Solver message of fluid flowing out of domain

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

 October 2, 2007, 17:52 Solver message of fluid flowing out of domain #1 KM Guest   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. *************************Message************* 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.

 October 3, 2007, 11:45 Re: Solver message of fluid flowing out of domain #2 Wooster Guest   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

 October 3, 2007, 17:07 Re: Solver message of fluid flowing out of domain #3 CycLone Guest   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. -CycLone

 October 4, 2007, 01:58 Re: Solver message of fluid flowing out of domain #4 S. Guest   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.

 October 5, 2007, 15:19 Re: Solver message of fluid flowing out of domain #5 KM Guest   Posts: n/a Hi, 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.

 October 7, 2007, 16:29 Re: Solver message of fluid flowing out of domain #6 Omer Guest   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. Regards.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post acro CFX 15 September 23, 2016 11:16 Saturn CFX 45 February 8, 2016 05:42 windhair CFX 5 September 5, 2013 20:45 bearcat CFX 6 April 28, 2008 14:08 Tuhin Rakshit Main CFD Forum 0 June 16, 2005 10:03

All times are GMT -4. The time now is 02:43.