CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

water inject tube, huge different results by icoFoam and Fluent

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 29, 2015, 17:52
Default water inject tube, huge different results by icoFoam and Fluent
  #1
New Member
 
CA
Join Date: Jul 2015
Posts: 2
Rep Power: 0
cchuran is on a distinguished road
Hi all, I am a beginner to use openfoam. A simple case: water injection into 2D tube, x*y=2*0.4. But the velocity distribution is huge different when use openFOAM and Fluent. Why?

The icoFoam and Fluent were both used to simulate the steady-state process. The BCs are:

openFOAM
left: fixed velocity 0.05 m/s, zeroGrident for p
right: zeroGrident for U, fixed 0 for p
upDown: fixed (0,0,0) for U, zeroGrident for p
frontback: empty

fluent
left: velocity-inlet 0.05 m/s, zeroGrident for p
right: pressure-outlet, fixed for pressure
upDown: wall, no-slip

Attached is the comparisons of the openFOAM and Fluent results. Thanks!
Attached Images
File Type: jpg fluent.jpg (13.0 KB, 25 views)
File Type: jpg icoFoam.jpg (16.1 KB, 25 views)
File Type: jpg model.jpg (16.6 KB, 23 views)
File Type: jpg Capture.jpg (35.3 KB, 26 views)
Attached Files
File Type: zip boxtest.zip (4.8 KB, 2 views)

Last edited by cchuran; July 29, 2015 at 21:19.
cchuran is offline   Reply With Quote

Old   July 30, 2015, 05:05
Default
  #2
New Member
 
Lukasz
Join Date: Apr 2012
Posts: 8
Rep Power: 6
loook is on a distinguished road
Hi cchuran

what did you set for the turbulence in both cases? it seems that in openFoam you have laminar flow while in fluent the profile looks like turbulent.
loook is offline   Reply With Quote

Old   July 30, 2015, 13:21
Default
  #3
New Member
 
CA
Join Date: Jul 2015
Posts: 2
Rep Power: 0
cchuran is on a distinguished road
Thanks for your reply. The fluent also uses laminar model (the same as openFOAM)
cchuran is offline   Reply With Quote

Old   July 31, 2015, 06:27
Default kinematic viscosity of 0.01
  #4
Senior Member
 
Fabian Roesler
Join Date: Mar 2009
Location: Germany
Posts: 210
Rep Power: 10
fabian_roesler is on a distinguished road
Have a look into the transportProperties inside constant folder.
The kinematic viscosity of 0.01 is ten thousand times larger than the one of water 1.004e-6. This gives you a perfect parabolic profile even withing this large diameter tube.

Cheers

Fabian
fabian_roesler is offline   Reply With Quote

Old   July 31, 2015, 08:30
Default
  #5
Senior Member
 
Join Date: Jan 2014
Posts: 105
Rep Power: 4
hxaxtma is on a distinguished road
It looks like that you are simulating different Reynoldsnumbers and in assumption that you set the velocity (0,05 m/s) and the viscosity (water=1.04e-06) for both Fluent and OF, there is one left, the scaling of your geometry!

Please, verify that your case in fluent AND in OpenFOAM is set up in meters.

If you want to simulate laminar pipe flow, the critical Reynoldsnumber should be

Re_crit=u*d/<2320

P.S.:
your OF simulation looks for laminar pipe flow right, cause the peak velocity of the parabolic profile should be around 2*u_in = 2*0,05=0,1m/s
hxaxtma is offline   Reply With Quote

Old   August 3, 2015, 08:05
Default
  #6
Senior Member
 
Join Date: Jan 2014
Posts: 105
Rep Power: 4
hxaxtma is on a distinguished road
you fixed your problem?
hxaxtma 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
Curious results in icoFoam differ from fluent hemph OpenFOAM Running, Solving & CFD 6 December 16, 2005 15:27


All times are GMT -4. The time now is 22:51.