## 2 Validation of the CFD Approach
### CFD Models  
The ANSYS CFX V17 software platform has been used for the CFD simulations. Figure 3 shows the different CFD models which have been tested: in each box the first row describes the analysis type (steady or transient) and the interface option between impeller and diffuser (Stage, i.e., mixing plane or transient), the second row denotes the advection scheme and the third row refers to the turbulence model. The CFX nomenclature is used, in particular, for the advection upwind scheme, which corresponds to a first order accuracy, while high resolution corresponds to a second order accuracy. The turbulence models adopted are the k-\(\omega\), the SST and the model k-\(\varepsilon\) with scalable wall functions. The following boundary conditions have been set: inlet total pressure and temperature (\(\mathrm{T_{t}}\,\mathrm{ln}\), \(\mathrm{P_{t}}\,\mathrm{ln}\)), inlet turbulence intensity (5%), outlet mass-flow rate and a uniform impeller rotational speed. The mass flow rate at the exit boundary has been set, instead of the usual static pressure, because the analyses have been performed far from the choking condition. Moreover, a circumferential periodicity has been fixed because the model includes only a sector of the compressor, consisting of two impeller channels and three diffuser channels. Finally, all the solid walls have been modelled as adiabatic with no slip condition. Figure 2: Mesh details of [convergent duct + impeller] (left) and diffuser (right). Two operating conditions have been simulated: point M (close to design) and point P1 (close to surge). The numerical simulations for the operating point M did not show stability problems. On the other hand, point P1 has been investigated with different models because of numerical instabilities in the original CFD settings. The activation of the turbulence model k-\(\omega\) turned out to be necessary in order to dampen the instabilities. In Figure 3 a sketch of the simulation dataset for both operating points is shown. Steady models have been validated after comparing the area averaged numerical results with the corresponding experimental results along the measurement planes, 2M and 7M, as suggested by [PERSON] [24]. In all the simulations, a maximum error lower than 5% for the main averaged flow quantities (p, p\({}_{t}\), T\({}_{t}\), Ma, \(\alpha\)) in the above sections has been obtained with respect to the experimental data. The only exception concerns the results with the model HR-SST in the operating point P1, where a stall cell appeared in one of the three diffuser channels and errors for Mach number and flow angle are much greater. The simulation interested by the stall has one low-velocity channel and two channels with high velocity (because of redistribution of mass flow), as shown by the contours of Mach number in Figure 4. No stall is calculated if, in the operating point P1, a turbulence model k-\(\omega\) is used. The stall simulated in P1 with the model HR-SST induces an additional energy loss that is the cause of a lower pressure ratio at the diffuser exit, as shown in Figure 5, where the predicted overall performance is compared with experimental data. However, it must be considered that the stall in a three-diffuser vane model has a much greater relative effect on the performance than it would have in a complete model. This occurs because the mass flow redistributes over three channels rather than over the whole annulus, giving a more relevant change in incidence angle to the blade channels involved. Transient simulations have been validated by checking that both area-averaged and local results had their time-averaged values close to the corresponding values from steady analysis. Several monitoring points have been defined at the same probe positions of the measurement devices. The stall by adopting the turbulence model HR-SST in P1 is still present in the transient calculation and is confirmed inside the same diffuser vane.