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

attack angle in CFX

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 26, 2008, 10:20
Default attack angle in CFX
  #1
anne
Guest
 
Posts: n/a
we all know that there are tow ways to consider attack angle in CFX simulation:

method 1: rotate geometry and remesh

method 2: modify inlet velocity components, as well as in intialization conditions.

however, in my case (I tried both of them), only method 2 works. method 1 can be run, but after I finish the running, i can't get all of the results (only part of them), i.e. i can't save the results correctly.

it doesn't make any sense, does it?

do your guys have any comments on it? a new bug? or i did sth wrong?

any comments are welcome

many thanks

anne
  Reply With Quote

Old   November 27, 2008, 10:15
Default Re: attack angle in CFX
  #2
CycLone
Guest
 
Posts: n/a
Method 1 will work if you have done the geometry steps properly. Make sure you are rotating only the part of interest (presumably an airfoil or aircraft?) and if you did some kind of enclosure operation or boolean to create the fluid volume, you need to insert the rotation ahead of this operation, otherwise the fluid region will be unaffected.

There are a few other alternatives:

3. Rotate the geometry within CFX using the moving mesh capability. If you do this, you'll need to solve the mesh motion equations, so you may want to do a few iterations to move the geometry then restart with mesh motion turned off.

4. Place your body within a cylindrical or spherical domain and rotate the grid surrounding the body by using a mesh transformation in CFX-Pre.

5. Place you body with a cylindrical or spherical domain and apply a "frozen rotor" interface between the domains. The frozen rotor interface is only available if you have rotating frames of reference, but you can still use it for stationary domains. If you apply it, make sure the axis of rotation is aligned with the axis of your sphere or cylinder. The Frozen Rotor interface allows you to specify a clocking angle, which is normally used to examine the effect of grid alignment between rotors and stators. Rather than rotating the grid, the solver will offset the "virtual" alignment of faces at the interface, but the effect is the same.

6. Use the grid motion as in 2, but apply it to a cylindrical or spherical domain.

The advantage to doing this at the solver level is that you can write a CEL expression to clock the angle to achieve the desired CL on the fly.

-CycLone
  Reply With Quote

Old   November 28, 2008, 08:50
Default Re: attack angle in CFX
  #3
anne
Guest
 
Posts: n/a
thanks, cyclone.

however, what about if I only rotate the geometry, and then modify the mesh a little (the mesh around the body is a cylindrical mesh), like reprojet some points, etc in order to make sure the mesh quality is still good. is that OK? actually that's what I have done, running can be started, but I can't save the results correctly. what do you think about this?

many thanks

  Reply With Quote

Old   November 28, 2008, 12:11
Default Re: attack angle in CFX
  #4
CycLone
Guest
 
Posts: n/a
Where are you rotating it? In what application and how?
  Reply With Quote

Old   December 2, 2008, 07:42
Default Re: attack angle in CFX
  #5
anne
Guest
 
Posts: n/a
it's nacelle application, let's assume flow direction is x-axis, so I rotate it along y or z and make it incline an angle with x-axis, which is the attack angle or side angle.

so what do you think

  Reply With Quote

Old   December 2, 2008, 11:13
Default Re: attack angle in CFX
  #6
CycLone
Guest
 
Posts: n/a
Are you only rotating the nacelle?
  Reply With Quote

Old   December 4, 2008, 10:55
Default Re: attack angle in CFX
  #7
anne
Guest
 
Posts: n/a
yes, then remesh around the nacelle.
  Reply With Quote

Old   December 5, 2008, 00:12
Default Re: attack angle in CFX
  #8
CycLone
Guest
 
Posts: n/a
Why would you remesh around the nacelle only?
  Reply With Quote

Old   December 12, 2008, 13:00
Default Re: attack angle in CFX
  #9
anne
Guest
 
Posts: n/a
because there is o-grid around nacelle. outside o-grid there is no big change because of the small attack angle
  Reply With Quote

Old   December 16, 2008, 21:33
Default Re: attack angle in CFX
  #10
CycLone
Guest
 
Posts: n/a
How's the grid quality? Why just remesh locally?
  Reply With Quote

Old   December 17, 2008, 14:31
Default Re: attack angle in CFX
  #11
anne
Guest
 
Posts: n/a
mesh quality is good, above 0.35, and it is a structured mesh, no need to change the far field area, anyway, many thanks for your points
  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
Getting lift force at zero angle of attack Shamoon Jamshed FLUENT 15 September 4, 2012 23:16
when the angle of attack =?, the total lift coefficient begin to decrease suddenly liujmljm Main CFD Forum 6 August 3, 2012 05:46
[ICEM] Angle of Attack wolvi_ak ANSYS Meshing & Geometry 8 August 5, 2011 09:31
how to plot attack angle along with impeller span direction at leading edge wildli FLUENT 0 August 31, 2010 14:47
Angle measurement in CFX sham CFX 0 September 2, 2006 00:26


All times are GMT -4. The time now is 16:25.