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

AOA in CFX

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 3, 2010, 00:12
Default AOA in CFX
  #1
Senior Member
 
Nick
Join Date: Nov 2010
Posts: 120
Rep Power: 6
Nick R is on a distinguished road
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.
Nick R is offline   Reply With Quote

Old   November 3, 2010, 05:36
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,665
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Are you sure your boundaries are far enough away to not be affecting things? That could explain the difference.
ghorrocks is offline   Reply With Quote

Old   November 3, 2010, 05:38
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,665
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   November 3, 2010, 05:56
Default
  #4
Senior Member
 
Nick
Join Date: Nov 2010
Posts: 120
Rep Power: 6
Nick R is on a distinguished road
Thanks. I actually changed my lower and upper rectangular regions into an additional inlet and opening and it seems to have resolved the issue!
Nick R is offline   Reply With Quote

Old   November 3, 2010, 06:04
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,665
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
That'll explain it
ghorrocks is offline   Reply With Quote

Old   May 9, 2011, 05:37
Default
  #6
Member
 
iswadi
Join Date: Feb 2010
Posts: 44
Rep Power: 7
icemaniac178 is on a distinguished road
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.
icemaniac178 is offline   Reply With Quote

Old   May 9, 2011, 05:53
Default
  #7
siw
Senior Member
 
Join Date: Jul 2009
Posts: 443
Rep Power: 13
siw will become famous soon enough
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)
siw is offline   Reply With Quote

Old   May 9, 2011, 10:19
Default
  #8
Senior Member
 
Nick
Join Date: Nov 2010
Posts: 120
Rep Power: 6
Nick R is on a distinguished road
@icemmaniac
In CFX you can choose multiple regions for inlet/outlet etc just highlight them

@Stuart thanks for the reminder.
Nick R is offline   Reply With Quote

Old   May 9, 2011, 21:52
Default
  #9
Member
 
iswadi
Join Date: Feb 2010
Posts: 44
Rep Power: 7
icemaniac178 is on a distinguished road
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?
icemaniac178 is offline   Reply With Quote

Old   May 9, 2011, 22:32
Default
  #10
Senior Member
 
Nick
Join Date: Nov 2010
Posts: 120
Rep Power: 6
Nick R is on a distinguished road
I normally select the left and bottom as inlet, top and right as outlet. Hope that helps.
Nick R is offline   Reply With Quote

Old   May 10, 2011, 02:48
Default
  #11
siw
Senior Member
 
Join Date: Jul 2009
Posts: 443
Rep Power: 13
siw will become famous soon enough
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.
Attached Images
File Type: jpg Boundary Conditions.jpg (31.3 KB, 23 views)
siw is offline   Reply With Quote

Old   May 11, 2011, 22:09
Default
  #12
Member
 
iswadi
Join Date: Feb 2010
Posts: 44
Rep Power: 7
icemaniac178 is on a distinguished road
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 is offline   Reply With Quote

Old   May 16, 2011, 02:44
Default
  #13
Member
 
iswadi
Join Date: Feb 2010
Posts: 44
Rep Power: 7
icemaniac178 is on a distinguished road
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.
icemaniac178 is offline   Reply With Quote

Old   May 16, 2011, 12:46
Default
  #14
siw
Senior Member
 
Join Date: Jul 2009
Posts: 443
Rep Power: 13
siw will become famous soon enough
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.
siw is offline   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
[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 02:20
CFX pressure in Simulations problem nasdak CFX 1 April 14, 2010 13:22
PhD using CFX Rui CFX 9 May 28, 2007 05:59
CFX 4.4 installation problem Pandu Sattvika CFX 1 December 1, 2001 05:07


All times are GMT -4. The time now is 17:42.