## 3 Development of AI-FEM Multiple Cracks Growth Algorithm  
### The Overall Procedure for Multiple Cracks Growth in AI-FEM  
AI-FEM is a Python-based plugin for the commercial finite element analysis (FEA) program Abaqus (2018), which automatically simulates crack growth using re-meshing techniques. Although AI-FEM was originally designed to simulate single-crack growth, additional functionality has been developed through this study to simulate the growth of multiple cracks. Figure 2 illustrates the algorithm of AI-FEM for simulating the growth of multiple cracks. First, the initial crack information, including the shape and location of the multiple cracks, as well as the geometry of the structure, is input. Then, AI-FEM automatically \begin{table}
\begin{tabular}{c c c} \hline \hline
**Document** & \begin{tabular}{c} **Flaw Interaction Criteria** \\ **(_a/c\(\leq\)1_)** \\ \end{tabular} & \
\begin{tabular}{c} **Flaw Interaction Criteria** \\ **(_a/c-1_)** \\ \end{tabular} \\ \hline \hline
\begin{tabular}{c} ASME Section XI \\ API 579 \\ BS 7910 (and R6) \\ \end{tabular} & \(S\leq S_{m}(=0.5\text{max}(a_{1},a_{2}))\) & - \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Summary of industrial codes for multiple crack coalescence criteria. Figure 2: The algorithm of the multiple crack growth analysis in AI-FEM. generates elements based on the input information. As shown in Figure 3, C3D20R elements (quadratic brick elements with reduced integration) are used for the crack-tip region, C3D10 elements (quadratic tetrahedral elements) are used for the region around the crack, and C3D8R elements (linear reduced-integration elements) are used for the rest of the structure. The reason for using tetrahedral elements (C3D10) in the region around the crack is to provide higher degrees of freedom when modeling the crack. The reason for using reduced integration elements is to reduce computational time costs while maintaining analysis accuracy. The appropriateness of the element type applied to each region was previously verified by [PERSON] et al. [23] through comparison with theoretical results. The spider-web configuration of the crack-tip elements is essential for accurately calculating the SIF [25]. Next, depending on the user's needs, the initial stress field can be mapped using Abaqus (2021 version) 'Map Solution' function. This step is optional and can be omitted if not needed. Subsequently, the SIF is calculated through FEA, and the amount of crack growth is determined based on Paris' law input by the user, preparing for modeling subsequent cracks. The newly modeled crack contains more elements compared to the previous crack model. This is to represent the larger crack shape as the crack grows. On the other hand, the element size varies depending on the region. For the crack-tip region (C3D20R), the initial element size set by the user is maintained, whereas for the region surrounding the crack-tip (C3D10), the element size changes adaptively. As shown in Figure 3, the farther the distance from the crack tip, the larger the C3D10 element size becomes. In the next step, the distance (\(S\)) between adjacent cracks is calculated, and it is determined whether the calculated distance is smaller or larger than the proposed critical distance (\(S_{proposed}\)) defined by the new coalescence criteria proposed in this study. If \(S\) is smaller than or equal to \(S_{proposed}\) (\(S\leq S_{proposed}\)), the two separate surface cracks are coalesced into a single crack, and the curvature of the re-entrant region resulting from the coalescence is applied to simulate the natural crack growth of multiple cracks. In the overall algorithm presented in Figure 2, the boxes related to the new coalescence criteria, coalescence method, and growth algorithm for multiple cracks are marked with red borders, and these aspects are discussed in Section 3.2. Finally, once the cracks are modeled, AI-FEM evaluates whether the user-specified final cycle or time has been reached.