# New Construction Solutions of Gear Using in Space Vehicle Control Systems
## 2 Materials and Methods  
The shape of the flexible was modified bearing in mind that it has a considerable length (L); therefore, attempts were made to reduce it. During the search for the most favourable solutions, the values of the radius (R\({}_{2}\)) at the bottom and the flange were also changed. In the Siemens NX computer program, many models of flexsplines with different body shapes were developed. All tested structures had the same parameters for the rim of the toothed wheel. In the analysis presented, only a few of the most characteristic design solutions were taken into account, allowing coherent and constructive conclusions to be drawn. A strength analysis of the harmonic drives was done in the Abaqus program using the finite element method (FEM). In numerical calculations using FEM, the spatial model of a harmonic drive with a cam generator was used to guarantee the most thorough inspection of the form of deformation of the flexspline. The geometrical parameters of the gear were previously designated by the created calculation sheet. The analysis showed that the harmonic drive is a double wave with the number of flexspline teeth equal to 198, while the circular spine has two or more teeth. The modulus is equal to 0.76 mm, so the pitch diameter has the value d\({}_{1}\) = 150.4 mm. The harmonic drive moves the power N = 1.1 [kW], and its gear ratio is equal to u = 100. The form of neutral layer deformation of the flexspline has a significant impact on the accuracy of the gear and correctness of tooth engagement in the meshing area. Wave gear elements also transmit a torsional moment, which directly influences stresses in the flexspline. By the wave generator, the flexspline not only deforms radially with respect to its center of rotation, but also turns [20; 21]. In view of the above, numerical strength calculations include the fact that the flexspline works under complex load conditions and its elastic deformation is large. During the FEM analysis of the impact of the sleeve shape on the flexspline strength, particular attention was paid to mapping real work conditions and gear loads. Used in calculations, the Abaqus program is an advanced calculation tool, so it is possible to exact the definition of material strength properties, contact conditions, cooperation parts of harmonic drive, and the impact of external factors. Because a very large amount of output data was gathered as a result of the calculations, it was necessary to filter and analyze in the postprocessor of the Abaqus program to show conclusions from the research in a clear and precise way. To determine the impact and shape of the flexspline on its strength, spatial models of harmonic drives were used. However, in view of the large number of finite elements necessary for discretization, it is advisable to introduce some limitations. Due to the symmetry of deformation and load, only partial models of the transmission elements were used. The circular spline, flexspline, and cam wave generator were cut and left only for half of the models, which were limited by a minor generator axis (Figure 3). Furthermore, it was designed for most rounds, holes, or chamfers, which would affect increasing the number of finite elements necessary for the description of geometry. These actions allow for a significant speeding up of the calculation time, which is important with a large number of solutions, but do not have an impact on the accuracy of the results obtained. Ultimately, all calculation models were subjected to a discretization process mainly by means of hexahedral square elements (hexagonal 20 node quadratic brick--C3D20R), which in the models were from 250,000 (variant 2) to more than 2,700,000 depending on the analyzed case. A constant size of finite elements has been imposed on the body of the flexspline for all calculation variants, and hence a different number of them results when discretized for different shapes of the flexspline. For all calculation variants on the toothed wheel, the rim forced a higher density of finite element mesh.