## 4 Finite Element Analysis
### Finite Element Analysis  
SolidWorks software was used for three-dimensional modeling, and ABAQUS software is used for finite element analysis after modeling. C3D8R element is used for meshing. Local mesh encryption was made in the vicinity of key chamfers of the flat cover and contacts the part between the spherical model and the flat cover, with mesh size of 1 mm, compared to the mesh size of 20 mm in other parts. The small chamfer was not included in the calculation model, because when the crack was inserted into the model, the stress concentration at the crack tip would be the dominant factor, and the stress concentration at the small chamfer was no longer important. The whole structure model was used in finite element calculation to obtain the critical stress area and the surface crack was inserted into the local model after stress analysis. Figure 15 gives the whole model for stress analysis. The ballast tank used in the deep-sea submersible was subjected to uniformly distributed hydrostatic pressure, which was applied both in the spherical shell and the flat cover. In order to eliminate the overall rigid body displacement without hindering the relative deformation, the boundary conditions were set symmetrically with six displacement components constrained by the three-point support method recommended in [22]. The contact surface between the flat cover and the sphere was set as the friction contact with the friction coefficient of 0.1.  
Figure 14: \(\Delta K\) and \(\Delta K(1-R)\) values of 18 Ni(350) determined by unstable crack growth properties.  
When a crack is simulated, the crack will be inserted into a sub-model. The sub-model was taken out separately for the study. The calculation can be conducted by using the connection between the global model and the sub-model, thus greatly reducing unnecessary computation and time costs. According to the results of previous failure observations, the defective part of the cover is treated as a sub-model and the crack with the length of 3 mm and the depth of 1.5 mm is inserted into the model. After static analysis, the stress intensity factor of crack front can be obtained. The position relationship between the sub-model and the global model is shown in Figure 16.  
When the flat cover is subjected to different external pressures from 5 to 85 MPa, the stress intensity factors of the crack can be obtained. Figure 17 depicts the stress intensity factors along the crack front with increasing the external pressure. Figure 18 shows the changing of the stress intensity factors at  
Figure 16: The position relationship between the sub-model and the global model.  
Figure 15: Finite element model for stress analysis.  
the surface points and the deepest point with the external pressure. The stress intensity factor in the length direction is larger than that in the depth direction. The maximum value of the stress intensity factor occurs at the surface points. When the external load increases to about 75-85 MPa, the stress intensity factor at the crack tip reaches 35-42 MPa\(\cdot\)m\({}^{1/2}\), i.e., approximating to the value of fracture toughness, 38 MPa\(\cdot\)m\({}^{1/2}\), shown in Figure 14, which is the ultimate cause of the damage.