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

Modeling Backflow for a 3D Airfoil (Wing of Finite Span)

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 11, 2009, 11:06
Default Modeling Backflow for a 3D Airfoil (Wing of Finite Span)
  #1
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 10
Josh is on a distinguished road
Hi everyone -

The purpose of my current simulation is to demonstrate the backflow caused by the leading edge of a 3D airfoil. The backflow occurs along the side of the airfoil in the span-wise direction. A velocity profile above the airfoil should look somewhat (very crude drawing) like this:
http://picasaweb.google.com/lh/photo...eat=directlink

After creating my simulation, my velocity profile above the airfoil looks like this:
http://picasaweb.google.com/lh/photo...eat=directlink

Zooming in:
http://picasaweb.google.com/lh/photo...eat=directlink

You can see minor accounts of backflow. After further refinement:
http://picasaweb.google.com/lh/photo...eat=directlink

Zooming in:
http://picasaweb.google.com/lh/photo...eat=directlink

Although backflow is occurring, it is on a very minute scale. Here is a zoomed out picture demonstrating the plane I used to produce the above two pictures (the plane is in the top right corner):
http://picasaweb.google.com/lh/photo...eat=directlink

As shown, the plane, and thus the area of backflow, is tiny. The backflow should be conspicuous. Here are some important characteristics about my geometry, mesh, and setup.

Geometry

NACA 0012 airfoil cut out of 1 m length, 0.5 m width, at a 15 degree angle of attack, from a fluid domain of dimensions 5 m high, 2.5 m wide, and 15 m long:
http://picasaweb.google.com/lh/photo...eat=directlink

Note that the airfoil is split down its center as symmetry will be used later to produce the full geometry:
http://picasaweb.google.com/lh/photo...eat=directlink

Mesh

Default body spacing of 0.2 m:
http://picasaweb.google.com/lh/photo...eat=directlink

Line control along span-wise airfoil edge of 0.0075 m spacing and 0.2 m radius of influence:
http://picasaweb.google.com/lh/photo...eat=directlink

40 layers of inflation with expansion of 1.02, y+ = 1, Re = 1E7, with the airfoil as a boundary. Here is a photo showing the airfoil meshing:
http://picasaweb.google.com/lh/photo...eat=directlink

Setup

http://picasaweb.google.com/lh/photo...eat=directlink

Steady State analysis.

Inlet boundary with axial velocity of 650 m/s to produce a Reynolds number of approximately 1E7. Outlet boundary with 0 Pa relative pressure. No slip airfoil boundary. Symmetry on the lowest z coordinate face. Free slip boundaries elsewhere.

An SST turbulence model was used for this particular run, although the Omega Reynolds Stress model was also used for previous runs (but with very similar results).

An RMS convergence criteria of 1E-5 was used.

________________________________________

Does this simulation seem reasonable? I used the SST turbulence and Omega Reynolds Stress turbulence models because of their good approximations of flow separation and complex effects. Can anyone recommend a better model(s)? Is my Post analysis an effective way to produce qualitative backflow effects?

Here is my CCL file:
http://rapidshare.de/files/48090177/...onCCL.ccl.html

Thanks for any and all help!
Josh is offline   Reply With Quote

Old   August 11, 2009, 14:54
Default
  #2
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 10
Josh is on a distinguished road
I just tried running the simulation with a 5 degree angle of attack (rather than 15) in order to avoid stall effects. Here's the result:

http://picasaweb.google.com/lh/photo...eat=directlink

Clearly, there is no backflow present (or it is so minute that it is negligible).

Any help? Please and thanks.
Josh is offline   Reply With Quote

Old   August 11, 2009, 16:47
Default
  #3
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 10
Josh is on a distinguished road
The solution hasn't been converging, I just realized. I did a quick Solver analysis to guess the issues.

The v-Mom and w-Mom residuals did not converge.

Here are the locations of the maximum residuals:

+--------------------------------------------------------------------+
| Locations of Maximum Residuals |
+--------------------------------------------------------------------+
| Equation | Node # | X | Y | Z |
+--------------------------------------------------------------------+
| U-Mom | 229483 |-9.187E-05 | 8.038E-06 | 5.001E-01 |
| V-Mom | 235721 | 1.195E-03 |-7.901E-03 | 5.001E-01 |
| W-Mom | 83248 | 2.454E-02 |-2.934E-02 | 5.000E-01 |
| P-Mass | 214056 | 3.267E-02 |-2.520E-02 | 5.001E-01 |
| K-TurbKE | 152221 | 6.814E-03 |-1.622E-02 | 2.301E-01 |
| O-TurbFreq | 22473 | 4.634E-02 |-3.962E-02 | 5.000E-01 |
+--------------------------------------------------------------------+

As seen above, most of the maximum residuals are at approximately [0, 0, 0.5], which is the location of the vertex of the airfoil's leading edge:

http://picasaweb.google.com/lh/photo...eat=directlink

Also, the maximum residuals are significantly larger (at least 1E2 x larger) than the RMS residuals, further leading me to believe that the problem is in a local region (i.e. the vertex of the leading edge).

With my current turbulence models (SST or Omega Reynolds Stress), could there be something wrong with my meshing, or am I way off here?
Josh is offline   Reply With Quote

Old   August 11, 2009, 19:12
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Here is some initial comments:
http://www.cfd-online.com/Wiki/Ansys...gence_criteria

To get an accurate simulation you need to ensure your simulation is mesh, timestep and residual converged. If you have not checked the accuracy of these three parameters (or mesh and residual in steady state) then you are just getting random numbers.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   August 12, 2009, 16:02
Default
  #5
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 10
Josh is on a distinguished road
In the link you provided, I have completed most of the steps:

I have read the Help file section on obtaining convergence and have diagnosed my problem based on its suggestions.

I used monitor points to monitor the u-velocity along the span-wise side of the airfoil at different points to see if it was ever negative (indicating backflow), but to no avail.

I used a larger physical timescale by using the residence time as my physical timescale. (I found the residence time by creating a streamline in Post, and used the maximum value from "Time on Streamline 1" in the "Variables" tab as the residence time.) Convergence was still not obtained.

I coarsened my mesh around the airfoil. This allowed convergence to occur, but with less accurate results (and still no backflow is present).

When I suppressed the inflation effects, the solution converged. When I left inflation unsuppressed and suppressed the line control, the solution did not converge. This leads me to believe that inflation could be causing the convergence problems.

The physics are correct - it is a simple simulation - flow through a rectangular domain over a 3D airfoil. Backflow should be seen on the sides. I used a seemingly appropriate turbulence model, so I cannot see what is wrong in that respect.

About the only thing the aforementioned article recommends that I haven't done is run the simulation as transient, but I can't see this as being necessary.

Any further suggestions, comments, or ideas?
Josh is offline   Reply With Quote

Old   August 12, 2009, 23:06
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Hi,

Small backflow regions like this tend to be transient. You may be forced to run transient to resolve them correctly. When you coarsen the mesh you are simply not able to resolve them and it converges much easier.

These small backflows also tend to be very sensitive to freestream turbulence levels, surface roughness, geometric abberations and other details which are difficult to control.

Glenn Horrocks
ghorrocks is offline   Reply With Quote

Old   August 13, 2009, 10:28
Default
  #7
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 10
Josh is on a distinguished road
Thanks for the help, Glenn. I owe you a virtual beer.

I'll try running the simulation as transient and see how it goes.

Josh
Josh is offline   Reply With Quote

Old   August 13, 2009, 15:04
Default
  #8
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 10
Josh is on a distinguished road
I ran the simulation as transient with adaptive time steps. There are no backflow or trailing vortex regions.

Any clues?
Josh is offline   Reply With Quote

Old   August 13, 2009, 18:24
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
The vorticies may take some time to develop. Try using a run which has the vorticies as an initial condition and see if the transient run keeps them going or if they disappear.

Also, I assume you have done all the normal checks on mesh sensitivity, adequate convergence and now you are considering transient simulations timestep size. These all need to be OK for the simulation to be accurate.
ghorrocks is offline   Reply With Quote

Old   August 18, 2009, 11:31
Default
  #10
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 10
Josh is on a distinguished road
I have produced trailing vortexes along the side of the 3D airfoil. Success!

Backflow, however, still remains very small (roughly only 1 mm from the wall) or non-existent, depending on the simulation method.

After trying several different methods (parameterization, various methods of convergence, turbulence modeling, mesh refinement, transient runs, physics checks, etc.) of obtaining significant backflow, none seem to prevail, despite that the various solutions have converged.

I am beginning to suspect that perhaps very little backflow along the side is to be expected.

Thanks for all the help! Any further comments or suggestions are welcome.
Josh is offline   Reply With Quote

Reply

Tags
3d airfoil, backflow, separation, turbulence, wing

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
finite wing Analysis kartikkp FLUENT 1 April 30, 2009 15:15
Modeling of airfoil rotary motion Agni FLUENT 0 November 24, 2008 04:43
Airfoil boundary condition Frank Main CFD Forum 1 April 21, 2008 18:36
airfoil_ finite volumes method Bounecer Main CFD Forum 11 October 17, 2005 11:14
Aircraft wing modeling serhat kilerci FLUENT 0 January 13, 2001 15:51


All times are GMT -4. The time now is 17:07.