CFD Online Discussion Forums

CFD Online Discussion Forums (
-   CFX (
-   -   AOA in CFX (

Nick R November 3, 2010 00:12

Hi everyone,

I'm trying to simulate flow past a 3d airfoil. I've used two different methods

1) Keeping the airfoil horizontal and changing the incoming freestream velocity according to AOA ( U cos AOA, U sin AOA)

2) Changing the AOA of the airfoil and setting the incoming flow parallel to the horizon

The problem is I get completely different results in Cf (LIFT coefficient) and flow pattern is different too. I am wondering if I'm doing something wrong. The second method yields better results but that means having to mesh the geometry several times for various AOAs and creating a new geometry also. Some help would be excellent.
This is a turbulent simulation BTW.

ghorrocks November 3, 2010 05:36

Are you sure your boundaries are far enough away to not be affecting things? That could explain the difference.

ghorrocks November 3, 2010 05:38

Oh yes, and another way of doing it is to put the airfoil in a cylindrical region joined to the rest of the flow with a GGI. Then you can easily rotate the cylinder to any AOA but keep the far field the same.... If that is important.

Nick R November 3, 2010 05:56

Thanks. I actually changed my lower and upper rectangular regions into an additional inlet and opening and it seems to have resolved the issue!

ghorrocks November 3, 2010 06:04

That'll explain it :)

icemaniac178 May 9, 2011 05:37

Dear Mr Nick R,
can you or anybody explain to me how do we changed our upper and lower rectangular region into an 'additional inlet and opening'. i have the same problem with u, mr nick.

siw May 9, 2011 05:53

It might be a bit late now but make sure you are not getting confused between the fresstream aligned lift and drag coefficients and the vehicle aligned normal and axial force coefficients which are only the same at AoA=0deg:

CL = CN*cos(AoA) - CA*sin(AoA)
CD = CN*sin(AoA) + CA*cos(AoA)

Nick R May 9, 2011 10:19

In CFX you can choose multiple regions for inlet/outlet etc just highlight them

@Stuart thanks for the reminder.

icemaniac178 May 9, 2011 21:52

mr nick,
i know that we can select multiple region for inlet/outlet.Do you mean if we have a box shape domain, we have to select front, upper and lower face to be also define as inlet? can u explain to me the correct selection of BC for a box shape domain?

Nick R May 9, 2011 22:32

I normally select the left and bottom as inlet, top and right as outlet. Hope that helps.

siw May 10, 2011 02:48

1 Attachment(s)
When I did a set of simulations of an aircraft at different angles of attack I made a hemipsherical domain considerabley larger that the aircraft so that the domain boundaries would not be influenced by the aircraft being there. The image shows what I used and I set the upstream half of the hemisphere to an inlet (blue) and the downstream half to an outlet (green). This way I did not have to think about side boundaries that you get if the domain is a box. So for each angle of attack I just changed the inlet velocity components. I then had to convert the CFD-Post force_x and force_z to CL and CD using the equations in my other post. My results matched well with other results on the same aircraft at the same conditions.

However, there is one small problem with this. At the higher AoA there is a small amount of inflow on the outlet at the top of the domain. But the domain was large enough that I did not have an influence on the aircraft.

icemaniac178 May 11, 2011 22:09

thanks nick and siw,
it was really help me. i have managed to get the idea and implemented in my model.
i got a good results

icemaniac178 May 16, 2011 02:44

mr stuart,
do you have any publications or reference regarding on your domain type? i consider it most helpful for me and the others if there is reference about the this type of domain.

siw May 16, 2011 12:46

For a reference use the popular vaildation case, which is what my simulations are of, at:

and read the various presentations:

Notice, that none are given using CFX. Which is one reason I'm doing mine.

For example, the Fluent simulations used the FARFIELD boundary condition on the entire hemisphere face. Of course, CFX is different to Fluent and so that is why I had to split the hemispherical face into 2 pieces for an INLET and OUTLET.

All times are GMT -4. The time now is 15:07.