Hi all,

having no experience in turbomachinery related CFD I have some basic questions. As far as I have heard people seldom model the whole rotor and stator using moving grids, which is the most logic way for a beginner (although it might be quite time consuming). Instead they using some kind of rotating coordinate systems. Could someone give some comments what is behind that approach and what errors do I get with that simplification compared to the sliding mesh technique of the whole rotor ? Do I still have to run the job in transient mode ?

Cheers,

Mark

(1). Even for a person like me, several years in turbomachinery, I don't ask such questions at all. (2). In the turbomachinery design, we handle the design piece-by-piece, in a rather idealized way. In other words, when you are dealing with the nozzle (or the stator), you used stationary reference frame attached to the nozzle. In this way, the surface is always stationary, and you can easily apply the boundary conditions. (3). When you move on to the rotor, you use the rotating reference frame rotating with the rotor. In this way, the blade surface is still stationary in the rotating frame, but the inlet boundary conditions must be converted to the rotating frame from the stator exit conditions. The conversion is a very simple vector conversion, with the rotor tangential velocity involved. (4). At theis point, the nozzle exit condition is always averaged in the circumferential direction first, so that it can be used as the inlet condition for the rotor calculation. (5). The design is always steady state, and there is no rotor-stator interaction issue. (5). For small rotor-stator gaps, the leading edge region of the rotor flow will in reality have some upstram effect on the nozzle (stator) trail edge flow field. This effect has been attempted by calculating the multi-stage flow which include the stators and the rotors at the same time, but still under the steady state condition. (6). Whether this type of flow can be done properly is someting else to be studies. (7). The real flow is everywhere 3-D transient. It is possible to simulate such flow field, but the transient 3-D flow is very time consuming, and it is not practical as a parametric design tool yet. (8). Since the turbulence model alone is still not reliable in "most" cases, the real value of such multi-stage calculation is quite limited. It has been used to show that the "clocking" (relative circumferential position of the blade between blade rows) can reduce the loss by a small amount, because of the transient wake and leading edge interaction. (9). So, you have three stages of simulation: (a).from the design side, it is row-by-row steady state calculation, with exit conditions averaged. (b). multi-stage steady calculations, with exit condition averaged. (c). true multi-stage transient calcuations. (boundary conditions between the stationary and the rotating frames of reference must be properly handled. In this case, you have the sliding meshes)

If you think that your rotor and stator are closely coupled then a transient solution is really needed. However there are a couple of work arounds that you could use to avoid waiting 'till Christmas for the answers: a) If you're analysing axial turbomachinery that is radially stacked, running the CFD on a 2D slice (say at mid-span) may be valid (of course you won't get any endwall effects or tip leakage). b) Take advantage of any axisymmetry. If your turbomachine has 40 stators and 60 rotors then you only need to model 2 stators and 3 rotors and add a periodic boundary condition to take account of the rest of the blade row.

comment on (b) it is often the case that the number of blades in an adjacent rotor and stator are relatively prime. meaning that the highest common divisor is 1 (eg 21 and 25). so often the use of periodic bc to reduce the size of the domain is not possible. this is done for structural reasons