Surface strengthening crack propagation overload numerical simulation method based on node release method

Abstract

The invention provides a surface strengthening crack propagation overload numerical simulation method based on a node release method, and relates to the technical field of aeronautical materials. The method comprises the following steps: simulating crack propagation and prefabricating residual stress based on a node release method, and establishing a finite element model with specified load and material attributes; wherein the residual stress is obtained by stripping the surface layer by layer by adopting an electrolytic polishing method, detecting numerical values of the residual stress in different depth directions by adopting an X-ray diffraction method, fitting the residual stress in different depth directions into a polynomial by utilizing Python, writing a residual stress user subprogram by adopting a sinini program, adjusting and modifying an inp file, and importing the sinini subprogram; and finally, performing post-processing by using a Python script to obtain the crack propagation length and the propagation life, and finally calculating the relationship between the stress intensity factor and the crack length. According to the method, resources and cost required by a traditional experiment are reduced, and meanwhile a new way is provided for analog simulation of the aeronautical material surface strengthening technology.

Description

Technical Field

[0001] The invention relates to the technical field of aviation materials, and in particular to a surface strengthening crack propagation overload numerical simulation method based on a node release method. Background Art

[0002] Key components such as aircraft wings and aircraft engines are often subjected to reciprocating vibration loads during long-term work, and the fatigue crack growth behavior of aviation materials has an important impact on the safety of the workpiece. In order to improve the fatigue life of aviation materials and reduce the crack growth rate, the surface of aviation materials will be strengthened, including ultrasonic rolling, ultrasonic impact, and laser impact. These strengthening methods mainly introduce large residual compressive stresses on the surface of the sample to reduce the crack growth rate, thereby improving fatigue life. However, with the change of strengthening process parameters, the number of experiments required increases, and the time and funds spent also gradually increase. Therefore, if experimental research and numerical simulation can be combined to analyze the crack growth behavior of surface strengthening under overload conditions, it will greatly promote the development of surface strengthening of aviation materials.

[0003] With the development of ABAQUS finite element simulation technology, it has been widely used in the field of crack propagation. However, the crack propagation of traditional metal materials often uses the extended finite element method XFEM, but the XFEM-based crack is sometimes inconsistent with the actual crack direction, and it is impossible to observe the crack propagation rate under various parameter conditions when the crack direction is specified. Summary of the invention

[0004] The technical problem to be solved by the present invention is to provide a surface strengthening crack propagation overload numerical simulation method based on the node release method in view of the deficiencies of the above-mentioned prior art. Based on the node release theory, the crack propagation direction is specified, and prefabricated residual stress is applied on the surface of the specimen to simulate the surface strengthening process, thereby realizing the simulation of the surface strengthening crack propagation behavior of aviation materials, laying the foundation for subsequent fatigue life prediction and damage tolerance design.

[0005] In order to solve the above technical problems, the technical solution adopted by the present invention is: a surface enhanced crack extension overload numerical simulation method based on the node release method, based on the node release method to simulate crack extension and prefabricate residual stress, and establish a finite element model with specified load and material properties; the residual stress is obtained by electrolytic polishing to peel off the surface layer by layer, and the residual stress values ​​in different depth directions are detected by x-ray diffraction, and then the residual stress in different depth directions is fitted into a polynomial using Python, and the residual stress user subroutine is written using the sigini program, the inp file is adjusted and modified, and the sigini subroutine is imported; finally, the Python script is used for post-processing to obtain the crack extension length and extension life, and finally the relationship between the stress intensity factor and the crack length is calculated. Specifically including the following steps:

[0006] Step 1: Perform a crack extension test on the TC4 titanium alloy sample to calculate the stress intensity factor and crack length, and perform a tensile test to obtain material properties; perform an ultrasonic rolling strengthening test on the TC4 titanium alloy sample to measure the residual compressive stress values ​​under different depth conditions;

[0007] Step 1.1: Perform a crack extension experiment on the TC4 titanium alloy specimen, calculate the stress intensity factor and crack length, and perform a tensile test to obtain the material properties of different regions of the TC4 titanium alloy specimen;

[0008] According to GB / T 6398 standard, crack extension test was carried out on TC4 titanium alloy specimens. When the crack length reached the set position, constant load overload test was carried out to calculate the stress intensity factor and crack length. The weld area and the base material area were cut into micro specimens, and their respective stress-strain relationship was measured using a tensile testing machine with an extensometer. The elastic modulus was calculated to obtain the material properties of TC4 titanium alloy specimens.

[0009] Step 1.2: Conduct ultrasonic rolling strengthening experiments on TC4 titanium alloy samples to measure the residual compressive stress values ​​under different depth conditions;

[0010] Ultrasonic rolling strengthening is performed on TC4 titanium alloy samples. The TC4 titanium alloy samples are clamped on the fixture of the ultrasonic rolling device to carry out ultrasonic rolling strengthening experiments. After strengthening, residual compressive stress will be generated on the surface of the sample along the depth direction.

[0011] Then, the TC4 titanium alloy samples after ultrasonic rolling strengthening were electropolished by electropolishing method; and the residual compressive stress values ​​at different depths were measured by X-ray diffractometer;

[0012] Step 2: Use ABAQUS software to build a three-dimensional crack propagation finite element model of the TC4 titanium alloy specimen and perform crack propagation simulation based on node release;

[0013] The crack propagation finite element model of TC4 titanium alloy specimens before and after ultrasonic rolling was constructed, and only half of the model was retained in the vertical direction to improve the calculation accuracy and efficiency. The model was meshed using a two-into-one meshing method. The mesh was refined in the crack propagation area and further encrypted in the overload area. According to the crack surface after meshing, i.e., the XZ plane, M static analysis steps were set according to the number of nodes in any row from the prefabricated crack node to the end node of the overload refinement area along the X direction.

[0014] The node release extension mode is used for single crack extension. A bonding master surface and a bonding slave surface are defined, and the nodes on the bonding master surface are defined as a set. The bonding master surface and the bonding slave surface are bonded together through these nodes. The user sets the debonding conditions so that the bonded nodes are gradually debonded, thereby achieving the purpose of crack extension.

[0015] Step 3: Load setting for crack extension finite element model;

[0016] The crack extension simulation includes three processes, namely normal crack extension, overload application, and restoration of normal crack extension. First, a concentrated force is set in the first analysis step, and the periodic amplitude is set at the central reference point on the upper surface of the crack extension finite element model. The second and subsequent analysis steps sequentially transfer the same load as the first analysis step. When the crack length reaches the set position, an overload test with a constant load is performed, that is, the periodic amplitude with an overload ratio of 2.6 is modified and called in the corresponding analysis step, and then the amplitude is modified in the next analysis step of the corresponding analysis step to restore to normal crack extension, and it is transferred until the end of the crack extension simulation.

[0017] Step 4: Generate a bonding plane for the crack propagation finite element model and set boundary conditions;

[0018] First, call the Python script to create N debonding planes. Each newly generated bonding plane has one less node set along the Z direction than the previous bonding plane. Let the M static analysis steps set in the simulation correspond to the M bonding planes respectively, that is, each analysis step releases a bonding plane in sequence, thereby simulating crack propagation.

[0019] Then, the boundary conditions are set. The analysis step types are all displacement rotation. The corresponding bonding plane is selected for each analysis step, and the displacement in the Y direction is constrained. In addition, the front and back surfaces, bottom surface and side surface of the crack start end of the model are constrained so that these four surfaces are only allowed to move in the Y direction when simulating crack propagation.

[0020] Step 5: Set environmental variables for the crack extension finite element model;

[0021] In the load module of ABAQUS, set a set of predefined fields, starting from Initial; set a set of Sigini residual stress values ​​arbitrarily;

[0022] Step 6: Design the Sigini prefabricated residual stress subroutine to assign residual stress before and after the crack propagation finite element model in ABAQUS simulation;

[0023] First, use Python to perform polynomial fitting on the residual stress values ​​corresponding to different depths obtained in step 1 to obtain the fitted residual stress curve; next, write the fitted residual stress polynomial and the corresponding position information into the sigini subroutine in the Fortran language. This subroutine is used to prefabricate residual stress in the crack propagation model and simulate the ultrasonic rolling strengthening effect;

[0024] In the ABAQUS simulation, residual stress is assigned before and after the crack extension finite element model. Due to different positions, the amplitude of residual stress needs to be readjusted according to the corresponding position, and the corresponding residual stress polynomial is written in Python; modify the INP file and submit the JOB analysis. After the simulation starts, check whether the prefabricated residual stress is correctly introduced into the model. If it is correctly introduced, compressive stress clouds will be displayed at the crack;

[0025] Step 7: After the crack propagation simulation is completed, the crack propagation data of the crack propagation finite element model is read using a Python script program to calculate the relationship between the stress intensity factor and the crack propagation length;

[0026] Design a Python script program to extract and calculate the maximum stress intensity and minimum stress intensity factor at the crack tip during crack propagation from the ODB file of ABAQUS, and calculate the stress intensity factor change amplitude ΔK of each analysis step to analyze the stress change during crack propagation;

[0027] The Python script uses the cumulative sum, material thickness, energy release rate G, and elastic modulus E to calculate the maximum stress intensity factor Kmax and minimum stress intensity factor Kmin at the crack tip; Kmax and Kmin represent the stress intensity factors of the crack tip in different states, and these data are saved in two text files;

[0028] The energy release rate G is related to the stress intensity factor K as follows:

[0029]

[0030] The energy release rate G is calculated based on the finite element crack growth simulation as shown in the following formula:

[0031]

[0032] Where: B is the thickness of TC4 titanium alloy sample, is the reaction force of the nodal force on the crack tip, is the node displacement of the crack extension finite element model in the Y direction, Δa is the unit crack extension length, and N is the number of nodes at the one-dimensional crack tip;

[0033] Afterwards, the Python script calculates the relationship between Kmax and Kmin and obtains the stress intensity factor change amplitude ΔK:

[0034] ΔK=2×|Kmax-Kmin| (3)

[0035] Finally, the text file is imported into Excel, and the relationship between stress intensity factor and crack extension length is calculated according to the requirements of the Paris rate formula.

[0036] The beneficial effect produced by adopting the above technical scheme is that: the present invention provides a surface strengthening crack extension overload numerical simulation method based on the node release method, and adopts the node release technology to simulate the crack extension. On the other hand, there is very little content on the prefabricated residual stress on the surface of the crack extension specimen. The present invention adopts the node release method to simulate the crack extension mode, and adopts the sigini subroutine in the Fortran language to prefabricate residual stress on the specific surface of the specimen, and numerically simulates the crack extension of the metal material. This method research is innovative. At the same time, the present invention also creates a python extraction program to extract the relationship between the calculated stress intensity factor and the crack length in the simulation result file. The present invention not only reduces the resources and costs required for traditional experiments, but also provides a new way for the simulation of the surface strengthening technology of aviation materials. BRIEF DESCRIPTION OF THE DRAWINGS

[0037] Figure 1 A flow chart of a method for numerical simulation of surface strengthening crack propagation overload based on a node release method provided in an embodiment of the present invention;

[0038] Figure 2 A finite element mesh distribution diagram of overload crack extension provided by an embodiment of the present invention;

[0039] Figure 3 A flow chart of creating a debonded plane code provided by an embodiment of the present invention;

[0040] Figure 4 A flowchart of a user subroutine for creating residual stress provided by an embodiment of the present invention;

[0041] Figure 5 A flow chart of extracting crack growth data provided by an embodiment of the present invention;

[0042] Figure 6 Correct introduction of prefabricated residual compressive stress cloud diagram provided by the embodiment of the present invention;

[0043] Figure 7 A stress cloud diagram presented during the prefabrication residual stress simulation process provided by an embodiment of the present invention;

[0044] Figure 8 A stress cloud diagram presented during a simulation of an overload ratio of 2.6 provided in an embodiment of the present invention;

[0045] Fig. 9 A stress cloud diagram presented during the simulation of the prefabrication residual stress + overload ratio 2.6 provided in an embodiment of the present invention;

[0046] Fig.10 A relationship diagram between stress intensity factor and crack extension length provided in an embodiment of the present invention. DETAILED DESCRIPTION

[0047] The specific implementation of the present invention is further described in detail below in conjunction with the accompanying drawings and examples. The following examples are used to illustrate the present invention, but are not intended to limit the scope of the present invention.

[0048] This embodiment takes the TC4 laser welded joint M(t) specimen as an example, and adopts a surface enhancement crack propagation overload numerical simulation method based on a node release method of the present invention to simulate the surface enhancement crack propagation behavior of the specimen.

[0049] In this embodiment, a surface strengthening crack propagation overload numerical simulation method based on the node release method is as follows: Figure 1 As shown, the following steps are included:

[0050] Step 1: Perform a crack extension test on the TC4 laser welded joint M(t) sample to calculate the stress intensity factor and crack length, and perform a tensile test to obtain material properties; perform an ultrasonic rolling strengthening test on the TC4 titanium alloy M(t) sample to measure the residual compressive stress values ​​under different depth conditions;

[0051] Step 1.1: Perform a crack extension experiment on the TC4 laser welded joint M(t) specimen, calculate the stress intensity factor and crack length, and perform a tensile test to obtain the material properties of different regions of the TC4 laser welded joint M(t) specimen;

[0052] According to GB / T 6398 standard, crack extension test was carried out on the M(t) specimen of TC4 laser welded joint. An overload test of 2.6 times constant load (93Mpa) was carried out at the position where the crack length reached 9mm, and the stress ratio was 0.1. Subsequently, the stress intensity factor and crack length were calculated. Next, by cutting the weld area and the base material area into micro specimens respectively, their respective stress-strain relationships were measured using a tensile testing machine with an extensometer, and the elastic modulus was calculated. These stress-strain data were then input into the material properties, and other relevant properties of the material were obtained, as shown in Table 1. (Specific crack extension test and tensile test) The purpose of this step is to obtain test data to provide a basis for subsequent numerical simulation.

[0053] Table 1 Mechanical properties of TC4 laser welded joints

[0054]

[0055] In this embodiment, the crack extension experiment is carried out using a Langjie 100 fatigue testing machine. The test is carried out in an air environment, the temperature is maintained at 25±2°C, and the humidity is between 45% and 55%. A sine wave is used as the test load, a tensile load is used as the load type, the stress cycle ratio is R=0.1, and the loading frequency is 10Hz. Before the test begins, a stress load of 110MPa is used to preform the crack so that it reaches a specified length of about 1.5mm, and then three load reductions are performed to stabilize the initial crack extension rate, and the load is constant after reaching a predetermined load reduction level. This embodiment uses a constant stress of 93MPa for the test. Every certain number of loading cycles, a 50x reading microscope is used to measure the crack length a, and an aN relationship curve between the crack length and the number of loading cycles is drawn. The aN relationship curve is derived to obtain the crack extension rate da / dN. In order to ensure the accuracy and stability of the data, the average value is taken after observing and reading on both sides.

[0056] According to the Paris rate formula, the crack growth rate (FCG) is determined by the crack growth increment (da) per loading cycle (dN). The functional relationship between the crack growth rate and the change amplitude of the stress intensity factor can be expressed as follows:

[0057]

[0058] Among them, C and m are material constants, and △K is the variation range of stress intensity factor.

[0059] The variation range of the stress intensity factor △K of the material under the condition of equal amplitude load is as follows:

[0060]

[0061] Among them, △P=Pmax -P min is the applied load range, B is the crack extension specimen thickness of TC4 laser welded joint M(t) specimen, a is the current crack length, and W is the specimen width of TC4 laser welded joint M(t) specimen.

[0062] Step 1.2: Perform ultrasonic rolling strengthening experiment on TC4 titanium alloy M(t) sample and measure the residual compressive stress value under different depth conditions;

[0063] Ultrasonic rolling strengthening was performed on the TC4 titanium alloy M(t) sample. The TC4 titanium alloy M(t) sample was clamped on the fixture of the ultrasonic rolling device. The ultrasonic rolling strengthening experiment was performed with a static pressure of 500N and an amplitude of 20kHz. The strengthened sample will produce residual compressive stress along the depth direction on the sample surface.

[0064] Then, the TC4 laser welded joint samples after ultrasonic rolling strengthening were electropolished by electropolishing; and the residual compressive stress values ​​under different depth conditions were measured by X-ray diffractometer; in this embodiment, the electropolishing used an electrolyte with a ratio of methanol:perchloric acid of 1:9, a constant current of 5A, and a voltage of about 15V.

[0065] Step 2: Use ABAQUS software to build the crack propagation finite element model of the TC4 laser welded joint M(t) specimen, and perform crack propagation simulation based on node release;

[0066] The crack propagation finite element model of the TC4 laser welded joint was constructed based on the crack propagation test samples before and after ultrasonic rolling, and only half of the model was retained in the vertical direction to improve the calculation accuracy and efficiency. A two-into-one meshing method was used to mesh the model. The mesh is refined in the crack propagation area and further encrypted in the overload area to more accurately observe and measure the stress distribution. When drawing the mesh, the mesh needs to be divided step by step to avoid errors. Usually, it can be divided gradually from top to bottom and from left to right, and regular lines that can run through the entire figure are selected for cutting to ensure that the drawn mesh is standardized. Figure 2 Shown is the finite element mesh distribution of overload crack growth.

[0067] In this embodiment, the size of the crack extension model is 30mm x 240mm x 2mm. In order to ensure that cracks can be generated in a specific area and single cracks can be extended, the node release extension mode is adopted. The node release extension mode is one of the methods of ABAQUS to simulate crack extension. Define a bonding master surface and a bonding slave surface, and define the nodes on the bonding master surface as a set. The bonding master surface and the bonding slave surface are bonded together through these nodes. The user sets the debonding conditions so that the bonded nodes are gradually debonded, thereby achieving the purpose of crack extension. The specific settings are as follows:

[0068] First, the mesh is divided. Due to the symmetry of the problem, only 1 / 4 of the TC4 laser welded joint M(t) specimen is modeled, and ABAQUS is used to perform crack propagation simulation based on node release. Since the sensitivity of the mesh will affect the size and distribution of the crack tip stress, the mesh is refined in the middle of the TC4 laser welded joint M(t) specimen.

[0069] Furthermore, since this simulation test includes full-process crack extension and overload crack extension, two sets of mesh refinement methods are used. Full-process crack extension requires full-process refinement in the central area, and the mesh size is about 0.1mm. Therefore, the full-process crack extension finite element model contains 452,524 elements and 474,337 nodes. For overload crack extension, only the overload area needs to be locally refined, and the minimum mesh size is about 0.015mm. Therefore, the overload crack extension model contains 451,392 elements and 471,195 nodes. Figure 2 It can be seen that according to the cutting characteristics of the specimen, it is necessary to set the degree of freedom of activity in the y direction for the side (i.e., YZ plane) of the crack extension finite element model and the overload crack extension model. For simplicity, this embodiment makes the following assumptions: the crack tip is a straight line perpendicular to the YZ plane of the crack extension finite element model, and in addition, the crack edge is assumed to be a plane that allows the application of symmetry.

[0070] Next, according to the crack surface after meshing, i.e., the XZ plane, the analysis step is set according to the number of nodes in any row from the prefabricated crack node to the end node of the overload refinement area along the X direction. In the simulation of this embodiment, 196 static general analysis steps need to be set. The time length is 0.1 second, and the incremental step size is 0.01, so that ten frames are analyzed in one analysis step. A constraint is set in the interaction module of ABAQUS to couple the upper surface of the crack extension finite element model with the upper surface center reference point, and constrain the translational degrees of freedom in the three directions of U1, U2, and U3.

[0071] Step 3: Load setting for crack extension finite element model;

[0072] In this embodiment, the crack extension simulation includes three processes, namely normal crack extension, overload application, and restoration of normal crack extension. First, a concentrated force is set in the first analysis step Step 1, and a periodic amplitude is set at the central reference point 1 on the upper surface of the crack extension finite element model. The second and subsequent analysis steps sequentially transfer the same load as the first analysis step; when the crack length reaches 9 mm, an overload test of 2.6 times the constant load is performed, that is, in the 98th analysis step Step 98, the periodic amplitude with an overload ratio of 2.6 is modified and called, and then in the 99th analysis step Step 99, the amplitude is modified to restore to normal crack extension, and it is transferred until the end of the crack extension simulation.

[0073] Step 4: Generate a bonding plane for the crack propagation finite element model and set boundary conditions;

[0074] In order to better simulate crack propagation, the node release method analyzes the contact problem of the crack surface by means of the master-slave contact surface, bonds the nodes between the master and slave surfaces together, and achieves the purpose of crack propagation by releasing the bonded nodes. Generally, manually selecting nodes in ABAQUS is time-consuming and laborious and is likely to be wrong, so this embodiment calls a Python script to create a debonding plane. The Python script code program flowchart is as follows Figure 3 shown.

[0075] In this embodiment, after the Python script is created, 196 bonding plane tests will be generated, and each newly generated bonding plane test has one less node set along the Z direction than the previous bonding plane. Let the 196 static analysis steps set in the simulation correspond to the 196 bonding planes respectively, that is, each analysis step releases a bonding plane in sequence to simulate crack propagation.

[0076] Then set the boundary conditions, the analysis step type is displacement rotation, each analysis step selects the corresponding bonding plane test, and constrains the displacement in the Y direction. In addition, the front and back surfaces, bottom surface and side surface of the crack start end of the model need to be constrained so that these four surfaces are only allowed to move in the Y direction when simulating crack propagation.

[0077] Step 5: Set environmental variables for the crack extension finite element model;

[0078] In the load module of ABAQUS, a set of predefined fields need to be set, starting with Initial. In this step, a set of Sigini residual stress values ​​can be set at will; then, when running the Job, the INP file needs to be modified to import the prefabricated residual stress subroutine written in Fortran for calculation. After the simulation run is completed, the Python script file needs to be executed to extract the crack length and fatigue life parameters in the ODB file.

[0079] Step 6: Design the Sigini prefabricated residual stress subroutine to assign residual stress before and after the crack propagation finite element model in ABAQUS simulation;

[0080] First, use Python to perform polynomial fitting on the residual stress values ​​corresponding to different depths obtained in step 1 to obtain the fitted residual stress curve; next, write the fitted residual stress polynomial and the corresponding position information into the sigini subroutine in the Fortran language. This subroutine is used to prefabricate residual stress in the crack propagation model and simulate the ultrasonic rolling strengthening effect;

[0081] In the ABAQUS simulation, residual stress is assigned before and after the crack extension finite element model. Due to the different positions, the amplitude of the residual stress needs to be readjusted according to the corresponding position, and the corresponding residual stress polynomial is written in Python. The residual stress user subroutine flow chart is as follows Figure 4 Modify the INP file and submit the JOB analysis. After the simulation starts, check whether the prefabrication residual stress is correctly introduced into the model. If it is correctly introduced, compressive stress clouds will be displayed at the crack, such as Figure 6 shown.

[0082] Step 7: After the crack propagation simulation is completed, the crack propagation data of the crack propagation finite element model is read using a Python script program.

[0083] In this embodiment, the Python script for extracting crack extension data is as follows: Figure 5 As shown in the figure, in this script, the ODB file of the simulation results is first read, and the steps to be read are specified. Considering that the overload simulation includes three different processes: normal crack growth, overload crack growth, and then normal crack growth again. In the overload simulation, the crack growth data of each frame under these three steps needs to be extracted separately.

[0084] In this embodiment, the purpose of the Python script program is to extract and calculate the maximum and minimum stress intensity factors (Kmax and Kmin) at the crack tip during crack propagation from the ODB file of ABAQUS, and calculate the stress intensity factor change amplitude ΔK for each analysis step to analyze the stress change during crack propagation.

[0085] Running the Python script first opens the specified ODB file, which contains detailed result data for each step in the simulation. Next, the Python script sets some basic parameters, such as the step range and data file path. It loops through each step and extracts reaction force and displacement data from a specific set of nodes. In the simulation, crack growth occurs step by step by releasing nodes, so the reaction force and displacement will change as the crack grows. The Python script extracts this data from different frames for each step and calculates the sum of the products of the reaction force component in the Y direction and the displacement in the Y direction. This sum of products is used to calculate the stress intensity factor.

[0086] The Python script uses the cumulative sum, material thickness, energy release rate G, and elastic modulus E to calculate the maximum and minimum stress intensity factors Kmax and Kmin at the crack tip. Kmax and Kmin represent the stress intensity factors at the crack tip in different states, and these data are saved in two text files.

[0087] The energy release rate G is related to the stress intensity factor K as shown in the following formula:

[0088]

[0089] The energy release rate G is approximately calculated based on finite element crack growth simulation as shown in the following formula:

[0090]

[0091] Where: B is the thickness of the TC4 laser welded joint M(t) specimen, is the reaction force of the nodal force on the crack tip, is the node displacement of the crack extension finite element model in the Y direction, Δa is the unit crack extension length, and N is the number of nodes at the one-dimensional crack tip;

[0092] Both Kmax and Kmin can be calculated using Formula 2 for calculating the stress intensity factor K. In this embodiment, Kmax and Kmin are respectively extracted and calculated from the third frame and the eighth frame of each analysis step.

[0093] Afterwards, the Python script calculates the relationship between Kmax and Kmin, and further obtains the stress intensity factor change amplitude ΔK:

[0094] ΔK=2×|Kmax-Kmin| (5)

[0095] Finally, the text file is imported into Excel, and the relationship between stress intensity factor and crack extension length is calculated according to the requirements of the Paris rate formula.

[0096] In this embodiment, the stress cloud diagram during the simulation process is further processed. The stress cloud diagrams presented during the simulation process of the crack extension model of the prefabricated residual stress, the crack extension model with only an overload ratio of 2.6, and the crack extension model of the prefabricated residual stress + overload ratio of 2.6 are respectively as follows: Figure 7 , Figure 8 and Fig. 9 As shown. Among them, the residual compressive stress can be clearly observed at the overload position in the simulation of overload ratio 2.6 and prefabricated residual stress + overload ratio 2.6. In addition, the crack extension model of prefabricated residual stress, the crack extension model with only overload ratio 2.6, and the crack extension model of prefabricated residual stress + overload ratio 2.6 are respectively represented by usrp, 2.6ol and 2.6ol+usrp. The curves of the stress intensity factor and crack extension length simulation results are shown in Fig.10 shown.

[0097] Finally, it should be noted that the above embodiments are only used to illustrate the technical solutions of the present invention, rather than to limit it. Although the present invention has been described in detail with reference to the aforementioned embodiments, those skilled in the art should understand that they can still modify the technical solutions described in the aforementioned embodiments, or make equivalent replacements for some or all of the technical features therein. However, these modifications or replacements do not cause the essence of the corresponding technical solutions to deviate from the scope defined by the claims of the present invention.

Claims

1. A method for numerical simulation of surface strengthening crack propagation overload based on node release method, characterized in that: Based on the node release method, crack propagation is simulated and residual stress is prefabricated, and a finite element model with specified loads and material properties is established; the residual stress is obtained by electrolytic polishing to peel off the surface layer by layer, and the X-ray diffraction method is used to detect the values ​​of residual stress in different depth directions, and then the residual stress in different depth directions is fitted into a polynomial using Python, and the sigini program is used to write a residual stress user subroutine, the inp file is adjusted and modified, and the sigini subroutine is imported; finally, the Python script is used for post-processing to obtain the crack extension length and extension life, and finally the relationship between the stress intensity factor and the crack length is calculated.

2. The surface strengthening crack propagation overload numerical simulation method based on the node release method according to claim 1 is characterized in that: The following steps are involved: Step 1: Perform a crack extension test on the TC4 titanium alloy sample to calculate the stress intensity factor and crack length, and perform a tensile test to obtain material properties; perform an ultrasonic rolling strengthening test on the TC4 titanium alloy sample to measure the residual compressive stress values ​​under different depth conditions; Step 2: Use ABAQUS software to build a three-dimensional crack propagation finite element model of the TC4 titanium alloy specimen and perform crack propagation simulation based on node release; Step 3: Load setting for crack extension finite element model; Step 4: Generate a bonding plane for the crack propagation finite element model and set boundary conditions; Step 5: Set environmental variables for the crack extension finite element model; In the load module of ABAQUS, set a set of predefined fields, starting from Initial; set a set of Sigini residual stress values ​​arbitrarily; Step 6: Design the Sigini prefabricated residual stress subroutine to assign residual stress before and after the crack propagation finite element model in ABAQUS simulation; Step 7: After the crack propagation simulation is completed, the Python script program is used to read the crack propagation data of the crack propagation finite element model and calculate the relationship between the stress intensity factor and the crack propagation length.

3. The surface strengthening crack propagation overload numerical simulation method based on the node release method according to claim 2 is characterized in that: The specific method of step 1 is: Step 1.1: Perform a crack extension experiment on the TC4 titanium alloy specimen, calculate the stress intensity factor and crack length, and perform a tensile test to obtain the material properties of different regions of the TC4 titanium alloy specimen; According to GB / T 6398 standard, crack extension test was carried out on TC4 titanium alloy specimens. When the crack length reached the set position, constant load overload test was carried out to calculate the stress intensity factor and crack length. The weld area and the base material area were cut into micro specimens, and their respective stress-strain relationship was measured using a tensile testing machine with an extensometer. The elastic modulus was calculated to obtain the material properties of TC4 titanium alloy specimens. Step 1.2: Conduct ultrasonic rolling strengthening experiments on TC4 titanium alloy samples to measure the residual compressive stress values ​​under different depth conditions; Ultrasonic rolling strengthening is performed on TC4 titanium alloy samples. The TC4 titanium alloy samples are clamped on the fixture of the ultrasonic rolling device to carry out ultrasonic rolling strengthening experiments. After strengthening, residual compressive stress will be generated on the surface of the sample along the depth direction. Then, the TC4 titanium alloy samples were electropolished after ultrasonic rolling strengthening by electropolishing method; and the residual compressive stress values ​​under different depth conditions were measured by X-ray diffractometer.

4. The surface strengthening crack propagation overload numerical simulation method based on the node release method according to claim 3 is characterized in that: The specific method of step 2 is: The crack propagation finite element model of TC4 titanium alloy specimens before and after ultrasonic rolling was constructed, and only half of the model was retained in the vertical direction to improve the calculation accuracy and efficiency. The model was meshed using a two-into-one meshing method. The mesh was refined in the crack propagation area and further encrypted in the overload area. According to the crack surface after meshing, i.e., the XZ plane, M static analysis steps were set according to the number of nodes in any row from the prefabricated crack node to the end node of the overload refinement area along the X direction. The node release extension mode is used for single crack extension. A bonding master surface and a bonding slave surface are defined, and the nodes on the bonding master surface are defined as a set. The bonding master surface and the bonding slave surface are bonded together through these nodes. The user sets the debonding conditions so that the bonded nodes are gradually debonded, thereby achieving the purpose of crack extension.

5. The surface strengthening crack propagation overload numerical simulation method based on the node release method according to claim 4 is characterized in that: The specific method of step 3 is: The crack propagation simulation includes three processes, namely normal crack propagation, overload application, and restoration of normal crack propagation. First, a concentrated force is set in the first analysis step, and the periodic amplitude is set at the central reference point on the upper surface of the crack propagation finite element model. The second and subsequent analysis steps sequentially transfer the same load as the first analysis step. When the crack length reaches the set position, an overload test with a constant load is performed, that is, the periodic amplitude with an overload ratio of 2.6 is modified and called in the corresponding analysis step, and then the amplitude is modified in the next analysis step of the corresponding analysis step to restore it to normal crack propagation, and it is transferred until the end of the crack propagation simulation.

6. The surface strengthening crack propagation overload numerical simulation method based on the node release method according to claim 5 is characterized in that: The specific method of step 4 is: First, call the Python script to create N debonding planes. Each newly generated bonding plane has one less node set along the Z direction than the previous bonding plane. Let the M static analysis steps set in the simulation correspond to the M bonding planes respectively, that is, each analysis step releases a bonding plane in sequence, thereby simulating crack propagation. Then set the boundary conditions. The analysis step types are all displacement rotations. For each analysis step, the corresponding bonding plane is selected and the displacement in the Y direction is constrained. In addition, the front and back surfaces, bottom surface and side surface of the crack starting point of the model are constrained so that these four surfaces are only allowed to move in the Y direction when simulating crack propagation.

7. The surface strengthening crack propagation overload numerical simulation method based on the node release method according to claim 6 is characterized in that: The specific method of step 6 is: First, use Python to perform polynomial fitting on the residual stress values ​​corresponding to different depths obtained in step 1 to obtain the fitted residual stress curve; next, write the fitted residual stress polynomial and the corresponding position information into the sigini subroutine in the Fortran language. This subroutine is used to prefabricate residual stress in the crack propagation model and simulate the ultrasonic rolling strengthening effect; In the ABAQUS simulation, residual stress is assigned before and after the crack extension finite element model. Due to the different positions, the amplitude of the residual stress needs to be readjusted according to the corresponding position, and the corresponding residual stress polynomial is written in Python; the INP file is modified and submitted for JOB analysis. After the simulation starts, check whether the prefabricated residual stress is correctly introduced into the model. Correct introduction will display compressive stress clouds at the crack.

8. The surface strengthening crack propagation overload numerical simulation method based on the node release method according to claim 7 is characterized in that: The specific method of step 7 is: Design a Python script program to extract and calculate the maximum stress intensity and minimum stress intensity factor at the crack tip during crack propagation from the ODB file of ABAQUS, and calculate the stress intensity factor change amplitude ΔK of each analysis step to analyze the stress change during crack propagation; The Python script uses the cumulative sum, material thickness, energy release rate G, and elastic modulus E to calculate the maximum stress intensity factor Kmax and minimum stress intensity factor Kmin at the crack tip; Kmax and Kmin represent the stress intensity factors of the crack tip in different states, and these data are saved in two text files; Afterwards, the Python script calculates the relationship between Kmax and Kmin and obtains the stress intensity factor change amplitude ΔK: ΔK=2×|Kmax-Kmin| Finally, the text file is imported into Excel, and the relationship between stress intensity factor and crack extension length is calculated according to the Paris rate formula.

9. The surface strengthening crack propagation overload numerical simulation method based on the node release method according to claim 8 is characterized in that: The energy release rate G is related to the stress intensity factor K as follows: The energy release rate G is calculated based on the finite element crack growth simulation as shown in the following formula: Where: B is the thickness of TC4 titanium alloy sample, is the reaction force of the nodal force on the crack tip, is the nodal displacement of the crack extension finite element model in the Y direction, Δa is the unit crack extension length, and N is the number of nodes at the one-dimensional crack tip.

Images