CFD Online Discussion Forums - Lund Recycled Method for LES (flat plate)

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)

- - Lund Recycled Method for LES (flat plate) (https://www.cfd-online.com/Forums/openfoam-solving/123889-lund-recycled-method-les-flat-plate.html)

Dear all,

Does anyone know what the boundary conditions for velocity(U) and pressure(p) used in Joachims example ( Lund Recycled Method for LES (flat plate)) are?

Yes, the boundary condition for the velocity is:

Code:

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2.2.0                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

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

FoamFile

{

    version     2.0;

    format      ascii;

    class       volVectorField;

    object      U;

}

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



dimensions      [0 1 -1 0 0 0 0];



internalField   uniform (1 0 0);



boundaryField

{

    inlet

    {

        type            scaledMappedVelocity;

        deltaInlet      0.243;

        thetaInlet      0.028;

        Ue              1;

        nu              2e-5;

        t               2e-2;

        UMeanSpanTime   uniform (0 0 0);

        value           uniform (1 0 0);

    }

    outlet

    {

        type            advective;

    }

    plate0

    {

        type            fixedValue;

        value           uniform (0 0 0);

    }

    plate1

    {

        type            fixedValue;

        value           uniform (0 0 0);

    }

    top0

    {

        type            zeroGradient;

    }

    top1

    {

        type            zeroGradient;

    }

    front0

    {

        type            cyclic;

    }

    front1

    {

        type            cyclic;

    }

    back0

    {

        type            cyclic;

    }

    back1

    {

        type            cyclic;

    }

    interface0

    {

        type            cyclic;

    }

    interface1

    {

        type            cyclic;

    }

}

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

and the boundary condition for the pressure is:

Code:

/*--------------------------------*- C++ -*----------------------------------*\

| =========                 |                                                 |

| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |

|  \\    /   O peration     | Version:  2.2.0                                 |

|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |

|    \\/     M anipulation  |                                                 |

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

FoamFile

{

    version     2.0;

    format      ascii;

    class       volScalarField;

    object      p;

}

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



dimensions      [0 2 -2 0 0 0 0];



internalField   uniform 0;



boundaryField

{

    inlet

    {

        type            zeroGradient;

    }

    outlet

    {

        type            fixedValue;

        value           uniform 0;

    }

    plate0

    {

        type            zeroGradient;

    }

    plate1

    {

        type            zeroGradient;

    }

    top0

    {

        type            fixedValue;

    value        uniform 0;

    }

    top1

    {

        type            fixedValue;

    value        uniform 0;

    }

    front0

    {

        type            cyclic;

    }

    front1

    {

        type            cyclic;

    }

    back0

    {

        type            cyclic;

    }

    back1

    {

        type            cyclic;

    }

    interface0

    {

        type            cyclic;

    }

    interface1

    {

        type            cyclic;

    }

}



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

All the best,
Christoph

Dear Christoph,

Thank you so much for your quick reply!!!
I have really been struggling to get the boundary conditions right for
this problem. I will try them right away!

Dear Christoph,

Thank you for uploading the BC files. I tried them with my case and was able to get the problem working after some modifications.
The major problem other than the BC's was the accuracy in my solves at each time step. The lack of accuracy was creating
artificial turbulence and corrupting my solution.

Sincerely,
-Tsuyoshi Koyama

Hi Foamers,

I'm really curious about this method, but unfortunately there is nothing in the dropbox link...Can anyone send me a copy of the test case to the address zfr2078@gmail.com ? Thanks in advance!!:)

Regards
J Zhang

Dear all,

You might be interested in looking at a python package I have written, it allows to rescale sampled velocity fields using the Lund's rescaling procedure and save them in a format readable by OpenFOAM.

There is a User guide available here:
http://eddylicious.readthedocs.io/
And the code is here
https://github.com/timofeymukha/eddylicious

Hi Joachim,

I am very interested in Lund's recycling methods but unfortunately it is used for incompressible flows. So I studied recaling-recycling method and extend it for compressible flows just by adding Van Driest velocity to scaledMappedVelocity and creating scaledMappedTemperature. But I have encountered a problem: I run these boundary conditions well using single processor but failed in parallel calculating. By the way, have you ever calculated in parallel using your code? I just modified your code by adding some extra codes and I think it doesn't affect parallel process. Here's my attached codes for compressible flows.

P.S. my OpenFOAM version is 2.4.0

Quote:

Originally Posted by cfd.with.openfoam (Post 463790)

In this rescaling technique it seems that I would still need a mean profile for different variables at the inlet of my domain. After that I would need to perturb the domain e.g using the perturbU utility. After following these steps I should expect a self sustaining turbulent BL. Is that correct?

Hi All,

I wonder where perturbU utility is, there's no such utility in offical version of OpenFOAM, and I don't know how to calculate the initial field for following LES calculation. Any suggestions?

Best,
Eric

That utility has been taken out of the standard version (not sure why?) but there's a link in the wiki explaining how to add it back:
https://openfoamwiki.net/index.php/Contrib/perturbU
it's very simple and straightforward.

Hi Mahdi,

Thanks for your quick response, I have download perturbU and successfully compiled it on OpenFOAM-2.4.0. I opened the perturbU.C and after scanning the code I know that

Code:

if (setBulk)

{}

is to set the mean velocity profile and

Code:

if (perturb)

{}

is to set perturbation. To see how the perturbation is generated. I found it in the following codes:

Code:

 if (perturb)

        {

            // streak streamwise velocity

            U[celli][streamDir] +=

                (utau * duplus/2.0) * (yplus/40.0)

                * Foam::exp(-sigma * Foam::sqr(yplus) + 0.5)

                * Foam::cos(betaPlus*zplus)*deviation;



            // streak spanwise perturbation

            U[celli][spanDir] =

                epsilon

              * Foam::sin(alphaPlus*xplus)

              * yplus

              * Foam::exp(-sigma*Foam::sqr(yplus))

              * deviation;

        }

I don't know why use these formula to set perturbation.
Is there any perturbation theory or related references?

Best

Random perturbations will be easily damped out if they lack a spatial correlation. Also to initialize don't use turbulent profile, use laminar.
Those streaks are based on a paper by Schoppa and Hussain:
https://www.researchgate.net/publica...all_turbulence
They are the best way to excite the near wall fluctuations and transient into turbulent.

Quote:

Originally Posted by Eric Brant (Post 624597)

Hi Eric，
I tried your BCs. Add "mpp.distribute(URecycled);" in scaledMappedTemperatureFixedValueFvPatchField.C, and it will work fine in parallel calculating.
Of course， you may have already solved this problem.
By the way, which paper are your BCs based on？And how do you set your boundary condition for field p?
Best
Yifan

Hi,

I need this BC for my DNS simulation, can anyone share the code and additional files to me? My email is 32420171152101@stu.xmu.edu.cn

Thank you very much.

Could you send me a copy of your case files? It would be great help to setup a base case for comparison of synthetic inflow generation method. My email is y.wang@ttu.edu. Thanks a lot.

Hi all,

Can anyone please send me the Joachim's code? I did bit of search but couldn't find it anywhere online. Email: oguzhanmurat06@gmail.com

Thanks.

Dear all

I'm really curious about this method, but unfortunately there is nothing in the dropbox link...Can anyone send me a copy of the test case to the address shawnhu94@gmail.com ? Thanks in advance!:D

Quote:

Originally Posted by Loey (Post 603753)

Hi, Vishwakarma
Thank you for your kindness. I have got a copy, but I have a question to ask: How is the initial internalField generated?
Loey

Dear Loey

I'm really curious about this method, but unfortunately there is nothing in the dropbox link...Can anyone send me a copy of the test case to the address shawnhu94@gmail.com ? Thanks in advance!

Run runLundRescaling --config=rescalingConfigBot

Hi Foamers

Can somebody please tell me how to proceed with this runLundRescaling --config=rescalingConfigBot

as mentioned in https://github.com/timofeymukha/eddy..._lund.rst#id15
I am unable to run this command.

Hi. So, did you install eddylicious? The command is part of the package.

Hi,

I'm really interested in the Lund's method,but the test case in the dropbox doesn't exist. Can anyone share the files to me? My email is jayddkt@sjtu.edu.cn

Thanks a lot.