Numerical simulation of residual stress and deformation of butt weld of SUS304 stainless steel pipe
Stainless steel has excellent corrosion resistance and plays an important role in the process of ship building in China, especially for some key bearing parts of ship lift, stainless steel plays an irreplaceable role . In the manufacturing process of stainless steel components, welding is the most common means of connection. However, the welding residual stress and deformation are inevitable when the component undergoes local heating and rapid cooling during welding [2-3]. Because the ship works on water for a long time, the corrosion environment is bad. Under the joint action of corrosion medium and welding residual stress, it is easy to induce stress corrosion phenomenon, which greatly reduces the service life of the workpiece. In addition, the welding deformation after welding not only affects the appearance of the product, but also brings assembly problems. Correcting the welding deformation not only prolongs the production cycle but also increases the manufacturing cost [4-6]. Therefore, how to effectively predict and control welding residual stress and deformation in actual welding production has very important engineering application value.
Based on ABAQUS finite element analysis software, the “thermo metallurgical mechanical” coupling finite element calculation method is developed for the butt welded joint of SUS304 steel pipe. This method is used to simulate the temperature field, residual stress and welding deformation of the welded joint. The characteristics of temperature field and weld pool distribution of TIG welded joint, as well as the influence of angle change on the distribution of residual stress on the inner and outer surface of steel pipe are discussed.
Table of Contents
The test object is SUS304 steel pipe butt welding joint, the specification is Φ 48 mm × 5 mm, and the filler material is a308l. The welding method is manual TIG welding with direct current positive connection. The protective gas is pure argon with gas flow of 10-15 L / min. the pipe is filled with pure argon with flow of 1-2 L / min. other welding parameters are shown in Table 1. Before welding, the sundries within 2cm of the interface end shall be cleaned. The temperature between welding layers shall be lower than 150 ℃, and the sample size and weld bead layout are shown in Figure 1.
Table 1 Welding parameters of SUS304 steel pipe butt welding
Figure 1 Sample size and weld bead arrangement
Finite element method
Based on ABAQUS finite element commercial software, the “thermal elastic plastic” finite element method is used to simulate the welding process of steel pipe. In this method, the sequential coupling method is used to calculate, that is, the temperature field is calculated first to get the temperature cycle history of each node in the finite element model, and then in the calculation of the stress and deformation field, it is used as the thermal load to calculate the displacement of each node and the stress-strain value of each element.
In the calculation of material model, the change process of various thermophysical parameters and mechanical property parameters of the material with temperature is considered. The thermophysical parameters of the material are shown in Table 2, and the mechanical property parameters are shown in Table 3. At the same time, in the process of mesh generation of the finite element model, in order to balance the calculation time and efficiency, the mesh generation is relatively intensive near the weld and heat affected zone, and relatively sparse in other areas. The number of nodes of the whole model is 31080, and the number of elements is 25200. The finite element mesh model of the three-dimensional model is shown in Figure 2. Among them, the element type is dc3d8 in the calculation of temperature field and c3d8i in the calculation of stress and deformation field.
Table 2 Thermophysical parameters of materials
Table 3 Mechanical property parameters of materials
Figure 2 Three dimensional finite element mesh model
Calculation of temperature field
In the calculation of the temperature field, the DFLUX equal density heat source  subroutine written by FORTRAN is used to simulate the heat input in the welding process. The welding heat analysis process is a typical nonlinear transient heat transfer process, and its control equation can be expressed as
In the formula:
- ρ – material density, g / mm3;
- C — specific heat capacity of material, J / (g ·℃);
- T — temperature, ℃;
- T — time, s;
——Heat flux vector, w / mm2;
Q – heating rate of internal heat source, w / mm3;
——Space gradient Laplacian operator.
The conduction process of arc heat in workpiece is described by Fourier nonlinear heat conduction law. The conduction equation is
In the formula: K — thermal conductivity, J / (mm · s ·℃).
In the welding process, not only the heat conduction inside the workpiece, but also the heat exchange between the workpiece and the external environment should be considered. The process of the workpiece radiating heat from the surface to the environment includes convection and radiation. In the calculation, the ambient temperature is set as 20 ℃, and Newton’s law is used for the convection heat transfer calculation. The convection heat transfer equation is
HC – heat transfer coefficient, HC = 33 × 10-6 w / (mm2 ·℃);
TS — workpiece surface temperature, ℃;
T0 – link temperature, ℃.
In addition, the influence of radiation and heat dissipation should be considered. According to Boltzmann’s law, the heat dissipation equation is
ε – thermal emissivity, ε = 0.8;
σ – Stefan soltaman constant.
In addition, the influence of the latent heat of crystallization during the welding process is also considered. For SUS304 stainless steel, the latent heat value of crystallization is 260 J / g, and the temperature of liquidus and solidus are 1 390 ℃ and 1 340 ℃, respectively.
Calculation of stress and deformation field
In fact, the calculation of stress and deformation field is the analysis process of mechanical problems. Using the same mesh model as the previous thermal analysis, the node temperature cycle calculated by the temperature field is loaded in the form of thermal load to obtain the residual stress and deformation in the welding process. The elastic stress-strain relationship follows the Hooke’s law, while the von Mises criterion is used to describe the plastic behavior. For austenitic stainless steel, work hardening will occur during cyclic loading. The annealing effect of the next welding heat input on the previous weld should also be considered. The material model of isotropic work hardening and annealing temperature  1000 ℃ should be used to describe this phenomenon. Since welding is a short heating process and the residence time at high temperature is very short, the influence of phase transformation and creep is ignored here, so the total strain formula is
ε e — elastic strain;
ε p – plastic strain;
ε th – thermal strain.
In addition, because the thickness of the workpiece is thin, the overall stiffness is small, and the number of weld passes is small, so the calculation process not only considers the material nonlinearity in the welding heating process, but also considers the geometric nonlinearity of the model, so it involves the theoretical calculation of large deformation. Set the boundary conditions in the model as shown in Figure 2 to limit the rigid body displacement.
Calculation results and discussion
During the welding process, the model experienced two thermal cycles. The comparison between the peak distribution nephogram and the test results of the welded joint is shown in Figure 3. The gray area in the right simulation diagram is the melting pool area higher than the solid phase temperature of the base metal. Assuming that 1400 ℃ is melted, the script program written by Python is used to extract the peak temperature of each node and then write it into the calculation result file. The left side is the actual welded joint, where the dotted black line is the fusion line. It can be seen that the distribution of weld pool and heat affected zone calculated by the finite element method is basically consistent with the experimental value, which shows that the actual welding temperature field can be obtained by the finite element simulation method. Figure 4 shows the thermal cycle curve of points a, B, C and D in Figure 3 after two heating processes. It can be seen that the maximum temperature is about 1750 ℃, and the interlayer temperature of the two passes of welding is lower than 100 ℃.
Fig. 3 Comparison of peak distribution cloud chart and test results at welded joint
Figure 4 Welding thermal cycle curve
Stress deformation field
According to the path shown in Figure 5, the corresponding data is extracted from the finite element simulation results and drawn into Figure 6. Among them, FIG. 6 (a) to Fig. 6 (d) are the axial residual stress and circumferential residual stress of the inner wall and outer wall of the steel pipe at different angles. It is obvious from Fig. 6 (b) and Fig. 6 (d) that the distribution of axial residual stress is not sensitive to the change of different angle positions, no matter the inner wall or the outer wall of the tube. However, in the inner wall, the peak value of the stress in the initial position and the adjacent area (0 ° position) is higher than that in other positions, while in the center of the outer wall weld, the stress in the 90 ° position is lower than that in other angles. In general, these differences can be ignored.
Figure 5 Residual stress extraction path
Fig. 6 Residual stress distribution at different positions
However, for the circumferential residual stress, the distribution and peak value of the residual stress in the inner and outer wall of the steel tube are significantly affected by the change of the angle position. Comparing Fig. 6 (a) and Fig. 6 (c), it can be seen that the peak value of the stress at the 270 ° position in the inner wall is about 100 MPa higher than that at other angular positions, while the peak value changes at the other three angular positions are not so obvious. However, it can still be seen that with the increase of the angle of the inner wall of the tube, the peak value of the circumferential residual stress is also larger, and the range in the high stress area is gradually widened, but the peak value of the stress appears in the fusion line and the nearby heat affected zone. This is because in the process of welding, when the heat source moves continuously, the heat is transmitted in the workpiece, making the temperature of the first welding position slightly lower. At the end of welding, because the heat conduction effect has raised the temperature of the unwelded area to a higher temperature, when the heat source moves to these areas, the temperature will rise higher, so the stress at the beginning and end of the cooling position Values will show a corresponding difference. Compared with the research of Deng et al. , it is found that the larger the pipe diameter is, the smaller the difference of different angles will be. However, in the outer wall of the steel tube, the peak value of the circumferential residual stress is small, which does not exceed the yield strength of the material, so there is not much discussion here, but it can be seen from the figure that the change of angle has a certain impact on its distribution.
Compare the contour map of the workpiece before and after deformation (as shown in Figure 7), in which the red contour line represents the shape before deformation, and the entity map is the cloud map after deformation after 5 times magnification. It can be clearly seen from Figure 7 that the whole workpiece has shrinkage deformation along the z-axis direction and the circumferential direction near the weld. Establish path 1 and path 2 as shown in Figure 8, extract the axial displacement of each node along the two paths in the calculation results, and then add the absolute values and take the average value, and the average axial shrinkage is 0.735 mm; establish path 3, extract the radial displacement, and take the average value to get the radial shrinkage of 0.171 mm.
Figure 7 Contour map of comparison before and after welding deformation
Figure 8 Welding deformation extraction path
- (1) The results of the finite element simulation are consistent with the experimental results, which proves the validity of the method.
- (2) The peak and distribution of the axial residual stress of the austenitic stainless steel pipe calculated by this test method are basically the same at different angles, and the distribution of the axial residual stress of the outer wall and the inner wall is opposite. The axial residual stress of the inner wall weld and its adjacent area presents high tensile stress, while that of the outer wall presents high compressive stress, while that of the inner wall presents high circumferential residual stress The higher the stress value, the smaller the circumferential residual stress value of the outer wall, and are very sensitive to the change of the angle, which shows that the terminal effect is very obvious when the stainless steel pipe is welded.
- (3) It can be concluded from the calculation that the axial and radial shrinkage deformation will occur after the stainless steel pipe is welded, in which the average axial shrinkage is 0.735 mm and the average radial shrinkage is 0.171 mm.
Source: Network Arrangement – China Stainless Steel Pipe Manufacturer – Yaang Pipe Industry Co., Limited (www.steeljrv.com)
(Yaang Pipe Industry is a leading manufacturer and supplier of nickel alloy and stainless steel products, including Super Duplex Stainless Steel Flanges, Stainless Steel Flanges, Stainless Steel Pipe Fittings, Stainless Steel Pipe. Yaang products are widely used in Shipbuilding, Nuclear power, Marine engineering, Petroleum, Chemical, Mining, Sewage treatment, Natural gas and Pressure vessels and other industries.)
If you want to have more information about the article or you want to share your opinion with us, contact us at firstname.lastname@example.org
Please notice that you might be interested in the other technical articles we’ve published:
- What is a steel pipe
- Research Progress on corrosion characteristics of CO2 marine storage system pipeline
-  Zhang Lan. Research status and progress of stainless steel welding process in China [J]. Shanxi metallurgy, 2007 (2): 1-5
-  UEDA Y.Welding Deformation and Residual Sstress Prevention[M].Oxford: Elsevier LTD, 2012.
-  MA C, PENG Q, MEI J, et al.Microstructure and corrosion behavior of the heat affected zone of a stainless steel 308L-316L weld joint[J].Journal of Materials Science & Technology, 2018, 34（10）: 1823-1834.
-  Sun Jiamin. Numerical simulation of temperature field, residual stress and welding deformation of electroslag welded joint of steel structure box column [D]. Chongqing: Chongqing University, 2015
-  Hou Zhiwei, Li qianyun. Analysis of the influence of welding process on welding deformation of stainless steel [J]. Internal combustion engine and accessories, 2018 (22): 86-87
-  ZHOU G, LIU X, YAN D, et al.Prediction for welding deformation reducing by welding sequence optimization of upper plate[J].Transactions of the China Welding Institution, 2009, 30（9）: 109-112.
-  Zhou Jun, Deng De’an, Feng Ke, et al. Numerical simulation of welding deformation of single bead welding of low carbon steel sheet [J]. Journal of welding, 2013, 34 (12): 101-104
-  Deng De’an, kiyoshima S. effect of annealing temperature on the calculation accuracy of welding residual stress of SUS304 stainless steel [J]. Acta metalica Sinica, 2014, 50 (5): 626-632
-  DENG D, MURAKAWA H, LIANG W.Numerical and experimental investigations on welding residual stress in multi-pass butt-welded austenitic stainless steel pipe[J].Computational Materials Science, 2008, 42（2）: 234-244.
-  PENG Jingliang1, CHEN Danfa1, LI Pei1, HU Xing2 Numerical Simulation of Residual Stress and Deformation in Butt Weld of SUS304 Stainless Steel Pipe DOI: 10.19291/j.cnki.1001-3938.2019.2.007