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

scalar equation not converging

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 16, 2002, 08:52
Default scalar equation not converging
  #1
hennie
Guest
 
Posts: n/a
Hi, in my IC engine simulation, I'm trying to add combustion to the simulation. I want to use the Weller flame model and have 5 scalars specified as combustion related scalars. The initial flow field consist of constant concentrations with const concentrations spesified at the boundaries. All of these values are for stoichiometric air fuel ratio. The problem is that the scalar equations do not converge. Can anybody please advise a solution. The following warnings occur:

*** WARNING #013 *** MAXIMUM SPECIFIED CORRECTOR STAGES 20 REACHED BEFORE CONVERGENCE CRITERION IS SATISFIED.

<<<<SCALAR EQUATION 2 NOT CONVERGED>>>>

<<<<SCALAR EQUATION 5 NOT CONVERGED>>>>

----YOU MAY USE SWITCH 87 TO TURN OFF SCALAR CHECK IN PISO

*** WARNING #052 *** INITIAL RESIDUAL BELOW ROUND-OFF ERROR LIMIT SOLUTION ,EQ: SC1

setting the UR factors for the scalars did not solve my problem. I also changed the max number of PISO correctors to 300, still not solving the problem
  Reply With Quote

Old   July 17, 2002, 06:57
Default Re: scalar equation not converging
  #2
john YL
Guest
 
Posts: n/a
Does this occur at the begining of calculation or is it persistent? For transient calculation, under-relaxation factor for scalars is not used. It seems the problem may be caused by linear solver not solving the equation at all as indicated by waring #052. Try adjusting round-off level for the solver by using REAL CONSTANT 30: the default is 1.e-12 for double precision run, reduce this value to 1.e-16 (say). If you are not running double precision, you may have to use it.
  Reply With Quote

Old   July 24, 2002, 04:06
Default Re: scalar equation not converging
  #3
hennie
Guest
 
Posts: n/a
Thanks for the response. After trying your solution and not solving the problem, I realized that mine was a more fundamental problem. As I'm using tetrahedral meshes, the pressure boundary at the intake gives convergence problems. I read in the user manual that one needs at least two cell layers next to a pressure boundary to counteract this error. After adding some hexahedral cells to the upstream side of the intake, with an arbitrary couple in between the two regions, the problem seems solved.

Cheers

Hennie
  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
Solving an equation for a scalar with sources XiZao FLOW-3D 1 January 16, 2009 01:54
Scalar Equation source term Merck CFX 0 May 11, 2007 05:30
UDS - scalar equation tomik FLUENT 0 May 17, 2006 04:17
Equation for scalar source niklas OpenFOAM Running, Solving & CFD 7 September 15, 2005 07:13
scalar equation Arturo Ortiz FLUENT 3 October 8, 2000 12:36


All times are GMT -4. The time now is 09:08.