hallo everybody; I'm trying to calculate centrifugal compresor flow using fluent(one chanel). My question is: what can be the reason of wrong axis of rotation of periodic boundaries. I created per. bound. in fluent using text command. I should add that matching tolerance had to be increased from 0.05 to 50. Grid was created in ICEM CFD grid generator. How fix this problem?

Hi Michael

Matching tolerances should not exceed 0.5.

Are you sure that you set the periodic parameters in ICEM CFD when creating the mesh? I need more info relating to how the grid was created in order to help you. For example, which meshing ICEM CFD application did you use HEXA or TETRA?

In fluent did you set the correct fluid axis for the periodic condition before you used the text command for making the periodic BC.

Mark

Thanks for your interest in this case. Corresponding to Your questions: This is a HEXAhedral mesh. In ICEM CFD 5.0 I have specified In mesh>global mesh settings>definde periodicity> axis of rotatin defined by vector, and angle specified. Aditionally in blocking>edit block>periodic nodes are specifed. Corresponding to the fluent... I didn't set the axis becaouse I don't know how( If I create periodic bouondaries, fluent asks only for: periodic zone[], shadow zone[], rotational? and make periodic? Maybe that's the source of error?

Fluent defaults to a rotaional axis about the z-axis. You can change this in the boundary conditions panel by selecting your fluid zone and redefining the axis to match the required axis for the periodic bc you want to model. This must be done before you use the "make periodic" command.

Good Luck

Mark

Thanks a lot Mark!!! Now it's ok.