Metal component fatigue life evaluation method based on ABAQUS secondary development and considering elastic-plastic damage

Abstract

The invention discloses an ABAQUS secondary development-based metal component fatigue life evaluation method considering elastic-plastic damage, which comprises the following steps of: firstly, completing metal component modeling based on ABAQUS or other three-dimensional software, further completing pretreatment setting in the ABAQUS, calling a UMAT subprogram by using UserMateria in a material attribute definition module, and carrying out material attribute definition on the material attribute definition module by using a UMAT subprogram; and meanwhile, corresponding material parameters and state variable quantity are defined. A cycle jump algorithm is adopted to save calculation cost, the damage and the service life of the metal component are calculated according to an elastic-plastic damage evolution criterion when calculation of a specific cycle block is completed, and a calculation result can be visually obtained through a Visualization module. The fatigue life evaluation method considering the elastic-plastic damage of the metal component is developed on the basis of ABAQUS secondary development, the dangerous area of the metal component can be accurately identified, the fatigue life of the metal component can be predicted, and effective theoretical guidance is provided for structural optimization design, service life prolonging and reliability improvement of the metal component.

Description

Technical Field

[0001] The present invention relates to a method for evaluating the fatigue life of metal components considering elastoplastic damage based on secondary development of ABAQUS. Background Art

[0002] Metal components are prone to fatigue failure under long-term alternating loads, and the damage process is characterized by high concealment and rapid development in the fracture stage. It is usually difficult to accurately evaluate the life of metal components during the design stage, which is likely to cause major accidents.

[0003] The traditional design concept based on the yield criterion cannot accurately reflect the current complex and changeable actual working conditions; critical plane methods such as Brown-Miller, Morrow, and SWT evaluate the global life of components based on the stress level of components without damage, and there may be large errors in the calculation results; prototype experiments have deficiencies such as long cycle, requiring a large amount of manpower and material resources, and extending the product development cycle;

[0004] Although existing simulation technologies can partially replace experiments, they are relatively complex in form and require a large number of fatigue experiments to calibrate damage parameters, which limits the application of simulation methods. Moreover, existing simulation methods do not consider the influence of isotropic hardening / softening and are difficult to be popularized in engineering practice.

[0005] Therefore, there is an urgent need to develop a method for evaluating the fatigue life of metal components. Summary of the Invention

[0006] The purpose of the present invention is to provide a method for evaluating the fatigue life of metal components considering elastoplastic damage based on secondary development of ABAQUS to solve the problems existing in the prior art.

[0007] The technical solution adopted to achieve the purpose of the present invention is as follows: a method for evaluating the fatigue life of metal components considering elastoplastic damage based on secondary development of ABAQUS includes the following steps:

[0008] 1) Establish a geometric model of the metal component: Use the Part module of ABAQUS to establish a geometric model of the metal component or draw a three-dimensional model of the metal component through a drawing software and import it into the ABAQUS software in STEP format;

[0009] 2) Complete the preprocessing settings of the metal component model through the ABAQUS software:

[0010] 2-1) Based on the Property module of ABAQUS, define the material properties of the metal component and the number of state variables through UserMaterial and Depvar;

[0011] 2-2) Complete the assembly of metal components based on the Assembly module of ABAQUS;

[0012] 2-3) Set the time step for the simulation of metal components based on the Step module of ABAQUS, and set the output of state variables in the FieldOutput module;

[0013] 2-4) Set the contact characteristics of metal components based on the Interaction module;

[0014] 2-5) Set the load conditions and constraints of metal components based on the Load module;

[0015] 2-6) Complete the mesh division of metal components based on the Mesh module;

[0016] 2-7) Create a Job in the Job module, and select the subroutine Damage_and_fatigue_life_evaluation for fatigue life assessment of metal components considering elastoplastic damage written in Fortran in the UserSubroutineFile;

[0017] 3) Complete the construction of the elastoplastic constitutive model of metal components based on the subroutine Damage_and_fatigue_life_evaluation:

[0018] a) The elastic stage of the metal component material is determined by the generalized Hooke's law;

[0019] b) The plastic stage of the metal component material is determined by nonlinear isotropic hardening / softening and kinematic hardening;

[0020] c) The Damage_and_fatigue_life_evaluation subroutine constructs the stiffness matrix by reading the material parameters defined in ABAQUS;

[0021] d) The Damage_and_fatigue_life_evaluation subroutine calculates the trial stress by reading the strain calculated in ABAQUS and according to the stiffness matrix;

[0022] e) Judge whether the component undergoes plastic deformation by comparing the trial stress and the transient yield strength;

[0023] f) When the component does not undergo plastic deformation, the trial stress is the true stress;

[0024] g) When the component undergoes plastic deformation, the Damage_and_fatigue_life_evaluation subroutine determines the plastic strain increment through the Newton iteration algorithm, further determines the plastic stress / strain according to the plastic flow criterion, and then calculates the stiffness matrix in the plastic stage through the consistent tangent modulus algorithm;

[0025] 4) The Damage_and_fatigue_life_evaluation subroutine adopts a loop skipping algorithm to accelerate the calculation:

[0026] i) One load cycle in the Damage_and_fatigue_life_evaluation subroutine is regarded as an actual ΔN load cycle (i.e., a cycle block);

[0027] ii) Within the same cycle block, the stress-strain history of each cycle is regarded as the same, the damage and life are not updated, and the life ΔN of each element is the same;

[0028] 5) Damage and fatigue life assessment of metal components:

[0029] I) The total damage in the Damage_and_fatigue_life_evaluation subroutine is defined as the sum of elastic damage and plastic damage, and the total damage growth rate is equal to the sum of the elastic damage growth rate and the plastic damage growth rate;

[0030] II) The elastic damage growth rate is determined by the octahedral shear stress, damage parameter, and damage variable;

[0031] III) The plastic damage growth rate is determined by the equivalent stress, material parameters, damage parameters, damage variables, and cumulative plastic strain;

[0032] IV) When a cycle block ends, the Damage_and_fatigue_life_evaluation subroutine calculates the damage growth rate of each element according to the stress-strain of this cycle block;

[0033] V) The element with the maximum damage growth rate is determined as the critical element, and its damage growth rate is determined as the critical damage growth rate;

[0034] VI) The maximum damage increment ΔD of each cycle block in the Damage_and_fatigue_life_evaluation subroutine is set to be the same, and the critical damage value is set to D C ;

[0035] VII) The actual number of cycles ΔN of the current cycle block can be obtained by dividing the maximum damage increment ΔD by the critical damage growth rate;

[0036] VIII) The damage increment of each element in the current cycle block can be obtained by multiplying the actual damage growth rate of each element by the actual number of cycles ΔN;

[0037] IX) The damage value of a specific element can be obtained by further accumulating the damage increments of that element;

[0038] Ⅹ) The number of cycles of the current component can be obtained by accumulating the actual number of cycles ΔN of each cycle block;

[0039] XI) The material mechanical property parameters of the damaged elements can be updated according to the damage;

[0040] 6) When the maximum damage in all elements reaches the critical damage value D C crack initiation can be regarded as occurring, and the Damage_and_fatigue_life_evaluation subroutine can be terminated. At this time, the actual number of cycles of the metal component is its fatigue life;

[0041] 7) Further, the damage distribution characteristics of the metal component can be viewed through the Visualization module of ABAQUS to determine the dangerous area.

[0042] Furthermore, the generalized Hooke's law described in step a) is calculated using the following formula:

[0043]

[0044] where is the elastic strain, E and ν are the elastic modulus and Poisson's ratio respectively, σ ij and σ kk are the stresses, D is the damage variable, and δ ij is the Kronecker symbol.

[0045] Furthermore, the nonlinear isotropic hardening / softening described in step b) is calculated using the following formula:

[0046] σ y = σ y0 + σ ym (1 - e -bΔp ) (2)

[0047] where σ y is the transient yield limit, σ y0 is the initial yield limit, and σ yma and b are the magnitudes and saturation rates of isotropic hardening / softening respectively, and Δp is the accumulated plastic strain, which can be obtained through uniaxial cyclic experiments; when the material is isotropically hardened, σ ym is positive; when the material is isotropically softened, σ ym is negative; under the influence of isotropic hardening / softening, the yield surface of the material expands or contracts equally in all directions;

[0048] The non-linear kinematic hardening is calculated using the following formula:

[0049]

[0050] where α ij is the back stress, M is the magnitude of the hardening modulus, C k and γ k are kinematic hardening parameters, which can be obtained through uniaxial tensile experiments, is the accumulated plastic strain rate, and is calculated using the following formula:

[0051]

[0052] where is the plastic multiplier, is the plastic strain rate, and is calculated using the following formula:

[0053]

[0054] where F is the yield function, S ij is the deviatoric stress component, and "eq" refers to the equivalent stress part.

[0055] Furthermore, the following formula is used to determine whether plasticity occurs in step e):

[0056]

[0057] Furthermore, the damage described in step I) is represented by the ratio of the damaged area A D to the total area A:

[0058]

[0059] Then the total damage can be represented by the sum of the elastic damage D e and the plastic damage D p :

[0060] D = D e + D p (8)

[0061] Furthermore, the elastic damage rate dD e / dN is calculated using the following formula:

[0062]

[0063] Among them, Δτ8 is the octahedral shear stress range, and is calculated by the following formula:

[0064]

[0065] Among them, S ij,t and are the deviator stress components at times t and t0 respectively;

[0066] The elastic damage parameters τ r and m can be calculated by the following formula:

[0067]

[0068] Among them, τ f and B are fatigue parameters and can be obtained through torsion tests.

[0069] Furthermore, the plastic damage rate dD p / dN in step III) is calculated by the following formula:

[0070]

[0071] Among them, σ max is the maximum equivalent stress, Δp is the cumulative plastic strain, and q and S are plastic damage parameters, which are calculated by the following formula:

[0072]

[0073] Furthermore, the maximum damage growth rate in step V) can be calculated by the following formula:

[0074]

[0075] Among them, i is the cycle block number and j is the element number.

[0076] Furthermore, the actual number of cycles ΔN represented by the current cycle block in step VII) can be calculated by the following formula:

[0077]

[0078] Furthermore, the damage increment of each element in the current cycle block in step VIII) can be calculated by the following formula:

[0079]

[0080] Furthermore, the total damage of each element at the current moment in step IX) can be calculated by the following formula:

[0081]

[0082] Furthermore, the total life of each unit at the current moment in step X) can be calculated using the following formula:

[0083] N i+1 = N i + ΔN i (20)

[0084] Furthermore, the material mechanical property parameters of the damaged unit in step XI) can be updated according to the following formula:

[0085]

[0086] where is the current material parameter, is the yield limit of the damaged material degradation.

[0087] The beneficial effects of the present invention are as follows:

[0088] A. The present invention has a wider applicability: The present invention fully considers the non-linear isotropic hardening / softening and kinematic hardening characteristics of metal materials in the plastic stage, can more accurately describe the plastic behavior of metal components, and can provide more accurate life assessments for a wider range of metal components;

[0089] B. The present invention develops a new damage evolution model: The elastic damage evolution equation is determined by the octahedral shear stress, damage parameter, and damage variable, and the plastic damage control equation is determined by the equivalent stress, material parameter, damage parameter, damage variable, and cumulative plastic strain. The damage control equation is simplified, reducing the calculation amount, improving the calculation efficiency, and having sufficient calculation accuracy;

[0090] C. The present invention has extremely high implementability: The present invention only needs three groups of fatigue experiments with different stress levels to determine all damage parameters, overcomes the deficiency of requiring a large number of fatigue experiments to determine damage parameters, effectively saves experimental time and cost, makes this method easier to implement, and the shear stress-life curve fitted according to the experiment can provide guidance for preliminary life assessment;

[0091] D. The present invention establishes a mapping relationship between material parameters and damage parameters: The present invention proposes an inevitable connection between material parameters and damage parameters. The shear stress-life relationship fitted based on torsional fatigue experiments can further solve the damage parameters according to the mapping relationship, simplifying the calibration process of damage parameters;

[0092] E. The present invention has higher calculation accuracy for failure modes dominated by shear stress: The present invention is dominated by octahedral shear stress, accurately matches rolling contact fatigue and torsional fatigue failure, fully considers the influence of shear stress, has higher calculation accuracy, and also has sufficient accuracy for failure modes such as tension-compression and bending-torsion. Description of the Drawings

[0093] Figure 1 It is the overall flowchart of the simulation method of the present invention;

[0094] Figure 2 It is the mesh division diagram of the metal component;

[0095] Figure 3 It is the damage distribution diagram of the metal component;

[0096] Figure 4 It is the plastic strain distribution diagram of the metal component. Detailed Embodiment

[0097] The present invention will be further described below in conjunction with embodiments, but it should not be understood that the above-mentioned subject scope of the present invention is limited to the following embodiments. Without departing from the above technical idea of the present invention, various substitutions and changes made according to common technical knowledge and customary means in the art should be included within the protection scope of the present invention.

[0098] Embodiment 1:

[0099] This embodiment provides a fatigue life assessment method for metal components considering elastoplastic damage based on secondary development of ABAQUS, including the following steps:

[0100] 1) Establish a geometric model of the metal component: Use the Part module of ABAQUS to establish a geometric model of the metal component or draw a three-dimensional model of the metal component through a drawing software and import it into the ABAQUS software in STEP format;

[0101] 2) Complete the preprocessing settings of the metal component model through the ABAQUS software:

[0102] 2-1) Based on the Property module of ABAQUS, define the material properties of the metal component and the number of state variables through UserMaterial and Depvar;

[0103] 2-2) Complete the assembly of the metal component based on the Assembly module of ABAQUS;

[0104] 2-3) Set the time step of the metal component simulation based on the Step module of ABAQUS, and set the state variable output in the FieldOutput module;

[0105] 2-4) Set the contact characteristics of the metal component based on the Interaction module;

[0106] 2-5) Set the load conditions and constraints of the metal component based on the Load module;

[0107] 2-6) Complete the mesh division of the metal component based on the Mesh module;

[0108] 2-7) Create a Job in the Job module and select the subroutine Damage_and_fatigue_life_evaluation for evaluating the fatigue life of the metal component considering elastoplastic damage written in Fortran in the UserSubroutineFile;

[0109] 3) Complete the construction of the elastoplastic constitutive model of the metal component based on the subroutine Damage_and_fatigue_life_evaluation:

[0110] 3-1) The elastic stage of the metal component material is determined by the generalized Hooke's law;

[0111] 3-2) The plastic stage of the metal component material is determined by nonlinear isotropic hardening / softening and kinematic hardening;

[0112] 3-3) The Damage_and_fatigue_life_evaluation subroutine constructs the stiffness matrix by reading the material parameters defined in ABAQUS;

[0113] 3-4) The Damage_and_fatigue_life_evaluation subroutine calculates the trial stress by reading the strain calculated in ABAQUS and according to the stiffness matrix;

[0114] 3-5) Determine whether the component undergoes plastic deformation by comparing the trial stress and the transient yield strength;

[0115] 3-6) When the component does not undergo plastic deformation, the trial stress is the true stress;

[0116] 3-8) When the component undergoes plastic deformation, the Damage_and_fatigue_life_evaluation subroutine determines the plastic strain increment through the Newton iteration algorithm, further determines the plastic stress / strain according to the plastic flow criterion, and then calculates the stiffness matrix in the plastic stage through the consistent tangent modulus algorithm;

[0117] 4) The Damage_and_fatigue_life_evaluation subroutine uses the loop jump algorithm to accelerate the calculation:

[0118] One load cycle in the Damage_and_fatigue_life_evaluation subroutine is regarded as an actual ΔN load cycle (i.e., a cycle block).

[0119] 4-2) Within the same cycle block, the stress-strain history of each cycle is regarded as the same, damage and life are not updated, and the life ΔN of each element is the same.

[0120] 5) Damage and fatigue life evaluation of metal components:

[0121] 5-1) The total damage in the Damage_and_fatigue_life_evaluation subroutine is defined as the sum of elastic damage and plastic damage, and the total damage growth rate is equal to the sum of the elastic damage growth rate and the plastic damage growth rate.

[0122] 5-2) The elastic damage growth rate is determined by the octahedral shear stress, damage parameter, and damage variable.

[0123] 5-3) The plastic damage growth rate is determined by the equivalent stress, material parameters, damage parameter, damage variable, and accumulated plastic strain.

[0124] 5-4) When a cycle block ends, the Damage_and_fatigue_life_evaluation subroutine calculates the damage growth rate of each element according to the stress-strain of this cycle block.

[0125] 5-5) The element with the maximum damage growth rate is determined as the critical element, and its damage growth rate is determined as the critical damage growth rate.

[0126] 5-6) The maximum damage increment ΔD of each cycle block in the Damage_and_fatigue_life_evaluation subroutine is set to be the same, and the critical damage value is set to D C ;

[0127] 5-7) Dividing the maximum damage increment ΔD by the critical damage growth rate can obtain the actual number of cycles ΔN of the current cycle block.

[0128] 5-8) Multiplying the actual damage growth rate of each element by the actual number of cycles ΔN can obtain the damage increment of each element in the current cycle block.

[0129] 5-9) Further accumulating the damage increment of a specific element can obtain the damage value of this element.

[0130] 5-10) The cyclic count of the current component can be obtained by accumulating the actual cyclic counts ΔN of each cyclic block;

[0131] 5-11) The material properties of the damaged elements can be updated according to the damage;

[0132] 6) When the maximum damage in all elements reaches the critical damage value D C a crack initiation can be considered, and the Damage_and_fatigue_life_evaluation subroutine can be terminated. At this time, the actual cyclic count of the metal component is its fatigue life;

[0133] 7) View the damage distribution characteristics of the metal component through the Visualization module of ABAQUS to determine the dangerous area.

[0134] Example 2:

[0135] The main content of this example is the same as that of Example 1. Among them, this example is the fatigue damage process of a 18CrNiMo7-6 metal plate with a semi-circular notch under cyclic tensile loading. According to the Figure 1 shown process steps, simulations are carried out, which specifically include the following steps:

[0136] 1) Establish the geometric model of the metal component: Since the structure of this example is relatively simple, the modeling of the metal plate with a semi-circular notch is completed through the Part module of ABAQUS.

[0137] 2) Complete the preprocessing settings of the metal component model through ABAQUS software:

[0138] 2-1) Based on the Property module of ABAQUS, define the material properties of the metal component and the number of state variables through UserMaterial and Depvar; In this example, the default units mm-N-MPa are adopted. Define the material behavior in the EditMaterial of the Property module, and set the number of state variables Depvar to 78. Input UserMaterial according to Table 1 in sequence;

[0139] Table 1 18CrNiMo7-6 material parameters

[0140]

[0141] 2-2) Complete the assembly of the metal component based on the Assembly module of ABAQUS; Import the metal component Part in the Assembly module to complete the assembly;

[0142] 2-3) Set the time step for the simulation of the metal component based on the Step module in ABAQUS, and set the output of state variables in the FieldOutput module; create a static analysis and set large deformation. In Step1, set the global duration to 130 s and the initial increment to 1 s. Add the STATUS and SDV options to the default options in FieldOutput to output state variables;

[0143] 2-4) Set the contact characteristics of the metal component based on the Interaction module; there is only one metal component in this case, so there is no contact involved, but relevant contact properties need to be defined in other models with contact;

[0144] 2-5) Set the load conditions and constraints of the metal component based on the Load module; define the Pressure amplitude through Tabular in the Load module and apply it to the top surface of the metal component, and constrain the degrees of freedom of the bottom surface of the metal component through Displacement / Rotation;

[0145] 2-6) Complete the mesh division of the metal component based on the Mesh module; use An8-nodelinearbrick, reducedintegration, hourglasscontrol (C3D8R) to complete the mesh division of the metal component. The mesh of the semi-circular notch part is refined, and a total of 72,000 elements are generated. In this embodiment, only the operation process is demonstrated, so the mesh independence verification is not carried out;

[0146] 2-7) Create a Job in the Job module, and select the subroutine Damage_and_fatigue_life_evaluation for evaluating the fatigue life of the metal component considering elastoplastic damage written in Fortran in the UserSubroutineFile. At the same time, select multithreading to accelerate the calculation, and complete the variable assignment according to the damage parameters shown in Table 2 in the Damage_and_fatigue_life_evaluation subroutine.

[0147] Table 2 Damage parameters of 18CrNiMo7-6

[0148]

[0149] 3) Complete the construction of the elastoplastic constitutive model of the metal component based on the subroutine Damage_and_fatigue_life_evaluation:

[0150] a) The constitutive relationship in the elastic stage of the metal component material is determined by the generalized Hooke's law and is calculated using the following formula:

[0151]

[0152] Among them, is the elastic strain, E and ν are the elastic modulus and Poisson's ratio respectively, and σ ij and σ kk are the stresses, D is the damage variable, and δ ij is the Kronecker symbol;

[0153] b) The plastic stage of the metal component material is determined by nonlinear isotropic hardening / softening and kinematic hardening. The isotropic hardening / softening criterion is determined by the following formula:

[0154] σ y = σ y0 + σ ym (1 - e -bΔp ) (2)

[0155] Among them, σ y is the transient yield limit, σ y0 is the initial yield limit, σ ym and b are the amplitude and saturation rate of isotropic hardening / softening respectively, and Δp is the cumulative plastic strain, which can be obtained through uniaxial cyclic experiments; when the material is isotropic hardening, σ ym is positive; when the material is isotropic softening, σ ym is negative; under the influence of isotropic hardening / softening, the yield surface of the material expands or contracts equally in all directions;

[0156] The nonlinear kinematic hardening criterion is calculated by the following formula:

[0157]

[0158] Among them, α ij is the back stress, M is the quantity of the hardening modulus, C k and γ k are the kinematic hardening parameters, which can be obtained through uniaxial tensile experiments, is the cumulative plastic strain rate, and is calculated by the following formula:

[0159]

[0160] Among them is the plastic multiplier, is the plastic strain rate, and is calculated by the following formula:

[0161]

[0162] Among them, F is the yield function, S ij is the deviatoric stress component, and "eq" refers to the equivalent stress part;

[0163] c) The Damage_and_fatigue_life_evaluation subroutine constructs the stiffness matrix by reading the material parameters defined in ABAQUS;

[0164] d) The Damage_and_fatigue_life_evaluation subroutine calculates the trial stress by reading the strain calculated in ABAQUS and based on the stiffness matrix;

[0165] e) To determine whether plastic deformation occurs in the component by comparing the trial stress with the transient yield strength, the following formula can be used:

[0166]

[0167] f) When no plastic deformation occurs in the component, the trial stress is the true stress;

[0168] g) When plastic deformation occurs in the component, the Damage_and_fatigue_life_evaluation subroutine determines the plastic strain increment through the Newton iteration algorithm, further determines the plastic stress / strain according to the plastic flow criterion, and then calculates the stiffness matrix in the plastic stage through the consistent tangent modulus algorithm;

[0169] 4) The Damage_and_fatigue_life_evaluation subroutine uses a loop jump algorithm to accelerate the calculation:

[0170] i) One load cycle in the Damage_and_fatigue_life_evaluation subroutine is regarded as an actual ΔN load cycle (i.e., a cycle block);

[0171] ii) Within the same cycle block, the stress-strain histories of each cycle are regarded as the same, the damage and life are not updated, and the life ΔN of each element is the same;

[0172] 5) Damage and fatigue life assessment of metal components:

[0173] I) In the Damage_and_fatigue_life_evaluation subroutine, the damage is defined as the damaged area A D and is expressed as the ratio of the total area A:

[0174]

[0175] Then the total damage can be represented by the elastic damage D e and the plastic damage D p The sum is expressed as:

[0176] D = D e + D p (8)

[0177] II) The elastic damage growth rate dD e / dN is determined by the octahedral shear stress, damage parameter, and damage variable, and is calculated using the following formula:

[0178]

[0179] Among them, Δτ8 is the octahedral shear stress range, and is calculated using the following formula:

[0180]

[0181] Among them, S ij,t and are the deviatoric stress components at times t and t0, respectively;

[0182] The elastic damage parameters τ r and m can be calculated using the following formula:

[0183]

[0184] Among them, τ f and B are fatigue parameters, which can be obtained through torsion tests;

[0185] III) The plastic damage growth rate dD p / dN is determined by the equivalent stress, material parameters, damage parameters, damage variable, and accumulated plastic strain, and is calculated using the following formula:

[0186]

[0187] Among them, σ max is the maximum equivalent stress, Δp is the accumulated plastic strain, q and S are plastic damage parameters, and are calculated as follows:

[0188]

[0189]

[0190] IV) When a cycle block ends, the Damage_and_fatigue_life_evaluation subroutine calculates the damage growth rate of each element based on the stress and strain of this cycle block;

[0191] V) The element with the maximum damage growth rate is determined as the critical element, and its damage growth rate is determined as the critical damage growth rate, and is calculated using the following formula:

[0192]

[0193] where i is the loop block number and j is the unit number;

[0194] VI) The maximum damage increment ΔD of each loop block in the Damage_and_fatigue_life_evaluation subroutine is set to be the same, and the critical damage value is set to D C , and in this embodiment, the maximum damage increment is taken as ΔD = 0.05, and the critical damage value is taken as D C = 0.95;

[0195] VII) Dividing the maximum damage increment ΔD by the critical damage growth rate can obtain the actual number of cycles ΔN of the current loop block, which is calculated using the following formula:

[0196]

[0197] VIII) Multiplying the actual damage growth rate of each unit by the actual number of cycles ΔN can obtain the damage increment of each unit in the current loop block, which can be expressed by the following formula:

[0198]

[0199] IX) Further accumulating the damage increments of specific units can obtain the damage value of this unit, which can be calculated by the following formula:

[0200]

[0201] Ⅹ) By accumulating the actual number of cycles ΔN of each loop block, the number of cycles of the current component can be obtained, which can be expressed as follows:

[0202] N i+1 = N i + ΔN i (20)

[0203] XI) The material mechanical property parameters of the damaged unit can be updated according to the damage, which is calculated using the following formula:

[0204]

[0205] where is the current material parameter, is the yield limit of the damaged material degradation.

[0206] 6) When the maximum damage in all units reaches the critical damage value D CWhen it occurs, it can be regarded as crack initiation, and the Damage_and_fatigue_life_evaluation subroutine can be terminated. At this time, the actual number of cycles of the metal component is its fatigue life.

[0207] 7) View the damage distribution characteristics of the metal component through the Visualization module of ABAQUS to determine the dangerous area.

[0208] This embodiment is convenient and accurate, and simultaneously considers non-linear isotropic hardening / softening and kinematic hardening.

[0209] Example 3:

[0210] The main steps of this embodiment are the same as those of Example 2. Further, the metal plate with a semi-circular notch in step 1) can be replaced by any other form of metal component, and the 18CrNiMo7-6 material can also be replaced by other metal materials.

[0211] Example 4:

[0212] The main steps of this embodiment are the same as those of Example 2. Further, the number of state variables Depvar in step 2-1) can be adjusted according to actual needs.

[0213] Example 5:

[0214] The main steps of this embodiment are the same as those of Example 2. Further, in step 2-4), if the metal component is multiple components that cooperate with each other, corresponding contacts need to be defined in the Interaction module.

[0215] Example 6:

[0216] The main steps of this embodiment are the same as those of Example 2. Further, in step 2-6), for complex metal components, mesh independence analysis needs to be carried out to ensure the calculation accuracy.

[0217] Example 7:

[0218] The main steps of this embodiment are the same as those of Example 2. Further, in step b), for kinematic hardening, in order to better fit the stress-strain curve, the number of hardening moduli is usually defined as M = 3.

[0219] Example 8:

[0220] The main steps of this embodiment are the same as those of Example 2. Further, in step I), the damage can be defined as the ratio of the degraded elastic modulus E D to the initial elastic modulus E0, which is expressed by the following formula:

[0221]

[0222] Example 9:

[0223] The main steps of this example are the same as those of Example 2. Further, in step VI), the maximum damage increment and the critical damage value can be set to other values as needed, such as ΔD = 0.01, D C = 0.99.

[0224] Example 10:

[0225] The main steps of this example are the same as those of Example 2. Further, in step 7), the accumulated plastic strain (SDV13), damage (SDV38), equivalent stress (SDV39), plastic damage rate (SDV44), elastic damage rate (SDV56), number of cycles (SDV57), and von Mises stress (SDV76) of the metal component can be viewed through the Visualization module of ABAQUS.

Claims

1. A fatigue life assessment method for metal components considering elastoplastic damage based on secondary development of ABAQUS, characterized in that: It includes the following steps: 1) Establish the geometric model of the metal component: Use the Part module of ABAQUS to establish the geometric model of the metal component, or draw the 3D model of the metal component through drawing software and import it into ABAQUS software in STEP format; 2) Complete the preprocessing settings of the metal component model through ABAQUS software: 2-1) Based on the Property module of ABAQUS, define the material properties of the metal component and the number of state variables through UserMaterial and Depvar; 2-2) Complete the assembly of the metal component based on the Assembly module of ABAQUS; 2-3) Set the time step of the metal component simulation based on the Step module of ABAQUS, and set the state variable output in the FieldOutput module; 2-4) Set the contact characteristics of the metal component based on the Interaction module; 2-5) Set the load conditions and constraints of the metal component based on the Load module; 2-6) Complete the mesh division of the metal component based on the Mesh module; 2-7) Create a Job in the Job module, and select the subroutine Damage_and_fatigue_life_evaluation for evaluating the fatigue life of the metal component considering elastoplastic damage written in Fortran in the UserSubroutineFile; 3) Complete the construction of the elastoplastic constitutive model of the metal component based on the subroutine Damage_and_fatigue_life_evaluation: 3-1) The elastic stage of the metal component material is determined by the generalized Hooke's law; 3-2) The plastic stage of the metal component material is determined by nonlinear isotropic hardening / softening and kinematic hardening; 3-3) The Damage_and_fatigue_life_evaluation subroutine constructs the stiffness matrix by reading the material parameters defined in ABAQUS; 3-4) The Damage_and_fatigue_life_evaluation subroutine calculates the trial stress by reading the strain calculated in ABAQUS and according to the stiffness matrix; 3-5) Judge whether the component undergoes plastic deformation by comparing the trial stress and the transient yield strength; 3-6) When the component does not undergo plastic deformation, the trial stress is the true stress; 3-8) When the component undergoes plastic deformation, the Damage_and_fatigue_life_evaluation subroutine determines the plastic strain increment through the Newton iteration algorithm, further determines the plastic stress / strain according to the plastic flow criterion, and then calculates the stiffness matrix in the plastic stage through the consistent tangent modulus algorithm; 4) The Damage_and_fatigue_life_evaluation subroutine uses the cyclic jump algorithm to accelerate the calculation: In the Damage_and_fatigue_life_evaluation subroutine, one load cycle is regarded as an actual ΔN load cycle (i.e., a cycle block). Within the same cycle block, the stress-strain history of each cycle is regarded as the same, damage and life are not updated, and the life ΔN of each element is the same. 5) Damage and fatigue life assessment of metal components: 5-1) In the Damage_and_fatigue_life_evaluation subroutine, the total damage is defined as the sum of elastic damage and plastic damage, and the total damage growth rate is equal to the sum of the elastic damage growth rate and the plastic damage growth rate. 5-2) The elastic damage growth rate is determined by the octahedral shear stress, damage parameter, and damage variable. 5-3) The plastic damage growth rate is determined by the equivalent stress, material parameter, damage parameter, damage variable, and accumulated plastic strain. 5-4) When a cycle block ends, the Damage_and_fatigue_life_evaluation subroutine calculates the damage growth rate of each element according to the stress-strain of this cycle block. 5-5) The element with the maximum damage growth rate is determined as the critical element, and its damage growth rate is determined as the critical damage growth rate. In the Damage_and_fatigue_life_evaluation subroutine, the maximum damage increment ΔD for each loop block is set to be the same, and the critical damage value is set to D C ; 5-7) The actual number of cycles ΔN of the current cycle block can be obtained by dividing the maximum damage increment ΔD by the critical damage growth rate. 5-8) The damage increment of each element in the current cycle block can be obtained by multiplying the actual damage growth rate of each element by the actual number of cycles ΔN. 5-9) Further accumulating the damage increments of specific elements can obtain the damage value of this element. 5-10) The number of cycles of the current component can be obtained by accumulating the actual number of cycles ΔN of each cycle block. 5-11) The material properties of damaged elements can be updated according to the damage. 6) When the maximum damage in all units reaches the critical damage value D C it can be regarded as crack initiation, and the Damage_and_fatigue_life_evaluation subroutine can be terminated. At this time, the actual number of cycles of the metal component is its fatigue life; 7) View the damage distribution characteristics of metal components through the Visualization module of ABAQUS to determine the dangerous area.

2. A fatigue life assessment method for metal components considering elastoplastic damage based on secondary development of ABAQUS according to claim 1, characterized in that: The generalized Hooke's law described in step 3-1) is expressed as follows: where is the elastic strain, E and ν are the elastic modulus and Poisson's ratio respectively, and σ ij and σ kk are the stresses, D is the damage variable, and δ ij is the Kronecker symbol.

3. A method for evaluating the fatigue life of a metal component considering elastoplastic damage based on secondary development of ABAQUS according to claim 1, characterized in that: The nonlinear isotropic hardening / softening described in step 3-2) is calculated using the following formula: σ y = σ y0 + σ ym (1 - e -bΔp ) (2) where σ y is the transient yield limit, σ y0 is the initial yield limit, σ ym and b are the magnitudes and saturation rates of isotropic hardening / softening respectively, and Δp is the cumulative plastic strain, which can be obtained through uniaxial cyclic experiments; when the material is isotropic hardening, σ ym is positive; when the material is isotropic softening, σ ym is negative; under the influence of isotropic hardening / softening, the yield surface of the material expands or contracts equally in all directions; The nonlinear kinematic hardening is calculated using the following formula: where α ij is the back stress, M is the amount of the hardening modulus, C k and γ k are the kinematic hardening parameters, which can be obtained through uniaxial tensile tests, is the cumulative plastic strain rate, which is calculated by the following formula: where is the plastic multiplier, is the plastic strain rate, and is calculated using the following formula: where F is the yield function, S ij is the deviatoric stress component, and "eq" refers to the equivalent stress part.

4. A method for evaluating the fatigue life of a metal component considering elastoplastic damage based on secondary development of ABAQUS according to claim 1, characterized in that: In step 3-5), the following formula is used to judge whether plasticity occurs 5. A fatigue life assessment method for metal components considering elastoplastic damage based on secondary development of ABAQUS according to claim 1, characterized in that: The damage described in step 5-1) is represented by the ratio of the damaged area A D to the total area A: The total damage can be represented by the sum of the elastic damage D e and the plastic damage D p as follows: D = D e + D p (8) 6. A method for evaluating the fatigue life of metal components considering elastoplastic damage based on secondary development of ABAQUS according to claim 1, characterized in that: Step 5-2) The elastic damage rate dD e / dN is calculated using the following formula: where Δτ8 is the octahedral shear stress range, which is calculated using the following formula: where S ij,t and are the deviatoric stress components at times t and t0, respectively; The elastic damage parameter τ r and m can be calculated using the following formula: where τ f and B are fatigue parameters that can be obtained through a torsion test.

7. A method for evaluating the fatigue life of a metal component considering elastoplastic damage based on secondary development of ABAQUS according to claim 1, characterized in that: The plastic damage rate dD p / dN is calculated using the following formula: where σ max is the maximum equivalent stress, Δp is the cumulative plastic strain, q and S are plastic damage parameters, and are calculated using the following formulas:

8. A method for evaluating the fatigue life of metal components considering elastoplastic damage based on secondary development of ABAQUS according to claim 1, characterized in that: In step 5-9), the total damage of each element at the current moment can be calculated using the following formula: where i is the loop block number and j is the unit number, is the damage increment of each unit.

9. A method for evaluating the fatigue life of a metal component considering elastoplastic damage based on secondary development of ABAQUS according to claim 1, characterized in that: In step 5-10), the total life of each element at the current moment can be calculated using the following formula: N i+1 = N i + ΔN i (17) 10. A method for evaluating the fatigue life of metal components considering elastoplastic damage based on secondary development of ABAQUS according to claim 1, characterized in that: In step 5-11), the mechanical property parameters of the material can be updated using the following formula: Among them are the current material parameters is the yield limit of the damaged material degradation

Images