*sqr(yPlus) + 0.5)*cos(betaPlus*zPlus)*deviation,
                0.0,
                epsilon*sin(alphaPlus*xPlus)*yPlus*exp(-sigma*sqr(yPlus))*deviation
            )
        #};
    }
);

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

The following link is an animation:
https://twitter.com/ennovacfd/status...96828440895488

[1] https://github.com/wyldckat/perturbU
[2] https://www.openfoam.com/documentati...xprFields.html

Hope this helps,
Fumiya

What is the theory for this code? Because I want to simulate for channel flow but different the size with this tutorial so I need to write a new code but I don't know how to write it. could you tell me what is the theory to write the code?
thank you

[olesen]

Originally Posted by fumiya

The setExprFields utility in OpenFOAM v2006 does not work if the entry "condition" is empty as shown below:

        condition
        #{
        #};

That should be fixed in the 2012 release, and in the 2006 maintenance branch.

[ht2017]

Originally Posted by olesen

That should be fixed in the 2012 release, and in the 2006 maintenance branch.

Hi Olesen,
I have run both the case. case 1 that is a tutorial available in Openfoam chanel395 and another case (case 2) I run with create fluctuation velocity with this code. But I get the result different about velocity mean and R11. Could you tell me how to run with the code more correct result?

case2: Run with code to create fluctuation.

velocity mean magnitu


UPrime2Mean_XX (R11)



Case 1: chanel395

velocity mean magnitude



UPrime2Mean_XX (R11)

[ht2017]

Originally Posted by fumiya

As you know, perturbU utility [1] can be used
to generate an initial velocity field for large eddy simulation
of channel flow. This utility is not included in the official release
version but we can substitute setExprFields utility [2] for it.
The settings of setExprFields utility are specified in system/setExprFieldsDict file.

The following code is an implementation of perturbU by setExprFields utility
for the tutorial incompressible/pimpleFoam/LES/channel395.

You can play around with the tutorial by changing its mesh resolution.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v2006                                 |
|   \\  /    A nd           | Website:  www.openfoam.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      setExprFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

expressions
(
    U
    {
        field       U;
        dimensions  [0 1 -1 0 0 0 0];

//        constants
//        {
//        }

        variables
        (
            "Retau = 395"
            "Ubar = 0.1335"
            "nu = 2e-05"
            "h = 1"
            "utau = Retau*nu/h"
            "y = (pos().y() <= h) ? pos().y() : 2.0*h - pos().y()"
            "yPlus = y*Retau/h"
            "xPlus = pos().x()*Retau/h"
            "zPlus = pos().z()*Retau/h"
            "duPlus = Ubar*0.25/utau"
            "betaPlus = 2.0*pi()/200.0"
            "sigma = 0.00055"
            "alphaPlus = 2.0*pi()/500.0"
            "epsilon = Ubar/200.0"
            "deviation = pos().x()/pos().x() + 0.4*(rand() - 0.5)"
        );

        condition
        #{
            (pos().x() > -10)
        #};

        expression
        #{
            vector
            (
                1.5*Ubar*pos().y()*(2.0*h - pos().y())
              + (utau*duPlus/2.0)*(yPlus/40.0)*exp(-sigma*sqr(yPlus) + 0.5)*cos(betaPlus*zPlus)*deviation,
                0.0,
                epsilon*sin(alphaPlus*xPlus)*yPlus*exp(-sigma*sqr(yPlus))*deviation
            )
        #};
    }
);

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

The following link is an animation:
https://twitter.com/ennovacfd/status...96828440895488

[1] https://github.com/wyldckat/perturbU
[2] https://www.openfoam.com/documentati...xprFields.html

Hope this helps,
Fumiya

Do you know how to consider the sigma parameter? When I run with the meter scale may be the value 0.0005 it is well working but when I run with millimeter-scale it it not well for working.

[Michael@UW]

Originally Posted by olesen

That should be fixed in the 2012 release, and in the 2006 maintenance branch.

I tested in 2106.
If you do not need a condition, then condition block should be commented out, otherwise, it gives a syntax error.

The following does not work

        condition
        #{
            //(pos().y() > -10) && (pos().z() > -10)
        #};

Need to comment out the whole block:

        // condition
        // #{
        //     (pos().y() > -10) && (pos().z() > -10)
        // #};