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

Lift error of 2D flow around airfoil

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 8, 2016, 04:06
Default Lift error of 2D flow around airfoil
  #1
New Member
 
WJ
Join Date: Feb 2016
Location: MyHome
Posts: 11
Rep Power: 6
misospider is on a distinguished road
Hi.
I am doing 2d simulation of flow around airfoil with kw SST model.
My Reynolds number is around 3e4 to 5e4.
I am using low reynolds number approach, k=1e-12, w=omegawallfunction, nut=calculated at wall.
Wind tunnel data is available, my goal is to compare Cd, Cl, Cm result of CFD and experiment.

So far, Drag coefficient and Momentum coefficient are close enough to experiment, say less than 3 % error.

But lift is significantly different from experiment.
At experiemnt Cl was minus and order of e-1, say -0.1 to -0.2.
But CFD result is plus and order of e-1. say 0.1 to 0.2.

I checked lift direction definition in controldict, it looks ok and it works in other cases.

Can any one suggest what can I try to fix lift issue?

Thanks in advance.
misospider is offline   Reply With Quote

Old   December 14, 2016, 06:25
Default
  #2
New Member
 
Join Date: Oct 2016
Posts: 22
Rep Power: 6
Mahe88 is on a distinguished road
Hello misospider,

i am working on the same topic right now. Calculating the lift, drag and pressure coefficients of an airfoil.
However I am using High Reynolds approach. Therefore I have set up simulations using simpleFoam with KomegaSST and the SpalartAllmaras turbulence model.

My experience so far is, that the simpleFoam solver with KOmegaSST is quite good in predicting the lift coefficient, but is far away from the drag results. So just the opposite you discovered. Maybe we can work together and get the best out of two worlds

Could you maybe share more information on your setup? Solver, boundary conditions etc?

Also I want to use PimpleFoam for transient simulations, but when using it, my deltaT is around 1e-5, which seems to me really small.( using a Co of 3 and nOuterCorrectors 5). The length of my Farfield is 100c (c=1m) that means it takes 2s for the air to flow through my simulation area, which takes around 48h?! Maybe any ideas on that? Or experience using pimple?

Thanks!
Mahe88 is offline   Reply With Quote

Old   December 14, 2016, 12:29
Default
  #3
Member
 
Joshua
Join Date: Dec 2016
Location: St. Louis, Missouri
Posts: 91
Rep Power: 5
Joshua14 is on a distinguished road
A few things that I can think of:
1) Check your mesh. As you are running at a low Re you are prone to having vortex shedding. If you mesh is not fine enough to capture those effects off the airfoil, that maybe causing the distortion.
2) I can't remember the trend, but when I was running airfoil simulations we got better data by rounding the trailing tip instead of having it come to a sharp point.
3) Try running your simulation at a lower angle of attack for comparison and not stall. (Not sure what AOA your running)
4) With the vortex shedding I would suggest assuming the solution is unsteady, aka using a transient solver.

I hope this helps!

Joshua
Joshua14 is offline   Reply With Quote

Old   December 17, 2016, 06:20
Default
  #4
Member
 
Join Date: Mar 2014
Posts: 78
Rep Power: 8
mzzmrt is on a distinguished road
Since the Re is low, I suspect the kOmegaSST will work with this problem. As far as I know OpenFOAM implementation of kOmegaSST is for highRe only and can be used with wall functions. (There are community developed lowRe versions of kOmegaSST but must be compiled, you can find them in this forum)

You need to resolve the boundary layer so do not use wall functions. Due to the Reynolds regime transition phenomena will also be important. In that case the most suitable and available model for your problem may be considered as kkLOmega, this model is also not perfect though. If the AoA is low you can also start with the SA model.

The initial boundary conditions, yPlus (must be <1), solver settings (must be transient), grid resolution and quality are also very important...
mzzmrt is offline   Reply With Quote

Old   January 10, 2017, 04:45
Default Re:
  #5
New Member
 
WJ
Join Date: Feb 2016
Location: MyHome
Posts: 11
Rep Power: 6
misospider is on a distinguished road
Sorry for the late reply.

I am still in same problem, but I have found some clues.

I was using same domain size as wind tunnel, but after changing domain into larger domain, the values are more reasonable.

Also I have tried k-kl-w model, it works better in wind tunnel domain, but its value has larger error in larger domain.

I am going to discuss this issue with my supervisor, once I got some insights will post here.

Thanks for the all your replies and help!
misospider 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
wrong SU2 calculation for lift and drag coefficient for NAC4421 mechy SU2 7 January 9, 2017 06:18
Low Re Flow over S1223 Airfoil devanson FLUENT 7 October 10, 2014 18:36
SU2 AOA optimization 454514566@qq.com SU2 8 July 7, 2014 08:01
Unsteady Flow past circular cylinder-Re=100 (fluctuating drag and lift co-efficients) Vino Main CFD Forum 0 April 10, 2014 10:39
Inviscid Drag at subsonic, subcritical Mach # Axel Rohde Main CFD Forum 1 November 19, 2001 13:19


All times are GMT -4. The time now is 07:10.