## 2 Computational Fluid Dynamics (CFD) Simulations and Flow Model Test (FMT) Experiments
### Computational Fluid Dynamics (CFD) Simulations  
CFD simulations are carried out by ANSYS Fluent 17.1 [28]. On the basis of grid convergence analysis, which is shown in Appendix A, the three-dimensional meshing model is established with the real scale. It ranges from \(-5132\) mm to \(32\),\(008\) mm in the X direction, from \(-11\),\(000\) mm to \(22\),\(489\) mm in the Y direction and from \(-10\),\(155\) mm to \(9465\) mm in the Z direction. The total meshing number is about \(3.85\) million. Hex/Wedge and Tet/Hybrid grids are used to demonstrate the meshing geometry. For simplification, several assumptions are made for the calculation: (1) the model is considered to be adiabatic since the SCR-deNO\({}_{x}\) facility is covered with an aluminum silicate blanket, which works as the thermal insulator, (2) no chemical reaction is introduced, (3) the gas flow is considered to be incompressible fluid, (4) the ash particles are treated as inert particles, and (5) the diameters for \(99.50\%\) of the ash particles are larger than \(2.50\times 10^{-3}\) mm [25; 26; 29]. Accordingly, the Raynolds Averaged Navier Stokes (RANS) equations are used to handle the turbulence and the standard k-\(\varepsilon\) model is adopted. Meanwhile, the semi-implicit method for pressure-linked equation (SIMPLE) algorithm is chosen to solve the governing equations and second order upwind is used as the discretization scheme. The discrete phase model (DPM), which is under a Lagrange framework, is used to track the particle trajectories. The particles interact with the gas flow and the corresponding diameter distribution follows the Rosin-Rammler rule. According to the data in Table 1, the mean diameter and the spread parameter is calculated to be \(3.5\times 10^{-2}\) mm and \(0.79\), respectively. Boundary conditions are given as follows: the facility inlet is set to be velocity inlet with the flow rate of \(4.50\) m/s while the facility outlet is set to be pressure outlet. Moreover, the porous zone model is used to represent the catalyst layers with an inertial resistance coefficient of \(30.85\). In the simulation cases, an observation plane named plane 1 is located \(200\) mm above the catalyst layer \(\#1\) to represent the velocity distribution and particle distribution at the entrance of the catalyst layers. Another observation plane named plane 2 is located at the entrance of turning 2, representing the particle distribution in the vertical duct. To study the ash particle accumulation, CFD simulations are carried out with the arrangement shown in Figure 2. The particle distributions of plane 1 and plane 2 are presented subsequently. Based on the flow field, a triangular deflector is presented and installed in the vertical duct, aiming to disperse the accumulated particles and avoid severe impact on the velocity distribution. The sectional view of the triangular deflector is shown in Figure 3. Two sets of simulations are carried out to determine the optimal geometry of the triangular deflector. The first set is to investigate the optimal angle against the wind. The angle is set to be \(10^{\circ}\), \(15^{\circ}\), \(30^{\circ}\), \(45^{\circ}\), \(60^{\circ}\) respectively, with a fixed height of \(300\) mm. The second set aims to achieve the optimal height of the deflector. The height is set to be \(100\) mm, \(200\) mm, \(300\) mm, \(500\) mm, \(700\) mm respectively, while the angle is maintained at \(15^{\circ}\). The simulation results are compared and analyzed based on the velocity distribution, total pressure loss and particle accumulation. Attempts are also made to investigate the optimal installing position for the triangular deflector in the vertical duct. The deflector is installed at three different heights, as shown in Figure 4. The corresponding simulations are carried out with a low deflector installation, a middle deflector installation and a high deflector installation, respectively.