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

Setting the Reynolds number

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 28, 2011, 21:40
Default Setting the Reynolds number
  #1
New Member
 
Join Date: Jun 2010
Posts: 24
Rep Power: 6
Echidna is on a distinguished road
I am currently making an analysis of a dual-element wing in CFX.
The problem is that i cannot set my intended Reynolds number so i will have accurate results. I will describe below what exactly i do to see if there is something i am doing wrong.

Re=67778 x speed x length
In my example the length is the chord of the wing which is 0.32m and the speed of the air is 50m/s, so

Re=1.084e6

I leave the operating pressure of the fluid at default (1atm) but then the Reynolds number of the fluid is, according to the solver, 1.34e7.

Could you please help me?
How can i set the Reynolds number of the fluid?
Thanks a lot!
Echidna is offline   Reply With Quote

Old   November 29, 2011, 04:06
Default
  #2
Senior Member
 
Lance
Join Date: Mar 2009
Posts: 491
Rep Power: 10
Lance is on a distinguished road
The Reynolds number that is given in the output from the solver uses a length scale that is (domain volume)^(1/3) and not the cord length.

Does that solve your problem?
Lance is offline   Reply With Quote

Old   November 29, 2011, 06:10
Default
  #3
New Member
 
Join Date: Jun 2010
Posts: 24
Rep Power: 6
Echidna is on a distinguished road
Quote:
Originally Posted by Lance View Post
The Reynolds number that is given in the output from the solver uses a length scale that is (domain volume)^(1/3) and not the cord length.

Does that solve your problem?
Thanks for your reply.
Does this affect the accuracy of my analysis? If yes, how can i solve it?
How can i "tell" the software that the length of interest in my analysis is the chord length and not the cubic root of the whole domain volume?
Echidna is offline   Reply With Quote

Old   November 29, 2011, 07:21
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,131
Rep Power: 79
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The display of Reynolds number in the output file is for the information of the user only. It is not used in the solution at all. Ignore it.
ghorrocks is offline   Reply With Quote

Old   November 29, 2011, 07:30
Default
  #5
New Member
 
Join Date: Jun 2010
Posts: 24
Rep Power: 6
Echidna is on a distinguished road
Quote:
Originally Posted by ghorrocks View Post
The display of Reynolds number in the output file is for the information of the user only. It is not used in the solution at all. Ignore it.
OK thanks!
So, it will be sure that the Reynolds number used by the solver will be the one i need? I set the reference pressure at default (1 atm) and air ideal gas as the fluid.
My solution is low speed (50m/s). Do you think it is correct to set the operating pressure at 1atm? I also set the average static pressure at the outlet at 0 Pa, as is done in WS02:Airfoil tutorial.
Thanks a lot for all the help!

Last edited by Echidna; November 29, 2011 at 07:48.
Echidna is offline   Reply With Quote

Old   November 29, 2011, 17:17
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,131
Rep Power: 79
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
CFX is a dimensional solver, it does not non-dimensionalise the equations so any talk of Reynolds number is purely for the user only. The equations are solved in metres, seconds and kilograms (or any other consistent unit set).

You normally set the reference pressure to be the base pressure (either the inlet or outlet pressure) in a simulation, and use 0 pressure for that boundary. This is good practise.
ghorrocks is offline   Reply With Quote

Old   November 29, 2011, 19:11
Default
  #7
New Member
 
Join Date: Jun 2010
Posts: 24
Rep Power: 6
Echidna is on a distinguished road
So you think that by setting the reference pressure to 1atm is a good practise for my simulation? The fluid velocity is 50m/s. After reading the WS02:Airfoil tutorial, i found out that you will have to calculate the reference pressure of the simulation, but only if there is any compressibility effect. In my analysis, the speed is low, so there is not any compressibility.
Do you think that it's correct to set the reference pressure to 1atm and the average static pressure (relative pressure) on the outlet at 0 Pa?
Echidna is offline   Reply With Quote

Old   November 30, 2011, 05:54
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,131
Rep Power: 79
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
It is a good idea to use a sensible reference pressure regardless of whether the flow is incompressible or compressible. In your case a reference pressure of 1 atm seems sensible.
ghorrocks is offline   Reply With Quote

Old   November 30, 2011, 06:33
Default
  #9
New Member
 
Join Date: Jun 2010
Posts: 24
Rep Power: 6
Echidna is on a distinguished road
Thanks a lot!
Echidna 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
Setting Reynolds number in Fluent for plunging airfoil quarkz FLUENT 1 January 24, 2011 15:02
Low Reynolds Number k-epsilon formulation CFX 10.0 Chris CFX 4 December 8, 2009 00:51
Reynolds Number Matt CFX 0 February 25, 2009 06:40
BlockMeshmergePatchPairs hjasak OpenFOAM Native Meshers: blockMesh 11 August 15, 2008 07:36
Warning 097- AB CD-adapco 6 November 15, 2004 05:41


All times are GMT -4. The time now is 02:07.