## 4 Numerical Simulation Results and Validation
### Validation of Finite Element Results  
The finite element simulation can accurately determine the TVMS of gears, which was fully verified during the study [29; 30]. In order to verify the correctness of the proposed method, finite element simulation of the internal gear pair was conducted using Abaqus 2022. Modeling based on the internal gear pair parameters is provided in Table 1. In order to expedite the solution, five pairs of teeth were selected for simulation. The corresponding simulation model is shown in Figure 10. Before the simulation, the following tasks must be completed. First, the model should be divided into grids of different sizes based on their significance to the simulation results. The grid type is hexahedral, as shown in Figure 10. The grid sizes of the gear teeth, the gear foundation connected to the retained gear teeth, and the remaining hub section were as follows:\(0.8\times 0.8\times 0.8\) mm, \(2\times 1\times 1\) mm, \(4\times 2\times 1\) mm. The number of elements in the driving gear and the driven gear were 83,148 and 153,374, respectively. Second, the elastic modulus and density were determined based on the material properties of the model. Third, the interaction setting: the contact type was 'hard contact', and the friction coefficient was 0.1. The primary and secondary surfaces were the tooth surfaces of the driving gear and the driven gear, respectively. Fourth, to facilitate the application of boundary conditions, the nodes of the driving and driven gear shaft holes were coupled with their corresponding central nodes. Finally, the axial rotational freedom of the driven wheel was released, and the rotational speed and load were applied to the driving and driven gears, respectively. The simulation model was solved to obtain the desired results. The expression for TVMS is as follows:  
\[K=\frac{T}{\Delta\theta r_{b}^{2}} \tag{27}\]  
where \(T\) is the gear load torque, \(\Delta\theta\) represents the angular displacement difference, and \(r_{b}\) is the base radius.  
\[\Delta\theta=\left|\theta_{2}^{\prime}-\theta_{2}\right| \tag{28}\]  
where \(\theta_{2}^{\prime}\) and \(\theta_{2}\) represent the actual and theoretical rotation angles of the driven gear, respectively.  
\begin{table}
\begin{tabular}{c c c} \hline \hline
**Parameters** & **Pinion** & **Gear** \\ \hline Teeth number \(Z\) & 18 & 68 \\ Normal module \(m_{n}\) (mm) & 5 & \\ Pressure angle \(\alpha\) (\({}^{\circ}\)) & 20 & \\ Face width \(B\) (mm) & 50 & \\ Helix angle \(\beta\) (\({}^{\circ}\)) & 13 & \\ Young’s modulus \(E\) (GPa) & 210 & \\ Poisson’s ratio \(v\) & 0.3 & \\ \hline \hline \end{tabular}
\end{table}
Table 1: Basic parameters of the internal helical gear.  
In this paper, the change of mesh stiffness when the gear load torque was 600 N\(\cdot\)m was verified by finite element simulation, as shown in Figure 11. The results indicate that within a mesh cycle, the proportions of the three-tooth and two-tooth mesh areas were basically the same, and the trend in mesh stiffness changes was generally consistent. The results were similar in the three-tooth mesh area, and the maximum error was only 2.78%. However, the finite element results for the two-tooth contact area were slightly larger than the calculated results presented in this paper. The maximum error was approximately 7.48%, and the minimum error was around 3.13%. The average value error was about 4% in the entire mesh cycle. It is evident that the overall change trend and the average value error were within the acceptable range. Therefore, the effectiveness of the proposed method was demonstrated through finite element simulation.