# Zero equation turbulence model gives better result??

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 June 16, 2011, 09:52 Zero equation turbulence model gives better result?? #1 Member   Sanyo Join Date: Apr 2009 Location: India Posts: 54 Rep Power: 9 Hello All, I am doing flow simulation of 90 Deg. duct bend. Fluid is air at 500 Deg C. The area of duct upstream is low while that of downstream is quite more. Hence the flow separation is taking place. When I tried with k-e, SST & RSM model, flow is packing towards the outer wall of the bend, resulting in high velocity in that part. Though this is practical, the separation region is over-predicted (Separation region is more in area). Hence the velocity values are also over-predicted (as more quantum of fluid is passing through less area). When I tried with zero equation turbulence model, though separation region is under-predicted; the velocity values are near to ground data (as flow is more distributed). This obviously confused me because as per my knowledge, 2 equation models are more accurate than zero equation model. I can not use zero equation model throughout the domain, as there are some turbulent dominant areas in the domain. Is there any intermediately accurate model between zero equation & SST? I would appreciate all the help I could get. Thanks in advance. Regards, --Sanyo

 June 16, 2011, 19:34 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,831 Rep Power: 100 I like the logic - zero equation is underpredicted, two equation is over predicted so a one equation model should be about right. Unfortunately it does not work that way. Predicting separation lengths is very tricky for turbulence models. I think your best bet would be to use SST and activate some of the advanced features, I think some of these include models to improve separation lengths. I cannot remember the names off hand, hopefully people can recall the options I have in mind. If this does not work then you should consider DES, LES or SAS approaches. pranab_jha, ojha.mayank485 and vsammartano like this.

 June 17, 2011, 08:37 #3 Member   Sanyo Join Date: Apr 2009 Location: India Posts: 54 Rep Power: 9 Hi Glenn, I would like to admit that your replies always help me a lot & would like to thank you for the efforts you take for CFD community. Probably I missed to convey my message clearly. I didnt want to say that zero equation model under predicts & hence its more accurate. I just found that two equation model or even RSM somehow was not able to capture the flow distribution at bend (where flow changes its direction at 90 Deg.) & giving the much different velocity values against ground data. On the other hand zero equation model gave the results much closer to ground data. I just wanted to know, if I was missing something in turbulence modeling. I also came across to the low Re K-e model of Fluent. I didnt find such model in CFX. I also read that K-w could be such model, but I didnt find the results promising. So I was wondering if such model could be implemented in CFX? Do you suggest to use the advance feature of SST such as "streamline curvature correction model"? In that case, how to determine the values of constants? Thank you for your help. Regards, -Sanyo

 June 17, 2011, 08:42 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,831 Rep Power: 100 I would not use any of the unusual turbulence models like low Re k-e or k-w unless you have a good reason to do so. The SST model is the best all-purpose turbulence model in CFX by far so use that one. Additionally the SST model has the extra options of things like curvature correction which the others do not. No need to adjust the constants in the model. Leave them at the defaults. What Re is the duct flowing at? vsammartano likes this.

 June 19, 2011, 05:22 #5 Member   Sanyo Join Date: Apr 2009 Location: India Posts: 54 Rep Power: 9 Hi Glenn, Thanks for the reply. The Re at duct is 9.5e+5. Regards, -Sanyo

 June 19, 2011, 06:41 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,831 Rep Power: 100 OK, mid level turbulence. SST should be as good as anything for this flow regime.

 June 21, 2011, 09:30 #7 Member   Sanyo Join Date: Apr 2009 Location: India Posts: 54 Rep Power: 9 Hi Glenn, Sorry for late reply. Can you suggest what model to be used if Re is around or less than 35000? In my case, for another set of operating conditions, Re is 37000. Thanks in advance. Regards, -Sanyo

 June 21, 2011, 20:08 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,831 Rep Power: 100 SST is the best general purpose turbulence model.

 June 22, 2011, 03:32 #9 Member   Sanyo Join Date: Apr 2009 Location: India Posts: 54 Rep Power: 9 Thanks a lot.

 June 24, 2011, 16:34 #10 New Member   Joseph Tipton Join Date: Jun 2010 Posts: 14 Rep Power: 8 I'm not sure if this will be helpful to your situation or not, but I experienced what sounds like a similar problem with turbulent flow over a backward facing step. The reattachment point didn't correspond to experiment and, upon further inspection, the cross-section flow profiles were "off" as well. The problem turned out to be convergence-related. The default RMS value of 1E-4 was not sufficient for achieving a fully converged solution.

 June 26, 2011, 10:58 #11 Member   Sanyo Join Date: Apr 2009 Location: India Posts: 54 Rep Power: 9 Hi jtipton2, Thank you very much for your reply. I will definitely try to achieve more stringent convergence norm. Regards, -Sanyo

 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 nedved OpenFOAM Running, Solving & CFD 2 November 30, 2014 23:43 Blob Main CFD Forum 0 May 29, 2009 08:35 Beginner Main CFD Forum 1 January 7, 2009 06:36 Biga Main CFD Forum 5 March 22, 2005 21:06 Yi FLUENT 0 October 26, 2001 13:37

All times are GMT -4. The time now is 02:57.

 Contact Us - CFD Online - Top