CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > FLUENT

Wind tunnel simulation; Varying the angle of attack

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

Like Tree2Likes
  • 1 Post By vinerm
  • 1 Post By vinerm

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 4, 2020, 01:23
Default Wind tunnel simulation; Varying the angle of attack
  #1
Member
 
Dronzer's Avatar
 
Join Date: Apr 2016
Posts: 51
Rep Power: 7
Dronzer is on a distinguished road
Hi,

I hope you all are doing good.
I am trying to simulate the flow through a wind tunnel and measure the aerodynamic force coefficients of an airfoil placed at the test section of the wind tunnel. I need to do this at various angles of attack.
I know that adjusting the flow direction (and keeping the airfoil horizontal) can do it (PFA pic1). But, this does not seem to be the right method for the simulation of the flow through the wind tunnel (PFA pic2), especially at higher angles of attack.
Does anybody know how to adjust the angle of attack in the wind tunnel simulation without remeshing the geometry for each angle of attack?
Do I need an overset mesh for this?
Please let me know. Thanks in advance.
Attached Images
File Type: png pic1.png (9.4 KB, 7 views)
File Type: png pic2.png (8.1 KB, 7 views)
Dronzer is offline   Reply With Quote

Old   May 5, 2020, 09:06
Default Angle of Attack
  #2
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 33
vinerm will become famous soon enough
There are at least three ways to do it. One is with moving mesh, another one with dynamic mesh, and another one with overset.

You can cut the region around the airfoil in a circular shape. You have to define interface between the circular region and the rest of the fluid region of the tunnel. For each angle of attach, you can rotate the mesh of the circular region and then recreate the interface. Rotation has to be done using Moving Mesh. You can define a rotational velocity, doesn't matter what value, and then view the mesh motion for a certain period of time. The period of time must be such that the product of time-period and velocity specified gives you required rotation. Then, disable the mesh motion and run the simulation. Interfaces will reduce the accuracy a little bit. But if you keep interface far away from the airfoil, then it will have very less effect.

Second method is by remeshing but within Fluent. You need triangular mesh (tetrahedral in 3D). This would not require an interface, hence, no compromise on accuracy. Using dynamic mesh, you can rotate the airfoil to required angle.

Third option is overset, similar to the first one.
Dronzer likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   May 6, 2020, 02:33
Thumbs up Thank you!
  #3
Member
 
Dronzer's Avatar
 
Join Date: Apr 2016
Posts: 51
Rep Power: 7
Dronzer is on a distinguished road
Hi,

Thanks for the detailed reply.

I preferred a structured mesh (using ICEM CFD, PFA Pic1) as I thought it would help the calculation. Therefore, I will go for either option 1 or 3.

Can I perform a steady-state simulation for this? (Since I will have to input rotation rate and time)

In any case, I will do a few trials. I hope I can update the thread if I have any other concerns about the simulation.

Thanks again.
Attached Images
File Type: jpg Capture.jpg (194.4 KB, 12 views)
Dronzer is offline   Reply With Quote

Old   May 6, 2020, 04:28
Default AoA
  #4
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 33
vinerm will become famous soon enough
If you want to use structured mesh and variation in AoA is not very large, then I'd suggest method 2. You can use only smoothing option wherein Fluent will not remesh but compress and expand the cells slightly. Since the variation is to be handled by compression and expansion of cells, therefore, variation in AoA should not be very large. How large depends on mesh cell sizes. I suppose within a variation of \pm 10^o, it should work fine.
Dronzer likes this.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Old   May 7, 2020, 02:12
Default
  #5
Member
 
Dronzer's Avatar
 
Join Date: Apr 2016
Posts: 51
Rep Power: 7
Dronzer is on a distinguished road
Quote:
Originally Posted by vinerm View Post
If you want to use structured mesh and variation in AoA is not very large, then I'd suggest method 2. You can use only smoothing option wherein Fluent will not remesh but compress and expand the cells slightly. Since the variation is to be handled by compression and expansion of cells, therefore, variation in AoA should not be very large. How large depends on mesh cell sizes. I suppose within a variation of \pm 10^o, it should work fine.
Thank you. I will look into that too. Appreciate it.
Dronzer is offline   Reply With Quote

Reply

Tags
airfoil, angle of attack, fluent 14.5, remeshing, wind tunnel

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Wind Tunnel Simulation with Rotation Wheel andr3s_diaz STAR-CCM+ 5 May 6, 2018 07:09
Wind tunnel blockage simulation for VAWT urbanzakapa FLUENT 0 March 11, 2016 03:39
[How to obtain supersonic flow inside a supersonic wind tunnel ?] yx213 Siemens 1 September 17, 2014 13:52
wind turbine simulation inside the wind tunnel shaohua FLUENT 4 April 11, 2014 17:01
Wind Tunnel Website now online Mike Worthey Main CFD Forum 0 June 6, 2000 02:27


All times are GMT -4. The time now is 23:27.