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

Problem with drag coefficient

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 3, 2012, 07:18
Default Problem with drag coefficient
  #1
New Member
 
Mindaugas
Join Date: Jun 2012
Posts: 25
Rep Power: 4
newminde is on a distinguished road
Hi everyone, I'm modeling Turbulent flow around cylinder, the main aim is to dicover Cd dependence on Reynolds numeber.
The cylinder is in the infinite field, material air, Diameter of cylinder 1m, Re=10000.
Model RNG,k-epsilon.
I'm changing only tubulent kinetic energy and tubulent Dissipation Rate.
And the resut is Cd=0.58, in case it should be approximatelly 1.1-1.2.
Maybe someone had done similar work, and have some advices.

Regards,
Mindaugas
newminde is offline   Reply With Quote

Old   August 3, 2012, 07:31
Default
  #2
Senior Member
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,032
Rep Power: 17
flotus1 will become famous soon enough
I encountered the same problem at Re=10^5. The best result I got was at about 70% of the experimental value.

Maybe you could try a k-omega based turbulence model or even RSM.
Don't worry though, I wouldn't expect a RANS model to yield perfect results in the detached flow over a blunt body.
flotus1 is offline   Reply With Quote

Old   August 3, 2012, 07:36
Default
  #3
New Member
 
Mindaugas
Join Date: Jun 2012
Posts: 25
Rep Power: 4
newminde is on a distinguished road
I thing the main problems are:
1) Bad mesh, at monday I'll try to change it.
2) Bad calculation of Turbulent kinetic energy, turbulent dissipation rate.
Also I have tried to change turbulent intensity and hydraulic diameter, but as I understand hydraulic diameter is essiantial only for pipes.
But project is 2D cylinder.

Laminar flow was quit good 1-3% inaccurate.

I thing for this exeriment k-epsilon model is good.
newminde is offline   Reply With Quote

Old   August 3, 2012, 07:48
Default
  #4
Senior Member
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,032
Rep Power: 17
flotus1 will become famous soon enough
I already did a mesh dependency study for this case.

Changing the turbulent kinetic energy and its dissipation rate at the inlet is not the right way to fix the results.
You can assume that the measurement was carried out with very low turbulent intensities upstream of the cylinder.
So increasing k at the inlet in your simulation might yield a higher C_d, but then the simulation no longer corresponds to the experiment.
flotus1 is offline   Reply With Quote

Old   August 3, 2012, 07:54
Default
  #5
New Member
 
Mindaugas
Join Date: Jun 2012
Posts: 25
Rep Power: 4
newminde is on a distinguished road
But you certainly must change parametres on the boundary conditions, because turbulence parametres dependent on Reynols number.

quate
Note by default, the FLUENT GUI enters k=1 m/s and ε =1m/s. These values
MUST be changed, they are unlikely to be correct for your simulation.
newminde is offline   Reply With Quote

Old   August 3, 2012, 08:09
Default
  #6
Senior Member
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,032
Rep Power: 17
flotus1 will become famous soon enough
But which value do you want to use? Unless you have a model of the wind tunnel that was used for the experiment, it seems impossible to me to "guess" correct values.

Aren't wind tunnels usually equipped to produce a homogneous flow field with very little turbulent disturbances?
flotus1 is offline   Reply With Quote

Old   August 3, 2012, 17:38
Default
  #7
Senior Member
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,032
Rep Power: 17
flotus1 will become famous soon enough
BTW: The turbulence parameters at the inlet do NOT depend on the Reynolds number of the flow around the cylinder.

Just imagine that in the experiment, instead of the cylinder with 1m diameter, a smaller with d=0.1m is used.
The Reynlods number decreases by a factor of 10, but the flow in the wind tunnel is still the same with the same turbulent quantities.
flotus1 is offline   Reply With Quote

Old   August 6, 2012, 01:45
Default
  #8
New Member
 
Mindaugas
Join Date: Jun 2012
Posts: 25
Rep Power: 4
newminde is on a distinguished road
All parametres can be defined:

http://hpce.iitm.ac.in/website/Manua...ug/node217.htm

I don't know what is a problem?
Maybe others have modeled turbulence flow and results were approximately equals to experimental ones?
newminde is offline   Reply With Quote

Old   August 7, 2012, 02:50
Default
  #9
New Member
 
Mindaugas
Join Date: Jun 2012
Posts: 25
Rep Power: 4
newminde is on a distinguished road
Results become more accurate. Re=10000 , Cd=0.9. I have changed turbulent model Spalart-Allmaras, turbulent intensity 0.5 and turbulent length scale 0.07, but still the result should be 1.15-1.2.
Maybe some advices, how to improve results.
newminde is offline   Reply With Quote

Old   August 7, 2012, 03:34
Default
  #10
Senior Member
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,032
Rep Power: 17
flotus1 will become famous soon enough
A wall-resolving LES should yield better results here.

Still there is the problem of the unknown Reynolds stresses and length scales at the inlet, which becomes even more crucial in a LES.
In my opinion, 0.9 is quite a good result as an approximation of the drag coefficient.
flotus1 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
problem with saving drag coefficient colopolo FLUENT 5 April 12, 2013 10:59
lift and drag ceofficient problem icemaniac178 CFX 6 August 17, 2011 18:40
Problem in plotting drag coefficient Sarinagara FLUENT 2 September 28, 2010 06:54
Drag Coefficient Convergence Problem John FLUENT 16 September 4, 2009 02:44
drag coefficient pukiwawa FLUENT 10 August 29, 2008 15:31


All times are GMT -4. The time now is 03:53.