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

Change in boundary conditions before rerun

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 5, 2008, 23:42
Default My case is Flow through a Vent
  #1
New Member
 
Aditya Chunekar
Join Date: Mar 2009
Posts: 18
Rep Power: 8
achuneka is on a distinguished road
My case is Flow through a Venturi and I am using lesCavitatingFoam. BC - Velocity inlet and uniform pressure outlet.

I would like to run the case for a higher value of outlet pressure to get initial set of field values.

I then want to reduce the outflow pressure and continue running it further. I am running the job in parallel.

The problem is the modification of boundary conditions in the time files formed.

Please let me know
achuneka is offline   Reply With Quote

Old   August 6, 2008, 04:40
Default - Stop the simulation and edit
  #2
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
- Stop the simulation and edit the last time dump (in all the processor directories). Set startTime to latestTime and restart

- Or use one of timeVaryingUniformFixedValue or timeVaryingMappedFixedValue to automatically vary a fixedValue b.c. (search this forum - see simpleFoam/pitzDailyExptInlet tutorial)
mattijs is offline   Reply With Quote

Old   August 6, 2008, 09:20
Default Thanks Mattijs. The problem
  #3
New Member
 
Aditya Chunekar
Join Date: Mar 2009
Posts: 18
Rep Power: 8
achuneka is on a distinguished road
Thanks Mattijs.

The problem in doing that is this.

The BC for pressure in a "non-decomposed" file looks like this.

outflow
{
type fixedValue;
value uniform 2e5;
}

When I decompose the file into n number of processors, on each processor the file looks like

outflow
{
type fixedValue;
value nonuniform 0();
}

Followed by a list of faces which actually have the same value 2e5.

Same thing applies in the boundary section of dumped time files.

So now if I have to modify these files, I have to
change each of them. Is there any other way to do that ?
achuneka is offline   Reply With Quote

Old   August 6, 2008, 09:36
Default Did you try with 'reconstructP
  #4
Senior Member
 
Mark Olesen
Join Date: Mar 2009
Location: http://olesenm.github.io/
Posts: 777
Rep Power: 18
olesen will become famous soon enough
Did you try with 'reconstructPar', edit the boundary files, 'decomposePar -fields' and then restart?

Or else, if you use the time-varying boundary condition like Mattijs mentioned, you can do a restart without needing to edit the field values themselves. The new value will get taken from the file.
olesen is offline   Reply With Quote

Old   August 6, 2008, 11:21
Default Thanks Mark... reconstructPar
  #5
New Member
 
Aditya Chunekar
Join Date: Mar 2009
Posts: 18
Rep Power: 8
achuneka is on a distinguished road
Thanks Mark... reconstructPar works ..
achuneka 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
Burgerbs equation non constant Boundary Conditions Initial Conditions arkangel OpenFOAM Running, Solving & CFD 1 October 2, 2008 14:48
change boundary conditions adrien FLUENT 3 May 2, 2007 07:52
Integral boundary conditions turbulent intensitylength boundary conditions olesen OpenFOAM Running, Solving & CFD 0 July 27, 2006 07:18
change of boundary conditions luca FLUENT 2 November 22, 2004 11:31
rerun with same flow field, different fluid props Tim Phoenics 0 March 3, 2004 15:51


All times are GMT -4. The time now is 17:49.