[PatLe]

Hello together,

i started a new project formy university, so i have to do particle tracking with CFX in a turbine. I never did particle tracking before, so i have some questions.

1. Which kind of interface would you recommend between rotor and stator for a steady state simulation? Normaly i would choose the stage interface, but for the particle tracking the stage interface doesn't seem to be that useful for me because of the circumferential averaging, i think the particles will exit the interface at a random circumferential position so i would choose the frozen rotor

2. Have you any ideas for the post processing? I'm mostly interested in the particle behavior at the blades. I set an equation dependent wall intersection at the blades with a perpendicular restitution coeff. of 0.1, so my particles would bounce of the wall. I want to know the particle impact velocity and the impact angle at the wall, but haven'tfound any option to get this information. I would also be nice to create an contour plot to see the particle impact regions at the wall, but i haven't found a useful variable. Any ideas how i could get these information.

Thank you very much for your help.

[Gert-Jan]

1) Frozen Rotor.
2) You can read out particles that end on a boundary (R=0). Look for Output Control > Export. You'll obtain a .csv-file with variables you select, like velocity.

Mind that when you take out particles (R=0), they no longer influence the flow, so this make a fully coupled calculation troublesome. Especially when you have multiple rows with blades. A work around is:

Define 2 types of particles in one calculation. The first type is the bulk of particles, fully coupled, that bounce off everywhere with a coefficient you like above 0. Since these are fully coupled, these determine the path of the gas through your geometry.

The second type of particles is just for postprocessing. It has the same properties as the first type, but are only one-way coupled (The amount of mass does not matter). These particles are released at the end of your CFD calculation, after your first type of particles has set the velocity field fully coupled. The second type of particles will follow this flow field.

Let the second type of particles end (R=0) where ever you want to determine their impact, using the export file as given above.
You can make as many sets of particles as consecutive rows with blades you have.