CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CD-adapco (http://www.cfd-online.com/Forums/cd-adapco/)
-   -   scalar equation not converging (http://www.cfd-online.com/Forums/cd-adapco/52965-scalar-equation-not-converging.html)

hennie July 16, 2002 08:52

scalar equation not converging
 
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

john YL July 17, 2002 06:57

Re: scalar equation not converging
 
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.

hennie July 24, 2002 04:06

Re: scalar equation not converging
 
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


All times are GMT -4. The time now is 14:18.