I want to simulate the flow through a centrifugal pump (steady-state). Do I need to assign a rotating wall boundary to walls of the impeller in the rotating zone? If not, would it be wrong (result wise) to do so?
Additionally, what do I do with stationary walls (e.g. casing walls) that are also located in the MRF volume that is necessary for the rotating zone? Do I need to assign a rotating wall boundary condition with a zero velocity (rad/s) to it?
When using an MRF region, everything that is inside the cell zone that you created will be rotated, so it is important that you can create a zone that only includes the rotating parts.
Also, there is no need to assign the rotating faces to Rotating Wall, let them be automatically modelled as No-slip walls by leaving them unassigned
Have a look at the following documents to use as reference:
thank you for your detailed answer. Last week I watched the SimScale webinar about Turbomachinery. As far as I’m aware your US colleague aunni created a rotating zone for a centrifugal pump that also cuts through the stationary casing walls of the pump. Additionally, he defined a rotating wall boundary conditions to all the rotating walls inside the rotating zone.
Is this workflow specific to the new Simerics solver in SimScale?
Anything inside a rotating zone will be rotating - you can verify this by plotting velocities on the post-processor and analyzing the velocities on the walls. In short, if you leave walls inside a rotating zone with “No-slip”, they will already be rotating (as Fillia mentioned).
The second case, where we have a wall that should not rotate but is inside the rotating zone requires caution. Only in this case it’s necessary to define a rotating wall boundary condition with zero angular velocity, otherwise the portion of the wall inside the rotating zone will rotate.
To answer your question: at the moment it’s necessary to define the walls as rotating walls for the subsonic analysis. There will be a patch soon, to apply this condition automatically, so it works exactly like in the OpenFOAM solvers.