# Crasworthiness Analysis to Evaluate the Performance of TDM-Shielded Street Poles Using FEA
## Methodology
### FEA Model  
The FEA models simulated in these tests are the front collision and corner collisions against the shielded street pole. Abaqus/Explicit is used for this collision due to the severe forms of nonlinearities present in this problem. One factor includes the instantaneous contact between the high-speed vehicle and the street pole shell due to the collision, which is usually difficult for Abaqus/Standard to converge. Moreover, non-linear material behaviors, such as metal plasticity and ductile damage, have been added onto the street pole and vehicle's geometry for a realistic transfer of energy between the two bodies. Other forms of non-linearity, such as geometric non-linearity, have been included using the NLGEOM function in Abaqus. The material for the vehicle's exterior body, engine body and tire is the same as the one conducted in [1], which is Aluminium-6061. The street pole considered in this study, however, will only be the one made from Steel ASTM A36. The properties of these metals can be found in Tables 1 and 2. Furthermore, the stress-strain profile used to extract the plastic data of these alloys is also the same as the values used in [1]. The reason why this specific material was chosen is that the results shown by [PERSON] et al. [1] concluded that the steel poles had lesser SEA than the Aluminium-5052-based street pole, which meant that the impact energy absorbed by the vehicle during the crash would increase and would cause more risk to the passengers onboard the vehicle. Another reason was also that the aluminum street poles had their structure severed from the base while the vehicle was still in motion. In contrast, the steel pole decelerated the vehicle to a halt. This means that the energy will increase throughout the course of the deceleration. This overall increase, therefore, must be mitigated using a layer of TDM. Moreover, the reinforcements are geometrically and sectionally modeled as solid continuum elements. This decision was made because the thickness-to-length ratio exceeded the ratio for the street pole to be considered as a thin shell. The solid elements are of the type C3D8R, which means they are 3D stress elements for explicit analysis. The R signifies that the elements have reduced orders of integrations. Furthermore, enhanced hourglass control was declared to avoid results accuracy losses and maintain analysis stability. Finally, since the visualization of the degradation is not critical, element deletion of the reinforcement was enabled while the degradation of the elements was set at 0.8. To optimally chose the correct element size without compromising on the computation time, the global size of the elements for the TDM-based reinforcements on the street pole was set at 10 mm. Sensitivity analysis for the pole and vehicle was already covered extensively in [1]. Furthermore, no further sensitivity analysis was performed on the vehicle and pole to ensure that results extracted from the paper's simulations would be valid when compared to simulations using the same number of mesh presented in [1]. Mesh sensitivity analysis was, however, performed on the pole reinforcement. Three tests were taken with element sizes of 10 mm (50,000 elements), 20 mm (27,000 elements) and 30 mm (23,500 elements). Since the pole did not contain material with plastic properties, the only means of understanding sensitivity was using the deformation results of the three simulations. A probe was added to the center of impact of the reinforced shield. This is done as the contact between the vehicle, and the shield would contain many sources of contact. These contacts would be highly sensitive to the results; therefore, refinement is required in these critical regions to ensure convergence of results is maintained. As seen in Figure 2, convergence is fairly satisfied after 30,000 elements. Therefore, the simulation included the shield with 10 mm of element sizing to extract reliable results. Therefore, the total number of mesh cells used in this simulation equaled to approximately 60,000 elements.