
[Sponsors] 
May 6, 2013, 07:22 
Flow around a cylinder with kepsilon model

#1 
New Member
Join Date: May 2013
Posts: 4
Rep Power: 6 
Hello,
I'm trying to simulate a simple flow around the cylinder using CFX. The Reynolds number is 2000, and I use the kepsilon model as turbulence model. the temperature difference between the cylinder wall and the fluid is 1K. the simulation is running and it also converges but there is no karman vortex Street in this case. But when I simulate the same problem as laminar, then I can see this swirl. the following fotos shows the most important settings for this problem. regards 

May 6, 2013, 07:46 

#2 
Senior Member
Lance
Join Date: Mar 2009
Posts: 606
Rep Power: 14 
Re = 2000 and using turbulence model? I would guess that the turbulence model introduce additional dissipation that removes the vortex street. That would explain why you see the vortex street when you are using a laminar approach.
Why are you using gravity? Is buoyancy important in your flow? 

May 6, 2013, 08:29 

#3 
Senior Member
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 314
Rep Power: 7 
You have low Reynolds number flow with questionable turbulence. Also it's flow over a cylinder so I assume you have some sort of vortex shedding. I would'nt use keps if you were to use a turbulence model. Try komega SST, with low turbulence intensity at the boundaries, also try it with and without the gammatheta transitional model switched on. That transitional model is optimized for low external Re flows.
But before doing that I'd question if it's even turbulent. 

May 7, 2013, 03:59 

#4 
New Member
Join Date: May 2013
Posts: 4
Rep Power: 6 
hi,
first of all thanks for your tipps. i have increased the raynolds number to 4000, but still no karman street can be observed (see the attachement). i also tried Komega SST model without considering buoyant effect and obtained the similar results as using Kepsilon model. regards. 

May 7, 2013, 19:41 

#5 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,463
Rep Power: 104 
You need a lowdissipation numerical model to get the vorticies. Are you using a second order space and time discretisation scheme? And time steps small enough (adaptive timestepping is STRONGLY recommended)?


May 8, 2013, 11:58 

#6 
New Member
Irin Sun
Join Date: Jan 2010
Posts: 5
Rep Power: 9 
thank u for your reply.
we used high resolution scheme for this problem. To reduce the additional dissipation caused by turbulence model, now I am going to try CDS for advection scheme, second order backward euler for transient scheme. which scheme will u suggest for turbulence numerics. Should i also use second order since it seems that first order is recommended for turbulence equations. thanks. irinsun 

May 8, 2013, 14:14 

#7 
Senior Member
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 13 
Are you using scalable wlal funcition? How about using automatic wall function, and using Y+ values of  say close to 1 etc? This will capture the phenomena near wall well and will also work if there are laminar/transition flow structures around your cylinder.
I wouldn't consider keps here because of low turbulence and its dissipation. kwSST is a better choice. Also, refining the mesh might help in reducing dissipation. OJ 

May 8, 2013, 16:40 

#8  
Senior Member
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 314
Rep Power: 7 
Quote:


May 8, 2013, 16:57 

#9 
Senior Member
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 13 
I just suggested that omega based model with automatic wall function might fare better than epsilon based model with scalable wall function in this particular case, as he was considering. The use of keps is to be avoided in this case, primarily because of disspation it will introduce, eating up all the transient/turbulent instabilities that give rise to vortices. In cases of higher Re, keps may fare better.
OJ 

May 8, 2013, 22:48 

#10 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,463
Rep Power: 104 
Agreed, SST or kw are the turbulence models to try here.
But second order time stepping is a MUST. You will need this. 

May 9, 2013, 06:36 

#11  
Senior Member
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 314
Rep Power: 7 
Quote:


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Turbulence model for flow over a cylinder at Re=10000  ojha.mayank485  CFX  13  May 19, 2015 02:09 
Flow over 2D Cylinder, Laminar and Turbulent  Tsr63  FLUENT  5  November 13, 2014 13:13 
Water subcooled boiling  Attesz  CFX  7  January 5, 2013 04:32 
Orifice Plate with a fully developed flow  Problems with convergence  jonmec  OpenFOAM Running, Solving & CFD  3  July 28, 2011 05:24 