
[Sponsors] 
May 25, 2014, 16:27 
Problems modelling developed flow on inlet

#1 
New Member
James
Join Date: May 2012
Posts: 11
Rep Power: 13 
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! Last edited by Allankey; May 25, 2014 at 17:54. Reason: Clarity 

May 25, 2014, 19:38 

#2 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,573
Rep Power: 141 
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.


May 25, 2014, 19:44 

#3 
Senior Member
Join Date: Jun 2009
Posts: 1,744
Rep Power: 30 
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, 

May 25, 2014, 19:52 

#4  
New Member
James
Join Date: May 2012
Posts: 11
Rep Power: 13 
Quote:
Thank you both so much for your replies, that makes a lot more sense now! Will give it a try. Thanks again 

Tags 
boundary condition u, cfx, laminar 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Fully developed flow at inlet ?  sezenempire  FLUENT  0  March 27, 2012 06:37 
Fully Developed Flow in Starcd  SMM  STARCD  0  September 5, 2011 23:08 
How to specify an inlet boundary conditions for a fully developed gas flow in a duct.  legendyxg  FLUENT  2  May 11, 2010 08:32 
ATTENTION! Reliability problems in CFX 5.7  Joseph  CFX  14  April 20, 2010 16:45 
Problems modeling subsonic engine air inlet with flow separation  TWaung  CFX  2  March 29, 2009 19:42 