## 2 Physical Modelling and Numerical Methodology
### Numerical Simulation
#### 2.1.3 Numerical Methods and Setup  
The numerical simulations in this study were performed using the commercial package ANSYS(r) Fluent (CFD), considering an Eulerian-Lagrangian approach with two-way coupling as the solution method. The Finite Volume Method (FVM) was used for the domain, where the fluid phase is solved for transient and isothermal flow, using the _segregated pressure-based_ algorithm and _semi-implicit method for pressure-linked equations_ (SIMPLE). The transport equations for k and \(\epsilon\) are discretized using a _Second Order Upwind scheme_. This is combined with a correction equation for the pressure derived from the continuity equation and the momentum equation, that is discretized using the PRESTO1 scheme (_Pressure Staggering Option_), which is suitable for flows with strong streamline curvatures. A hybrid initialization was implemented, solving the Laplace equation from the boundary conditions to determine the initial velocity and pressure field. In the simulations, an adaptive time step was used for the fluid phase with a Courant number of 0.5. For the discrete phase, the Courant number is set to 1, and the equation is solved using a Runge-Kutta scheme with the linearized source terms.  
For a proper convergent solution, the admissible local error in the residual (cell level) was set to \(10^{-11}\), and the convergence criterion of the global residual was \(10^{-5}\) for the continuity equation, and \(10^{-6}\) for the other equations. The time interval of the simulation is subject to the following criteria: (i) the difference of the mass flow rate between the pipe inlet and outlet should be below \(10^{-5}\), (ii) stabilisation of the pressure drop along the pipe, (iii) convergence of the average velocity at the pipe outlet, (iv) convergence of \(y^{+}\), and (v) the mass flow rate of uniformly injected particles at the inlet of the pipe is like that at the outlet.  
Explanation and details of the simulation: Once the transport phase flow has been initialized, the ANSYS Fluent temporal integration scheme proceeds with an adaptive time step for a Courant number of 0.5 as mentioned: With the residuals falling, the time step is set at 0.001 until the residuals stabilize in the order of \(10^{-5}\) for the continuity equation and, \(10^{-6}\) for the impulse equation as for the dissipation and kinetic energy equations (the \(y^{+}\) is monitored preventively within the range of the logarithmic layer). Then, a solution period \"\(t_{e}\)\" required to achieve a stable statistical flow is defined, for this the pressure drop in the elbow and the velocity profile in the cross section at the outlet of the pipe are monitored. Once the flow field of the transport phase is resolved, the Lagrangian module or \"DPM\" of FLUENT is attached and continuous injection of particles is started. Said injection continues for a travel time \"\(t_{r}\)\" until the mass flow of particles that enters the domain in each time interval is like that of the output, then, when a \"stationary\" condition is reached in the flow of particles, the statistics--_Data Sampling for Time Statistics_--are collected, for a sampling time \"\(t_{m}\)\" equivalent to two runs of the pipe. It is worth mentioning that the total number of particles inside the pipe when a constant flow is achieved is approximately 550,000 particles (depending on the case). The times used are referential, it should be checked if the five criteria mentioned were achieved. Table 3 contains the times corresponding to the periods described, specific to the case.  
The stability of the numerical calculations, if problematic, was improved by reducing the under-relaxation factor to 0.2 for pressure and 0.5 for momentum [4]. The simulations were parallelized on an Intel(r) Core(tm) i7-7700 CPU @ 3.60 Ghz (8 CPUs), with 8 Gb RAM and NVIDIA GeForce GTX video card 970.