CFD Online Logo CFD Online URL
Home > Forums > CFX

Vortex shedding?

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

LinkBack Thread Tools Display Modes
Old   April 25, 2008, 23:05
Default Vortex shedding?
Posts: n/a

My project is to investigate the effects of confining walls on the vortex shedding of a heated square cylinder in uniform cross-flow.

This is my first time using CFD and i have done some tutorials, created a mesh etc and got soms results.

trouble is i cant see any vortex shedding what so ever, it looks like laminar flow over the square (yes it detaches but no shedding in the wake after reattaching). I have run both transient and steady state problems. and the domain is alot larger than the cylinder at present to simulate just an open cross flow situation and i still get no shedding in the wake.

I am plotting velocity contours to view the vortices? is this correct? the mesh is also quite fine.

Any help appreciated , thanks
  Reply With Quote

Old   April 27, 2008, 14:06
Default Re: Vortex shedding?
Posts: n/a
What conditions are you modelling? What velocities, cylinder size and turbulence model?

1) For turbulent flow, you need a fine mesh, very fine near the cylinder wall with y+ ~ 1 to capture vortex shedding well. You probably want to use the SST turbulence model, not k-epsilon.

2) Look up the Strouhal number (wikipedia has a page - but you should find it in good textbooks), and estimate the shedding frequency for your system. You need a transient simulation to see vortex shedding (you should start from a steady state solution, so that the velocity field away from the cylinder is good, but a steady-state solution will not itself show vortex shedding!). The timestep should be a small fraction of the shedding period (1/frequency) predicted by the Strouhal number. I am not an expert at this, but I got quite good results recently using 1/50 of the period. You will need to check your results are independent of the timestep selected.

3) Plotting velocity vectors and pressure contours will show the vorticies, but once you have them you can select the best plots yourself. Place monitor points behind the cylinder so you can see vortices forming from the solver manager.

4) Search the archives of this forum - lots of other people have asked about this in the past and the answers they received should help you.

Good luck - it can be done, and I'm sure you'll get there. I hope others will also give you advice.

  Reply With Quote

Old   April 27, 2008, 15:43
Default Re: Vortex shedding?
Posts: n/a
Thanks for the reply andy,

I believe the problem may lie in the mesh...As i have no clues as to what you mean by y+ , i vaguely remember it in the cfx tutorials but ill sit down and have a better look at it today.

Can incorrect meshing around the cylinder cause the vortex capture to be incorrect like i have? I did add an inflated boundary layer around the cylinder and the wake is also fine where i believe shedding should be.

Lastly , my cylinder is 19mm side length (square) flow rate 3.2m/s and i have been using SST.

Thanks again,ill brows the archives later on today.
  Reply With Quote

Old   April 27, 2008, 18:08
Default Re: Vortex shedding?
Posts: n/a
"Can incorrect meshing around the cylinder cause the vortex capture to be incorrect like i have?"

Yes - it certainly can cause such problems. But I don't know the details of your mesh, so I cannot say for sure if this is the case for you.

Learning about y+ (yplus) is a very important part of learning about CFD. It is a fundemental part of understanding how to simulate all turbulent flows correctly, and you really do need to study it ASAP! The CFX help system discusses this. Look up the section on modelling flows near walls in the help system...

Basically, the thickness of turblent boundary layers and the laminar sub-layers at a wall boundary varies from one flow to another, but by calculating a non-dimensional value known as y+ you can work out whether your first mesh node sits in the laminar layer, or the turbulent layer, or the main flow. To simulate a phenomenom such as vortex shedding, where the boundary layer behaviour is crucial, you need to have mesh nodes in the laminar sublayer near the wall. That normally needs a very fine mesh near the wall.

1) Go into CFX Post and plot contours of yplus on the boundary of the square. If it is much above 1 you need to refine your mesh.

2) For a square, the Strouhal number is about S=0.11 over a wide range of Reynolds numbers. So for a square of d=0.019 [m] and a flow of U=3.2 [m s^-1], the shedding frequency is expected to be:

f = S * U / d = 0.11 * 3.2 [m/s] / 0.019 [m] = 18.5 Hz

=> Period of vortex shedding = 1/f ~ 0.05 [s]

So you need a timestep which is about a 1/50 of 0.05 [s]. I.e. you need a timestep of about 0.001 [s] to resolve vortex shedding. Is your timestep this small?

Good luck. Andy.
  Reply With Quote

Old   April 27, 2008, 19:57
Default Re: Vortex shedding?
Glenn Horrocks
Posts: n/a

You have not stated the Re number you are running at. That will determine whether there is vortex shedding at all, and whether it is laminar or turbulent.

Also, the most important thing in simulations like this is to use high order differencing. You will need a second order spacial scheme (like hybrid differencing with the blend factor set to 1.0 or close to it) and a second order temporal scheme.

Glenn Horrocks
  Reply With Quote


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
K-Epsilon for Vortex Shedding Sham FLUENT 31 September 18, 2015 16:04
Transiet Animation - vortex shedding derz CFX 5 May 10, 2010 09:21
Vortex shedding, FSI-analysis, turbulence numerics tallknuseren CFX 3 May 10, 2010 04:31
Vortex shedding behind cylider in cross flow Muthu FLUENT 0 March 6, 2006 11:29
basic vortex shedding john Main CFD Forum 4 November 6, 2000 14:23

All times are GMT -4. The time now is 16:33.