I'm sorry, the trunk version really outputs particle statistics on inlets/outlets. Thanks for suggestion and for the program! Other, statistical, variable (Part_bndy_mass_flux) is still zero, but it doesn't matter because it's not for particular boundary. I just have to mention that the statistics for boundary particle parameters is very desirable because changes of mass flow rate from iteration to iteration is very sufficient due to mechanism used (model particles instead of model tracks). For those who work with coal firing an averaged particle composition on outlets (ash, char, volatiles, moisture) is very important to estimate losses with unburnt carbon (for this case with cyclone it is, naturally, not needed).
Regarding the slowdown. This weekend I calculate the same cyclone geometry on different (simpler) mesh to check the mesh dependence (the same is being done with Fluent now). I used Saturne-5 (trunk version) on my home PC with Ubuntu. First time I started with settings I used earlier and when I woke up and checked the solution "my jaw was almost on the floor" how they say in English
. It was incredibly slow and made up to 2000 "linear" iterations for pressure on each top level (fluid flow) iteration. For linear solver, for all equations "BicGStab2" was selected (as in my case for 4.0 version, I didn't change it) because I remember that this algorythm worked better than default in Version 4.0 in other cases (not a cyclone). When I switched to Automatic linear algotythm for all equations the solver's speed became great and it prodused 4000+ iterations on a 1.0M-cells mesh during 2 days. I understand that I understand nothing in these linear algorythms but I think that there is a difference in them between versions 4.0 and trunk that makes cases good for 4.0 (with BicGStab2) very slow on new version. If an Automatic settigng for linear algotythm will be good for all cases, we can just forget about this slowdown issue.Update
I found some inconsistence in resulting cyclone efficiency calculated with various methods on the same variant.
Method 1: Solver output for particle flow through the outlet (Efficiency=100%*[InletFlow-OutletFlow]/InletFlow).
Efficiency is 87%.
Method 2: Outlet particle flow is a numerical integral of [mean_particle_velocity_Y*mean_particle_volume_fraction*2300] over the outlet section (area) in ParaView (2300 kg/m3 is a particle density).
Efficiency is 94%.
I tried to move the slice for outlet section in ParaView, to switch from particle to gas velocity (it's reasonable for small particles like 10 microns or so), to change the number of iterations for averaging solver's particle flow output (because it "jumps" from iteration to iteration significantly). Results (efficiencies) almost didn't change. At the same time, the integral (in method 2) over the inlet (with Velocity_X) gives very good but not excellent agreement with given boundary flow (1 kg/s is given, about 0.98 kg/s is calculated, this is not the real particle flow, but it makes no sense because the fluid flow is frozen). Solver's particle mass flow for the inlet is absolutely as it should be (1 kg/s).
But this difference in efficiencies matters. What method is more precise, what method should I use in practice? May it be that there is something wrong with average volume fractions and velocities of particles in cells near the outlet, or I use these variables incorrectly? Particles at the outlet are distributed in relatively narrow annular area, mesh cell size is big enough compared with radial size of this area.
Update
I found another issues with particles...
1. Boundary particle mass flow information in listing is only a summary for the type of boundary, while to estimate the cyclone efficiency one needs to know particle flow rates through particular BC. It leaves only one useful method with mean volume parts and velocities in cells that may be not so precise as "real" flow rate calculated by solver. I found it when I introduced another one BC at the bottom of the cyclone to consume (deposit) particles, because, in realyty, there is an outlet for particles (but not for gas).
2. Resulting mass flow through the cyclone outlet is strongly dependent on the particle timestep. I work on mesh dependency study, and for "coarse" mesh with the 0.01s timestep for particles I reached almost steady state where there was very few particles passing through the outlet. But when I switched to 0.003s timestep lots of particles came from the bottom part of the cyclone and went to the outlet, particle mass flow at the outlet was several times higher than at the inlet (because all these particles that didn't leave the domain with larger timestep directed up to the outlet). I understand that the CFD is not so easy, but the user has no any clue to decide is this time step for particles is correct or not. Fluent has special parameter that tells the solver to limit spatial particle step with the size of the mesh cell or part of this size (it uses trajectory approach in steady state mode). With different meshes in Fluent, I have different cyclone efficiencies (92...98%), but not so different as with Saturne...
Update
I was lucky to obtain the reasonable efficiency (86%) with Saturne on a coarse mesh with the time step for particles 0.003s (almost the same as on finer mesh that has 3 times more cells, as I said before, the efficiency was 87% if estimated with outlet flow in listing). In previous case, on finer mesh, gas flow pattern was different and particles tended to be on outer walls of the cyclone. On coarse mesh flow pattern changed in some extent and particles began to go up from the bottom of the cyclone to the outlet. But, in reality, there should be less particles in that bottom region, so I introduced the deposit BC there and obtained "good" efficiency (this BC is not so important for fine mesh case).
But the time-step dependence of particle flow through the outlet, that I described before, is an open question.