## 2 Materials and Methods
### Numerical Simulations  
A numerical replication of the experimental burst test was performed for validation and to improve the understanding of the failure mechanisms. ABAQUS [41] was used as FEM package software to create the CAD model for the global and local models, generate the finite element meshes, perform the global-local FEM calculations, and post-process the results. The CAD model of the repaired pipe according to the burst test was reported in Figure 3 and in Figure 1 with some highlights of the defect position and size. The considered material was the API 5L X60 steel used for the seamless pipe shown in Figure 2. The main mechanical properties considered here are listed in Table 1, whereas the true stress true strain diagram is reported in Figure 4. With reference to the repairing materials, Tables 2 and 3 comprise the main mechanical properties of the composite sleeve and the adhesive filler (Methyl Methacrylate Monomer), respectively. The sleeve was made up of multiple E-glass fibre composite layers with the direction of fibres in the tangential direction to the pipe (direction of the hoop stress). Since the composite sleeve presented orthotropic  
Figure 2: Flow of operations to produce the test article: (**a**) API 5L X60 steel pipeline, (**b**) cut and closed with lateral caps to obtain a tank; (**c**) machined defect and corresponding (**d**,**e**) repairing process through the composite sleeve. 3D CAD and FEM models were set up. The final assembled CAD model is shown in Figure 6, whereas the corresponding FEM model is shown in Figure 7. The machined volume was considered as completely filled with the adhesive material. Due to the in-significance of the stress distribution in the filler material, only its elastic behaviour was considered (material data listed in Table 3). A total of 8 composite reinforcing layers were 3D modelled around the damaged section. The orientation of the fibres was assigned by defining local coordinates for each layer, as shown in Figure 5. The direction of axis 1 represents the (tangential) direction of fibres that were directed in such a way to reinforce the sleeve against the highest stresses (hoop stress). Axes 2 and 3 represent the directions perpendicular to the fibres inside and outside the layer planes, respectively. Figure 5: CAD model of the different layers of the composite sleeve with a highlight of the local coordinate systems. Figure 6: Submodelled positions of the global CAD model. A coarse mesh was produced for the global FEM model, see Figure 7a. Consequently, the sub-modelling technique was used to improve the accuracy of the FEM results. This  
Figure 7: Meshes generated for the different models: (**a**) global model, (**b**) SM1, (**c**) SM2. sub-modelling consisted of the modelling of smaller parts of the overall CAD model, thus allowing for much finer meshes and more detailed modelling in these localized regions. Displacement boundary conditions, calculated by means of the global FEM model, were applied to the cut sections of submodels in order to replicate the displacement fields within these localized regions of interest. Once the displacement fields were replicated locally, highly accurate local stresses and strains were calculated accordingly. For these reasons, sub-modelling represents a widely applied technique when there is the need to obtain the local fields of interest with high accuracy, e.g., for fracture [42; 43; 44; 45; 46] or fatigue [47] assessments. Two submodels were created so as to calculate the data for the repaired and the healthy pipe sections, see Figures 6 and 7. With submodel 1 (SM1), the stress distribution in the defective section, filled with the adhesive and reinforced with the composite layers was examined. With submodel 2 (SM2), the stress distribution was examined in an undamaged section. The number and type of elements used in each model are listed in Table 4.  
A non-linear quasi-static analysis was performed with a constantly increasing internal pressure applied to the entire internal surface reaching up to 204 bar.