# Has anyone successfully used transition modell..p2

 Register Blogs Members List Search Today's Posts Mark Forums Read

 May 19, 2006, 15:18 Has anyone successfully used transition modell..p2 #1 PetrK Guest   Posts: n/a 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

 May 20, 2006, 07:40 Re: Has anyone successfully used transition modell #2 Chebeba Guest   Posts: n/a 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

 May 20, 2006, 08:21 Re: Has anyone successfully used transition modell #3 PetrK Guest   Posts: n/a 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.

 May 20, 2006, 15:22 Re: Has anyone successfully used transition modell #4 Chebeba Guest   Posts: n/a 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

 May 21, 2006, 06:03 Re: Has anyone successfully used transition modell #5 Chebeba Guest   Posts: n/a 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 ?

 May 21, 2006, 14:50 Re: Has anyone successfully used transition modell #6 Francesco Guest   Posts: n/a 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

 May 21, 2006, 15:33 Re: Has anyone successfully used transition modell #7 PetrK Guest   Posts: n/a My mesh (19 layers,exp.f 1.5)

 May 21, 2006, 19:33 Re: Has anyone successfully used transition modell #8 Glenn Horrocks Guest   Posts: n/a 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

 May 22, 2006, 07:19 Re: Has anyone successfully used transition modell #9 Chebeba Guest   Posts: n/a 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

 May 24, 2006, 08:07 Re: Has anyone successfully used transition modell #10 Chebeba Guest   Posts: n/a 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

 May 24, 2006, 08:59 Re: Has anyone successfully used transition modell #11 Stuart Guest   Posts: n/a 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 ?

 May 24, 2006, 11:53 Re: Has anyone successfully used transition modell #12 Francesco Guest   Posts: n/a 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

 May 26, 2006, 17:27 Successfully used transition modell! #13 Chebeba Guest   Posts: n/a 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.