# Inlet & Outlet Velocity BC issue

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

 November 30, 2012, 06:14 Inlet & Outlet Velocity BC issue #1 New Member   Emiliano Join Date: Oct 2012 Posts: 2 Rep Power: 0 Hi all, I'm new to this forum and i'm trying to solve some problem with a simpleFoam case (k-epsilon on). I need to fix, in a quite complex volume, inlet velocity and outlet velocity. Currently I set the same magnitude for the velocity (inlet&outlet BC). U: inlet { type fixedValue; value uniform ( 0 -0.12608 -1.19953 ); } outlet { type fixedValue; value uniform ( 0 0.6030 1.0445); } And the following setup for k and epsilon k: inlet { type fixedValue; value uniform 0.0058; } outlet { type zeroGradient; } epsilon: inlet { type fixedValue; value uniform 0.0004464; } outlet { type zeroGradient; } I've tried different relaxation factors and a non-orthogonal corrector (up to 3), but the solution diverges in any case, here follows one of the last time step of the last try: Time = 118 DILUPBiCG: Solving for Ux, Initial residual = 0.249643, Final residual = 0.0101623, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.51045, Final residual = 0.0151908, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.358048, Final residual = 0.0100483, No Iterations 1 DICPCG: Solving for p, Initial residual = 0.096591, Final residual = 0.000935744, No Iterations 95 DICPCG: Solving for p, Initial residual = 0.0110689, Final residual = 0.00322944, No Iterations 1001 DICPCG: Solving for p, Initial residual = 0.00880522, Final residual = 0.000360479, No Iterations 1001 DICPCG: Solving for p, Initial residual = 0.00457367, Final residual = 0.000729296, No Iterations 1001 time step continuity errors : sum local = 9201.84, global = 165.064, cumulative = 1181.92 DILUPBiCG: Solving for epsilon, Initial residual = 0.46882, Final residual = 0.016255, No Iterations 1 bounding epsilon, min: -1.24386e+11 max: 3.21053e+29 average: 2.27437e+23 DILUPBiCG: Solving for k, Initial residual = 0.306587, Final residual = 0.0120154, No Iterations 1 ExecutionTime = 82751.3 s ClockTime = 85751 s Are the BCs right? or to fix inlet and outlet velocity in this way can produce this kind of error? Any suggestion is welcome or address me to an existing thread if I miss it. Thanks to all

 November 30, 2012, 06:48 #2 Senior Member   Bernhard Join Date: Sep 2009 Location: Delft Posts: 790 Rep Power: 14 What are the boundary conditions for pressure? If you look at the log file, you see that you need a lot of iterations on p, this is not a good sign, it doesn't look like it is converging at all. Try foamLog and check some of the initial residuals, e.g p_0, and you will probably see that it is not really decreasing, which is should. At some point it diverges on epsilon, but that is not the big issue. Can you try to set outlet velocity bc to zeroGradient, outlet pressure to fixedValue (0 if you like) and inlet pressure to zeroGradient?

 November 30, 2012, 11:41 #3 Senior Member   Lieven Join Date: Dec 2011 Location: Leuven, Belgium Posts: 297 Rep Power: 14 Why are you fixing velocity at both inlet and outlet? Since you're running an incompressible solver the mass flow rate through inlet and outlet must match exactly or you'll get continuity problems (i.e. problems with the pressure equation). And "matching exactly" is practically impossible. So if I were you I would set a Neumann boundary condition at the outlet (unless you have somewhere a second outlet). Regards, L

 December 19, 2012, 08:14 #4 New Member   Emiliano Join Date: Oct 2012 Posts: 2 Rep Power: 0 Thank a lot Bernhard and Lieven Now my runs work properly with Neumann conditions. Also the foamLog was a very useful suggestion for the analysis of the residuals. One day I'll try pyFoam to add functionalities

 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 Ozgur_ FLUENT 5 August 25, 2015 04:58 BigPapi34 OpenFOAM Running, Solving & CFD 4 August 2, 2014 11:39 Janshi CFX 5 February 2, 2012 05:51 aruelle FLUENT 1 March 18, 2010 12:53 greg FLUENT 2 March 7, 2006 08:16

All times are GMT -4. The time now is 21:25.