## 2 Methods
### Theoretical Study
Inside the three-dimensional computational domain, a cross-section was selected where a boundary condition of the 'fan' type was specified (see Figure 5). The air flow passing through this cross-section experienced a prescribed pressure jump \(\Delta P(V)\), determined based on the head-flow characteristic (Figure 3). However, the head-flow characteristic \(\Delta P(V)\) in the ANSYS model did not coincide with the curve in Figure 3 due to neglecting shock losses at the inlet and outlet of the flow from the bench, as well as due to several other factors. The polynomial function \(\Delta P(V)\) was chosen so that, at an HRR of zero and a given angle of rotation of the valve at the outlet, the air flow rate in the inclined part of the channel matched that in the experiment. It should be noted that Figure 5 shows openings No. 1 and No. 2 on opposite sides of the channel. The same orientation was used on the laboratory bench shown earlier in Figure 2. In the laboratory bench, this orientation of openings No. 1 and No. 2 was more convenient from the point of view of ease of access and for performing measurements. An important aspect during the initial parameterization of the model was the choice of the heat transfer coefficient through the channel wall. Part of the heat imparted to the flow from the heat source is removed through the walls of the channel into the surrounding atmosphere. Moreover, this thermal factor is more pronounced for the section of the channel below the heat source. Therefore, to account for this thermal factor, the heat transfer coefficient was selected to achieve the best agreement between the model and measured values of average air temperatures in sections below the heat source (see Figure 4). The effective value of the heat transfer coefficient was 150 W/(m\({}^{2.\circ}\)C). The numerical solution of the system of Equations (4)-(11) with specified boundary conditions was carried out in the Fluent module of the ANSYS software package (version 2021 R2) using the finite volume method. The velocity and pressure fields were linked using the SIMPLE (Semi-Implicit Method for Pressure-Linked Equations) algorithm [47; 48]. Spatial discretization was carried out using schemes of second-order accuracy (for pressure and velocity equations) and first-order accuracy (for equations of transfer of turbulent characteristics). Time discretization was performed using an implicit first-order scheme. Gradients of scalar quantities were calculated using the least squares method. To speed up the numerical calculations, a parallelization procedure was used on central processor cores (24 cores). The process of finding a solution at each time iteration was also carried out iteratively using the Multigrid Cycles algorithm [49]. The subiterative procedure at each time iteration continued until relative residuals of \(10^{-4}\) were achieved for all variables. One calculation took from 3 to 16 h, depending on the initial and boundary conditions. The mesh was generated in the Meshing module of the ANSYS software package. An irregular tetrahedral finite-volume mesh with a prismatic boundary layer near solid walls was constructed. The mesh parameters were selected to ensure the solution's independence from the mesh. In this work, mesh convergence was studied by controlling the pressure drop in the inclined section of the domain for various initial values of the mass flow entering the computational domain. The results of the comparison of the controlled parameters are given in \[\frac{\partial(\rho\mathbf{u})}{\partial t}+\
abla\cdot(\rho\mathbf{u}\mathbf{u})=-\
abla p +\
abla\cdot[(\mu+\mu_{t})\
abla\mathbf{u}]+\mathbf{g}\rho \tag{5}\]0  
Table 1 shows that when the cell size changes from 0.3 m to 0.2 m, the change in pressure drop in the study area was no more than 3% for the entire range of considered flow rates. Thus, for further calculations, a mesh with a cell size of 0.3 m on the free surface was selected. The final number of cells was 1,586,296.