CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Turbulent kinetic Intensity greater than 100%

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

Like Tree1Likes
  • 1 Post By Bane

Reply
 
LinkBack Thread Tools Display Modes
Old   November 6, 2012, 11:47
Default Turbulent kinetic Intensity greater than 100%
  #1
New Member
 
Join Date: Nov 2012
Posts: 3
Rep Power: 4
FlorianM is on a distinguished road
Hello,

I am modelizing a gas flow through a Laval nozzle. (the flow become supersonic) with a 2D axisymmetric model. I started the simulation with a laminar flow to ease convergence. Then I want include Turbulence in my model.

I read enough the FLUENT documentation and my former turbulence courses to understand the main ideas of the different models available. The RMS model being quite unstable, I decide, in order to complete my converged-laminar-solution, to set up a k-e model with enhanced wall function ( my mesh is not wall-resolved). My max Reynolds number being ~50 000 and considering the hydraulic diameter, I set a Intensity of 5% at inlet and outlet.

The solution converged quite well, with physically coherent results, and the flow pattern is not deeply changed from the laminar solution. But by plotting the Turbulent intensity, it appears that my TI is ~1e6 on almost all the nozzle domain ! The TI should be between 0% to 100% or maybe I misunderstood something very important, how is it possible ? I wonder wether the supersonic flow can make the turbulence model incorrect ?

Thank you

Florian
FlorianM is offline   Reply With Quote

Old   November 6, 2012, 12:27
Default
  #2
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
This indicates that your solution is not fully converged if every thing else is OK.
Far is offline   Reply With Quote

Old   November 6, 2012, 12:56
Default
  #3
New Member
 
Join Date: Nov 2012
Posts: 3
Rep Power: 4
FlorianM is on a distinguished road
Thanks, but the residuals of the Turbulence parameters (k and epsilon) converge as well, reached 10-5, just as the other residuals. And my intuition is that a 10000% of turbulent intensity should totally deteriorate the flow pattern and the flow should appear as a big mess, am I wrong ?

Florian
FlorianM is offline   Reply With Quote

Old   November 6, 2012, 15:07
Default
  #4
Member
 
vicarious's Avatar
 
Pedram Mojtabavi
Join Date: Apr 2011
Location: Iran
Posts: 66
Rep Power: 6
vicarious is on a distinguished road
Send a message via Yahoo to vicarious
With a Re number that you mentioned, the whole inside of domain is naturally a mess and turbulent intensity gets very high. I do not suppose that it's wrong since your parameters converged.

Best regards.
vicarious is offline   Reply With Quote

Old   November 6, 2012, 15:16
Default
  #5
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
can a turbulent intensity goes beyond 100%? What does this physically mean?
Far is offline   Reply With Quote

Old   November 7, 2012, 06:47
Default
  #6
New Member
 
Join Date: Nov 2012
Posts: 3
Rep Power: 4
FlorianM is on a distinguished road
The turbulent intensity is defined by Uturb/Uavg : ratio of the turbulent velocity with the mean flow velocity. I read everywhere than TI = 10% is already a quite turbulent flow, but of course, nothing mathematically prevent Uturb (named u' in ANSYS help if I remember well) to be bigger than Uavg, except maybe if some high order term in (Uturb/Uavg)^(n) are neglicted to derive the averaged Navier Stokes equation and the other turbulent-relevant equations, but I don't think so. Imagine a fast flow going rigth into a wall perpendicular to the flow direction. At the stagnation point, the turbulent flow is way higher than the mean flow, isn't it ?

I would like plot actually separatly Uavg and Uturb, is it possible ?
FlorianM is offline   Reply With Quote

Old   November 7, 2012, 07:49
Default
  #7
Member
 
vicarious's Avatar
 
Pedram Mojtabavi
Join Date: Apr 2011
Location: Iran
Posts: 66
Rep Power: 6
vicarious is on a distinguished road
Send a message via Yahoo to vicarious
[QUOTE=FlorianM;390764]The turbulent intensity is defined by Uturb/Uavg : ratio of the turbulent velocity with the mean flow velocity. I read everywhere than TI = 10% is already a quite turbulent flow, but of course, nothing mathematically prevent Uturb (named u' in ANSYS help if I remember well) to be bigger than Uavg, except maybe if some high order term in (Uturb/Uavg)^(n) are neglicted to derive the averaged Navier Stokes equation and the other turbulent-relevant equations, but I don't think so. Imagine a fast flow going rigth into a wall perpendicular to the flow direction. At the stagnation point, the turbulent flow is way higher than the mean flow, isn't it ?


It is. Extreme fluctuations could result in high jump of u'.
Attached Images
File Type: jpg uuprime.jpg (86.0 KB, 37 views)
vicarious is offline   Reply With Quote

Old   November 7, 2012, 10:37
Default
  #8
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
It is logical and I agree.
Far is offline   Reply With Quote

Old   November 8, 2012, 10:14
Default
  #9
New Member
 
Join Date: Jul 2012
Posts: 3
Rep Power: 5
Bane is on a distinguished road
Hi all,

I had some problems with the turbulence intensity myself. One suggestion that could resolve the affair is that FLUENT is apparently not normalizing the u' on the local mean velocity but on a velocity selected in the "Reference Value" tab.
So, if your inlet velocity is relatively small compared to the maximum velocity found in the domain and you chose inlet section as your reference value, unreasonably huge intensities will appear due to the high fluctuation velocities are not normalized on the high local mean velocity, but on the rather small inlet velocity.
If the flow is looking as expected and the other values are realistic, I would not worry too much.

It is just a postprocessing problem after all...
FlorianM likes this.
Bane is offline   Reply With Quote

Old   November 8, 2012, 10:31
Default
  #10
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,971
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Yes, correct. How to overcome this issue in Fluent?
Far is offline   Reply With Quote

Old   May 8, 2013, 20:43
Default Turbulence Intensity
  #11
New Member
 
Pete
Join Date: Mar 2012
Posts: 11
Rep Power: 5
Tech Neo is on a distinguished road
You can go under Report tab in Fluent 14.5 and select "from inlet" in Compute form. Also, depending on the length scale of the your problem change the value of Length. Run the solution of a few iterations. It will give you reasonable values of Turbulence Intensity.
Tech Neo is offline   Reply With Quote

Old   May 10, 2013, 11:55
Default
  #12
Member
 
david
Join Date: Oct 2012
Posts: 57
Rep Power: 4
davidwilcox is on a distinguished road
I just thought i'd throw some of my thoughts into the mix here. Theoretically, the turbulence intensity is a function of k and U. And if you're getting values over 100%, the results are pretty much rubbish ( as with most CFD results lol). You've mentioned that you have used the k-epsilon turbulence model. This eddy-viscosity turbulence model calculates your dissipation rate thru the eddy viscosity ratio. If you've received some warning during your calculations saying turbulent viscosity ratio limited to 1e-6 or something like that, chances are your k values are wrongly calculated. Not sure if it might help you but just something i would just like to share.
davidwilcox is offline   Reply With Quote

Old   June 2, 2014, 17:26
Post
  #13
Member
 
John M.
Join Date: Jul 2011
Posts: 57
Rep Power: 6
villager is on a distinguished road
Quote:
Originally Posted by Bane View Post
Hi all,
One suggestion that could resolve the affair is that FLUENT is apparently not normalizing the u' on the local mean velocity but on a velocity selected in the "Reference Value" tab.
Quote:
Originally Posted by Far View Post
Yes, correct. How to overcome this issue in Fluent?
Defining custom field function:
Code:
SQRT(2/3*turb-kinetic-energy)/velocity-magnitude
will give you turbulent intensity (fractions).
You may multiply it by 100 to get TI as percentage.
villager is offline   Reply With Quote

Reply

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
question about turbulent kinetic energy junker4236 Main CFD Forum 9 July 27, 2015 14:58
Problem with divergence TDK FLUENT 10 September 8, 2012 01:11
Turbulent intensity swe704 Main CFD Forum 0 November 13, 2009 04:42
setting value of turbulent intensity and turbulent viscosity ratio in wind tunnel nuimlabib Main CFD Forum 0 August 4, 2009 00:05
Turbulent Kinetic Energy Olga FLUENT 2 October 11, 2002 15:05


All times are GMT -4. The time now is 20:04.