## 4 Numerical Verification for Design  
### 3D Analysis Modeling  
In this chapter, the aim was to validate the reliability of test results by numerically analyzing the seismic performance of the hydrogen storage vessel through the construction of a 3D dynamic analysis model. To achieve this, the commercial structural analysis software ABAQUS was used. In the finite element analysis (FEA) modeling, time history analysis--one of the prominent numerical analysis methods used to understand the dynamic performance of structures--was employed to examine the seismic behavior. Typically, dynamic behavior is more accurate than static behavior, and nonlinear behavior is more accurate than linear behavior for structures. Time history analysis is generally the most accurate method for understanding the nonlinear dynamic behavior of structures and is commonly used for evaluating the seismic performance of target structures. Furthermore, it can provide more objective and accurate results since it can capture dynamic behavior characteristics such as relative displacements, anchor load transfers, and acceleration responses, which cannot be determined through static analysis or response spectrum analysis [35]. The configuration of the Finite Element (FE) modeling, as shown in Figure 5, consisted of the hydrogen storage vessel, support columns, and foundation concrete, using three degrees of freedom at eight nodes and minimal integration points with 8-Node Solid elements (C3D8R). Additionally, pre-installed set anchors, used to secure the structure to the concrete, were also implemented using C3D8R elements. The FE model consisted of a total of 295,643 nodes and 222,556 elements. The mesh size for the connection points between the main body and support columns--where stress concentration was anticipated--was set to 10 mm \(\times\) 10 mm. For anchors and the lower plates of support columns, a mesh size \begin{table}
\begin{tabular}{c c c c c c c} \hline \hline \multirow{2}{*}{**Type**} & \multicolumn{2}{c}{**Weight**} & \multicolumn{3}{c}{**Size (mm)**} & \multirow{2}{*}{**Description**} \\  & **(kg)** & **L** & **W** & **H** & **t** & \\ \hline \multirow{2}{*}{Vessel} & 1046 & 530 & 530 & 2420 & 6 & \multicolumn{2}{c}{S400} \\  & & & & & & L-shape angle (75 \(\times\) 75 \(\times\) 9.5) \\ \multirow{2}{*}{RC slab} & 908 & 1570 & 1570 & 290 & 150 & \multicolumn{2}{c}{\(f_{\text{d}}\): 30 Mpa} \\  & & & & & & & \multicolumn{2}{c}{Protrusion concrete (200 \(\times\) 200 \(\times\) 140)} \\ \multirow{2}{*}{Anchor} & \multirow{2}{*}{-} & \multirow{2}{*}{250} & \multirow{2}{*}{-} & \multirow{2}{*}{-} & \multirow{2}{*}{-} & \multicolumn{2}{c}{ASTM A36 [34], M20} \\  & & & & & & & \multicolumn{2}{c}{Embedment depth: 200} \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Specifications of the test specimen. Figure 4: Summary diagram of specimen design for shaking table testing (unit: mm). of 5 mm \(\times\) 5 mm was utilized. Mesh configurations for areas other than vulnerable points were appropriately designed to facilitate convergence time during analysis. To represent the areas of the target structure used in the shaking table test that were connected by welding in the analysis, the welding effect was implemented by combining the Tie function and Coupling function of the ABAQUS platform. This involved constraining degrees of freedom according to the coupling direction, based on translational and rotational degrees of freedom. To model the contact surfaces between two elements with different material properties that can induce sliding effects considering friction, the Interaction feature, which allows for interaction within the analysis program, was employed [36]. To model the boundary conditions of the anchor (as shown in Figure 6), the contacting surface between areas where gaps (such as between the anchor and nut) are not anticipated, is simulated using a monolithic (e.g., tied surfaces in ABAQUS).