Saturne is not calculating

For all those who are struggling to make C_S run, the solution is simple: if you want to run a steady case, be sure you have a asteady phenomenon, otherwise go for unsteady.
In any of both cases, you're very likely to need more than 100 iterations, and it's recomended that you use lower than by default relaxation coefficients (0.5 or less). Give also logical initialization values to the speed and any other scalar you may have defined. Check also that your mesh is adequate for the case; it's harder to notice, but a good method is starting with coarse meshes and then refine as you see the solution converges.
Following these hints I was able to run very nice simulations, or at lest the colors are fancy . Happy C_S:cheer: .

Hello,

I'll just add that I have never needed (nor tried) relaxation coefficients under 0.7, but with some meshes (even purely hexahedral meshes with stretched/warped sections), using relaxation is the only way to obtain convergence (or at least avoid divergence). Other parameters, such as flux reconstruction at the boundaries, number of sweeps, linear solver precision, etc. are important, but in the case of a problem, I would recommend trying relaxation first.

Also, when running unsteady calculations, watch your CFL number. Code_Saturne uses a segregated solver, not a coupled solver, and CFL numbers above 5 should be avoided if possible (CFL values up to 20 in a small number of cells may be acceptable, but it is not recommended to have an average CFL above 5 (1 for LES calculations).

The CFL (Courant) number may be visualized in Code_Saturne's postprocessing output, which is the best way of checking it.

Note also that some of us from the Code_Saturne developpement team check this forum occasionally, but check the code-saturne.info forum more regularly (though registration requires sending an e-mail to saturne-support, as described on the site)

Best regards,

Yvan

I personally use the same inlet velocity for both steady and unsteady runs. I've got good results, but I think it only delays or accelerates convergence without affecting convergence itself, i.e. in a straight simple channel you're very likely to get values very close to the inlet's in most of the flow field, so for a steady simulation it wouldn't make much sense IMHO to start with zero velocities (it will converge slower). Now, for an unsteady simulation it might be different, in the sense that you may want to see the effects of accelerating flow.
I've made an unsteady simulation of an air extracting system with two inlets, one which injects and other extracting. I set the initial velocity matching the magnitude, direction and sense of the injection inlet, but rather opposite to the extracting inlet. The results were very nice even with a quite coarse mesh. I made the simulation as unsteady, laminar and 1000 steps of 0.01s... took only 12mins . All steps exhibited a generally good behaviour of the variables according to qualitative experimental data, so initial velocity wasn't a key factor. Courant's number was also well below 5 in practically every point across space-time.

Post edited by: CAVT, at: 2010/09/09 15:42<br /><br />Post edited by: CAVT, at: 2010/09/09 15:46