CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   FLUENT (https://www.cfd-online.com/Forums/fluent/)
-   -   seggregated and coupled (https://www.cfd-online.com/Forums/fluent/42244-seggregated-coupled.html)

 SEETA September 6, 2006 06:08

seggregated and coupled

hi, i want to solve energy equation along with momentum equatins for my problem. for that i have choosen seggregated solver and i have run the case and solution is converged where as if i choose the coupled solver, when its getting iterating, y and z velocity residuals keeps on increasing and they are comming like 3.084878e+3.... and i have choosen the courent number as 0.5. To solve energy equation, which solver is the best one . to get convergence in coupled solver what parameters i have to modify? or whats making difference with these two solvers? thanks for ur patience..

 Jason September 6, 2006 07:26

Re: seggregated and coupled

The solver choice is dependent on your problem. Search the forum for more information.

The segregated solver is a pressure based solver and works well in the incompressible regime or with large separation regions. It works well in the subsonic compressible regime as well. I've used it with great results through Mach 1.5, but once you start introducing shocks into your system, the segregated solver will try to smooth out the shocks. Refining the mesh at the shock helps this, but it shows that the stronger the shock, the more mesh dependent you will be and the more care you'll have to pay to having a refined mesh at the shock (adaption doesn't always fix the problem either... in fact, I personally have a hard time trusting adapted meshes... I use it as a first guess, then go back and rebuild my mesh based on the results and rerun it).

The coupled solver is a density based solver. The downfall is in the incompressible regime (where density is constant) or in separation regions (where the density changes are negligible). They've made improvements on the standard coupled solvers that help, but I've still never had luck below Mach 0.3.

Fluent introduced a pressure based coupled solver (in Fluent 6.3) that theoretically would fix the problem with the coupled solver in incompressible regimes and separation regions, but I haven't used it, so I can't honestly comment on it.

If you're running Fluent 6.2 or earlier, and your flow is incompressible, then I wouldn't bother with the coupled solver. If you're running with the segregated solver, you can usually speed up convergence by setting your solution limits (solve->controls->limits). Your maximum pressure should never exceed the maximum total pressure you're injecting, but set the limit a little higher than this (to give the solver room to converge). Estimate what you think your minimum pressure would be and set a limit lower than that. Do the same for your temperatures. This should help bound the solver, which tends to lead to a converged solution faster than the default limits.

Hope this helps, and good luck, Jason

 seeta September 7, 2006 01:46

Re: seggregated and coupled

hi jason, tahnk you very much for ur clear explanation.

 All times are GMT -4. The time now is 05:12.