CFD Online Logo CFD Online URL
Home > Forums > CFX

Question Regarding Turbulence Numerics

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

LinkBack Thread Tools Display Modes
Old   November 2, 2010, 12:24
Default Question Regarding Turbulence Numerics
New Member
Join Date: Mar 2010
Posts: 20
Rep Power: 7
cfdengineer is on a distinguished road
Hello, after being a Fluent user for the past 10 years I have made the jump to use CFX for the past 6 months since this is the software the company I now work for uses. I have found that all CFD models that are run here use only 1st order turbulence numerics. I was told that version 10 did not have a high resolution option and basically they haven't tried the high resolution and felt that the results would not change much if high resolution was used. We now use version 12. The CFD work we deal with the most is turbine blades. So, we do have a highly turbulent swirling flow. We use the SST option with automatic wall functions. My argument is that since most of the meshes are tets with prism layer that using high resolution is paramount to achieve a better accurate solution over 1st order turbulence. Unless, bear in mind convergence issues. I am having a very difficult time convincing senior and management engineers here to go forth and use high resolution. Any ideas? Also, are there any studies out there comparing CFX's 1st order and high resolution turbulence numerics and also if there are any CFX vs. Fluent turbulence comparisons? Thanks
cfdengineer is offline   Reply With Quote

Old   November 2, 2010, 16:46
Senior Member
Join Date: Apr 2009
Posts: 529
Rep Power: 12
stumpy is on a distinguished road
I haven't ran many cases using high resolution turbulence, but those I have ran have shown little difference. Turbulence is a fairly diffusive process, so I can see that it's often not necessary to resolve sharp gradients. Also switching to high resolution may be insignificant considering some of the other approximations made in two-equation turbulence models. Still, I'd be interested to see any good comparisons.
stumpy is offline   Reply With Quote

Old   November 2, 2010, 17:42
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,298
Rep Power: 88
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I would have thought the way forward is obvious - run a test case with and without high order turbulence numerics and see if accuracy improves. That should make the case as to whether it is worth the effort better than any theoretical arguement.

Try asking CFX support for some papers looking at the high order numerics.
ghorrocks is offline   Reply With Quote

Old   November 2, 2010, 18:00
jola's Avatar
Jonas Larsson
Join Date: Jan 2009
Location: Gothenburg, Sweden
Posts: 224
Rep Power: 10
jola is on a distinguished road
Send a message via MSN to jola Send a message via Skype™ to jola
It isn't that critical to use a very high-order scheme for the turbulent variables. These variables are very source term dominated and the accuracy of the convection scheme isn't very important. It is more important that the scheme behaves well and never creates unphysical oscillations that can trigger turbulence problems.

Many years ago I did a study comparing results for turbine blades using 1st and 2nd order schemes in Fluent. This was on structured hex meshes though. The study showed that most of the time it was okay to use first order schemes for k and epsilon. It might be more important on coarses tet meshes though, I do not know since I rarely use tets on blading simulations.

For the non-turbulence variables having something better than first-order upwind is critical though, but I assume that you are well aware of that.

If you are working on turbines and are worried about turbulence. Have you ever looked at, for example, eddy-viscosity ratios in the region just outside of the suction side after the suction peak and further down-stream between the wakes? Most two-equation models have a tendency to produce completely unphysical eddy-viscosity ratios there, especially if you run with fairly large (and realistic) inlet length-scales. That is something to show to your scepetic seniors/management if they think they know everything about turbulence modeling
jola is offline   Reply With Quote

Old   April 20, 2014, 13:21
Default Querry regarding Turbulence numeric
New Member
Join Date: Jan 2014
Posts: 14
Rep Power: 3
manpreet is on a distinguished road
Hello everyone,

I need help. I would like to know about turbulence numeric term. What is its physical significance. In my project, When I use first order it show me smooth graph of K and epsilon in CFX solver. On the other hand, using hogh resolution leads to lot of variation in graph. Why it has happened.
Kindly consider my request.
Manpreet Singh
manpreet is offline   Reply With Quote

Old   April 20, 2014, 23:38
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,298
Rep Power: 88
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
High order differencing is resolving lots of smaller scale detail which the low order scheme damps out.
ghorrocks is offline   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
Turbulence dampening due to magnetic field in LES and RAS eelcovv OpenFOAM 0 June 8, 2010 11:35
RSM shortcoming in onset of Turbulence Hatef Main CFD Forum 0 October 23, 2007 08:12
turbulence model and sol init_best practice sam Main CFD Forum 0 October 18, 2006 01:10
Question...Turbulence Intensity & Viscosity ratio Jay FLUENT 1 October 6, 2005 04:41
Turbulence boundary values lego CFX 9 October 25, 2002 11:55

All times are GMT -4. The time now is 22:34.