# Evaluation of Three-Dimensional Environmental Hydraulic Modeling in Scour Hole
## 2 Methodology
### Numerical Study
#### 2.2.3 Numerical Setup  
To achieve the best comparison between the two models, the numerical study settings in OpenFOAM and Fluent were selected as similar (as shown in Table 2). A computational mesh that resembles the laboratory experiment was created by OpenFOAM and converted to mesh input file of Ansys Fluent (Figure 2).  
\begin{table}
\begin{tabular}{c c c c} \hline \hline \multirow{2}{*}{**Model**} & \multirow{2}{*}{**Turbulent Model**} & \multirow{2}{*}{**Pressure Scheme**} & **Velocity/Turbulence** & **Pressure-Velocity** \\  & & & **Scheme** & **Coupling** \\ \hline \multirow{2}{*}{OpenFOAM} & \multirow{2}{*}{\(k-\omega SST\)} & second-order (GAMG) & second-order \\  & & & (smoothSolver) \\ \hline \multirow{2}{*}{FLUENT} & \multirow{2}{*}{second-order (PRESTO)} & second-order (-) & \\  & & & \\ \hline \hline \end{tabular}
\end{table}
Table 2: Setup of numerical models.  
The domain of numerical study was set same as the laboratory experiment setup, which was 12.5 m in length and 0.6 m in width. To optimize the calculation results near the wall, the mesh was gradually set to refine toward the bottom. Additionally, the grid size in the scoured area, where the flow is supposed to be complicated, was also created smaller to enhance the results. Moreover, a study about the grid size and the time step convergence were conducted to select the appropriate parameters, as is always recommended [8,9]. This step helps to reduce the errors from the discretization. To get an optimal combination of the two parameters, the simulation results from three different grid sizes (accounting for the first cell from the wall) of \(\Delta z\) = 1, 1.5, and 3 mm (\(\Delta z/h_{0}\) = 4.7 \(\times\) 10\({}^{-3}\), 7.0 \(\times\) 10\({}^{-3}\), 1.4 \(\times\) 10\({}^{-2}\)) and three different time steps increase from \(\Delta t\) = 1.0 \(\times\) 10\({}^{-5}\) to 1.0 \(\times\) 10\({}^{-4}\) and 1.0 \(\times\) 10\({}^{-3}\) s, which are compared in Figure 3. Here, the horizontal velocities \(u_{x}\) were collected at 4.5 m downstream. The result indicates that the time step of \(\Delta t\) = 1.0 \(\times\) 10\({}^{-4}\) s and grid size of minimum \(\Delta z\) = 1.5 mm (close to the wall boundary) and maximum of 10 mm (near the atmosphere boundary) are sufficient to produce the results within 0.1% of the higher resolution cases.  
All of OpenFOAM simulations in this present study were operated with the pisoFoam module, a transient solver for incompressible flow with many choices for turbulence  
Figure 3: Grid size and time step convergence.  
Figure 2: Schematic model setup and mesh grid (not to scale).  
simulation. The Gaussian integration with different interpolation schemes was applied for the spatial discretization of differential operators. The second-order linear interpolation was used for the gradient terms. The linear corrected interpolation method was applied for Laplacian terms. The limited linear interpolation was employed for the divergence terms. The GAMG solver with Gauss Seidel smoother was used for pressure, and the smooth Solver 177 with Gauss Seidel smoother was applied for velocity and turbulence. The pressure-velocity coupling was calculated by the Pressure Implicit with Splitting of Operators (PISO) method, which is an efficient approach to solve the Navier-Stokes equations in unsteady problems.  
In Fluent simulations, the PRESTO scheme was used for pressure, while the second-order scheme was applied for velocity and turbulence. Similar to OpenFOAM, the PISO method was employed for the pressure-velocity coupling calculation. The under-relaxation factor of 0.5 was used for pressure, momentum, and turbulent quantities to avoid the divergence of numerical simulations and archive the full convergence.