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, 06:37

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, 06:53

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, 11:19

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

@Stuart thanks for the reminder.

icemaniac178 · May 9, 2011, 22:52

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, 23:32

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

siw · May 10, 2011, 03:48

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, 23:09

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, 03:44

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, 13:46

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

http://aaac.larc.nasa.gov/tsab/cfdlarc/aiaa-dpw/

and read the various presentations:

http://aaac.larc.nasa.gov/tsab/cfdla...sentations.htm

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.

November 3, 2010, 00:12	AOA in CFX	#1
Nick R Senior Member Nick Join Date: Nov 2010 Posts: 126 Rep Power: 16	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.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[ICEM] Proper way to name boundaries on 2D model for use in CFX?	RossFS	ANSYS Meshing & Geometry	4	November 10, 2011 03:38
Pros and Cons for CFX, CFdesign, COMSOL	Val	Main CFD Forum	3	June 10, 2011 03:20
CFX pressure in Simulations problem	nasdak	CFX	1	April 14, 2010 14:22
PhD using CFX	Rui	CFX	9	May 28, 2007 06:59
CFX 4.4 installation problem	Pandu Sattvika	CFX	1	December 1, 2001 05:07

November 3, 2010, 05:36		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,844 Rep Power: 144	Are you sure your boundaries are far enough away to not be affecting things? That could explain the difference.

November 3, 2010, 05:38		#3
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,844 Rep Power: 144	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.

November 3, 2010, 05:56		#4
Nick R Senior Member Nick Join Date: Nov 2010 Posts: 126 Rep Power: 16	Thanks. I actually changed my lower and upper rectangular regions into an additional inlet and opening and it seems to have resolved the issue!

November 3, 2010, 06:04		#5
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,844 Rep Power: 144	That'll explain it

May 9, 2011, 06:37		#6
icemaniac178 Member iswadi Join Date: Feb 2010 Posts: 44 Rep Power: 16	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.

May 9, 2011, 06:53		#7
siw Senior Member Stuart Join Date: Jul 2009 Location: Portsmouth, England Posts: 739 Rep Power: 26	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 = CNcos(AoA) - CAsin(AoA) CD = CNsin(AoA) + CAcos(AoA)

May 9, 2011, 11:19		#8
Nick R Senior Member Nick Join Date: Nov 2010 Posts: 126 Rep Power: 16	@icemmaniac In CFX you can choose multiple regions for inlet/outlet etc just highlight them @Stuart thanks for the reminder.

May 9, 2011, 22:52		#9
icemaniac178 Member iswadi Join Date: Feb 2010 Posts: 44 Rep Power: 16	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?

May 9, 2011, 23:32		#10
Nick R Senior Member Nick Join Date: Nov 2010 Posts: 126 Rep Power: 16	I normally select the left and bottom as inlet, top and right as outlet. Hope that helps.

May 11, 2011, 23:09		#12
icemaniac178 Member iswadi Join Date: Feb 2010 Posts: 44 Rep Power: 16	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

May 16, 2011, 03:44		#13
icemaniac178 Member iswadi Join Date: Feb 2010 Posts: 44 Rep Power: 16	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.

May 16, 2011, 13:46		#14
siw Senior Member Stuart Join Date: Jul 2009 Location: Portsmouth, England Posts: 739 Rep Power: 26	For a reference use the popular vaildation case, which is what my simulations are of, at: http://aaac.larc.nasa.gov/tsab/cfdlarc/aiaa-dpw/ and read the various presentations: http://aaac.larc.nasa.gov/tsab/cfdla...sentations.htm 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.