Fluent 6.2: How to solve a leakage case with long narrow channels and gaps 2nd order without babysitting
The attached figure <a target=_blank href="http://www.fluentusers.com/support/solutions/1122/solution.pdf">http://www.fluentusers.com/support/solutions/1122/solution.pdf</a>http://www.fluentusers.com/support/solutions/1122/solution.pdf shows a typical geometry encountered when one is interested in leakage flow in turbomachinary etc. One faces multiple inlets/outlets, larger volumes connected by multiple narrow gaps and long narrow channels (order of 1000 smaller diameter than the other elements). The pressure difference between in and outlets are moderate to large and it is problematic to propagate the solution quickly through the narrow flow passages due to the fine, high aspect ratio mesh in the channels. This is a challenging problem for multigrid solvers. (1) solve/control/limits: Set the solution limits close to the expected max and min values of the solution. (2) solve/initialize/initialize: Initialize solution from one of the inlets. It is not critical which one is chosen since the subsequent fmg (full multigrid initialization) will propagate and smooth the initial solution field. (3) TUI: solve/initialize/setfmginitialization: max. allowable levels 5 (default). Use the default residual (0.001), however increase the number of cycles ideally to the point where convergence is achieved on each level (especially coarse levels). Often this is about 10 times the default values which one can afford in 2d cases (careful for 3d cases!). Also set verbosity to yes (so the latter convergence can be monitored) and go with the default Courant number (0.75). (4) TUI: solve/initialize/fmginitialization Choose yes. The initialization can take several minutes, depending on the size of the case. Monitor convergence and eventually increase the number of iterations (step 3) and repeat initialization (step 2, 3 and 4). (5) Once you are satisfied with the initialization save cas and dat file. Solve/iterate/iterate. If you get convergence (or fluent does not blow up (amg error) you are all set, otherwise consider points below. (6) Read back saved cas and dat file. solve/control/multigrid: Set verbosity to 1. This enables to monitor if the solutions converge sufficiently on the multigrid levels. Iterate 1 iteration. Especially pressure has to be monitored. In many cases the pressure does not converge sufficiently and increasing the "max cycles" to 60 while decreasing the termination criterion for pressure to 0.01 helps. (7) solve/iterate/iterate does the problem seem to converge now? is the convergence of the pressure equation in the amg (step 6) better? If you think it might work now turn off verbosity and let it iterate. If not work with the momentum equations in solve/control/multigrid similarly to what has been done with the pressure equations. This last step hardly ever is necessary. 

