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

How to create a case with a karman vortex using openfoam?

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

Like Tree3Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   December 4, 2012, 08:16
Default How to create a case with a karman vortex using openfoam?
  #1
New Member
 
Join Date: Dec 2012
Posts: 1
Rep Power: 0
dualshock is on a distinguished road
Hi guys,

I am a newbie at using openfoam and was recently requested to create a simulation of a flow over a cylinder with karman vortex behind the it and I have no idea how to begin. The geometry of the cylinder is shown below and the length of the no-slip wall on the top and bottom are both 15m. The height of the inlet and outlet are 5m. The inlet velocity of the fluid is 1m/s and the pressure at the outlet is 0 Pa. I would like to know how do I create the above geometry and which solver should I be using (potentialfoam or icofoam?). In addition what is the condition for karman vortex?
Attached Images
File Type: png Picture1.png (1.9 KB, 132 views)
dualshock is offline   Reply With Quote

Old   December 4, 2012, 10:06
Default
  #2
Senior Member
 
immortality's Avatar
 
Ehsan
Join Date: Oct 2012
Location: Iran
Posts: 2,210
Rep Power: 19
immortality is on a distinguished road
hi
top and bottom should be symmetryplane left surface inletoutlet and right zerogradient
if you want slip on cylinder must use potentialfoam and symmetryplane on cylinder.if no-slip use icoFoam and fixedValue on cylinder with value uniform (0 0 0).its easier to make mesh in fluent and enter to openfoam with fluentMeshToFoam in command shell.
if have any question tell me.
immortality is offline   Reply With Quote

Old   January 29, 2013, 00:24
Default Hi !!
  #3
New Member
 
jobito_2012
Join Date: Oct 2012
Location: Chile
Posts: 28
Rep Power: 6
jobito_2012 is on a distinguished road
Quote:
Originally Posted by dualshock View Post
Hi guys,

I am a newbie at using openfoam and was recently requested to create a simulation of a flow over a cylinder with karman vortex behind the it and I have no idea how to begin. The geometry of the cylinder is shown below and the length of the no-slip wall on the top and bottom are both 15m. The height of the inlet and outlet are 5m. The inlet velocity of the fluid is 1m/s and the pressure at the outlet is 0 Pa. I would like to know how do I create the above geometry and which solver should I be using (potentialfoam or icofoam?). In addition what is the condition for karman vortex?

I need to do the same problem, can you send me the file please...I´m learning OpenFoam...thanks!!

my mail is aguilera1623@mail.com
jobito_2012 is offline   Reply With Quote

Old   January 29, 2013, 08:09
Default
  #4
Senior Member
 
Joern Beilke
Join Date: Mar 2009
Location: Dresden
Posts: 203
Rep Power: 12
JBeilke is on a distinguished road
Here is a ready to run example where I used pimpleFoam. It contains a coarse and a fine grid created with GridPro. Have fun.

www.beilke-cfd.de/Karmann_OpenFoam.tar.gz
vaveila_m likes this.
JBeilke is offline   Reply With Quote

Old   January 29, 2013, 11:38
Default Ok! :)
  #5
New Member
 
jobito_2012
Join Date: Oct 2012
Location: Chile
Posts: 28
Rep Power: 6
jobito_2012 is on a distinguished road
Quote:
Originally Posted by JBeilke View Post
Here is a ready to run example where I used pimpleFoam. It contains a coarse and a fine grid created with GridPro. Have fun.

www.beilke-cfd.de/Karmann_OpenFoam.tar.gz

Ok!! thanks a lot...I will review the files
jobito_2012 is offline   Reply With Quote

Old   May 2, 2014, 08:17
Default
  #6
Member
 
Avdeev Evgeniy
Join Date: Jan 2011
Location: Togliatty, Russia
Posts: 61
Blog Entries: 1
Rep Power: 14
j-avdeev will become famous soon enough
Send a message via Skype™ to j-avdeev
It works!
Thanks, JBeilke.
http://youtu.be/hZm7lc4sC2o
j-avdeev is offline   Reply With Quote

Old   May 2, 2014, 08:29
Default
  #7
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,978
Blog Entries: 39
Rep Power: 108
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
FYI: I've moved this thread to the OpenFOAM forum, as it was wrongly placed at the Main CFD forum.
vaveila_m likes this.
wyldckat is offline   Reply With Quote

Old   March 17, 2015, 05:22
Default How to make it work
  #8
New Member
 
Jeremy
Join Date: Oct 2014
Posts: 6
Rep Power: 4
jemz is on a distinguished road
Quote:
Originally Posted by j-avdeev View Post
It works!
Thanks, JBeilke.
http://youtu.be/hZm7lc4sC2o
Hi j-avdeev,

I am trying to make the tar.gz file that JBeilke uploaded. I did the following commands:
tar -zxvf Karmann_OpenFoam.tar.gz
cd karmann_gridpro_pimple
pimpleFoam

I also tried simpleFoam command but it didnt work. =(

Here is the error code:

--> FOAM FATAL IO ERROR:
keyword laplacian(rAUf,p) is undefined in dictionary "/home/JeremyVM/OpenFOAM/JeremyVM-2.3.1/run/karmann_gridpro_pimple/system/fvSchemes.laplacianSchemes"


file: /home/JeremyVM/OpenFOAM/JeremyVM-2.3.1/run/karmann_gridpro_pimple/system/fvSchemes.laplacianSchemes from line 44 to line 50.


From function dictionary::lookupEntry(const word&, bool, bool) const
in file db/dictionary/dictionary.C at line 437.


FOAM exiting

Is it more complicated than this? Please help. I really new to OpenFoam and I need to run some tests that is computationally and process intensive. This is a really good example but I can't get it to work.

Please Advise.

Jeremy
jemz is offline   Reply With Quote

Old   March 17, 2015, 06:49
Default
  #9
Member
 
Avdeev Evgeniy
Join Date: Jan 2011
Location: Togliatty, Russia
Posts: 61
Blog Entries: 1
Rep Power: 14
j-avdeev will become famous soon enough
Send a message via Skype™ to j-avdeev
Quote:
Originally Posted by jemz View Post
Here is the error code:

--> FOAM FATAL IO ERROR:
keyword laplacian(rAUf,p) is undefined in dictionary "/home/JeremyVM/OpenFOAM/JeremyVM-2.3.1/run/karmann_gridpro_pimple/system/fvSchemes.laplacianSchemes"
It says that "keyword laplacian(rAUf,p) is undefined" and if you open system/fvSchemes you will not find it.
It is happen because case was made and worked on older OpenFOAM version - I see you use the newest 2.3.1. And OpenFOAM developers have changed some variables-fields names (I hope they had reasons, becaue it happens frequently, almost every release ).

So. I think if you add

Code:
laplacian(rAUf,p) Gauss linear corrected;
instead of

Code:
laplacian((1|A(U)),p) Gauss linear corrected;
to file system/fvSchemes it will start work fine.
j-avdeev is offline   Reply With Quote

Old   March 17, 2015, 08:07
Default
  #10
New Member
 
Jeremy
Join Date: Oct 2014
Posts: 6
Rep Power: 4
jemz is on a distinguished road
Quote:
Originally Posted by j-avdeev View Post
It says that "keyword laplacian(rAUf,p) is undefined" and if you open system/fvSchemes you will not find it.
It is happen because case was made and worked on older OpenFOAM version - I see you use the newest 2.3.1. And OpenFOAM developers have changed some variables-fields names (I hope they had reasons, becaue it happens frequently, almost every release ).

So. I think if you add

Code:
laplacian(rAUf,p) Gauss linear corrected;
instead of

Code:
laplacian((1|A(U)),p) Gauss linear corrected;
to file system/fvSchemes it will start work fine.
Thank you for your help!

Sorry I misunderstood. I got what you mean. Its working now. Thanks!

Last edited by jemz; March 17, 2015 at 15:31.
jemz is offline   Reply With Quote

Old   March 17, 2015, 15:05
Default
  #11
Member
 
Avdeev Evgeniy
Join Date: Jan 2011
Location: Togliatty, Russia
Posts: 61
Blog Entries: 1
Rep Power: 14
j-avdeev will become famous soon enough
Send a message via Skype™ to j-avdeev
Hi, jemz
I have tryed and it works in OpenFOAM 2.3.1 with following system/fvSchemes:

Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         Euler;
}

gradSchemes
{
    default         Gauss linear;
    grad(p)         Gauss linear;
    grad(U)         Gauss linear;
}

divSchemes
{
    default         none;
    div(phi,U)      Gauss limitedLinearV 1;
    div(phi,k)      Gauss limitedLinear 1;
    div(phi,epsilon) Gauss limitedLinear 1;
    div(phi,R)      Gauss limitedLinear 1;
    div(R)          Gauss linear;
    div(phi,nuTilda) Gauss limitedLinear 1;
    div((nuEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         none;
    laplacian(nuEff,U) Gauss linear corrected;
//     laplacian((1|A(U)),p) Gauss linear corrected;
    laplacian(rAUf,p) Gauss linear corrected;
    laplacian(DkEff,k) Gauss linear corrected;
    laplacian(DepsilonEff,epsilon) Gauss linear corrected;
    laplacian(DREff,R) Gauss linear corrected;
    laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
    interpolate(U)  linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p               ;
}
jemz likes this.
j-avdeev is offline   Reply With Quote

Old   August 24, 2015, 17:53
Default piso/pimple vs. ico?
  #12
New Member
 
Paul W. Fontana
Join Date: Jul 2013
Posts: 5
Rep Power: 6
pfontana is on a distinguished road
I've seen examples using pisoFoam, and now pimpleFoam. What's the advantage over using icoFoam? In any solver, is it necessary to generate an initial fluctuation to stimulate the instability?
pfontana is offline   Reply With Quote

Old   August 26, 2015, 18:17
Default
  #13
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,978
Blog Entries: 39
Rep Power: 108
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Quote:
Originally Posted by pfontana View Post
I've seen examples using pisoFoam, and now pimpleFoam. What's the advantage over using icoFoam?
Quick answer: http://www.cfd-online.com/Forums/ope...s-icofoam.html

Quote:
Originally Posted by pfontana View Post
In any solver, is it necessary to generate an initial fluctuation to stimulate the instability?
Depends on what you want to do?!
wyldckat is offline   Reply With Quote

Old   August 26, 2015, 18:43
Default
  #14
New Member
 
Paul W. Fontana
Join Date: Jul 2013
Posts: 5
Rep Power: 6
pfontana is on a distinguished road
@wyldckat Thanks. I'm aware of the differences in principle. I was wondering about application to this particular case. Since pisoFoam with turbulence set to "laminar" is the same as icoFoam, is there some reason not to simulate vortex shedding with icoFoam?

Some time ago I was working on a DNS of vortex shedding from a CFD text/workbook, not in openFoam. Because a symmetrical flow is a solution, it was necessary to give the flow a kick in the form of a small random perturbation in order to cause the vortex shedding instability to be excited. I was wondering if people do that in their openFoam simulations of vortex shedding, or if not, why it's not necessary? Is numerical error enough to seed the instability? (I thought maybe that was what people used pisoFoam for - to include some small initial turbulence to get the shedding going.)
pfontana is offline   Reply With Quote

Old   August 30, 2015, 16:56
Default
  #15
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,978
Blog Entries: 39
Rep Power: 108
wyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of lightwyldckat is a glorious beacon of light
Quick answers: I was hoping someone else on this thread would answer, but since not, here's what I know:
  • http://openfoamwiki.net/index.php/Contrib/perturbU - this utility for initializing the flow field with perturbed flow is more commonly used for LES simulations.
  • icoFoam is sort-of considered an "example solver": http://www.openfoam.org/mantisbt/view.php?id=791#c2023 - you can still use it, but keep in mind what it is...
  • Not requiring initialization with icoFoam in symmetric cases might have to do with the meshes rarely being numerically perfect symmetric meshes. In other words: even if it seems perfect, it's probably not and it will reveal itself sooner or later if not perfect.
wyldckat is offline   Reply With Quote

Old   December 23, 2016, 06:47
Default Case Request
  #16
New Member
 
Kevin
Join Date: Mar 2012
Posts: 10
Rep Power: 7
kevinlipps is on a distinguished road
Hello,

is it possible that the files with a tutorial case on karman vortex street may be uploaded once again?

I don't really know how to setup the problem but I would like to learn from an example, maybe in icoFoam and pimpleFoam for comparision turbulent vs. laminar solver??

Thx in advance
Kevin
kevinlipps is offline   Reply With Quote

Old   December 23, 2016, 08:19
Default
  #17
Member
 
Avdeev Evgeniy
Join Date: Jan 2011
Location: Togliatty, Russia
Posts: 61
Blog Entries: 1
Rep Power: 14
j-avdeev will become famous soon enough
Send a message via Skype™ to j-avdeev
Quote:
Originally Posted by kevinlipps View Post
Hello,

is it possible that the files with a tutorial case on karman vortex street may be uploaded once again?

I don't really know how to setup the problem but I would like to learn from an example, maybe in icoFoam and pimpleFoam for comparision turbulent vs. laminar solver??

Thx in advance
Kevin

JBeilke link server looks unstable.

You can try download same case from my git:
https://github.com/j-avdeev/KarmanPimple
j-avdeev is offline   Reply With Quote

Old   December 24, 2016, 05:32
Default
  #18
New Member
 
Kevin
Join Date: Mar 2012
Posts: 10
Rep Power: 7
kevinlipps is on a distinguished road
Hi there, thanks!

But it doesnt seem to run on my system... what do I need? I only have OpenFOAM 4.1 installed, do I need anymore software to be able to run your programm? I guess I must execute the Allrun script? But nothing really happens when I do that...

One more question, how do I reset paraView? It seems like I messed up the standard layout and now I dont know how to get the left side part of the programm window back.

Merry X-Mas, btw.
kevinlipps is offline   Reply With Quote

Old   December 24, 2016, 06:20
Default
  #19
Senior Member
 
Join Date: Jun 2012
Location: Germany, Bochum
Posts: 129
Rep Power: 8
Bazinga is on a distinguished road
The tutorial can only be used for older version of OpenFOAM. You would need to adjust some files according to the new file structure. Check a similar tutorial of the solver and readjust the entries in the files.
Bazinga is offline   Reply With Quote

Old   December 24, 2016, 06:30
Default
  #20
Member
 
Avdeev Evgeniy
Join Date: Jan 2011
Location: Togliatty, Russia
Posts: 61
Blog Entries: 1
Rep Power: 14
j-avdeev will become famous soon enough
Send a message via Skype™ to j-avdeev
Quote:
Originally Posted by kevinlipps View Post
Hi there, thanks!

But it doesnt seem to run on my system... what do I need? I only have OpenFOAM 4.1 installed, do I need anymore software to be able to run your programm? I guess I must execute the Allrun script? But nothing really happens when I do that...
Yes, you have to just execute Allrun.
This cas works on OpenFOAM 2.1.x. So you probably can get some errors during OpenFOAM 4.1, but usually it is easy to correct, because error output usually detailed enough.
If you have no output after Allrun ececution - have you run OpenFOAM environment setting script before it?

Code:
$ of41
Also you can open Allrun file in text editor and run it line by line. It will something like:

Code:
decomposePar
mpirun -np 3 simpleFoam -parallel
reconstructPar
Quote:
Originally Posted by kevinlipps View Post
One more question, how do I reset paraView? It seems like I messed up the standard layout and now I dont know how to get the left side part of the programm window back.

Merry X-Mas, btw.
It seems like you closed your Papeline Browser, Properties and Information tabs - you can turn on them back under View top menu.
Thank you, happy foam-holidays you too
j-avdeev 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
How to Create .msh file so that when converted to OpenFOAM will have some BC jaypatel OpenFOAM 12 December 5, 2016 12:29
[GAMBIT] How to plot S pipe mariam.sara ANSYS Meshing & Geometry 36 November 7, 2013 16:22
karman vortex street help please SSeth STAR-CCM+ 7 January 10, 2011 12:31
Free surface boudary conditions with SOLA-VOF Fan Main CFD Forum 10 September 9, 2006 12:24
Kármán vortex street in cavitating flow behind bodies in the cavitation tunnel L. Könözsy Main CFD Forum 0 April 17, 2000 13:16


All times are GMT -4. The time now is 07:32.