## 2 Materials and Methods
### Research Methods  
All the results presented in this work were obtained using the ANSYS Fluent 2021R1 CFD package. This software package has a wide set of models that allows one to fully solve the tasks. Since the entire particle bed is located in the cells of the distribution device, presumably \"free\" fluidization will be observed \"locally\" in each cell formed by the distribution grid (Figures 2b, 3 and 4) individually and not throughout the entire section of the reactor. For this reason, it was decided to simulate only one cell, and not the entire section of the apparatus. \begin{table}
\begin{tabular}{c c} \hline \hline
**Name of the Parameter** & **Parameter Value** \\ \hline Catalyst particle size, mm & 1.5–3.0 * \\ Apparent density of catalyst particles, kg/m3 & 2500 \\ Heat capacity of catalyst particles, J/(kg\(\cdot\)K) & 962.6 \\ Volume fraction of catalyst in the catalyst–inert material mixture, \% & 20 \\ Particle size of inert material, mm & 2–4 * \\ Apparent density of inert material particle, kg/m3 & 2200 \\ Heat capacity of particles of inert material, J/(kg\(\cdot\)K) & 879.7 \\ \hline \hline \end{tabular}  
* the particle size distribution was determined by the Rosin–Rammler powder law [61].  
\end{table} 
Table 2: Parameters of catalyst and inert material particles. Figure 3: View of the finite element mesh (Euler mesh). Simulating a single cell rather than an entire layer allows the researchers to achieve the following:  
1. to conduct three-dimensional simulation, since the reduced scale frees up a significant amount of computing power;
2. to use more precise models, such as the Unresolved Discrete Particle Model (UDPM), and Resolved Discrete Particle Model (RDPM), which are not capable of simulating objects larger than the laboratory size. In this work, preference was given to UDPM, since, according to the assumptions obtained, the interaction of particles between themselves and the walls, and not between gas and particles, plays a decisive role in the behavior of the particle bed;
3. to reduce the total time of each calculation, which allows one to make more calculations to collect more detailed information about the system. The following models were chosen to solve all the problems: 1. a multiphase model: DPM [49]; the gas-particle drag law of [PERSON] and [PERSON] [49]; 2. for DPM: the rheological \"spring-damper\" scheme determines the nature of collisions of the particles with objects. In this case it implies an inelastic collision; for the particle-plane symmetry pair, an ideally elastic collision was chosen. The lateral faces of the upper part of the simulated cell (Figure 4) were set as planes of symmetry, since they represent the gas-gas interface planes, i.e., there is a gas phase in front of and behind the plane; 3. a turbulence model: the realizable \(k\)-\(\varepsilon\) model with restriction of the turbulence kinetic energy generation term and viscous heating to make calculations taking heating into account [49]. Figure 4: Geometry of the research area (the scale is shown in the lower part). Since ANSYS Fluent uses the finite volume method, i.e., the entire volume of the modeled object is divided into many elements of various shapes (tetrahedron, hexahedron, polyhedron, etc. ), it is necessary to determine the minimum size of the element of the final mesh, which is also called the Euler mesh. For UDPM, it is necessary for the minimum size of the Euler mesh to exceed the size of the largest particle; in our case, these inert material particles are 4 mm in diameter. However, the considered problem also includes particles that have a smaller size, but an excessively large mesh will lead to a larger number of particles happening to be in one ensemble, so simulation of their movement would be incorrect. Therefore, the minimum size of 6 mm of the mesh elements for the tetrahedral shape of the elements was chosen.