## 2 Experimental and Numerical Setup
### Numerical Setup  
The CFD simulations were made using commercial software Ansys Fluent 19.2. Four basic geometries, each representing a different level of simplification, were used: a 2D axisymmetric model, a 3D periodic model without inlet port, a 3D periodic model with  
Figure 2: The typical high-speed image with measured positions. inlet port and a full-scale 3D model with three inlet ports. The 2D axisymmetric model with the swirl component is the simplest approach but is widely used, see Figure 3 left. Note here that the inlet velocity has to be set to conserve the mass flow rate in the radial direction and conserve the angular momentum in the tangential direction. As it is later shown in this paper, this approach underestimates the swirl velocity magnitude. Thus, the second option used here is to set the mean velocity inside the inlet port, \(v_{p}\), as the swirl velocity. The geometrical design of the atomizer allows for the use of periodic boundary conditions, since the atomizer can be divided into three identical parts, each 120\({}^{\circ}\) section. In this way, the 3D periodic model was created. Two periodic models are compared. The first one contains the inlet port (Figure 3 right) and the second one is without the inlet port, a no-port version. The main advantage of the no-port version is simplicity in the mesh generating process. The tangential connection of the port creates skewed elements near the swirl chamber wall. This could be overdone by slight displacement of the port towards the atomizer centreline or using the unstructured tetrahedral or polyhedral mesh. The pressure outlet was set to the outer boundaries and the no-slip condition was used on the internal wall boundaries for all cases. For the turbulent models, the value of turbulence intensity of 1% and hydraulic diameter of 4.9 mm were set on the inlet. Pressure-velocity coupling was performed using the PISO scheme for the transient solution and the pseudo transient Coupled scheme for the steady solution. Turbulence and momentum used Second-Order Upwind discretization. The liquid-air interaction was captured by a Volume of Fluid model with a geo-reconstruct scheme for transient models or a Compressive scheme for the steady cases and LES. Surface tension between air and liquid was set as a constant value. The air was treated with constant density. The gravity force was also considered. The transient solution used variable time stepping with a Courant number of 0.15. A typical time step size was approximately 2 \(\times\) 10\({}^{-6}\) s. After reaching a quasi-static solution, time averaging was applied, with a minimum of 0.1 s recorded. Several turbulence models based on a Reynolds-averaged Navier-Stokes (RANS) equation, LES and laminar solver, which solves directly the Navier-Stokes equations, were used and compared to achieve results comparable to the experiment. The governing equations of the used methods and models are well known and can be found elsewhere [27]. Simple two-equation models represented by \(k\)-\(\varepsilon\) and \(k\)-\(\omega\) were chosen for their good accuracy and versatile use for industrial applications. These models determine a turbulent length scale and a time scale by solving two separate transport equations. The \(k\)-\(\varepsilon\) model is based on a transport equation for turbulent kinetic energy \(k\) and dissipation rate \(\varepsilon\). In this paper, the RNG and realizable \(k\)-\(\varepsilon\) models were used. The wall treatment was performed  
Figure 3: (**Left**): The 2D mesh. (**Right**): The 3D periodic mesh with inlet port. using the scalable wall function for meshes without a boundary layer and Enhanced wall treatment (WT) was used for meshes with a boundary layer. The \(k\)-\(\omega\) SST model with low \(Re\) correction was used with meshes with boundary layer only. This model combines the standard \(k\)-\(\omega\) model for near wall treatment and the standard \(k\)-\(\varepsilon\) model in the free stream flow.