## 3 Methodology
### FEA Model
The total time of the explicit step was 0.7 s for corner impact, while the central impact had a total step time of 0.6 s. These times were decided after an initial simulation showed that the separation of the car and the street pole's surface pairs occur during this time; therefore, any subsequent results were obsolete for the scope of this paper. The corner impact simulation is longer to compensate for the time it takes for the vehicle to initially contact the street pole. All parts were entirely meshed using linear hexahedral explicit elements for Abaqus to output suitable accuracy for the results. To reduce the distortion or exaggeration of the mesh elements, a degradation control of 0.75 was used with element deletion enabled. The total number of mesh cells required for the simulations amounted to about 22,400 elements. All shell elements were assigned with reduced integration 4-noded quadrilateral elements, S4R, while the interior solid component had 3D continuum reduced integration hexahedral elements, C3D8R. The reason why these many elements were required is dictated from a sensitivity analysis of the mesh. Three points were declared to be used as a probe. The 3 points, as seen in Figure 7, were used as these were the main regions of contact between the vehicle and the pole. Therefore, any large variations in the model suggested that values are highly sensitive and mesh refining is mandatory in these regions. The only mesh elements that were refined were the car bumper and the street pole. Other bodies in these mesh elements were not of interest and were not included in the mesh sensitivity analysis to save computation time. The plastic equivalent strain results were used to analyze the mesh sensitivity analysis, as it is expected that the accuracy of the damage or plasticity must be conserved as much as possible, regardless of mesh refinement, with minimal changes only happening due to any anomalous elements that may suffer from numerical singularities. After about 20,000 mesh cells, a convergence had taken place, as shown in Figure 8. Therefore, to maintain a good balance in providing both a qualitative \begin{table}
\begin{tabular}{c c c c c} \hline \hline \multirow{2}{*}{**Material**} & **Young’s Modulus** & \multirow{2}{*}{**Poisson’s Ratio**} & **Yield Stress** & **Density** \\  & **(GPa)** & & **(MPa)** & **(kgm\({}^{-3}\))** \\ \hline
**Aluminum-5052** & 68.9 & 0.33 & 140 & 2690 \\ \hline
**Aluminum-6061** & 69.5 & 0.33 & 220 & 2780 \\ \hline
**Steel ASTM A36** & 210 & 0.29 & 247.5 & 7869 \\ \hline \hline \end{tabular}
\end{table} 
Table 1: General properties of the three materials that were used in this paper including the elastic properties, plastic initialization, and the density as a requisite for dynamic explicit simulations. \begin{table}
\begin{tabular}{c c c} \hline \hline \multirow{2}{*}{**Material**} & \multirow{2}{*}{**Fracture Strain**} & \multicolumn{2}{c}{**Displacement after Fracture**} \\  & & **(m)** \\ \hline
**Aluminum-5052** & 0.105 & 0.002625 \\ \hline
**Aluminum-6061** & 0.061 & 0.001525 \\ \hline
**Steel ASTM A36** & 0.24 & 0.006 \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Ductile damage properties of the three materials that were used in the simulations. and quantitative analysis, altogether, it was agreed that an optimum mesh seed of 0.025 m (equivalent to 22,400 elements) was sufficient for the model. Using the points, it was found that after using ten processors to solve the Abaqus FEA problem, each simulation took about 24 min to solve. The graphical representation of the mesh can also be seen in Figure 7.