## 2 Simulation Framework  
### Numerical Model  
The CFD open source software OpenFOAM(r) (v1912 version) was used to assess the efficiency of the device and perform the simulations. In the discretization of time and space domains for the Navier-Stokes equation, the solver applied the finite volume method using a grid over the fluid domain. For the NWT, the domain geometry was created with the _blockMesh_ utility, which decomposes the domain in hexahedral blocks. For spatial discretization, the standard Gaussian integration by finite volume method was employed, which is based on the sum of the values of cell faces and interpolated from cell centers [26]. For the description of the fluid dynamics, the momentum equation in the volume of fluid (VOF) was defined for both air and water phases, assuming incompressible fluids and laminar flow existed. The Navier-Stokes equation for the conservation of momentum is given by:  
\[\rho\frac{\partial\mathbf{u}}{\partial t}+\rho\
abla(\mathbf{uu})+\
abla p=\
abla\cdot \left(\mu\left(\
abla\mathbf{u}+(\
abla\mathbf{u})^{T}\right)\right)+\rho g \tag{1}\]  
where, according to the Cartesian coordinates \((x,y,z)\), \(\mathbf{u}\) describes the velocity vector field in the fluid, \(\rho\) the density of the fluid, \(p\) is the pressure, and \(\mu\) the dynamic viscosity. Considering the conservation of the mass, the continuity equation for incompressible fluids is described by:  
\[\
abla\cdot\mathbf{u}=0 \tag{2}\]  
and the scalar equation for the water-air phase fraction can be written as:  
\[\frac{\partial\alpha}{\partial t}+\
abla\cdot\mathbf{u}\alpha+\
abla\mathbf{u}_{c} \alpha(1-\alpha)=0 \tag{3}\]  
where \(\mathbf{u}_{c}\) is the compressive velocity. To delimit the free surface in the multiphase flow solver, the VOF method applies parameter \(\alpha\), based on the volume fraction of each phase to differentiate the water and air interface, where \(\alpha=1\) for water and \(\alpha=0\) for the air, and the phase volume fraction \(0<\alpha<1\) represents the cell accommodating the water-air interface.  
In the _InterFoam_ solver, both the fluid and WEC motion are integrated. In each time step, the algorithm of the implicit motion solver updates the position, calculates the forces,and updates the acceleration, and then, moves the object at its new position. In the final step, the solver moves the mesh to accommodate the new changes, relative to the previous time step [27]. After the motion solver is evaluated, the fluid solver begins with the correction of the flow field by means of the VOF method using the multidimensional universal limiter for explicit solution (MULES), which considers a delimiter factor of the flow in the temporal solution. The following step in the procedure is to solve the momentum and pressure equation with the implementation of the pressure implicit method for pressure-linked equation (PIMPLE) algorithm. PISO (pressure implicit with splitting of operators) and SIMPLE (semi-implicit method for pressure-linked equation) algorithms were combined to achieve the PIMPLE algorithm. Within this PIMPLE algorithm, the following time step was begun until the maximum number of iterations was achieved, and this procedure was repeated until the end of the simulation. The complete method is detailed elsewhere [28].