CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

M6 Validation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 2, 2010, 18:17
Default M6 Validation
  #1
New Member
 
steve levitt
Join Date: Jun 2010
Location: UK
Posts: 9
Rep Power: 7
steve1 is on a distinguished road
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.

untitled.JPG

Any ideas on where to proceed.

Steve
steve1 is offline   Reply With Quote

Old   October 4, 2010, 17:59
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,658
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   October 6, 2010, 17:36
Default M6 Validation
  #3
New Member
 
steve levitt
Join Date: Jun 2010
Location: UK
Posts: 9
Rep Power: 7
steve1 is on a distinguished road
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.
steve1 is offline   Reply With Quote

Old   October 6, 2010, 17:50
Default
  #4
Senior Member
 
Michael P. Owen
Join Date: Mar 2009
Posts: 195
Rep Power: 8
michael_owen is on a distinguished road
Quote:
Originally Posted by steve1 View Post
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.
michael_owen is offline   Reply With Quote

Old   October 7, 2010, 04:49
Default
  #5
New Member
 
steve levitt
Join Date: Jun 2010
Location: UK
Posts: 9
Rep Power: 7
steve1 is on a distinguished road
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.

press.jpg


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

Mach.JPG
steve1 is offline   Reply With Quote

Old   October 7, 2010, 06:20
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,658
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   October 7, 2010, 14:44
Default
  #7
Senior Member
 
Michael P. Owen
Join Date: Mar 2009
Posts: 195
Rep Power: 8
michael_owen is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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.
michael_owen is offline   Reply With Quote

Old   October 11, 2010, 10:52
Default
  #8
New Member
 
steve levitt
Join Date: Jun 2010
Location: UK
Posts: 9
Rep Power: 7
steve1 is on a distinguished road
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
steve1 is offline   Reply With Quote

Old   October 11, 2010, 18:05
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,658
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Do a sensitivity study on all of them.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
OpenFOAM - Validation of Results Ahmed OpenFOAM Running, Solving & CFD 9 June 22, 2011 18:59
Aug 2006 Focus Area: Validation and test cases Jonas Larsson CFD-Wiki 3 March 14, 2008 06:02
Urgent: RAE 2822 validation NID Main CFD Forum 0 September 3, 2004 10:34
Turbulent Flat Plate Validation Case Jonas Larsson Main CFD Forum 0 April 2, 2004 10:25
code validation Ma Main CFD Forum 8 February 14, 2002 11:25


All times are GMT -4. The time now is 04:36.