Sphere drag Nasa vs. SimpleFoam

Xuavsed · July 1, 2015, 04:00

Hi everybody!

I need to verify my simpleFoam calculations on a basic case. I chose the sphere, I found values at different Reynolds numbers from the NASA : https://www.grc.nasa.gov/www/K-12/ai...ragsphere.html

In OpenFoam I used simpleFoam with a k-omega SST turbulence model. I worked with rho=1025 (seawater) and I used "slip" boundary conditions on the sides of my domain. I'm not really sure about my initial conditions, but I tried to change them and the differences are neglectible.

You can see my results compared to the NASA's data in the PNG file. I get a small error for some values of the Reynolds number but I get up to 75% errors for some others Reynolds. Any idea where it could come from ? Did anybody ever try to verify these values with openfoam ?

Thanks a lot.

Benjamin

andrea · July 2, 2015, 04:03

Hi,
you should give us more information about your setup, mesh refinement, etc.
Are you using wall functions or not, which are the boundary conditions on the sphere?

I tested simpleFoam on the sphere case and up to certain degree the results were fine.

Cheers

Xuavsed · July 2, 2015, 05:24

Andrea,
Thanks for the reply.

I used a blockmesh of size 40*16*16 and a refinement box close to the sphere and behind to capture the turbulence.
I also used 20 layers around the sphere with max thickness = 0.1

I used a wall function for k, omega and nut on the sphere. After some tests I'm thinking that my problem could come from my initial condition for nut (which is 0 everywhere in my domain). How should it be calculated ?

About your results, I'd be very interested to see your test case if possible.

Benjamin

tomf · July 5, 2015, 04:52

With this range of Reynolds numbers you are going from steady laminar flow, to transient laminar flow, to transitional flow and fully turbulent flow. In some parts you will also have a large vortex street behind the sphere, which you cannot accurately capture using simpleFoam (steady state). So depending on the Reynolds number you may need to use a transition model or pimpleFoam to get close to the experimental drag values.

If you use the proper solver only than things like mesh/boundary conditions may be tuned to get you closer if needed.

Regards,
Tom

Xuavsed · July 6, 2015, 10:40

Thanks Tom!
I'm trying to solve it with pimpleFoam, I'll give my results here. I wasn't sure about that, I thought a steady state solver would be fine because the drag coeff doesn't depend on time.
If anybody has a drag calculation case using pimpleFoam I'd be really interested to see it.

Benjamin

blais.bruno · July 14, 2015, 20:54

Quote:

Originally Posted by Xuavsed

Thanks Tom!
I'm trying to solve it with pimpleFoam, I'll give my results here. I wasn't sure about that, I thought a steady state solver would be fine because the drag coeff doesn't depend on time.
If anybody has a drag calculation case using pimpleFoam I'd be really interested to see it.

Benjamin

If I were you, I would try to first verify that you can get Stokes solution for Re --> 0 first. Because even at low Re (100 or so) you seem to have a very large error. For Re=100, you can go straight DNS pretty much, so the difference should be close to 0...

Xuavsed · July 15, 2015, 04:36

Thanks Bruno.
I am currently solving it for high Re using pimpleFoam, and the results seem to be much better so far. So you're suggesting that I don't need to use a turbulence model for Re < 100. But would you still use a transient solver or steady-state ?

blais.bruno · July 15, 2015, 08:21

À transient solver is always better for this case otherwise you underestimate drag. Usually you get unsteady oscillating structure, just like a von karman alley and those increase the drag. In steady state those structures are not allowed to form, thus reducing the drag artificially. In my opinion, for anything above Re=1 you will get better results in unsteady.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Study of smooth sphere drag vs golf ball drag	tkolba	FLUENT	2	May 4, 2015 03:59
Guidance sought - drag of a sphere with bump	Europa	OpenFOAM Running, Solving & CFD	0	February 5, 2015 10:51
Experimental data vs SimpleFoam sphere test case : Cd do not match	alsdia	OpenFOAM Verification & Validation	1	November 2, 2012 05:37
CFX analysis of a sphere - drag too low	Rob Findlay	CFX	6	March 26, 2007 10:11
meshing F1 front wing	Steve	FLUENT	0	April 17, 2003 12:37

July 2, 2015, 04:03		#2
andrea Member Andrea Petronio Join Date: Mar 2009 Location: Trieste, Italy Posts: 43 Rep Power: 17	Hi, you should give us more information about your setup, mesh refinement, etc. Are you using wall functions or not, which are the boundary conditions on the sphere? I tested simpleFoam on the sphere case and up to certain degree the results were fine. Cheers

July 2, 2015, 05:24		#3
Xuavsed New Member Benjamin Desvaux Join Date: Jul 2015 Posts: 4 Rep Power: 10	Andrea, Thanks for the reply. I used a blockmesh of size 401616 and a refinement box close to the sphere and behind to capture the turbulence. I also used 20 layers around the sphere with max thickness = 0.1 I used a wall function for k, omega and nut on the sphere. After some tests I'm thinking that my problem could come from my initial condition for nut (which is 0 everywhere in my domain). How should it be calculated ? About your results, I'd be very interested to see your test case if possible. Benjamin

July 5, 2015, 04:52		#4
tomf Senior Member Tom Fahner Join Date: Mar 2009 Location: Breda, Netherlands Posts: 638 Rep Power: 32	With this range of Reynolds numbers you are going from steady laminar flow, to transient laminar flow, to transitional flow and fully turbulent flow. In some parts you will also have a large vortex street behind the sphere, which you cannot accurately capture using simpleFoam (steady state). So depending on the Reynolds number you may need to use a transition model or pimpleFoam to get close to the experimental drag values. If you use the proper solver only than things like mesh/boundary conditions may be tuned to get you closer if needed. Regards, Tom

July 6, 2015, 10:40		#5
Xuavsed New Member Benjamin Desvaux Join Date: Jul 2015 Posts: 4 Rep Power: 10	Thanks Tom! I'm trying to solve it with pimpleFoam, I'll give my results here. I wasn't sure about that, I thought a steady state solver would be fine because the drag coeff doesn't depend on time. If anybody has a drag calculation case using pimpleFoam I'd be really interested to see it. Benjamin

July 15, 2015, 04:36		#7
Xuavsed New Member Benjamin Desvaux Join Date: Jul 2015 Posts: 4 Rep Power: 10	Thanks Bruno. I am currently solving it for high Re using pimpleFoam, and the results seem to be much better so far. So you're suggesting that I don't need to use a turbulence model for Re < 100. But would you still use a transient solver or steady-state ?

July 15, 2015, 08:21		#8
blais.bruno Member Bruno Blais Join Date: Sep 2013 Location: Canada Posts: 64 Rep Power: 12	À transient solver is always better for this case otherwise you underestimate drag. Usually you get unsteady oscillating structure, just like a von karman alley and those increase the drag. In steady state those structures are not allowed to form, thus reducing the drag artificially. In my opinion, for anything above Re=1 you will get better results in unsteady.