CFD Online URL
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Karman vortex street

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 8, 2005, 10:11
Default Hi all, I want to simulate
  #1
gellert
Guest
 
Posts: n/a
Hi all,

I want to simulate the flow around a cylinder and the Karman vortex street appearing
behind. Would icoFoam be the right solver? Or is it better/easier to use an LES solver
like oodles?
(Geometry should be a channel with inlet/outlet, rigid walls on top and bottom and
empty b.c. left and right.)

Thank you.
Marcus
  Reply With Quote

Old   June 8, 2005, 10:23
Default This is a difficult problem be
  #2
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 11
eugene is on a distinguished road
This is a difficult problem because you have laminar and turbulent flow. Your best (and probably only) bet would be LES with a dynamic SGS model to cope with transition. I have never used Foam's dynamic models though, so I cant help you with this aspect.
eugene is offline   Reply With Quote

Old   June 8, 2005, 10:27
Default What Reynolds number do you wa
  #3
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 12
henry is on a distinguished road
What Reynolds number do you want to run at?
henry is offline   Reply With Quote

Old   June 8, 2005, 11:25
Default I choose the inflow as parabol
  #4
gellert
Guest
 
Posts: n/a
I choose the inflow as parabolic profile. The Reynolds number will be around Re=200.
Meanwhile I already tested icoFoam and get a steady state without detaching
vortices nearly independent on the used resolution.
On the other hand the needed resolution is not that high, so a direct simulation should
be possible!?
  Reply With Quote

Old   June 8, 2005, 11:36
Default At Re=200 you do not need LES
  #5
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 12
henry is on a distinguished road
At Re=200 you do not need LES and running in 2D is probably OK but you might want to check if you are likely to get 3D structures at this Re.

If your mesh and initial conditions are symmetric you may get a symmetric stready solution unless you perturb it to break the symmetry. Also you should use use second-order differencing in time and space. What schemes have you chosen?
henry is offline   Reply With Quote

Old   June 8, 2005, 12:56
Default The center of the cylinder is
  #6
gellert
Guest
 
Posts: n/a
The center of the cylinder is not exactly placed on the symmetry axis of the channel and inflow.
The chosen schemes are CrankNicholson for time derivatives and (Gauss) upwind for spatial
derivatives. As already mentioned the solution looks symmetric and steady.
  Reply With Quote

Old   June 8, 2005, 13:01
Default I am not surprised you get a s
  #7
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 12
henry is on a distinguished road
I am not surprised you get a symmetric and steady solution using upwind spatial differencing, why did you choose such a low-order scheme? Why not use linear (central-differencing)?
henry is offline   Reply With Quote

Old   June 8, 2005, 17:48
Default Ok, I changed to (Gauss) linea
  #8
gellert
Guest
 
Posts: n/a
Ok, I changed to (Gauss) linear scheme as found in the cavity test case. Nevertheless only a steady-state is reached.
I prepared a short web page with some pictures, the case files and some calculation data. If somebody wants to take
a look and suggest some further improvements, I would be happy.

The URL is http://www-user.tu-cottbus.de/~gelle...an/karman.html

-marcus
  Reply With Quote

Old   June 8, 2005, 18:01
Default What happened when you perturb
  #9
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 12
henry is on a distinguished road
What happened when you perturbed the solution to break symmetry?
henry is offline   Reply With Quote

Old   June 8, 2005, 18:16
Default You need to trigger the instab
  #10
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,748
Rep Power: 20
hjasak will become famous soon enough
You need to trigger the instability and then all will be well.

Try this: use the current solution and make the top and bottom of the channel to be fixedVelocity boundaries (not sure what you're using now), but specify different velocities at top and bottom. Then, run the simulation for a hundred time-steps or so - this will create a non-symmetric solution. Using that, restart with the proper boundary conditions and the cylinder will start shedding.

If this sounds too complex to you :-) and you're brave, try relaxing the pressure tolerance, run a few time-steps (checking the solution visually). The run will be slowly blowing up. When you get some assymetry (but before the whole thing has blown to bits!), tighten the tolerances again and you'll get the shedding.

This is a fun problem - enjoy!

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   June 8, 2005, 18:43
Default Increase the Reynolds number (
  #11
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 11
eugene is on a distinguished road
Increase the Reynolds number (by lowering nu) until the case starts to shed, then change it back to normal.
eugene is offline   Reply With Quote

Old   June 8, 2005, 20:26
Default Your mesh is not 2D, it's 2 ce
  #12
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 12
henry is on a distinguished road
Your mesh is not 2D, it's 2 cells thick with empty patches on the front and back which allows nearly all the flow to "leak out" through those boundaries rendering the simulation totally incorrect. Apart from this gross error in the mesh it is also highly distorted and could be greatly improved in structure. It is also rather coarse in the wake-region.

I don't think the use of forth-order differencing is a good idea for this case and linear should be fine particularly on such a non-orthogonal mesh. Try running check mesh on it and you will see what I mean.
henry is offline   Reply With Quote

Old   June 9, 2005, 06:45
Default Thank you for all your help. I
  #13
gellert
Guest
 
Posts: n/a
Thank you for all your help. I will first reduce the 3rd direction to one cell thickness and
try to perturb the initial conditions. If it's not 'enough' next step will be improving
the mesh (for me that is most time consuming).
  Reply With Quote

Old   June 9, 2005, 06:53
Default Given that your geometry is qu
  #14
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 12
henry is on a distinguished road
Given that your geometry is quite assymetric you probably won't need to perturb the initial conditions. However, I would strongly recommend you improve and refine the mesh particularly in the wake region. Take a look at the mesh structure used in the plateHole stressedFoam tutorial for guidance.
henry is offline   Reply With Quote

Old   June 17, 2005, 13:18
Default After some optimisations now t
  #15
gellert
Guest
 
Posts: n/a
After some optimisations now the vortex shedding appears (albeit at slightly higher Re as expected).

I updated the above mentioned web page. The complete case file is also there - perhaps usable as
additinal icoFoam tutorial case?

-marcus
  Reply With Quote

Old   June 17, 2005, 13:19
Default After some optimisations now t
  #16
gellert
Guest
 
Posts: n/a
After some optimisations now the vortex shedding appears (albeit at slightly higher Re as expected).

I updated the above mentioned web page. The complete case file is also there - perhaps usable as
additional icoFoam tutorial case?

-marcus
  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
low Re (30-170) Karman vortex street Sponi FLUENT 0 March 16, 2007 15:27
Von karman Vortex street yoshi Main CFD Forum 6 September 10, 2005 23:09
karman vortex street michael CD-adapco 5 April 30, 2003 06:04
Karman vortex street Zhipeng FLUENT 5 June 24, 2002 12:00
Karman vortex street Achilleas Tsompanos Main CFD Forum 4 April 25, 2000 08:26


All times are GMT -4. The time now is 13:19.