# Outflow Boundary Condition Implementation

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 November 9, 2012, 22:31 Outflow Boundary Condition Implementation #1 New Member   Mijail Febres Join Date: May 2010 Posts: 4 Rep Power: 7 Hi guys, Recently i've implemented a CFD code for unstructured meshes using FV method with collocated variables for incompresible, steady-state Navier Stokes equations. I had pretty good results with this code when compared to Ghia's results and others benchmark results for lid-driven cavities problems. Now i'm trying to implement velocity inlet and outflow BCs, but i'm having serious problems with it, i get negative sources for Momentum eqs and really large velocities and my code diverges really quick. I know that velocity inlet is really simple, it's the same as wall BCs, zero gradient for pressure, and mass flow rate know. Outflow BC for what i read consists on impose zero gradient for velocities at the outflow faces, this of course corrected with the relation m_dot_in/m_dot_out to ensure conservation. Since mass flow rate is calculated with Rho*V.A at inlet i get negative mass flow rates because of the face normal vector and positive mass flow rates for outflow (also because of the face normal vector). Hence, m_dot_in/m_dot_out can get negative, affecting signal on u and v on faces. Could that be the problem? What do i do with the pressure on outflow Bc faces? What is the proper way to impose outflow BCs on unstructured meshes? I appreciate in advance any responses. Mijail.

 February 13, 2013, 00:55 #2 New Member   Debanjan Deep Join Date: Mar 2009 Posts: 14 Rep Power: 8 I have a question regarding the mass flow rate during outflow boundary condition employed. I am wondering why this mass flow rate ratio is required to put in fluent since I believe fully developed flow (velocity gradient zero) is sufficient bc condition to satisfy NS equation. Am I right? In case of multiple outflow outlet bc, it is mandatory to put those mass flow weight ratio to get a perfect simulation result as I have experienced before. Why is it required? Any idea? Thanks. Deep

 February 13, 2013, 03:58 #3 Senior Member     Paolo Lampitella Join Date: Mar 2009 Location: Italy Posts: 534 Blog Entries: 14 Rep Power: 17 From the mathematical point of view, such incompressible flow issues are related to the way the problem is solved. More precisely with the Helmholtz-Hodge decomposition. I try to explain it very roughly. When you predict the velocity (before pressure correction) you can actually fix only tangential velocity components on the boundary while normal ones are somehow free (indeed they do not satisfy the divergence free constraint). You could fix them to satisfy overall continuity on the boundary but this is fully arbitrary and the following pressure correction is likely to create problems. What is usually done here is to use the null gradient hypothesis on the outflow for the diffusive term, possibly coupled with a significant convection velocity (so, not necessarily a crude extrapolation). Still, no extrapolation can ever ensure a full mass conservation. Normal velocity components on boundaries are instead to be fixed in the pressure correction stage, where they actually belong. But, at this point, you don't have any more an equation to do that and you can only prescribe the overall continuity to be satisfied. When multiple outflows are present, there is no chance to get an exact information on the distribution of the outflow mass rates over the different exits and some assumption is needed for the final correction. Notice that the assumption made in Fluent is really strong and final results can be strongly affected. My preferred approach when multiple outflows are present is to collect them in a single face so that a single unitary coefficient is used for all of them.

February 13, 2013, 07:42
#4
Senior Member

andy
Join Date: May 2009
Posts: 129
Rep Power: 8
Quote:
 Originally Posted by skyblue_mech I have a question regarding the mass flow rate during outflow boundary condition employed. I am wondering why this mass flow rate ratio is required to put in fluent since I believe fully developed flow (velocity gradient zero) is sufficient bc condition to satisfy NS equation. Am I right? In case of multiple outflow outlet bc, it is mandatory to put those mass flow weight ratio to get a perfect simulation result as I have experienced before. Why is it required? Any idea? Thanks. Deep
Consider a flow with two long pipes as outlets so that a zero gradient condition on the velocity is a reasonable one. Downstream of the zero gradient exit condition one of the pipes is blocked by a wall while the other one is open to the atmosphere. The solution is no flow at one of the exits and fully developed flow equal to the inlet flow at the other but we have no way to specify this and distinguish it from the case of a 50:50 flow split or 75:25 split or whatever... Clearly insufficient information has been specified about the conditions at the boundary to pin down the infinite number of possible solutions to the incompressible Navier-Stokes equations within the solution region to just one.

Specifying the mass flow split is the commonest way to provide this missing boundary information for incompressible flow but, for the example above, fixing the pressure at the two outlets would also work if reverse flow is truncated.

 February 14, 2013, 01:24 #5 New Member   Debanjan Deep Join Date: Mar 2009 Posts: 14 Rep Power: 8 Thank you a lot for these useful responses. Deep

February 14, 2013, 02:08
#6
Senior Member

Arjun
Join Date: Mar 2009
Location: Nurenberg, Germany
Posts: 373
Rep Power: 10
Quote:
 Originally Posted by andy_ Consider a flow with two long pipes as outlets so that a zero gradient condition on the velocity is a reasonable one. Downstream of the zero gradient exit condition one of the pipes is blocked by a wall while the other one is open to the atmosphere. The solution is no flow at one of the exits and fully developed flow equal to the inlet flow at the other but we have no way to specify this and distinguish it from the case of a 50:50 flow split or 75:25 split or whatever... Clearly insufficient information has been specified about the conditions at the boundary to pin down the infinite number of possible solutions to the incompressible Navier-Stokes equations within the solution region to just one. Specifying the mass flow split is the commonest way to provide this missing boundary information for incompressible flow but, for the example above, fixing the pressure at the two outlets would also work if reverse flow is truncated.

i don't get it. If the other outlet is further blocked by wall, there will still be flow throw it. Just because there is wall ahead why shall flow stop before the wall?

February 14, 2013, 06:32
#7
Senior Member

andy
Join Date: May 2009
Posts: 129
Rep Power: 8
Quote:
 Originally Posted by arjun i don't get it. If the other outlet is further blocked by wall, there will still be flow throw it. Just because there is wall ahead why shall flow stop before the wall?
I am not sure I fully understand your question. If a pipe is blocked then there will be no flow down it. For an incompressible fluid the mass flow across every section through the pipe must be the same and so if the exit flow is zero so is the flow across every other section. At the inlet you may get some flow down the pipe balanced by the same amount of flow up the pipe.

 February 14, 2013, 07:38 #8 Senior Member   Filippo Maria Denaro Join Date: Jul 2010 Posts: 1,653 Rep Power: 23 I am not sure to understand your discussion ... the general rule for incompressible flows are 1) Int [S] n.V dS = 0 -> the flow-rate is conserved 2) on BCs only one between velocity or pressure can be prescribed 3) Div.V = 0 can be satisfied at machine accuracy for the exact projection method or at the level of the local truncation error for the approximate projection method. If some of these three condition is not fulfilled then there should be a bug in the code

 Tags outflow bcs

 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 peob OpenFOAM Running, Solving & CFD 2 August 14, 2014 09:07 tsikroria0 OpenFOAM 0 June 28, 2011 16:39 CFD XUE FLUENT 0 July 9, 2010 02:53 bearcharge Main CFD Forum 0 May 14, 2010 11:32 J. Weiler FLUENT 5 May 10, 2001 05:11

All times are GMT -4. The time now is 12:55.

 Contact Us - CFD Online - Top