
[Sponsors] 
Inlet boundary profile: can I prescribe flow angles? 

LinkBack  Thread Tools  Search this Thread  Display Modes 
July 24, 2015, 17:47 
Inlet boundary profile: can I prescribe flow angles?

#1 
New Member
Join Date: Jul 2015
Posts: 13
Rep Power: 10 
Hello,
I want to specify a boundary profile at my domain inlet using my own 2D data for P_total, T_total, swirl angle, pitch angle, k, and omega fields. Each of these fields are nonaxisymmetric. My problem is that CFX does not seem to have a variable for swirl angle or pitch angle. Has anyone encountered this problem before, and does anyone have a solution? Many thanks! 

July 24, 2015, 20:53 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,748
Rep Power: 143 
Swirl angle and pitch angle are just in a different coordinate system. You can define a relevant coordinate system in CFX, or use transformations from existing coordinate systems.


July 26, 2015, 03:17 

#3 
Senior Member
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 241
Rep Power: 13 
Can he describe that by the tabular data ??
__________________
Quick Tips and Tricks, Tutorials FLuent/ CFX (CFD) https://howtooansys.blogspot.com/ 

July 27, 2015, 12:22 

#4  
New Member
Join Date: Jul 2015
Posts: 13
Rep Power: 10 
Quote:
It is not possible to translate coordinate system from just swirl and pitch angles to velocity components u, v, w. To do so would require additional knowledge of the velocity magnitude at each location, which I do not have. I only want to fix the two velocity angles. I am aware that CFX allows userdefined coordinate systems, but this would only help me convert between Cartesian and polar coordinates. This doesn't solve the problem that I have insufficient information to specify a (u,v,w) vector  or equivalently a (v_r, v_theta, v_phi) vector  at each point in my inlet boundary profile. What I think I need is the option to specify only velocity angles, not magnitudes, as an inlet boundary profile. Does anyone know of a way to implement this in CFX, or is it not an option? Thanks for any help. 

July 27, 2015, 14:07 

#5 
Senior Member
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33 
I do not think you need a new option. Since you are familiar with the definition of swirl and pitch angles, you should be able to write the unit velocity vector as function of those. That is,
swirl_angle = F (u_hat, v_hat, w_hat) pitch_angle = G (u_hat, v_hat, w_hat) where V_hat = (u, v, w) / sqrt(u^2 + v^2 + w^2) Or write V_hat as a function of swirl, and pitch. Either way, you then use the flow direction boundary condition options. Notice you can also decompose it on the cylindrical flow direction components as well. It should be an exercise on representing a vector on a different basis, regardless of coordinate frame selected. 

July 28, 2015, 07:33 

#6  
New Member
Join Date: Jul 2015
Posts: 13
Rep Power: 10 
Quote:
This won't work, as I only have swirl and pitch angles, with no information on the velocity magnitudes. By assuming unit vectors, I would be constraining the velocity magnitudes at each point at my inlet to be unity. This is not a constraint I want to make (this is a combustor exit flow entering a HP turbine, after all). There is mathematically no way to convert only pitch and swirl angles into 2D or 3D velocity components, in any coordinate system, without knowledge of the velocity magnitudes. My question is not "how can I convert my pitch and swirl angles into velocity components" but rather "is there way to implement only constraints on the velocity angles, in an inlet boundary profile. 

July 28, 2015, 09:02 

#7 
Senior Member
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33 
Your mileage may vary, but you are saying is incorrect. If you are imposing a total pressure boundary condition, you only need the flow direction and not the velocity profile.
ANSYS CFX provides multiple ways to constrain the flow direction, and having the swirl and pitch angle is just an exercise in math. Swirl and pitch angles are defined as follows: Code:
Swirl angle = atan (Velocity Tangential / Velocity Axial) Pitch angle = atan (Velocity Radial / Velocity Axial) Code:
Velocity Axial = Value of your choice Velocity Tangential = Value of your choice * tan (Swirl Angle) Velocity Radial = Value of your choice * tan (Pitch Angle) In practice, you can verify that ANSYS CFX normalizes any user input flow direction anyways; therefore, you only have to do is Code:
Unit Vector r Component = tan (Pitch Angle) Unit Vector Theta Component = tan (Swirl Angle) Unit Vector Axial Component = 1 

July 31, 2015, 09:08 

#8 
New Member
Join Date: Jul 2015
Posts: 13
Rep Power: 10 
Thanks a lot for your help, Opaque. I've done what you suggested. Will let you know how it goes!
Last edited by turbomax; August 6, 2015 at 11:09. 

August 6, 2015, 11:08 

#9 
New Member
Join Date: Jul 2015
Posts: 13
Rep Power: 10 
Hi Opaque,
Thank you for your help. I was able to implement my velocity direction constraints at my inlet boundary by specifying the unit vector velocity components in cylindrical coordinates just as you suggested. I had previously not realized that ANSYS CFX normalizes user input flow directions, and I didn't want to constrain the velocity magnitude. Problem solved. Thanks a lot! 

August 6, 2015, 15:01 

#10 
Senior Member
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33 
You are most welcome.. Glad it worked.


Tags 
boundary profiles, inlet boundary, pitch angle, swirl angle, velocity profile 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
sliding mesh problem in CFX  Saima  CFX  46  September 11, 2021 07:38 
Wind turbine simulation  Saturn  CFX  58  July 3, 2020 01:13 
mass flow in is not equal to mass flow out  saii  CFX  12  March 19, 2018 05:21 
Strange velocity profile at the inlet for a flow inside a cylindrical pipe  michmich  OpenFOAM Running, Solving & CFD  0  July 2, 2012 03:37 
what the result is negatif pressure at inlet  chong chee nan  FLUENT  0  December 29, 2001 05:13 