## 3 Simulation of the Stress Intensity Factor Correction Factor  
### Model Establishment  
In order to obtain the stress intensity factor correction factor \(F\), we take the bottleneck surface of the pressure vessel as the research object and use the ABAQUS simulation software platform to establish the model. The model is an axisymmetric structure with fixed constraints on the bottom, shown in Figure 1, where \(h\) is the wall thickness of the cylinder, \(r_{1}\) is the outer diameter of the bottleneck, \(r_{2}\) is the inner diameter of the bottleneck, and \(R\) is the radius of curvature of the joint surface between the bottleneck and the bottle body. We use 35 CrMo as the material, and its relevant parameters are shown in Table 1.  
The thermal conductivity \(K_{I}\) and constant pressure heat capacity \(C\) of 35 CrMo are both functions of temperature change, and the satisfied relations are presented as Equations (13) and (14):  
\[K_{I}=36.51209+0.04898653T^{-1}-1.012462T^{2}+4.653864T^{3} \tag{13}\]  
\[C=3.55.4448+0.2848T-5.000001T^{2} \tag{14}\]  
The constitutive equation of the 35 CrMo is presented as Equation (15):  
\[\sigma=\ln\left\{\Bigg{[}\frac{\dot{\epsilon}\cdot\exp\bigl{(}\frac{368925}{ RT}\bigr{)}}{1.11768\times 10^{14}}\Bigg{]}^{0.18099}+\left[\left[\frac{\dot{ \epsilon}\cdot\exp\bigl{(}\frac{368925}{RT}\bigr{)}}{1.11768\times 10^{14}} \right]^{0.18099}+1\right]^{0.5}\right\} \tag{15}\]  
where \(\dot{\epsilon}=1.11768\times 10^{14}[\sin\mathrm{h}(0.0097\sigma)]^{5.525058}\exp \bigl{(}-\frac{368925}{RT}\bigr{)}\). Additionally, the fracture toughness of 35 CrMo is presented in Table 2.  
After the setup of the corresponding parameters of 35 CrMo, setting the working environment of the pressure vessel at room temperature, ABAQUS adopts the VonMises criterion, and the overall analysis adopts the ABAQUS/standard general static analysis step to carry out the ultimate load analysis of the structure. A uniform pressure load of 2.5 MPa is applied to the inner wall of the pressure vessel, and the moment module is added to the joint surface of the pressure vessel bottleneck and the bottle body to simulate the elastic flexural bearing capacity. In addition, the displacement constraints of \(U_{x}=0\) and \(U_{y}=0\) are applied, and an inertial load \(g=9.8\) m/s\({}^{2}\) is applied in the X direction. The analysis process adopts the Newton iteration method for automatic load step loading. The stress load diagram of the pressure vessel is shown in Figure 2a.  
The grid density of the curved surface is set to 0.25 mm, and the other parts are set to 5 mm. The mesh model is shown in Figure 2b; the mesh around the surface is denser. As shown in Figure 3, it is the plan view of the normal direction of the crack growth model. The stress intensity distribution is calculated by FEA (finite element analysis). The brighter colors indicate higher stress, and it can be observed that the area of the crack tip has the greatest stress intensity.  
\begin{table}
\begin{tabular}{c c c c} \hline \hline
**Density** & **Elastic Modulus E** & **Poisson’s Ratio** & **Linear Expansion** \\ \(\rho\) (kg/m\({}^{3}\)) & **(GPa)** & \(\mu\) & **Coefficient (\(U^{c}\)C)** \\ \hline
7800 & 210 & 0.3 & \(1.35\times 10^{-5}\) \\ \hline \hline \end{tabular}
\end{table}
Table 1: Pressure vessel material parameters.  
Figure 1: The geometric model of the surface of the pressure vessel bottleneck.