## 4 Case Study  
### Finite Element Modelling  
The tank used in this study represents a typical design found in petroleum depots. Its key geometrical and mechanical properties are detailed in Table 2. The tank wall thickness varies linearly from 21 mm at the base to 9 mm at the top to account for axial and hoop stress distributions. The FE model was developed using ABAQUS v2021 software [42], as illustrated in Figure 6. The tank wall was modeled using S4R shell elements, four-node quadrilateral elements with reduced integration. These elements capture both bending and membrane behavior, essential for simulating buckling and stress distributions. The liquid inside the tank was represented using potential-based fluid elements, which allow for accurate modeling of hydrodynamic pressures without manual configuration of the fluid-structure interaction surface. The model includes all essential structural components, such as the roof, bottom plate, and cylindrical wall. Non-structural accessories, such as the nozzles, piping, fire extinguisher system, and stairs, have not been included in the model. To accurately simulate the seismic behavior of an existing tank with pre-deformed geometry, a detailed inspection was performed using 3D laser scanning technology. This process captured the actual shape of the tank, identifying local deformations such as dents, uneven wall thicknesses, and residual out-of-plane displacements. The scanned data were used to create a virtual model of the tank's deformed shell. Figure 7 illustrates the deformation pattern identified, which is critical for accurately capturing the tank's modified stiffness, mass distribution, and dynamic properties. The modal analysis of the FE model provided key dynamic characteristics of the tank-liquid system (Table 3); characteristics such as impulsive mass \(m_{i}\), convective mass \(m_{c}\), impulsive stiffness \(k_{i}\), convective stiffness \(k_{c}\), impulsive frequency \(f_{i}\), and convective frequency \(f_{c}\) were retrieved, which were used to define the two degree of freedom system representing the simplified mechanical model of the tank. \begin{table}
\begin{tabular}{c c c c c c c} \hline \hline
**Diameter** & **Height** & **Fluid Height** & **Wall Thickness** & **Fluid Density** & **Steel Strength** & **Elastic Modulus** \\ \(D(\mathbf{m})\) & \(L(\mathbf{m})\) & \(H(\mathbf{m})\) & \(t(\mathbf{mm})\) & \(\rho(\mathbf{kg}/\mathbf{m}^{3})\) & \(f_{y}(\mathbf{MPa})\) & \(E_{s}(\mathbf{MPa})\) \\ \hline
54.9 & 14.6 & 13.5 & 21 (base) to 9 (top) & 980 & 235 & 210,000 \\ \hline \end{tabular}
\end{table} 
Table 2: Mechanical and geometrical properties of the cylindrical tank. Figure 5: Procedure to obtain fragility curves using incremental dynamic analysis (IDA). The following assumptions were made in developing the FE model: (1) the tank was assumed to be supported on a rock foundation, neglecting soil-structure interaction effects; (2) the fluid was considered incompressible and inviscid, consistent with standard hydrodynamic modeling approaches; and (3) non-linearities in the material's behavior, such as yielding, were limited to critical regions to maintain computational efficiency. While these assumptions provide a reasonable approximation for the tank's seismic response, future studies could incorporate soil-structure interactions and advanced material models for enhanced accuracy. \begin{table}
\begin{tabular}{c c c c c c} \hline \(f_{i}(\mathbf{Hz})\) & \(f_{e}(\mathbf{Hz})\) & \(m_{i}(\mathbf{t})\) & \(m_{e}(\mathbf{t})\) & \(k_{i}(\mathbf{kN}/\mathbf{m})\) & \(k_{e}(\mathbf{kN}/\mathbf{m})\) \\ \hline
6.39 & 0.11 & 9,391 & 22,181 & 2,159,800 & 10,500 \\ \hline \end{tabular}
\end{table} 
Table 3: Dynamic characteristics of the tank–liquid system.