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

Velocity different than Expected

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

Reply
 
LinkBack Thread Tools Display Modes
Old   June 3, 2013, 21:27
Default Velocity different than Expected
  #1
New Member
 
AJ Hunter
Join Date: Feb 2013
Posts: 29
Rep Power: 4
ajhunte is on a distinguished road
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.
ajhunte is offline   Reply With Quote

Old   June 3, 2013, 22:32
Default
  #2
Senior Member
 
Join Date: Dec 2009
Posts: 129
Rep Power: 10
mjgraf is on a distinguished road
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:
Originally Posted by ajhunte View Post
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.
mjgraf is offline   Reply With Quote

Old   June 3, 2013, 23:23
Default
  #3
New Member
 
AJ Hunter
Join Date: Feb 2013
Posts: 29
Rep Power: 4
ajhunte is on a distinguished road
1) it did converge (1e-4 RMS)
2) m-dots all make sense (inlet = outlet = \sum 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:
Originally Posted by mjgraf View Post
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.
ajhunte is offline   Reply With Quote

Old   June 4, 2013, 05:55
Default
  #4
Senior Member
 
hmasenger's Avatar
 
hamed
Join Date: Apr 2009
Posts: 148
Rep Power: 8
hmasenger is on a distinguished road
Which turbulent model do you use in your model? I think your model has swirling flow and maybe K-e is not proper. Try changing your turbulent model .by the way some times 10e-4 for RMS is not enough .let the solver goes for 10e-6 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
hmasenger is offline   Reply With Quote

Old   June 4, 2013, 06:55
Default
  #5
Senior Member
 
Join Date: Dec 2009
Posts: 129
Rep Power: 10
mjgraf is on a distinguished road
the k-e 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 nano-scale pipes are macro size piping?

hmasenger provided the best suggestion, setup monitor points in the pipes.

Quote:
Originally Posted by hmasenger View Post
Which turbulent model do you use in your model? I think your model has swirling flow and maybe K-e is not proper. Try changing your turbulent model .by the way some times 10e-4 for RMS is not enough .let the solver goes for 10e-6 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 domainís 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
mjgraf is offline   Reply With Quote

Old   June 4, 2013, 07:28
Default
  #6
Senior Member
 
OJ
Join Date: Apr 2012
Location: United Kindom
Posts: 475
Rep Power: 11
oj.bulmer will become famous soon enough
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 k-eps 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
oj.bulmer is offline   Reply With Quote

Old   June 4, 2013, 11:03
Default
  #7
Senior Member
 
Edmund Singer P.E.
Join Date: Aug 2010
Location: Minneapolis, MN
Posts: 494
Rep Power: 11
singer1812 is on a distinguished road
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.
singer1812 is offline   Reply With Quote

Old   June 4, 2013, 11:47
Default
  #8
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,098
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
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?
flotus1 is offline   Reply With Quote

Old   June 5, 2013, 05:59
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,830
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Let's keep it even simpler - there is an FAQ on this: http://www.cfd-online.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.
ghorrocks is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 17:57.