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?

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

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

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

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?

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

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

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

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 ?

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

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

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

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?

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.

Alright. Then how can I judge whether separation occurs or not? Is there any means to see it?

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.

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?

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.