## 3 Finite Element Model  
### Discretization and Assumptions  
In order to analyze the chassis response to force components and generate input for the O.A., a computer model was developed using the F.E.A. software ANSYS v.2019 [2]. To reduce analytical complexity, only the composite section of the structure was modeled, with corresponding adjustments to boundary conditions. Although this approach may lead to structural over-design, it was justified by the need to avoid errors arising from modeling the entire hybrid chassis. Regarding geometric partitioning, the software makes multiple element types available, though results depend on element type, size, and order. \begin{table}
\begin{tabular}{c c c c c} \hline \hline
**Elastic Moduli (GPa)** & & \multicolumn{2}{c}{**Strength Properties (MPa)**} & \multicolumn{1}{c}{**Strain Limits**} \\ \hline E\({}_{11}\) & 120.43 & Direction 1 (tension) & 1442.0 & 0.015 \\ E\({}_{22}\) & 7.724 & Direction 2 (tension) & 29.0 & 0.0032 \\ E\({}_{33}\) & 7.724 & Direction 3 (tension) & 29.0 & 0.0032 \\ v\({}_{12}\) & 0.295 & Direction 1 (compression) & \(-\)1230.0 & \(-\)0.0108 \\ v\({}_{13}\) & 0.295 & Direction 2 (compression) & \(-\)200.0 & \(-\)0.0192 \\ v\({}_{23}\) & 0.237 & Direction 3 (compression) & \(-\)200.0 & \(-\)0.0192 \\ G\({}_{12}\) & 2.517 & Shear XY & 137.7 & 0.012 \\ G\({}_{13}\) & 2.517 & Shear YZ & 32.0 & 0.011 \\ G\({}_{23}\) & 3.121 & Shear XZ & 94.25 & 0.012 \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Properties of unidirectional CFRP laminate. \begin{table}
\begin{tabular}{c c c c} \hline \hline
**Elastic Moduli (GPa)** & & \multicolumn{2}{c}{**Strength Properties (MPa)**} & \multicolumn{1}{c}{**Strain Limits**} \\ \hline E\({}_{11}\) & 55.0 & Direction 1 (tension) & 782.3 & 0.0126 \\ E\({}_{22}\) & 55.0 & Direction 2 (tension) & 661.8 & 0.0126 \\ E\({}_{33}\) & 6.9 & Direction 3 (tension) & 50.0 & 0.008 \\ v\({}_{12}\) & 0.064 & Direction 1 (compression) & \(-\)550.0 & \(-\)0.0102 \\ v\({}_{13}\) & 0.064 & Direction 2 (compression) & \(-\)550.0 & \(-\)0.0102 \\ v\({}_{23}\) & 0.32 & Direction 3 (compression) & \(-\)170.0 & \(-\)0.012 \\ G\({}_{12}\) & 4.27 & Shear XY & 118.0 & 0.022 \\ G\({}_{13}\) & 4.27 & Shear YZ & 118.0 & 0.019 \\ G\({}_{23}\) & 4.27 & Shear XZ & 86.0 & 0.019 \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Properties of woven CFRP laminae. Therefore, it was deemed necessary to conduct experiments to determine the optimal mesh configuration for the model. After examining the analogous literature [23; 24] as well as the nature of the experiments to be performed on the chassis, specific test schemes were adopted to grade the performance of F.E.A. software elements. These tests aimed to evaluate the behavior of elements in bending and torsion, while varying their dimensions and making comparisons with the analytical solutions. Finally, in order to further focus the search, only four types of elements were tested, according to software manual [2] and previous studies [23; 24], with more details about the experiments presented subsequently. In the initial test scenario, whose details are included in Table 3, the geometry under investigation was modeled as a thin-walled cylinder, characterized by a thickness-to-internal-diameter ratio of 1/20. Accordingly, for a unit thickness, the internal diameter of the cylinder was specified as 20 mm. The cylinder's length and the applied torque at the nodes along the internal diameter at the free end were both set to 1 Nm to execute the computational analysis. Furthermore, the meshing of the geometry was conducted uniformly using a single element type throughout the volume, with the element categories evaluated including SOLID185, SOLID186, SHELL181, and SHELL281 [2]. The geometry was assigned an orthotropic material model, incorporating the mechanical properties detailed in the problem statement. The results were subsequently validated through comparison with the analytical solution for the torsion of cylindrical composite shafts [1].