
[Sponsors] 
June 3, 2013, 21:27 
Velocity different than Expected

#1 
New Member
AJ Hunter
Join Date: Feb 2013
Posts: 29
Rep Power: 4 
I have just ran a fluid model with a given mass flow rate for water. I did hand calculations and determined that my velocity at a particular point of the setup should be about 57 ft/s. However, CFX gives me a velocity of 107.88 ft/s. Does anyone know why this might happen.
ABOUT THE MODEL: A single pipe comes in and then splits into 25 smaller channels, which then go back into a single pipe of different diameter. The channels are the locations where I calculated the expected velocity. 

June 3, 2013, 22:32 

#2  
Senior Member
Join Date: Dec 2009
Posts: 129
Rep Power: 10 
lots of things come to mind.
residuals? did it converge.... check the mdot in the model at the inflow and outflow? what about in each pipe? without seeing the geometry is the mdot being evenly distributed? If all the pipe centers are in the same plane you can put a plane that goes through the center along the length and plot a contour of the massflow to see the distribution. did your hand calc assume mdot_total/25 cross check the fluid properties, etc., etc. Quote:


June 3, 2013, 23:23 

#3  
New Member
AJ Hunter
Join Date: Feb 2013
Posts: 29
Rep Power: 4 
1) it did converge (1e4 RMS)
2) mdots all make sense (inlet = outlet = pipes) 3) Hand Calc was for velocity and it did ensure that all 25 channels were considered. The mass flow is being evenly distributed based on your advice and looking at the cross sectional view (small variance, but negligible based on geometry). Just had someone double check my hand calculation. They did it completely independently, not just a review of my calc, but a calc of their own and got the exact same values. Quote:


June 4, 2013, 05:55 

#4 
Senior Member
hamed
Join Date: Apr 2009
Posts: 148
Rep Power: 8 
Which turbulent model do you use in your model? I think your model has swirling flow and maybe Ke is not proper. Try changing your turbulent model .by the way some times 10e4 for RMS is not enough .let the solver goes for 10e6 and monitor variation of velocity at the spectating point while solving the problem. Make sure it is converged to a constant value.
And one more thing are you sure about your fluid domain’s mesh quality? Did you use inflated boundary layer near walls? Is the velocity profile fully developed at location? What about your outlet boundary condition?This all would affect your answer 

June 4, 2013, 06:55 

#5  
Senior Member
Join Date: Dec 2009
Posts: 129
Rep Power: 10 
the ke model should get the mass flow correct in the piping system, when setup and run properly.
the thoughts on the convergence are correct. without more information about the model, how it was run, for how long, timestep, etc. we have little to go on. One could converge down to that RMS with an extremely small, inappropriate timestep and the fluid massflow has "moved" a very small amount. how was it initialized? automatic? Are we talking nanoscale pipes are macro size piping? hmasenger provided the best suggestion, setup monitor points in the pipes. Quote:


June 4, 2013, 07:28 

#6 
Senior Member
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11 
As suggested, setup some monitor points, surface monitors, and a volumetric mass imbalance monitor, only their flatness indicates the convergence and not the residual values.
Using realizable turbulence model can be beneficial here, since it is not very diffusive as keps model. This should give you better results. Mesh independence study is a must for any cfd simulation to be perceived as accurate. Have you done that? OJ 

June 4, 2013, 11:03 

#7 
Senior Member
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 508
Rep Power: 11 
How are you monitoring the flow velocity? How are you hand calcing the V?
Are you are handcalcing V_average, (perhaps just doing V=mdot/rho*A or what not)? Is your CFX a monitor point in the flow centerline (or point V somewhere in pipe) or is it a V_average over a plane? If it is centerline V compared to a V_average for handcalc, you need to take into account the V profile. For your numbers, V_average/V_centerline=0.53. For turbulent profile, a fully developed flow, with an assumed power law profile gives the power n=2. This would be appropriate for low Re (Re<10^4). But that could put you in in a laminar region (V_ave/V=0.67). Be regardless, the point is, dont compare V_ave to V_point in CFD. If that is not what you are doing, ignore my post. 

June 4, 2013, 11:47 

#8 
Senior Member
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,134
Rep Power: 19 
Lets keep it simple guys.
How exactly did you reach the conclusion that the velocity at your point of interest should be 57 ft/s? What were the assumptions for your hand calculations? 

June 5, 2013, 05:59 

#9 
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 11,275
Rep Power: 88 
Let's keep it even simpler  there is an FAQ on this: http://www.cfdonline.com/Wiki/Ansys..._inaccurate.3F
Once the thread author has worked their way through the basics in the FAQ then let's start bouncing some ideas around. By the way  if you think the FAQ has missed something then feel free to add it. It is open to anybody to update. 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Plotting Radial Velocity and Tangential Velocity in CFD Post  ashtonJ  CFX  5  July 13, 2015 02:49 
Compiling OpenFOAM13 on AMD64 with OpenSUSE 101  silent_missile  OpenFOAM Installation  5  August 10, 2007 07:31 
Velocity in Porous medium : HELP! HELP! HELP!  Kali Sanjay  Phoenics  0  November 6, 2006 07:10 
Neumann pressure BC and velocity field  Antech  Main CFD Forum  0  April 25, 2006 02:15 
what the result is negatif pressure at inlet  chong chee nan  FLUENT  0  December 29, 2001 06:13 