CFD Online Logo CFD Online URL
Home > Forums > OpenFOAM Running, Solving & CFD

mixed inflow/outflow downstream boundary condition question

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

Like Tree2Likes
  • 2 Post By peob

LinkBack Thread Tools Display Modes
Old   July 19, 2011, 14:21
Default mixed inflow/outflow downstream boundary condition question
New Member
Join Date: Mar 2011
Location: West Des Moines, Iowa, U.S.A.
Posts: 5
Rep Power: 6
peob is on a distinguished road
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 steady-state runs, or Courant numbers for time-accurate 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 "well-posed" mathematically for a true outflow boundary: one variable specified (pressure) and the remainder are extrapolated. However, they are not well-posed 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, well-posed 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 well-posed BC, and my prior-divergent 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.)


Last edited by peob; July 20, 2011 at 13:00. Reason: correct some mistakes in the message
peob is offline   Reply With Quote

Old   October 15, 2011, 10:53
New Member
Join Date: Mar 2011
Location: West Des Moines, Iowa, U.S.A.
Posts: 5
Rep Power: 6
peob is on a distinguished road
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.

peob is offline   Reply With Quote

Old   August 14, 2014, 09:07
Join Date: Jul 2013
Posts: 37
Rep Power: 3
ni-openfoam-user is on a distinguished road
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,

ni-openfoam-user is offline   Reply With Quote


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
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

All times are GMT -4. The time now is 20:26.