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

Explicit algorithm

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 22, 2008, 04:53
Default Hi there, I want to know if
  #1
New Member
 
Rina Oldek
Join Date: Mar 2009
Posts: 5
Rep Power: 8
rinao is on a distinguished road
Hi there,

I want to know if there is an explicit algorithm in OpenFoam, where multiple time steps are used in the simulations depending on the parameters or space step (delta x).

Thanks

Rina
rinao is offline   Reply With Quote

Old   October 22, 2008, 06:16
Default I'm not entirely clear what yo
  #2
Senior Member
 
Gavin Tabor
Join Date: Mar 2009
Posts: 181
Rep Power: 8
grtabor is on a distinguished road
I'm not entirely clear what you mean here; but if you construct an equation object where the only fvm:: operator used is the time derivative, then you have an explicit algorithm. Eg. for the heat equation;

solve(fvm::ddt(T) == kappa*fvc::laplacian(T));

is an explicit algorithm. fvc:: is always an explicit evaluation of the field.

Gavin
grtabor is offline   Reply With Quote

Old   October 22, 2008, 07:43
Default Hi Gavin, Thanks for your e
  #3
New Member
 
Rina Oldek
Join Date: Mar 2009
Posts: 5
Rep Power: 8
rinao is on a distinguished road
Hi Gavin,

Thanks for your email.

What I ment by explicit algrithm is by the ability to change the time step throughout the simulation depending on the courant number, for example in the case of a pressure wave.
Is it possible?

Rina
rinao is offline   Reply With Quote

Old   October 22, 2008, 08:01
Default If you want to use a Courant-b
  #4
Super Moderator
 
niklas's Avatar
 
Niklas Nordin
Join Date: Mar 2009
Location: Stockholm, Sweden
Posts: 693
Rep Power: 19
niklas will become famous soon enough
If you want to use a Courant-based timestep you might have to modify the code.
Dont worry, it is very easy.

Lets take turbFoam as an example.
open up turbFoam.C with your favourite editor and
after this line
# include "initContinuityErrs.H"
add this
# include "readTimeControls.H"

and after this line
# include "CourantNo.H"
add this
# include "setDeltaT.H"

now run wmake

to use it you need to edit the system/controlDict
by adding these lines

adjustTimeStep on;
maxCo 0.1;

and thats it.

N
niklas 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
implicit or explicit laure FLUENT 2 June 2, 2007 06:45
Explicit Solver wessels OpenFOAM Running, Solving & CFD 1 September 26, 2005 05:39
LES (explicit) filtering John Main CFD Forum 2 July 29, 2004 18:03
explicit formulations Muhammad zubair FLUENT 1 June 14, 2004 00:44
Coupled Explicit Andrew Parker FLUENT 1 October 12, 2001 07:18


All times are GMT -4. The time now is 11:36.