## 2 Materials and Methods
### Theory and Application of the CFD Method  
In the presented research, two conventionally used methods of physics and mathematics are integrated. The first one is the numerical CFD method, which is well-known, and the second one is the method based on the ANNs. The theory of the CFD and ANN is extensive, but in the following chapters, only substantial facts necessary for the novel methodology for the temperature fields prediction explanation are described [37]. The CFD method is known for a few decades, but its application for complex problems is still time-consuming. The CFD stands for computational fluid dynamics, which is a branch of fluid mechanics. The method uses numerical analysis and data structures to analyze and solve the problems involving fluid flows. For a better understanding, the methodology is directly explained on the example of the iSTC-21v jet engine. The 3D model, in our case the 3D models shown in Figure 2, is imported into the ANSYS software, and the mesh for the particular parts is created. In our case, at first, the stator section of the turbine is meshed [38; 39]. The 3D mesh is created by mapping the 2D mesh of the particular parts of the stator section. The mesh of the turbine stator section is shown in Figure 3a. In Figure 3b, the 3D mesh created on the basis of the geometry can be seen. It is the rotor section of the turbine of the iSTC-21v jet engine. Finally, the meshed nozzle, as can be seen in Figure 3c, is created. All three parts in our case consist of the hexa elements [40; 41]. \begin{table}
\begin{tabular}{c c c c} \hline
**Regime** & **Temperature-\(T_{3t}\) (°C)** & **Pressure-\(P_{3t}\) (Pa)** & **Speed (rpm)** \\ \hline
1 & 824.0 & 197,700 & 36,079 \\
2 & 851.0 & 197,900 & 36,110 \\
3 & 862.6 & 211,300 & 37,920 \\
4 & 891.3 & 229,000 & 39,960 \\
5 & 914.3 & 264,400 & 41,660 \\
6 & 942.9 & 268,200 & 44,080 \\
7 & 977.9 & 288,100 & 46,020 \\
8 & 1007.0 & 307,300 & 47,860 \\
9 & 1067.0 & 339,100 & 50,120 \\
10 & 1127.0 & 361,300 & 51,990 \\ \hline \end{tabular}
\end{table} 
Table 1: Overview of boundary conditions for the computational fluid dynamics (CFD) analyses. The overall approach for the solution of the presented problem starts with the definition of the CFD simulation. In order to define and set the above-mentioned simulation, the Turbomachinery wizard was used. The mesh of the stator, rotor and nozzle was imported and combined, as it is shown in Figure 3d. The Frozen Rotor simulation was performed and then modified to define the Transient Rotor-Stator simulation. The Transient Rotor-Stator simulation was performed using the steady-state Frozen Rotor for the initial guess. Finally, the results of this analysis are used for further processing. The final model prepared for the CFD simulation is presented in Figure 3d, where the boundary conditions are applied for one regime. Subsequently, boundary conditions were applied for other regimes. For the particular regimes, the rotor speeds, temperatures and pressures were applied according to the obtained results from the experimental measurements performed on the iSTC-21v jet engine (summarized in Table 1). The axis of the rotation for the simulation is the \(Z\)-axis, as shown in Figure 3d. The CFD model consists of 2,756,789 elements, the element size for the blade is 0.0035 mm, \(y\)+ value is 0.9565, the 2D mesh of the blade is shown in Figure 4. The general information of the turbine vane and blade is listed below. The chord of the turbine blade is 25 mm, the span of the turbine blade is 26 mm, the pitch has a value of 17.5 mm for the blade. The Inlet angle is 20.5 degrees, and the outlet angle is 58 degrees. The distance between the stator vane and rotor blade of the turbine is 12 mm. Chord line of the stator vane is 40 mm, the span of the vane is 25 mm, and the pitch is 22 mm. The turbulent model for the simulation is chosen, the shear stress transport model, which is one of the most accurate models.