# Optimization of Customized Industrial Pneumatic Nozzle to Reduce Noise Emissions
## 2 Materials and Methods
### CFD Analysis  
The software ANSYS Fluent 2022/R2 was used to implement the model for conducting the CFD analysis on the nozzle presenting the higher air consumption. The geometry of the fluid domain was the same as that presented in Figure 4, but two additional cylinders were added above each final duct to simulate and calculate the flow characteristics in the area just outside the nozzle considered for the analysis. This was because the noise was generated in that region; hence, the jet power and range should be estimated for that region. The additional cylinders were 20 mm long and 7 mm in diameter. These dimensions were defined such that the flow could fully develop along the width and length without boundary constraints. The final mesh of the fluid domain for the CFD analysis of the actual model is shown in Figure 6.  
The present analysis was performed by investigating the fluid domains of different nozzles after applying some changes in the geometry with respect to the reference nozzle  
Figure 5: Pneumatic scheme of the test bench. Figure 6: Mesh of the fluid domain for the CFD analysis. actually in use, whereas the boundary conditions and dimensions of the additional cylinders were kept constant during the entire analysis. In addition to the reference model (Figure 4), eight other models were created by increasing or decreasing the length or diameter of the final ducts or main duct one at a time. In Table 1, each model is described and compared with the actual model, which is the reference model (R). The objective of the first analysis was to establish the successful geometry from the point of view of the emitted noise. Therefore, the meshing technique and dimensions of the meshing elements of all the models were kept constant (\(6\times 10^{-4}\) m for the final ducts, \(4\times 10^{-4}\) m for the additional cylinders, and default dimensions for the other regions that were less relevant to the analysis). The model created with the geometry of the reference nozzle actually in use has a mesh with totals of 42,810 cells, 120,048 faces, and 35,287 nodes. All the other models, because they have different geometries, have different numbers of nodes, cells, and faces, but the order of magnitude remains the same. The model for a real viscous fluid \"SST (shear stress transport) k-omega\" was chosen [14]. The boundary conditions were the same for all the models and were set as follows: The mass flow inlet on the inflow surface of the main duct (blue arrows in Figure 7) was equal to the experimental inlet at the supply pressure of 0.5 bar. The pressure outlet at the boundary surfaces of the extra cylinders was equal to the room-gauge pressure, which was 0 bar (red arrows in Figure 7). Impervious walls were used on all the other surfaces, with a null roughness height, because it has been verified that its relevance is negligible (a difference of 500 \(\upmu\)m in the roughness height causes a variation of just 7 m/s in the peak speed). This first set of simulations allowed for a comparison of the estimated experimental speed with the simulated value, as well as for the identification of some promising models that were used to conduct the next simulations. \begin{table}
\begin{tabular}{l c c c c c c c c c} \hline \hline
**Model No.** & **R** & **M1** & **M2** & **M3** & **M4** & **M5** & **M6** & **M7** & **M8** \\ \hline Additional cylinder length (mm) & 20 & 20 & 20 & 20 & 20 & 20 & 20 & 20 & 20 \\ Main duct diameter (mm) & 8.7 & 8.7 & 8.7 & 8.7 & 8.7 & 8.7 & 6 & 8.7 & 8.7 \\ Final duct diameter (mm) & 2.5 & 2.5 & 4 & 2.5 & 1.5 & 2.5 & 2.5 & 2.5 & 2.5 \\ Main duct length (mm) & 24.15 & 24.15 & 24.15 & 24.15 & 24.15 & 24.15 & 24.15 & 18.15 & 34.15 \\ Final duct length (mm) & 17.7 & 27.7 & 17.7 & 9.7 & 17.7 & 17.7 & 17.7 & 17.7 \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Geometric parameters of the models for the CFD analysis. Figure 7: Boundary conditions; inlet in blue, outlet in red.