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

Cyclic inletoutlet with icoFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 30, 2008, 13:27
Default I'm curious if you can have a
  #1
Member
 
Scott Ripplinger
Join Date: Mar 2009
Posts: 30
Rep Power: 8
sripplinger is on a distinguished road
I'm curious if you can have a cyclic inlet and outlet with the icoFoam solver. I mean, I know you can set the inlet and outlet boundaries as cyclic, but how do you get the fluid to move? Can you set a mass flow rate or pressure gradient? If so, how? I've looked at the channelOodles tutorial case, but haven't figure this out yet.
sripplinger is offline   Reply With Quote

Old   October 30, 2008, 15:41
Default You can set up a mean velocity
  #2
New Member
 
Steven Parole
Join Date: Mar 2009
Posts: 3
Rep Power: 8
steven is on a distinguished road
You can set up a mean velocity, ubar, instead of mass flow rate or pressure gradient.

Steve
steven is offline   Reply With Quote

Old   October 31, 2008, 10:43
Default You'll have to use a modified
  #3
Senior Member
 
John Deas
Join Date: Mar 2009
Posts: 160
Rep Power: 8
johndeas is on a distinguished road
You'll have to use a modified version of icoFoam though. See the channeloodles solver as a source of inspiration.
johndeas is offline   Reply With Quote

Old   October 31, 2008, 11:25
Default Sounds like more work than it'
  #4
Member
 
Scott Ripplinger
Join Date: Mar 2009
Posts: 30
Rep Power: 8
sripplinger is on a distinguished road
Sounds like more work than it's worth to me right now. I'll likely just deal with a entrance region and take my data farther downstream. Thanks.
sripplinger is offline   Reply With Quote

Old   November 5, 2008, 04:04
Default You could try the directMapped
  #5
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
You could try the directMapped boundary condition which recycles sampled data (from inside the domain) to the inlet. See the oodles/pitzDailyDirectMapped case.
mattijs is offline   Reply With Quote

Old   November 8, 2008, 05:48
Default hi guys I've tried this in
  #6
Member
 
antonio segalini
Join Date: Mar 2009
Posts: 75
Rep Power: 8
antonio_ing is on a distinguished road
hi guys

I've tried this in a simulation of a channel flow just adding a constant pressure gradient to the icoFoam solver, so modifing the equations. In this way it is possible to work with a dummy pressure that can be cyclic (0 in steady state).
You can take the icoFoam solver folder in /OpenFOAM/applications/solvers/incompressible/icoFoam
copy it and rename as you wish (i used flatChannel). then rename the icoFoam.c as flatChannel.C and add the pressure gradient term as:

fvVectorMatrix UEqn
(
fvm::ddt(U)
+ fvm::div(phi, U)
- fvm::laplacian(nu,U)
+ dpdx
);

in the createField.H you have to add a term that recall a file inside the directory 0 named dpdx. The expression is the same of the call at the p file so you can just modify it.
Then in the 0 directory you have to create a file dpdx similar to the pressure file (remember that the dimensions are different i.e. [0 1 -2 0 0 0]) and set everywhere it constant

also, you have to change the call to the function icoFoam in the directory of the new solvers (follow the pogrammers guide for a better explanation)

i know that is a mess but it worked fine for me in a channel flow. Any suggestions for easier ways are welcome

bye
antonio_ing 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
Inletoutlet rengu OpenFOAM Running, Solving & CFD 7 June 8, 2015 03:02
Density in icoFoam Densidad en icoFoam manuel OpenFOAM Running, Solving & CFD 8 September 22, 2010 04:10
Velocity Jump at InletOutlet cliffoi OpenFOAM Running, Solving & CFD 0 September 8, 2008 05:34
TwoPhaseEulerFoam and InletOutlet boundary condition hemph OpenFOAM Running, Solving & CFD 10 January 29, 2007 10:47
TwoPhaseEulerFoam and InletOutlet BC hemph OpenFOAM Bugs 0 January 29, 2007 05:57


All times are GMT -4. The time now is 21:33.