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

problem : "reversed flow in 77 faces on outflow 12."

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

Like Tree3Likes
  • 2 Post By -mAx-
  • 1 Post By -mAx-

Reply
 
LinkBack Thread Tools Display Modes
Old   June 23, 2009, 16:32
Default problem : "reversed flow in 77 faces on outflow 12."
  #1
New Member
 
Mohammad Ali Amini
Join Date: Jun 2009
Posts: 8
Rep Power: 8
aliamini is on a distinguished road
Hi
It's my first post in this Forum.
I try to solve a problem in fluent. The problem is a steady state water flow in a chamber with one inlet and one outlet. The radius of this chamber is ten times bigger than inlet and outlet parts. of course inlet of this chamber has some intricacies that causes difficulties.
after different kinds of methods and initial conditions and checking the geometry this warning is still showing.
warning :

"reversed flow in 77 faces on outflow 12.
turbulent viscosity limited to viscosity ratio of 1.000000e+005 in 138423 cells."


This is very interesting that in all conditions and iterations, finally I reach to a constant numbers in the error text. that are 77 faces on outflow and 138423 cells limited viscosity ratio. and after about 50 iterations these numbers remain constant even after 1000 iterations.
Thank you for your help.
aliamini is offline   Reply With Quote

Old   June 24, 2009, 01:43
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,973
Rep Power: 30
-mAx- will become famous soon enough
switch outflow with pressure-outlet
*reversed flow indicates that you have an vertex at your outlet
*turbulent viscosity warning is basicaly a problem of turbulence setting and/or mesh issue (skewness)
mr_mxd and fanke like this.
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   June 24, 2009, 08:06
Default
  #3
New Member
 
Mohammad Ali Amini
Join Date: Jun 2009
Posts: 8
Rep Power: 8
aliamini is on a distinguished road
But naturally the vortex should not happen.
I examined your suggestion about pressure outlet but warnings is still showing with larger numbers of faces involve.
after 1000 iterations with these warnings I checked the contour plot of pressure and velocity. I don't know why a big part of my domain in the middle of chamber don't have any contour value and remained dark.( inlet and outlet of domain have contour values.)
I don't know what it means and what should I do to convergence.
thanks a lot for your answers.
aliamini is offline   Reply With Quote

Old   June 25, 2009, 00:55
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,973
Rep Power: 30
-mAx- will become famous soon enough
Warnings can occure at the begining of the computation, as the solution isn't converged.
The number of cells involved in the warning may decrease and the warning should disappear.
Post a picture of the contour, you described...
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   June 25, 2009, 05:09
Default
  #5
New Member
 
Mohammad Ali Amini
Join Date: Jun 2009
Posts: 8
Rep Power: 8
aliamini is on a distinguished road
http://xs540.xs.to/xs540/09264/velocity_contour734.jpg
http://xs540.xs.to/xs540/09264/pressure_contour246.jpg

These are velocity and pressure contours.
inlet is in the bottom and outlet is in the top.
As you see the big fraction of both contours are empty.
and afetr some iterations it seems that the condition of converging doesn't change and all the residuals and faces that have reverse flow remain constant.
aliamini is offline   Reply With Quote

Old   June 25, 2009, 07:53
Default
  #6
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,973
Rep Power: 30
-mAx- will become famous soon enough
create planes in your domain (sweep / surface)
and check if you still have this phenomenon.
Check also the mass conservation between inlet and outlet (report/fluxes/mass-flow-rate)
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   June 25, 2009, 12:22
Default
  #7
New Member
 
Mohammad Ali Amini
Join Date: Jun 2009
Posts: 8
Rep Power: 8
aliamini is on a distinguished road
I checked sweep planes but the problem has remained.
a big part of domain doesn't have value in contour plot.
mass flow rate is OK.
further I found that I had forgotten to scale my domain to millimeter.
after this correction the problem of limited viscosity ratio solved and my solution converged. but the problem of reversed flow remained unsolved and when I checked the sweep planes and contour plots, a big big part of my domain remains dark and without any value
what does it mean?
even after conversion I have many faces with reverse flow and a big part of my domain doesn't have any value.
aliamini is offline   Reply With Quote

Old   June 25, 2009, 12:49
Default
  #8
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,973
Rep Power: 30
-mAx- will become famous soon enough
Is your model well meshed inside?
If you create a plane in the middle of your domain, can you see cells where you get no data?
If you create path lines from inlet, do you have lines where you get no data?
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   June 25, 2009, 16:55
Default
  #9
New Member
 
Mohammad Ali Amini
Join Date: Jun 2009
Posts: 8
Rep Power: 8
aliamini is on a distinguished road
http://xs.to/xs.php?h=xs940&d=09264&...elocity450.jpg
http://xs.to/xs.php?h=xs940&d=09264&...ressure744.jpg
http://xs.to/xs.php?h=xs940&d=09264&f=path_line914.jpg

These are the pictures that you suggest.
unfortunately I think I have many cells that have no data.
I think this solution thinks that it doesn't need to fill the chamber.
but I think in experiment surely in steady state condition, chamber must be full of water.
aliamini is offline   Reply With Quote

Old   June 26, 2009, 00:36
Default
  #10
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,973
Rep Power: 30
-mAx- will become famous soon enough
pathlines seem to be ok.
The warning about reversed flow is link with your short outlet. You may extend it.
Check you mesh (in Gambit?) if the region in the middle is connected with the other region
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   June 26, 2009, 03:29
Default
  #11
New Member
 
Mohammad Ali Amini
Join Date: Jun 2009
Posts: 8
Rep Power: 8
aliamini is on a distinguished road
How can I check the connection of my mesh in gambit?
In the Gambit,first I meshed some faces and then meshed my volume.
In Fluent I checked it and understood that I have grids in all part of volume. but about connection I don't know how can I check it.
aliamini is offline   Reply With Quote

Old   June 26, 2009, 04:01
Default
  #12
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,973
Rep Power: 30
-mAx- will become famous soon enough
if you only have one volume, then you don't have any connection's problem
Else in gambit, click on the icon with the magnifying glass. The interface between connected volumes should be pink
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   June 26, 2009, 15:02
Default
  #13
New Member
 
Mohammad Ali Amini
Join Date: Jun 2009
Posts: 8
Rep Power: 8
aliamini is on a distinguished road
I have only one volume so what's the problem about cells that don't have any data?
Maybe in the solution their velocity should be zero. on the other hand actually they are motionless and don't influence the solution.
What do you think?
aliamini is offline   Reply With Quote

Old   June 26, 2009, 16:41
Default
  #14
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,973
Rep Power: 30
-mAx- will become famous soon enough
re-plot the contour of velocity, disable the autoscale option.
Set the min to 0 and the max to 1m/s
Enable the "filled" option.
et re-post the pictures.
It should show the low velocity distribution in the middle of your domain.
You may adjust the max velocity in the scale, to capture the distribution.
If you see an discontinuity, then you have a problem.
If not, then it should be ok (but I don't know anything from what you want to compute)
shaker likes this.
__________________
In memory of my friend Hervé: CFD engineer & freerider

Last edited by -mAx-; June 26, 2009 at 16:54. Reason: complement
-mAx- is offline   Reply With Quote

Old   June 27, 2009, 02:57
Default
  #15
New Member
 
Mohammad Ali Amini
Join Date: Jun 2009
Posts: 8
Rep Power: 8
aliamini is on a distinguished road
http://xs.to/xs.php?h=xs840&d=09266&..._scaled257.jpg

Hi
your thought was true. This model doesn't have any problem. only the scale of contour causes this misunderstanding. My goal is velocity profile in outlet and I wanted to be sure that my model is physically realistic.
Thanks a lot for your answers.
aliamini is offline   Reply With Quote

Old   February 6, 2014, 15:06
Default
  #16
Senior Member
 
Ke Wu
Join Date: Jan 2012
Posts: 179
Rep Power: 5
itsme_kit is on a distinguished road
Quote:
Originally Posted by -mAx- View Post
re-plot the contour of velocity, disable the autoscale option.
Set the min to 0 and the max to 1m/s
Enable the "filled" option.
et re-post the pictures.
It should show the low velocity distribution in the middle of your domain.
You may adjust the max velocity in the scale, to capture the distribution.
If you see an discontinuity, then you have a problem.
If not, then it should be ok (but I don't know anything from what you want to compute)
hi

I experienced the problem as to 'turbulent viscosity limited to viscosity ratio' and temperature limit

I'm modelling air flow around a 3D building in addition with solar load model

I have a solid base to be treated as soil

The bottom of soil is set to a constant temperature as a heat sink

However, I couldn't understand why the temperature of side wall of soil has reached the temperature limit

It doesn't make sense

Can you help me a little bit?

Thanks
itsme_kit 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
Stability Problem with sonicFoam for Nozzle Flow Julian K. OpenFOAM 2 June 29, 2009 19:46
3D Fluid Flow Convergence problem Emily FLUENT 2 March 21, 2007 23:18
good cold flow results but problem with hot flow Rams FLUENT 0 June 20, 2006 00:52
Periodic flow boundary condition problem sudha FLUENT 3 April 28, 2004 08:40
Inviscid Drag at subsonic, subcritical Mach # Axel Rohde Main CFD Forum 1 November 19, 2001 13:19


All times are GMT -4. The time now is 14:41.