## 3 Preliminary Analysis and Design Direction  
### Preliminary Analysis Conditions  
This section details the preliminary finite element analysis (FEA) performed to establish an initial design direction for the ultra-high-pressure hydrogen solenoid valve. The FEA aimed to compare the performance of the proposed concave contact geometry with that of a conventional rectangular contact geometry. Two configurations of the concave geometry were investigated: one with the plunger curvature radius greater than the seat curvature radius \(R_{p}>R_{s}\), and another with \(R_{p}<R_{s}\). For these initial simulations, eccentricity \(e\) was maintained at 1.0 mm to isolate the influence of the curvature radii. The specific geometric design variables for these three initial contact configurations (conventional rectangular, concave \(R_{p}>R_{s}\), and concave \(R_{p}<R_{s}\)) are detailed in Table 1. The results of this preliminary analysis informed the subsequent optimization study presented in Section 4. The FEA was conducted using the commercial software ANSYS Mechanical 2023 R2 [21]. The material properties assigned to the plunger (Polyamide-imide, PAI) and the seat (Aluminum Bronze) for the FEA are detailed in Table 2.  
PAI was selected for its favorable hydrogen penetration resistance and dimensional stability, while aluminum bronze offers good resistance to hydrogen embrittlement, corrosion, and wear. To accurately capture the elasto-plastic response of the PAI plunger under the anticipated high-stress conditions, a multilinear kinematic hardening (MKIN) model was adopted, defined using experimental stress-strain data. A summary of the key parameters for the numerical setup, including element type and meshing details, is provided in Table 3. \begin{table}
\begin{tabular}{c c c c} \hline \hline \multirow{2}{*}{**Design Variable**} & **Rectangular** & **Concave** & **Concave** \\  & **(Original)** & **(\(R_{p}>R_{s}\))** & **(\(R_{p}<R_{s}\))** \\ \hline \(R_{p}\) (mm) & 5.5 & 5.5 & 5.5 \\ \(R_{s}\) (mm) & - & 5.0 & 6.0 \\ \(e\) (mm) & 1.0 & 1.0 & 1.0 \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Design variables for finite element analysis of contact geometries. \begin{table}
\begin{tabular}{c c c} \hline \hline \multirow{2}{*}{**Property**} & **Plunger** & **Seat** \\  & **(PAI)** & **(Aluminum Bronze)** \\ \hline Density (kg/m\({}^{3}\)) & 1420 & 7450 \\ Young’s modulus (GPa) & 4.5 & 117 \\ Poisson’s Ratio & 0.45 & 0.34 \\ Compressive strength (MPa) & 186 & 685 \\ \hline \hline \end{tabular}
\end{table} 
Table 2: Material properties for finite element analysis. A two-dimensional axisymmetric model was developed, for which 4-node structural solid elements (e.g., PLANE182 or an equivalent type in ANSYS Workbench) were employed. These lower-order quadrilateral elements were chosen for their balance of accuracy in stress analysis and computational efficiency, particularly for problems involving nonlinear material behavior and contact under axisymmetric conditions. The finite element model, including mesh details, contact definition, and applied boundary conditions, is illustrated in Figure 5. As shown in Figure 5a, the mesh was significantly refined in the critical contact area between the plunger and seat, with a minimum element size of approximately 4.29 \(\upmu\)m. An average element quality metric of 0.93 was maintained. This level of mesh refinement and element quality in the critical contact area was achieved by 1.25 \(\upmu\)m. The results of the proposed method are shown in Figure 5b. Figure 5: Finite element model details: (**a**) mesh refinement in the contact zone; (**b**) contact surface definition; (**c**) applied loads and boundary conditions.