
[Sponsors] 
August 31, 2007, 11:28 
2D Low Speed Airfoil Problem when altering Inlet

#1 
Guest
Posts: n/a

I am having problems running a simple 2D mesh of a NACA aerofoil section through CFX 10.
I am trying to vary the angle of attack of the section to extract a lift polar, however if I use cartesian velocity components (U,V,W) to create an inlet flow angle of attack (ie rectangular domain with section lying in domain axis), the drags extracted are 100 times larger than expected, and the lift curve gradient is less than expected. (CASE 1) Due to this I decided to create a number of geometries where the airfoil section was rotated (to allow the inlet velocity to be inputted using only one component ie. U). When running this through CFX I get a lift curve that matches experimental data and the drags are a factor of 10 to large 9which is better than 100!). (CASE 2) I am having trouble explaining why this is happening, and was wondering if someone may be able to shed any light on the matter? Or how to solve it. I understand that my meshes will be different do to the geometry rotating in the second case but the mesh spacing i used i kept constant and in the same relative positions. Results for both case converge to e5 after about 60 iterations. I have compared the locations of the max residuals and found that for both cases they are in roughly the same place (taking into account the rotation). The domain is a rectangular one and is set up as follows and I have ran SST, SST + TT and KEpsilon all with the same trends: CASE 1; Airfoil Section: Wall (no slip), Outlet: outlet Relative pressure 0, Domain Top: Wall (free slip), Domain Sides: Symmetry planes, Inlet and domain base: Inlets with the relevant cartesian velocities. CASE 2; Airfoil Section: Wall (no slip), Outlet: outlet Relative pressure 0, Domain Top: Wall (free slip), Domain Sides: Symmetry planes, Domain Base: Wall (free slip), Inlet: Inlet with velocity in +U Any help would be much appreciated! Thanks in advance 

August 31, 2007, 18:30 
Re: 2D Low Speed Airfoil Problem when altering Inl

#2 
Guest
Posts: n/a

Hi,
What Re number? Any surface roughness? What range of angle of attack? Glenn Horrocks 

September 5, 2007, 11:21 
Re: 2D Low Speed Airfoil Problem when altering Inl

#3 
Guest
Posts: n/a

CFX is using a reynolds of about 6mill and I have no added roughness, the problem occurs at all alphas above 0 degrees to the cartesian velocity component runs. Cheers


September 5, 2007, 18:38 
Re: 2D Low Speed Airfoil Problem when altering Inl

#4 
Guest
Posts: n/a

Hi,
Have you done a mesh refinement study? Glenn Horrocks 

September 6, 2007, 06:04 
Re: 2D Low Speed Airfoil Problem when altering Inl

#5 
Guest
Posts: n/a

Yes, I have tried a mesh refinement study and I get slightly better results (for a finer mesh) in that they are closer to the wind tunnel test results but there is still a vast difference in drag between the rotated geometry and the cartesian corrected geometry for angle of attack.
I have come across some other projects where the same problem has been identified but without results as to why there is a differnce between the results when the geometries are essentially the same, only the domain set up being different. 

September 9, 2007, 18:43 
Re: 2D Low Speed Airfoil Problem when altering Inl

#6 
Guest
Posts: n/a

Hi,
But have you established a mesh independent solution? If the solution changes with a finer mesh it sounds like you have not achieved mesh independence yet. Can you post some images of your mesh? Glenn Horrocks 

September 11, 2007, 10:15 
Re: 2D Low Speed Airfoil Problem when altering Inl

#7 
Guest
Posts: n/a

I have achieved mesh independance, in that by increasing the mesh density the solution does not reduce anymore. However the two meshes are still generating the same problem, I have hosted mesh images on the links below; the first being the one where the flow inlet is the left hand side of the domain at 90degrees, which gives a result when submitting a full polar of an extremly similar lift curve to wind tunnel data, and say drag values of a factor of 10:
or if above doesnt work http://img378.imageshack.us/img378/6...sectionew1.jpg The second image shows the rotated flow mesh, where the flow inlets the domain along the left and bottom sides of the domain, with cartesian velocity components to give the same angle of attack as the previous image (so the flow is flowing diagonally up from the left to the right). This gives a result where the lift gradient is shallower than wind tunnel results and drag values of a factor of 100 (ten times the previous mesh): or if above doesnt work http://img442.imageshack.us/img442/3...tedflowpc0.jpg I hope the images work, and they show some clues as to why I am getting theresults I am. Cheers 

September 14, 2007, 19:29 
Re: 2D Low Speed Airfoil Problem when altering Inl

#8 
Guest
Posts: n/a

Hi,
Looks like a good quality mesh. How does it look at the trailing edge? Does your turbulence inlet condition match the wind tunnel? You are running with a significant blockage factor. Have you checked the proximity of your outlet and top and bottom wall does not affect things or matches the wind tunnel? I assume you have checked the basics: correct fluid, turbulence model, wind velocity, surface roughness etc etc. For the record you should be able to get a pretty accurate answer for both lift and drag in this Re regime, I would guess 1% on lift and 5% on drag (just my guesses, no science behind that estimate) so something is wrong somewhere. Glenn Horrocks 

September 18, 2007, 09:15 
Re: 2D Low Speed Airfoil Problem when altering Inl

#9 
Guest
Posts: n/a

Im not as concerned about not getting the CFD results equal to the wind tunnel results at the moment, my main concern is why the results are so different for the two different meshes, where in theroy they should give the same results (obviously give or take 1% or so for mesh differences) as they are modelling the same problem, only in two different ways. The first with the geometry at the required angle of attack, and the second using cartesian velocities to mimic that same angle of attack, Any Ideas? Cheers Mike


September 19, 2007, 08:25 
Re: 2D Low Speed Airfoil Problem when altering Inl

#10 
Guest
Posts: n/a

I have done some more analysis upon the two CFX setups and have found that the locations of the maximum residuals are in the same locations (relative to the section) for both the rotated flow and the rotated section geometries (see previous images for geometry examples). I have also carried out some boundary layer analysis and found tha the rotated flow results (blue) give a thinner boundary layer that expands at a slower rate, than the rotated section (red) see the image below;
http://img217.imageshack.us/img217/9...rylayerxr5.jpg I thought this may be of some use as to why the results are so different between the two set ups? but it has confused me more as the geometry giving me higher drag results (rotated flow) gives a thinner boundary layer, would this be expected? Thanks in advance Mike 

September 19, 2007, 18:20 
Re: 2D Low Speed Airfoil Problem when altering Inl

#11 
Guest
Posts: n/a

Hi,
Have you done a sensitivity check of the proximity of your inlet, outlet and top/bottom wall boundaries? If they are too close it will show up as a difference between the two approaches. Glenn Horrocks 

September 26, 2007, 14:29 
Re: 2D Low Speed Airfoil Problem when altering Inl

#12 
Guest
Posts: n/a

Thanks Glen, I have now carried out a study into the domain size to see if there are any problems with the walls and found that the domain needed to be enlarged by a factor of about 6! So I have now done this, although I have got a new problem that I didnt notice before, although it has been there all along... For the Alpha = 0 degrees case there is an offset in CD of +0.003 compared to the wind tunnel test data, I realise that there should not be such a large difference (considering WT CD=0.006 and CFX CD=0.009 at Alpha=0) So I an now beginning to think that my fluid setup etc is incorrect, could you have a look through the begging of the CFX post out file and see if there are any glaring problems if I was wanting to run these using SST with Transitional Turbulence, velocity=68m/s, P=101325Pa, Air@25degC:
Setting up CFX5 Solver run ... ++    CFX Command Language for Run    ++ LIBRARY: MATERIAL: Air at 25 C Material Description = Air at 25 C and 1 atm (dry) Material Group = Air Data, Constant Property Gases Option = Pure Substance Thermodynamic State = Gas PROPERTIES: Option = General Material Thermal Expansivity = 0.003356 [K^1] ABSORPTION COEFFICIENT: Absorption Coefficient = 0.01 [m^1] Option = Value END DYNAMIC VISCOSITY: Dynamic Viscosity = 1.831E05 [kg m^1 s^1] Option = Value END EQUATION OF STATE: Density = 1.185 [kg m^3] Molar Mass = 28.96 [kg kmol^1] Option = Value END REFRACTIVE INDEX: Option = Value Refractive Index = 1.0 [m m^1] END SCATTERING COEFFICIENT: Option = Value Scattering Coefficient = 0.0 [m^1] END SPECIFIC HEAT CAPACITY: Option = Value Reference Pressure = 1 [atm] Reference Specific Enthalpy = 0. [J/kg] Reference Specific Entropy = 0. [J/kg/K] Reference Temperature = 25 [C] Specific Heat Capacity = 1.0044E+03 [J kg^1 K^1] Specific Heat Type = Constant Pressure END THERMAL CONDUCTIVITY: Option = Value Thermal Conductivity = 2.61E02 [W m^1 K^1] END END END END EXECUTION CONTROL: PARALLEL HOST LIBRARY: HOST DEFINITION: laptop Installation Root = C:\Program Files\Ansys Inc\CFX\CFX%v Host Architecture String = intel_p4.sse2_winnt5.1 END END PARTITIONER STEP CONTROL: Multidomain Option = Independent Partitioning Runtime Priority = Standard MEMORY CONTROL: Memory Allocation Factor = 1.0 END PARTITIONING TYPE: MeTiS Type = kway Option = MeTiS Partition Size Rule = Automatic END END RUN DEFINITION: Definition File = C:/Documents and Settings/Mike and Annie/My \ Documents/Mikes Docs/UNI/Dissertation/FYP/Validation/Mesh \ Dependancy/Alpha0 Domain Size/23012_Domain_180sq.def Interpolate Initial Values = Off Run Mode = Full END SOLVER STEP CONTROL: Runtime Priority = Standard EXECUTABLE SELECTION: Double Precision = Off END MEMORY CONTROL: Memory Allocation Factor = 1.0 END PARALLEL ENVIRONMENT: Number of Processes = 1 Start Method = Serial END END END FLOW: DOMAIN: Domain 1 Coord Frame = Coord 0 Domain Type = Fluid Fluids List = Air at 25 C Location = Assembly BOUNDARY: Inlet Boundary Type = INLET Location = Inlet BOUNDARY CONDITIONS: FLOW REGIME: Option = Subsonic END MASS AND MOMENTUM: Option = Cartesian Velocity Components U = 68 [m s^1] V = 0 [m s^1] W = 0 [m s^1] END TURBULENCE: Option = Medium Intensity and Eddy Viscosity Ratio END END END BOUNDARY: Outlet Boundary Type = OUTLET Location = Outlet BOUNDARY CONDITIONS: FLOW REGIME: Option = Subsonic END MASS AND MOMENTUM: Option = Average Static Pressure Relative Pressure = 0 [Pa] END PRESSURE AVERAGING: Option = Average Over Whole Outlet END END END BOUNDARY: Top Boundary Type = WALL Location = Top BOUNDARY CONDITIONS: WALL INFLUENCE ON FLOW: Option = Free Slip END END END BOUNDARY: Base Boundary Type = WALL Location = Base BOUNDARY CONDITIONS: WALL INFLUENCE ON FLOW: Option = Free Slip END END END BOUNDARY: Port Boundary Type = SYMMETRY Location = Port END BOUNDARY: Starboard Boundary Type = SYMMETRY Location = Starboard END BOUNDARY: Section Boundary Type = WALL Location = Section BOUNDARY CONDITIONS: WALL INFLUENCE ON FLOW: Option = No Slip END END END DOMAIN MODELS: BUOYANCY MODEL: Option = Non Buoyant END DOMAIN MOTION: Option = Stationary END REFERENCE PRESSURE: Reference Pressure = 101325 [Pa] END END FLUID MODELS: COMBUSTION MODEL: Option = None END HEAT TRANSFER MODEL: Option = None END THERMAL RADIATION MODEL: Option = None END TURBULENCE MODEL: Option = SST TRANSITIONAL TURBULENCE: Option = Fully Turbulent END END TURBULENT WALL FUNCTIONS: Option = Automatic END END END INITIALISATION: Option = Automatic INITIAL CONDITIONS: Velocity Type = Cartesian CARTESIAN VELOCITY COMPONENTS: Option = Automatic END K: Option = Automatic END OMEGA: Option = Automatic END STATIC PRESSURE: Option = Automatic END END END OUTPUT CONTROL: RESULTS: File Compression Level = Default Option = Standard END END SIMULATION TYPE: Option = Steady State 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 CONVERGENCE CONTROL: Length Scale Option = Conservative Maximum Number of Iterations = 300 Timescale Control = Auto Timescale END CONVERGENCE CRITERIA: Residual Target = 0.00001 Residual Type = RMS END DYNAMIC MODEL CONTROL: Global Dynamic Model Control = On END END END COMMAND FILE: Version = 10.0 Results Version = 10.0 END ++    Solver    ++ ++    ANSYS CFX Solver 10    Version 2005.07.1110.24 Mon Jul 11 10:26:04 GMTDT 2005   Executable Attributes     single32bitoptimisedsupfortnoprofnospaglcomp     Copyright 19962005 ANSYS Europe Ltd.  ++ ++  Job Information  ++ Run mode: serial run Host computer: LAPTOP Job started: Wed Sep 26 15:59:57 2007 ++  Memory Allocated for Run (Actual usage may be less)  ++ Data Type Kwords Words/Node Words/Elem Kbytes Bytes/Node Real 36547.7 345.12 412.05 142764.6 1380.49 Integer 10310.7 97.36 116.24 40276.1 389.46 Character 2322.8 21.93 26.19 2268.3 21.93 Logical 40.0 0.38 0.45 156.2 1.51 Double 1072.4 10.13 12.09 8377.9 81.01 ++  Total Number of Nodes, Elements, and Faces  ++ Domain Name : Domain 1 Total Number of Nodes = 105898 Total Number of Elements = 88698 Total Number of Prisms = 71898 Total Number of Hexahedrons = 16800 Total Number of Faces = 177796 ++  Average Scale Information  ++ Domain Name : Domain 1 Global Length = 1.4797E+01 Minimum Extent = 1.0000E01 Maximum Extent = 1.8000E+02 Density = 1.1850E+00 Dynamic Viscosity = 1.8310E05 Velocity = 6.8000E+01 Advection Time = 2.1761E01 Reynolds Number = 6.5121E+07 ++  Checking for Isolated Fluid Regions  ++ No isolated fluid regions were found. ++  The Equations Solved in This Calculation  ++ Subsystem : Wall Scale Wallscale Subsystem : Momentum and Mass UMom VMom WMom PMass Subsystem : TurbKE and TurbFreq KTurbKE OTurbFreq CFD Solver started: Wed Sep 26 16:00:27 2007 THANKS! Mike 

August 3, 2010, 11:06 
boundary layer meshing

#13 
New Member
anil
Join Date: Jul 2010
Location: india
Posts: 3
Rep Power: 6 
hello friends how can i get boundary layer meshing on naca in GAMBIT.
pls help me i stucked here 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
GroovyBC problem in the defining inlet velocity  iampolaris  OpenFOAM Running, Solving & CFD  7  October 18, 2014 09:25 
Low Speed Airfoil  Mancusi  FLUENT  7  April 3, 2014 06:11 
Inlet boundary condition problem  Martin_D  FLUENT  1  January 10, 2013 13:58 
Gambit  meshing over airfoil wrapping (?) problem  JFDC  FLUENT  1  July 11, 2011 05:59 
Oscillating airfoil problem  ganesh  Main CFD Forum  2  June 27, 2005 13:57 