Drag coefficient of a sphere

RobertK · December 9, 2016, 05:32

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?

`e` · December 9, 2016, 16:15

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).

RobertK · December 12, 2016, 04:32

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).

LuckyTran · December 13, 2016, 02:38

What about reference density? Check all your reference values.

RobertK · December 14, 2016, 05:41

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?

danny9019 · June 19, 2018, 03:35

Quote:

Originally Posted by RobertK

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?

Hey, i've your same problem! how did you resolved it? Please i'm getting mad! I'm trying to simulate a sphere at Re=1e+7 with a Cd expected of 0.19 but i'm not getting this value at all. Could you help me to understand how to resolve it? Thanks!!

hectorgabriel85 · September 4, 2019, 14:09

Quote:

Originally Posted by danny9019

Hey, i've your same problem! how did you resolved it? Please i'm getting mad! I'm trying to simulate a sphere at Re=1e+7 with a Cd expected of 0.19 but i'm not getting this value at all. Could you help me to understand how to resolve it? Thanks!!

Hi Danny. Did you succeed simulating at Re=1e7? What did you do?

hectorgabriel85 · September 4, 2019, 14:10

Quote:

Originally Posted by RobertK

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?

Hi Robert:
Which turbulence model did you use exactly? Did you use pimpleFoam or pisoFoam?

December 9, 2016, 05:32	Drag coefficient of a sphere	#1
RobertK New Member Join Date: Dec 2016 Posts: 4 Rep Power: 9	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.

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 05:18
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 08:43
meshing F1 front wing	Steve	FLUENT	0	April 17, 2003 12:37

December 9, 2016, 16:15		#2
`e` Senior Member Join Date: Mar 2015 Posts: 892 Rep Power: 18	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).

December 12, 2016, 04:32		#3
RobertK New Member Join Date: Dec 2016 Posts: 4 Rep Power: 9	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).

December 13, 2016, 02:38		#4
LuckyTran Senior Member Lucky Join Date: Apr 2011 Location: Orlando, FL USA Posts: 5,675 Rep Power: 66	What about reference density? Check all your reference values.

December 14, 2016, 05:41		#5
RobertK New Member Join Date: Dec 2016 Posts: 4 Rep Power: 9	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?