CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

PerturbU

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

Like Tree11Likes
  • 1 Post By hadi
  • 2 Post By alberto
  • 1 Post By wyldckat
  • 1 Post By amanbearpig
  • 4 Post By adambarfi
  • 2 Post By wyldckat

Reply
 
LinkBack Thread Tools Display Modes
Old   July 3, 2007, 05:22
Default Hi to all, I am a new openF
  #1
Member
 
hadi tartoussi
Join Date: Mar 2009
Location: paris
Posts: 48
Rep Power: 8
hadi is on a distinguished road
Hi to all,

I am a new openFoam user,and i would like to know if the perturbU utility exists by default in openFOam or i should add it?
can u please tell me how to get this utility?

thanks in advance
Hadi
hua1015 likes this.
hadi is offline   Reply With Quote

Old   July 3, 2007, 07:00
Default Hello, it's not included in O
  #2
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Hello,
it's not included in OpenFOAM. You can download it here:

- For a channel:

http://www.cfd-online.com/OpenFOAM_D...ages/1/40.html

- For a cylinder:

http://www.cfd-online.com/OpenFOAM_D...es/1/2946.html

With kind regards,
Alberto
songwukong and jarpve like this.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   July 3, 2007, 07:23
Default Thank you very much Alberto
  #3
Member
 
hadi tartoussi
Join Date: Mar 2009
Location: paris
Posts: 48
Rep Power: 8
hadi is on a distinguished road
Thank you very much Alberto

regards
Hadi
hadi is offline   Reply With Quote

Old   December 14, 2013, 14:44
Default
  #4
New Member
 
Join Date: Feb 2013
Posts: 8
Rep Power: 4
pante is on a distinguished road
hello,
I try to download perturbU utility for using it in a pipe flow, but for some reason I get a file of type .unk (unknown). Can anyone provide me a valid link for downloading perturbU utility?
pante is offline   Reply With Quote

Old   December 14, 2013, 19:21
Default
  #5
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,253
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings pante,

The old forum had this safety mechanism, where the attached files were renamed to always have the file extension ".unk".

The solution is simple: after you download the file, you have to manually rename the file extension to the correct extension, as indicated on the surrounding text for the link you used for the download. In this case, change "unk" to "tgz".

Best regards,
Bruno
songwukong likes this.
wyldckat is offline   Reply With Quote

Old   March 10, 2014, 08:23
Default
  #6
Member
 
sqing
Join Date: Sep 2012
Location: Dalian
Posts: 77
Rep Power: 4
Sunxing is on a distinguished road
Quote:
Originally Posted by alberto View Post
Hello,
it's not included in OpenFOAM. You can download it here:

- For a channel:

http://www.cfd-online.com/OpenFOAM_D...ages/1/40.html

With kind regards,
Alberto
Hi Alberto,

I'm using the perturbU utility to generate a terbulent initial filed for a wall-jet case. However, I don't know how to set the parameters in the perturbUDict, such as duplus, betaPlus, alphaPlus, sigma and epsilon. Is there a rule for setting them?
The following picture is the schematic of the domain for my case.

Best Regards.
sunxing
Attached Images
File Type: jpg schematic of the domain for wall jet case.jpg (12.7 KB, 64 views)
Sunxing is offline   Reply With Quote

Old   April 10, 2014, 10:01
Default
  #7
Senior Member
 
Join Date: Nov 2012
Location: Bavaria
Posts: 144
Rep Power: 4
aylalisa is on a distinguished road
Dear Sunxing,

did you read thesis of Eugene de Villiers:
"The Potential of Large Eddy Simulation for the Modeling of Wall Bounded Flows"
Page. 164 ff. and the the file perturbU.C till line 78.
It does not directly answer your question but could improve understanding.



Best regards,
aylalisa
aylalisa is offline   Reply With Quote

Old   April 10, 2014, 20:22
Default
  #8
Member
 
sqing
Join Date: Sep 2012
Location: Dalian
Posts: 77
Rep Power: 4
Sunxing is on a distinguished road
Quote:
Originally Posted by aylalisa View Post
Dear Sunxing,

did you read thesis of Eugene de Villiers:
"The Potential of Large Eddy Simulation for the Modeling of Wall Bounded Flows"
Page. 164 ff. and the the file perturbU.C till line 78.
It does not directly answer your question but could improve understanding.



Best regards,
aylalisa
Hi aylalisa,

Thanks for your reply.

Regards
Sunxing
Sunxing is offline   Reply With Quote

Old   April 11, 2014, 04:16
Default
  #9
Senior Member
 
Join Date: Nov 2012
Location: Bavaria
Posts: 144
Rep Power: 4
aylalisa is on a distinguished road
Hi Sunxing,

I've found yesterday (after I've replied your thread): http://lists.cfd-online.com/pipermai...ch/019398.html

Aylalisa
aylalisa is offline   Reply With Quote

Old   May 7, 2014, 06:27
Default
  #10
Member
 
Niu
Join Date: Apr 2014
Posts: 42
Rep Power: 3
Z.Q. Niu is on a distinguished road
Hello aylalisa,
I has download purturbU from http://www.cfd-online.com/OpenFOAM_D...ages/1/40.html for channel.I wmake it in my open foam 2.2.0, but it points that "mathematicalConstant" is not declared. Do you wmake perturbU successfuly? would you mind sending me your file of perturbU? My email is silence@tju.edu.cn
Thank you !
Z.Q. Niu is offline   Reply With Quote

Old   May 7, 2014, 14:45
Default
  #11
Member
 
Join Date: Apr 2011
Posts: 36
Rep Power: 6
amanbearpig is on a distinguished road
I do not have version 2.2.0, but I encountered the same issue in 2.2.2. It's due to how pi is defined in different versions of OpenFOAM. Thankfully it is not a difficult fix.

If you edit the .C perturbU file and change any references (I believe there are 2) of 'mathematicalConstant' to 'constant::mathematical', this should rectify the issue.
songwukong likes this.
amanbearpig is offline   Reply With Quote

Old   May 7, 2014, 22:27
Default
  #12
Member
 
Niu
Join Date: Apr 2014
Posts: 42
Rep Power: 3
Z.Q. Niu is on a distinguished road
Thank you, amanbearpig! I have solved it ,the problem is indeed due to mathematicalConstant, I has corrected it successfully!
Z.Q. Niu is offline   Reply With Quote

Old   May 9, 2014, 01:27
Default
  #13
Senior Member
 
adambarfi's Avatar
 
Mostafa Mahmoudi
Join Date: Jan 2012
Posts: 314
Rep Power: 6
adambarfi is on a distinguished road
Send a message via Yahoo to adambarfi Send a message via Skype™ to adambarfi
here you are the modified perturbU utility for OF-2.0.0 to OF-2.3.0:
Attached Files
File Type: gz perturbU.tar.gz (47.9 KB, 90 views)
songwukong, mgg, Artur and 1 others like this.
adambarfi is offline   Reply With Quote

Old   May 27, 2014, 03:50
Default
  #14
Senior Member
 
adambarfi's Avatar
 
Mostafa Mahmoudi
Join Date: Jan 2012
Posts: 314
Rep Power: 6
adambarfi is on a distinguished road
Send a message via Yahoo to adambarfi Send a message via Skype™ to adambarfi
hi everybody,

The perturbU utility was ran for channel395 correctly. I changed the geometry to a perfect channel which the conditions at inlet and outlet patches are cyclic. then I ran the perturbU but it set a zero velocity field for U. I can't understand why it didn't make any perturbation of my velocity field?????

anybody knows what and where is the problem?

the blockMeshDict is as follow:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(
    (0 0 0)
    (1 0 0)
    (1 1 0)
    (0 1 0)
    (0 0 4)
    (1 0 4)
    (1 1 4)
    (0 1 4)

    (2 0 0)
    (2 1 0)
    (2 0 4)
    (2 1 4)

    (1 2 0)
    (0 2 0)
    (1 2 4)
    (0 2 4)

    (2 2 0)
    (2 2 4)
);

blocks
(
    hex (0 1 2 3 4 5 6 7) (25 25 20) simpleGrading (10 10 1)
    hex (1 8 9 2 5 10 11 6) (25 25 20) simpleGrading (0.1 10 1)
    hex (3 2 12 13 7 6 14 15) (25 25 20) simpleGrading (10 0.1 1)
    hex (2 9 16 12 6 11 17 14) (25 25 20) simpleGrading (0.1 0.1 1)

);

edges
(
);

boundary
(
    outlet1_1
    {
        type cyclic;
        neighbourPatch  inlet1_1;
        faces
        (
            (4 7 6 5)
        );
    }
    inlet1_1
    {
        type cyclic;
        neighbourPatch  outlet1_1;
        faces
        (
            (0 3 2 1)
        );
    }


    outlet1_2
    {
        type cyclic;
        neighbourPatch inlet1_2;
        faces
        (
            (5 6 11 10)
        );
    }
    inlet1_2
    {
        type cyclic;
        neighbourPatch  outlet1_2;
        faces
        (
            (1 2 9 8)
        );
    }



    outlet2_1
    {
        type cyclic;
        neighbourPatch  inlet2_1;
        faces
        (
            (7 15 14 6)
        );
    }
    inlet2_1
    {
        type cyclic;
        neighbourPatch  outlet2_1;
        faces
        (
            (3 13 12 2)
        );
    }



    outlet2_2
    {
        type cyclic;
        neighbourPatch  inlet2_2;
        faces
        (
            (6 14 17 11)
        );
    }
    inlet2_2
    {
        type cyclic;
        neighbourPatch  outlet2_2;
        faces
        (
            (2 12 16 9)
        );
    }

    fixedWalls
    {
        type wall;
        faces
        (
            (4 7 3 0)
            (7 15 13 3)
            (10 11 9 8)
            (11 17 16 9)

            (4 0 1 5)
            (5 1 8 10)
            (15 13 12 14)
            (14 12 16 17)
        );
    }
);

mergePatchPairs
(
);

// ************************************************************************* //
and the perturbUDict is as
Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.0                                   |
|   \\  /    A nd           | Web:      http://www.openfoam.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

FoamFile
{
    version         2.0;
    format          ascii;
    instance        "system";

    class           dictionary;
    object          perturbUDict;
}

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


// Expected turbulent Re(tau) Reynolds number with respect to utau
Retau 395;

// Streamwise component of flow. 0=x, 1=y, 2=z
streamwise 2;

// Spanwise component of flow. 0=x, 1=y, 2=z
spanwise 1;

// Halfheight of channel. This is the direction normal to both streamwise and
// spanwise directions.
h 1;

// Set (overwrite) velocity to laminar profile
setBulk true;

// Perturb velocity with some cosine like perturbations
perturb false;

// Perturbation properties
//wall normal circulation as a fraction of Ubar/utau
duplus 0.25;
//spanwise perturbation spacing in wall units
betaPlus 200;
//streamwise perturbation spacing in wall units
alphaPlus 500;
//transverse decay
sigma 0.00055;
//linear perturbation amplitude as a fraction of Ubar
epsilon 0.005;


// ************************************************************************* //
any tip or hint would be appreciated.

Regards,
Mostafa
adambarfi is offline   Reply With Quote

Old   May 27, 2014, 04:51
Default
  #15
Senior Member
 
adambarfi's Avatar
 
Mostafa Mahmoudi
Join Date: Jan 2012
Posts: 314
Rep Power: 6
adambarfi is on a distinguished road
Send a message via Yahoo to adambarfi Send a message via Skype™ to adambarfi
Quote:
Originally Posted by adambarfi View Post
hi everybody,

The perturbU utility was ran for channel395 correctly. I changed the geometry to a perfect channel which the conditions at inlet and outlet patches are cyclic. then I ran the perturbU but it set a zero velocity field for U. I can't understand why it didn't make any perturbation of my velocity field?????

anybody knows what and where is the problem?

the blockMeshDict is as follow:
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(
    (0 0 0)
    (1 0 0)
    (1 1 0)
    (0 1 0)
    (0 0 4)
    (1 0 4)
    (1 1 4)
    (0 1 4)

    (2 0 0)
    (2 1 0)
    (2 0 4)
    (2 1 4)

    (1 2 0)
    (0 2 0)
    (1 2 4)
    (0 2 4)

    (2 2 0)
    (2 2 4)
);

blocks
(
    hex (0 1 2 3 4 5 6 7) (25 25 20) simpleGrading (10 10 1)
    hex (1 8 9 2 5 10 11 6) (25 25 20) simpleGrading (0.1 10 1)
    hex (3 2 12 13 7 6 14 15) (25 25 20) simpleGrading (10 0.1 1)
    hex (2 9 16 12 6 11 17 14) (25 25 20) simpleGrading (0.1 0.1 1)

);

edges
(
);

boundary
(
    outlet1_1
    {
        type cyclic;
        neighbourPatch  inlet1_1;
        faces
        (
            (4 7 6 5)
        );
    }
    inlet1_1
    {
        type cyclic;
        neighbourPatch  outlet1_1;
        faces
        (
            (0 3 2 1)
        );
    }


    outlet1_2
    {
        type cyclic;
        neighbourPatch inlet1_2;
        faces
        (
            (5 6 11 10)
        );
    }
    inlet1_2
    {
        type cyclic;
        neighbourPatch  outlet1_2;
        faces
        (
            (1 2 9 8)
        );
    }



    outlet2_1
    {
        type cyclic;
        neighbourPatch  inlet2_1;
        faces
        (
            (7 15 14 6)
        );
    }
    inlet2_1
    {
        type cyclic;
        neighbourPatch  outlet2_1;
        faces
        (
            (3 13 12 2)
        );
    }



    outlet2_2
    {
        type cyclic;
        neighbourPatch  inlet2_2;
        faces
        (
            (6 14 17 11)
        );
    }
    inlet2_2
    {
        type cyclic;
        neighbourPatch  outlet2_2;
        faces
        (
            (2 12 16 9)
        );
    }

    fixedWalls
    {
        type wall;
        faces
        (
            (4 7 3 0)
            (7 15 13 3)
            (10 11 9 8)
            (11 17 16 9)

            (4 0 1 5)
            (5 1 8 10)
            (15 13 12 14)
            (14 12 16 17)
        );
    }
);

mergePatchPairs
(
);

// ************************************************************************* //
and the perturbUDict is as
Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.0                                   |
|   \\  /    A nd           | Web:      http://www.openfoam.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

FoamFile
{
    version         2.0;
    format          ascii;
    instance        "system";

    class           dictionary;
    object          perturbUDict;
}

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


// Expected turbulent Re(tau) Reynolds number with respect to utau
Retau 395;

// Streamwise component of flow. 0=x, 1=y, 2=z
streamwise 2;

// Spanwise component of flow. 0=x, 1=y, 2=z
spanwise 1;

// Halfheight of channel. This is the direction normal to both streamwise and
// spanwise directions.
h 1;

// Set (overwrite) velocity to laminar profile
setBulk true;

// Perturb velocity with some cosine like perturbations
perturb false;

// Perturbation properties
//wall normal circulation as a fraction of Ubar/utau
duplus 0.25;
//spanwise perturbation spacing in wall units
betaPlus 200;
//streamwise perturbation spacing in wall units
alphaPlus 500;
//transverse decay
sigma 0.00055;
//linear perturbation amplitude as a fraction of Ubar
epsilon 0.005;


// ************************************************************************* //
any tip or hint would be appreciated.

Regards,
Mostafa
solved, I made a mistake and defined the Ubar=(0.1335 0 0) instead of Ubar=(0 0 0.1335).
sorry for that

Regards,
Mostafa
adambarfi is offline   Reply With Quote

Old   March 21, 2015, 14:34
Default
  #16
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,253
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings to all!

I've given a proper wiki page and git repository to perturbU and all of the 3 variants I found that were made by Eugene de Villiers:
May anyone feel free to update that wiki page and fork from that repository!

Best regards,
Bruno
songwukong and rt08 like this.
wyldckat is offline   Reply With Quote

Old   June 1, 2015, 05:54
Default perturbU + precursor inlet
  #17
Member
 
SM
Join Date: Dec 2010
Posts: 57
Rep Power: 6
canopus is on a distinguished road
Hi!
I want to do LES of a diffuser.
For the inlet I want to run a precursor LES of channel for which I set cyclic for inlet and outlet.
Then I run perturbUChannel but the original 0/U file is replaced by some numbers.
Is it OK to run with this condition? How does the solver know about cyclic patches then?
canopus is offline   Reply With Quote

Old   June 1, 2015, 06:49
Default
  #18
Senior Member
 
Join Date: Nov 2012
Location: Bavaria
Posts: 144
Rep Power: 4
aylalisa is on a distinguished road
Hi Canopus,

yes, start simulation with the new field.

You define your patches in constant/polyMesh/blockMeshDict.

Quote:
boundary
(
inlet
{
type cyclic;
neighbourPatch outlet;
matchTolerance 0.01;
faces
(
(0 1 5 4)
);
}
...
)
Ayla
aylalisa is offline   Reply With Quote

Old   June 2, 2015, 07:31
Default
  #19
Member
 
SM
Join Date: Dec 2010
Posts: 57
Rep Power: 6
canopus is on a distinguished road
Thanks for your reply.
I found that the numbers are the initial field and the boundary conditions of 0/U still exist and can be found in the bottom of the file.
canopus is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
PerturbU nzy102 OpenFOAM Running, Solving & CFD 0 April 23, 2007 20:06


All times are GMT -4. The time now is 20:55.