[Julian121]

I have heard different ways of detecting stall in numerical simulations from my colleagues. I wonder which one is correct. Here, stall is used to refer rotating stall or surge instabilities.

1- static pressure at outlet / total pressure at inlet should drop at stall

2- total pressure at outlet / total pressure at inlet should drop at stall

3- simulation should diverge and CFX should stop

4- sometimes it is written as the last stable point in papers

Personally, when I reduce mass flow rate, both total pressure at outlet / total pressure at inlet and static pressure at outlet / total pressure at inlet increase until a point is reached, where further decrease in flow rate would cause a significant drop in those pressure ratios.

Sometimes, however static pressure at outlet / total pressure at inlet drops sooner than the total pressure at outlet / total pressure at inlet.

Should the reduction in both pressure ratios happen simultaneously to be considered as stall point or when one of them starts dropping is a sign of stall?

[Jiricbeng]

Detection of surging point / stall point operation is a difficult problem and you need a correlation with experiment. There are several more factors indicating the surge point, e.g. axial velocity at the impeller inlet, temperature rise at the impeller inlet or oscillation of the monitored values.



I would not rely on the facts that decreasing both pressures should indicate stall etc. Indication in terms of absolute values needs enough experimental data to correlate. If you performed optimization (impeller meridian shape, diffuser shape, diffuser vanes, spiral...) you could use these parameters for the relative comparison, however in terms of absolute values you need the correlation with experiments to find the parameters for your CFD setup.

[Julian121]

Originally Posted by Jiricbeng

Detection of surging point / stall point operation is a difficult problem and you need a correlation with experiment. There are several more factors indicating the surge point, e.g. axial velocity at the impeller inlet, temperature rise at the impeller inlet or oscillation of the monitored values.

I would not rely on the facts that decreasing both pressures should indicate stall etc. Indication in terms of absolute values needs enough experimental data to correlate. If you performed optimization (impeller meridian shape, diffuser shape, diffuser vanes, spiral...) you could use these parameters for the relative comparison, however in terms of absolute values you need the correlation with experiments to find the parameters for your CFD setup.

What type of correlation should I be looking for? Could you give me an example?

I have full experimental data except velocity measurement.

The compressor I am simulating is prone to stall at the tip. At stall point, is it expected to have negative or zero axial velocity near the tip?

You mentioned that oscillation of the monitored value can be used to indicate stall point. Can axial velocity at rotor inlet for example be used for this purpose?

I have calculated axial velocity and temperature at the inlet of the rotor. The location of the measurement is shown in the photos. Based on these numbers, axial velocity is decreasing but does it show stall inception? Should they be measured at the rotor leading edge plane?

[Jiricbeng]

I am sorry for a late response. I know that axial velocity can indicate surging point if the velocity profile near shroud (maximum radius) is negative. The negative axial velocity near shroud at the impeller inlet may initiate surge at rotor blade leading edge. However, it could be a good tool for a relative comparison at constant operation point to see what is going on with axial velocity when changing geometry for example. But based on your data, the integral value of axial velocity just correlates with decreasing mass flow. Focusing on the profile shape could be a bit more beneficial. It should be therefore rather measured near impeller leading edge shroud to obtain "some number".



I know that impeller inlet temperature rise should be presented when reaching surge point. However, I had the very same experience, there is no sensitivity to temperature, similairly as your data.



I had quite good experience with the oscillations of the monitored value during analysis. As I was getting closer to surge point, the monitored values (efficiency, compression ratio) started to oscillate, but of course not always, although I was at surge point. Do not forget to have a look at the velocity across diffuser, sometimes you may encounter a stall area rotating circumferentially in diffuser channel even in steady state mode (depending in which iteration you stop the analysis).

[TurBoris]

What would be the most appropriate exit boundary condition for full-wheel transient rotating stall simulation in CFX ? Is using mass flow outlet BC for such a simulation mathematically correct ? In literature, choked nozzle (supersonic outlet) is used for rotating stall simulations, however this requires remeshing the geometry for throttling mass flow rate since the mass flow rate is adjusted by reducing nozzle diameter (outlet area).

[Stel]

Originally Posted by TurBoris

What would be the most appropriate exit boundary condition for full-wheel transient rotating stall simulation in CFX ? Is using mass flow outlet BC for such a simulation mathematically correct ? In literature, choked nozzle (supersonic outlet) is used for rotating stall simulations, however this requires remeshing the geometry for throttling mass flow rate since the mass flow rate is adjusted by reducing nozzle diameter (outlet area).

I believe that the Exit Corrected Mass Flow Rate outlet should be appropriate for this. I mean, at least in theory, because for me it turns out to be very hard to get good convergence with this, so I always end up using something else.