Numerical simulation method and system for continuous laser irradiation of 7075 aluminum alloy under action of external load based on modified Johnson-cook model

Abstract

The invention discloses a numerical simulation method and system for continuous laser irradiation of 7075 aluminum alloy under the action of an external load based on a modified Johnson-cook model. According to the scheme, on the basis of the heat conduction principle and an elastic-plastic model, a heat-force coupling model of the continuous laser irradiation 7075 aluminum alloy is established through a finite element method; through continuous laser irradiation and tensile experiments, the effectiveness of the numerical simulation model of the continuous laser irradiation spaceflight-grade high-strength 7075 aluminum alloy under the action of the external load is verified; the laser energy density, the light spot pattern and the external load are imported into the model by adding vdflux and vuamp programs written by a Fortran language, and a correction factor function is added for regulation and calculation. According to the method, a correction factor function is adjusted in a Fortran program along with working conditions to ensure that stress field distribution, temperature field distribution and plate deformation conditions of the high-strength aluminum alloy under the combined action of laser and an external load are flexibly and accurately simulated.

Description

Technical Field

[0001] This invention belongs to the field of laser damage technology, and in particular relates to a numerical simulation method and system for continuous laser irradiation of 7075 aluminum alloy under external load based on a modified Johnson-Cook model. Background Technology

[0002] 7075 aluminum alloy, as a cold-worked forging alloy, is lightweight, has a compact structure, strong corrosion resistance, and good strength below 150 degrees Celsius. It is widely used in aircraft skin, wing spars, bulkheads, landing gear components, and hydraulic system components. However, aircraft are subjected to loads during flight. Unlike without external loads, under combined loading, the target material may fail and fracture before reaching its melting point. With laser irradiation, the target material temperature rises, and due to the preload, the target material will undergo strain hardening and thermal softening, behaviors that affect its yield strength.

[0003] Currently, there is a wealth of research on the damage effects caused by laser processing and cutting. However, research on the failure behavior of high-strength aluminum alloys under laser irradiation under external loads is relatively limited due to the complex thermo-mechanical coupling field. Material damage under different parameters is mainly obtained through repeated and numerous experiments. This method is not only time-consuming and resource-wasting, but also has many limitations, as experimental conditions under certain specific parameters are difficult to achieve. Summary of the Invention

[0004] The purpose of this invention is to provide a numerical simulation method and system for continuous laser irradiation of 7075 aluminum alloy under external load based on a modified Johnson-Cook model, which improves accuracy and expands the scope of application.

[0005] To achieve the objective of this invention, a numerical simulation method for continuous laser irradiation of 7075 aluminum alloy under external load based on a modified Johnson-Cook model is provided, characterized by comprising the following steps:

[0006] Step 1: Construct a finite element analysis model by defining the geometric model and material parameters, and declaring the loads;

[0007] Step 2: Based on the laser heat source parameters of the finite element analysis model, obtain the laser surface heat source model through a one-dimensional Gaussian function; the laser heat source parameters are attached to the laser surface heat source model by writing a vdflux subroutine.

[0008] Step 3: Set up the Johnson-Cook elastoplastic model based on the finite element analysis model;

[0009] Step 4: Simulate real-world test conditions by setting boundary and initial conditions for the temperature field and the stress field of the Johnson-Cook elastoplastic model and the laser surface heat source model. The boundary conditions for the temperature field are edge adiabatic conditions, the initial conditions for the temperature field are ambient temperature, the boundary conditions for the stress field are fixed constraint conditions and external displacement boundary conditions, and the initial conditions for the stress field are set to no initial displacement and no initial velocity field.

[0010] Step 5: Based on the laser surface heat source model and the Johnson-Cook elastoplastic model, divide the finite element mesh and define the analysis step to obtain the Johnson-Cook elastoplastic numerical simulation model that simulates the thermo-mechanical coupling behavior; the finite element mesh is a mesh that is divided into different regions, from sparse to dense and then back to sparse, and the mesh type is assigned as c3d8r in ABAQUS; the defined analysis step is dynamic explicit and temperature-displacement coupled.

[0011] Step 6: Based on the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior, a tensile model simulating real displacement load is obtained by conducting a real-world experiment of laser irradiation on aluminum alloy under preload, recording displacement-time data, and performing data fitting. The tensile model simulating real displacement load is implemented by writing a vuamp subroutine for the fitting function.

[0012] Step 7: Using a tensile model simulating real-world displacement loads, combined with a Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior, a pre-simulation of laser irradiation of aluminum alloy under preload is performed. The pre-simulated stress-time plot is compared with the stress-time plot of the actual laser-irradiated aluminum alloy under preload. The correction factor of the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior is determined by inversion. Then, real-world experiments of laser irradiation of high-strength 7075 aluminum alloy under various preload sizes are conducted. The stress-time plots of the real experiments are compared with the stress-time plots of the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior to verify the effectiveness of the correction factor of the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior.

[0013] Step 8: Combining the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior with the results of laser irradiation experiments on high-strength 7075 aluminum alloy under various preloads, analyze the changes in the mechanical behavior of the high-strength 7075 aluminum alloy target.

[0014] On the other hand, the present invention also provides a system for implementing the above-mentioned numerical simulation method for continuous laser irradiation of 7075 aluminum alloy under external load based on a modified Johnson-Cook model, comprising the following modules:

[0015] The finite element analysis module is used to establish a geometric model of aerospace-grade high-strength 7075 aluminum alloy irradiated by continuous laser and to perform mesh generation;

[0016] The parameter selection module is used to select different laser energy densities;

[0017] The experimental verification module is used to verify the model by continuously irradiating aerospace-grade high-strength 7075 aluminum alloy with laser, and to compare the stress curves obtained from the experiment and simulation, as well as the experimental damage morphology diagram and the stress curve obtained from the simulation.

[0018] The damage threshold calculation module is used to calculate the damage threshold of the material based on the input parameters.

[0019] The laser irradiation experimental platform module is used to build the experimental environment, control the irradiation time and parameters, and record the temperature change curve over time and the dynamic damage process.

[0020] The finite element analysis module is used to perform numerical simulation of the finite element analysis model of aerospace-grade high-strength 7075 aluminum alloy under continuous laser irradiation, and to extract the temperature field and stress field distribution of the position-sensitive detector, as well as the temperature and stress variation curves of the center point of the position-sensitive detector surface over time.

[0021] The curve comparison module is used to compare the stress-time curves obtained from experiments with those obtained from simulations, and to compare the experimental damage morphology diagrams with those obtained from simulations, in order to determine the effectiveness of the model.

[0022] Compared with the prior art, the significant advancements of this invention are: (1) High-precision simulation: This invention adds a correction factor by modifying the Johnson-Cook plasticity model, which enables better fitting of the stress curve; (2) Experimental verification: This invention verifies the accuracy of the model in actual application by comparing actual laser irradiation experiments with simulation results; (3) Wide applicability: This invention is not only applicable to specific types of aluminum alloys, but can also be extended to other types of aluminum alloys and different laser irradiation conditions; (4) Highly flexible simulation: This invention can flexibly and quickly adjust the correction factor by adding the vdflux subroutine, and also supports flexible adjustment by subsequent developers.

[0023] To more clearly illustrate the functional characteristics and structural parameters of the present invention, further explanation is provided below in conjunction with the accompanying drawings and specific embodiments. Attached Figure Description

[0024] The accompanying drawings, which are included to provide a further understanding of the invention and form part of this application, illustrate exemplary embodiments of the invention and, together with their description, serve to explain the invention and do not constitute an undue limitation thereof. In the drawings:

[0025] Figure 1 This is a flowchart of the steps of the present invention;

[0026] Figure 2 This is a schematic diagram of the damage test conditions for continuous laser irradiation of aerospace-grade high-strength 7075 aluminum alloy according to the present invention.

[0027] Figure 3 This is a schematic diagram of the three-dimensional modeling and mesh generation of aerospace-grade high-strength 7075 aluminum alloy by continuous laser irradiation according to the present invention;

[0028] Figure 4 This is a comparison graph of the pre-simulated stress-time curve and the pre-experimental data after fitting with correction factors;

[0029] Figure 5 This is a comparison of the experimental and simulated stress-time curves of the present invention under different experimental parameters. Figure (a) corresponds to a laser power density of 216 W / cm2, Figure (b) corresponds to a laser power density of 261 W / cm2, Figure (c) corresponds to a laser power density of 315 W / cm2, and Figure (d) corresponds to a laser power density of 351 W / cm2.

[0030] Figure 6 This is a diagram illustrating the necking effect of continuous laser irradiation on aerospace-grade high-strength 7075 aluminum alloy, successfully simulated by this invention.

[0031] Figure 7 This is a damage effect diagram of aerospace-grade high-strength 7075 aluminum alloy successfully simulated by continuous laser irradiation according to the present invention;

[0032] Figure 8 This is the damage morphology of aerospace-grade high-strength 7075 aluminum alloy under continuous laser irradiation under the experimental conditions of this invention. Detailed Implementation

[0033] The technical solutions of the present invention will be clearly and completely described below with reference to the accompanying drawings of the embodiments of the present invention. Obviously, the described embodiments are only some embodiments of the present invention, and not all embodiments. Based on the embodiments of the present invention, all other embodiments obtained by those skilled in the art without creative effort are within the scope of protection of the present invention.

[0034] This invention provides a numerical simulation method for continuous laser irradiation of 7075 aluminum alloy under external load based on a modified Johnson-Cook model, combined with... Figure 1 This includes the following steps:

[0035] Step 1: Perform ABAQUS (finite element simulation software) simulation preprocessing by defining geometric models and material parameters, and declaring loads to construct a finite element analysis model;

[0036] Step 2: Based on the laser heat source parameters of the finite element analysis model, obtain the laser surface heat source model through a one-dimensional Gaussian function; the laser heat source parameters are attached to the laser surface heat source model by writing the vdflux subroutine (a surface heat source model definition program in ABAQUS);

[0037] Step 3: Set up the Johnson-Cook (the inventor of an elastic-plastic model used in this invention, after whom the elastic-plastic model is named) elastic-plastic model according to the finite element analysis model;

[0038] Step 4: Simulate real-world test conditions by setting boundary and initial conditions for the temperature field and the stress field of the Johnson-Cook elastoplastic model and the laser surface heat source model. The boundary conditions for the temperature field are edge adiabatic conditions, the initial conditions for the temperature field are ambient temperature, the boundary conditions for the stress field are fixed constraint conditions and external displacement boundary conditions, and the initial conditions for the stress field are set to no initial displacement and no initial velocity field.

[0039] Step 5: Based on the laser surface heat source model and the Johnson-Cook elastoplastic model, divide the finite element mesh and define the analysis step to obtain the Johnson-Cook elastoplastic numerical simulation model that simulates the thermo-mechanical coupling behavior; the finite element mesh is a mesh that is divided into different regions, from sparse to dense and then back to sparse, and the mesh type is assigned as c3d8r in ABAQUS; the defined analysis step is dynamic explicit and temperature-displacement coupled.

[0040] Step 6: Based on the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior, a tensile model simulating real displacement load is obtained by conducting a real-world experiment of laser irradiation on aluminum alloy under preload, recording displacement-time data, and performing data fitting. The tensile model simulating real displacement load is implemented by writing a subroutine of the fitting function vuamp (a displacement load definition program in ABAQUS).

[0041] Step 7: Using a tensile model simulating real-world displacement loads, combined with a Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior, a pre-simulation of laser irradiation of aluminum alloy under preload is performed. The pre-simulated stress-time plot is compared with the stress-time plot of the actual laser-irradiated aluminum alloy under preload. The correction factor of the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior is determined by inversion. Then, real-world experiments of laser irradiation of high-strength 7075 aluminum alloy under various preload sizes are conducted. The stress-time plots of the real experiments are compared with the stress-time plots of the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior to verify the effectiveness of the correction factor of the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior.

[0042] Step 8: Combining the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior with the results of laser irradiation experiments on high-strength 7075 aluminum alloy under various preloads, analyze the changes in the mechanical behavior of the high-strength 7075 aluminum alloy target.

[0043] The material in step 1 has a three-dimensional plate shape and a thickness greater than the absorption thickness of the laser incident material. It is made of opaque metal.

[0044] In step 2, the laser surface heat source model is a VDflux subroutine, which includes the target structure dimensions and material parameters. The structure dimensions include length, width, and thickness. The material parameters include density, specific heat capacity, and thermal conductivity. The laser parameters used include laser power density and spot radius. The laser surface heat source model is a one-dimensional Gaussian function distributed surface heat source model, as shown in the following formula:

[0045]

[0046] Where q is the heat source and Q is the power, with units of mW / mm². 2 ; The normalization factor ensures that 99.7% of the heat flux is concentrated in the central area; α is the target absorptivity; R0 is the Gaussian radius in the x-direction, used for width control; W y y is the width of the uniform distribution in the y direction; x is the global x-coordinate of the current calculation point; x0 is the global x-coordinate of the heat source center.

[0047] The Johnson-Cook elastoplastic model in step 3 is shown in the following formula:

[0048]

[0049] Where, σ flowThe flow stress is obtained from the equation on the right side. The equation on the right side can be considered as the product of three terms: strain hardening, strain rate-dependent hardening, and temperature softening. In the entire flow stress calculation formula, A is the yield strength at room temperature, a fixed value that can be obtained from literature or experiments; A0 is a correction factor; B is the work hardening modulus, which, along with the hardening exponent n, controls the material's hardening behavior based on the equivalent plastic strain ε in the plastic stage. In the second term, C is the strain rate reference value, a constant, which, along with the strain rate reference value... correspond. The term represents the equivalent plastic strain rate, specifically the strain rate-controlled hardening term. In the third term, T0 is the reference temperature; in this paper, room temperature (293.15 K) is used. melt Let t be the melting point of the material, T be the current temperature, and g(t) be the temperature softening coefficient, which is not considered in the elastic stage. When the tensile stress passes the yield point and the plastic stage begins, the mechanical behavior that controls the transition from plasticity to failure is simultaneously initiated. This term reflects the change in flow stress caused by the change in temperature field under temperature variations, and is 1 at room temperature.

[0050] The initial conditions for the temperature field in step 4 are as follows:

[0051] T nwe (x, y, z, t)| t=0 =T1;

[0052] Where T1 is the initial temperature, t is the time, x, y, z are the position coordinates, and T new Let x, y, z be the temperature at time t; in the initial analysis step, the entire high-strength 7075 aluminum alloy target model is analyzed with a uniform room temperature initial temperature field, ignoring the thermal convection and thermal radiation effects of the aluminum alloy and air.

[0053] In step 4, the fixed constraint boundary conditions of the stress field are as follows: the degree of freedom of one end is completely fixed, U1=U2=U3=UR1=UR2=UR3=0, and the other end is used as the tension end. At the center of the surface, rpdot (a general name for the reference point) is set as the reference point, and the surface is set as a distributed coupling structure. The boundary conditions are set as U2=U3=0, and U1 is the acceleration boundary condition with the amplitude set to user definition, which serves as the interface for the subsequent vuamp displacement subroutine.

[0054] The mesh generation method in step 5 is as follows: the central region with the greatest stress and temperature gradient exists, so it is divided into the finest mesh, and the region is determined by the radius of our Gaussian formula. Then, it gradually becomes thicker around the perimeter. The analysis step is dynamic explicit and temperature-displacement coupled.

[0055] Step 6 specifically includes the following steps:

[0056] Step 7-1: Based on the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior, conduct a real-world experiment of laser irradiation on aluminum alloy under preload, select a set of preload and laser power density as reference, conduct the experiment, and record the values ​​of displacement sensor and tension sensor.

[0057] Step 7-2: Perform nonlinear fitting in Origin (a data processing software), select the fitting function y=A1*exp(-x / t1)+y0 to fit the displacement data, calculate the acceleration of the fitted displacement data and write it as a vuamp subroutine to obtain a tensile model simulating real displacement load.

[0058] Step 7 specifically includes the following steps:

[0059] Step 8-1: Using a tensile model simulating real-world displacement loads, combined with a Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior, a pre-simulation of laser-irradiated aluminum alloy under preload is performed. The stress-time diagrams from the real experiment are compared with those from the pre-simulation, and the values ​​of the correction factor A0, g(t), the start time of the step function, and the magnitude of the correction are adjusted. This yields accurate parameters for the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior.

[0060] Step 8-2: Based on the accurate Johnson-Cook elastoplastic numerical simulation model parameters that simulate thermo-coupling behavior, conduct simulation and real-world experiments under different laser power densities and preload conditions to verify the feasibility of the accurate Johnson-Cook elastoplastic numerical simulation model parameters that simulate thermo-coupling behavior.

[0061] Step 8-3: Compare the stress-time curves obtained from the experiment to verify the effectiveness of the stress simulation module;

[0062] Step 8-4: If the deviation between the stress-time curves of the actual experiment and the numerical simulation is small, it is considered that the numerical simulation method can simulate the process of continuous laser irradiation of aerospace-grade high-strength 7075 aluminum alloy well.

[0063] A system for implementing the above-mentioned numerical simulation method for continuous laser irradiation of 7075 aluminum alloy under external load based on the modified Johnson-Cook model includes the following modules:

[0064] The finite element analysis module is used to establish a geometric model of aerospace-grade high-strength 7075 aluminum alloy irradiated by continuous laser and to perform mesh generation;

[0065] The parameter selection module is used to select different laser parameters;

[0066] The experimental verification module is used to verify the model by continuously irradiating aerospace-grade high-strength 7075 aluminum alloy with laser, and to compare the stress curves obtained from the experiment and simulation, as well as the experimental damage morphology diagram and the stress curve obtained from the simulation.

[0067] The damage threshold calculation module is used to calculate the damage threshold of the material based on the input parameters.

[0068] The laser irradiation experimental platform module is used to build the experimental environment, control the irradiation time and parameters, and record the temperature change curve over time and the dynamic damage process.

[0069] The finite element analysis module is used to perform numerical simulation of the finite element analysis model of aerospace-grade high-strength 7075 aluminum alloy under continuous laser irradiation, and to extract the temperature field and stress field distribution of the position-sensitive detector, as well as the temperature and stress variation curves of the center point of the position-sensitive detector surface over time.

[0070] The curve comparison module is used to compare the stress-time curves obtained from experiments with those obtained from simulations, and to compare the experimental damage morphology diagrams with those obtained from simulations, in order to determine the effectiveness of the model.

[0071] Example

[0072] Based on such Figure 2 The boundary conditions are shown in the schematic diagram of the three-dimensional numerical simulation model of the present invention. Figure 3 As shown. To ensure the reliability of the numerical calculation results, the following assumptions and simplifications are made to the model:

[0073] (1) Assume that the materials of each functional layer of the device have uniformity and isotropic characteristics;

[0074] (2) Considering that the geometric size of the model is much larger than the diameter of the laser spot, the boundary is set to adiabatic conditions, that is, heat will not be conducted to the boundary area during laser irradiation;

[0075] (3) The bottom surface of the model also adopts adiabatic boundary conditions;

[0076] (4) In thermodynamic analysis, convective heat transfer and thermal radiation effects at the boundary are ignored;

[0077] (5) Liquid phase flow is not considered. If a liquid phase region exists, it is treated as heat conduction.

[0078] The detailed working principle of this method is as follows:

[0079] Step 1: Geometric Modeling and Physics Modeling

[0080] like Figure 2 As shown, the established geometric model is a regular 100mm*10mm*1mm high-strength 7075 aluminum alloy cuboid target.

[0081] like Figure 2 As shown, this invention studies the damage behavior of high-strength 7075 aluminum alloy under the combined action of preload and laser. The physical fields of thermodynamics and elastoplastic-fracture mechanics are established, and explicit dynamic analysis is performed using thermo-mechanical coupling.

[0082] Step 2: Parameter settings and laser surface heat source model writing

[0083] Table 1 Physical and mechanical properties of 7075 aluminum alloy

[0084]

[0085] Table 2. Thermophysical parameters of 7075 aluminum alloy as a function of temperature

[0086]

[0087]

[0088] The Johnson-Cook parameters used to find material parameters are shown in the table below.

[0089] Table 3. Johnson-Cook model parameters for 7075 aluminum alloy

[0090]

[0091] After defining the material properties, the room temperature of the entire model is defined as 293.15 K, absolute zero as 0 K, and the Stefan-Boltzmann constant as 5.67E-11. Cross sections are created, and the entire material model is categorized into the created cross sections.

[0092] The Abaqus subroutines used in this invention were implemented in an environment of Abaqus 2023 + Microsoft Visual Studio 2019 + Intel Visual Fortran 2020. A user-defined subroutine `vdflux` was declared in the load settings, and a new user-defined amplitude subroutine `vuamp` was declared in the amplitude settings, serving as the program interface. The corresponding interface format was found by consulting the Abaqus help manual, and the corresponding subroutines were written in Fortran language in Microsoft Visual Studio 2019.

[0093]

[0094] The aforementioned laser spot is incorporated into the vdflux subroutine as a surface heat flux. Because the vdflux subroutine reads, calculates, and returns the diffusion flux to the Abaqus solver at the start of each analysis step, the surface heat source represented by the laser is written in Fortran within the vdflux subroutine, declaring the extraction of the global coordinates of the current analysis step time and the calculation point.

[0095] Step 3: Setting up the Johnson-Cook elastoplastic model

[0096] The modified Johnson-Cook plasticity model in step 3 is as follows:

[0097]

[0098] A0 is inserted as a correction factor into the plastic strain hardening term to adjust the mechanical properties of the material. g(t) is the temperature softening coefficient and is not considered in the elastic stage. When the tensile stress passes the yield point and the plastic stage is initiated, the mechanical behavior of the material from the plastic stage to the failure stage is simultaneously initiated.

[0099] Step 4: Establishing the temperature and stress fields

[0100] (1) Boundary conditions and initial conditions of the temperature field

[0101] Neglecting heat convection and heat radiation, the boundary conditions are adiabatic.

[0102] The initial conditions are:

[0103] T new (x, y, z, t)| t＝0 =T1;

[0104] Where T1 is the initial temperature, t is the time, x, y, z are the position coordinates, and T new Let x, y, z be the temperature at time t; in the initial analysis step, the entire high-strength 7075 aluminum alloy target model is analyzed with a uniform room temperature initial temperature field, ignoring the thermal convection and thermal radiation effects of the aluminum alloy and air.

[0105] (2) Boundary conditions and initial conditions of the stress field

[0106] The fixed constraint boundary conditions of the stress field are as follows: the degrees of freedom of one end are completely fixed, U1=U2=U3=UR1=UR2=UR3=0, and the other end is used as the tension end. An rpdot is set at the center of the surface as a reference point and is set to be structurally distributed coupled with the surface. The boundary conditions are set as U2=U3=0, and U1 is the acceleration boundary condition with an amplitude set to user definition, which serves as the interface for the subsequent vuamp displacement subroutine.

[0107] Step 5: Mesh Generation

[0108] The meshing method is as follows: the region with the greatest stress and temperature gradient in the central region under laser irradiation is divided into the finest mesh, and the region is determined by the radius of our Gaussian formula. Then the mesh gradually becomes thicker around the perimeter. The analysis step is dynamic and explicit, with temperature-displacement coupling, and the mesh is also explicitly temperature-displacement coupled.

[0109] Step 6: Simulate and display the tensile model of displacement load.

[0110] A set of preload and laser power density were selected as references. Experiments were conducted and the values ​​of displacement sensor and tension sensor were recorded. Nonlinear fitting was performed in Origin. The fitting function y=Al*exp(-x / t1)+y0 was selected to fit the displacement data. The acceleration of the fitted displacement data was calculated and written as a vuamp subroutine.

[0111] The temperature and stress field distributions were obtained through finite element iterative calculations.

[0112] Step 7: Conduct laser irradiation experiments, determine the magnitude of the correction factor using the inversion method, and compare the experimental results with the simulated stress-time curves and damage morphology to verify the effectiveness of the numerical simulation method.

[0113] 1. Compare the stress-time curve obtained from the preliminary experiment with the stress-time curve obtained from the simulation, and adjust the value of the correction factor A0, as well as the start time and correction value of g(t) as the step function;

[0114] 2. After correction, experiments were conducted on the system under different laser power densities and preload conditions to verify the feasibility of a numerical simulation method and system for continuous laser irradiation of 7075 aluminum alloy under external load based on the modified Johnson-Cook model.

[0115] 3. Compare the damage morphology of the damaged specimens obtained from the experiment with the stress simulation results to verify the effectiveness of the stress simulation module.

[0116] 4. If the experimental results deviate little from the simulation results, it is considered that the numerical simulation method can effectively simulate the process of continuous laser irradiation of aerospace-grade high-strength 7075 aluminum alloy.

[0117] Step 8: Analyze the mechanical behavior

[0118] By combining the temperature and stress field distributions from simulations and experiments, the stress-time curves of high-strength 7075 aluminum alloy sputtering targets were analyzed.

[0119] This embodiment integrates multiple steps such as finite element analysis, experimental verification, parameter selection, and multiphysics coupling to efficiently and accurately analyze the damage threshold, providing a theoretical basis for damage research on aerospace aluminum materials and having significant implications for estimating the destructive effects of high-energy laser weapons.

[0120] In the model simulation calculation stage, the main operation process is as follows: select a suitable solver for solving, and here select the dynamic explicit analysis step. After completing the above settings, the simulation calculation can be performed.

[0121] In the post-processing stage of the model, the main operation process is as follows: obtain the RF support reaction force and displacement in the U1 direction of the rpdot point, process them in Origin to obtain stress-time curves and motion quantities, obtain the temperature of the material center point to determine the temperature rise, and obtain stress cloud map and temperature cloud map to intuitively display the damage process and fracture morphology.

[0122] The embodiments of the present invention can be implemented using ABAQUS finite element simulation software.

[0123] This embodiment establishes a model of continuous laser irradiation of aerospace-grade high-strength 7075 aluminum alloy, the geometric model of which is as follows: Figure 2 As shown, Figure 2 The target material is 1mm*10mm*100mm aluminum material. The center of the target material is the laser surface heat source model with a width of 7mm. One end of the target material is a fixed constraint condition, and the other end is a tensile model simulating real displacement load. Figure 3 Mesh generation was performed; preliminary experiments were conducted and fitted to obtain a comparison between the simulated stress-time curve and the experimental curve, for example... Figure 4 The coordinate system uses time (seconds) on the horizontal axis and stress (MPa) on the vertical axis. Red represents the stress-time curve measured in real-world experiments, while green represents the stress-time curve calculated in the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior. Comparisons between experimental and simulation results under different laser power densities and preload conditions are obtained. Figure 5 As shown in (a)-(d), respectively Figure 5 (a) Stress-time curves of 7075 aluminum alloy sputtering targets under different preload conditions corresponding to a power density of 216 W / cm^2. Figure 5 (b) Stress-time curves of 7075 aluminum alloy sputtering targets under different preload conditions corresponding to a power density of 261 W / cm². Figure 5 (c) Stress-time curves of 7075 aluminum alloy sputtering targets under different preload conditions corresponding to a power density of 315 W / cm^2. Figure 5 (d) Stress-time curves of 7075 aluminum alloy targets under different preload conditions at a power density of 351 W / cm²; stress distribution cloud maps at necking and failure are obtained as follows. Figure 6, Figure 7 As shown, the cloud map represents the stress magnitude in MPa; the effectiveness of the model was verified through laser irradiation experiments. Figure 8 The crack morphology of the target material fractured in the real experiment is shown, with the crack exhibiting a U-shape similar to that in the simulation.

[0124] It should be noted that, in this document, relational terms such as "first" and "second" are used only to distinguish one entity or operation from another, and do not necessarily require or imply any such actual relationship or order between these entities or operations. Furthermore, the terms "comprising," "including," or any other variations thereof are intended to cover non-exclusive inclusion, such that a process, method, article, or apparatus that comprises a list of elements includes not only those elements but also other elements not expressly listed, or elements inherent to such process, method, article, or apparatus.

[0125] Although embodiments of the invention have been shown and described, it will be understood by those skilled in the art that various changes, modifications, substitutions and alterations can be made to these embodiments without departing from the principles and spirit of the invention, the scope of which is defined by the appended claims and their equivalents.

Claims

1. A numerical simulation method for continuous laser irradiation of 7075 aluminum alloy under external load based on a modified Johnson-Cook model, characterized in that, Includes the following steps: Step 1: Construct a finite element analysis model by defining the geometric model and material parameters, and declaring the loads; Step 2: Based on the laser heat source parameters of the finite element analysis model, obtain the laser surface heat source model through a one-dimensional Gaussian function; the laser heat source parameters are attached to the laser surface heat source model by writing a vdflux subroutine. Step 3: Set up the Johnson-Cook elastoplastic model based on the finite element analysis model; Step 4: Simulate real-world test conditions by setting boundary and initial conditions for the temperature field and the stress field of the Johnson-Cook elastoplastic model and the laser surface heat source model. The boundary conditions for the temperature field are edge adiabatic conditions, the initial conditions for the temperature field are ambient temperature, the boundary conditions for the stress field are fixed constraint conditions and external displacement boundary conditions, and the initial conditions for the stress field are set to no initial displacement and no initial velocity field. Step 5: Based on the laser surface heat source model and the Johnson-Cook elastoplastic model, divide the finite element mesh and define the analysis step to obtain the Johnson-Cook elastoplastic numerical simulation model that simulates the thermo-mechanical coupling behavior; the finite element mesh is a mesh that is divided into different regions, from sparse to dense and then back to sparse, and the mesh type is assigned as c3d8r in ABAQUS; the defined analysis step is dynamic explicit and temperature-displacement coupled. Step 6: Based on the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior, a tensile model simulating real displacement load is obtained by conducting a real-world experiment of laser irradiation on aluminum alloy under preload, recording displacement-time data, and performing data fitting. The tensile model simulating real displacement load is implemented by writing a vuamp subroutine for the fitting function. Step 7: Using a tensile model simulating real-world displacement loads, combined with a Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior, a pre-simulation of laser irradiation of aluminum alloy under preload is performed. The pre-simulated stress-time plot is compared with the stress-time plot of the actual laser-irradiated aluminum alloy under preload. The correction factor of the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior is determined by inversion. Then, real-world experiments of laser irradiation of high-strength 7075 aluminum alloy under various preload sizes are conducted. The stress-time plots of the real experiments are compared with the stress-time plots of the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior to verify the effectiveness of the correction factor of the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior. Step 8: Combining the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior with the results of laser irradiation experiments on high-strength 7075 aluminum alloy under various preloads, analyze the changes in the mechanical behavior of the high-strength 7075 aluminum alloy target.

2. The numerical simulation method for continuous laser irradiation of 7075 aluminum alloy under external load based on the modified Johnson-Cook model according to claim 1, characterized in that, The material in step 1 has a three-dimensional plate shape and a thickness greater than the absorption thickness of the laser incident material. It is made of opaque metal.

3. The numerical simulation method for continuous laser irradiation of 7075 aluminum alloy under external load based on the modified Johnson-Cook model according to claim 2, characterized in that, In step 2, the laser surface heat source model is a VDflux subroutine, which includes the target structure dimensions and material parameters. The structure dimensions include length, width, and thickness. The material parameters include density, specific heat capacity, and thermal conductivity. The laser parameters used include laser power density and spot radius. The laser surface heat source model is a one-dimensional Gaussian function distributed surface heat source model, as shown in the following formula: Where q is the heat source and Q is the power; α is the normalization factor; R0 is the target absorptivity; R0 is the Gaussian radius in the x-direction, used for width control; W y y is the width of the uniform distribution in the y direction; x is the global x-coordinate of the current calculation point; x0 is the global x-coordinate of the heat source center.

4. The numerical simulation method for continuous laser irradiation of 7075 aluminum alloy under external load based on the modified Johnson-Cook model according to claim 3, characterized in that, The Johnson-Cook elastoplastic model in step 3 is shown in the following formula: Where, σ flow Let A be the flow stress, A be the yield strength at room temperature, and A0 be the correction factor; B be the work hardening modulus, n be the hardening exponent, ε be the equivalent plastic strain, and C be the strain rate reference value. Strain rate reference value T is the equivalent plastic strain rate, T0 is the reference temperature, and T melt Let T be the melting point of the material, T be the temperature at the current moment, and g(t) be the temperature softening coefficient.

5. The numerical simulation method for continuous laser irradiation of 7075 aluminum alloy under external load based on the modified Johnson-Cook model according to claim 4, characterized in that, The initial conditions for the temperature field in step 4 are as follows: T new (x, y, z, t)| t＝0 =T1; Where T1 is the initial temperature, t is the time, x, y, z are the position coordinates, and T new Let x, y, z be the temperatures at time t; In step 4, the fixed constraint boundary conditions of the stress field are as follows: the degree of freedom of one end is completely fixed, U1=U2=U3=UR1=UR2=UR3=0, the other end is the tension end, rpdot is set as the reference point at the center of the surface, and the surface is set as a distributed coupling of the structure, and the boundary conditions are set U2=U3=0, U1 is the acceleration boundary condition, and the amplitude is set to user definition, which serves as the interface for the subsequent vuamp displacement subroutine.

6. The numerical simulation method for continuous laser irradiation of 7075 aluminum alloy under external load based on the modified Johnson-Cook model according to claim 5, characterized in that, The mesh generation method in step 5 is as follows: the central region with the greatest stress and temperature gradient exists, so it is divided into the finest mesh, and the region is determined by the radius of our Gaussian formula. Then, it gradually becomes thicker around the perimeter. The analysis step is dynamic explicit and temperature-displacement coupled.

7. The numerical simulation method for continuous laser irradiation of 7075 aluminum alloy under external load based on the modified Johnson-Cook model according to claim 6, characterized in that, Step 6 specifically includes the following steps: Step 7-1: Based on the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior, conduct a real-world experiment of laser irradiation on aluminum alloy under preload, select a set of preload and laser power density as reference, conduct the experiment, and record the values ​​of displacement sensor and tension sensor. Step 7-2: Perform nonlinear fitting in Origin, select the fitting function y=A1*exp(-x / t1)+y0 to fit the displacement data, calculate the acceleration of the fitted displacement data and write it as a vuamp subroutine to obtain the tensile model simulating the real displacement load.

8. The numerical simulation method for continuous laser irradiation of 7075 aluminum alloy under external load based on the modified Johnson-Cook model according to claim 1, characterized in that, Step 7 specifically includes the following steps: Step 8-1: Using a tensile model simulating real-world displacement loads, combined with a Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior, a pre-simulation of laser-irradiated aluminum alloy under preload is performed. The stress-time diagrams from the real experiment are compared with those from the pre-simulation, and the values ​​of the correction factor A0, g(t), the start time of the step function, and the magnitude of the correction are adjusted. This yields accurate parameters for the Johnson-Cook elastoplastic numerical simulation model simulating thermo-mechanical coupling behavior. Step 8-2: Based on the accurate Johnson-Cook elastoplastic numerical simulation model parameters that simulate thermo-coupling behavior, conduct simulation and real-world experiments under different laser power densities and preload conditions to verify the feasibility of the accurate Johnson-Cook elastoplastic numerical simulation model parameters that simulate thermo-coupling behavior. Step 8-3: Compare the stress-time curves obtained from the experiment to verify the effectiveness of the stress simulation module.

9. A system for implementing the numerical simulation method for continuous laser irradiation of 7075 aluminum alloy under external load based on a modified Johnson-Cook model as described in any one of claims 1-8, characterized in that, Includes the following modules: The finite element analysis module is used to establish a geometric model of aerospace-grade high-strength 7075 aluminum alloy irradiated by continuous laser and to perform mesh generation; The parameter selection module is used to select different laser parameters; The experimental verification module is used to verify the model by continuously irradiating aerospace-grade high-strength 7075 aluminum alloy with laser, and to compare the stress curves obtained from the experiment and simulation, as well as the experimental damage morphology diagram and the stress curve obtained from the simulation. The damage threshold calculation module is used to calculate the damage threshold of the material based on the input parameters. The laser irradiation experimental platform module is used to build the experimental environment, control the irradiation time and parameters, and record the temperature change curve over time and the dynamic damage process. The finite element analysis module is used to perform numerical simulation of the finite element analysis model of aerospace-grade high-strength 7075 aluminum alloy under continuous laser irradiation, and to extract the temperature field and stress field distribution of the position-sensitive detector, as well as the temperature and stress variation curves of the center point of the position-sensitive detector surface over time. The curve comparison module is used to compare the stress-time curves obtained from experiments with those obtained from simulations, and to compare the experimental damage morphology diagrams with those obtained from simulations, in order to determine the effectiveness of the model.

Images