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

Accuracy Problem with Flow over 2D cylinder at Transcritical Reynolds Number

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 25, 2014, 05:30
Default Accuracy Problem with Flow over 2D cylinder at Transcritical Reynolds Number
  #1
New Member
 
Join Date: Nov 2012
Posts: 12
Rep Power: 3
zx9cp is on a distinguished road
Hi all,

I am trying to perform what I thought would be a fairly straightforward validation case in which I want to predict the Strouhal Number and mean drag coefficient for a 2D circular cylinder at a Reynolds number of 5,000,000 but am getting nowhere near the results I should be, can anyone help?!

I am comparing against data given in a paper by Roshko (1961) found here: http://authors.library.caltech.edu/10105/1/ROSjfm61.pdf

From this paper I should be achieving a Cd of approx 0.7 and St of approx 0.27 (I know other authors cite anywhere between 0.25 and 0.27 so I'd be happy with anything like this!). My results are way off the mark so any advice would be great!

My setup is:

Cylinder diameter: 5m

Reynolds number: 5,000,000.

Domain extents: upstream 10D, downstream 20D, Upper and Lower 10D.

SST turb model (runs both with and without trans turbs gamma theta model)

Timestep of approx 1/50 expected shedding frequency, my monitor points look really smooth so I don't think there is any issue here although I will do a time-step sensitivity study when I have checked everything in the setup.

Mesh: Fully hexahedral with an average yplus oscillating between 0.6 and 0.9. There are approx 125 streamwise nodes along the cylinder surface.

Convergence criteria at 1E-5, each iteration is solving within 4 coefficient loops and the RMS Courant Number is around 4.4.

Boundary conditions:

Inlet: Normal velocity inlet 15.45m/s (Based on air at 25C properties, isothermal flow and required Reynolds Number of 5,000,000).
Outlet: Average static pressure 0Pa (across whole outlet)
Upper and Lower: Free slip walls.
Cylinder end planes: Symmetry.
Cylinder: No-slip smooth wall.
Default turbulence intensity of 5%.

Results:

Without transitional turbulence: Cd=approx 0.4, St=approx 0.32
With trans turbulence (gamma theta): Cd=approx 0.23, St= approx 0.4
Results are independent of mesh but no time-step dependency study has been done, I want to have my setup checked first.

Any help would be gratefully received, I know there are other posts of this nature but I cant see anything that helps me past where I already am.

I can post the CCL for the most recent run if neccessary,

Cheers,

Chris
zx9cp is offline   Reply With Quote

Old   February 25, 2014, 17:27
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,432
Rep Power: 76
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I would do a time step size and convergence tolerance sensitivity check, but if you say you are converging to 4 coeff loops per iteration then your current time step looks pretty good.

There is an FAQ on accuracy but you appear to have looked at most of the issues discussed on the page. Still it is worth a look, it might remind you of something you missed: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

Please post your CCL and images of you mesh.
ghorrocks is offline   Reply With Quote

Old   February 26, 2014, 07:31
Default
  #3
New Member
 
Join Date: Nov 2012
Posts: 12
Rep Power: 3
zx9cp is on a distinguished road
Hi Glenn,

Thanks for looking at this. I've put a link below to the CCL for the run with no transitional turbulence, can put the other up if necessary. Also in the same place are a few mesh images

https://www.dropbox.com/sh/kvxj8ziq37rjqpa/EiQ4VU2Ns6

Any help greatly appreciated

Chris
Attached Files
File Type: txt SST_No_Transition.txt (23.7 KB, 4 views)
zx9cp is offline   Reply With Quote

Old   February 26, 2014, 16:56
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 9,432
Rep Power: 76
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
* Use adaptive time stepping, or at least do a time step sensitivity check on the time step you are using.
* Check that the inlet turbulence you have specified is not diffusing the vorticies. Try with a very low inlet turbulence.
* Your y+ is averaged over the whole cylinder. This includes the front section which has a boundary layer, and the rear section which will have a large separation. Getting the average y+ over both these regions does not appear useful. I would think calculating y+ up until separation (of maybe just the front half) would be useful.
* Check whether your separation point is about right. It might give you a clue.
* You have first order turbulence numerics. You might need second for this.
ghorrocks is offline   Reply With Quote

Old   February 28, 2014, 17:58
Default
  #5
New Member
 
Join Date: Nov 2012
Posts: 12
Rep Power: 3
zx9cp is on a distinguished road
Thanks for the advice, been a bit distracted by another job but will look. At these points on Monday...............
zx9cp is offline   Reply With Quote

Reply

Tags
2d simulation, cylinder, drag coefficients, high reynolds number, vortex shedding

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
Foam::error::PrintStack almir OpenFOAM 45 July 8, 2014 04:12
Flow past rotating cylinder: Problem with ForeCoeffs raf1111 OpenFOAM 1 December 16, 2013 09:45
Flow past a cylinder, Reynolds No: 100, Tracking strouhal Number. Karan FLUENT 7 October 7, 2013 12:37
Can 'shock waves' occur in viscous fluid flows? diaw Main CFD Forum 105 November 20, 2009 04:19
Difficulties in solving a high Reynolds number Flow? wowakai Main CFD Forum 10 December 29, 1998 13:46


All times are GMT -4. The time now is 05:38.