Inlet boundary profile: can I prescribe flow angles?

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

 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 non-axisymmetric. 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. anon_h likes this.

 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:
 Originally Posted by ghorrocks 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.
Hi Ghorrocks,

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 user-defined 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:
 Originally Posted by Opaque 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.
Hi Opaque,

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)``` Therefore, the velocity profile can be defined as 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)``` However, because you do NOT need the velocity profile, but the flow direction, you normalize (only if you want), and there is no need for the "value of your choice", and the flow direction vector is the made of the expression above divided by the magnitude. 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``` Hope I did not make any mistakes above.. No need for a new boundary condition. chongbazh likes this.

 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.