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

DIverging on 1st iteration

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 15, 2004, 11:58
Default DIverging on 1st iteration
  #1
Anna (aka new-user)
Guest
 
Posts: n/a
Hi All!

What does it mean that my model is diverging in first iteration? all the mesh checks and boundary checks were ok (at least those several ones necessary to run the calculation), the geom. file is created, but... it doesn't want to run - just diverges on the first step (was decreasing the time step to 10e-06)...

Please tell me what information I should add to make my problem more comprehensible for you (in general I study the natural convection around solid in max temperature 323K).

Could it be caused by some cells of veeeery bad quality (I know that I have them)?

Thank you!!!
  Reply With Quote

Old   November 15, 2004, 20:08
Default Re: DIverging on 1st iteration
  #2
Samir
Guest
 
Posts: n/a
Make sure you have no unused cells(created twice), Also i am not sure why u would like to use such a small time step. I have solved a complex 2-D problem earlier and a time step of around 0.0005 used to work really well. You can also try playing around(seeing how it affects the residuals) with the relaxation factors, particularly pressure.
  Reply With Quote

Old   November 16, 2004, 04:16
Default Re: DIverging on 1st iteration
  #3
Anna (aka new-user)
Guest
 
Posts: n/a
HI,

Yes I know this time step was ridiculously small... it was just to 'play around' ;-)

What is astonishing is that the model explodes already on first iteration no matter what is changed in the settings....

DOuble cells should have been reported during checks, right? The checks were ok....
  Reply With Quote

Old   November 16, 2004, 07:04
Default Re: DIverging on 1st iteration
  #4
matej
Guest
 
Posts: n/a
Have you checked the info file? no warrnings? is it a mass conservation which is running sky up?

Try some simple physics. Like laminar flow with incompressible fluid, isothermal.....

so you're sure, that there is no probelm with the geometry, but you have to inspect the physics and numerics.

good luck, matej
  Reply With Quote

Old   November 16, 2004, 10:41
Default Re: DIverging on 1st iteration
  #5
Oliver Lauer
Guest
 
Posts: n/a
Make sure you have no collapsed faces. These are not checked during geomwrite!

check all,,facecollapse news

Good luck

Oliver
  Reply With Quote

Old   November 16, 2004, 21:17
Default Re: DIverging on 1st iteration
  #6
Kevin
Guest
 
Posts: n/a
To add to what Oliver said, these checks are also important,

check,cset,,areaface,value,.001,news If you get too many change the tolerance of .001 to something else,

check,cset,,aspect,500,news This check will also tell you if a face is collasped even when it passes the face check.

Also it is good to check for negative volume with a tolerance, check,cset,,negvol,.001,news

How you initialize the domain could also be a factor, but usually it is some bad cells.

Kevin
  Reply With Quote

Old   November 17, 2004, 06:45
Default Re: DIverging on 1st iteration
  #7
Anna (aka new-user)
Guest
 
Posts: n/a
Thanks, thanks, thanks!!!

Exactly: the tolerances were increased, so I was allowed to create the .geom file, but there were some bad couples when the check was performend with the default tolerances. NOw it seems to be all right (after some local corrections of the vertexes)...

a.
  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
VOF, Diverging or not? Renato Pacheco FLUENT 0 April 10, 2008 12:21
Converging then Diverging Residuals??? Erika Johnson FLUENT 8 September 19, 2006 10:45
converging-diverging nozzle seok Jang CD-adapco 1 June 3, 2002 11:50
2D diverging duct simulation venugopal Main CFD Forum 0 November 2, 2001 19:49
Converging-Diverging part Jungyoon hahm FLUENT 4 December 15, 2000 09:19


All times are GMT -4. The time now is 20:28.