**2. Methods**

#### *2.1. CFD Simulation*

## 2.1.1. Model Descriptions

The Euler–Euler two-phase flow model is used to simulate the proppant transportation in the cross fractures. This model takes the multitude of particles as an artificial solid phase that can interpenetrate the continuous water phase [11,12]. The KTGF approach is used to simulate the particle collisions. Based on the KTGF approach, an additional equation, i.e., the particle temperature equation, is solved to represent the fluctuations of the particles. This equation leads to additional terms as the particle pressure force and so on. More details about this model were detailed in the previous paper [10,13].

#### 2.1.2. Geometry and Mesh

The geometry of the cross fractures in the numerical simulation is shown in Figure 1. The cross fractures contain one primary fracture and one secondary fracture. The secondary fracture intersects the primary fracture at a certain angle (bypass angle θ). It is assumed that the height of the cross fractures remains constant along the moving direction of the mixture, and the height of the primary fracture equals that of the secondary fracture. The scales of the primary fracture and secondary fracture are length × height = 1000 mm × 150 mm and 600 mm × 150 mm, respectively. The horizontal distance between the entrance of the secondary fracture and the primary fracture is 400 mm. The width and bypass angle (θ) of the primary and secondary fracture are varied in di fferent cases. The geometry references the experiment apparatus of Alotaibi and Miskimins [5], Tong and Mohanty [11], and Patankar et al. [14]. The mixture of the proppants and water enters the primary fracture from an inlet which is simplified as a rectangular opening. In actual hydraulic fractures, the proppants are generally blocked by an unruptured stratum. That means that the front end of the cross fractures is closed. Therefore, a wall is set at the end of the geometry in the numerical model. The mixture is only permitted to flow out of the cross fractures through the outlet on the top of the wall (Figure 1). The flow field is divided into hexahedral structured cells due to the consideration of computation accuracy and convergence. A standard case is first calculated with the proppant density ρ*s* = 3300 kg/m3, the proppant diameter *ds* = 0.5 mm, the water density ρ*l* = 1000 kg/m3, the water viscosity μ*l* = 0.001 Pa·s, the secondary fracture width *wb* = 1.5 mm, the primary fracture width *wa* = 5 mm, the injection velocity (*U*0) 0.2 m/s, and inlet proppant volume fraction (<sup>α</sup>*s*0) 3%. To evaluate the mesh independence, three kinds of mesh with different sizes are performed. The mesh size in the height, length, and width is 4 × 4 × 1 mm (coarse), 2 × 2 × 1 mm (medium), and 2 × 2 × 0.5 mm (fine), respectively. The EPH obtained from the medium grid is similar to that from the fine grid. So, the grid size 2 × 2 × 0.5 mm is used.

**Figure 1.** The geometry representing the cross fractures. The cross fractures consist of a primary fracture and a secondary fracture in length × height: 1000 mm × 150 mm and 600 mm × 150 mm, respectively. The width and the bypass angle will be changed in different cases.

#### 2.1.3. Initial and Boundary Conditions

Initially, the cross fractures are filled with water, and then the proppants begin to enter the cross fractures. The velocity inlet is set. Different pumping flow rates and sand ratios are imposed by varying the injection rates and the inlet volume fraction of the proppants. The inner walls of the cross fractures are set as the no-slip wall boundary conditions for each phase. The pressure outlet is set to be zero gauge pressure. The values of the parameters used in the numerical simulation are listed in Table 1. The ANSYS FLUENT software is used for the numerical simulation.


