I am trying to get a good reference solution for an underwater bulb.

My reference model is simple: a revolved NACA0012 profile in free water, speed = 5m/s and angle of attack = 0.

I am comparing with expected results derived from Hoerners "Fluid Dynamic Drag" for a fully turbulent solution (in my case the numbers are L=3.94m, d=0.47m, U=5.0m/s, Re=19.7e6 gives Cf=0.0027, Cd=0.072, which gives me the Drag D=157N).

I have worked with the mesh and boundary layer to get low residuals and good Y+. In this process I have achieved reasonable results in terms of the total Drag of the bulb, 142N. A lower result than the reference should be expected due to the perfectly non-rough surface.

BUT here is my problem: I some very weird numerical effect that I don't know the cause of. The pressure on the bulb has a periodic wave overlaid on the expected result. I have not seen this phenomen before, and I am wondering if someone can explain the cause and what to do to fix it:

Here are a couple of images to visualize the result:





The simulation converges in about 55 iterations. All residuals are then below 1e-4 RMS and the drag calculated as force_x()@Bulb has become steady.

I am running CFX/64 v11.0.1 in Double Precision on WinXP/64.

Relevant parts of the input CCL: (Slightly compressed to make the post reasonable length)

--------------------------------------------------------

LIBRARY: MATERIAL: Water TYPE: Option = Steady State DOMAIN: Default Domain, Coord Frame = Coord 0, Domain Type = Fluid, Fluids List = Water, Location = LIVE

BOUNDARY: BULB, Boundary Type = WALL, Location = BULB, BOUNDARY CONDITIONS: WALL INFLUENCE ON FLOW: Option = No Slip

BOUNDARY: Inlet, Boundary Type = INLET, Location = IN, BOUNDARY CONDITIONS: FLOW REGIME: Option = Subsonic MASS AND MOMENTUM: Normal Speed = 5 [m s^-1], Option = Normal Speed, TURBULENCE: Option = Low Intensity and Eddy Viscosity Ratio

BOUNDARY: Outlet, Boundary Type = OUTLET, Location = OUT, BOUNDARY CONDITIONS: FLOW REGIME: Option = Subsonic MASS AND MOMENTUM: Option = Average Static Pressure, Relative Pressure = 0 [Pa], PRESSURE AVERAGING: Option = Average Over Whole Outlet

BOUNDARY: WALL, Location = WALLS, Boundary Type = WALL, BOUNDARY CONDITIONS: WALL INFLUENCE ON FLOW: Option = Free Slip

DOMAIN MODELS: BUOYANCY MODEL: Option = Non Buoyant DOMAIN MOTION: Option = Stationary REFERENCE PRESSURE: Reference Pressure = 1 [atm]

FLUID MODELS: TURBULENCE MODEL: Option = SST, TURBULENT WALL FUNCTIONS: Option = Automatic

INITIALISATION: Option = Automatic INITIAL CONDITIONS: Velocity Type = Cartesian CARTESIAN VELOCITY COMPONENTS: Option = Automatic with Value U = 5 [m s^-1] V = 0 [m s^-1] W = 0 [m s^-1]

EPSILON: Option = Automatic K: Option = Automatic STATIC PRESSURE: Option = Automatic

------------------------------------------------------------------

Mesh Statistics Total Number of Nodes = 1838274 Total Number of Elements = 3119718 Total Number of Tetrahedrons = 1531323 Total Number of Prisms = 144 Total Number of Hexahedrons = 1547228 Total Number of Pyramids = 41023 Total Number of Faces = 41027

Oh well, what a complete and utter laugh!

I have been staring at this problem the whole weekend. And now I realize that it was caused by the actual geometry that the surface elements of the bulb was projected onto.

The default ICEM setting for curve and surface approximation was simply to coarse, causing the bulb surface to have edges. Small edges certainly, not even visible unless you looked for them, but still significant for the flow.