Hi,

Just starting out with CFX and I thought to learn I would model a sphere and compare drag with theory.

One inch diameter sphere in 60 m/s airflow should have a Cd around 0.42 with total drag of around 0.46 N. My CFX results give a drag of 0.28 N (62% of theory).

I was hoping people might be able to suggest a number of reasons I could be getting this low result. The output file for the run is located at: http://teambasic.files.wordpress.com...phere2_002.doc

But I will precis what I have done below... I would greatly appreciate any help you can give me.

Regards, Rob

Loosly based on the "flow over a blunt body" tutorial. Default values unless stated.

Steady State, Air Ideal Gas, Shear Stress Transport turb model (y+ at the ball is < 1, approx 15 nodes within the boundary layer thickness). Domain size: 3 x sphere diameter in front and to sides of sphere; 10 x sphere diameter behind. 2 x symmetry planes, 2 x free slip walls. sphere is no slip. inlet is subsonic, normal vel 60m/s, turb 5% medium. outlet is subsonic, static pressure, 0 atm. init conditions: y velocity 60m/s, turb eddy dissip selected. solver control: resudual RMS 1e-5, physical timescale 1/3 of time taken to flow through domain (did another run multiplied by 4, no real difference) mesh adaption based on abs pressure, eddy visc, velocity. 3 steps. total nodes 700,000. Solution Var * edge length. 50 iterations, RMS, 1e-4.

The residuals looked okay, one order magnitude between RMS & max, no major change of drag values as i increased the mesh size. Do I need to be looking at transitional turbulence model??

Like I said, all help would be appreciated! Rob

Domain size: 3 x sphere diameter in front and to sides of sphere ... too small increase to 5.

The nature of the vortex shedding may require transient analysis. Your steady state convergence is poor.

The massive separation may also require DES, SAS-SST i.e. this is an ahmed body like problem.

There may be turbulence transition effects, although your inlet velocities are high.

Calculate the drag coefficient in the solver not in Post.

You have used a symmetry plane. So the force is for half a ball or what?



| Pressure Force On Walls

X-Comp. Y-Comp. Z-Comp.

ball 2.4304E-01 6.6143E-02 2.4464E-01

Hi,

Thanks for your response.

I used two symmetry planes - therefore 1/4 of the ball. I multiplied the force by 4 and that is the value that is 60% of expected.

Cheers, Rob

Joe,

Thanks. I will try all of the above and post another response with my results.

Regards, Rob

You might also wanna try to use a different advection scheme. In my last project with a blunt body the high-res-scheme did not yield very accurate results. SBF=1 worked much better - however there occured convergence issues from time to time.

which means you did not do a mesh refinement study?