# Dust Dispersion Characteristics of Open Stockpiles and the Scale of Dust Suppression Shed
## 2 Numerical Methods
### Numerical Models
#### 2.2.2 Simulation Setup  
The whole process of simulation was inseparable from computational fluid dynamics (CFD). CFD is a more convenient and economical option for solving complex problems in  
Figure 1: Distribution of geometry.  
Figure 2: Flow field distribution at \(Z=75\) m.  
practice. CFD can provide a theoretical basis for the actual layout of the yard framework. The CFD method consists of the following steps: (1) pre-processing, (2) selection of the solver and setting of the computational model, and (3) post-processing. The pre-processing is mainly concerned with the construction of the geometric model and the delineation of mesh. Post-processing mainly covers the presentation of the simulation results and the summary analysis of the results.  
For the meshing of the geometric model, ICEMCFD was used. Structured mesh was chosen for the stockpile model. Structured mesh is significantly more accurate than unstructured mesh for CFD with a simple geometry. The high mesh quality of the model provides a certain basis for the accuracy of the simulation. The grid near the sand pile is encrypted. In addition, appropriate dense treatment was also applied to the downwind side of the stockpile. In Figure 3, for the particular shape of the truncated cones, the structured mesh is created using O-gridding. The walls of the truncated cones and the ground in the vicinity of the truncated cones are grid encrypted, due to the fact that the velocity gradient changes the most in this region. The total number of meshes obtained for the model are 23 million.  
Fluent was used for the computational simulation. The solver performs step-by-step iterative solutions using pressure coupling. For the gas phase, the \(k-\omega\) SST dual equation model was used, which was more applicable to the bypass phenomenon. For the particle phase, the DPM method was used as described in the previous section. The simulation was decomposed into two parts, one for the steady calculation of the gas phase and the other for the unsteady calculation of the solid phase. A stable flow field can be obtained because the velocity of the boundary conditions was stable. The unsteady state calculation of the particles was closer to reality, and it can reduce the errors in the simulation. In this study, the mass flow rate of the particles was assumed to be constant. The particles on the sand pile were not immediately spread by the wind, due to the friction between the gravels. Therefore, the sands and gravels were only released when the wind speed reached a certain level.  
To simulate the particle transport, many static particles initially were assumed to be distributed uniformly on the surface of the stockpile. Then, the total number of particles was determined by the time of particle transport and the number of grids on the surface of the stockpile. An overview of the simulation parameter and particle/fluid phase properties for the coupled DPM-CFD simulations was given in Table 1. Boundary conditions settings were shown in Figure 1.  
Figure 3: Meshing result.  
In order to simulate the flow field accurately, instead of using a single wind speed at the velocity inlet, a variable wind speed associated with height was used. In Figure 4, variation of wind speed was exponentially distributed with height. The distribution of inlet velocity can be calculated from the following equation:  
\[u_{y}=u_{0}\cdot(\frac{y}{y_{0}})^{\alpha} \tag{1}\]  
where \(u_{y}\) is the velocity at a vertical height of \(y\). \(u_{0}\) is the velocity at a vertical height of \(y_{0}\), and \(\alpha\) is the surface roughness coefficient, chosen as 0.15 in this study.