Calculation of Reynolds Number In CFX

ashtonJ · January 18, 2011, 03:38

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

Lance · January 18, 2011, 03:49

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

rskrishna87 · January 25, 2011, 06:12

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.

Lance · January 25, 2011, 06:13

Have you tried areaAve(Velocity)@inlet ?

rskrishna87 · January 25, 2011, 06:35

yup...Its showing 150.659 which is more higher

rskrishna87 · January 25, 2011, 07:00

Does anyone know how to calculate Reynolds number manually in CFD-Post using an expression??

ghorrocks · January 25, 2011, 17:05

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.

mdshirazi · November 9, 2013, 06:50

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?

ghorrocks · November 9, 2013, 07:21

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.

mdshirazi · November 9, 2013, 08:31

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?

ghorrocks · November 10, 2013, 05:30

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.

nimap · July 17, 2015, 04:56

Quote:

Originally Posted by ghorrocks

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?

ghorrocks · July 17, 2015, 07:32

Any CFD textbook can define you how to get the hydraulic diameter. Then it is usually straight forward to implement it in CFD-Post.

January 18, 2011, 03:38	Calculation of Reynolds Number In CFX	#1
ashtonJ Senior Member Ashkan Javadzadegan Join Date: Sep 2010 Posts: 255 Rep Power: 17	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

January 18, 2011, 03:49		#2
Lance Senior Member Lance Join Date: Mar 2009 Posts: 669 Rep Power: 22	CFX use Volume^(1/3) to calculate the length scale, that why you dont get the same Reynolds number. From your data: ((0.02^2pi/4)(5.4e-1-2e-2))^(1/3)10602e-2/3.7e-3 = 313 Ethan_Sparkle and mukhtar like this.

January 25, 2011, 06:12	mean Velocity at Inlet	#3
rskrishna87 Member Join Date: Jan 2011 Posts: 37 Rep Power: 15	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.

January 25, 2011, 17:05		#7
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	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, bayramuks and aero_head like this.

November 9, 2013, 06:50		#8
mdshirazi New Member shirazi Join Date: Dec 2012 Posts: 2 Rep Power: 0	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? bayramuks likes this.

January 25, 2011, 06:13		#4
Lance Senior Member Lance Join Date: Mar 2009 Posts: 669 Rep Power: 22	Have you tried areaAve(Velocity)@inlet ?

January 25, 2011, 06:35		#5
rskrishna87 Member Join Date: Jan 2011 Posts: 37 Rep Power: 15	yup...Its showing 150.659 which is more higher

January 25, 2011, 07:00		#6
rskrishna87 Member Join Date: Jan 2011 Posts: 37 Rep Power: 15	Does anyone know how to calculate Reynolds number manually in CFD-Post using an expression??

November 9, 2013, 07:21		#9
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	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. Abhi.shek and bayramuks like this.

November 9, 2013, 08:31		#10
mdshirazi New Member shirazi Join Date: Dec 2012 Posts: 2 Rep Power: 0	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?

November 10, 2013, 05:30		#11
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	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.

July 17, 2015, 07:32		#13
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,871 Rep Power: 144	Any CFD textbook can define you how to get the hydraulic diameter. Then it is usually straight forward to implement it in CFD-Post.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[snappyHexMesh] SnappyHexMesh for internal Flow	vishwa	OpenFOAM Meshing & Mesh Conversion	24	June 27, 2016 09:54
air bubble is disappear increasing time using vof	xujjun	CFX	9	June 9, 2009 08:59
Reynolds Number Again	Ogbeni	CFX	2	June 3, 2005 00:34
Reynolds number in CFX	tuks	CFX	0	May 25, 2005 02:16
Low Reynolds number K-Omega modeling	Athar Zaidi	Main CFD Forum	0	October 31, 1999 14:59