CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   M6 Validation (http://www.cfd-online.com/Forums/cfx/80663-m6-validation.html)

steve1 October 2, 2010 18:17

M6 Validation
 
1 Attachment(s)
Thanks for all the advice so far on this problem. I am still having the same problem with the M6 wing validation. The simulations work fine for any subsonic flow, however once the flow goes supersonic over the upper surface, the resulting pressure distribution is incorrect. A plot of the Mach number over the upper surface is attached and it shows 2 distinct regions of high speed flow. I have also done this simulation if fluent and it gives accurate results. in CFX, the region of high speed flow at the leading edge is smaller than fluent giving a smaller region of low pressure at the leading edge than is required. The aft region does not exist in fluent and in CFX it therefore gives a region of low pressure over the aft section where it should not be. I have a Y+ value of 1 or less on the wing.

Attachment 4849

Any ideas on where to proceed.

Steve

ghorrocks October 4, 2010 17:59

Do you know what is causing the 2 regions? A shock? Separation? Something else? That would give you a clue as to where to start looking.

steve1 October 6, 2010 17:36

M6 Validation
 
Thanks Glenn

I am not sure what is causing this problem. I have tried diffrent meshes, even without inflation layers, diffrent turbulence models, diffrent turb models. I have left turbulent wall functions on automatic, is it worth trying these.

michael_owen October 6, 2010 17:50

Quote:

Originally Posted by steve1 (Post 277517)
Thanks for all the advice so far on this problem. I am still having the same problem with the M6 wing validation. The simulations work fine for any subsonic flow, however once the flow goes supersonic over the upper surface, the resulting pressure distribution is incorrect. A plot of the Mach number over the upper surface is attached and it shows 2 distinct regions of high speed flow. I have also done this simulation if fluent and it gives accurate results. in CFX, the region of high speed flow at the leading edge is smaller than fluent giving a smaller region of low pressure at the leading edge than is required. The aft region does not exist in fluent and in CFX it therefore gives a region of low pressure over the aft section where it should not be. I have a Y+ value of 1 or less on the wing.

Attachment 4849

Any ideas on where to proceed.

Steve

I presume you are using a compressible fluid? Total energy equation? Viscous work term? What turbulence model are you using? Is your reference pressure correct? How are you specifying the boundary conditions? What is different between the FLUENT and CFX models (turbulence equations, etc)?

I can't make heads or tails of your image, by the way.

steve1 October 7, 2010 04:49

2 Attachment(s)
This is the basic setup I have been using.


General Options:
Fluids List; Air Ideal Gas
Reference Pressure; 1 atm
Buoyancy Option; Non Buoyant
Domain Motion; Stationary
Fluid Models:
Heat Transfer Option; Total Energy
Inc Viscous Work Term Select
Turbulence Model; SST
Transitional Turbulence Select
Turbulent Wall Functions; Automatic


Far Field ( Inlet )
Flow Regime Option Subsonic
Mass and Momentum
Cart. Vel. & Pressure
U = 270.715
V = 27.74
W = 0
Turbulence Option; Low Intensity 1%
Heat Transfer, Static Temperature = 263
Downstream ( Outlet )
Flow Regime Option; Subsonic
Mass and Momentum Option;
Average Static Pressure, Relative Pressure; 0 Pa
Pressure Averaging; Average Over Whole Outlet

Inboard ( Symmetry ) Symmetry

Wing ( Wall )
Wall Influence on flow - Wall, no-slip / No-Slip
Heat Transfer - Adiabatic

Global Initial Conditions
Velocity Type; Cartesian
Cartesian Velocity Components; Automatic With Value, U = 270.715 m/s V = 28.74 m/s
Static Pressure Option; Automatic
Turbulence Kinetic Energy Option; Automatic
Turbulence Eddy Dissipation (Select) Option; Automatic

Solver Control Criteria
Basic Settings:
Advection Scheme Option; High Resolution
Convergence Control; Automatic Timescale
Max. Iterations; 1000
Length Scale Option Aggressive
Convergence Criteria; Residual Type, Max
Residual Target; 1e-6

The domain is a parabolic one with a symmetry plane. the wing is level and the domain is inclined for the angle of attack.

The pressure plot on the surface is fine for subsonic and low angle of attack. At the M0.84 and 5 degrees, the plot on the upper surface disagrees with the wind tunnel data.

Attachment 4882


The mach number distribution in this region shows two areas of high speed flow. There should be only one region of high speed flow.

Attachment 4883

ghorrocks October 7, 2010 06:20

Your mach number plot gives the game away - if your contour lines are jagged like that then your mesh is too coarse. You need a finer grid. Your results on this coarse grid are rubbish.

michael_owen October 7, 2010 14:44

Quote:

Originally Posted by ghorrocks (Post 278239)
Your mach number plot gives the game away - if your contour lines are jagged like that then your mesh is too coarse. You need a finer grid. Your results on this coarse grid are rubbish.

Glenn beat me to it. Your mesh is terrible.

steve1 October 11, 2010 10:52

Thanks for the help.

I currently have 280 points on the upper surface, expanding away at a rate of 1.2. There is a boundary layer with ten layers giving a Y+ of 1.

Is it the number of points or the expansion rate that I should be concentrating on.

Steve

ghorrocks October 11, 2010 18:05

Do a sensitivity study on all of them.


All times are GMT -4. The time now is 05:30.