Wheel fatigue life prediction method based on impact damage transmission
By combining ANSYS explicit and static modules in simulation analysis, residual stress and deformation information after wheel impact tests are extracted, solving the problem of disconnect between impact and fatigue analysis in traditional methods, and realizing high-precision fatigue life prediction and design optimization.
Patent Information
- Authority / Receiving Office
- CN · China
- Patent Type
- Applications(China)
- Current Assignee / Owner
- YANCHENG INST OF TECH
- Filing Date
- 2026-01-15
- Publication Date
- 2026-06-09
AI Technical Summary
Existing technologies cannot effectively transfer the damage state of wheels after impact, such as plastic deformation and residual stress, to the fatigue analysis process as initial conditions, resulting in overly optimistic fatigue life predictions and potential safety hazards.
The ANSYS explicit dynamics module was used to simulate wheel impact tests. The residual stress tensor and the node number after deformation were extracted. Fatigue analysis was performed in conjunction with the ANSYS statics module. A finite element model including impact damage was established, fatigue test boundary conditions were applied, and static solutions and fatigue life prediction were performed.
It achieves high-precision fatigue life prediction, accurately reflects the performance changes of wheels in actual use, avoids experimental implementation problems caused by large deformation due to impact, and provides a reliable basis for wheel design optimization.
Smart Images
Figure CN122174358A_ABST
Abstract
Description
Technical Field
[0001] This invention belongs to the field of fatigue life prediction technology for automotive parts, specifically relating to a method for predicting wheel fatigue life based on impact damage transmission. Background Technology
[0002] As a critical safety component of automobiles, wheels must withstand the combined effects of impacts and fatigue loads from various road conditions during their service life. Current standards require wheel impact tests and wheel fatigue tests to evaluate their impact resistance and fatigue life. However, aluminum alloy wheels may be subjected to complex dynamic and static loads during actual use, especially impact loads during accidents, which may significantly alter their structural properties and thus affect their subsequent fatigue life.
[0003] Traditional methods of separate testing or independent simulation cannot accurately capture the impact of impact damage on subsequent fatigue performance, leading to overly optimistic fatigue life predictions and posing safety hazards. Current technologies lack effective means to accurately transfer post-impact damage states such as plastic deformation and residual stress as initial conditions to subsequent fatigue analysis processes. Furthermore, this condition typically occurs after a vehicle accident and has not received sufficient attention from wheel manufacturers and vehicle users, posing a significant safety risk. If wheel fatigue failure occurs during subsequent driving, it could result in serious harm to life and property.
[0004] Therefore, there is an urgent need for a wheel fatigue life prediction method based on impact damage transmission, which can comprehensively consider the sequential loading conditions of impact tests and fatigue tests to accurately predict the fatigue life of wheels after impact damage, and provide a theoretical basis for product design and optimization. Summary of the Invention
[0005] The purpose of this invention is to address the problem in the prior art of lacking an effective means to accurately transfer the damage state such as plastic deformation and residual stress after impact to the subsequent fatigue analysis process as initial conditions. This invention proposes a simulation analysis method that can simulate the fatigue performance of a wheel after experiencing wheel impact damage, thus solving the problem of predicting the fatigue life of a wheel after it has been subjected to impact damage during its service life.
[0006] The present invention provides a method for predicting wheel fatigue life based on impact damage transmission, comprising the following steps: Step 1: Obtain the wheel geometry model and, based on the ANSYS explicit dynamics module, establish a finite element model containing the wheel and impact hammer to simulate the wheel impact test process. Solve the model using the explicit dynamics module to obtain the plastic strain and stress results of the wheel after the impact. Step 2: Extract the global residual stress tensor and the node number after deformation from the stress results in Step 1 (since the wheel deforms after the impact, its node coordinates change, but the node number remains unchanged). Step 3: Import the plastic strain results obtained in Step 1 into the ANSYS statics analysis module, and use the residual stress tensor extracted in Step 2 as the initial condition, map it to the deformed nodes according to the node number, and input it into the ANSYS statics analysis module to jointly establish a wheel finite element model containing impact damage. Step 4: Apply the boundary conditions and fatigue loads of the wheel fatigue test to the finite element model of the wheel containing impact damage in Step 3, perform static solution, and obtain the stress results of the wheel under fatigue load considering impact damage. Step 5: Import the finite element model containing the wheel and impact hammer from Step 1 into the ANSYS statics analysis module. Using the same boundary conditions and fatigue loads as in Step 4, establish a finite element model of the wheel fatigue test without impact damage, and perform statics solution to obtain the stress results of the wheel fatigue test without impact damage. Step Six: Import the stress results obtained in Step Four and Step Five into two ANSYS nCode modules respectively. Combine the material SN curve and fatigue algorithm to predict fatigue life, output the fatigue life distribution of the wheel under two conditions, and compare and analyze them.
[0007] As a further preferred option, the wheel impact test is any one of the wheel 13° impact test, wheel 30° impact test, and wheel 90° impact test; the wheel fatigue test includes any one of the bending fatigue test, radial fatigue test, and biaxial fatigue test.
[0008] As a further preferred option, in step one, the finite element model of the impact hammer is created using the SpaceClaim 3D modeling module built into ANSYS. The finite element model of the impact hammer is placed 0.1 mm above the impact surface of the wheel finite element model, and the angle is adjusted according to the requirements of the wheel impact test method. The wheel is an existing model provided by the manufacturer.
[0009] As a further preferred option, in step one, during the wheel impact test, the properties of aluminum alloy material (corresponding to the wheel) and structural steel material (corresponding to the impact hammer) are created separately, and Poisson's ratio, density and Young's modulus coefficient are added to both. Stress-strain curves and SN curves are added separately for aluminum alloy material, and the material properties are assigned to the wheel and impact hammer respectively.
[0010] As a further preferred option, in step one, the surface-to-surface contact between the impact hammer and the wheel is defined as bonded contact, and the contact detection adopts the Trajectory algorithm.
[0011] As a further preferred option, in step one, the explicit dynamics module mesh is set to first-order explicit mesh by default, and second-order mesh cannot be used. In step three, the statics analysis module is set to second-order mechanical mesh by default. In order to ensure that the results of the explicit dynamics module can be directly mapped to the statics analysis module according to the node number, both the wheel and the hammer in the statics analysis module are set to first-order mechanical mesh, with the wheel mesh element size being 5mm and the hammer mesh element size being 10mm.
[0012] As a further preferred option, in step one, during the explicit dynamics solution process, mass scaling technology is used to control computational efficiency.
[0013] As a further preferred option, in step two, since the data connection line cannot directly transfer the stress results from the explicit dynamics module to the statics analysis module, it is necessary to export the residual stress tensor and the deformed node sequence file (file format .csv) from the explicit dynamics module. The residual stress tensor includes the normal stress σ. XX σ YY σ ZZ Shear stress τ XY τ YZ τ XZ The deformed node number and its corresponding residual stress tensor are input into the static analysis module through the external data module.
[0014] As a further preferred option, in step three, the plastic strain result refers to the wheel mesh model that has undergone plastic deformation. The data is directly transferred from the explicit dynamics module to the statics analysis module via the data connection line, serving as the input condition for the statics analysis module, without the need for further mesh generation.
[0015] As a further preferred option, in step three, the residual stress tensor is mapped to the deformed nodes according to the node number using ANSYS's Imported Load function.
[0016] As a further preferred option, in step four, the geometry and mesh of the punch need to be deleted to avoid affecting the subsequent bending fatigue test.
[0017] As a further preferred option, in step four, the material properties of the wheel fatigue test are directly shared with the material properties of the wheel impact test model via a data connection line.
[0018] As a further preferred option, in step five, in order to facilitate the comparison of wheel fatigue test results with and without impact damage, the wheel fatigue test model without impact damage adopts the same mesh as the finite element model before deformation of the wheel fatigue test model with impact damage (i.e., the mesh of the wheel impact test model), and the mesh is directly shared by data connection lines. The material properties are also shared, and the mesh model of the impact hammer finite element model is also deleted.
[0019] As a further preferred option, step six includes setting up fatigue analysis as follows: defining the load spectrum, inputting the material SN curve, using the Goodman model for mean stress correction, selecting the stress-life method as the fatigue algorithm, and using the Miner linear damage accumulation rule.
[0020] Compared with existing technologies, this invention accurately predicts the fatigue life of wheels after impact damage during service by simulating the sequential loading process of wheel impact and fatigue tests. Extracting the plastic deformation and stress results after the impact test as initial conditions more realistically reflects the performance changes of the wheel in actual use. This method proposes a complete analysis process, simulating the continuous process of "impact damage-fatigue verification," avoiding the experimental implementation problem of wheels being unable to be fixed on subsequent fatigue testing machines due to large impact deformation. This method achieves high-precision fatigue life prediction, providing a reliable basis for the design optimization of aluminum alloy wheels and the assessment of their fatigue life after impact. Attached Figure Description
[0021] Figure 1 This is a schematic diagram of the overall process of the present invention; Figure 2 This is a front view of the finite element model of the 13° impact test in an embodiment of the present invention; Figure 3 This is a bottom view of the finite element model of the 13° impact test in an embodiment of the present invention; Figure 4 This is a data transfer diagram of the finite element model in an embodiment of the present invention; Figure 5 This is a finite element model diagram of a bending fatigue test containing impact damage in an embodiment of the present invention; Figure 6 This is a finite element model diagram of the bending fatigue test without impact damage in an embodiment of the present invention; Figure 7 This is a bending fatigue life cloud diagram without impact damage in an embodiment of the present invention; Figure 8 This is a bending fatigue life cloud diagram containing impact damage in an embodiment of the present invention. Detailed Implementation
[0022] The technical solution of the present invention will be further described in detail below with reference to the accompanying drawings and examples.
[0023] Reference Figure 1 This embodiment involves a 13° wheel impact test and a bending fatigue test. This embodiment presents a simulation analysis method based on the 13° wheel impact test and bending fatigue test, including: Step 1: Obtain the wheel geometry model from the wheel manufacturer, and then establish a finite element model containing the wheel and impact hammer based on the ANSYS explicit dynamics module to simulate the 13° impact test process of the wheel and solve for the plastic strain and stress results of the wheel after the impact. Step 2: Extract the residual stress tensor of the entire wheel and the node number of the wheel after impact deformation from the solution results of Step 1. Step 3: Import the plastic strain results obtained in Step 1 into the ANSYS statics analysis module. Use the residual stress tensor extracted in Step 2 as the initial condition, map it to the deformed nodes according to the node number, and input it into the ANSYS statics analysis module to jointly establish a wheel model containing impact damage. Step 4: Apply the boundary conditions and fatigue loads of the wheel fatigue test to the wheel model containing impact damage in Step 3, perform static solution, and obtain the stress results of the wheel under fatigue load considering impact damage. Step 5: Import the finite element model containing the wheel and impact hammer from Step 1 into the new ANSYS statics analysis module. Using the same boundary conditions and fatigue loads as in Step 4, establish a finite element model of the wheel fatigue test without impact damage, and perform statics solution to obtain the stress results of the wheel fatigue test without impact damage. Step Six: Import the stress results obtained in Step Four and Step Five into two ANSYS nCode modules respectively. Combine the material SN curve and fatigue algorithm to predict fatigue life, output the fatigue life distribution of the wheel under two conditions, and compare and analyze them.
[0024] As described above, the present invention provides a simulation analysis method that can simulate the bending fatigue performance of a wheel after experiencing 13° impact damage, solving the problems of disconnect between impact and fatigue analysis and inaccurate fatigue prediction in traditional methods.
[0025] More specifically, the simulation analysis method involved in the examples of this invention includes the following steps.
[0026] Step 1: Obtain the wheel geometry model. Based on the ANSYS explicit dynamics module, establish a 13° impact test finite element model including the wheel and impact hammer, as shown below. Figure 2 , 3As shown, a represents the impact hammer, b represents the local coordinate system of the impact hammer, c represents the wheel, d represents the gravitational acceleration, e represents the displacement constraint of the impact hammer, and f represents the wheel fixation constraint for a 13° impact. A 400×150×20mm impact hammer model (i.e., impact hammer a) was created using the SpaceClaim 3D modeling module built into ANSYS. It was placed 0.1 mm above the wheel impact surface and rotated 13° according to the requirements of the 13° wheel impact test method. The material properties of aluminum alloy and structural steel were created separately. The density of the aluminum alloy material is 2700 kg / m³. 3 The Young's modulus is 71 GPa, the Poisson's ratio is 0.33, and the density of the structural steel is 650,000 kg / m³. 3 (The density of the structural steel is determined based on the modeling volume of the impact hammer (simplified model) and the mass of the impact hammer (actual model) provided by the wheel manufacturer.) Young's modulus is 210 GPa, Poisson's ratio is 0.3. Stress-strain curves and SN curves for gravitational acceleration are added separately for the aluminum alloy material. The properties of the two materials are assigned to the wheel and impact hammer respectively. The surface-to-surface contact between the impact hammer and the wheel is defined as bonded contact, and the contact detection uses the Trajectory algorithm. Since the explicit dynamics module's mesh defaults to a first-order explicit mesh and cannot use a second-order mesh, while the statics analysis module defaults to a second-order mechanical mesh, to ensure that the results from the dynamics module can be directly mapped to the statics analysis module according to the node number, both the wheel and the impact hammer are set to first-order mechanical meshes. The wheel mesh is single... The element size is 5mm, and the hammer mesh element size is 10mm. A local coordinate system (i.e., hammer local coordinate system b) is established for the hammer, with the hammer impact direction along the Y-axis. Initial conditions of a drop of 230mm and an impact velocity of 2.1239m / s are added to the hammer in the local coordinate system, with an impact time of 0.1s. Gravitational acceleration (i.e., gravitational acceleration d) is added to the wheel and hammer in the local coordinate system, with the impact direction along the gravitational acceleration direction. Five degrees of freedom of the hammer impact surface are constrained in the local coordinate system, and the degree of freedom of its impact direction is released (i.e., hammer displacement constraint e). A 13° impact wheel fixed constraint f is arranged on the wheel flange mounting surface, constraining six degrees of freedom. Mass scaling is added to the explicit dynamic solver to control computational efficiency. The 13° impact test process of the wheel is simulated, and the plastic strain and stress results of the wheel after the impact are obtained.
[0027] Step 2: Extract the residual stress tensor and the deformed node numbers over the entire wheel region from the solution results of Step 1. Since the data connection line cannot directly transfer the stress results from the explicit dynamics module to the statics analysis module, it is necessary to export the residual stress tensor (including the normal stress σ) from the explicit dynamics module. XX σ YY σ ZZShear stress τ XY τ YZ τ XZ The six components and the deformed node numbers (file format .csv), as shown in Table 1, are input into the statics analysis module through the external data module, as follows: Figure 4 As shown.
[0028] Table 1. Examples of some .csv files in embodiments of the present invention.
[0029] Step 3: Import the deformation results from the explicit dynamics module into the ANSYS statics analysis module. The deformation results from the explicit dynamics module (i.e., the wheel k after impact deformation) can be directly transferred via data connection lines as input conditions for the statics analysis module, such as... Figure 4 As shown; the geometry and mesh in the statics analysis module are obtained by the explicit dynamics module through the data connection line, and no further meshing is required; the residual stress tensor extracted in step two is used as the initial condition, and the six types of residual stress fields (i.e., residual stress tensor m) are mapped to the deformed nodes according to the node number using ANSYS's "Imported Load" function to establish a wheel model containing impact damage.
[0030] Step Four: As Figure 5 As shown, g is the cosine load in the Z direction, h is the sine load in the X direction, i is the remote point connection, j is the fixed constraint for wheel bending fatigue, k is the wheel after impact deformation, and l is the position of the wheel with large deformation (as shown in the figure). Figure 6 (Comparison of the non-impact wheel model), m is the residual stress tensor; a finite element model for bending fatigue test is established on the model in step three, and the impact hammer mesh model is deleted to avoid its influence on subsequent bending fatigue tests; the material properties of the bending fatigue test are directly shared with the material properties of the 13° impact test model through the data connection line; fixed constraints j for bending fatigue of the wheel are arranged on the six degrees of freedom of the inner flange plane of the wheel rim; two remote periodic bending moment loads with a distance of 1000mm are applied to the flange mounting surface (i.e., the bending moment load is connected to the wheel through the remote point connection i), with an amplitude of 5664N (given by the OEM) and a frequency of 1 / 24Hz (24 load steps are set to intuitively reflect the performance of the wheel in one cycle), namely the sine load (sine load h) in the X direction and the cosine load (cosine load g) in the Z direction; static solution is performed to obtain the stress results of the wheel under bending load considering impact damage.
[0031] Step 5: As Figure 6As shown, g is the cosine load in the Z direction, h is the sinusoidal load in the X direction, i is the remote point connection, j is the fixed constraint for wheel bending fatigue, and c is the wheel; to facilitate the comparison of bending fatigue test results with and without impact damage, the bending fatigue test model without impact damage uses the same mesh as the bending fatigue test model with impact damage before deformation (i.e., the mesh of the 13° impact test model), directly sharing the mesh using data connection lines, sharing material properties, and deleting the geometry and mesh of the impact hammer; using the same loads and boundary conditions as in step four, in Fixed constraints j for wheel bending fatigue are arranged on the inner flange plane of the wheel rim, constraining 6 degrees of freedom. Two remote periodic bending moment loads (connected to the wheel via remote point i) with an amplitude of 5664N and a frequency of 1 / 24Hz are applied to the flange mounting surface at a distance of 1000mm. These are a sine load (i.e., sine load h) in the X direction and a cosine load (i.e., cosine load g) in the Z direction. A finite element model of bending fatigue test without impact damage is established, and static solution is performed to obtain the stress results of bending fatigue test without impact damage.
[0032] Step Six: Import the stress results and 24 load steps obtained in Steps Four and Five into two ANSYS nCode modules respectively. Define the load spectrum (generate 24 load step signals based on the 24 load steps, and then concatenate them sequentially to form the load spectrum signal). Input the material SN curve (determined according to GB / T 4337—2015 "Metallic Materials Fatigue Test - Rotational Bending Method"). Use the Goodman model for mean stress correction, select the stress-life method as the fatigue algorithm, and use the Miner linear damage accumulation rule to predict fatigue life. Output fatigue life cloud maps for the wheel under two conditions. Figure 7 As shown, the bending fatigue life without impact damage is 4.344 × 10⁻⁶. 6 r; such as Figure 8 As shown, the bending fatigue life including impact damage is 3.554 × 10⁻⁶. 5 The fatigue life of this wheel was reduced by a factor of 12 after being subjected to a 13° impact load, indicating that impact damage has a significant impact on the wheel's bending fatigue life. Subsequent tests showed that the bending fatigue life without impact damage was 4,021,436 r, while the bending fatigue life with impact damage was 107,410 r, showing good agreement with the simulation predictions and validating the effectiveness of the simulation analysis method.
Claims
1. A method for predicting wheel fatigue life based on impact damage transmission, characterized in that, Includes the following steps: Step 1: Obtain the wheel geometry model and, based on the ANSYS explicit dynamics module, establish a finite element model containing the wheel and impact hammer to simulate the wheel impact test process. Solve the model using the explicit dynamics module to obtain the plastic strain and stress results of the wheel after the impact. Step 2: Extract the global residual stress tensor and the node number after deformation from the stress results in Step 1; Step 3: Import the plastic strain results obtained in Step 1 into the ANSYS statics analysis module, and use the residual stress tensor extracted in Step 2 as the initial condition, map it to the deformed nodes according to the node number, and input it into the ANSYS statics analysis module to jointly establish a wheel finite element model containing impact damage. Step 4: Apply the boundary conditions and fatigue loads of the wheel fatigue test to the finite element model of the wheel containing impact damage in Step 3, perform static solution, and obtain the stress results of the wheel under fatigue load considering impact damage. Step 5: Import the finite element model containing the wheel and impact hammer from Step 1 into the ANSYS statics analysis module. Using the same boundary conditions and fatigue loads as in Step 4, establish a finite element model of the wheel fatigue test without impact damage, and perform statics solution to obtain the stress results of the wheel fatigue test without impact damage. Step Six: Import the stress results obtained in Step Four and Step Five into two ANSYS nCode modules respectively. Combine the material SN curve and fatigue algorithm to predict fatigue life, output the fatigue life distribution of the wheel under two conditions, and compare and analyze them.
2. The wheel fatigue life prediction method based on impact damage transmission according to claim 1, characterized in that: The wheel impact test is any one of the following: wheel 13° impact test, wheel 30° impact test, and wheel 90° impact test; the wheel fatigue test includes any one of the following: bending fatigue test, radial fatigue test, and biaxial fatigue test.
3. The method for predicting wheel fatigue life based on impact damage transmission according to claim 1, characterized in that: In step one, the finite element model of the impact hammer is created using the SpaceClaim 3D modeling module built into ANSYS. The impact hammer finite element model is placed 0.1 mm above the impact surface of the wheel finite element model, and the angle is adjusted according to the requirements of the wheel impact test method.
4. The wheel fatigue life prediction method based on impact damage transmission according to claim 1, characterized in that: In step one, during the wheel impact test, aluminum alloy material properties are created for the wheel and structural steel material properties are created for the impact hammer. Poisson's ratio, density, and Young's modulus are added to both. Stress-strain curves and SN curves are added to the aluminum alloy material, and the material properties are assigned to the wheel and the impact hammer respectively.
5. The method for predicting wheel fatigue life based on impact damage transmission according to claim 1, characterized in that: In step one, the explicit dynamics module mesh is set to first-order Explicit mesh by default. In step three, the wheel and hammer in the statics analysis module are set to first-order Mechanical mesh, with the wheel mesh cell size being 5mm and the hammer mesh cell size being 10mm.
6. The method for predicting wheel fatigue life based on impact damage transmission according to claim 1, characterized in that: In step two, the residual stress tensor and the deformed node number file are exported from the explicit dynamics module. The residual stress tensor includes the normal stress σ. XX σ YY σ ZZ Shear stress τ XY τ YZ τ XZ The deformed node number and its corresponding residual stress tensor are input into the static analysis module through the external data module.
7. The wheel fatigue life prediction method based on impact damage transmission according to claim 1, characterized in that: In step three, the plastic strain results are transferred from the explicit dynamics module to the statics analysis module via a data connection line, serving as the input conditions for the statics analysis module.
8. The method for predicting wheel fatigue life based on impact damage transmission according to claim 1, characterized in that: In step three, the residual stress tensor is mapped to the deformed nodes according to the node number using ANSYS's Imported Load function.
9. The method for predicting wheel fatigue life based on impact damage transmission according to claim 1, characterized in that: In step four, the material properties of the wheel fatigue test are shared with the material properties of the wheel impact test model via a data connection line.
10. The method for predicting wheel fatigue life based on impact damage transmission according to claim 1, characterized in that: In step five, the fatigue test model of the wheel without impact damage uses the same mesh as the finite element model of the fatigue test model of the wheel with impact damage before deformation. The mesh is shared by data connection lines and material properties are shared. The mesh model of the impact hammer finite element model is deleted.