# Flow around a cylinder with k-epsilon model

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

May 6, 2013, 07:22
Flow around a cylinder with k-epsilon model
#1
New Member

Join Date: May 2013
Posts: 4
Rep Power: 5
Hello,
I'm trying to simulate a simple flow around the cylinder using CFX. The Reynolds number is 2000, and I use the k-epsilon 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
Attached Images
 01.png (21.9 KB, 39 views) 04.jpg (28.4 KB, 33 views) 06.jpg (56.2 KB, 53 views) 07.jpg (13.6 KB, 31 views) 08.jpg (25.9 KB, 30 views)

 May 6, 2013, 07:46 #2 Senior Member   Lance Join Date: Mar 2009 Posts: 594 Rep Power: 12 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: 312 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 k-eps if you were to use a turbulence model. Try k-omega SST, with low turbulence intensity at the boundaries, also try it with and without the gamma-theta 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: 5
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 K-omega SST model without considering buoyant effect and obtained the similar results as using K-epsilon model.
regards.
Attached Images
 Velocity_Post.jpg (30.0 KB, 34 views)

 May 7, 2013, 19:41 #5 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 You need a low-dissipation 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: 8 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: 12 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 k-eps here because of low turbulence and its dissipation. kw-SST 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: 312
Rep Power: 7
Quote:
 Originally Posted by oj.bulmer 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 k-eps here because of low turbulence and its dissipation. kw-SST is a better choice. Also, refining the mesh might help in reducing dissipation. OJ
Hi OJ. Surely having a Y+ less than 11 using k-eps is pointless as it will use scalable wall functions.

 May 8, 2013, 16:57 #9 Senior Member   OJ Join Date: Apr 2012 Location: United Kindom Posts: 475 Rep Power: 12 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 k-eps 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, k-eps may fare better. OJ

 May 8, 2013, 22:48 #10 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 Agreed, SST or k-w 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: 312
Rep Power: 7
Quote:
 Originally Posted by oj.bulmer 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 k-eps 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, k-eps may fare better. OJ
Oh absolutely, I do agree. In fact I did recommend the k-omega SST in my earlier post. I just thought you were referring to a Y+ of less than 1 for the k-eps.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post ojha.mayank485 CFX 13 May 19, 2015 02:09 Tsr63 FLUENT 5 November 13, 2014 13:13 Attesz CFX 7 January 5, 2013 04:32 jonmec OpenFOAM Running, Solving & CFD 3 July 28, 2011 05:24

All times are GMT -4. The time now is 15:04.