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

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

December 4, 2012, 08:16
How to create a case with a karman vortex using openfoam?
#1
New Member

Join Date: Dec 2012
Posts: 1
Rep Power: 0
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
 Picture1.png (1.9 KB, 74 views)

 December 4, 2012, 10:06 #2 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,205 Rep Power: 18 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.

January 29, 2013, 00:24
Hi !!
#3
New Member

jobito_2012
Join Date: Oct 2012
Location: Chile
Posts: 28
Rep Power: 5
Quote:
 Originally Posted by dualshock 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

 January 29, 2013, 08:09 #4 Senior Member   Joern Beilke Join Date: Mar 2009 Location: Dresden Posts: 185 Rep Power: 9 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.

January 29, 2013, 11:38
Ok! :)
#5
New Member

jobito_2012
Join Date: Oct 2012
Location: Chile
Posts: 28
Rep Power: 5
Quote:
 Originally Posted by JBeilke 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

 May 2, 2014, 08:17 #6 Member   Avdeev Evgeniy Join Date: Jan 2011 Location: Togliatty, Russia Posts: 52 Blog Entries: 1 Rep Power: 12 It works! Thanks, JBeilke. http://youtu.be/hZm7lc4sC2o

 May 2, 2014, 08:29 #7 Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 8,697 Blog Entries: 34 Rep Power: 88 FYI: I've moved this thread to the OpenFOAM forum, as it was wrongly placed at the Main CFD forum. vaveila_m likes this.

March 17, 2015, 05:22
How to make it work
#8
New Member

Jeremy
Join Date: Oct 2014
Posts: 6
Rep Power: 2
Quote:
 Originally Posted by j-avdeev 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.

Jeremy

March 17, 2015, 06:49
#9
Member

Avdeev Evgeniy
Join Date: Jan 2011
Location: Togliatty, Russia
Posts: 52
Blog Entries: 1
Rep Power: 12
Quote:
 Originally Posted by jemz 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;`

Code:
`laplacian((1|A(U)),p) Gauss linear corrected;`
to file system/fvSchemes it will start work fine.

March 17, 2015, 08:07
#10
New Member

Jeremy
Join Date: Oct 2014
Posts: 6
Rep Power: 2
Quote:
 Originally Posted by j-avdeev 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.

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

Last edited by jemz; March 17, 2015 at 15:31.

 March 17, 2015, 15:05 #11 Member   Avdeev Evgeniy Join Date: Jan 2011 Location: Togliatty, Russia Posts: 52 Blog Entries: 1 Rep Power: 12 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.

 August 24, 2015, 17:53 piso/pimple vs. ico? #12 New Member   Paul W. Fontana Join Date: Jul 2013 Posts: 5 Rep Power: 4 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?

August 26, 2015, 18:17
#13
Super Moderator

Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,697
Blog Entries: 34
Rep Power: 88
Quote:
 Originally Posted by pfontana I've seen examples using pisoFoam, and now pimpleFoam. What's the advantage over using icoFoam?
Quick answer: pimpleFoam vs simpleFoam vs pisoFoam vs icoFoam?

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

 August 26, 2015, 18:43 #14 New Member   Paul W. Fontana Join Date: Jul 2013 Posts: 5 Rep Power: 4 @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.)

 August 30, 2015, 16:56 #15 Super Moderator   Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 8,697 Blog Entries: 34 Rep Power: 88 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.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post [GAMBIT] How to plot S pipe mariam.sara ANSYS Meshing & Geometry 36 November 7, 2013 16:22 jaypatel OpenFOAM 11 June 7, 2012 10:33 SSeth STAR-CCM+ 7 January 10, 2011 12:31 Fan Main CFD Forum 10 September 9, 2006 12:24 L. Könözsy Main CFD Forum 0 April 17, 2000 13:16

All times are GMT -4. The time now is 18:07.