Introduction

Pipeline transportation has become the preferred scheme for long-distance oil, natural gas, and other materials transportation due to its advantages of high efficiency, low cost, small footprint, and strong continuity1. By the end of 2023, the total length of China’s long-haul oil and gas pipelines had reached 185,000 km, and the total length of the world’s long-haul oil and gas pipelines had exceeded 1.919 million kilometers. Long-distance pipelines spanning complex geological environment is susceptible to external soil compression2, rockfall impact3, and other disasters during laying and service, resulting in radial displacement and local depression. The indentation damages the structural integrity of the pipeline, is detrimental to the passage of the internal detector and pig, and in serious cases leads to pipeline fracture, leakage, and other safety accidents. Oil and gas are characterized by inflammability, explosiveness, and toxicity, and leakage or explosion will lead to economic losses and environmental pollution, and even cause huge casualties4,5. Therefore, there is an urgent need for more analysis and research on pipelines with indentation defects to clearly define the mechanical behavior characteristics of pipelines under indentation deformation, so as to adopt effective remedial measures to ensure the safe operation of the pipelines in the future.

The causes of dental defects in pipelines are diverse. When pipelines traverse complex areas such as soil settlement, landslides, tunnels, and bridges, they are susceptible to additional loads, rigid constraints, and geological disasters, which can lead to stress concentration and eventually evolve into localized indentation deformation6,7,8. To understand the overall stress level and stress distribution characteristics of long-distance pipelines under adverse external factors, many scholars have conducted comprehensive analytical research on long-distance pipelines. Ren et al.9 analyzed the deformation evolution characteristics of long-haul pipelines in the subsidence area of coal mine goaf under factors such as mining face, buried depth, internal pressure, and reaction force, and identified the failure mode of pipelines in the process of soil settlement. Wang et al.10 and Melissianos et al.11 proposed a three-dimensional numerical model considering the dynamic response, and established a finite element model of a long-distance pipeline with a length of several hundred meters using ABAQUS to analyze the dynamic response of the pipeline failure under the action of sudden inclined slip faults, and discussed the influence of fault velocity, internal pressure of the pipeline, and wall thickness on the pipeline stress. Based on the vector finite element (VFIFE) method, Qiu12 carried out finite element calculation on the long-distance pipeline passing through the tunnel area, taking into account three constraint types of pipelines, namely anchored buttress, supported buttress, and buried buttress, and obtained the stress distribution of the whole pipeline, pointing out that under different combined conditions of temperature and pressure load, the stress concentration of the pipeline at the entrance and exit of the tunnel is significant, and it is urgent to conduct pipeline deformation control. Uckan et al.13 used beam elements and nonlinear soil springs to simulate the interaction of pipe and soil, and analyzed the long-distance pipeline with a fault crossing angle of 90°, obtaining the stress characteristics of the pipeline crossing the fault area, and found that the stress and strain of the pipeline at the fault were the maximum value.

The stress level and stress distribution characteristics of the pipeline can be mastered through the overall stress analysis of the long-distance pipeline, but the local indentation characteristics of the pipeline cannot be simulated in detail, and it is difficult to show the evolution of the local indentation of the pipeline. In order to clarify the local indentation behavior of pipelines, many scholars have carried out research on local pipelines. Li et al.14 and Shuai et al.15 established a pipeline model with local indentation by using ABAQUS finite element software to analyze the indentation rebound of the pipeline under different fluctuating internal pressure loads. Based on the existing evaluation methods, Guo et al.16 established a pipeline model with local indentation to reasonably evaluate the circumferential bending strain, axial bending strain, and axial film strain of the pipeline. Hu et al.17 proposed a detection method combining the detection of pipeline deformation detector and three-dimensional scanner. They used the three-dimensional scanner to scan and detect the dented pipeline, established a pipeline model with local denting, and conducted pressure analysis of the dented pipeline with the help of finite element software ABAQUS. Yang18 established a local pipeline model with volumetric corrosion defects by using ABAQUS software, compared the simulation results with the hydraulic test results and evaluation criteria, and evaluated the adaptability of the residual strength of pipelines with corrosion defects. Zhang et al.19 studied the influence of internal pressure, indenter displacement, diameter-to-thickness ratio, indenter shape, and other factors on the resilience behavior of locally depressed pipelines during service and shutdown, and established the parametric equation of the rounding coefficient through nonlinear regression analysis. Based on the two-dimensional hydrodynamic and sediment mathematical model flow-3D, Hu et al.20 numerically simulated the local erosion of submarine pipelines under the action of constant flow, and studied the different influence characteristics of local erosion of submarine pipelines. Su and Ren21 established a submarine pipeline model with initial defects, analyzed the buckling behavior of the pipeline under bending, axial load, and external hydrostatic pressure, and found that the local buckling form of the pipeline was affected by the shape and size of the defect, and the ability of the pipeline to withstand external hydrostatic pressure became weaker after bending. Zhang et al.22 established a local finite element model of pipe-soil by using solid element C3D8R and four-node S4R shell element, respectively, to clarify the mechanical behavior of pipelines passing through active faults, focusing on the influence of horizontal fault displacement, fault type, and fault inclination on the structural response of pipelines. However, considering the calculation accuracy and efficiency, only small sections of pipelines (ranging from several meters to tens of meters) are usually simulated during the fine calculation of pipe indentation behavior, and the end constraints have a great influence on the calculation results, and the form and parameters of the end constraints cannot be reasonably determined.

It can be seen that if the fine local model of the whole line is established, the calculation amount is huge and the calculation efficiency often cannot meet the engineering needs. If the local deformation characteristics of the pipeline are not considered, the calculation results of the whole model cannot simulate the fine characteristics of the pipeline when the local depression deformation is taken into account. The method of combining whole and local structural analysis has been applied to many fields23,24,25,26,27, but it has not been involved in the study of indentation of long-distance pipelines. This paper presents for the first time the method of combining the whole and the local to analyze the indentation behavior of long-distance pipelines. Based on the principle of VFIFE, a simple, fast, and effective analysis method is provided. The whole pipeline model is established by using the self-developed mechanical analysis software of long-distance pipelines, and the mechanical response of the entire pipeline is analyzed considering the nonlinear relationship of pipes, additional load, hard constraint, and pipe-soil interaction. Then the shell element is used to establish a local pipeline model, and the calculation results of the overall model are applied to the local model as load conditions to realize the fine simulation of the local indentation characteristics, and then the stress–strain response of the sunken pipeline is studied. In this study, the whole analysis and local analysis are organically combined to achieve the stress analysis of the entire line of pipelines, in order to obtain a method that is suitable for engineering, simple in modeling, industry and problem-oriented, and has the prospect of industry popularization and application, providing new technical ideas and guarantees for the development of the mechanical analysis industry of long-distance oil and gas pipelines.

Whole pipeline analysis

Pipeline constitutive model

The whole response generally has the characteristics of a “beam”; the deformation is like a beam, and the force mechanism is similar to that of a beam. Therefore, the beam element is generally used to calculate and analyze the entire pipeline. Material nonlinearity, geometric nonlinearity, contact nonlinearity, and large displacement in the mechanical analysis of long-distance pipelines can easily lead to convergence issues in the calculation. Considering the strong nonlinear problems of long-haul pipelines, the mechanical analysis software for long-haul oil and gas pipelines developed by ourselves is used to analyze the entire pipeline. In order to obtain the deformation characteristics of the pipeline realistically, the nonlinear relationship should be considered in the whole analysis, the constitutive relationship of the pipeline should be selected reasonably, and appropriate load and constraint conditions should be imposed on the pipeline according to the service environment of the pipeline in the actual project.

The stress–strain relationship in the plastic hardening stage of pipe materials is complex and is often simplified using various models. Common simplified models include the ideal elastic–plastic model, bilinear model28,29,30, trilinear model, and Ramberg–Osgood model31,32,33,34. The ideal elastic–plastic model cannot analyze situations where the pipeline stress exceeds the strength limit. The bilinear hardening model simplifies the constitutive curve into two lines, where the stress–strain curve during the hardening stage is represented by a line with a fixed slope. Although the trilinear model divides the behavior into elastic, elastic–plastic, and plastic states, it is primarily used for theoretical analysis methods, and its use in evaluating pipeline conditions becomes more complex. The Ramberg–Osgood model introduces material parameters and describes the stress–strain relationship using a single equation. This model not only considers the plastic deformation of the pipeline but also provides simplicity and convenience in application. Therefore, this paper adopts the Ramberg–Osgood model to describe the stress–strain relationship of the pipe material, as shown in Eq. (1). The parameters in the equation can be selected reasonably according to the "Technical Specification for Seismic Design of Oil and Gas Pipelines" (GB/T 50470-2017).

$$\varepsilon = \frac{\sigma }{E} + \alpha \frac{\sigma }{E}\left( {\frac{\sigma }{{\sigma_{0} }}} \right)^{{n_{1} - 1}}$$
(1)

where \(\varepsilon\) is the pipeline strain, \(\sigma\) is the pipe stress, E is the elastic modulus of the pipe, \(\alpha\) is the yield offset, \(\sigma_{0}\) is the yield stress of the pipe and \(n_{1}\) is the reinforcement index.

Loads and constraints

Long-distance pipelines will be subjected to additional loads and rigid constraints during service. The additional loads on the pipeline usually include the dead weight of the conveying medium, the dead weight of the pipeline, internal pressure load, temperature load, and soil displacement. The dead weight of the pipeline affects the static load and deformation of the pipeline, while the dead weight of the conveying medium affects the internal pressure distribution and the working state of the pipeline. The internal pressure load will cause radial and circumferential stress in the pipeline, which will affect the strength and stability of the pipeline. Thermal expansion or contraction due to temperature changes can cause thermal deformation of the pipe, especially in the presence of fixed supports or pipe clamp constraints, which can lead to additional thermal stress and deformation. Soil displacement will cause lateral and vertical displacement of the pipeline, and then produce bending stress. Rigid constraints are fixed conditions used to limit the movement or deformation of pipelines. Common rigid constraints include anchor buttresses, pipe clamps, vibration isolation supports, elastic supports, and flange joints. In the whole analysis, it is also necessary to avoid the influence of the model end conditions on the pipeline, and the measures commonly used can be divided into two kinds. One is to extend the length of the whole model so that the stress caused by soil settlement is zero at the end, and the other is to apply an equivalent axial spring to the end of the whole model35.

Therefore, before finite element calculation of the entire long-distance pipeline in engineering practice, a field survey must be carried out to determine the types of additional loads and constraints on the pipeline. According to the engineering data and survey results, the exact load and constraint conditions are applied to the entire pipeline, and the mechanical behavior of the pipeline in the actual service environment is simulated.

Pipe soil coupling model

The interaction between pipe and soil is particularly significant in long-distance oil and gas pipelines. How to consider the interaction between pipe and soil is key to the mechanical analysis of buried pipelines. The deformation of the ground will affect the force and deformation of the pipeline, and the soil around the pipeline will produce a reaction force on the pipeline under the extrusion of the pipeline deformation, thus restricting the deformation of the pipeline36. The pipe-soil coupling model is often simulated by the soil spring model37 and the nonlinear contact model. The nonlinear contact model requires all the elements of the pipeline and the surrounding soil, and the full coupling calculation on the contact surface. The modeling of this method is complicated and the calculation is large, so it is difficult to directly adopt it in practical engineering. The soil spring model simulates the soil mass into a series of equivalent elastic–plastic springs38, which can be coupled with the beam element or the shell element for calculation, and can also be analyzed to obtain a semi-analytical solution, which is very easy to popularize and apply.

The pipe-soil coupling model adopted in this paper is shown in Fig. 1 (DL is the distance of soil spring junction, zu, yu and xu are the yield displacements of the spring in axial, vertical and horizontal directions, respectively. fu, qu and pu are the ultimate resistance of the spring in axial, vertical and horizontal directions respectively.). The pipe-soil coupling mode are divided into pipe axial, horizontal and vertical directions. According to the "Seismic Technical Code for Oil and Gas Transmission Pipeline Engineering" GB/T 50470-2017, three soil springs are used to simulate the axial soil friction, horizontal, and vertical soil pressure of the pipeline. Among them, the axial soil spring is determined by the mechanical characteristics of the backfill soil and the buried depth of the pipeline, and the horizontal soil spring and the vertical soil spring are determined by the mechanical characteristics of the soil around the pipeline.

Fig. 1
figure 1

Soil spring force–displacement curves.

Full size image

Development of mechanical analysis software for long distance pipeline

The VFIFE method

The mechanical analysis of long-distance pipelines has strong nonlinearity and complicated pipe-soil coupling. The traditional finite element method needs to constantly update the element stiffness matrix to solve this kind of problem, and the calculation is complicated. In addition, the whole analysis of internal pressure, temperature, and soil displacement load will cause the pipeline to produce a large degree of displacement. In this case, the traditional finite element method has a large error in solving simple statics problems, and the hypothesis of small deformation is no longer applicable. Shih et al.39 pointed out that the traditional finite element calculation of rigid body displacement is much larger than the pure deformation may lead to unstable results. In view of the shortcomings of the traditional finite element method in large deformation and large displacement of long-distance pipelines, the VFIFE method is adopted to simulate and analyze the entire pipeline.

The VFIFE method is an innovative method developed based on vector mechanics and the finite particle method, which was first proposed by Ting et al.40 The VFIFE discretizes the structure into particles, calculates the node displacement in the path element by Newton’s second law, and then calculates the pure deformation and internal force of the structure by the way of inverse motion, which does not need to correct the geometric nonlinearity of large deformation and large displacement of the structure. At present, the VFIFE has been developed into beam elements41, membrane elements42, plate elements43, solid elements44, and so on. Compared with the traditional finite element method, the VFIFE does not need to solve the complex global matrix when dealing with nonlinear problems, but directly operates the nodes when dealing with contact problems, and calculates the structural response by using a vector equation set, which can be solved simply and quickly.

In this paper, the self-developed mechanical analysis software for long-distance pipelines is used for calculation, which is compiled in Fortran language based on the principle of VFIFE. The software has advantages in dealing with contact, geometric nonlinearity, material nonlinearity, large displacement problem, parallel computation and so on. The dynamic tube-soil contact algorithm suitable for VFIFE, combined with the tube-shell coupling algorithm and MPI parallel technology, improves the calculation efficiency by reducing the calculation amount and improving the mechanical calculation efficiency of the long-distance pipeline. In Fig. 2, the comparison and analysis of the calculation results of the self-developed software with the finite element results and analytical solutions in literature verifies the feasibility of the software for the overall calculation of long-distance pipeline45. More verification data on the feasibility of using this software for mechanical calculation of long-distance pipelines can be found in literature46,47.

Fig. 2
figure 2

Comparison between software calculation results and literature. (a)\(\beta = 30^\circ\), (b) \(\beta = 45^\circ\) (\(\beta\) is the angle of the pipeline crossing the fault zone).

Full size image

Governing equation

The VFIFE discretizes the structure into a finite number of particles to describe the deformation and movement of the structure under load, and the mass (moment of inertia) of the element is equivalently concentrated in the element node to become the particle48. The motion of a particle is described by Newton’s second law:

$${\mathbf{M}}_{\alpha } \frac{{{\text{d}}^{2} {\mathbf{x}}_{\alpha } }}{{{\text{d}}t^{2} }}(t) = {\mathbf{P}}_{\alpha } {(}t{)}{\mathbf{ + f}}_{\alpha } {(}t{)}\quad \left( {\alpha = 1, \, 2, \, 3, \ldots N} \right)$$
(2)
$${\mathbf{I}}_{\alpha } \frac{{{\text{d}}^{2} {{\varvec{\uptheta}}}_{\alpha } }}{{{\text{d}}t^{2} }}(t) = {\mathbf{Q}}_{\alpha } {(}t{)}{\mathbf{ + m}}_{\alpha } {(}t{)}\quad \left( {\alpha = 1, \, 2, \, 3, \ldots N} \right)$$
(3)

where \({\mathbf{M}}_{\alpha }\) and \({\mathbf{I}}_{\alpha }\) represent the mass matrix and the moment of inertia matrix of the particle respectively; \({\mathbf{x}}_{\alpha }\) is the position of the particle; \(t\) is the time; \({{\varvec{\uptheta}}}_{\alpha }\) is the rotation vector; \({\text{d}}t\) is the size of the time step; \({\mathbf{P}}_{\alpha } {(}t{)}\) is the external force; \({\mathbf{f}}_{\alpha } {(}t{)}\) is the internal force, and \({\mathbf{Q}}_{\alpha } {(}t{)}\) and \({\mathbf{m}}_{\alpha } {(}t{)}\) are the external and the internal moments matrix, respectively.

In order to avoid the complicated iteration and convergence problems caused by the implicit solution, the VFIFE method often uses the central difference equation to solve the above-mentioned governing equations. The acceleration of a particle is expressed by the central difference equation as:

$${\mathbf{\ddot{x}}}_{n} = \frac{1}{{{\text{d}}t^{{2}} }}({\mathbf{x}}_{n + 1} - 2{\mathbf{x}}_{n} + {\mathbf{x}}_{n - 1} )$$
(4)

where \({\mathbf{x}}_{n + 1}\), \({\mathbf{x}}_{n}\) and \({\mathbf{x}}_{n - 1}\) are the displacement vectors of a particle at step n + 1, step n and step n−1, respectively.

By substituting Eq. (4) into Eq. (2), we get:

$${\mathbf{x}}_{{n + 1}} = \frac{{{\text{d}}t^{2} }}{{{\mathbf{M}}_{\alpha } }}{\mathbf{F}} + 2{\mathbf{x}}_{n} - {\mathbf{x}}_{{n - 1}}$$
(5)

Inverse motion and internal force calculation

The traditional finite element method uses the total displacement function including the rigid body displacement to simulate the total deformation of the element, and deducts the rigid body displacement by derivation, so as to obtain the strain and stress of the element. The VFIEF method uses the idea of inverse motion to make the beam element experience a virtual inverse motion and deduct the rigid body motion to calculate the pure deformation of the element49. Take element AB at ta time a as the initial position, and make \({\text{A}}_{b} {\text{B}}_{b}\) at tb time a virtual reverse motion, and reach \({\text{A}}^{\prime \prime } {\text{ B}}^{\prime \prime }\) after deducting the rigid body motion. At this time \({\text{A}}^{\prime \prime } {\text{ B}}^{\prime \prime }\) and \({\text{A}}_{a} {\text{B}}_{a}\) parallel, the morphological difference between the two is the pure deformation of the element within the path element (Fig. 3). The pure displacement obtained by the space beam element through reverse motion is:

$$\Delta \hat{l} = l_{b} - l_{a} = \left| {{\text{x}}_{B}^{b} - } \right.\left. {{\text{x}}_{A}^{b} } \right| - \left| {{\text{x}}_{B}^{a} - } \right.\left. {{\text{x}}_{A}^{a} } \right|$$
(6)
$$\Delta \hat{\varphi }_{i} = \left[ \begin{gathered} \Delta \hat{\varphi }_{ix} \hfill \\ \Delta \hat{\varphi }_{iy} \hfill \\ \Delta \hat{\varphi }_{iz} \hfill \\ \end{gathered} \right] = \left[ \begin{gathered} \Delta \hat{\theta }_{ix} - \hat{\theta }_{Ax} \\ \Delta \hat{\theta }_{iy} - \hat{\gamma }_{y} \\ \Delta \hat{\theta }_{iz} - \hat{\gamma }_{z} \\ \end{gathered} \right]\;\;(i = {A},{B})$$
(7)

where \(\Delta \hat{l}\) is axial elongation; \(\Delta \hat{\varphi }_{Bx}\) is the twist Angle of the meta axis;\(\Delta \hat{\varphi }_{Ay}\) and \(\Delta \hat{\varphi }_{Az}\) are the two corners of node A;\(\Delta \hat{\varphi }_{By}\) and \(\Delta \hat{\varphi }_{Bz}\) are the two corners of node B; \(\gamma\) is the rotational vector.

Fig. 3
figure 3

Reverse motion diagram of beam element.

Full size image

Based on the six pure deformation quantities obtained by the reverse motion of the element, the increment of the element internal force can be obtained according to the combined deformation and superposition principle of material mechanics. The matrix expression of internal force increment is as follows:

$$\left( {\begin{array}{*{20}c} {\frac{{E^{a} A^{a} }}{{l^{a} }}} & 0 & 0 & 0 & 0 & 0 \\ 0 & {\frac{{G^{a} \hat{I}_{x}^{a} }}{{l^{a} }}} & 0 & 0 & 0 & 0 \\ 0 & 0 & {\frac{{4G^{a} \hat{I}_{y}^{a} }}{{l^{a} }}} & {\frac{{2G^{a} \hat{I}_{y}^{a} }}{{l^{a} }}} & 0 & 0 \\ 0 & 0 & {\frac{{2G^{a} \hat{I}_{y}^{a} }}{{l^{a} }}} & {\frac{{4G^{a} \hat{I}_{y}^{a} }}{{l^{a} }}} & 0 & 0 \\ 0 & 0 & 0 & 0 & {\frac{{4G^{a} \hat{I}_{z}^{a} }}{{l^{a} }}} & {\frac{{2G^{a} \hat{I}_{z}^{a} }}{{l^{a} }}} \\ 0 & 0 & 0 & 0 & {\frac{{2G^{a} \hat{I}_{z}^{a} }}{{l^{a} }}} & {\frac{{4G^{a} \hat{I}_{z}^{a} }}{{l^{a} }}} \\ \end{array} } \right)\left( {\begin{array}{*{20}c} {\Delta \hat{l}} \\ {\hat{\varphi }_{Bx} } \\ {\hat{\varphi }_{Ay} } \\ {\hat{\varphi }_{By} } \\ {\hat{\varphi }_{Az} } \\ {\hat{\varphi }_{Bz} } \\ \end{array} } \right){ = }\left( {\begin{array}{*{20}c} {\Delta \hat{f}_{Ay} + \Delta f_{T + P} } \\ {\Delta \hat{m}_{Bx} } \\ {\Delta \hat{m}_{Ay} } \\ {\Delta \hat{m}_{By} } \\ {\Delta \hat{m}_{Az} } \\ {\Delta \hat{m}_{Bz} } \\ \end{array} } \right)$$
(8)

where \(E^{a}\) and \(G^{a}\) are the elastic modulus and shear model of the element material respectively; \(A_{a} ,I_{x}^{a} ,I_{y}^{a}\) and \(I_{z}^{a}\) are the section area of the beam element, the torsion section moment and the bending section moment in two directions, respectively; \(\Delta f_{T + P}\) is the equivalent axial force caused by the pressure and temperature inside and outside the pipeline.

The equivalent axial force caused by the internal and external pressure and temperature of the pipeline can be calculated by the following equation50:

$$\Delta f_{T + P} = E^{a} A^{a} \Delta T^{b - a} + \frac{\pi }{4}(1 - 2\nu )(p_{i} D_{i}^{2} - p_{o} D_{o}^{2} )$$
(9)

where \(\Delta T^{b - a}\) is the temperature change from time ta to time tb; \(D_{i}^{{}}\) and \(D_{o}^{{}}\) are respectively the equivalent inner diameter and outer diameter of the pipeline;\(p_{i}\) and \(p_{o}\) are respectively the internal and external pressure of the pipeline; \(\nu\) is Poisson’s ratio of wall material.

In VFIEF, the mass of the structure is borne by the element node, and the element has no mass. At any time, the element should satisfy the static equilibrium condition. In the process of reverse motion of the space beam element, the 6 degrees of freedom of the element AB are eliminated. In order to satisfy the static equilibrium condition, there are also six static equilibrium equations, that is, the resultant force and the resultant moment in the x, y and z directions are 0.

$$\sum {\hat{F}_{x} } = 0,\Delta \hat{f}_{Ax} = - \Delta \hat{f}_{Bx}$$
(10)
$$\sum {\hat{F}_{y} } = 0,\Delta \hat{f}_{Ay} = - \Delta \hat{f}_{By}$$
(11)
$$\sum {\hat{F}_{z} } = 0,\Delta \hat{f}_{Az} = - \Delta \hat{f}_{Bz}$$
(12)
$$\sum {\hat{M}_{x} } = 0,\Delta \hat{m}_{Ax} = - \Delta \hat{m}_{Bx}$$
(13)
$$\sum {\hat{M}_{y} } = 0,\Delta \hat{f}_{Bz} = \frac{1}{{l^{a} }}(\Delta \hat{m}_{Ay} + \Delta \hat{m}_{By} )$$
(14)
$$\sum {\hat{M}_{z} } = 0,\Delta \hat{f}_{By} = - \frac{1}{{l^{a} }}(\Delta \hat{m}_{Az} + \Delta \hat{m}_{Bz} )$$
(15)

Whole-local analysis process

In this paper, a combination of whole and local methods is proposed to analyze the indentation behavior of long-distance pipeline (Fig. 4). The overall model of the whole pipeline is established by the beam element, and the stress–strain response of the whole pipeline under soil displacement load and soil constraint is obtained by considering the pipe-soil interaction, additional load and hard constraint. In order to clarify the local indentation deformation characteristics of the pipeline, the shell element is used to establish a fine local model of the local pipeline, and the whole analysis result is used as a load on the local model to simulate the fine characteristics of the pipeline.

Fig. 4
figure 4

Schematic diagram of whole-local calculation process.

Full size image

Local pipeline analysis

Establishment of local model

The analysis of local indentations in pipelines focuses on the calculation of detailed features, aiming to assess the mechanical behavior of the pipeline under adverse loads and clarify the causes of failure. When analyzing the local model of the pipeline, it is essential to apply reasonable boundary conditions and validate the accuracy of the local model.

The whole model analysis can obtain the whole change characteristics of long-distance pipeline under external adverse load. But can’t give the local indentation deformation of pipeline. In order to determine the stress–strain response of the local area of the pipeline, the geometric modeling of the local pipeline is carried out by the shell element with the help of ABAQUS finite element software to realize the fine simulation of the local indentation characteristics. The constitutive relation of the pipeline is consistent with the whole analysis, and the connection between the pipeline and other components can be realized by binding, coupling, contact and other commands, and the detailed simulation analysis of the local pipeline can be combined with the calculation results of the whole pipeline model.

Determination of boundary conditions of local models

Due to the calculation accuracy and efficiency, the research carried out usually only simulates a small section of pipeline, and the form and parameters of the end constraints are difficult to determine, and the end constraints have a great influence on the accuracy of the calculation results. Therefore, based on the Saint–Venant principle, the analysis results of the whole pipeline model can be extracted as the boundary conditions of the local model to solve the constraint uncertainty problem of the local model end.

In mechanical analysis, if the surface force on a small part of the boundary of an object is transformed into a different but statically equivalent surface force, the stress distribution near the object will be significantly changed, but the effect at a distance will be negligible. For the pipeline model, the right end face of the pipeline is subject to the action of concentrated force F, shear force Q and bending moment M. Since the length of the long pipeline is much larger than the diameter, the left and right end faces belong to the secondary boundary, and the secondary boundary condition of the right end is concentrated load (Fig. 5), it is difficult to list the precise Eq. (16) of stress boundary condition. However, the equivalent boundary conditions can be listed according to the principle of Saint–Venant to calculate the analysis.

$$\begin{gathered} l(\sigma_{x} )_{s} + m(\tau_{yx} )_{s} = \overline{f}_{x} \hfill \\ m(\sigma_{y} )_{s} + l(\tau_{xy} )_{s} = \overline{f}_{y} \hfill \\ \end{gathered}$$
(16)

where l and m are the direction cosine of the angle between the section normal and the x and y axes, \(\sigma_{x}\)、\(\sigma_{y}\) are the stress of the pipe in the x and y directions, \(\tau_{yx}\) and \(\tau_{xy}\) are the shear stress.

Fig. 5
figure 5

Force diagram of local pipeline model.

Full size image

It is assumed that there is a set of surface force systems, at the right free boundary, which are statically equivalent to the concentrated loads F, Q and M, we can obtain:

$$\int\limits_{d/2}^{D/2} {\overline{f}_{x} dy} = F \int\limits_{d/2}^{D/2} {\overline{f}_{y} dy} = Q \int\limits_{d/2}^{D/2} {y\overline{f}_{x} dy} = M$$
(17)

The relationship between the assumed surface force system and its corresponding stress component at the free end of the pipeline is as follows:

$$2\pi y(\sigma_{x} )_{x = l} = \overline{f}_{x} ,\;\;2\pi y(\tau_{xy} )_{x = l} = \overline{f}_{y}$$
(18)

Combining Eqs. (18), (17) is renewed as:

$$\int\limits_{d/2}^{D/2} {2\pi y(\sigma_{x} )_{x = l} dy} = F\;\int\limits_{d/2}^{D/2} {2\pi y(\tau_{xy} )_{x = l} dy} = Q\;\int\limits_{d/2}^{D/2} {2\pi y^{2} (\sigma_{x} )_{x = l} dy} = M$$
(19)

The Eq. (19) shows that on the boundary of the free end of the pipeline, the principal vector and principal moment of the stress to be found at the boundary are equal to the resultant force and moment of the external force. It can also be expressed that on a small boundary, the principal vector and principal moment of the stress should be equal to the principal vector and principal moment of the surface force, respectively, and the values are the same and the direction is also the same.

Verification of finite element model

To ensure the accuracy of the finite element model, the finite element simulation analysis is carried out on the uniaxial strain gradient behavior test of X80 steel pipe indentation carried out by the literature51, and the finite element simulation results are compared with the test results. The quasi-static compression test is carried out on an INSTRON8502-250kN tester with spherical indenter radius of 10 mm, pipe diameter of 44 mm, wall thickness of 2 mm, and pipe made of X80 steel. Specific parameters are shown in Table 1. The pipe is placed in the steel saddle-shaped groove, and the simulation of depression deformation is divided into pre-loading, loading and unloading, as shown in Fig. 6.

Table 1 Material properties for X80 pipeline steel.
Full size table
Fig. 6
figure 6

Schematic diagram of test and simulation process.

Full size image

As can be seen from Table 2, when the displacement loads of the indenter are 4mm, 7mm and 10mm respectively, the test results are very close to the values of the rebound coefficients of the finite element simulation results, and the errors are all within 5%. Considering the influence of the boundary conditions at the bottom of the pipeline, both errors are reasonable in a certain range, which shows that the finite element model and the numerical calculation method are effective.

Table 2 Comparison table between test results and finite element simulation results.
Full size table

Project case application

Project overview

In this section, the analysis of the indentation behavior of long-distance pipelines is conducted using the whole-to-local analysis approach. A self-developed mechanical analysis software for long-distance pipelines is utilized to consider the constraints and loading conditions of actual engineering projects, enabling the computation of the whole pipeline behavior. Taking into account the connection between the pipeline and supporting structures in practical scenarios, and considering nonlinear contact issues, a local model of the pipeline and support bus is established, with the results from the global analysis applied as boundary conditions to the local model. Based on the computed Mises stress, plastic strain, and depression depth, the deformation characteristics of local indentations in the pipeline are analyzed under bending loads, concentrated loads, and internal pressure loads.

In the second Mawan Branch pipeline project of South China Pipeline Guangdong Oil Transmission, the diameter of the pipeline is 323.9 mm, the material of the pipeline is X52, and the wall thickness is 6.4 mm. During the in-pipeline detection and IMU detection, it was found that there were 25 depressed deformation points at the bottom of a section of the pipeline (Fig. 7a). The length of this section of the pipeline is 233 m, and the locations of the depression deformation points are mainly distributed in four sections of the pipeline. As shown in Fig. 7b, the pipeline is located on the concrete buttress, and the site survey found that the indentation is located at the concrete buttress position, and the indentation is more obvious, with the maximum deformation of the indentation reaching 28 mm.

Fig. 7
figure 7

Schematic diagram of pipe indentation deformation. (a) buttresses mileage distribution, (b) Pipe deformation.

Full size image

In order to understand the current stress level and stress concentration section of the pipeline, and provide a basis for further formulation of excavation and treatment plans, this case study will examine the mechanical response characteristics of the pipeline section under adverse load by adopting the whole-local analysis process on the basis of data compilation and field investigation, and then evaluate the stress level and stress distribution characteristics of the pipeline.

Whole analysis

Whole model

The grade of the pipe steel is X52. The constitutive model is the Ramberg–Osgood model mentioned above, where the elastic modulus is 2.1 × 105 MPa and the yield strength is 389 MPa, the yield offset is 1.699, and the strengthening index is 14.14. The stress–strain curve of the pipeline is shown in Fig. 8. In order to avoid the influence of pipeline end deformation on the calculation results, the whole model size of this analysis is 650 m, and the whole modeling of the pipeline is carried out using beam elements. The mesh size of the curved pipe section is 0.1 m, and the mesh size of the straight pipe section is 0.2 m, which meets the requirement of GB/T 50470-2017 that the maximum mesh size is not more than 1 times the diameter of the pipe. In order to simulate the constraining effect of the buttresses on the pipeline, the lateral and vertical displacement of the pipeline are limited at the contact position between the pipe and the buttresses. The interaction between the pipeline and the soil mass is simulated by a nonlinear three-way soil spring, the soil mass is buried 2 m deep and the soil layer is medium sandy soil (Table 3). The specific parameters of the soil spring can be obtained by solving the problem (Table 4).

Fig. 8
figure 8

Stress–strain curve of X52 pipeline steel.

Full size image
Table 3 Soil parameters table.
Full size table
Table 4 Soil spring parameters table.
Full size table

Load conditions

The field observation shows that the overlying soil of this section of the pipeline produces displacement settlement under the influence of external unfavorable factors. The supporting capacity of the backfill under the pipeline becomes weak, and the pressure of the overlying soil above the pipeline and the dead weight of the pipeline are mainly borne by the concrete buttresses (Fig. 9). The influence of settlement displacement on the pipeline is applied to the analysis model by means of displacement loading. According to the field investigation data, the maximum settlement displacement of soil is 0.05m, and the pipe with depression section is located in the center area of soil settlement. In order to grasp the stress level and distribution characteristics of the pipeline under soil settlement, the settlement displacement of 25 dental pipeline sections can be set as the maximum uniform distribution, and the displacement load from this section of pipe to the left and right end faces of the model is gradually reduced to 0, which satisfies the continuous distribution of soil settlement. In the engineering case studied in this paper, according to the geological and climatic conditions, the temperature change is not significant, and the influence of temperature on the calculation results is not considered for the time being.

Fig. 9
figure 9

Model diagram of pipeline load.

Full size image

Whole calculation and analysis

Considering the main sources that affect the stress level of the pipeline, the whole model analyzes the stress variation of the pipeline under two different concrete distributions. As shown in Fig. 10a, the first distribution form is based on the IMU test results of the pipeline, assuming that the concrete buttress is only located at the position where the pipeline is dented. As shown in Fig. 10b, the second distribution assumes that the concrete buttresses are evenly distributed and spaced 5 m apart. The whole pipeline model is shown in Fig. 11. The indentation deformation is mainly located in the pipeline segment from 200 to 400 m along the axis. Whether the concrete support buttress is distributed uniformly or non-uniformly, the pipe will bear the bending action under the soil settlement and displacement load. There is a significant stress concentration in the pipe at the position of the support buttress. The upper part of the pipe at the position of the support buttress is strained and the lower part is pressured, and the upper part of the pipe between the two buttresses is pressured and the lower part is strained.

Fig. 10
figure 10

Distribution diagram of concrete buttress. (a) Non-uniform distribution, (b) Uniform distribution.

Full size image
Fig. 11
figure 11

Schematic diagram of the whole pipeline model change.

Full size image

The stress calculation results and restraint forces for the pipeline are illustrated in Fig. 12. They show that the distribution form of the supports has a significant impact on the vertical bending stress of the pipeline when the soil experiences displacement and settlement, but have little effect on the horizontal bending stress and the average axial stress of the pipeline. When the supports are unevenly distributed, the bending stress of the pipeline at the support locations fluctuates significantly, with a maximum value of up to 110 MPa. When the supports are uniformly distributed, the bending stress of the pipeline at the support locations remains relatively consistent, with a magnitude of approximately 60 MPa. The bending stress at the two end supports is slightly higher, approaching 80 MPa. The distribution form of the supports has a significant impact on the restraint forces of the pipeline. When the supports are unevenly distributed, there is a larger variation in the forces experienced by the pipeline at the support locations, with the maximum restraint force being 95.5 kN and the minimum being 81.4 kN. When the supports are uniformly distributed, the pipeline experiences relatively consistent forces at the support locations, with the restraint forces ranging between 84 and 86 kN.

Fig. 12
figure 12

The result of whole calculation. (a) Pipeline stress change curve of non-uniform distribution, (b) Pipeline stress change curve of uniform distribution, (c) Restraint forces of non-uniform distribution, (d) Restraint forces of uniform distribution.

Full size image

Local analysis

Local model

The local model consists of the pipeline and concrete buttress. Because stress concentration is likely to occur in the contact area between the pipeline and concrete buttress under external adverse loads, and the contact analysis between hard supports such as concrete buttress and pipeline shows strong nonlinear behavior, a three-dimensional finite element model is established using nonlinear finite element software ABAQUS for analysis. The pipeline is modeled using the S4R three-dimensional shell element. The length of the pipeline is 5 m, and the thickness is consistent with the pipe diameter and the whole model (thickness 0.0064 m, pipe diameter 0.3239 m). The rigid rectangular model (length 0.8 m, width 3 m and height 0.4 m) is selected for the concrete buttress. The simulation of any dent size can be realized by changing the rectangular size, so that the model is closer to the actual situation.

To improve the calculation efficiency, the grid in the contact area between the pipeline and the concrete buttress is refined, and the grid in other areas of the pipeline is coarser. The global size of the whole model is, width 0.04 m, the mesh refinement size of the contact area between the pipeline and the concrete buttress is 0.01 m, and the size of the concrete buttress is 0.1 m. The ring division is 64 copies, the number of nodes is 113,383, the number of grids is 106,368, and the grid division form can meet the calculation accuracy requirements after a lot of trial calculations. The contact between the pipe and the concrete buttress is set to be face-on contact. The concrete buttress surface is the main surface, while the outer surface of the pipe is the slave surface. Normal “hard” contact and tangential friction-free contact are made to ensure the continuity of the force and deformation of the pipeline, release the vertical constraints of the concrete buttress, and allow the axial displacement and vertical rotation of the pipeline, as shown in Fig. 13.

Fig. 13
figure 13

Model diagram.

Full size image

Local calculation and analysis

The calculation and analysis are carried out on the two working conditions of uniform distribution and non-uniform distribution respectively. As can be seen in Fig. 14, the local indentation deformation of the pipeline obtained by finite element calculation and analysis is basically consistent with the indentation characteristics of the field survey.

Fig. 14
figure 14

Diagram of local deformation of pipeline.

Full size image

The stress of the pipe can be analyzed and evaluated according to the shape change energy density theory. According to the specific energy theory of shape change, the specific energy density of shape change is the main factor causing material yield. Under the general stress state, as long as the specific energy of shape change somewhere in the material reaches the limit value of the material yield, the material will exhibit significant plastic yield there. Therefore, it is more appropriate to use the Mises equivalent stress following the shape-changing energy density theory to evaluate pipeline stress for the stress problem studied in this paper.

Figure 15 and Table 5 shows the local calculation results. In Fig. 15a, the stress concentration phenomenon is relatively obvious at the contact point between the pipe and the concrete buttress, and the stress distribution presents a “dumbbell” shape. The influence area of stress variation is large when the concrete buttresses are non-uniformly distributed. The maximum Mises stress is 424.9 MPa when the buttresses are non-uniformly distributed, and the maximum Mises stress is 411 MPa when the buttresses are uniformly distributed. The stress distribution trend of the two conditions is basically the same, and the maximum values are the same at the contact edge of the pipeline and concrete buttress, and the Mises values exceeded the yield stress of the pipeline, while in the intermediate contact area between the pipeline and concrete buttresses, the Mises changed little and the minimum values appeared in the center, basically conforming to the deformation characteristics of the shell structure.

Fig. 15
figure 15

The result of local calculation. (a) Mises stress, (b) PEEQ, (c) depression depth.

Full size image
Table 5 Local pipe calculation results table.
Full size table

In Fig. 15b, the plastic strain (PEEQ) appears at the contact edge of the pipeline and concrete buttress and extends to the middle. The maximum PEEQ of the pipeline is 0.89% when the concrete buttresses are non-uniformly distributed. The maximum PEEQ of the pipeline is 0.42% when the concrete buttresses are uniformly distributed. The PEEQ increases first and then decreases along the axial position from the center of the pipeline to the edge and reaches the maximum value at the contact edge between the pipeline and the concrete buttress. The PEEQ of the pipeline is greater when the concrete buttresses are non-uniformly distributed at the same position than when the concrete buttresses are uniformly distributed.

In Fig. 15c, when the concrete buttresses are non-uniformly distributed, the depth deformation of the pipeline is 30.08 mm, with a ratio of 8.9% to the outside diameter. When the concrete buttresses are uniformly distributed, the depth deformation of the pipeline is 21.57 mm, with a ratio of 6.4% to the outside diameter. The deformation of the pipe depression is generally consistent with the local deformation characteristics obtained from the site survey. Under the two buttress distribution patterns, the indentation variation trend of the contact area between the pipe and the buttress is basically the same, and the edge of the pipe along the axis gradually decreases.

Analysis of influencing factors

Concentrated load

The field data indicates that the deformation of the pipeline varies at different buttress locations. According to the comprehensive analysis and calculation results, the stress levels and deformation characteristics of the pipeline under both uniform and non-uniform distribution of buttresses have been analyzed in the preceding section. To further clarify the stress response characteristics of the pipeline under external loads, the significance analysis of external loads is required.

Figure 16 shows the change curves of the middle depth, PEEQ and Mises stresses of the pipeline when the concentrated load ranges from 80 to 96kN. In Fig. 16a, when the bending load is 60 MPa and the axial load is 6 MPa, the indentation depth deformation is the same in the contact area between the pipeline and the buttress, and the maximum value is reached at the contact edge. Away from the contact area between the pipeline and the buttress, the indentation depth gradually decreases, and the concentrated load gradually increases from 80 to 96 kN. The maximum dip depth of the pipe increased from 20.35 mm to 24.61 mm, with an increment of 4.26 mm. It can be seen from Fig. 16b and c that when the concentrated load gradually increased from 80 to 96 kN, the maximum PEEQ increased from 0.29% to 0.64% with an increment of 0.35%, and the Mises stress increased from 407.14 MPa to 420.25 MPa with an increment of 13.11 MPa. With the gradual increase of the center distance of the pipeline, the PEEQ and Mises stress of the pipeline first increased and then decreased. The maximum value is obtained at the contact edge between the pipe and the support buttress. The minimum value is obtained at the contact center.

Fig. 16
figure 16

Change curve of contact area between pipeline and support buttress under concentrated load. (a) depression depth, (b) PEEQ, (c) Mises stress.

Full size image

Moment load

Figure 17 shows the change curves of the middle depth, PEEQ and Mises stresses of the pipeline when the bending load ranges from 60 to 140 MPa. In Fig. 17a, when the concentrated load is 80 kN and the axial load is 6 MPa, the deformation trend of the depression depth in the contact area between the pipeline and the concrete buttress is consistent under different bending moment loads, and the maximum value is reached at the contact edge. Away from the contact area between the pipeline and the concrete buttress, the depression depth gradually decreases, and the bending load gradually increases from 60 to 120 MPa. The dip depth of the pipeline gradually increased from 20.35 mm to 28.37 mm, with an increment of 8.02 mm. As shown in Fig. 17b and c, when the bending load gradually increased from 60 to 120 MPa, the maximum PEEQ increased from 0.29% to 0.43% with an increment of 0.14%, and the Mises stress increased from 407.14 MPa to 412.85 MPa with an increment of 5.71 MPa. With the gradual increase of the center distance of the pipeline, the PEEQ and Mises stress of the pipeline first increased and then decreased, and the maximum value was obtained at the contact edge (the most disadvantaged position) between the pipeline and the concrete buttress. The minimum value was obtained at the contact center, which is consistent with the deformation trend of the pipeline discussed under concentrated load, and the stress response of the pipeline under concentrated load is more significant.

Fig. 17
figure 17

Variation curve of contact area between pipe and support buttress under different bending moment load. (a) depression depth, (b) PEEQ, (c) Mises stress.

Full size image

Internal pressure load

During the service of the pipeline, the inner wall of the pipeline will be subjected to pressure due to the presence of the conveying medium, which will affect the force and deformation of the pipeline. Therefore, it is necessary to simulate and analyze the mechanical response of the pipeline under internal pressure load to obtain the deformation characteristics of the pipeline under internal pressure load. The depth and stress at the contact edge point between the concrete buttress and the pipeline under internal pressure load from 0 to 9 MPa and concentrated load from 80 to 100 kN are showed in Fig. 18. In Fig. 18a, with the gradual increase of internal pressure, the indentation deformation of the pipeline first decreases and then increases. When the internal pressure increases from 0 to 4 MPa, the indentation rebound at the contact edge point becomes smaller and smaller. However, the depression deformation gradually increased in the process of increasing from 4 to 9 MPa. It can be seen from Fig. 18b that with the gradual increase of internal pressure, the Mises stress in the pipeline first decreased and then increased, and the Mises stress changed significantly with the increase of internal pressure load. When the internal pressure load is 4 MPa, the Mises stress reaches the minimum value. During the service of the pipeline, low pressure load can reduce the stress state of the pipeline to a certain extent, making the pipeline indentation deformation rebound. However, high pressure load will aggravate the indentation deformation of the pipeline, which is not conducive to the continued service of the pipeline.

Fig. 18
figure 18

Change curve of contact edge points under internal pressure load. (a) Depression depth, (b) Mises stress.

Full size image

Conclusion

In order to grasp the deformation characteristics of dented pipeline in engineering practice, a method combining the whole and the local is proposed to calculate and analyze the pipeline. Based on the whole and local method, the deformation characteristics of long-distance oil and gas pipelines under typical working conditions are analyzed.

The results show that:

  1. (1)

    Based on the principle of VFIFE, the mechanical analysis software of long-distance oil and gas pipeline is developed by ourselves considering the conditions of pipe-soil interaction, additional load and hard constraint. The software is convenient to calculate the whole pipeline, and the stress level and stress distribution characteristics of the pipeline can be obtained.

  2. (2)

    The pipeline deformation in the project case is basically consistent with the actual situation, and the feasibility of combining the whole and the local analysis method is verified. The Mises stress, PEEQ and depression depth of the pipeline reach the maximum value at the contact edge between the pipeline and the support buttress, which is the most unfavorable position of the pipeline. Compared with the bending load, the pipe stress under concentrated load changes significantly.

  3. (3)

    With the gradual increase of internal pressure, The Mises stress decreased first and then increased. When the internal pressure load was 4 MPa, the Mises stress reached the minimum value. During the service stage of the pipeline, low-load conditions can lead to the elastic recovery of indentation deformation in the pipeline, but high-load conditions will exacerbate the indentation deformation, which is detrimental to the continued service of the pipeline.

The dental defects are not conducive to the safe operation of the pipeline, which will cause cracks in the pipeline in serious cases, and then lead to the leakage of the conveying medium, resulting in environmental pollution or security risks. In order to reduce the dented deformation of the pipeline, based on the content of this study, some protective and remedial measures related to the dented pipeline in the project are withdrawn:

  1. (1)

    Foundation treatment should be carried out when pipeline is laid, and the bearing capacity of soil should be enhanced by foundation reinforcement and grouting. Under the pipeline can be laid with a high bearing capacity of gravel, gravel and other cushions to provide more stable support to prevent pipeline settlement.

  2. (2)

    The steel plate or sleeve is used to strengthen the part of the pipeline in contact with the support buttress, pipe clamp and other structures to enhance the strength of the pipeline and improve the local bearing capacity of the pipeline.

  3. (3)

    The spacing and shape of the support structure should be reasonably designed, and the contact area between the support structure and the pipeline should be increased to avoid excessive local stress of the pipeline.