# On the Design of Bionic Hierarchical H-Type Whip Restraints for Nuclear Power Plants
## 2 Materials and Method
### Finite Element Model Construction  
Numerical models are established to explore the energy absorption characteristics of the NBDHMCs using ABAQUS/Explicit (2022, Dassault Systemes, Providence, RI, USA). As shown in Figure 4, the bionic tube is sandwiched between two rigid plates simulated by the analytical rigid body, with a height of 600 mm. The upper rigid plate is given a mass of 1200 kg, and exerts an impact on the tube at a velocity of 60 m/s to enhance computational efficiency. The impact distance is set to 450 mm. To ensure sufficient calculation accuracy, the total kinetic energy should be much less than the total internal energy during the crushing process [42]. The lower rigid plate is connected to the tube while constraining all degrees of freedom. The tube is modeled with a shell element and meshed using the S4R shell elements. The rigid plates are meshed using the R3D4 shell elements. A general contact algorithm is used to control the contact behavior of the whole structure, and the friction factor is 0.3.  
The aluminum alloy AA6061-O is used in the simulation of tubes. A standard elastic-plastic isotropic hardening constitutive model is utilized to characterize the mechanical properties of the aluminum alloy. The experimental results reveal that the material exhibits the following properties: density \(\rho\) of 2700 kg/m\({}^{3}\), [PERSON]'s modulus \(E\) of 70 GPa, Poisson's ratio \(\
u\) of 0.31, initial yield stress \(\sigma_{y}\) of 83.58 MPa, and ultimate stress \(\sigma_{u}\) of 165.92 MPa. The  
Figure 4: Finite element model.  
true stress-plastic strain curve of the material is presented in Figure 5. The strain rate is not considered in the simulation, since AA6061-O exhibits insensitivity to the strain rate.  
The mesh size significantly impacts the numerical simulation results, necessitating the selection of an NBIHMC structure with \(\mathbf{m}=16\) for a mesh convergence analysis. Nine different mesh sizes were used for testing, including 2 mm, 2.5 mm, 3 mm, 3.5 mm, 4 mm, 4.5 mm, 5 mm, 5.5 mm, and 6 mm. The numerical simulation results are shown in Figure 6 and Table 1. From the results, it can be observed that the force-displacement curves with mesh sizes from 2 mm to 4 mm almost overlap, and their EA differences are all less than 1%. The EA difference between 5 mm and 2 mm is around 5%, and in order to balance the computational efficiency with the computational accuracy, the mesh size for the subsequent numerical simulations is selected to be 5 mm. The reliability of this finite element model was verified experimentally in our previous work [41]. It is worth noting that the localized folding patterns observed in compression experiments are often affected by small geometric defects introduced during the manufacturing process. These defects, such as slight wall thickness variations or surface defects, are difficult to characterize and replicate in simulation models. Therefore, while our model reliably captures the overall response, some variations in localized fold formation are expected and do not affect the validity of the overall conclusions.  
\begin{table}
\begin{tabular}{c c c c c} \hline
**Mesh Size (mm)** & **EA (kJ)** & **EA Difference (\%)** & **IPF (kN)** & **IPF Difference (\%)** \\ \hline
2 & 97.32 & 0 & 424.98 & 0 \\
2.5 & 97.38 & 0.06 & 427.38 & 0.56 \\
3 & 97.46 & 0.14 & 426.80 & 0.42 \\
3.5 & 97.61 & 0.30 & 426.18 & 0.28 \\
4 & 97.92 & 0.62 & 427.58 & 0.61 \\
4.5 & 100.74 & 3.51 & 426.94 & 0.46 \\
5 & 102.20 & 5.01 & 425.63 & 0.15 \\
5.5 & 105.57 & 8.47 & 427.18 & 0.52 \\
6 & 106.67 & 9.61 & 426.66 & 0.73 \\ \hline \end{tabular}
\end{table}
Table 1: Mesh sensitivity data.  
Figure 5: True stress–plastic strain curve of AA6061-O aluminum alloy.