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

Outflow boundary Control Volume SIMPLE Help !!!

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 21, 2011, 22:55
Default Outflow boundary Control Volume SIMPLE Help !!!
  #1
New Member
 
anonymous
Join Date: Aug 2011
Posts: 5
Rep Power: 5
Mizerable is on a distinguished road
Hi guys,

I'm new to this forum community, but I have been a long time lurker so I'm really hoping I can access some of the great help you guys give.

I'm just a bit confused about how to implement the outflow boundary condition. I've been reading Versteeg's book on the control volume method and SIMPLE, and my code is based on the teachings of that book.

I've written a little program in C for 2D transient problems that works well with the lid-driven problem, but now I'm trying to calculate the flow around a circle obstacle and I can't seem to get the outflow boundary to work!

I have a rectangle region where the west wall is inflow and the other three walls are to be outflow. In the middle is the circular obstacle. At the inflow I've specified the velocity in the X direction and zero velocity in the Y direction.

I've read in Versteeg that I should take the boundary velocities at the outflows equal to the velocities of the adjacent outer-most layer of interior cells. It says I should then adjust the velocities perpendicular to the outflow boundaries by the ratio of total velocities per cell summed across the inflow divided by the total perpendicular-to-outflow velocities per cell summed across the outer-most layer of interior cells adjacent to the outflow boundaries.

That is as much info as Versteeg gives. I'm wondering how this all fits into the SIMPLE algorithm... Once these velocities have been extrapolated for for the outflow cells should I treat them as dirichlet boundary cells for velocity? I am really kinda in the dark here... Where in the SIMPLE algorithm do I extrapolate these outflow velocities?

Any hints would be great! Thank you!
Miz
Mizerable is offline   Reply With Quote

Old   August 21, 2011, 23:38
Default
  #2
Senior Member
 
Cean
Join Date: Feb 2010
Posts: 128
Rep Power: 7
shirazbj is on a distinguished road
you could reference peric's 2dc\pipe\pcol1.f code

C################################################# ############
SUBROUTINE OUTBC
C################################################# ############
C In this routine, zero-gradient condition is implemented
C at outlet and the velocity is corrected to satisfy the
C global mass conservation. In this way, one can treat the
C velocity at outlet boundary as prescribed for one SIMPLE
C step, i.e. in the pressure-corrcetion equation, the
C velocity is assumed given at all boundaries and will not
C corrected.
C-------------------------------------------------------------

Last edited by shirazbj; August 26, 2011 at 01:56.
shirazbj is offline   Reply With Quote

Old   August 22, 2011, 11:33
Default this is a classic question
  #3
Member
 
Wu Jian
Join Date: Jun 2009
Location: Poitiers
Posts: 33
Rep Power: 8
harbinyg is on a distinguished road
Send a message via MSN to harbinyg
hi,

do not be upset, many people meet these kinds of people when they first start the CFD study...

as for the outflow boundary condition treatments, there are three main kinds of methods , there are some good references and you can have a search ....

according to the information you described, i think you select a good method,

in my opinion,

'there is a global correction of mass fluxes at the outlet boudary to make them satisfy the global mass conservation; before solving the pressure-correction equation'

'when this is done, one can assume in the pressure-correction that the mass fluxes are prescribed at all boundaries and therefore need not be corrected, leading to Neumann boundary conditions for pressure correction at all boundaries.'

in practice,

1. you solve discrete momentum equations

2. do the outflow velocities correction;

3. solve pressure - correction equations, still with full neumann boundary conditions;

4. update velocities and pressure , noting, at all boudaries, no correction ...

best wishes !
harbinyg is offline   Reply With Quote

Old   August 22, 2011, 11:53
Default
  #4
New Member
 
anonymous
Join Date: Aug 2011
Posts: 5
Rep Power: 5
Mizerable is on a distinguished road
Quote:
Originally Posted by harbinyg View Post
hi,

do not be upset, many people meet these kinds of people when they first start the CFD study...

as for the outflow boundary condition treatments, there are three main kinds of methods , there are some good references and you can have a search ....

according to the information you described, i think you select a good method,

in my opinion,

'there is a global correction of mass fluxes at the outlet boudary to make them satisfy the global mass conservation; before solving the pressure-correction equation'

'when this is done, one can assume in the pressure-correction that the mass fluxes are prescribed at all boundaries and therefore need not be corrected, leading to Neumann boundary conditions for pressure correction at all boundaries.'

in practice,

1. you solve discrete momentum equations

2. do the outflow velocities correction;

3. solve pressure - correction equations, still with full neumann boundary conditions;

4. update velocities and pressure , noting, at all boudaries, no correction ...

best wishes !

Thank you so much for this explanation ! I will try this for now and see how it works for me
Mizerable is offline   Reply With Quote

Old   August 22, 2011, 13:00
Default
  #5
New Member
 
anonymous
Join Date: Aug 2011
Posts: 5
Rep Power: 5
Mizerable is on a distinguished road
I'm trying to implement it as suggested but I am unsure how to do the tri-diagonal method without a constant boundary value.

The way Versteeg has in his book is that the tri-diagonal method runs along a column of cells from cells 1 to N-1 where the values of cells 0 and N are defined boundary values. How do I do this algorithm without set boundary values like the outflow boundary?

Further I would like to ask how are the coefficients aE,aW,aN,aS calculated for cells adjacent to these outflow boundary cells?

Thanks so much!
Mizerable 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
mixed inflow/outflow downstream boundary condition question peob OpenFOAM Running, Solving & CFD 2 August 14, 2014 09:07
maintaining a logarithmic velocity distribution Morten Andersen CFX 1 January 8, 2007 12:37
SST in 2D? Jesper Sørensen CFX 16 December 23, 2006 09:40
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15
New topic on same subject - Flow around race car Tudor Miron CFX 15 April 2, 2004 06:18


All times are GMT -4. The time now is 23:38.