## CFD Methodology
### Computational Domain  
The computational domain is a simplification of the bubble reactor consisting of a 2D column. The width of the system is 900 mm and includes a distributed grid located at 200 mm from the bottom side of the reactor, with channels of 18 mm that restrict the air flow at the reactor. Figure 6 represents the main aspects of the computational domain and dimensions. The bottom side of the computational domain is the constant distributed gas velocity inlet (V = 0.1 m/s). The gas phase enters the computational domain and evolves before arriving to the grid channels. The top side is open at constant pressure. Other boundaries in the computational domain are non-slip wall boundaries.  
The mesh is performed by means of a Cartesian-based grid with different embedding local refinements near the region of the grid channels where higher gradients of velocity  
\begin{table}
\begin{tabular}{l l} \hline \hline
**Solver** & **StarCCM+\({}^{\text{\textregistered}}\) v.15.02.007 [31]** \\ \hline Turbulence Model & k-\(\omega\)-SST \\ Physical Models & Multiphase E-E (Air + Water) \\  & Multiple flow regime interaction [32] \\ Time discretization & Implicit; time step = 0.001 s \\ Transient & [0 s, 20 s] \\ Boundaries & Inlet: Velocity Inlet (V = 0.1 m/s; Mass Fraction Air = 1.0 \\  & Outlet: Pressure Outlet (P = Patm) \\ \hline \hline \end{tabular}
\end{table}
Table 1: Main CFD model parameters.  
Figure 6: Computational domain. Mesh and cell refinement around grid.  
are found. Furthermore, a mesh independence study was carried out to ensure accuracy of the CFD calculations by changing the reference cell size from 3 mm to 25 mm (minimum embedding cell size 0.75 mm and 6.25 mm respectively).  
Figure 7 shows the contours of volumetric fraction of water at t = 8 s obtained with the different meshes.  
Coarser meshes show less interaction between phases and the air appears to be diffused in the water. By contrast, finer meshes detect more heterogeneous flow in the reactor, and different scale of bubbles can be observed. Furthermore, these contours show that water column obtained by finer meshes tend to be lower.  
This statement is confirmed when observing the temporal variation of the water column position (Figure 8a). In this Figure, \(\Delta\)z = 0 m means initial position at t = 0 before air injection starts. After 3 s it is evident that results provided by finer meshes lead to final lower water level \(\Delta\)z = 0.25 m. Nonetheless, it is observed that water level trends to decrease after 5 s which should not be expected, since the operation conditions and the height of the reactor are adequate to avoid the water arriving at the top boundary condition. Figure 8b shows the water mass imbalance in the computational domain after 20 s for every cell size mesh. The CFD solver produces a numeric mass imbalance error that increases when reducing the computational cell size. These statements are in accordance with those from other authors [36; 37]. In multiphase flows the computational cell volumes have to be greater than the volume of the liquid for the Eulerian continuum approach to provide reasonable results.  
Therefore, an equilibrium between both features has been reached to achieve the most accurate possible solution. The cell size used in the solver mesh is 18 mm, which is considered a coarse mesh but without reaching cells too small to avoid surpassing 1% of mass imbalance.  
Figure 8: Mesh independence study. (**a**) Variation of water column height. (**b**) Liquid mass imbalance.  
Figure 7: Volume fraction of water. Mesh independence study.