# Optimization Design Method of Pipe-Insulating Joints Based on Surrogate Model and Genetic Algorithm
## 2 Methods  
### Finite Element Model for Insulating Joint  
The most adverse load considered for insulating joints is the bending moment caused by earthquakes or foundation deformation. When designing insulating joints, it is required that the failure of the insulating joint occurs later than the failure of the connected pipeline. Therefore, the most adverse load for the insulating joint is the bending moment transmitted at the time of failure of the adjacent pipeline. Before leaving the factory, insulated joints are subjected to a four-point bend test, as shown in Figure 3. Hence, this paper investigates the optimization of stress in insulating joints based on this test condition. It should be noted that the stress referred to in this study is the von Mises stress, which will hereinafter be simply referred to as stress [38]. This study takes the DN1400 insulating joint as an example to investigate the stress distribution pattern of a cross-section under bending tests. The detailed dimensions of the DN1400 insulated joints are in Appendix A. The insulating filler in the insulating joint is made of an epoxy glass laminated plate, the sealing ring is made of fluoroelastomers, and the remaining components are made of steel. The epoxy glass laminate is modeled using an orthotropic linear elastic model, and the fluoroelastomer is modeled using a two-parameter Mooney-Rivlin constitutive model with parameters set to C\({}_{10}\) = 8.5 and C\({}_{01}\) = 6.1. The steel is modeled using a bilinear isotropic hardening model, with the model's equation shown in Equation (1):  
\[\sigma= \begin{cases}E\epsilon,&\epsilon\leq\epsilon_{\rm s}\\ \sigma_{\rm s}+E_{1}(\epsilon-\epsilon_{\rm S}),&\epsilon>\epsilon_{\rm s}\end{cases}  \tag{1}\]  
where \(\sigma\) represents the material stress; \(\epsilon\) represents the material strain; \(E\) represents the material elastic modulus, taken as 2.06 \(\times\) 10\({}^{5}\) N/mm\({}^{2}\); \(\epsilon_{\rm s}\) represents the material strain at the yield point; \(E_{1}\) represents the material hardening modulus, taken as 1.45 \(\times\) 10\({}^{5}\) N/mm\({}^{2}\); \(\sigma_{\rm s}\) represents the yield stress, taken as 485 MPa. The specific parameters are shown in Table 1.  
All connections between steel components in the insulating joint are made by welding; hence, the contact relationships are defined as bonded connections. The contact relationships between other materials are characterized by friction. The coefficient of friction is 0.25 between steel and rubber, 0.45 between rubber and epoxy resin, and 0.3 between epoxy resin and steel [39; 40]. Before the bending test, the insulating joint is equipped with corresponding short pipes welded on its left and right sides. The pipes are then supported on the bottom surface and loaded on the top. The schematic diagram of the loading mechanics is shown in Figure 4. The finite element model of the insulating joint bending test is shown in Figure 5. \begin{table}
\begin{tabular}{c c c c} \hline \hline \multirow{2}{*}{**Materials**} & **Density** & **Elastic Modulus** & **Poisson’s Ratio** \\ \cline{2-4}  & Steel & 7850 & 206,000 & 0.3 \\ \hline \multirow{2}{*}{Epoxy Glass Laminated Plate} & Vertical Direction & 45,000 & 0.4 \\ \cline{2-4}  & Horizontal Direction & 10,000 & 0.3 \\ \hline \hline \end{tabular}
\end{table} 
Table 1: Material properties. Figure 4: Mechanical loading sketch of the bending test for the insulating joint. Figure 3: Insulating joint bending test. The load is a vertically downward distributed force, equivalently transformed into two equal concentrated forces, \(P\), acting at the center of the loading surface. The magnitude of the load is such that it brings the edge material of the left and right short pipes to the yield point.