[AtoHM]

Hi all. I am investigating flow through a last stage steam turbine and there is a effect I encounter, which I think is explainable and I want to hear your opinion on it.

The actual simulation includes flutter of the turbine blades, but currently I am looking more into pressure perturbation between stator and rotor. Therefore, I created 5 small surfaces in Post, which are positioned between R and S in the same distance and roughly follow the streamlines. 3 are positioned in the rotor domain, 2 in the stator domain.
The point of this is to see if the wake of the stator is visible in the rotor domain, if effects of the rotor passing by the stator are visible in its domain and finally how big these are in comparision to perturbations caused by the turbine flutter. Now, I extracted the average pressure on all these surfaces for a total amount of 240 time steps, which resolves the rotor passing 24 stator blades with 10 steps each. Then I used FFT to process the pressure-curves and here comes my problem.

The 2 areas in the stator domain are stationary, that means they can't inherit any disturbances from the stator itself. From FFT I get a clear peak at the closest frequency to 3250 Hz, which is the machine freq 50 Hz times 65 rotor blades. So, I can see the effect of rotor passing by in the stator domain, which is good. However, when I do this for the rotor-areas, the area right behind the TRS-interface has a huge peak at 3250 Hz as well, where I expected a clear peak near 3000 Hz, because the wake of the stator (60 blades) would be at that frequency. Approaching the rotor, this peaks gets smaller.
I did some research in the modelling guide, where it is stated, that TRS:

As with a Frozen Rotor interface, pitch
change is automatically accounted for by scaling of flows by the pitch ratio

My assumption is, that cfx scales the outgoing flow of the stator to the pitch of the rotor, which effectively increases the actual number of stator wakes seen by the rotor. Scaling one stator to one rotor increases it to 65 "blades" as well and giving me the incorrect frequency of 3250 Hz instead of 3000.

Sorry for the long text, I'd be happy for a second opinion.

[Opaque]

How many passages are you modeling for the stator, and for the rotor?

Have you reviewed the documentation about the treatment for transient rotor-stator inteface, and the modeling guidelines for transient blade row modeling?

Which version of the software are you using?

[AtoHM]

Thx for your reply.

Currently I am modelling 2 passages each, because then I can roughly see the turbine blades at an interblade-phase-angle of 180 degrees, which gives the highest total area-change during one cycle, leading to higher pressure perturbations from flutter. The fluctuations I want to see should be independent of the number of passages modelled, as the wake of the stator should be there anyway.

The quote I used is from the documentation, so yes, I think I checked the important stuff. I do not use Transient Blade Row Modelling, just the frame change/mixing model Transient Rotor Stator. This might be the point, w/o time-shifting or transformation of the profile, it gets scaled and the frequency is changed.

I use cfx 17.1.

[Opaque]

You got it.

If you are running a Transient analysis (Not Transient Blade Row), you are effectively using Profile Transformation and the frequency will be changed on the rotor side. The stator's frequency should be correct.

For flutter calculations you must use either the "equal pitch" configuration, or the Fourier Transformation Transient Blade Row model; otherwise, you are not seeing the correct frequency of the flow on the blade.

For your specific passage count, it seems the "equal pitch" configuration is the full geometry on both sides; therefore, a time consuming calculation. If you use the Fourier Transformation method, you only need the two passages on each row. However, I do not recall the Fourier Transformation method can handle two frequencies on the same geometry (flutter plus stator passing frequency) for ANSYS R17.1.

Besides reading the documentation further, you should contact ANSYS CFX support for additional information.