A numerical simulation-based flash forming prediction method for rotary friction welding

Abstract

The application discloses a kind of based on numerical simulation's rotary friction welding flash forming prediction method, belong to the field of welding numerical simulation, solve the problem that titanium alloy rotary friction welding numerical simulation flash forming prediction is not accurate.Based on titanium alloy continuous drive friction welding numerical simulation, first, establish finite element geometric model, then set material attribute parameter, carry out the friction heat production and interaction setting between contact surface, and set load, boundary condition, apply predefined temperature field, mesh division, finally, simulation calculation and post-processing analysis are carried out.The application considers the transition of interface friction behavior in the process of friction welding, makes the interface friction heat production model more accurate, so as to ensure the accuracy of titanium alloy flash forming prediction after welding, and has important value and significance for the research of titanium alloy continuous drive friction welding flash forming.

Description

Technical Field

[0001] This invention belongs to the field of welding numerical simulation technology. It describes the welding forming process, mechanism and evolution law of the surrounding physical field of high-performance titanium alloy for oil drill pipe. It is mainly used for predicting the flash formation of rotary friction welding. Background Technology

[0002] Rotary friction welding (RFW) is widely used in connecting oil drill pipes and joints due to its advantages such as a welding process interface temperature below the melting point, high welding efficiency, reliable joint quality, good process repeatability, energy saving, and environmental protection. Drilling and production pipes operate in complex environments with high temperature, high pressure, high corrosion, and dynamic loads. Titanium alloys, with their low density, high strength, corrosion resistance, and fatigue resistance, are ideal materials for drilling and production pipes. However, in actual production, the difficulty in removing the burrs on the inner wall of the friction welded drill pipe and threaded joint leads to increased forming costs. If the burrs on the inner wall of the friction welded oil drill pipe and threaded joint can be controlled, forming costs will be reduced and production efficiency will be improved. To achieve burr control, the formation of burrs must first be predictable before further control can be implemented. Therefore, predicting the formation of burrs in rotary friction welding is necessary.

[0003] The rotary friction welding process is generally divided into the following steps: Figure 1The basic processes illustrated are as follows: During welding, the rotating workpiece begins to rotate at high speed under the drive of a motor, while the moving workpiece gradually approaches the rotating workpiece under axial force. When the two workpieces contact and press together, some micro-protrusions on the friction interface first undergo adhesion and shearing, generating frictional heat. As the actual contact area increases, the frictional torque rises rapidly, and the temperature at the friction interface also rises accordingly. The friction interface is gradually covered by a layer of high-temperature viscoplastic metal. At this point, the relative movement of the two workpieces actually occurs within this viscoplastic metal layer, and the heat generation mechanism has changed from initial frictional heat generation to plastic deformation heat generation within the viscoplastic metal layer. As the frictional heat is conducted to the two workpieces, the temperature on both sides of the welding surface gradually increases. Under axial pressure, the metal in the weld nugget area undergoes radial plastic flow and is squeezed out, thus forming flash, and the axial shortening gradually increases. As the friction time extends, the friction interface temperature and frictional torque remain basically constant, the high-temperature zone gradually widens, and the flash gradually increases. When the deformation of the weld area reaches a certain level, the rotational speed of the rotating workpiece is already very low (inertial friction welding) or begins to brake (continuous drive friction welding). Then, an upsetting force is applied. During the holding pressure process after upsetting, the metals in the weld zone diffuse and recrystallize together, firmly welding the two metals together to complete the welding process. Throughout the welding process, the temperature at the friction interface generally does not exceed the melting point; therefore, friction welding is a solid-state welding process. Research on flash formation in rotary friction welding of titanium alloys is costly and difficult to conduct experiments. Numerical simulation, as an important tool for studying the rotary friction welding process, can provide a visual analysis of flash formation during the welding process. Analysis of the current research status both domestically and internationally shows that numerical simulation methods for rotary friction welding of titanium alloys are relatively scarce. The paper by Jin Feng of Northwestern Polytechnical University, "Influence of Ti-6Al-4V Rotary Friction Welded Joint Morphology on Radial Microstructure and Properties (Jin F, Rao H, Wang Q, et al. Heat-pattern induced non-uniform radial microstructure and properties of Ti-6Al-4V joint prepared by rotary friction welding[J]. Materials Characterization, 2023, 195: 112536), establishes a two-dimensional finite element model of continuous-drive friction welding of TC4 bars based on DEFORM. It studies the changes in stress-strain and temperature fields under different flash conditions and characterizes the extrusion behavior by the viscosity of the interfacial ductile metal and the radial extrusion speed, investigating the flash formation mechanism from a thermo-mechanical coupling perspective. The study found that the heat generation of the joint is mainly concentrated at the outer edge, and the width of the heat-affected zone is relatively small; the outer edge of the flash is subjected to axial tensile stress, and the axial tensile stress on the bonded flash is less than that on the separated flash.Furthermore, as the rotational speed increases, the viscosity of the interfacial ductile metal gradually decreases while the radial extrusion speed gradually increases, making it easy to form adhesive flash at low speeds and separation flash at high speeds. Li Wei's paper, "Numerical Simulation of Inertial Friction Welding of TC4 Titanium Alloy" (Li Wei. Numerical Simulation of Welding Process of TC4 Titanium Alloy Inertial Friction Welding [D]. Master's Thesis, Changchun University of Technology, 2018), studies the IFW process of TC4 bars based on ABAQUS. The study points out that the welding interface temperature and axial shortening are important indicators for selecting process parameters. The faster the welding interface temperature enters the steady-state stage and the greater the axial shortening of the weldment, the better the welding quality. The established model is calculated and analyzed to study the influence of different process parameters (moment of inertia, rotational speed, friction pressure) on the axial shortening of the weldment and the change in welding interface temperature. The optimal process parameters are determined, and welding experiments are conducted based on these parameters. The results show that the process parameters obtained from the numerical simulation have a certain guiding role in the welding optimization of inertial friction welding within a certain range. The actual welding results show good welding quality, and the changes basically conform to the welding rules of the numerical simulation. Although there has been some progress in numerical simulation research on titanium alloy rotary friction welding in recent years, the overall research is still not comprehensive enough, especially in the prediction of flash formation. Existing research cannot accurately predict the flash morphology of titanium alloy rotary friction welding. Therefore, it is of great significance to establish a flash formation prediction method based on numerical simulation. Summary of the Invention

[0004] To overcome the shortcomings of existing technologies, this invention proposes a numerical simulation-based method for predicting flash formation. Based on numerical simulation of continuous-drive friction welding of titanium alloys, and considering that the commonly used Johnson-Cook constitutive model cannot accurately reflect the rheological stress of TC4 titanium alloys above 1000℃, a table-based method is used to establish the material's constitutive model. Furthermore, the transformation of interfacial friction behavior during friction welding is fully considered to improve model accuracy. This provides a reference for the study of flash formation in rotary friction welding of titanium alloys.

[0005] The technical solution of this invention is:

[0006] A method for predicting flash formation based on numerical simulation, the specific steps of which are as follows:

[0007] Step 1: Establish a finite element geometric model;

[0008] First, using ABAQUS software, a two-dimensional finite element model of continuous driven friction welding of TC4 pipe titanium alloy is established in the Part module. The geometric model includes three parts: an axisymmetric shell element, a torsionally deformable workpiece, a welded top pipe and a welded bottom pipe, and the central axis of the welded pipe.

[0009] Step 2: Set material property parameters;

[0010] Enter the Property module of the ABAQUS simulation software, set the material property parameters of TC4 titanium alloy, create a homogeneous section of TC4 titanium alloy solid, and assign the cross-sectional properties of the axisymmetric shell element torsionally deformable workpiece geometric model from step 1.

[0011] The material properties include the density, Young's modulus, Poisson's ratio, inelastic thermal coefficient, thermal conductivity, specific heat capacity, and rheological stress of TC4 titanium alloy as a function of temperature. The rheological stress is different from the widely used Johnson-Cook constitutive model. The rheological stress of this invention is given in a table, and the data comes from JmatPro software.

[0012] Step 3: Establish a reference plane;

[0013] Enter the Assembly module of the ABAQUS simulation software, divide the top welded pipe and the bottom welded pipe into the base material area and the near-weld area respectively, and establish a reference plane at the division point;

[0014] Step 4: Set up welding time analysis steps and field output, process output;

[0015] Enter the Step module of the ABAQUS simulation software, establish a temperature-displacement coupled analysis step, and set the welding time; output the displacement of the jacking pipe, the interface temperature field, the stress-strain field and the change in heat flux density, and output the maximum interface temperature and the change in axial shortening during the welding process.

[0016] Step 5: Set the interaction and friction behavior between the contact surfaces;

[0017] In the Interaction module of the ABAQUS simulation software, first set the interaction between the contact surfaces. For the welded top pipe and welded bottom pipe, use the "balanced master-slave" setting, the contact type is face-to-face contact, the sliding method is finite sliding, and the discretization method is point-to-surface. Set self-contact for the welded top pipe and welded bottom pipe respectively, and the discretization method is point-to-surface. Set the welding interface to frictionless, and set the contact between the welding interfaces and between the welded pipe and the flash to soft contact.

[0018] Step 6: Set loads and boundary conditions, and apply a predefined temperature field;

[0019] Enter the Load module of the ABAQUS simulation software, apply uniformly distributed frictional pressure to the upper surface of the top pipe of the weldment, and apply thermal load to the welding interface of the top pipe and the bottom pipe of the weldment respectively. The heat flux density q is calculated by equation (1):

[0020]

[0021] In the formula, η is a coefficient related to the pressure distribution at the welding interface, τ is the shear force at the welding interface, ω is the rotational speed, r is the distance from the center of the circle, and R is the outer diameter of the pipe.

[0022] The welded bottom pipe is completely fixed, and no constraints are applied to the top pipe;

[0023] Since the welding process is very short, the heat generated by friction at the welding interface is much greater than the heat dissipation by convection during the welding time. Therefore, it is assumed that all boundaries are adiabatic.

[0024] The predefined temperature for the deformable workpiece is 20℃;

[0025] Step 7: Set mesh properties;

[0026] In the ABAQUS simulation software, the Mesh module is used to set the mesh size of the deformable workpiece using both overall and edge mesh methods; the default mesh size is used in the base material area, while a finer mesh size is used in the near-seam area.

[0027] Step 8: Simulation calculation and post-processing analysis;

[0028] In the Job module of the ABAQUS simulation software, a custom heat source subroutine is submitted, and then simulation calculations are performed. Mesh distortion is controlled through remeshing technology. The morphology of weld flash, temperature field, stress-strain field, interface temperature change, and axial shortening change are analyzed.

[0029] A further technical solution of the present invention is: the thermal conductivity and specific heat capacity of TC4 titanium alloy as a function of temperature in step 2 are calculated by equations (2) and (3), respectively:

[0030] λ = 0.01003T + 4.15762 × 10 -7 T 2 +6.55509 (2)

[0031] C = 0.2787T - 1.51277 × 10 -4 T 2 +602.60614 (3)

[0032] In equations (2) and (3), λ is the thermal conductivity, C is the specific heat capacity, and T is the temperature.

[0033] A further technical solution of the present invention is: in the expression for heat flux density q in step 6, the shear force at the welding interface changes with the progress of the friction process. When the frictional stress is less than the shear yield stress, the interface mainly generates heat through Coulomb sliding friction, and at this time τ f Equation (4) represents:

[0034] τ f =μP (4)

[0035] In equation (4), μ is the friction coefficient and P is the applied axial pressure.

[0036] When the frictional stress is greater than or equal to the shear yield strength, the entire interface is in an adhesive friction state, and the deformation resistance is equal to and remains constant with the shear yield strength of the metal. According to the Misise yield criterion, τ at this point... y Equation (5) represents:

[0037]

[0038] In the formula σ y The yield stress of the material is expressed using the Arrhenius constitutive model of equation (6):

[0039]

[0040] In equation (6), the Zener-Hollomon factor Z is represented by the following equation (7):

[0041]

[0042] In the formula Q is the strain rate, R is the activation energy of thermal deformation, T is the gas constant, and T is the absolute temperature.

[0043] A further technical solution of the present invention is: in step 7, the control attribute of the mesh is a quadrilateral free progressive algorithm, the element type is selected as implicit CGAX4HT (four-node temperature-displacement coupled axisymmetric quadrilateral element, bilinear displacement and temperature, using hybrid element, hourglass control) and CGAX3T (three-node temperature-displacement coupled axisymmetric triangular element, linear displacement and temperature, hourglass control), and the mesh size near the weld seam is 0.25;

[0044] A further technical solution of the present invention is as follows: the remeshing technique in step 8 is controlled by a Python script, and drastic deformation occurs in the mesh during each mesh redrawing analysis step. ABAQUS / CAE is used to extract the outer surface of the pipe, regenerate the surface, and remesh the pipe region. This process uses the Abaqus Scripting Interface PartFromOdb command, which is used to extract isolated mesh parts representing the deformed pipe. The mesh is then passed to the Part2DGeomFrom2DMesh command to create a geometric model. Once the outline of the geometric model is created, a new mesh can be drawn, which maps from the state variables of the previous analysis.

[0045] Beneficial effects

[0046] The beneficial effects of this invention are as follows: This invention fully considers that welding deformation mainly occurs above 1000℃, therefore, the accuracy and rationality of the rheological stress of TC4 titanium alloy in this temperature range is crucial. Given that the Johnson-Cook constitutive model widely used in existing numerical simulations of TC4 titanium alloys is inadequate in describing the rheological stress at high temperatures, this invention uses a table method to establish the material constitutive model, with data sourced from JmatPro software. Furthermore, this invention fully considers the transformation of interfacial friction behavior during friction welding, making the interfacial friction heat generation model more accurate, thereby ensuring the accuracy of the prediction of flash formation after titanium alloy welding. This has significant value and importance for the study of flash formation in continuous-drive friction welding of titanium alloys.

[0047] This invention provides a numerical simulation-based method for predicting flash formation in rotary friction welding, offering a reference for the study of flash formation mechanism in titanium alloy rotary friction welding, helping to reveal the flash formation law; exploring the scientific validity and reliability of flash control research in rotary friction welding, providing technical support for rotary friction welding of titanium alloys, and better serving the fields of deep oil and gas and combustible ice drilling and production, which is of great significance. Attached Figure Description

[0048] Figure 1 This is a schematic diagram of the rotary friction welding process.

[0049] Figure 2 The following are finite element geometric models of axisymmetric TC4 titanium alloy rotary friction welding in two embodiments of the present invention;

[0050] Figure 3 Here are the material property parameter tables for two embodiments of the present invention;

[0051] Figure 4 The following are the interface maximum temperature curves for two embodiments of the present invention: (a) Embodiment 1; (b) Embodiment 2;

[0052] Figure 5 The following is a comparison of the axial shortening variation curves and calculation results of the weldments in two embodiments of the present invention with the experimental results: (a) axial shortening variation curve of the weldment in Embodiment 1; (b) axial shortening variation curve of the weldment in Embodiment 2; (c) comparison of the axial shortening of the weldments in Embodiments 1 and 2 with the experimental results.

[0053] Figure 6 The temperature field evolution of two embodiments of the present invention is shown below: (a) Temperature field of Embodiment 1 at 0.41 s; (b) Temperature field of Embodiment 1 at 3.6 s; (c) Temperature field of Embodiment 2 at 0.34 s; (d) Temperature field of Embodiment 2 at 3.2 s.

[0054] Figure 7Comparison of post-weld flash forming and post-test flash forming in two embodiments of the present invention: (a) Embodiment 1; (b) Embodiment 2; Detailed Implementation

[0055] The present invention will be described in detail below with reference to specific embodiments.

[0056] In the finite element simulation of flash formation prediction in rotary friction welding, this invention employs a thermo-mechanical coupling numerical simulation method based on re-meshing technology and considering the transformation of interfacial frictional behavior, comprising the following steps:

[0057] Step 1: Establish the finite element geometric model:

[0058] Using the ABAQUS commercial simulation software, a two-dimensional finite element model of continuous-drive friction welding of TC4 pipe titanium alloy was established in the Part module. The geometric model consists of three parts: an axisymmetric shell element torsionally deformable workpiece, a welding top pipe and a welding bottom pipe, and the central axis of the welded pipe. In this geometric model, the welding bottom pipe of the axisymmetric deformable workpiece is completely fixed, while the welding top pipe serves as the free end for welding.

[0059] Step 2: Set material property parameters:

[0060] Step 2 is based on the finite element geometric model of TC4 titanium alloy continuous drive friction welding established in Step 1. Enter the Property module of the ABAQUS simulation software, set the material property parameters of TC4 titanium alloy, create a homogeneous solid section of TC4 titanium alloy, and assign the cross-sectional properties of the axisymmetric shell element torsionally deformable workpiece geometric model from Step 1. The material properties include the density, Young's modulus, Poisson's ratio, inelastic thermal coefficient, and thermal conductivity, specific heat capacity, and flow stress of TC4 titanium alloy as a function of temperature. The flow stress is given in a table format, and the data comes from JmatPro software. The thermal conductivity and specific heat capacity of TC4 titanium alloy as a function of temperature are calculated using equations (1) and (2), respectively.

[0061] λ = 0.01003T + 4.15762 × 10 -7 T 2 +6.55509 (1)

[0062] C = 0.2787T - 1.51277 × 10 -4 T 2 +602.60614 (2)

[0063] In equations (2) and (3), λ is the thermal conductivity, C is the specific heat capacity, and T is the temperature.

[0064] Step 3: Establish the reference plane, load application plane, and welding plane:

[0065] The simulation was performed using the Assembly module of the ABAQUS software. The top and bottom welded pipes were divided into the base material area and the near-weld area, respectively, and a reference surface was established at the division point. The upper surface of the top pipe was selected as the welding pressure application surface. The weld area was selected as the welding surface. The part where the top and bottom pipes of the welded part contacted was selected as the welding heat flow surface.

[0066] Step 4: Set up welding time analysis steps and field output, process output:

[0067] The simulation was performed using the Step module of the ABAQUS software. A temperature-displacement coupled analysis step was established, and the welding time was set. The displacement of the jacking pipe, the changes in the interface temperature field and stress-strain field were output, as well as the changes in the maximum interface temperature and axial shortening during the welding process.

[0068] Step 5: Set up the interaction and friction behavior between the contact surfaces:

[0069] Based on steps 1 to 4, the main simulation is performed in the Interaction module of the ABAQUS simulation software. First, the interaction between the contact surfaces is set. The welding top pipe and welding bottom pipe are set to "balanced master-slave". The contact type is face-to-face contact, the sliding method is finite sliding, and the discretization method is point to surface. Self-contact is set for the welding top pipe and welding bottom pipe respectively, and the discretization method is point to surface. The welding interface is set to frictionless, and the contact between the welding interfaces and between the welding pipe and the flash is set to soft contact.

[0070] Step 6: Set loads and boundary conditions, and apply a predefined temperature field:

[0071] Based on steps 1 to 4, the Load module of the ABAQUS simulation software is set up to apply uniformly distributed frictional pressure to the upper surface of the top pipe of the weldment, and apply thermal load to the welding interface of the top pipe and the bottom pipe of the weldment respectively. The heat flux density q is calculated by equation (3). The bottom pipe is completely fixed and no constraint conditions are applied to the top pipe. Since the welding process is very short, the frictional heat generated at the welding interface is much greater than the convection heat dissipation during the welding time. Therefore, it is assumed that all boundaries are adiabatic. The predefined temperature of the deformable workpiece is 20℃.

[0072]

[0073] In the formula, η is a coefficient related to the pressure distribution at the welding interface, τ is the shear force at the welding interface, ω is the rotational speed, r is the distance from the center of the circle, and R is the outer diameter of the pipe.

[0074] In the expression for heat flux density q, the shear force at the weld interface changes with the friction process. When the frictional stress is less than the shear yield stress, the interface mainly generates heat through Coulomb sliding friction, and at this time τ fEquation (4) represents:

[0075] τ f =μP (4)

[0076] In equation (4), μ is the friction coefficient and P is the applied axial pressure.

[0077] When the frictional stress is greater than or equal to the shear yield strength, the entire interface is in an adhesive friction state, and the deformation resistance is equal to the shear yield strength of the metal and remains unchanged. According to the Misise yield criterion, the interfacial shear force at this time is expressed by equation (5):

[0078]

[0079] In the formula σ y The yield stress of the material is expressed using the Arrhenius constitutive model of equation (6):

[0080]

[0081] In equation (6), the Zener-Hollomon factor Z is represented by the following equation (7):

[0082]

[0083] In the formula Q is the strain rate, R is the activation energy of thermal deformation, T is the gas constant, and T is the absolute temperature.

[0084] Step 7: Set mesh properties:

[0085] The mesh settings were configured in the Mesh module of the ABAQUS simulation software. During rotary friction welding, the weld metal is subjected to the combined effects of frictional heat and axial pressure, resulting in severe deformation. To ensure calculation accuracy, the mesh near the weld zone was refined. The base metal zone was less affected, mainly undergoing heat transfer; therefore, to save computational costs, a larger mesh size was selected for this region. The mesh size of the deformed workpiece was ultimately set using both overall and edge-based meshing methods. The mesh was gradually refined from the base metal zone to the weld zone. The mesh control properties were a quadrilateral free-order algorithm, and the element types selected were implicit CGAX4HT (four-node temperature-displacement coupled axisymmetric quadrilateral element, bilinear displacement and temperature, using hybrid elements, hourglass control) and CGAX3T (three-node temperature-displacement coupled axisymmetric triangular element, linear displacement and temperature, hourglass control). This invention sets the mesh size near the weld zone to 0.25 to ensure the accuracy of the numerical simulation calculation.

[0086] Step 8: Simulation calculation and post-processing analysis;

[0087] The steps involved, based on the correct setup of the previous six steps, involved submitting a custom heat source subroutine in the Job module of the ABAQUS simulation software, followed by simulation calculations. Mesh distortion was controlled using remeshing technology, controlled by a Python script. Severe deformation occurred in the mesh during each mesh redrawing analysis step. ABAQUS / CAE was used to extract the outer surface of the pipe, regenerate the surface, and remesh the pipe region. This process used the Abaqus ScriptingInterface PartFromOdb command to extract isolated mesh parts representing the deformed pipe. The mesh was then passed to the Part2DGeomFrom2DMesh command to create a geometric model. Once the outline of the geometric model was created, a new mesh was drawn, mapping the state variables from the previous analysis. Analysis was performed on the post-weld flash morphology, temperature field, stress-strain field, interface temperature changes, and axial shortening changes. This study explores the scientific validity and reliability of flash formation control in titanium alloy rotary friction welding, providing technical support for titanium alloy rotary friction welding and better serving the fields of deep oil and gas and combustible ice drilling and production.

[0088] Example 1:

[0089] The specific method of this embodiment includes the following steps:

[0090] (1) Steps for establishing a geometric model:

[0091] A torsional deformable workpiece with an axisymmetric shell element was created using the Part module in ABAQUS. The geometric model of the deformable workpiece is rectangular, 30mm long and 5mm wide, with the outer wall of the tube 12.5mm from the axis of symmetry. The deformable workpiece was divided into regions: the base material region was a 20*5mm rectangular geometric model, and the near-seam region was a 10*5mm rectangular geometric model. The finite element model described in this example is attached. Figure 2 .

[0092] (2) Steps for defining the mechanical, thermodynamic, and constitutive parameters of TC4 titanium alloy:

[0093] Material property parameters are defined using the Property module in ABAQUS, a solid homogeneous interface is created, and then assigned to the deformable workpiece. The material property parameters for this example are shown in the appendix. Figure 3 .

[0094] (3) Steps for establishing the reference plane, load application plane, and welding plane:

[0095] The simulation was performed using the Assembly module of the ABAQUS software. The top and bottom welded pipes were divided into the base material area and the near-weld area, respectively, and a reference surface was established at the division point. The upper surface of the top pipe was selected as the welding pressure application surface. The weld area was selected as the welding surface. The part where the top and bottom pipes of the welded part contacted was selected as the welding heat flow surface.

[0096] (4) Set the welding time analysis step and field output, process output:

[0097] The simulation was performed using the Step module in the ABAQUS software. A temperature-displacement coupled analysis step was established, with the welding time set to 3.2s, the maximum number of incremental steps to 10,000, the time increment set to 0.02, the minimum time increment set to 2E-05, the maximum time increment set to 0.02, and the maximum allowable temperature rise per incremental step set to 1000℃. The output showed the displacement of the jacking pipe, the changes in the interface temperature field and stress-strain field, as well as the changes in the maximum interface temperature and axial shortening during the welding process.

[0098] (5) Set the interaction and friction behavior between the contact surfaces:

[0099] The simulation was primarily conducted using the Interaction module of the ABAQUS simulation software. First, the interaction between the contact surfaces was set up. A "balanced master-slave" setting was adopted for both the welded top and bottom pipes, with face-to-face contact as the contact type, finite slip as the slip method, and point-to-surface discretization as the discretization method. Self-contact was set for both the welded top and bottom pipes, with point-to-surface discretization as the discretization method. The tangential behavior of the welding interface was set to frictionless, and the contact between welding interfaces, between the welded pipe and the flash, and the normal behavior of the welding interface were all set to soft contact. When the self-contact pressure was 0, the penetration was -0.01 mm; when the self-contact pressure was 1000 MPa, the penetration was 0. When the normal phase contact pressure was 0, the penetration was 0; when the normal phase contact pressure was 1800 MPa, the penetration was 0.1 mm.

[0100] (6) Set loads and boundary conditions, and apply a predefined temperature field:

[0101] Enter the Load module of the ABAQUS simulation software to set up a uniformly distributed frictional pressure of 55 MPa on the upper surface of the top pipe of the weldment. Apply thermal loads to the welding interfaces of the top pipe and the bottom pipe of the weldment respectively. The heat flux density q is calculated by equation (3). The bottom pipe is completely fixed and no constraint conditions are applied to the top pipe. Since the welding process is very short, the frictional heat generated at the welding interface is much greater than the convective heat dissipation during the welding time. Therefore, it is assumed that all boundaries are adiabatic. The predefined temperature of the deformable workpiece is 20℃.

[0102]

[0103] In the formula, η is the coefficient related to the pressure distribution at the welding interface, which is taken as 0.7; τ is the shear force at the welding interface; ω is the rotation speed, which is taken as 1500 rpm; r is the distance from the center of the circle; and R is the outer diameter of the pipe, which is taken as 25 mm.

[0104] In the expression for heat flux density q, the shear force at the weld interface changes with the friction process. When the frictional stress is less than the shear yield stress, the interface mainly generates heat through Coulomb sliding friction, and at this time τ f Equation (4) represents:

[0105] τ f =μP (4)

[0106] In equation (4), μ is the friction coefficient, which is taken as 0.577, and P is the applied axial pressure, which is taken as 55 MPa.

[0107] When the frictional stress is greater than or equal to the shear yield strength, the entire interface is in an adhesive friction state, and the deformation resistance is equal to the shear yield strength of the metal and remains unchanged. According to the Misise yield criterion, the interfacial shear force at this time is expressed by equation (5):

[0108]

[0109] In the formula σ y The yield stress of the material is expressed using the Arrhenius constitutive model of equation (6):

[0110]

[0111] In equation (6), the Zener-Hollomon factor Z is represented by the following equation (7):

[0112]

[0113] In the formula Q is the strain rate, R is the activation energy of thermal deformation, T is the gas constant, and T is the absolute temperature.

[0114] (7) Set mesh properties:

[0115] The steps described are set in the Mesh module of the ABAQUS simulation software; the mesh size of the base material area is 2.0, and the mesh size of the near-seam area is set to 0.25, and the entire deformed workpiece is meshed; the control attribute of the mesh is quadrilateral free progressive algorithm, and the element type is selected as implicit CGAX4HT (four-node temperature-displacement coupled axisymmetric quadrilateral element, bilinear displacement and temperature, using hybrid element, hourglass control) and CGAX3T (three-node temperature-displacement coupled axisymmetric triangular element, linear displacement and temperature, hourglass control).

[0116] (8) Calculation and post-processing analysis steps:

[0117] In the Job module of the ABAQUS simulation software, a custom heat source subroutine is submitted, and simulation calculations are performed. Mesh distortion is controlled using remeshing technology. Post-processing analysis involves analyzing the morphology of the weld flash, temperature field, interface temperature changes, and axial shortening. This study explores the evolution of flash formation in titanium alloy rotary friction welding under these process parameters. The post-processing analysis results for this example are attached. Figures 4-7 .

[0118] The results show that, under the process parameters of this embodiment, the welding calculations show that as the friction process proceeds, the process enters a steady state at 0.41s. At the same time, the welding flash is extruded, the weldment begins to shorten, and then the upper and lower flashes grow upward and downward respectively, eventually covering the outer wall of the pipe. The upper and lower flashes are basically symmetrical. The axial shortening after welding is 9.9mm, which is only 1% less than the experimental results. The flash formation is also basically consistent with the experimental results.

[0119] Example 2:

[0120] The specific method of this embodiment includes the following steps:

[0121] (1) Steps for establishing a geometric model:

[0122] Same as step (1) in Example 1.

[0123] (2) Steps for defining the mechanical, thermodynamic, and constitutive parameters of TC4 titanium alloy:

[0124] Same as step (2) in Example 1.

[0125] (3) Steps for establishing the reference plane, load application plane, and welding plane:

[0126] Same as step (3) in Example 1.

[0127] (4) Set the welding time analysis step and field output, process output:

[0128] Enter the Step module of the ABAQUS simulation software to set the welding time to 3.6s. The other settings are the same as step (4) in Example 1.

[0129] (5) Set the interaction and friction behavior between the contact surfaces:

[0130] Same as step (5) in Example 1.

[0131] (6) Set loads and boundary conditions, and apply a predefined temperature field:

[0132] Enter the Load module of the ABAQUS simulation software to set up a uniformly distributed frictional pressure of 65 MPa on the upper surface of the top pipe of the weldment. Apply thermal loads to the welding interfaces of the top pipe and the bottom pipe of the weldment respectively. The heat flux density q is calculated by equation (3). The bottom pipe is completely fixed and no constraint conditions are applied to the top pipe. Since the welding process is very short, the frictional heat generated at the welding interface is much greater than the convective heat dissipation during the welding time. Therefore, it is assumed that all boundaries are adiabatic. The predefined temperature of the deformable workpiece is 20℃.

[0133]

[0134] In the formula, η is the coefficient related to the pressure distribution at the welding interface, which is taken as 0.7; τ is the shear force at the welding interface; ω is the rotation speed, which is taken as 1500 rpm; r is the distance from the center of the circle; and R is the outer diameter of the pipe, which is taken as 25 mm.

[0135] In the expression for heat flux density q, the shear force at the weld interface changes with the friction process. When the frictional stress is less than the shear yield stress, the interface mainly generates heat through Coulomb sliding friction, and at this time τ f Equation (4) represents:

[0136] τ f =μP (4)

[0137] In equation (4), μ is the friction coefficient, taken as 0.577, and P is the applied axial pressure, taken as 65 MPa.

[0138] When the frictional stress is greater than or equal to the shear yield strength, the entire interface is in an adhesive friction state, and the deformation resistance is equal to the shear yield strength of the metal and remains unchanged. According to the Misise yield criterion, the interfacial shear force at this time is expressed by equation (5):

[0139]

[0140] In the formula σ y The yield stress of the material is expressed using the Arrhenius constitutive model of equation (6):

[0141]

[0142] In equation (6), the Zener-Hollomon factor Z is represented by the following equation (7):

[0143]

[0144] In the formula Q is the strain rate, R is the activation energy of thermal deformation, T is the gas constant, and T is the absolute temperature.

[0145] (7) Set mesh properties:

[0146] Same as step 7 in Example 1

[0147] (8) Calculation and post-processing analysis steps:

[0148] Similar to step (8) of Example 1, the post-processing analysis results of this example are shown in the appendix. Figures 4-7 .

[0149] The results show that, compared with Example 1, Example 2 increased the friction pressure to 65 MPa. The temperature change curves of the two examples show that increasing the friction pressure allows the welding process to enter the steady state stage more quickly, but it has no significant effect on the temperature at which the steady state stage is reached. At the same time, the axial shortening of the weldment and the flash formation in Example 2 are within a reasonable range compared with the experiment, which has important guiding significance for the prediction of flash formation in titanium alloy rotary friction welding.

[0150] It should be understood that those skilled in the art can make improvements or modifications based on the above description, and all such improvements and modifications should fall within the protection scope of the appended claims.

Claims

1. A method for predicting flash formation in rotary friction welding based on numerical simulation, characterized in that, The specific steps are as follows: Step 1: Establish a finite element geometric model; First, using the ABAQUS commercial simulation software, a two-dimensional finite element model of continuous driving friction welding of TC4 pipe titanium alloy was established in the Part module. The geometric model includes three parts: axisymmetric shell element torsionally deformable workpiece welding top pipe and welding bottom pipe and the central axis of the welded pipe. Step 2: Set material property parameters; Enter the Property module of the ABAQUS simulation software, set the material property parameters of TC4 titanium alloy, create a homogeneous section of TC4 titanium alloy solid, and assign the cross-sectional properties of the axisymmetric shell element torsionally deformable workpiece geometric model from step 1. The material properties include the density, Young's modulus, Poisson's ratio, inelastic thermal coefficient, thermal conductivity, specific heat capacity, and rheological stress of TC4 titanium alloy as a function of temperature. The rheological stress is presented in tabular form, and the data are from JmatPro software. Step 3: Establish a reference plane; Enter the Assembly module of the ABAQUS simulation software, divide the welded top pipe and welded bottom pipe into the base material area and the near-weld area respectively, and establish a reference plane at the division point; Step 4: Set up welding time analysis steps and field output, process output; Enter the Step module of the ABAQUS simulation software, establish a temperature-displacement coupled analysis step, and set the welding time; output the displacement of the jacking pipe, the interface temperature field, the stress-strain field and the change in heat flux density, and output the maximum interface temperature and the change in axial shortening during the welding process. Step 5: Set the interaction and friction behavior between the contact surfaces; In the Interaction module of the ABAQUS simulation software, first set the interaction between the contact surfaces. Use "balanced master-slave" setting for the welded top pipe and welded bottom pipe, with face-to-face contact as the contact type, finite slip as the sliding method, and point-to-surface as the discretization method. Set self-contact for the welded top pipe and welded bottom pipe respectively, with point-to-surface as the discretization method. Set the welding interface to frictionless, and set the contact between the welding interfaces and between the welded pipe and the flash to soft contact. Step 6: Set loads and boundary conditions, and apply a predefined temperature field; Enter the Load module of the ABAQUS simulation software, apply uniformly distributed frictional pressure to the upper surface of the top pipe of the weldment, and apply thermal load to the welding interface of the top pipe and the bottom pipe of the weldment respectively. The heat flux density q is calculated by equation (1): （1） In the formula, η is a coefficient related to the pressure distribution at the welding interface, τ is the shear force at the welding interface, ω is the rotational speed, r is the distance from the center of the circle, and D is the outer diameter of the pipe. The welded bottom pipe is completely fixed, and no constraints are applied to the top pipe; Since the welding process is very short, the heat generated by friction at the welding interface is much greater than the heat dissipation by convection during the welding time. Therefore, it is assumed that all boundaries are adiabatic. Step 7: Set mesh properties; In the ABAQUS simulation software, the Mesh module is used to divide the mesh using both overall and edge meshing methods, and the mesh size of the deformable workpiece is set. The default mesh size is used in the base material area, while a finer mesh size is used in the near-seam area. Step 8: Simulation calculation and post-processing analysis; In the Job module of the ABAQUS simulation software, a custom heat source subroutine is submitted, and then simulation calculations are performed. Mesh distortion is controlled by remeshing technology. The morphology of flash after welding, temperature field, stress-strain field, interface temperature change and axial shortening change are analyzed.

2. The method for predicting flash formation in rotary friction welding based on numerical simulation according to claim 1, characterized in that: In step 2, the thermal conductivity and specific heat capacity of TC4 titanium alloy as a function of temperature are calculated using equations (2) and (3), respectively: （2） （3） In equations (2) and (3), λ is thermal conductivity, C is specific heat capacity, and T is temperature.

3. The method for predicting flash formation in rotary friction welding based on numerical simulation according to claim 1, characterized in that: In step 6, the expression for the heat flux density q indicates that the shear force at the welding interface changes with the friction process. When the frictional stress is less than the shear yield stress, the interface generates heat through Coulomb sliding friction. Equation (4) represents: （4） In equation (4), μ is the friction coefficient and P is the applied axial pressure; When the frictional stress is greater than or equal to the shear yield strength, the entire interface is in an adhesive friction state, and the deformation resistance is equal to and remains constant with respect to the shear yield strength of the metal. According to the Misise yield criterion, at this point... （5） In the formula The yield stress of the material is expressed using the Arrhenius constitutive model of equation (6): （6） In equation (6), the Zener-Hollomon factor Z is represented by the following equation 4.3.8: （7） In the formula Q is the strain rate, R is the activation energy of thermal deformation, T is the gas constant, and T is the absolute temperature.

4. The method for predicting flash formation in rotary friction welding based on numerical simulation according to claim 1, characterized in that: The predefined temperature of the deformed workpiece in step 6 is 20℃.

5. The method for predicting flash formation in rotary friction welding based on numerical simulation according to claim 1, characterized in that: Step 7 uses a quadrilateral free progression algorithm for mesh control, with cell types CGAX4HT and CGAX3T selected, and the mesh size in the near-seam region being 0.

25.

6. The method for predicting flash formation in rotary friction welding based on numerical simulation according to claim 1, characterized in that: The remeshing technique in step 8 is controlled by a Python script. In each mesh redrawing analysis step, when the mesh undergoes severe deformation, the outer surface of the pipe is extracted using ABAQUS / CAE, the surface is regenerated, and the mesh of the pipe area is redrawn. This process uses the Abaqus Scripting Interface PartFromOdb command, which extracts isolated mesh parts representing deformable pipes; the mesh is then passed to the Part2DGeomFrom2DMesh command to create a geometric model; once the outline of the geometric model is created, a new mesh can be drawn, which maps from the state variables of the previous analysis.

Images