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

Turbulence model for flow over a cylinder at Re=10000

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

Like Tree2Likes
  • 1 Post By ghorrocks
  • 1 Post By hee

Reply
 
LinkBack Thread Tools Display Modes
Old   June 19, 2011, 00:10
Default Turbulence model for flow over a cylinder at Re=10000
  #1
New Member
 
ojha.mayank485's Avatar
 
Mayank Ojha
Join Date: May 2011
Posts: 22
Rep Power: 6
ojha.mayank485 is on a distinguished road
Hello,

Am trying to find the Lift coeff, Drag coeff and the Strouhal number for a cylinder in a cross flow at Re=10,000

Things I tried:
1. Created a mesh and ran cases for tstep=0.001, 0.0001 & 0.00001 using KW and SST turbulence model. The y+ for the mesh was around 3.5-4. So now I created another mesh.

2. For the new mesh, the y+ value over the cylinder surface was found to be 0.62. I ran with SST and KW at tstep=0.001 which is 2% of vortex shedding time. The time step is low enough to capture the vortex shedding.

Results:
1. My St number is 0.22 while the expected value from DNS and experimentsis 0.2~0.21
2. My Cd (average) was found to be 1.3 and expected value is 1.1
3. Lift coeff was found to be ~1 while expected value is 0.5 (which is where the real problem is). The value is almost double.


I would like to know if there is anything else I should be doing and where am I actually missing.

Thank you very much.

Ojha
ojha.mayank485 is offline   Reply With Quote

Old   June 19, 2011, 06:51
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,926
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Are you sure the lift coefficient is based on the correct reference area? Mixing up radius and diameter explains a factor of two.

Now that you have got a model which is pretty close (in everything except lift), if you wish to get more accurate you should do a proper convergence study to guide you into what options you have left. Consider Richardson extrapolation, grid convergence indexes and similar techniques to really squeeze the last drip of accuracy out of it. "Computational Fluid Dynamics" by Roache is the seminal textbook in this area, but a summary of some key concepts is here: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F - and the reference to JFE is highly recommended reading.
ghorrocks is offline   Reply With Quote

Old   June 19, 2011, 12:01
Default
  #3
New Member
 
ojha.mayank485's Avatar
 
Mayank Ojha
Join Date: May 2011
Posts: 22
Rep Power: 6
ojha.mayank485 is on a distinguished road
Thanks Glen. Appreciate your feedback.

I had another question. I am using 5% turbulence ( i.e medium intensity) at the inlet. Should this be causing the problem ???

I realize that this problem is slightly tricky because prior to separation, the flow is laminar while after separation its completely turbulent.

How about the BSL model and the non-linear RNG k-e model ? Literature say that they have been proved to be a good estimate for near wall flows and flows with rotation (which is exactly my case). But literature also say that SST should be the best (which it does not, so far).

Right now am running an LES for this case. Lets see how it goes.

BTW what is Richardson extrapolation and grid convergence indexes ??? Looks like the library is out of Roache's txt book.
ojha.mayank485 is offline   Reply With Quote

Old   June 19, 2011, 18:35
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,926
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Quote:
I am using 5% turbulence ( i.e medium intensity) at the inlet. Should this be causing the problem ???
If that is not representative of the turbulence levels of the experiment you are comparing to then definitely, yes.

Quote:
I realize that this problem is slightly tricky because prior to separation, the flow is laminar while after separation its completely turbulent.
In that case you might want to consider the turbulence transition model. That is the only turbulence model which can account for transition effects.

Quote:
Right now am running an LES for this case. Lets see how it goes.
Have you checked the dissipation is correct? Made sure you are getting the correct turbulence spectrum? Defined the inlet correctly for LES? Unless you have properly set this model up for LES you are kidding yourself. You cannot just turn on the LES option and rerun it and expect to get a reasonable answer.

Quote:
BTW what is Richardson extrapolation and grid convergence indexes ???
Looks like you need to find the textbook I referenced then! Also read the FAQ link I quoted and look them up on google. There are other ways besides the library these days.
joy2000 likes this.
ghorrocks is offline   Reply With Quote

Old   June 20, 2011, 13:01
Default
  #5
New Member
 
ojha.mayank485's Avatar
 
Mayank Ojha
Join Date: May 2011
Posts: 22
Rep Power: 6
ojha.mayank485 is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post

Have you checked the dissipation is correct? Made sure you are getting the correct turbulence spectrum?
I have never run an LES. Can I have some more details/references as to how to check for dissipation and turbulent spectrum ?

Thanks Glen.
ojha.mayank485 is offline   Reply With Quote

Old   June 20, 2011, 18:47
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,926
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
LES is a whole field of CFD in itself, your library should have textbooks on the topic. Otherwise start with general CFD books (eg Anderson) as they often introduce the concepts of LES.
ghorrocks is offline   Reply With Quote

Old   June 21, 2011, 13:17
Default
  #7
Member
 
Paulo Alexandre Costa Rocha
Join Date: Mar 2009
Posts: 71
Rep Power: 8
paulo is on a distinguished road
AFAIK a Reynolds number of 10000 is not fully turbulent for external flows. Pure RANS models are not proper. Maybe LES or a transition model can give better results.

My two cents.

Best regards,

Paulo Rocha
paulo is offline   Reply With Quote

Old   February 3, 2012, 21:49
Default
  #8
New Member
 
cfd
Join Date: Oct 2011
Posts: 17
Rep Power: 5
wind.cfd is on a distinguished road
Hi,
I am modelling the turbulent flow over the cylinder by fluent(k-epsilon model)
I have a basic question about defining the boundary conditions for the domain. The domain is rectangular. for specifying velocity inlet for domain, I have to define the turbulent intensity as well as hydraulic diameter, I want to know I should use the diameter of the cylinder as the Hydraulic diameter or the cross length of the inlet face?!
Thank you
wind.cfd is offline   Reply With Quote

Old   February 4, 2012, 06:33
Default
  #9
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,944
Blog Entries: 6
Rep Power: 39
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
You should use transition model for this Reynolds number.
Far is offline   Reply With Quote

Old   February 4, 2013, 04:44
Default
  #10
hee
New Member
 
Join Date: Jan 2013
Posts: 3
Rep Power: 4
hee is on a distinguished road
Hi everyone,

I'm running a 3D cylinder simulation in FLUENT with a Re of 100,000. I've used a Transition SST model with a time-step size of 1e-06 and 10,000 time steps. I'm trying to obtain the drag coefficient from this simulation

The results I've obtained shows an oscillatory motion, with the Cd value hitting a peak of 1.21 midway before falling back to 0.726 at the end of the 10,000 time steps.

Can anyone tell me why has this occurred? What do I need to do for the Cd values to be stablised?

Thanks!

Regards,
Hee
emreg likes this.
hee is offline   Reply With Quote

Old   February 4, 2013, 05:10
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,926
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Your question is about Fluent, not CFX and this is the CFX forum. But the answer is the same: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
ghorrocks is offline   Reply With Quote

Old   May 18, 2015, 20:11
Default
  #12
Senior Member
 
Emre G
Join Date: May 2011
Location: Turkey
Posts: 109
Rep Power: 6
emreg is on a distinguished road
Quote:
Originally Posted by hee View Post
Hi everyone,

I'm running a 3D cylinder simulation in FLUENT with a Re of 100,000. I've used a Transition SST model with a time-step size of 1e-06 and 10,000 time steps. I'm trying to obtain the drag coefficient from this simulation

The results I've obtained shows an oscillatory motion, with the Cd value hitting a peak of 1.21 midway before falling back to 0.726 at the end of the 10,000 time steps.

Can anyone tell me why has this occurred? What do I need to do for the Cd values to be stablised?

Thanks!

Regards,
Hee
is there a solution on this issue please?
emreg is offline   Reply With Quote

Old   May 18, 2015, 21:03
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,926
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
My post #11 is a pretty clear response to this.
ghorrocks is offline   Reply With Quote

Old   May 19, 2015, 02:09
Default
  #14
Senior Member
 
RicochetJ's Avatar
 
Mr CFD
Join Date: Jun 2012
Location: Britain
Posts: 291
Rep Power: 6
RicochetJ is on a distinguished road
Is zonal RANS a thing? I.e. define two subdomains? A laminar one and a turbulent RANS one?
RicochetJ 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
Modified k-e turbulence model UDF - help! Travis FLUENT 5 January 20, 2014 08:34
question about turbulence model selection and sensitivity karananand Main CFD Forum 1 February 26, 2010 05:41
Centrifugal Pump and Turbulence Model Michiel CFX 12 January 25, 2010 04:20
SSG Reynolds Turbulence Model Georges CFX 1 February 28, 2007 17:15
Turbulence model Herry Phoenics 1 May 29, 2003 13:19


All times are GMT -4. The time now is 11:34.