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

Problems modelling developed flow on inlet

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   May 25, 2014, 15:27
Exclamation Problems modelling developed flow on inlet
  #1
New Member
 
James
Join Date: May 2012
Posts: 11
Rep Power: 14
Allankey is on a distinguished road
Hi, I am trying to model a non uniform boundary condition at the inlet to represent fully developed laminar flow using CEL; but I am getting some strange results. I am following the methodology here:

http://www.arc.vt.edu/ansys_help/cfx...DefiCrea5.html


However, in my case the inlet is on the YZ plane, not in the XY plane in the example. I just noticed in the last sentence it says

"In this equation, x and y are defined as directions 1 and 2 (X and Y for Cartesian coordinate frames) respectively, in the selected reference coordinate frame."

Do you think I have a problem with referencing the coordinate where the radius is measured from?

I have attached an image of the resulting velocity across the inlet. As you can see it is not what I was aiming for i.e. fastest velocity in the center and 0 velocity at the wall.

Does anyone have any idea why this is happening or know of an alternative approach I can use to solve this problem?

Thanks in advance!
Attached Images
File Type: jpg Boundary Problem.jpg (36.7 KB, 7 views)

Last edited by Allankey; May 25, 2014 at 16:54. Reason: Clarity
Allankey is offline   Reply With Quote

Old   May 25, 2014, 18:38
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,749
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
For this approach to work you need to have the origin at the centre of the inlet boundary, and in the XY plane. If this is not the case you will need to account for the different origin location.
Allankey likes this.
ghorrocks is offline   Reply With Quote

Old   May 25, 2014, 18:44
Default
  #3
Senior Member
 
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33
Opaque will become famous soon enough
Definitely, there is a problem with the use of the "r" CEL variable in your setup. As explained in the tutorial you pointed out, "r" refers to the radius measures about the Z axis. In your setup, the proper axis for you expression is X, and the radius must be computed accordingly.

Alternatives:

1 - Create your own radius variable. For example, Myr = sqrt(y^2 + z^2).. Assuming the inlet of interest is centered respect to the coordinate frame; otherwise, adjust for the location of the coordinate frame respect to the inlet, i.e. sqrt( (y - y_o)^2 + (z - z_o)^2 )

2 - Change the option from Cartesian Components to Cylindrical Components, set Tangential, and Radial components to 0, and use your expression using Radius instead of "r" for you Axial component. Do not forget to set "x" for you Axis Definition. NOTE: Radius depends on the Axis Definition, while "r" is always about "z" axis.

3 - Create a new coordinate frame centered on the inlet with "local z" aligned with "global x". Now "r" is about the "local z" and it should work as you expect.

Hope the above helps,
Allankey likes this.
Opaque is offline   Reply With Quote

Old   May 25, 2014, 18:52
Default
  #4
New Member
 
James
Join Date: May 2012
Posts: 11
Rep Power: 14
Allankey is on a distinguished road
Quote:
1 - Create your own radius variable. For example, Myr = sqrt(y^2 + z^2).. Assuming the inlet of interest is centered respect to the coordinate frame; otherwise, adjust for the location of the coordinate frame respect to the inlet, i.e. sqrt( (y - y_o)^2 + (z - z_o)^2 )

Thank you both so much for your replies, that makes a lot more sense now! Will give it a try.

Thanks again
Allankey is offline   Reply With Quote

Reply

Tags
boundary condition u, cfx, laminar

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
Fully developed flow at inlet ? sezenempire FLUENT 0 March 27, 2012 05:37
Fully Developed Flow in Star-cd SMM STAR-CD 0 September 5, 2011 22:08
How to specify an inlet boundary conditions for a fully developed gas flow in a duct. legendyxg FLUENT 2 May 11, 2010 07:32
ATTENTION! Reliability problems in CFX 5.7 Joseph CFX 14 April 20, 2010 15:45
Problems modeling subsonic engine air inlet with flow separation TWaung CFX 2 March 29, 2009 18:42


All times are GMT -4. The time now is 03:41.