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

Inlet boundary profile: can I prescribe flow angles?

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

Like Tree2Likes
  • 1 Post By ghorrocks
  • 1 Post By Opaque

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 24, 2015, 17:47
Default Inlet boundary profile: can I prescribe flow angles?
  #1
New Member
 
Join Date: Jul 2015
Posts: 13
Rep Power: 10
turbomax is on a distinguished road
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!
turbomax is offline   Reply With Quote

Old   July 24, 2015, 20:53
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,748
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
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.
ghorrocks is offline   Reply With Quote

Old   July 26, 2015, 03:17
Default
  #3
Senior Member
 
Martin_Sz's Avatar
 
Marcin
Join Date: May 2014
Location: Poland, Swiebodzin
Posts: 241
Rep Power: 13
Martin_Sz is on a distinguished road
Can he describe that by the tabular data ??
__________________
Quick Tips and Tricks, Tutorials FLuent/ CFX (CFD)
https://howtooansys.blogspot.com/
Martin_Sz is offline   Reply With Quote

Old   July 27, 2015, 12:22
Default
  #4
New Member
 
Join Date: Jul 2015
Posts: 13
Rep Power: 10
turbomax is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
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.
turbomax is offline   Reply With Quote

Old   July 27, 2015, 14:07
Default
  #5
Senior Member
 
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33
Opaque will become famous soon enough
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.
Opaque is offline   Reply With Quote

Old   July 28, 2015, 07:33
Default
  #6
New Member
 
Join Date: Jul 2015
Posts: 13
Rep Power: 10
turbomax is on a distinguished road
Quote:
Originally Posted by Opaque View Post
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.
turbomax is offline   Reply With Quote

Old   July 28, 2015, 09:02
Default
  #7
Senior Member
 
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33
Opaque will become famous soon enough
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.
Opaque is offline   Reply With Quote

Old   July 31, 2015, 09:08
Default
  #8
New Member
 
Join Date: Jul 2015
Posts: 13
Rep Power: 10
turbomax is on a distinguished road
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.
turbomax is offline   Reply With Quote

Old   August 6, 2015, 11:08
Default
  #9
New Member
 
Join Date: Jul 2015
Posts: 13
Rep Power: 10
turbomax is on a distinguished road
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!
turbomax is offline   Reply With Quote

Old   August 6, 2015, 15:01
Default
  #10
Senior Member
 
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33
Opaque will become famous soon enough
You are most welcome.. Glad it worked.
Opaque is offline   Reply With Quote

Reply

Tags
boundary profiles, inlet boundary, pitch angle, swirl angle, velocity profile

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
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


All times are GMT -4. The time now is 22:05.