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

Drag coefficient of a sphere

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

Like Tree1Likes
  • 1 Post By RobertK

Reply
 
LinkBack Thread Tools Display Modes
Old   December 9, 2016, 06:32
Default Drag coefficient of a sphere
  #1
New Member
 
Join Date: Dec 2016
Posts: 3
Rep Power: 2
RobertK is on a distinguished road
Hello everyone,
I would like to ask you about drag coefficient calculations using Fluent.

The problem I am solving is a free flow around a sphere (3D analysis). I want to calculate coefficient of drag in function of Reynolds number. As a starting point I chose Re = 10 000 at which the Cd should be around 0.4 (based on literature). However the result I obtain is Cd=0.24. Below there are some more details. Maybe anyone can spot a mistake?

Ball diameter = 0.01m
Inlet velocity = 16.18 m/s

Domain is modelled without using symmetry plane (BC).
Reference values:
Area = 0.0000785 m2
Velocity = 16.18 m/s

In the drag monitor the sphere wall is selected and the X vector (direction of the flow).

Turbulence model used in solver: standard k- omega. I tried k-epsilon as well and results are almost identical.

Calculations are performed in steady state. I did transient analysis as well (0.1s time step) and the results are also very similar to the steady ones.

I can understand some discrepancies between CFD and measurements but not 2 times too small values.

Any ideas what's wrong?
shashanktiwari619 likes this.
RobertK is offline   Reply With Quote

Old   December 9, 2016, 17:15
Default
  #2
`e`
Senior Member
 
Join Date: Mar 2015
Posts: 800
Rep Power: 11
`e` is on a distinguished road
Flow over a sphere at Re = 10,000 is in the subcritical flow regime where the wake has turbulence, and vortices are shedding from the sphere. The transition from laminar to turbulence is a tricky phenomena to simulate and the k-e and k-w turbulence models are not well suited for this scenario (they diffuse the turbulence so well that you're finding a solution in steady state). If you want to simulate the flow accurately, then investigate large eddy simulations (there are plenty of papers in literature). You should select a small enough time step to accurately resolve the vortices (related to the Strouhal number; say 25 - 50 steps per vortex period).
`e` is offline   Reply With Quote

Old   December 12, 2016, 05:32
Default
  #3
New Member
 
Join Date: Dec 2016
Posts: 3
Rep Power: 2
RobertK is on a distinguished road
Thank you for the hint.

Indeed I tried out couple of viscous models and the one which gave me the expected results was the Scale Adaptive Simulation (SAS).
RobertK is offline   Reply With Quote

Old   December 13, 2016, 03:38
Default
  #4
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 1,886
Rep Power: 26
LuckyTran will become famous soon enoughLuckyTran will become famous soon enough
What about reference density? Check all your reference values.
LuckyTran is offline   Reply With Quote

Old   December 14, 2016, 06:41
Default
  #5
New Member
 
Join Date: Dec 2016
Posts: 3
Rep Power: 2
RobertK is on a distinguished road
Problem solved with SAS model. Reference density is calculated from the inlet values.
In incompressible flow it looks all right. The question is if this is still valid for the compressible flows with Mach number above 1.0?
RobertK 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
wrong SU2 calculation for lift and drag coefficient for NAC4421 mechy SU2 7 January 9, 2017 06:18
Error in Drag Coefficient for 3D sphere scyllakeeper FLUENT 0 June 7, 2016 08:22
Drag coefficient for a sphere Nico A. OpenFOAM Running, Solving & CFD 0 July 5, 2011 12:21
Automotive test case vinz OpenFOAM Running, Solving & CFD 98 October 27, 2008 09:43
meshing F1 front wing Steve FLUENT 0 April 17, 2003 12:37


All times are GMT -4. The time now is 19:30.