## 2 Design of Components and Fabrication
### Numerical Design  
In this section, we further investigate the proposed spring-actuated dynamic impact setup using finite element modeling (FEM). This modeling serves to investigate any source of discrepancies that could potentially impact the accuracy of recreating numerically the results of a dynamic impact (e.g., the effects of system friction and air resistance). This process could highlight the potential energy losses in the physical system when compared to idealized numerical models.  
Therefore, the eight dynamic impact scenarios (Table 5) were investigated using the FEM Abaqus/Explicit software-V22. The proposed simulation model is shown in Figure 5. The steel material was modeled as an elastic-plastic material with 5% damping and the mechanical properties listed in Table 6. The material properties adapted considered the high-strain rate of the impact.  
The model specifically focuses on the interaction between the impactor and the steel specimen, excluding detailed representations of the railing and motion system. However, the numerical results were calibrated by incorporating an estimated friction coefficient of 0.37, derived from the experimental data of five specific specimens (IDs 2, 3, 5, 6, and 7) as listed in Table 5. Moreover, spring dynamics, including extension and potential energy, were not modeled since their influence ceases prior to impact. Instead, the impact energy was calculated from the impactor's mass and velocity just before contact. This approach accurately captures the energy transfer during impact while simplifying the simulation.  
\begin{table}
\begin{tabular}{l l l} \hline \hline
**Parameter** & **Value** & **Unit** \\ \hline Mass Density & 7800 & Kg/m\({}^{3}\) \\ \hline Young’s Modulus & 210,000 & MPa \\ \hline Poisson’s Ratio & 0.3 & - \\ \hline Hydrostatic failure stress, dynamic & 410 & MPa \\ \hline Stress at zero plastic strain, dynamic & 302 & MPa \\ \hline Stress at 5\% plastic strain, dynamic & 320 & MPa \\ \hline Stress at 15\% plastic strain, dynamic & 351 & MPa \\ \hline \hline \end{tabular}
\end{table}
Table 6: The material definition implemented in numerical modeling [39].  
\begin{table}
\begin{tabular}{c c c c c c} \hline \hline \multirow{2}{*}{**ID**} & \multicolumn{2}{c}{**Spring Extension, x**} & \multirow{2}{*}{**Velocity, v (m/s)**} & **Impact Energy, E** & **Max. Displacement, d** & **Max. Impact Force, F** \\  & & & **(Joule)** & **(mm)** & **(N)** \\ \hline
1 & 2.00 & 0.40 & 3.16 & 22.9 & 343.2 \\ \hline
2 & 2.25 & 0.44 & 3.90 & 26.3 & 407.1 \\ \hline
3 & 2.50 & 0.48 & 4.57 & 29.2 & 464.2 \\ \hline
4 & 2.75 & 0.52 & 5.40 & 31.2 & 521.5 \\ \hline
5 & 3.00 & 0.55 & 5 The developed models were discretized using 4 \(\times\) 4 mm S4R mesh elements with reduced integration (four-node doubly curved thin shell elements) [40]. This choice was made based on a mesh sensitivity analysis with mesh sizes from 2 \(\times\) 2 mm to 6 \(\times\) 6 mm to provide convergence with minimal computational cost. The thickness of the specimens was approximated using [PERSON]'s integration rule with seven integration points. The supports were modeled with discrete rigid shells, and the rotation of the specimens was allowed at the supports. Since the impactor sustained no damage during the experimental testing, it was modeled as a discrete rigid shell having the mass and initial velocity as per the testing conditions.