CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

Inlet & Outlet Velocity BC issue

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 30, 2012, 05:14
Default Inlet & Outlet Velocity BC issue
  #1
New Member
 
Emiliano
Join Date: Oct 2012
Posts: 2
Rep Power: 0
naiter is on a distinguished road
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
naiter is offline   Reply With Quote

Old   November 30, 2012, 05:48
Default
  #2
Senior Member
 
Bernhard
Join Date: Sep 2009
Location: Delft
Posts: 782
Rep Power: 11
Bernhard is on a distinguished road
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?
Bernhard is offline   Reply With Quote

Old   November 30, 2012, 10:41
Default
  #3
Senior Member
 
Lieven
Join Date: Dec 2011
Location: Mol, Belgium
Posts: 294
Rep Power: 11
Lieven will become famous soon enough
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
Lieven is offline   Reply With Quote

Old   December 19, 2012, 07:14
Default
  #4
New Member
 
Emiliano
Join Date: Oct 2012
Posts: 2
Rep Power: 0
naiter is on a distinguished road
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
naiter is offline   Reply With Quote

Reply

Tags
outlet boundary condition, simplefoam convergence

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
Boundary Conditions: Pressure Inlet, Velocity Outlet BigPapi34 OpenFOAM Running, Solving & CFD 2 May 3, 2013 03:05
Problem with assigned inlet velocity profile as a boundary condition Ozgur_ FLUENT 2 August 3, 2012 05:54
Inlet and outlet boudary without wall between Janshi CFX 5 February 2, 2012 04:51
VOF Volume fraction in Velocity inlet aruelle FLUENT 1 March 18, 2010 12:53
Velocity on inlet and outlet greg FLUENT 2 March 7, 2006 07:16


All times are GMT -4. The time now is 01:25.