# Current Limitations for Predicting Liquid Dispersion in Continuous Flow Bubble Columns Using CFD
## 2 Materials and Methods
### CFD Simulations  
The numerical simulations were performed using ANSYS Fluent(r) 16.2 software (Ansys, Inc., Canonsburg, PA, USA) on an HP Z840 workstation (HP Inc., Palo Alto, CA, USA) with two Intel(r) Xeon(r) CPU E5-2670 v3 2.30 GHz processors and 128 GB of RAM. ANSYS Fluent uses the fundamental governing equations of fluid dynamics, which include the continuity equation, Navier-Stokes equations for momentum, and the energy equation (for compressible flows). ANSYS DesignModeler(r) was used for the 3D drawing of the bubble column. The CutCell (ANSYS Meshing(r)) assembly method was employed to obtain a mesh aligned with the flow direction. Several meshes were compared. They were generated by increasing the number of cells and using the \"inflation\" method of decreasing the size of cells in the direction normal to the wall. The result was a finer mesh near the wall. Details of the meshes are provided in the Supplementary Materials (Table S1). Grid-independent meshes were obtained for each scheme by observing the velocity profiles for air and water. For RANS models (using \(k\)-\(\varepsilon\) and E-E), the mesh had 3.9 \(\times\) 10\({}^{5}\) cells (maximum size 3.2 \(\times\) 10\({}^{-2}\) m). For LES models (using scale-adaptive simulation, SAS, and VOF), the mesh had 6.9 \(\times\) 10\({}^{5}\) cells (maximum size 1.6 \(\times\) 10\({}^{-2}\) m). Convergence was checked by comparing  
Figure 1: Geometric details of the bubble column, the air sparger, the liquid distributor, and the tracer injection port (**A**). Depiction of the optimum mesh (mesh of 6.9 \(\times\) 10\({}^{5}\) elements) (**B**). the residual at an iteration of a timestep with the residual at the beginning of the timestep (residuals below \(10^{-5}\)). The turbulence models included the standard \(k\)-\(\varepsilon\), realizable \(k\)-\(\varepsilon\), RNG \(k\)-\(\varepsilon\), SST, SAS detached eddy simulation (DES), and LES. Default configurations of the turbulence models in Fluent were used in the simulations. The turbulence models and the solution methods (discretization) are summarized in Table 1. Several turbulence models included in ANSYS Fluent(r) were first compared for tracer dispersion in single-phase water flow (no air sparging). Achieving a uniform tracer distribution through all the holes of the liquid distributor was essentially impossible; therefore, tracer injection was simulated exactly as in the validation experiments. The physical properties of fluids have been included in Table 2. The tracer inlet was included within the liquid inlet tube (Figure 1A). The inlet was defined as a mass flow inlet with a constant mole fraction of H\({}^{+}\) (tracer) depending on the pH of the inlet water. The duration (\(t_{i}\)) of the tracer injection pulse was 2.5 s, and the hydrochloric acid tracer injected had a H\({}^{+}\) mole fraction (\(x_{i}\)) of 0.2246 (Table 3). The tracer concentration was monitored in several positions by defining point surfaces at the locations where the pH electrodes were situated and monitoring these surfaces. Data for every time step was saved (\(t\) = 0.01 s). For the two-phase flow study, two experimental conditions with different extreme flow rates of water and air were simulated (Table 3). The air sparger was also defined as a mass flow inlet. The column outlet was defined as a constant atmospheric pressure outlet (1 atm), and no-slip conditions were assumed at the walls. The superficial velocities of air (\(u_{a}\)) and water (\(u_{w}\)) were calculated based on the cross-sectional area of the column. Convergence was assumed if the residuals were smaller than \(10^{-5}\) at each time step.