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

Calculation of Reynolds Number In CFX

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

Like Tree2Likes
  • 1 Post By ghorrocks
  • 1 Post By ghorrocks

Reply
 
LinkBack Thread Tools Display Modes
Old   January 18, 2011, 03:38
Question Calculation of Reynolds Number In CFX
  #1
Senior Member
 
Ashkan Javadzadegan
Join Date: Sep 2010
Posts: 234
Rep Power: 7
ashtonJ is on a distinguished road
Hi all

I simulated a steady flow in a pipe. Mean velocity at inlet of pipe is 0.02 [m/s]. The pipe diameter is 20 [mm]. The following data has been taken from CFX solver output file.

Global Length = 5.4614E-02
Minimum Extent = 1.9994E-02
Maximum Extent = 5.4000E-01
Density = 1.0600E+03
Dynamic Viscosity = 3.7100E-03
Velocity = 2.0012E-02
Advection Time = 2.7290E+00
Reynolds Number = 3.1227E+02

When I calculate the Reynolds number with above information. It becomes 114 while as it shown above, CFX calculated 312 for Reynolds number. Does anybody know how CFX calculated the Reynolds Number?


regards
Ashtonj
ashtonJ is offline   Reply With Quote

Old   January 18, 2011, 03:49
Default
  #2
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 522
Rep Power: 11
Lance is on a distinguished road
CFX use Volume^(1/3) to calculate the length scale, that why you dont get the same Reynolds number.

From your data:
((0.02^2*pi/4)*(5.4e-1-2e-2))^(1/3)*1060*2e-2/3.7e-3 = 313
Lance is offline   Reply With Quote

Old   January 25, 2011, 06:12
Default mean Velocity at Inlet
  #3
Member
 
Join Date: Jan 2011
Posts: 37
Rep Power: 6
rskrishna87 is on a distinguished road
Hi,


In my output file the Velocity is shown to be 70 but if i caluculate it in CFD -Post as ave(Velocity)@Inlet then it is much higher than that.It is 129.Can anyone please tell me what is the problem.I want to know this to calculate Reynolds number manualy in CFD-Post.

Last edited by rskrishna87; January 25, 2011 at 06:37.
rskrishna87 is offline   Reply With Quote

Old   January 25, 2011, 06:13
Default
  #4
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 522
Rep Power: 11
Lance is on a distinguished road
Have you tried areaAve(Velocity)@inlet ?
Lance is offline   Reply With Quote

Old   January 25, 2011, 06:35
Unhappy
  #5
Member
 
Join Date: Jan 2011
Posts: 37
Rep Power: 6
rskrishna87 is on a distinguished road
yup...Its showing 150.659 which is more higher
rskrishna87 is offline   Reply With Quote

Old   January 25, 2011, 07:00
Default
  #6
Member
 
Join Date: Jan 2011
Posts: 37
Rep Power: 6
rskrishna87 is on a distinguished road
Does anyone know how to calculate Reynolds number manually in CFD-Post using an expression??
rskrishna87 is offline   Reply With Quote

Old   January 25, 2011, 17:05
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,814
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If you want to calculate the Reynolds number you are comparing against literature values, you need to use the same definition of Reynolds Number.

These are my guesses:
Velocity scale = areaAve(Velocity)@inlet
Length scale = the diameter of the cylinder or chord length or whatever the geometry is
density scale = areaAve(Density)@inlet
Viscosity scale = areaAve(Viscosity)@inlet

Then you can define Re number using these numbers.
nimap likes this.
ghorrocks is offline   Reply With Quote

Old   November 9, 2013, 06:50
Default
  #8
New Member
 
shirazi
Join Date: Dec 2012
Posts: 2
Rep Power: 0
mdshirazi is on a distinguished road
Dear Ashton,
I am aware that it is a long time since you have posted here,but I need a help .I cannot find Reynolds number in CFX outputs in CFD post. I normally calculate Reynolds number by hand. As you have mentioned here; there is way how to get Reynolds number from cfx itself. Could you give me some information in this field?
mdshirazi is offline   Reply With Quote

Old   November 9, 2013, 07:21
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,814
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Write a CEL expression which calculates it and send it to a monitor point. Easy.

But don't be fooled by the Reynolds Number reported in the output file.
ghorrocks is offline   Reply With Quote

Old   November 9, 2013, 08:31
Default
  #10
New Member
 
shirazi
Join Date: Dec 2012
Posts: 2
Rep Power: 0
mdshirazi is on a distinguished road
Dear Glenn,
Thanks for your replay, The problem is that different part of a problem have different length scale. Are you suggesting that there is a built-in length scale function in CFX?
mdshirazi is offline   Reply With Quote

Old   November 10, 2013, 05:30
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,814
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
There is some built in functions. The turbulence transition model has some functions in the Gamma-theta model. There is the wall distance function for the SST turbulence model.

But usually you have to write your own function appropriate for your geometry.
mdshirazi likes this.
ghorrocks is offline   Reply With Quote

Old   July 17, 2015, 03:56
Default
  #12
New Member
 
nima
Join Date: Jul 2014
Posts: 9
Rep Power: 3
nimap is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
If you want to calculate the Reynolds number you are comparing against literature values, you need to use the same definition of Reynolds Number.

These are my guesses:
Velocity scale = areaAve(Velocity)@inlet
Length scale = the diameter of the cylinder or chord length or whatever the geometry is
density scale = areaAve(Density)@inlet
Viscosity scale = areaAve(Viscosity)@inlet

Then you can define Re number using these numbers.
What if the shape of geometry be so complicated, how can gain hydraulic diameter by CFD-post?
nimap is offline   Reply With Quote

Old   July 17, 2015, 06:32
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,814
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Any CFD textbook can define you how to get the hydraulic diameter. Then it is usually straight forward to implement it in CFD-Post.
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
SnappyHexMesh for internal Flow vishwa OpenFOAM Native Meshers: snappyHexMesh and Others 23 August 6, 2014 03:50
air bubble is disappear increasing time using vof xujjun CFX 9 June 9, 2009 07:59
Reynolds Number Again Ogbeni CFX 2 June 2, 2005 23:34
Reynolds number in CFX tuks CFX 0 May 25, 2005 01:16
Low Reynolds number K-Omega modeling Athar Zaidi Main CFD Forum 0 October 31, 1999 14:59


All times are GMT -4. The time now is 22:11.