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

InletOutlet boundary condition in motorBike tutorial

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 27, 2009, 06:52
Default InletOutlet boundary condition in motorBike tutorial
  #1
Senior Member
 
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 8
madad2005 is on a distinguished road
In the motorbike tutorial, the boundary condition for velocity at the pressure outlet is set to:

type inletOutlet
inlet uniform (0 0 0)
outlet uniform (20 0 0)

Can I ask why the inlet value has been set to (0 0 0)? I'm expecting this to be the same as what has been defined at the inlet itself, which was (20 0 0). All other quantities that use inletOutlet are set as I'd expect too.
madad2005 is offline   Reply With Quote

Old   November 27, 2009, 08:45
Default
  #2
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
Quote:
Originally Posted by madad2005 View Post
In the motorbike tutorial, the boundary condition for velocity at the pressure outlet is set to:

type inletOutlet
inlet uniform (0 0 0)
outlet uniform (20 0 0)

Can I ask why the inlet value has been set to (0 0 0)? I'm expecting this to be the same as what has been defined at the inlet itself, which was (20 0 0). All other quantities that use inletOutlet are set as I'd expect too.
I'm not sure which directories you have or which OpenFOAM version, but on my OpenFOAM-1.6.x tutorials/incompressible/simpleFoam/motorBike/0/U contains this

Code:
    outlet
    {
        type            inletOutlet;
        inletValue      uniform (0 0 0);
        value           $internalField;
    }
whereas the 0/k contains this:

Code:
    outlet
    {
        type            inletOutlet;
        inletValue      $internalField;
        value           $internalField;
    }
There are no 'inlet' or 'outlet' keywords, but rather 'inletValue' and 'value'.

The 'value' is needed to initialize the boundary condition class (also supplies a value for post-processing etc) and will be overwritten in subsequent time steps with the current values for those faces.

The 'inletValue' is the value that should be used if there are any flow reversals in the system. If there is somehow a flow reversal at the outlet boundary, a zero-velocity should be a reasonable approximation of the entrainment of a quiescent fluid from teh surrounding environment.
For turbulence quantities, using a zero-value for an entrainment condition when there is backflow might not be a great idea (eg, when epsilon -> zero, the equations are ill behaved). Using the same turbulence quantities as the normal inlet has can't really be exactly correct either, but probably not that bad. Even if it is a somewhat incorrect value, the flow reversal velocities are probably fairly short lived and not that strong. I don't think it should normally affect your solution.
olesen is offline   Reply With Quote

Old   November 27, 2009, 09:15
Default
  #3
Senior Member
 
Anonymous
Join Date: Mar 2009
Posts: 110
Rep Power: 8
madad2005 is on a distinguished road
Thanks for the reply.

Yes, those are the entries I am talking about. My mistake was due to the fact I wasn't refering directly to the code when I posted. But, thank you for taking the time to clarify exactly was it is doing.
madad2005 is offline   Reply With Quote

Reply

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
problem with boundary condition??? smn CFX 5 November 24, 2009 07:37
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
Axis Boundary Condition..what is it? CFDtoy FLUENT 6 February 13, 2007 06:51
How to set boundary condition in Fluent for the fo Peiyong FLUENT 1 November 10, 2006 12:44
How to resolve boundary condition problem? sam FLUENT 2 July 20, 2003 02:19


All times are GMT -4. The time now is 15:29.