# CFD Analyses: The Effect of Pressure Suction and Airflow Velocity on Coronavirus Dispersal
## 2 Material and Method
### CFD Setup  
The CFD simulation was performed with the ANSYS 2020 CFX package [26] using a virtual machine with computational capabilities of Processor Intel\({}^{\circledR}\) Core\({}^{\text{TM}}\)Y-7700 CPU @ 3.6 Hz, installed memory: 32 GB, system type: 64-bit operating system. The corresponding computational time was approximately 12 h/case of study. The geometry of the building was modeled and then loaded into ANSYS. The model was created using the Boolean algorithm (i.e., the solid domain is subtracted from the fluid domain). The use of this approach is essentially warranted for aerodynamic or fluid dynamic studies [27]. Thus, it was used in our study. Figure 2 shows how the mesh of the model was created using about \(16\times 10^{6}\) components. Figure 1: The geometry and specifications of the emergency department. Figure 3 shows how the number of elements was determined following mesh sensitivity analysis to guarantee that the findings were independent of the mesh size. The mesh sensitivity study was carried out using average velocity across a plane with an offset of 1.7 m from the floor, which is around the height of an average person in the Middle East region [28]. At around \(1.4\times 10^{6}\) elements, the findings become indifferent to mesh size, as seen in Figure 3. As a consequence, any mesh size larger than \(1.4\times 10^{6}\) is justified in order to ensure that the findings are independent of the mesh size. A mesh size of \(16\times 10^{6}\) elements was used for the simulation to give a better level of confidence. Furthermore, the mesh quality (Table 1) is consistent with previous findings in similar studies [29; 30; 31; 32]. The mesh was then exported to the CFX-PRE to specify the needed configuration, which corresponded to the study's scenario. Figure 3: Mesh sensitivity analyses with respect to the average velocity at 1.7 m offset. Figure 2: CFX mesh of the model. The k-Epsilon model was used to designate the analysis type as steady state. The fluid domain was chosen from the ANSYS models library as 'Air at 25 \({}^{\circ}\)C.' The model's solid domains were designated as 'No Slip Walls.' It should be noted that the goal of this study is to examine the worst-case scenario of COVID-19 dissemination, which, according to the World Health Organization (WHO), is fundamentally more severe in confined regions [8]. As a result, this simulation was run with the assumption that closed entrances were defined as 'No Slip Walls'. Finally, all of the inlet boundary conditions were set to velocity inlets with a turbulence intensity of 5% by default. The outlet boundary conditions, on the other hand, were all set to pressure outlets of 0.85 bar, which corresponds to the suction condition. As shown in Figure 4, the model converged with residual targets of \(1\times 10^{-3}\). The turbulence kinetic energy (\(k\)) was used to define the flow mixing level, according to the literature [33; 34; 35]. The turbulence kinetic energy (\(k\)) was chosen as a determinate parameter for this work since the degree of COVID-19 spread is strongly reliant on the level of flow mixing. Equations (1)-(4) [33; 34; 35] were used to plot the turbulence kinetic energy (\(k\)) in ANSYS CFX. \[k=\frac{3}{2}(UI)^{2} \tag{1}\] \begin{table}
\begin{tabular}{c c} \hline
**Property** & **Value** \\ \hline Elements maximum size (mm) & 100 \\ Number of elements & \(16\times 10^{6}\) \\ Growth rate & 1.2 \\ Defeature size (mm) & 0.5 \\ Curvature minimum size (mm) & 1 \\ Curvature normal angle (degree) & 18 \\ Skewness & 0.8 \\ Inflation transition ratio & 0.75 \\ Inflation number of layers & 5 \\ \hline \end{tabular}
\end{table} 
Table 1: Mesh properties. Figure 4: Convergence results. \[\varepsilon=c_{\mu}^{\frac{3}{2}}k^{\frac{3}{2}}l^{-1} \tag{2}\]  
\[I=0.16 Re^{-\frac{1}{8}} \tag{3}\]  
\[l=0.07L \tag{4}\]  
The results are displayed as 3D streamlines for the full fluid domain.