## 4 The Numerical Model  
Numerical simulations were carried out within the ABAQUS (Finite Element) FE environment. The composite region was discretized by means of 28,348 continuum shell elements with a reduced integration scheme (SC8R), while 27,468 solid elements with a reduced integration scheme (C3D8R) were used to model the metallic components. The mesh size was chosen based on a preliminary mesh sensitivity analysis, which is not reported here for the sake of brevity. Figure 8 shows the finite element model, highlighting the connections among the different sub-components.  
The damage onset and evolution were considered in the frame of the preformed tensile analyses. In particular, the [PERSON]'s limit failure criteria was used to simulate the damage in the composite sub-components, since they consider the interaction between the stresses acting on each lamina, distinguishing the failure mechanisms associated to both fibre and matrix failures due to tensile and compressive loads [59]. Moreover, a bilinear plasticity model was considered for the metallic sub-components.  
According to [PERSON]'s limit failure approach, separate criteria were introduced by Equations (1)-(4) to determine the damage status within the material:  
\[F_{ft}=\left(\frac{\sigma_{11}}{X_{T}}\right)^{2}+\alpha\left(\frac{\sigma_{12 }}{S_{L}}\right)^{2}=1\quad\text{if}\quad\sigma_{11}>0 \tag{1}\]  
\[F_{fc}=\left(\frac{\sigma_{11}}{X_{C}}\right)^{2}=1\quad\text{if}\quad\sigma_ {11}<0 \tag{2}\]  
\[F_{mt}=\left(\frac{\sigma_{22}}{Y_{T}}\right)^{2}+\left(\frac{\sigma_{12}}{S_ {L}}\right)^{2}=1\quad\text{if}\quad\sigma_{22}>0 \tag{3}\]  
\[F_{mc}=\left(\frac{\sigma_{22}}{2S_{T}}\right)^{2}+\left[\left(\frac{Y_{C}}{2 S_{T}}\right)^{2}-1\right]\left(\frac{\sigma_{22}}{Y_{C}}\right)^{2}+\left(\frac{ \sigma_{12}}{S_{L}}\right)^{2}=1\quad\text{if}\quad\sigma_{22}<0 \tag{4}\]  
In more detail, Equations (1)-(4), associated respectively to fibre failure in tension and compression and matrix failure in tension and compression, are expressed as a function of the fibre tensile (\(X_{T}\)) and compressive (\(X_{C}\)) strength, of the matrix tensile (\(Y_{T}\)) and compressive (\(Y_{C}\)) strengths, and of the transversal (\(S_{T}\)) and longitudinal (\(S_{L}\)) shear strengths. Once the Hashin's limit values have been reached, the material can be considered damaged, and the stiffness is gradually reduced by a coefficient \(d\), defined for each failure mode, ranging from 0 (undamaged condition) to 1 (completely damaged condition).  
Figure 8: Finite element model (FEM).  
For metallic sub-components, according to the introduced bilinear plastic model schematically represented in Figure 9, when stresses overcome the yield threshold, the resulting deformation \(\varepsilon_{tot}\) can be expressed as the sum of an elastic contribution \(\varepsilon_{el}\) (evaluated as the ratio between the applied stress \(\sigma\) and the elastic modulus E; \(\varepsilon_{el}=\sigma/\)E) and a plastic contribution \(\varepsilon_{p}\).  
ABAQUS TIE multipoint constraints were used to model the bonded connection between sub-components, as shown in Figure 10. These connections involved the composite skin and the composite omega stringers, the metal skin and the doubler, and the metal skin and the fillers.  
To numerically reproduce the fastener behaviour in fastened connections, two approaches were used:  
* Model with _Tie_: TIE constraints: this was used to connect the surfaces of the fastened subcomponents;
* Model with _Fastener_: the fasteners were numerically simulated by means of ABAQUS fastener connectors. An elastic behaviour was supposed for the fastener connectors, which were placed in the locations of the experimental test-case, reported in Figure 11.  
Figure 11: Fastener locations.  
Figure 9: Bilinear plastic model.