- **CFX**
(*http://www.cfd-online.com/Forums/cfx/*)

- - **Vortex shedding?
**
(*http://www.cfd-online.com/Forums/cfx/25730-vortex-shedding.html*)

Vortex shedding?
Hello,
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 |

Re: Vortex shedding?
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. andy |

Re: Vortex shedding?
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. |

Re: Vortex shedding?
"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. |

Re: Vortex shedding?
Hi,
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 |

All times are GMT -4. The time now is 02:17. |