# Analytical Model for the Structural Behavior of Pipelines During Lowering-In
## 3 Validation of Segmental Pipeline Models
### Finite Element Analysis for the Lowering-in Phase  
The segmental pipeline model for Models 1 and 2 was verified by finite element (FE) analysis using ABAQUS [31]. In the FE model, the pipeline is modeled with a 3-D beam element (B31) to simulate the bending behavior in the vertical and lateral plane. Also, the pipeline was assumed to behave in the elastic range. Its diameter and thickness were applied as 0.762 m and 0.021 m, respectively. The trench was modeled using 3-D shell elements (S4) and the geometry of the trench was determined considering the standard of SP 42-102-2004 [32] and the diameter of the pipeline. The deformable depth of a soil was assumed to be 1 m, considering the depth of the active layer and the freezing layer in common soil. This depth is reflected with the thickness of the shell element. The plastic behavior of the soil was ignored and considered as an elastic material. The material and geometric properties of the pipeline and trench are summarized in Table 1. The grade of the pipeline is X70 and considering the stiff soil condition, an elastic modulus and Poisson's ratio were 40 MPa and 0.32, respectively. The skid had the same material properties as the trench and its height was the initial position of the pipeline. The pipelayers control the displacement only to support the pipeline. A general contact option in ABAQUS was used to implement the contact boundary condition between the pipeline and the trench. The general contact was applied to provide interactions such as traction on the surface between the pipeline and the trench. Before the lowering-in, the boundary conditions of displacement for the pipeline were free but the displacement on all sides of the trench was fixed. The pipeline was placed by self-weight at the top of trench, assumed as a skid and the general contact was accommodated between the pipeline and the trench. During lowering-in, the pipeline was lowered into the trench bottom by the displacement loads at the lifting point of pipelayers. In this process, the surfaces between the pipeline and trench contacted with each other were applied as general contact. A hard contact condition and friction coefficient of 0.3 were considered for the normal and tangential behaviors of the contact surfaces, respectively. Typically, the frictional coefficients between the steel and soil have a range of 0.14 to 0.26. To prevent slippage between the pipeline and the soil, the frictional coefficient of the soil used was as 0.3, which is slightly larger than typical values.  
The static analysis was performed discretely for each phase of the lowering-in. The bending moments in the vertical and lateral plane were carried out from SM 1 and 2 in the output of Abaqus, respectively. Also, the output variables corresponding to the shear forces in the vertical and lateral plane are SF2 and 3. The results of FE analysis for Model 1 and Model 2 represented as shown in Figure 7.  
\begin{table}
\begin{tabular}{c c c} \hline
**Classification** & **Pipeline** & **Trench** \\ \hline \multirow{3}{*}{material properties} & density & 7850 kg/m\({}^{3}\) & 1520 kg/m\({}^{3}\) \\  & elastic modulus & 210 GPa & 50 MPa \\  & Poisson’s ratio & 0.3 & 0.32 \\ \multirow{3}{*}{geometric properties} & section property & \\  & length & 400 m & 400 m \\ \hline \end{tabular}
\end{table}
Table 1: Material and geometric properties for the finite element (FE) models.  
Figure 7: Sectional forces of FE model (rendering contour): (**a**) bending moments for Model 1 (unit : N\(\cdot\)m); (**b**) shear forces for Model 1 (unit : N); (**c**) bending moments for Model 2 (unit : N\(\cdot\)m); (**d**) shear forces for Model 2 (unit : N).