## 3 Specim Description and FE Model  
The numerical model described in the previous section is applied here to replicate the experimental results of skin-doubler specimens subjected to a three-points bending test [23]. The specimens are made of a 200 mm \(\times\) 100 mm skin with a 70 mm long doubler on top representing the stringer flange (Figure 5). The skin and the doubler are made of 8 plies of carbon-epoxy with the stacking sequence \([45/0/-45/90]_{\text{s}}\), and a ply thickness of 0.1875 mm. The total thickness of the skin and the doubler is 1.5 mm. The material properties adopted in the numerical analysis are reported in Table 1.  
The model is discretized in the Finite Element (FE) code ABAQUS [31] using a combination of continuum shell elements (SC8R) for the composite skin and the doubler, and zero-thickness cohesive elements (COH3D8) at the interface to simulate the initiation and growth of the delamination. The properties of the composite laminate are assigned to both the skin and the doubler using the Composite Layup functionality of ABAQUS, which allow to define the thickness and orientation of each lamina within the laminate. A global element size of 1 mm is adopted for the entire model, while a more detailed discretization is implemented in the region potentially interested by the propagation in order to have an accurate representation of the cohesive process zone. According to [30], a minimum of 5 elements is required to accurately represent the stress variation within the cohesive process zone. Using Equation (2) and the properties of the material under investigation, the length of the process zone is estimate to be approximately 1 mm. Therefore, to maintain a conservative approach, an element length of 0.1 mm is selected for the cohesive elements. The total number of elements in the FE model is approximately 220,000. The skin and the doubler are connected through shared nodes between the cohesive layer and the two plates. The nodes on top of the cohesive elements are shared with the elements of the doubler, while the nodes on the bottom are shared with the nodes of the skin. \begin{table}
\begin{tabular}{c c c} \hline \hline \multicolumn{3}{c}{**Lamina Properties**} \\ \hline E\({}_{1}\) & [MPa] & 147,000 \\ E\({}_{2}\) = E\({}_{3}\) & [MPa] & 8500 \\ G\({}_{12}\) = G\({}_{13}\) & [MPa] & 4500 \\ G\({}_{23}\) & [MPa] & 4000 \\ \(\
u_{12}\) = \(\
u_{13}\) & & 0.36 \\ \(\
u_{23}\) & & 0.45 \\ \(\tau_{\text{C}}\) & [MPa] & 40 \\ G\({}_{2\text{C}}\) & [J/m\({}^{2}\)] & 514 \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Material properties [23]. Figure 5: Specim geometry. To model the trilinear traction-separation law, the zero-thickness cohesive elements at the interface are doubled, resulting in two bilinear cohesive elements connected to the same nodes, as graphically represented in Figure 6.  
Considering the symmetry of the specimen and of the loading and boundary conditions, in the numerical analysis the delamination will start from both the edges of the doubler at the same time. However, during the experimental tests it can be observed that the damage always initiates from one of the corners, due to microstructural defects, and propagates toward the center of the specimen until the global collapse. To numerically represent this phenomenon, the delamination is allowed to propagate from one side of the specimen, while on the other side, only the elastic properties are assigned to the cohesive elements. The FE model and the stacking sequence are shown in Figure 7.  
In the experimental tests, the specimens are loaded and fixed using cylindrical supports located at a distance of 100 mm. In the numerical model, to reduce the computational times, the supports are not explicitly modelled, but appropriate boundary conditions are introduced to represent them.