CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   2D Low Speed Airfoil Problem when altering Inlet (http://www.cfd-online.com/Forums/cfx/24479-2d-low-speed-airfoil-problem-when-altering-inlet.html)

 mike wilson August 31, 2007 11:28

2D Low Speed Airfoil Problem when altering Inlet

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 e-5 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

 Glenn Horrocks August 31, 2007 18:30

Re: 2D Low Speed Airfoil Problem when altering Inl

Hi,

What Re number? Any surface roughness? What range of angle of attack?

Glenn Horrocks

 mike wilson September 5, 2007 11:21

Re: 2D Low Speed Airfoil Problem when altering Inl

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

 Glenn Horrocks September 5, 2007 18:38

Re: 2D Low Speed Airfoil Problem when altering Inl

Hi,

Have you done a mesh refinement study?

Glenn Horrocks

 mike wilson September 6, 2007 06:04

Re: 2D Low Speed Airfoil Problem when altering Inl

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.

 Glenn Horrocks September 9, 2007 18:43

Re: 2D Low Speed Airfoil Problem when altering Inl

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

 mike wilson September 11, 2007 10:15

Re: 2D Low Speed Airfoil Problem when altering Inl

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:

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):

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

 Glenn Horrocks September 14, 2007 19:29

Re: 2D Low Speed Airfoil Problem when altering Inl

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

 mike wilson September 18, 2007 09:15

Re: 2D Low Speed Airfoil Problem when altering Inl

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

 mike wilson September 19, 2007 08:25

Re: 2D Low Speed Airfoil Problem when altering Inl

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?

 Glenn Horrocks September 19, 2007 18:20

Re: 2D Low Speed Airfoil Problem when altering Inl

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

 Mike Wilson September 26, 2007 14:29

Re: 2D Low Speed Airfoil Problem when altering Inl

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 CFX-5 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 = 1.831E-05 [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 = 2.61E-02 [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 = k-way

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

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:

END

SOLUTION UNITS:

Length Units = [m]

Mass Units = [kg]

Solid Angle Units = [sr]

Temperature Units = [K]

Time Units = [s]

END

SOLVER CONTROL:

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 2005.07.11-10.24 Mon Jul 11 10:26:04 GMTDT 2005 | | Executable Attributes | | | | single-32bit-optimised-supfort-noprof-nospag-lcomp | | | | Copyright 1996-2005 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 = 1.0000E-01

Maximum Extent = 1.8000E+02

Density = 1.1850E+00

Dynamic Viscosity = 1.8310E-05

Velocity = 6.8000E+01

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

U-Mom

V-Mom

W-Mom

P-Mass

Subsystem : TurbKE and TurbFreq

K-TurbKE

O-TurbFreq

CFD Solver started: Wed Sep 26 16:00:27 2007

THANKS! Mike

 anil raj August 3, 2010 11:06

boundary layer meshing

hello friends how can i get boundary layer meshing on naca in GAMBIT.
pls help me i stucked here

 All times are GMT -4. The time now is 03:49.