Hi all, sorry for long answer, so I have created a new topic. Here are my results with the implementation of the transition model. It have given me results much closer to reality than simulation without it. As you can see, I have a small indication of the Chebeba's problem, but it is not fully developed. Perhaps it is due to unstructured mesh with less resolution. Anyway, I'll be glad, if you tell me any weakness of my simulation or any improvement hints. Best, PetrK

Here we go: (AoA=4 deg)

My mesh and Y+ (19 layers in the inflation layer)

Settings (it is not a secret )

FLOW:

DOMAIN: Wing

Coord Frame = Coord 0

Domain Type = Fluid

Fluids List = Air Ideal Gas

Location = Assembly

BOUNDARY: Inlet

Boundary Type = INLET

Location = Inlet

BOUNDARY CONDITIONS:

FLOW REGIME:

Option = Subsonic

END

MASS AND MOMENTUM:

Option = Cartesian Velocity Components

U = -VX

V = 0 [m s^-1]

W = VY

END

TURBULENCE:

Option = Zero Gradient

END

END

END

BOUNDARY: Outlet

Boundary Type = OUTLET

Location = Outlet

BOUNDARY CONDITIONS:

FLOW REGIME:

Option = Subsonic

END

MASS AND MOMENTUM:

Option = Static Pressure

Relative Pressure = 0 [Pa]

END

END

END

BOUNDARY: Attached

Boundary Type = SYMMETRY

Location = Attached wall

END

BOUNDARY: Free

Boundary Type = WALL

Location = Free wall

BOUNDARY CONDITIONS:

WALL INFLUENCE ON FLOW:

Option = Free Slip

END

END

END

BOUNDARY: WingWall

Boundary Type = WALL

Location = WingWall

BOUNDARY CONDITIONS:

WALL INFLUENCE ON FLOW:

Option = No Slip

END

END

END

BOUNDARY: Bottom

Boundary Type = INLET

Location = Bottom

BOUNDARY CONDITIONS:

FLOW REGIME:

Option = Subsonic

END

MASS AND MOMENTUM:

Option = Cartesian Velocity Components

U = -VX

V = 0 [m s^-1]

W = VY

END

TURBULENCE:

Option = Zero Gradient

END

END

END

BOUNDARY: Top

Boundary Type = OUTLET

Location = Top

BOUNDARY CONDITIONS:

FLOW REGIME:

Option = Subsonic

END

MASS AND MOMENTUM:

Option = Static Pressure

Relative Pressure = 0 [Pa]

END

END

END

DOMAIN MODELS:

BUOYANCY MODEL:

Option = Non Buoyant

END

DOMAIN MOTION:

Option = Stationary

END

MESH DEFORMATION:

Option = None

END

REFERENCE PRESSURE:

Reference Pressure = 1 [atm]

END

END

FLUID MODELS:

ADDITIONAL VARIABLE: Cp coef

Additional Variable Value = Cp expr

Option = Algebraic Equation

END

COMBUSTION MODEL:

Option = None

END

HEAT TRANSFER MODEL:

Fluid Temperature = 273.15 [K]

Option = Isothermal

END

THERMAL RADIATION MODEL:

Option = None

END

TURBULENCE MODEL:

Option = SST

TRANSITIONAL TURBULENCE:

Option = Gamma Theta Model

TRANSITION ONSET CORRELATION:

Option = Langtry Menter

END

END

END

TURBULENT WALL FUNCTIONS:

Option = Automatic

END

END

END

EXPERT PARAMETERS:

mg solver option = 2

pressure diffusion scheme = 1

relax mass = 1

stage reverse flow robustness = t

tef numerics option = 1

wallscale diffusion scheme = 2

wallscale relaxation factor = 1

END

INITIALISATION:

Option = Automatic

INITIAL CONDITIONS:

Velocity Type = Cartesian

CARTESIAN VELOCITY COMPONENTS:

Option = Automatic with Value

U = -83 [km hr^-1]

V = 0 [m s^-1]

W = 1 [km hr^-1]

END

EPSILON:

Option = Automatic with Value

END

K:

Option = Automatic

END

STATIC PRESSURE:

Option = Automatic with Value

Relative Pressure = 0 [Pa]

END

END

END

OUTPUT CONTROL:

MONITOR OBJECTS:

Monitor Coefficient Loop Convergence = False

MONITOR BALANCES:

Option = Full

END

MONITOR FORCES:

Option = Full

END

MONITOR PARTICLES:

Option = Full

END

MONITOR POINT: Wing CD

Expression Value = CD

Option = Expression

END

MONITOR POINT: Wing CL

Expression Value = CL

Option = Expression

END

MONITOR RESIDUALS:

Option = Full

END

MONITOR TOTALS:

Option = Full

END

END

RESULTS:

File Compression Level = Default

Option = Standard

END

END

SIMULATION TYPE:

Option = Transient

INITIAL TIME:

Option = Automatic with Value

Time = 0 [s]

END

TIME DURATION:

Maximum Number of Timesteps = 75

Option = Maximum Number of Timesteps

END

TIME STEPS:

Option = Timesteps

Timesteps = 0.1 [s]

END

END

SOLUTION UNITS:

Angle Units = [rad]

Length Units = [m]

Mass Units = [kg]

Solid Angle Units = [sr]

Temperature Units = [K]

Time Units = [s]

END

SOLVER CONTROL:

ADVECTION SCHEME:

Option = High Resolution

END

BODY FORCES:

Body Force Averaging Type = Volume-Weighted

END

CONVERGENCE CONTROL:

Maximum Number of Coefficient Loops = 1

Timescale Control = Coefficient Loops

END

CONVERGENCE CRITERIA:

Residual Target = 5e-4

Residual Type = MAX

END

INTERPOLATION SCHEME:

Pressure Interpolation Type = Trilinear

Shape Function Option = Geometric

Velocity Interpolation Type = Trilinear

END

TRANSIENT SCHEME:

Option = Second Order Backward Euler

END

END END COMMAND FILE:

Results Version = 10.0

Version = 10.0 END

The immediate differences I see is you have about 3x lower y+ values than I did, and an unstruct mesh. According to the tests in the CFX Modeling Manual the y+ difference is unimportant, but I will make a run with an even lower y+ and see if that changes anything.

What Reynolds number are you at approximately?

/C

about 7.5x6 (Speed at the inlet is 85 km/hod, reference lengh approx. 1.8m). THe y+ value is important due to the low-Re model (see documentation for more info) Good Luck, PetrK

Maybe you should try the same settings with an unstructured mesh and comare the results.

PetrK, what does your boundary layer look like? Number of layers and expansion ratio?

I am doing a run now with significantly lower y+, and it changes the results quite drastically. But I still have the same problem, although much less frequent. It seems maybe the plate tests and recommendations from the CFX manual are quite far from whats needed in reality.

/C

Well, nothing new, after all.Stil seeing the spikes with a mesh that answers all previous comments:

- y+ around 0.2 - 0.5 as in PetrK's case (Also my Re is almost identical to his, 6.5e+06). - Expansion Ratio 1.15 as Mr angtry suggested - 50 layers in the boundary layer combined with a finer tet mesh outside the BL gives a much smoother transition from BL to volume mesh as suggested by Glenn Horrocks.

For reference here is a closeup of the BL - Volume transition:



I will now have to change my meshing strategy from struct to unstruct, I suppose. It is the only thing I didn't try so far, since it is more work... It would be interesting to know if Fransesco was using struct or unstruct. Are you still around ?

Hi Chebeba,

the pressure and suction surfaces of the blade in my case are meshed with a structured scheme. These face meshes are then inflated using an expansion ratio of 1.15. The y+ values I am getting are 0.3-0.7. The rest of the volume is meshed with tets.

Francesco

My mesh (19 layers,exp.f 1.5)

Hi,

It seems to me that you have not achieved mesh-independance yet. Maybe you should take a 2D cross section out of your geometry and do a mesh-independance study on that. Once you have found the mesh-independant resolution return to the 3D geometry.

Glenn Horrocks

So it is interesting to notice that PetrK has good results even with a mesh expansion waay above what Mr Langtry considers appropriate (1.5 as opposed to 1.15), with his unstruct mesh, and me and Fransesco are getting spikes with our struct BL meshes.

I haven't hade time yet to complete an unstruct meshing of my foil, ICEM is giving me some headaches there, I will report back once I have succeded.

I'm not shure what Mr Horrocks refers to about mesh independence, I have very consistent (and wrong) results regardless of wether I have 100 or 200 streamwise nodes, y+ 0.2 or 2, expansion 1.15 or 1.3, 20 to 50 BL layers etc. I think I have tried now about 10 different permutations of mesh dimensions, with total element couns between 1.5 and 5M elements. All give the same results (+/- 10% or so), but they all exhibit the spikes.

/C

Well... There you have it. Exact same model, approx same mesh parameters, but unstruct boundary layer.

Beautiful transition!

Something with the hexa meshpoints being exactly downstream or something must screw up the transition model equations??? /C

Its interesting that the onset of transition appear to run parallel with the edges of the mesh !! It appears that the problems only occure when looking at true 3D problems. Does anyone know what geometries the model was tested against when it was developed ?

Well, seems like I'm going to have to give the unstructured mesh a try too!!

I hope that switching to unstructured mesh doesn't give other problems, considering the fact that the first elements in the boundary layer (that have extremely high aspect ratios) will not be aligned with the flow anymore.

Anyway, I will post the results as soon as I run the simulation.

Thanks Chebeba for posting the results of every run you did. It helped me.

Francesco

Well, for what it's worth, I'm happy and glad it helped, and thanks to all who provided input.

To close this topic of, here's a nice little comparision between my last results with CFX and XFoils take on the same problem. I have normalized a pressure curve plot from CFX and overlayed it on top of the XFoil results for comparision.