# Outlet boundary condition

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

 March 6, 2010, 01:39 Outlet boundary condition #1 New Member   Join Date: Jun 2009 Posts: 9 Rep Power: 9 I am modelling a multiphase flow using a rectangular box. The solid inlet is on the top and gas inlet at the side.My outlet is the other side. I specified my gas inlet boundary as inlet and the normal speed. The solid inlet is based on th fluid dependent. For the outlet boundary, i specified the boundary condition as outlet and the static pressure is zero. By doing this, the turbulence energy of the air was diverging and this resulted into domain instability. I need advise on how to resolve this problem and what outlet boundary condition is the best to use

 March 6, 2010, 05:35 #2 Member   Venkat Join Date: Nov 2009 Posts: 35 Rep Power: 8 Hi, Though i'm not an expert in CFX, i could tell you something about boundary conditions which i learnt from FLUENT presentation. But i worked in Multiphase flows using STAR CCM+. Pressure inlet / Presure outlet conditions normally leads to high fluctuations in Turbulence Kinetic energy and mass and momentum. Mass flow rate inlet / static pressure outlet is more robust than pressure inlet/outlet condition. Fluctuations would be minimal. I hope meshing wouldn't be an issue as you have a rectangular box model. Try refining the BCs. I hope this helps you.

 March 6, 2010, 05:41 #3 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 12,638 Rep Power: 98 Can you describe what you are modelling a bit more? Do you need to model the air on top of the liquid? If you use a degassing boundary at the liquid surface then you won't have to model the air and your turbulence problem disappears. But whether this is appropriate depends on what you are actually trying to model.

 March 8, 2010, 01:17 #4 New Member   Join Date: Jun 2009 Posts: 9 Rep Power: 9 I am modelling gas-solid interaction with the solid inlet at top of a rectangular box while the gas inlet is the side of the box. As advised, I changed the gas inlet to bulk mass flowrate with the volume fraction for air to be 1 and volume fraction for solid to be zero at the gas inlet. I maintained the outlet as outlet boundary condition but mass and momentum was modelled as static pressure. I got the notice below at each time steps but the solution didn't diverge. I don't understand what this means. ****** Notice ****** | | A wall has been placed at portion(s) of an OUTLET | | boundary condition (at 70.0% of the faces, 70.1% of the area) | | to prevent fluid from flowing into the domain. | | The boundary condition name is: Outlet. | | The fluid name is: Sand. | | If this situation persists, consider switching | | to an Opening type boundary condition instead.

 March 8, 2010, 04:10 #5 Member   Venkat Join Date: Nov 2009 Posts: 35 Rep Power: 8 Warning message alerts you about the outgoing flow re entering into the domain through outlet. CFX tries to close the portion of outlet face by covering the percentage of face with wall so that no re entry happens. Opening boundary condition enables the flow to interact with the atmosphere in which flow conditions at the outlet is almost exposed to atmospheric pressure and temperature. I could see that 70% face coverage with wall is higher. Face coverage upto 25 % is acceptable as suggested by CFX support engineer. Try refining the physical timescale. How is the convergence trend ? Do you see high fluctuations in the residuals ? Even i'm working on the convergence criteria as i stii didn't get smooth curve as expected. Always check the .out file for converged solution. Check whether solver has completed the run based on outer iterations reach or residual target reach. You would be aware as proper solution is achieved only after reaching residual target no matter how the fluctuations are.

 March 8, 2010, 14:53 #6 New Member   Chris Morton Join Date: Nov 2009 Location: Waterloo, Ontario, Canada Posts: 8 Rep Power: 8 When I come across problems like this, I usually manually stop the solution, and take a look at the results in CFX post. A velocity vector plot can usually identify the source of the problem (e.g., a stationary re-circulation zone intersecting with the outlet of the domain). If the size of the domain is not as important as the mixing characteristics near the inlet location(s), then increasing the distance between the inlet and outlet location(s) may help rectify the issue.

 March 8, 2010, 23:49 #7 Member   Venkat Join Date: Nov 2009 Posts: 35 Rep Power: 8 I tried with the concept of increasing the distance between the inlet and outlet to avoid the intersection of recirculation zone with outlet during one of the simulations in automotive EGR valve application. I didn't get the proper convergence trend. Moreover convergence stability was not great. I'm aware that there could be so many other factors that affect convergence stability like mesh, y+ condition at the boundary layers, etc.,.

 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 smn CFX 5 November 24, 2009 07:37 Pankaj CFX 9 November 23, 2009 05:05 psb Fluent UDF and Scheme Programming 0 November 10, 2009 03:40 siamak1424 OpenFOAM 2 August 15, 2009 11:14 CN FLUENT 6 May 22, 2005 09:37

All times are GMT -4. The time now is 00:15.