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

Airfoil Coefficient of Lift and Drag - Published Data vs CFD Results

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

Like Tree3Likes
  • 1 Post By ghorrocks
  • 2 Post By ghorrocks

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 22, 2020, 04:18
Default Airfoil Coefficient of Lift and Drag - Published Data vs CFD Results
  #1
New Member
 
Michael
Join Date: Apr 2020
Location: Newcastle, Australia
Posts: 3
Rep Power: 5
Mick2450 is on a distinguished road
Hi, I’m looking for some advice about how to generate more agreeable results for lift and drag coefficient from my CFD CFX simulation of air flow across an airfoil. I’m fairly new to CFD, but have some experience in basic CFD analysis.

I have created a C-grid style mesh around my airfoil using ICEM and established appropriate boundary conditions in CFX-Pre. I’ve set my turbulence model to SST and aimed for a Y+ max < 1 across my airfoil.
I’ve performed a steady state simulation, checked residuals are converging to at least e-5 at both low and high angles of attack (AoA), and checked that monitor points for lift and drag appear to steady out with time steps. I’ve managed to roughly capture the trend of published data, but my coefficient of lift (CL) is still pretty different. As my CL results appear to get worse around stall (~14°), I thought maybe I needed to run a transient analysis for higher AoA’s, however, residuals at 14° AoA still appear to show reasonable convergence, so I’ve stuck with steady state analysis.

I’ve tried increasing mesh element count, reducing/increasing y+, reducing RMS target, and using different turbulence models (SST, k-ω, SA). No matter what changes I make, I can’t seem to achieve better results. I’m a bit stumped. As I’m fairly new to CFD, I was wondering if anyone could give me advice to improve my CL results. Thanks.

mesh basic.jpg

mesh close.jpg

CL & CD vs AoA.JPG

def domain2.jpg

solver control.JPG
Mick2450 is offline   Reply With Quote

Old   April 22, 2020, 06:49
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
You appear to have missed two fundamental physics issues:

1) Your Re appears to be 128k. For most aerofoils this is a transitional Re number where there is a large laminar section and turbulence transition somewhere near mid-chord. You cannot model this with a standard 2 eqn turbulence model, these models all assume fully turbulent conditions. You will probably need to use a turbulence transition model to capture this.

2) Getting accurate results around stall is much more challenging than for other sections of the lift vs AOA curve. What generally happens is you start getting transient large vortex shedding, and again a traditional 2 eqn turbulence model cannot capture these sort of large scale transient features. You will need to consider LES, SAS or DES approaches to model this.

Note that you will be limited in options which cover both turbulence transition AND large scale vortex shedding. You may well find that you cannot model both of these physics at the same time. But hopefully you have a happy adventure trying them all out and finding out which one works good enough for you
aero_head likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 22, 2020, 07:14
Default
  #3
New Member
 
Michael
Join Date: Apr 2020
Location: Newcastle, Australia
Posts: 3
Rep Power: 5
Mick2450 is on a distinguished road
Thanks very much for your quick response! I'll do some more research into the physics of flow separation and appropriate turbulence models.
Mick2450 is offline   Reply With Quote

Old   April 23, 2020, 05:57
Default
  #4
New Member
 
Michael
Join Date: Apr 2020
Location: Newcastle, Australia
Posts: 3
Rep Power: 5
Mick2450 is on a distinguished road
I've done some further reading on low-Re flow characteristics and updated my turbulence model to transitional SST using the gamma-theta model.

I'm now struggling to reach convergence with my residuals, and my CL & CD appear to just oscillate. I've been analysing flow behaviour at an AoA of 5 degrees, and I think I can spot the point of separation and reattachment of flow around the mid-point of the airfoil, which I didn't notice before using just a 2 equation model - so I suppose this is probably a good thing.

Is there any advice you may give for achieving convergence? I've attempted refining my mesh by increasing element count, reducing my nodal growth rate to 1.01, and fiddling with time steps.
Mick2450 is offline   Reply With Quote

Old   April 23, 2020, 20:18
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
With turbulence transition at mid chord as I expected that means you definitely need a turbulence transition model.

I can also see that you have a classic laminar separation bubble - where the laminar boundary layer detaches from the surface, goes turbulent and reattaches. This attachment/reattachment forms a laminar separation bubble. So far so good.

But laminar separation bubbles are usually transient. They like to jiggle about, which means steady state convergence is challenging. While it is theoretically possible to damp this out in my experience the best way is just to use a steady state run to get close to converged, then switch to a transient simulation and run for long enough to get a few cycles so you can get a reasonable average CL or CD.

Comments on your attempts at convergence so far:
* finer mesh will make it harder to converge steady state, not easier (as the finer mesh has reduced dissipation). But the finer mesh should be more accurate.
* reduced growth rate will be useful as the laminar separation bubble happens a distance off the surface, so this means you will have better resolution of the bubble.
* Time steps - you probably won't get this to converge steady state regardless of time step size. When you do a transient run you should expect to need very fine time steps to get good convergence. But you only need to run a short amount of physical time so hopefully it is manageable.
Julian121 and aero_head like this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Calculation of lift and drag coefficients on airfoil CoolHersheys OpenFOAM Post-Processing 5 September 27, 2021 07:04
wrong SU2 calculation for lift and drag coefficient for NAC4421 mechy SU2 7 January 9, 2017 06:18
High drag for airfoil compared to XFOIL and wind tunnel data Ry10 SU2 15 October 30, 2016 18:27
Lift and Drag Coefficient data for NACA 2412 Airfoil mahbub03 Main CFD Forum 22 May 25, 2014 16:39
airfoil lift and drag coefficient amir_14 FLUENT 5 January 1, 2013 09:30


All times are GMT -4. The time now is 20:37.