## 2 Numerical and Experimental Methodologies  
### Operational Condition of An Axial Fan Model  
The studied fan was a low-speed axial fan with a backward sweep configuration. Figure 2 presents the axial fan with seven blades and the corresponding geometric model. The axial fan was an automotive cooling fan consisting of a hub, blades, and ring components with radii of 7 mm (r\({}_{h}\)), 17.0 mm (r\({}_{t}\)), and 18.5 mm (r\({}_{r}\)), respectively, from the center to the hub, blade tip, and ring, respectively (Table 1). The fan was operated under a constant rotational speed of 2100 rpm, corresponding to a period of 0.02857 s, equivalent to a low vehicle speed or the idle condition. The cylinder-type computational domain has a height of 401.5 cm in the streamwise direction and a diameter of 219 cm in the radial direction. The length corresponded to 11 times the fan diameter (Figure 3). The fan was placed in the middle of the cylinder domain at a distance of 5.5 D from the upstream and downstream boundaries. Here, D represents the fan diameter. When a computational domain with wave generation is modeled, the waves pass the domain and are reflected from the outlet boundary. The reflected waves disturb the domain and affect the numerical results; they even cause numerical instabilities. For this reason, \begin{table}
\begin{tabular}{c c c c} \hline \hline
**Unit** & **r\({}_{h}\)** & **r\({}_{t}\)** & **r\({}_{r}\)** \\ \hline cm & 7 & 17.9 & 18.5 \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Dimensions of an axial fan with seven blades. Figure 2: The actual product of an axial fan (**a**) and corresponding geometric cad model (**b**). to overcome such a limit at the end of the domain, the non-reflecting boundary condition was introduced in the study that enables waves to exit the domain, or in other words, they allow for wave absorption at the end of the domain. The fan rotated clockwise under an ambient pressure (zero velocity) with a turbulence intensity of 0.2% at the end of the computational domain where the general non-reflecting boundary condition was applied based on characteristic wave relations derived from the Euler equations. The fluid density was treated as ideal gas. The domain consisted of two parts, namely the rotating (small cylinder part) and stationary (large cylinder part) parts. The sliding mesh technique is applied to the rotating part, with one mesh interface zone in the shared faces with the stationary part, where the meshes overlap. The sliding mesh technique is a recommended method for calculating flows in multiple moving reference frames, but it is computationally more demanding compared with the multiple reference frame (MRF) approach, which is suitable for steady state simulations [24]. However, the recently developed deforming mesh technique requires considerable computational resources, and the only unsteady simulation method available for the present study is the sliding mesh technique. Steady state computation was first conducted for approximately 3000 iterations to have a convergence below \(10^{-4}\). Then, in unsteady computation, the steady state flow solution was exclusively used as the initial condition to speed up the convergence. The simulation took approximately 168 h for 13 revolutions when using a desktop computer with a Windows 10 operating system and a single CPU with eight cores. ANSYS FLUENT 19.4 employs a cell-centered finite-volume method based on a multi-dimensional linear reconstruction scheme, which permits the use of computational elements with arbitrary polyhedral topology, including hexahedral, tetrahedral, pyramidal, and hybrid meshes. For the computations presented in this paper, the convective terms and transient formulation were discretised using the bounded central differencing scheme and second order implicit.