Wing Tip Vortices
 

Hi guys,
I'm trying to simulate a wind tunnel test with a NACA0012 airfoil at a 10 deg angle of attack and I'm trying to see the wing tip vortices generated.

I have meshed with ICEM and imported into FLUENT where I ran a transient solution using a Reynolds Stress Model. The resulting velocity contours are shown below.

As you can see, I can't really make anything out. Does anybody know how I should go about postprocessing so that I can get a nice picture or animation of the vortices. I also need to know the rough size of the vortices generated.

Any help greatly appreciated,
Thanks.


Wing Front
http://www.cfd-online.com/Forums/att...1&d=1288533631

Wing Back
http://www.cfd-online.com/Forums/att...1&d=1288533631

Wing Side
http://www.cfd-online.com/Forums/att...1&d=1288533631

If you are looking for the vortices, you should not be looking at the velocity to be seeing these. The crudest way to visually see the trailing vortices would be to plot isosurfaces of vorticity magnitude. You can then plot this at several different levels to find an idea of the strengths and locations of the vortices. There are also more advanced ways of viewing the vortex cores such as the Q-criterion and the Lambda-2 criterion. Each of these are available in CFD-Post.

Is there a reason that you are running in transient? The trailing vortices will be present in a steady state run. I would first recommend a SS simulation so you understand the strengths and location of vortices. Then, only if needed, would I conduct a transient run.

Keep in mind the artificial dissipation. Artificial dissipation of the numerical schemes result in trailing vorticies that are overly dissipated. To reduce this keep a fine mesh in the region of the trailing vortex. Many modeling techniques are done to ensure this vortex is not overly dissipated. These techniques include moving Chimera grid schemes and alternative discretization schemes like Vorticity Confinement. I would recommend you investigate these techniques to understand the difficulty in modeling trailing vorticies.

rotating cylinder..
 

hello friends,
i m trying to simulate the flow over the naca 4424 airfoil with the leading edge replaced with the rotating cylinder... i just gave rotation to the cylinder by giving rotating wall option. by selecting the center of the cylinder as the orgin of the rotation. expe[IMG]file:///C:/DOCUME%7E1/AEROSR%7E1/LOCALS%7E1/Temp/moz-screenshot.png[/IMG]cted results are not coming...here i ve attached the picture of the mesh. pls help me friendz...

rotating cylinder..
 

hello friends,
i m trying to simulate the flow over the naca 4424 airfoil with the leading edge replaced with the rotating cylinder... i just gave rotation to the cylinder by giving rotating wall option. by selecting the center of the cylinder as the orgin of the rotation. expected results are not coming...here i ve attached the picture of the mesh. pls help me friendz...

Hi Nick, thanks for your reply, there's certainly some valuable information there especially about the artificial dissipation which I had no idea about.

The reason I ran a transient analysis was that I was looking for some animation of the vortices. I did however run a SS analysis first and after reading your post I plotted the vorticity magnitude on some iso-surfaces at various chord lengths downstream. The images that I got do indeed seem (to me at least!) to suggest that the vortices are over-dissipated.

How is it possible to implement some of these techniques to reduce the artificial dissipation in FLUENT?

Thanks again for your reply and you have definitely put me on the right track (I think!).

The vorticity plotted on iso-surfaces from the trailing edge up to 8 chord lengths downstream:

http://www.cfd-online.com/Forums/att...1&d=1288706917

dfitz-

Those plots are perfect in displaying the wing tip. And, yes it does appear that the vortex is being artificially dissipated. The simplest solutions is to make sure that you are running the solver at the higher-order possible. This means changing the advection and turbulence schemes from first-order to second-order. The next step would be to increase the mesh in the area downstream of the wing tip vortex (what mesher are you using?).

Basically that becomes the limitation of the solver. All solvers are going to have this phenomenon whether it is Fluent, CFX, Star, etc. It is an inherent nature of the discreatization (truncation error). If you want to get further into more complex methods, send me a private message and we can talk offline.

Nick

method
 

if u got the wingtip vortices can you tell me the procedure u used to find it!
i tried it with k epsilon model and when i plot the streamlines i just get the flow above it but not the vortices.

It's fairly simple but the problem is that there are too many differing opinions on the definition of a vortex.

But check out vortex identification critieria (Q-criterion, lambda-2, and stretched swirling strength method are popular).

vortex
 

hello, to get the vortices should we subtract the wing from the enclosure?
also... what model should we consider to do the analysis in fluent?
laminar or k-epsilon?

and.. i am a beginner so can u tell me how to plot a iso surface?

Hi, I m new member on cfd online. Can anyone explain me the method to plot vortex magnitude on iso surfaces? I m using CFD post. I m new to cfd and I need help completing my project. Thank you.