## 2 Materials and Methods
### Software  
#### 2.2.1 ABAQUS  
The primary software utilised in this study was ABAQUS/CAE 2017. Calculations were performed using the PLGrid Infrastructure, which provides access to clusters in five High-Performance Computing centres. Computational tasks were managed centrally through middleware that allocated resources across all hubs. For this analysis, the WCSS hub was used.  
To model the bidirectionally sinusoidal corrugated steel elements, three-dimensional shell finite elements with 4 nodes and reduced integration, known as S4R, were employed. These were the conventional stress/displacement shell elements. After conducting a thorough convergence analysis for various mesh sizes, it was determined that a mesh with an element size of 0.005 m provided the optimal balance between computational efficiency and accuracy. This mesh size was chosen to ensure that the results were both precise and reliable, capturing the essential details of the structural behaviour without introducing unnecessary computational overhead.  
The static analysis employed a direct method for solving the equation system, utilising the full Newton method as the solution technique. For the eigensolution method, the Lanczos method was chosen. Similarly, a nonlinear dynamic analysis (implicit dynamic analysis) was conducted using the direct method for solving the equation system. Damping was omitted in this analysis.  
\begin{table}
\begin{tabular}{c c c} \hline \hline
**Parameter** & **Unit** & **Adopted Values** & **Number of** \\  & & & **Combinations** \\ \hline \(t\) & mm & 3.0; 4.0; 5.0; 6.0 & 4 \\ \(n_{x}\) & - & 8 & 1 \\ \(n_{y}\) & - & 8 & 1 \\ \(f\) & mm & 0.0; 2.0; 4.0; 6.0; 8.0; 10.0; 12.0; 14.0 & 8 \\ \(L_{x}\) & m & 1.0 & 1 \\ \(L_{y}\) & m & 0.8 & 1 \\ \(F\) & kPa & 1.0-sin(62.83 rad/s-\(t\)1) & 1 \\ \(E_{s}\) & GPa & 210.0 & 1 \\ \(v_{z}\) & - & 0.30 & 1 \\ \(\rho_{s}\) & kg/m3 & 7850.0 & 1 \\ \hline \hline \end{tabular}  
* Where \(t\) is a time variable.  
\end{table}
Table 2: The values of the parameters adopted for the purpose of the dynamic analysis.  
\begin{table}
\begin{tabular}{c c c} \hline \hline
**Parameter** & **Unit** & **Adopted Values** \\ \hline \(t\) & mm & 5.0 \\ \(n_{x}\) & - & 8 \\ \(n_{y}\) & - & 8 \\ \(f\) & mm & 6.0 \\ \(L_{x}\) & m & 1.0 \\ \(L_{y}\) & m & 0.8 \\ \(F\) & kPa & 1.0 \\ \(E_{s}\) & GPa & 210.0 \\ \(v_{z}\) & - & 0.30 \\ \(\rho_{s}\) & kg/m3 & 7850.0 \\ \hline \hline \end{tabular}  
* Where \(t\) is a time variable.  
\end{table}
Table 3: The values of the parameters adopted for the purpose of the comparative analysis.  
The use of Python scripting in ABAQUS significantly advanced the research by enabling the automated generation of a large number of models with various parameters. The utilisation of this feature can be found in the latest studies [23; 24]. This automation greatly enhanced the efficiency and accuracy of the modelling process, allowing for a systematic exploration of bidirectionally sinusoidal corrugated steel shells with different geometrical and mechanical configurations. Python scripts were employed not only to create these models, but also to run simulations, which would be impractical to execute manually. Furthermore, the scripts were designed to extract specific results from the simulations, such as deflections, stresses, and dynamic responses. These results were then automatically saved into external text files, organised in a structured manner. This automated data extraction and storage facilitated an easy analysis and comparison of the results, ensuring that the data were consistently formatted and readily accessible for further processing. This approach not only streamlined the workflow, but also minimised the potential for manual errors, thereby improving the reliability and reproducibility of the study.