CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Karman vortex street (http://www.cfd-online.com/Forums/openfoam-solving/60575-karman-vortex-street.html)

gellert June 8, 2005 09:11

Hi all, I want to simulate
 
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

eugene June 8, 2005 09:23

This is a difficult problem be
 
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.

henry June 8, 2005 09:27

What Reynolds number do you wa
 
What Reynolds number do you want to run at?

gellert June 8, 2005 10:25

I choose the inflow as parabol
 
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!?

henry June 8, 2005 10:36

At Re=200 you do not need LES
 
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?

gellert June 8, 2005 11:56

The center of the cylinder is
 
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.

henry June 8, 2005 12:01

I am not surprised you get a s
 
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)?

gellert June 8, 2005 16:48

Ok, I changed to (Gauss) linea
 
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

henry June 8, 2005 17:01

What happened when you perturb
 
What happened when you perturbed the solution to break symmetry?

hjasak June 8, 2005 17:16

You need to trigger the instab
 
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

eugene June 8, 2005 17:43

Increase the Reynolds number (
 
Increase the Reynolds number (by lowering nu) until the case starts to shed, then change it back to normal.

henry June 8, 2005 19:26

Your mesh is not 2D, it's 2 ce
 
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.

gellert June 9, 2005 05:45

Thank you for all your help. I
 
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).

henry June 9, 2005 05:53

Given that your geometry is qu
 
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.

gellert June 17, 2005 12:18

After some optimisations now t
 
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

gellert June 17, 2005 12:19

After some optimisations now t
 
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


All times are GMT -4. The time now is 04:30.