# Numerical Simulation Study on the Performance of Buried Pipelines under the Action of Faults
## 2 Finite Element Model of Pipe-Soil System
### Establishment of the Model  
In ABAQUS software, version 6.13., the eight-node linear hexahedral solid element C3D8R and the four-node curved shell element S4R are selected to simulate the soil media around the pipe and the buried pipe, respectively. Referring to the research on the effective calculation length of a pipeline model and the code [24], for the calculation of buried pipelines across faults with equivalent boundaries, large deformation segments near the fault and the length of pipelines not less than 60 times the diameter of the pipeline should be analyzed. According to such regulations, the dimensions of the calculation model in the X, Y, and Z directions are taken as 12 times, 8 times, and 65 times the diameter of the pipe, respectively. The whole finite element model of the soil-pipeline system mainly includes three parts: fixed disk, movable disk, and buried pipeline (as shown in Figure 1).  
The focus of this study is to analyze the behavior of the buried pipeline under the action of faults. Taking into account the calculation accuracy, efficiency, and convergence, a more refined mesh division is carried out on the soil within 3 m around the pipeline and its surroundings, as shown in Figure 1. When determining the grid size of the calculation model, the authors referred to the suggestions in the relevant literature and achieved good calculation accuracy. According to the relevant studies [25; 26], the pipeline axis direction in the large deformation section is 20 m on both sides of the fault within the range of the pipeline mesh size, which is set to 0.1 m so as to accurately simulate the large deformation characteristics of pipelines, and the grid size of other pipe sections is set to 0.5 m, as shown in Figure 1.  
Figure 1: Finite element model of soil–pipeline system.  
A nonlinear contact model is used to simulate the interaction between the pipeline and soil, as well as between the soil on both sides of the faults. Since the stiffness of pipeline steel is significantly larger than that of soil media, the outer surface of the pipeline is set as the master surface of the contact pair, and the inner surface of the soil is set as the slave surface of the contact pair. The normal action between the contact surfaces is set as \"hard\" contact, so as to realize the simulation of extrusion on the contact surface between the pipeline and the soil. The tangential action is set as a \"penalty\" friction function, and the friction coefficient is defined to simulate the shear stresses between the pipeline and the soil in the process of fault misalignment. The shear stress between the pipe and the soil during fault misalignment is simulated by defining the friction factor. In addition, in order to simulate the behavior that the pipe and the soil separate from each other due to excessive relative displacement during the fault movement, the two parts are allowed to separate from each other after contact. Through this setting, the behavior between the pipeline and soil is made to be closer to the actual situation.  
This study conducts numerical analysis of the above-established model through the incremental application of fault displacement. The numerical calculation process includes the following three steps. Firstly, gravity loading is applied to the whole model to simulate the initial stress state of the soil in the actual situation. Secondly, an internal operating pressure is applied to the inner wall of the pipeline to simulate the buried gas pipeline under the normal operation state in the actual project. Finally, the fault movable disk is subjected to linear displacement loading.