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

reversed flow in xxxx faces on pressure outlet

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

Like Tree1Likes
  • 1 Post By Trev

Reply
 
LinkBack Thread Tools Display Modes
Old   June 23, 2009, 10:42
Default reversed flow in xxxx faces on pressure outlet
  #1
New Member
 
Franz Roman
Join Date: Jun 2009
Posts: 25
Rep Power: 8
franzdrs is on a distinguished road
Hi all,
I have a small question: during iterations I get the warning message "reversed flow in xxxx faces on pressure outlet". The number xxxx goes down with iterations. then the solution converges and there are still about 1000 faces in the outlet with reversed flow. If I continue the iterations the number keeps falling, and probably it will reach zero (no more warnings). What does this mean? Is the solution not really converged when FLUENT says so
(according to the default residuals criteria)? IS the solution converged when finally there are no more faces with reversed flow or when this number stays constant?
thanks
franzdrs is offline   Reply With Quote

Old   June 24, 2009, 01:33
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 2,992
Rep Power: 30
-mAx- will become famous soon enough
you have an vertex at the outlet.
It can slow the convergence, but it's harmless
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   June 24, 2009, 05:21
Default
  #3
Member
 
Neil
Join Date: Jun 2009
Location: The Moon
Posts: 42
Rep Power: 8
Trev is on a distinguished road
It also depends on what you are actually modelling aswell where reversed flow may physically occur. Such as in the modelling of hydrocyclones where the reversed flow message is desirable. If this isn't the case the messages will eventually subside but if they don't you could also try extending the boundaries where reversed flow occurs or reduce the back pressure on the outlet to suck the flow out of the domain.
Trev is offline   Reply With Quote

Old   June 24, 2009, 06:00
Default
  #4
New Member
 
Franz Roman
Join Date: Jun 2009
Posts: 25
Rep Power: 8
franzdrs is on a distinguished road
Hi, thanks for the answers. Trev, I am modeling a dryer for agricultural products. It is a pretty simple system. Yes, there could be a reversed flow if the bed of product does not make much resistance to the flow. In my case, this resistance could or could not be small enough to create reversed flow. I model the bed of product as porous media. If I disable the porous media region then I get reversed flow for sure. The problem is that the reversed flow starts happening at the beginning of the iterations at a high number of face elements of the outlet, it grows even more, and then it starts to drop. When the solution converges (when the residuals reach all 0.001) there are still around 1000 face elements with reversed flow. If I continue iterating after this convergence, the faces with reversed flow keep dropping and reaches finally 0. My guess is, that if the number of face elements with reversed flow stabilizes at some point before reaching 0, then that would be what is physically happening, but if the message eventually subsides, then the physical situation is without reversed flow. Am I right? Could somebody tell me? Thanks.
franzdrs is offline   Reply With Quote

Old   June 24, 2009, 10:51
Default
  #5
Member
 
Neil
Join Date: Jun 2009
Location: The Moon
Posts: 42
Rep Power: 8
Trev is on a distinguished road
If the number of faces with reversed flow keeps decreasing it is unlikely that the physical problem would exhibit much if any reversed flow. As a rule of thumb convergence isn't achieved until your residuals have flattened out and the mass flux is negligible. The standard 10-3 convergence limits fluent automatically imposes are not really sufficient for most cases so try iterating further till 10-4 or lower and put a surface monitor on the outlet for mass flow rate. Keep iterating till the mass flow rate has flattened out and the mass flux error is around 10-6. Then you can see if reversed flow is still occuring in which case it is likely to occur physically as the solution can be considered converged.
harsh_999 likes this.
Trev is offline   Reply With Quote

Old   October 18, 2010, 11:56
Default
  #6
Senior Member
 
maysmech's Avatar
 
Join Date: Jan 2010
Posts: 347
Blog Entries: 2
Rep Power: 8
maysmech is on a distinguished road
Hello,



Please tell me the solution of this problem. i mean, how can we revise the problem to remove this error?
maysmech is offline   Reply With Quote

Old   March 19, 2014, 04:16
Default Reverse flow on faces
  #7
New Member
 
Aalisha
Join Date: Jan 2014
Posts: 18
Rep Power: 3
aalisha is on a distinguished road
Hello, I am also facing the similar problem. I am working on a 3 blade tidal turbine and doing the calculations for the drag force on blades. It has a velocity inlet and pressure outlet. However, on every single iteration it shows a message saying that "reversed flow on XXXX faces on pressure outlet 11. The XXXX numbers first decreases and then increases again keep flowing this increase decrease thing. If any one can explain me what is the physical significance of this.

I mean what impact it will have on the turbine working. The results starts converging after 60 iterations.
aalisha 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
Outlet pressure for compressible flow Michelle CFX 12 September 1, 2015 18:38
Neumann pressure BC and velocity field Antech Main CFD Forum 0 April 25, 2006 02:15
pressure outlet BC for incompressible flow khaiching Main CFD Forum 6 October 15, 2005 02:58
what the result is negatif pressure at inlet chong chee nan FLUENT 0 December 29, 2001 06:13
Hydrostatic pressure in 2-phase flow modeling (CFX4.2) HB &DS CFX 0 January 9, 2000 14:19


All times are GMT -4. The time now is 17:32.