CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > CFX

Solver message of fluid flowing out of domain

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

LinkBack Thread Tools Search this Thread Display Modes
Old   October 2, 2007, 17:52
Default Solver message of fluid flowing out of domain
Posts: n/a
Hi there,

Sometimes I get the following message during my simulations. A few times it used to disappear with iterations but now it keeps coming with every iteration.

Will it affect my results? How can I get rid of it? Thanks a ton in advance !!!!

Best Regards, Kushagra Mittal.


A wall has been placed at portion(s) of an INLET boundary condition (at 40.4% of the faces, 40.4% of the area) to prevent fluid from flowing out of the domain. The boundary condition name is: inlet. The fluid name is: Water. If this situation persists, consider switching to an Opening type boundary condition instead.

  Reply With Quote

Old   October 3, 2007, 11:45
Default Re: Solver message of fluid flowing out of domain
Posts: n/a
I frequently get this for my outlet if there is turbulence nearby. Basically, there is a turbulence eddy that is being calculated at that boundary. Now, you've specified that water should be either going in or out at that boundary, but the calculation is saying that there are parts where this is not the case. CFX in this case will erect a temporary 'wall' that will prevent the fluid from going in the opposite direction from the one you specified. This is in the CFX manual so take a look in it to see if I've got the story 100%

The fix: If you have some kind of cylindrical geometry, then stretch it out to get away from areas of high turbulence. Basically, make sure that your in/out boundaries are far from high turbulence. -W
  Reply With Quote

Old   October 3, 2007, 17:07
Default Re: Solver message of fluid flowing out of domain
Posts: n/a
It isn't actually turbulence that is the problem, but rather recirculation. Moving your outlet or specifying it as an opening can help. Often the warning will only occur during part of the run, so if it goes away don't worry about it.

  Reply With Quote

Old   October 4, 2007, 01:58
Default Re: Solver message of fluid flowing out of domain
Posts: n/a
Whenever I get this error, I either move the boundary or specify an opening. Usually specifying the boundary as an opening works well when appropriate.
  Reply With Quote

Old   October 5, 2007, 15:19
Default Re: Solver message of fluid flowing out of domain
Posts: n/a

Thanks a lot to everyone for their reply. It Helps!

In my case, this message appears till the last iteration ! My solution converges, but it ends with the above mentioned message. Now I am wondering whether the converged results would be affected because of that message or not? Are they still considerable results?

As this message appears for the inlet boundary and the inlet pipe (rectangular) joins a cylindrical pipe at its cylindrical surface, I have not been creating OR meshing the rectangular pipe but taking its projection on the cylindrical face so that meshing complexities could be avoided in the joining area.

Thanks a ton !

Regards, KM.

  Reply With Quote

Old   October 7, 2007, 16:29
Default Re: Solver message of fluid flowing out of domain
Posts: n/a
Just wanted to add this to the the discussion. You cannot specify an Opening at the Inlet. Then it would mean what it means, it is an opening and not an Inlet.

You have a recirculation issue. Looks like you are modeling a Pipe junction of Rectangular and Circular Cross Section. It might be accurate but that's debateable.Because it's obvious that you will have flow seperations , recirculations , secondary flows at the juntion.

Only way to really find out, is by moving your inlet far away. Try to atleast free-mesh for the rectangular conduit, just as a test run, with considerable inlet distance upstream of the junction itself. I don't think it would be acceptable to have an rectangular inlet right at the junction which exhibits complex flow nature.

  Reply With Quote


Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
Wind turbine simulation Saturn CFX 58 July 3, 2020 01:13
Interface between fluid domain and porous domain windhair CFX 6 May 10, 2018 14:26
Can CFX do CHT simulations with a solid domain rotating in a stationary fluid domain? acro CFX 15 September 23, 2016 11:16
why the solver reject it? Anyone with experience? bearcat CFX 6 April 28, 2008 14:08
interfacing a fluid solver with abaqus Tuhin Rakshit Main CFD Forum 0 June 16, 2005 10:03

All times are GMT -4. The time now is 23:44.