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

NACA 2412 simulation in CFX

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 11, 2005, 10:17
Default NACA 2412 simulation in CFX
  #1
andrew
Guest
 
Posts: n/a
I tried to simulate NACA 2412 with CFX. I got acceptable result for Cl for 0 angle of attack (about 0.22), but when I changed AOA to 10 degrees Cl increased only up to about 0.35, while it was supposed to be about 1.2. Does anybody have any idea why?
  Reply With Quote

Old   October 11, 2005, 12:22
Default Re: NACA 2412 simulation in CFX
  #2
Robin
Guest
 
Posts: n/a
There are a number of factors to be aware of. For one, you should always check the influence of things like mesh density, location of boundary conditions, turbulence model etc. When comparing to tunnel data such as this, there are some specific challenges and it helps to know more about the tunnel data.

Separation: the experiment may be assumed to be 2 dimensional. In practice, however, this may not be the case, particularly if separation occurs (which is always a 3 dimensional effect).

Endwall effects: Are your endwalls the same as the wind tunnel's? As the angle of attack increases, there may be more interaction with the top and bottom walls, especially if they are close to the airfoil. How does moving or changing your endwall definition modify your results. Same goes for inlet/outlet locations.

Turbulence model: Is the inlet turbulence intensity and length scale appropriate. Are these conditions known from the experiment. If separation occurs you should use the SST model with an appropriate boundary layer resolution. If the inflow is laminar or the boundary layer relaminarizes at the leading edge, you may want to use the transition feature of SST.

Advection scheme: I assume you're using the default High Res scheme, but if not, try turning this back on.

These are just a few things to consider to improve your analysis.

Best regards, Robin
  Reply With Quote

Old   October 12, 2005, 01:53
Default Re: NACA 2412 simulation in CFX
  #3
andrew
Guest
 
Posts: n/a
Robin, thank you.

The objective of my experiment is to find out the conditions that would give me results similar to what is published for example in The Theory of Wing Section by Abbott. Then I intend to use this conditions for simulating other airfoils.

1. As I have found mesh density did not really affect the result.

2. Boundary conditions is, may be, a feature to play. In fact I placed a wing section about 3ft long and 0.3ft wide into a domain 30ft long, 20ft high and 0.3 wide, 12ft away from the inlet. Change of AOA was simulated by changing the vertical component of the velocity. Do you see anything wrong in the approach?

3. Separation. The side walls of the domain were simulated by Symmetry boundary condition. Therefore I expected to obtain a credible result for 2 dimensional experiment.

4. Endwall effects. When I looked at the velocity streamline I saw that endwall effect was remote enough from the wing section. I noticed no influence of inlet and outlet too.

5. Turbulance model. I tried k-e model for intial setup. Do you think use of SST model could result in higher value of Cl?

6. Advection scheme. Yes, I'm using the default Hight Res scheme.

Best regadrs,

Andrew
  Reply With Quote

Old   October 12, 2005, 08:50
Default Re: NACA 2412 simulation in CFX
  #4
Robin
Guest
 
Posts: n/a
Hi Andrew,

You're set up is appropriate for modelling a 2D airfoil in the free stream. The problem is not so much your model as the experiment itself.

In the lab, the airfoils is not a 2D sections, but has some width and the walls are not infinitely far away. For low angles of attack, this is fine, but as the angle of attack increases the end walls play a part by constraining the flow. Also, if separation does occur in the wind tunnel, the separated flow does not remain 2D.

So the question is not whether you have set up an appropriate domain/bc's for a 2D analysis, but whether you are comparing to the same.

Regards, Robin
  Reply With Quote

Old   October 12, 2005, 09:26
Default Re: NACA 2412 simulation in CFX
  #5
Myron
Guest
 
Posts: n/a
I'm wondering about inlet BC. You'll have the 10-deg at the inlet, but if you have top and bottom walls - won't the velocity start approaching zero AOA at the airfoil? If you take a cross-section just upstream of the airfoil, what does the velocity field look like? Is it still at 10-deg AOA?

What happens if you actually modify the orientation of the airfoil to 10-deg AOA?
  Reply With Quote

Old   October 12, 2005, 10:00
Default Re: NACA 2412 simulation in CFX
  #6
Robin
Guest
 
Posts: n/a
Good point. I was assuming that the top and bottom are either pressure openings with unspecified direction or periodic. If these are walls, you should change it.

-Robin
  Reply With Quote

Old   October 12, 2005, 10:41
Default Re: NACA 2412 simulation in CFX
  #7
andrew
Guest
 
Posts: n/a
Hi Robin and Myron,

Actually I choose free slip option for the top and bottom. And like I said, I noticed no influence upon the wing section while observing velocity streamline for 10 degrees AOA. Although near the wall streamline was distorted. Well, I thought of changing wing section orientation too instead of playing with the velocity components. OK, I'll try it too.

Thank you, guys.

Andrew

  Reply With Quote

Old   October 12, 2005, 13:23
Default Re: NACA 2412 simulation in CFX
  #8
Robin
Guest
 
Posts: n/a
Hi Andrew,

You definitely shouldn't use free slip. At the very least, using a periodic or opening boundary condition will allow you to move the boundary closer and make your mesh smaller. Neither will resolve the issue with comparison to data if your CFD model does not represent the lab setup.

Regards, Robin
  Reply With Quote

Old   October 12, 2005, 14:44
Default Re: NACA 2412 simulation in CFX
  #9
Meri
Guest
 
Posts: n/a
Robin, Why do you say not to use free slip ? Also could you possible explain your comments earlier on the effect of seperation. If Andrew's model was 3d will it make a difference ?
  Reply With Quote

Old   October 12, 2005, 17:03
Default Re: NACA 2412 simulation in CFX
  #10
Robin
Guest
 
Posts: n/a
A free slip condition will force the flow to be parallel to the wall. If you have the flow coming in at an angle at the inlet, it will be turned at the top and bottom boundaries, so the inlet angle will not be preserved. If the boundaries are very far away, it may not matter, but by very far I mean VERY far away. The effect will show up in the static pressure for sure, if not the velocity direction near the airfoil. If you were to rotate the airfoil and keep the inlet velocity in the normal direction, free slip isn't too bad. Still, a pressure opening with unspecified direction (entrainment condition) is better.

Regarding separation, if you only have a 2D model and the flow separates, the flow in the recirculation zone will be planar. In reality this is never the case. The airfoils tested are not two dimensional and if the flow separates, low momentum fluid from the side wall boundary layers will be entrained, adding a 3 dimensional component to the flow. In some cases the walls will have suction to remove boundary layers, but it's still nearly impossible to remove the swirl that develops in the separated zone. Separation is an unsteady, highly three dimensional phenomenon.

If you added the appropriate thickness to the model and enough nodes in the third dimension, you would pick up some of this effect.

Regards, Robin
  Reply With Quote

Old   October 12, 2005, 18:24
Default Re: NACA 2412 simulation in CFX
  #11
Glenn Horrocks
Guest
 
Posts: n/a
Hi Robin,

Some good suggestions here. Because questions on this topic are so common it sounds like adding a "Best practises guide to airfoil modelling" would be a good idea.

Alternately, Jonas has set up the FAQ section of the CFD Online website and it would be good to have some comments on that (http://www.cfd-online.com/Forum/cfx.cgi?read=11926).

Regards, Glenn
  Reply With Quote

Old   October 21, 2005, 09:58
Default Re: NACA 2412 simulation in CFX
  #12
Ramki
Guest
 
Posts: n/a
The top+bottom set to free slip will not produce the desired angle of attack. Instead, set the bottom to inlet flow (with the same conditions as the left side inlet flow), and set the top to outlet flow with the same pressure as the right side outlet flow. This is much easier to model than re-orient the airfoil to have the appropriate angle of attack.

-mvrk
  Reply With Quote

Old   October 24, 2005, 01:46
Default Re: NACA 2412 simulation in CFX
  #13
andrew
Guest
 
Posts: n/a
Thank you, Ramki.

My problem now is that I can not get appropriate separation neither with K-E, nor with SST option. In fact velocity vectors look very similar for both solution - the air flow is just laminar over the entire chord.

Any comments?
  Reply With Quote

Old   October 25, 2005, 00:59
Default Re: NACA 2412 simulation in CFX
  #14
DAK565656
Guest
 
Posts: n/a
You won't be able to see different vectors. It's all about the length of them. You also won't be able to see turbulence. These are just models that count one vector in boundary layer cell instead of thousands of small turbulent vortexes. This one vector contributes the same drag/lift as thousand vortexes.
  Reply With Quote

Old   October 25, 2005, 01:59
Default Re: NACA 2412 simulation in CFX
  #15
andrew
Guest
 
Posts: n/a
Alright. Then how can I judge whether separation occurs or not? Is there any means to see it?

  Reply With Quote

Old   October 25, 2005, 02:16
Default Re: NACA 2412 simulation in CFX
  #16
andrew
Guest
 
Posts: n/a
One more thing, SST method to my knowledge is being positioned as the one that solves separation problem. They used streamlines to demonstrate the separation zone to show how good this approach is comparing to K-E model. In my case velocity streamlines look the same for both K-E and SST models - laminar over the entire surface.

I still can not understand why.
  Reply With Quote

Old   October 26, 2005, 00:19
Default Re: NACA 2412 simulation in CFX
  #17
DAK565656
Guest
 
Posts: n/a
I actually don't know. In my point of view it is impossible to see different streamlines for each model or for separation because of model in first cell near BL. Try to plot streamline in immediate vicinity to surface. Maybe you'll see something... And who are "they" who used to demonstrate separation zone? Do you see sifference between Cp using K-E and SST models?
  Reply With Quote

Old   October 26, 2005, 01:38
Default Re: NACA 2412 simulation in CFX
  #18
andrew
Guest
 
Posts: n/a
Look at http://www.ansys.com/products/cfx/cf...turbulance.asp - The SST Model In ANSYS CFX. The difference in Cp is there, though I can not say at the moment how big it is.
  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
CFX thermo-fluid 2D simulation problems maryliz CFX 6 November 1, 2011 00:26
nucleate boiling simulation in CFX Anil CFX 3 August 25, 2010 14:18
CFX simulation file bank eslam CFX 2 June 15, 2007 07:46
Ansys CFX Vs. NACA Summary Report. Mismatch Result Santiago Orrego. CFX 3 February 5, 2007 13:05
NACA 0012 simulation results Luis FLUENT 3 February 15, 2006 12:42


All times are GMT -4. The time now is 11:45.