
[Sponsors] 
July 14, 2012, 09:12 
Problem with time average tangential velocity in swirl flow.

#1 
New Member
Join Date: Oct 2010
Posts: 20
Rep Power: 8 
I'm working on the swirl flow and I'm not able to get desired time average tangential velocity. My inlet velocity is 10 m/s and I was expecting tangential velocity to be around 19 m/s (since tangential velocity is 1.7 to 2.5 times the inlet velocity) but I'm getting 11.5 m/s only. In swirl flow velocity is not independent and is coupled to pressure, thus simply time averaging the tangential velocity (as given in FLUENT) is not giving good results, although the nature of tangential velocity is fine. All I need to have is the xvelocity "vx" , the yvelocity "vy" and the zvelocity "vz" . The mean zvelocity "vz" is same as the mean axial velocity "vaxial" . The mean tangential velocity "vθ" is to be obtained using Fluent custom field function:
vθ = vx cos θ + vy sin θ where "vx" is the time averaged xvelocity, "vy" is the time averaged yvelocity and "θ" is the angular coordinate. Now when I open Fluent custom field function, nowhere i can find "θ". The above expression tells that the coordinate system used is the Cartesian coordinate system because tangential velocity vθ is expressed in terms of vx and vy. But how to express this "θ". Do I have to write a UDF for this? If yes, how. Suggestions will be appreciated. 

July 14, 2012, 13:38 

#2 
Senior Member

cos (theta) = x/r = x / sqrt(x^2 + y^2)
sin (theta) = y/r = y / sqrt(x^2 + y^2) where theta is measured counterclockwise with respect to the positive x axis. In this case the formula for v_theta becomes (the one you wrote is for v_r): v_theta = (x * Vy  y * Vx) / sqrt(x^2 + y^2) where Vx and Vy are the velocity components along the x and y directions. While for v_r you get: v_r = (x * Vx + y * Vy) / sqrt(x^2 + y^2) Now it's up to you to substitute the correct velocity components and cell center coordinates in a custom field functions (still, i suggest using an UDF to control possible singularities on the axis). By the way, the statistics on unsteady flows (in general, not only Fluent) are just a postprocessing step. The coupling between pressure and tangential velocity has nothing to do with the correct postprocessing or computation. 

July 15, 2012, 01:13 

#3 
New Member
Join Date: Oct 2010
Posts: 20
Rep Power: 8 
Thanks sbaffini
I got it n I'll be trying it soon. I still have one question! Is the tangential velocity calculation made by fluent (one of its default option for velocities) different from the one given in your expression? 

July 16, 2012, 17:45 

#4 
Senior Member

I don't know this but certainly, if you agree with me on the derivation, it can't be different. What i'm sure of is that the tangential velocity is just a postprocessing quantity and not a solved one (except for 2D axysimmetric flows or some rotating frames... but that's another story)


July 16, 2012, 23:00 

#5 
New Member
Join Date: Oct 2010
Posts: 20
Rep Power: 8 
Thanx sbaffini for your reply. Yea you are right. Even fluent uses the same expression for the tangential velocity, which I've confirmed with the one given by you, and the results are the same.
sbaffini, I've one more question. What is the procedure for time averaging of any parameter in the simulation. Shall I start averaging right from the beginning of the simulation or when the simulation is about to converge and let it run for some extra time? I'm following the former one with extra run time. 

July 18, 2012, 16:28 

#6 
Senior Member

Forget the CFD case. If you had to make some averages of some quantity varying in time... would you wait for it first reaching a statistically steady state? I think you know the answer (which, just in case, is to wait until the statistically steady state is reached before averaging)


Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
High Courant Number @ icoFoam  Artex85  OpenFOAM Running, Solving & CFD  11  February 16, 2017 14:40 
Problem with FloatingObject  Leech  OpenFOAM Running, Solving & CFD  10  March 29, 2012 15:24 
convergence problem when use pisoFoam, LES for wind tunnel case  Forrest_Lei  OpenFOAM  3  July 19, 2011 06:00 
SimpleFoam k and epsilon bounded  nedved  OpenFOAM Running, Solving & CFD  1  November 25, 2008 21:21 
Variables Definition in CFX Solver 5.6  R P  CFX  2  October 26, 2004 02:13 