
[Sponsors] 
July 19, 2011, 14:21 
mixed inflow/outflow downstream boundary condition question

#1 
New Member
Phil
Join Date: Mar 2011
Location: West Des Moines, Iowa, U.S.A.
Posts: 11
Rep Power: 7 
Many of the simulations that I run have mixed inflow/outflow at the downstream boundary of my domain, and I'm trying to figure out the correct choice of downstream/outflow boundary conditions on the different field values (U, p, k, epsilon).
I have looked through most of the tutorials and currently specify the following for the downstream/outflow boundary: for U: type pressureInletOutletVelocity; value uniform ( 0 0 0 ); inletValue uniform ( 0 0 0 ); for p: type fixedValue; value uniform 101325; for k: type inletOutlet; value uniform 0.06; inletValue uniform 0.06; for epsilon: type inletOutlet; value uniform 25.46; inletValue uniform 25.46; However, I have found that in some cases (not all cases) I get solution divergence occurring at the outflow boundary where the flow is coming in (i.e. an inflow at the outflow boundary). [NOTE: in these divergent cases I have checked that the grid quality is good; I have lowered relaxation factors for steadystate runs, or Courant numbers for timeaccurate runs by orders of magnitude and the divergent behavior persists.] Now, when I look at the choice of boundary conditions (see above) I note that they are "wellposed" mathematically for a true outflow boundary: one variable specified (pressure) and the remainder are extrapolated. However, they are not wellposed mathematically for inflow at the outflow boundary. For inflow at the outflow boundary, there should be one variable extrapolated (ideally the outward running characteristic) and the remainder specified, but with my choice of BCs, I have all variables specified. So, I'll start out with two questions... 1) has anyone else experienced similar phenomena as described above (i.e. divergent solution at the outflow boundary when the boundary flow is mixed inflow/outflow)? 2) Does anyone have any suggestions as to appropriate boundary condition choices available in the current distribution of OpenFOAM (I'm using OpenFOAM 2.0.0 and 1.7.1) so that I have consistent, wellposed boundary conditions for a mixed inflow/outflow? (just as another note... I did switch the pressure boundary condition to "outletInlet", which does represent a reasonably wellposed BC, and my priordivergent solution was nicely stabilized and ran just fine. My concern with this choice of BC is that the downstream pressure, which I want specified at a fixed value, can now drift.) Thanks. Phil Last edited by peob; July 20, 2011 at 13:00. Reason: correct some mistakes in the message 

October 15, 2011, 10:53 

#2 
New Member
Phil
Join Date: Mar 2011
Location: West Des Moines, Iowa, U.S.A.
Posts: 11
Rep Power: 7 
I think I found the problem.
It looks like I needed to use the "totalPressure" boundary condition for pressure at the outflow boundary. When I do this, my current runs appear to stabilize nicely at the outflow boundary, and I get the expected behavior of the pressure at the outflow boundary. Phil 

August 14, 2014, 09:07 

#3 
Member
James
Join Date: Jul 2013
Posts: 38
Rep Power: 5 
Dear Phil,
I am currently faced with the problem of what settings for "open atmosphere" boundaries. I have followed your settings regarding U, P, k and epsilon, i.e.: U = pressureInletOutletVelocity p = totalPressure k = inletOutlet epsilon = inletOutlet However for some reason I get a build up of velocity, k, epsilon, alphat and mut at the extremities of my domain. Could you please comment on suitable settings for T, O2, N2, H2, mut and alphat as well? A detail description of my scenario can be found below (post 4): Free jet simulation Many thanks, James 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
velocity profile inlet boundary condition question  Lcw  FLUENT  3  August 3, 2012 05:53 
asking for Boundary condition in FLUENT  Destry  FLUENT  0  July 27, 2010 00:55 
Boundary condition question, help please!  fjalil  CFX  2  June 11, 2009 12:52 
a simple Boundary condition question  prapanj  OpenFOAM Running, Solving & CFD  1  March 16, 2009 08:51 
Question about the outlet boundary condition.  G.H.Lee  Main CFD Forum  5  April 29, 1999 04:50 