The double-ellipsoid heat source distribution model shown in Fig. 1, which can better depict the real welding pool morphology and heat source distribution under actual welding conditions, was adopted in the welding simulation (Obeid et al., 2017).

The heat flux distribution in the first semi-ellipsoid can be written as 1qf=63ffQπ3/2a1bcexp⁡-3xa12+yb2+zc2, where qf is the heat flow at point (xyz) in the first semi-ellipsoid heat source at time t, ff is the heat source partition coefficient in the first semi-ellipsoid, Q is the welding energy input rate, a1 is the half-axis length of the first semi-ellipsoid molten pool, b is the width of the molten pool, and c is the depth of the molten pool.

The heat flux distribution in the last semi-ellipsoid can be expressed as 2qr=63frQπ3/2a2bcexp⁡-3xa12+yb2+zc2, where qr is the heat flow at point (xyz) in the last semi-ellipsoid heat source at time t, fr is the heat source partition coefficient of the last semi-ellipsoid, and a2 is the half-axis length of the last semi-ellipsoid molten pool.

If P is the welding power and η is the welding heat source efficiency, respectively, the energy input rate can be deduced as 3Q=ηP. It can be seen that the welding heat input is related to the welding heat source efficiency and welding power. According to the manual of the welding process and the geometric dimensions of the pipeline, the submerged arc welding was adopted, and the welding heat source efficiency was determined as 0.8. An ABAQUS UMAT subroutine was programmed to describe the motion of the moving heat source accurately.

The dimensions of the welded pipeline are as follows: a diameter of 660 mm, a length of 2000 mm and a thickness of 6.4 mm. The welding finite-element model is shown in Fig. 2, the welding process is accomplished by three-pass submerged arc welding in a V-type groove (the bottom edge clearance of the V groove is 4 mm, and the groove angle is 60°), and the welding process parameters are listed in Table 1.

In the finite-element simulation, the welding metal and the base metal were assumed to be the same material, with the chemical compositions listed in Table 2. The thermal physical and mechanical properties are listed in Tables 3–4 (Yan et al., 2014). As can be seen, the physical and mechanical properties of X80 steel are highly dependent on the temperatures.

The governing equation of the transient heat transfer analysis during the welding process is given as 4ρcα∂T∂t=∂∂xλ∂T∂x+∂∂yλ∂T∂y+∂T∂zλ∂T∂z+Q, where ρ is the material density, cα is the specific heat, T is the temperature, t is the time, and λ is the thermal conductivity coefficient.

The radiation heat transfer dominates at the higher temperature near the welding seam, while convection heat transfer dominates at the surface of the welding zone with a lower temperature away from the welding zone. Therefore, the combined boundary conditions in Eq. (5) are used to apply convection and radiation to the surface of the welding zone in the form of convection by a comprehensive heat transfer coefficient H (Obeid et al., 2017), and the initial ambient temperature was set to 20 °C. 5H=0.0668T0<T<500°C0.231T-82.1T≥500°C The stress–strain calculation during the welding is always based on the results of the temperature field. Generally, the welding stress may exceed the yield limit, which requires the thermal–elastoplastic theory to calculate the thermal stress accurately. In ABAQUS, the total strain rate ε˙ can be decomposed and expressed as below: 6ε˙=ε˙e+ε˙p+ε˙th, where ε˙e is the elastic strain rate, ε˙p is the plastic strain rate, and ε˙th is the thermal strain rate.

The isotropic strain-hardening model was employed to describe the initial yield and cyclic yield behavior. During the mechanical simulation, the evolution of the yield surface radius R0 was described by 7R0=σ0+Qin1+e-b0ε‾pl, where σ0 is the yield stress of the zero plastic strain, Qin and b0 are the material parameters, and ε‾pl is the equivalent plastic strain.

Assuming that the temperature-related mechanical properties and stress–strain vary linearly over small time increments, the stress–strain relationship in the elastic or plastic state follows 8dσ=Ddε-CdT, where dσ is the stress increment, D is the elastic or plastic matrix, dε is the strain increment, C is the temperature-related vector, and dT is the temperature increment.

A certain element in an elastic or plastic state has the following equilibrium equation: 9dFe+dRe=Kedδe, where dFe is the force increment on the elemental node, dRe is the equivalent nodal force increment caused by temperature-induced initial strain, Ke is the element stiffness matrix, and dδe is the nodal displacement increment.

The finite-element-based thermal stress calculation during welding is listed as follows: when the welding temperature field is obtained, the displacement increment dδe and strain increment dεe of each node can be calculated by adding the temperature increment gradually. According to the stress–strain relationship shown in Eq. (6), the stress increment dσ of each element can be obtained. In this way, the dynamic stress–strain variation and the final residual stress distribution during the entire welding process can be obtained.

To clearly show the temperature change, path L1 at the inner surface and path L2 at the outer surface in the middle cross section M–M are selected, as shown in Fig. 3. By adjusting the welding heat source parameters, the temperature distribution of the welding molten pool can be obtained. Figure 4 demonstrates the molten pool morphology with the welding process parameters listed in Table 1. It can be found that the molten pool can melt through the welding seam, which indicates that the selected welding parameters are effective for the simulation.

Figures 5–6 show the time-dependent temperature at different positions at paths L1 and L2 during the third-pass welding. The maximum temperature of A1 located at the center of the inner surface of the welding seam is 1326 °C. Due to the spatial distance difference, the moments when inner-surface nodes A1, B1 and C1 reach their maximum temperature are delayed successively. Node A1 is closest to the welding heat source, so node A1 has the fastest heating rate and cooling rate. After 300 s, the temperatures of A1, B1 and C1 are very close, and the temperatures cool to room temperature after 4000 s. Node A2 located at the center of the outer surface of the welding seam has a maximum temperature of 2054 °C. The temperature cycles of outer-surface nodes A2, B2 and C2 are similar to those of the inner surface nodes.

The residual stress caused by the non-uniform welding temperature was simulated using the sequential coupling method. Figure 7 shows the residual stress in the welding seam. The high Mises stress is mainly concentrated in the welding seam and HAZ, and the peak value of the residual stress is up to 537 MPa, which approaches the yield strength of the X80 steel. Figures 8–9 demonstrate the residual stresses along paths L1 and L2 at the inner and outer surfaces, respectively. The residual stress distribution at the inner surface is slightly larger than that at the outer surface. The axial stress is always in tension along path L1. However, the axial stress in the center area of the outer surface is in compression, while the axial stress quickly transforms into tensile stress outward along the welding seam.

In this section, the effect of the welding groove angle on the residual welding stress is analyzed. Figure 10 demonstrates the influence of the groove angle on the residual Mises stress at the inner surface of the welding seam and the HAZ. With the increase in the welding groove angle from 40 to 80°, the residual Mises stress at the inner surface increases from 535 to 539 MPa. Figure 11 shows the influence in the groove angle on the residual Mises stress at the outer surface. With the increase in the welding groove angle, the peak Mises stress at the center of the welding seam decreases from 528 to 506 MPa, but the high-stress zone at the HAZ broadens. In general, the peak Mises stress at the outer surface is more sensitive to the change in the groove angle.

Figure 12 shows the effect of welding heat input on the Mises stress variation along path L1. As can be seen, the Mises stress at the inner surface increases with the increase in the welding heat input. Figure 13 shows the effect of welding heat input on Mises stress variation along path L2. The peak Mises stress at the center of the welding seam decreases, while the Mises stress at the HAZ increases with the increase in the welding groove angle. The influence of welding heat input on the residual Mises stress is the same as that of the welding groove angle. In the actual operation of pipeline welding, the welding process parameters can be optimized to reduce the residual welding stress.

To verify the effectiveness of finite-element simulation in welding residual stress, the actual X80 pipeline was welded circumferentially under the same conditions, and the residual stress of the welded pipeline was measured by the ultrasonic LCR wave-detecting method. Egle and Bray (1976) conducted extensive experiments to compare the traveling characteristics of different types of waves inside the metal material and found that the ultrasonic LCR waves have a higher sensitivity to stress than other types of ultrasonic waves.

According to the ultrasonic LCR wave-detecting method, within a fixed acoustic path L, the relationship between stress variation Δσ and acoustic traveling time difference Δt can be expressed as (Duquennoy et al., 2008) 10Δσ=KΔt=Kt-t0, where K is the stress coefficient in the formation 11K=-2V03λ+2μ/[(4λ+10μ+4mμ+2l-3λ-10μ-4mλ+2μ)L]., in which V0 represents the traveling velocity of the LCR wave in the zero-stress state, λ and μ are Lamé constants, and l and m are the Murnaghan constants (Akbarov, 2012).

According to Eq. (8), the quantitative relationship between stress and ultrasonic LCR wave traveling time can be established under different tensile states. To measure the residual stress, it is necessary to calibrate the stress coefficient K and the traveling time of the ultrasonic LCR wave in zero stress in advance. The flow chart of the ultrasonic LCR wave stress test platform is shown in Fig. 14, and the specific implementation steps are as follows: (1) place the ultrasonic transducer probe and specimen in a constant temperature box and inject 5 mL of coupling agent onto the contact surface between the probe and specimen using a syringe; (2) when the coupling agent reaches a stable state, measure the LCR wave propagation time t0 at the zero-stress state using an online stress ultrasonic measurement system; (3) fix the X80 specimen on a universal testing machine and adjust the propagation direction of the LCR wave parallel to the direction of the loading stress; (4) load the specimen, starting from the free state until the external load stress reaches about 70 % of the yield strength, and measure the traveling time of LCR waves under the load; and (5) analyze the results of the calibration experiments and determine the stress coefficient K. According to the traveling time difference, the calibration results of the X80 steel can be obtained and are shown in Fig. 15, in which the stress coefficient K equals 16.109 MPa ns-1.

The welding residual stress-detecting process of the X80 pipeline using the ultrasonic LCR wave method is shown in Fig. 16. The comparison between the stress detection and simulation results on the inner and outer surfaces of the welding seam is demonstrated in Fig. 17. Through the data analysis, the maximum error between the simulation results and test results is 26.7 %, which indicates that the welding process simulation of X80 pipelines with the finite-element method is feasible.