[LThomes]

Hello,
I’m having some trouble simulating laminar steady-state flow over a sphere (OpenFOAM). The solution is converged but I’m having about 15% error on the drag coefficient (CD) for 10 < Re < 100, and about 20% for Re <= 1. Please, see some pictures of my simulation in this website http://imgur.com/a/AxIWE.

1. Mesh
   I’ve tested finer meshes, and the mesh is converged. (The CD of this one differs only 1.5% from a 15.4% more refined mesh)
   
2. Solution convergence and CD
   
3. Post-processing
   From picture "Pressure over the sphere and U streamlines for Re = 80", it seems like the flow isn’t steady (because of the different size of the recirculation zone), but shouldn’t it be for Re = 80? The separation zone is increasing the pressure in the back of the sphere, is that right?
   
4. Results
   I think that there’s something strange with the pressure field, because for very low Reynolds numbers (<= 1) the drag should be predominantly viscous (my guess would be viscous CD > 90%).
   
5. Simulation parameters
   I’m using simpleFoam solver (SIMPLE algorithm), GAMG for pressure (p) field and smoothSolver for velocity field (U) (see pictures for fvSoultion and fvSchemes). I’ve already changed those field solvers (PGC, GAMG, …), refined the mesh, reduced the tolerance of p, checked the boundary conditions and checked the size of the fluid domain, but the results barely change.
   

Does anyone have any clue what’s wrong, please?
Thanks in advance.

[piu58]

Calculating pressures is one of the harder task in CFD, harder than calculation velocities. The reason: The pressure is calculated in an indirect way (by correction velocities.

The case you simulated is dome by others too. You may compare their results with the experimental findings of Schlichting: Deviations are more normal than absent.

[FMDenaro]

You could check your solution compared to the analytical solution for the flow around a sphere at low Re number...
How do you compute the stress at the wall?

[LThomes]

Originally Posted by FMDenaro

You could check your solution compared to the analytical solution for the flow around a sphere at low Re number...
How do you compute the stress at the wall?

There's a code that you write in the controlDict file that calculates the viscous ("integral of the shear stress on the area") and pressure drag.

[LThomes]

Originally Posted by FMDenaro

You could check your solution compared to the analytical solution for the flow around a sphere at low Re number...
How do you compute the stress at the wall?

I compared the simulation's with the analytical's velocities beginning at the top of the sphere and ending at the boundary of the domain (for Re = 0.05). The error is around 20%, just like the CD error. And the error of the velocity u (x axis) of the first node is 21.4%. Perhaps, the shearStress (=viscosity*du/dz) is following this error.
u.jpgw.jpg
Observations:

• The freestream velocity is 1 m/s and the velocity far away from the sphere is 1.03 m/s. Is that normal?
• I guess the analytical solution is not 100% correct, because the velocity will only be equal as the freestream velocity when z -> infinity;
• u = velocity in the x axis (freestream direction)
• w = velocity in the z axis

Any idea of what could be wrong in the simulation?

Thanks

[LThomes]

I found the problem, I was using a first order interpolation scheme for the advection term (Gauss upwind). So I did some research in the OpenFOAM User Guide and chose the Gauss linearUpwind, which is a second order scheme. And that was the problem indeed! After I did that I'm having a 1,3%-error for 20 < Re < 200. Unfortunately, for very low Reynolds numbers (Re = 1 and 0.5) the results are still the same.
p+Stream-Re80.jpg