# Modeling Polymer Microencapsulation Processes Using CFD and Population Balance Models
## 2 Materials and Methods
### CFD Simulation Strategy  
A geometrical model of the experimental setup for the simple emulsion microencapsulation process was constructed using Ansys DesignModeler. The rotor and stator sections of the agitator were modeled as separate volumes connected through a numerical interface, enabling the use of an MRF approach for the rotational frame during the CFD simulation setup. A tetrahedral mesh was generated using Ansys Meshing, with a global average element size of 0.4 mm for the entire domain. To ensure mesh independence, the surface meshes of the agitator rotor and stator walls were successively refined. Steady-state MRF CFD simulations were conducted using water as the operating fluid, with the agitator rotation speed set to 15,000 rpm. The rotor blades' torque was recorded for each case and used as the mesh convergence criteria. The selected mesh (Figure 3), meeting mesh independence requirements, consisted of approximately 6400 kEl, with a local average element size of 0.1 mm, and a growth factor of 1.2 for the agitator surfaces and 0.4 mm for the tank domain. Details on the mesh construction process and independency analysis can be found in [59]. Figure 3: Details of the computational mesh generated. Figure 2: Example of SEM images obtained for the experiments. Ansys Fluent 2020 R2 [60] was used to generate the CFD model, set up for a turbulent, steady-state flow. Following the suggestions of [PERSON] et al. [41; 42; 43], a MRF approach was utilized, with rotor blades' rotational speed set between 5000 and 15,000 rpm to replicate experimental conditions. The model employed a realizable \(k\)-\(\varepsilon\) model with a standard wall function to account for turbulence, and a Eulerian implicit approach was selected for the multiphase modeling. Additionally, a discrete PBM with five particle size bins was implemented, using [PERSON]'s model as the breakage kernel [4] and a turbulence aggregation kernel [60]. Table 2 details the numerical setup for the CFD model, and Table 3 summarizes the governing equations for the relevant models used in the CFD simulations. To validate the CFD + PBM simulation strategy, a model was constructed to replicate the study by [PERSON] et al. [41], which experimentally and numerically investigated a 15% \(v/v\) Conroe oil-water emulsion system at rotational speeds of 300, 400, and 600 rpm. As shown in Figure 4, there is a good agreement between the experimental results reported by [PERSON] et al. and the outcomes of the CFD model, demonstrating the model's accuracy in simulating the emulsion system and its reliability for predicting droplet size distributions in emulsification processes. \begin{table}
\begin{tabular}{l l} \hline \hline
**Parameter** & **Value** \\ \hline Solver & Pressure based, double precision \\ Viscous model & Realizable \(k\)-\(\varepsilon\) \\ Standard wall function \\ Multiphase model & Eulerian implicit \\ Population balance model & Discrete \\ Pressure-velocity coupling algorithm & SIMPLE \\ Discretization methods & Standard \\ Pressure & First order upwind \\ Momentum; Turbulence; Phases & \\ Under-relaxation factors & 0.3 \\ Pressure & 0.5 \\ Momentum; PEI bins & 0.5 \\ Turbulence kinetic energy & 0.8 \\ Turbulence dissipation rate & 0.7 \\ Residual convergence criteria & \textless{}0.001 \\ \hline \hline \end{tabular}
\end{table} 
Table 2: CFD model numerical setup.