## 2 Numerical Approach  
The numerical model was developed using a combination of ANSYS Component System ICEM and ANSYS Fluent for the case of flow around a circular cylinder. Due to limitations of the commercial software, no higher order methods could be used for a time-marching solution. Computational grids for two geometries were developed; flow around a cylinder of diameter \(D=20\) mm (Figure 1) and flow around the same cylinder with a cavity embedded within the body and a \(d_{o}=1.0\) mm wide rectangular orifice located at the top of the cylinder perpendicular to the freestream (Figure 2). The cylinder and orifice dimensions were identical to those used in a water tunnel experiment in the research group [23]. As the periodic vortex shedding from the cylinder and the operation of a synthetic jet was time dependent, a time marching solution was applied. An unsteady RANS simulation approach was implemented using the transition SST turbulence model as closure. The \(k-\epsilon\) model preforms well at predicting the behaviour of turbulent shear flows,  
Figure 1: Schematic view of the computational domain and boundary conditions. Figure 2: Schematic diagram of the circular cylinder with internal synthetic jet cavity and pseudo diaphragm, represented by an inlet velocity boundary condition. such as those found in the wake of a cylinder where periodic vortex shedding has been established. Yet the \(k-\epsilon\) model performs poorly when dealing with adverse pressure gradients, such as those found after the separation point on the surface of a cylinder in cross-flow [30]. For a more accurate flow behaviour in the boundary layer, the \(k-\omega\) model can be used. This model has proved reliable in the modelling of two-dimensional boundary layers with both adverse and favourable pressure gradients, decelerating and accelerating flow, making it more appropriate when dealing with separated flows [30; 31]. One drawback of the \(k-\omega\) model is its inability to resolve unsteady turbulent structures and free shear flows, such as those found in jets [32]. The transition SST model combines aspects of these two models and is better adapted at dealing with the flow regimes associated with a cylinder in cross-flow. This is achieved by utilising the \(k-\omega\) model in regions close to the wall boundary and the \(k-\epsilon\) model in the regions away from the wall. It is also more suitable for modelling free shear layers associated with separated wakes and jets [33]. Out of most common RANS turbulence models, the SST model has been shown to achieve vortex-shedding Strouhal numbers closest to those obtained through LES [34]. The semi-implicit method for pressure-linked equations (SIMPLE) scheme was used for the pressure-velocity coupling. The discretised momentum and pressure correction equations are solved implicitly, whereas the velocity correction is solved explicitly, thus resulting in a semi-implicit method. Second order upwind spatial discretisation was used for all variables, in combination with the least square cell-based method for the gradients. Through an iterative design process (Table 1), a computational grid was constructed with results that are independent of the mesh density. For two-dimensional simulations, the expected drag coefficient \(C_{D}\), RMS lift coefficient \(C_{L}^{\prime}\) and vortex shedding Strouhal number \(Sr\) are well established, with respective values of 1.74, 1.42 and 0.26 for flow around a cylinder at a Reynolds number \(Re=3900\)[25; 35]. The works of [PERSON] and [PERSON] [35] and [PERSON] et al. [25] were conducted using DNS and LES, respectively, for a 19-mm diameter cylinder and freestream velocity of 0.296 m/s. To attain the same \(Re\) for the 20-mm diameter cylinder in the present study, the freestream velocity at the inlet is set to a 0.312 m/s. For all cases (both actuated and unactuated), the turbulence intensity at the velocity inlet is set to 5%.