A method for simulating and analyzing strength of motor rotor lamination

Abstract

The present application relates to the technical field of motor rotor strength simulation, and particularly relates to a motor rotor lamination strength simulation analysis method, comprising: obtaining geometric models of each component of a rotor assembly and performing geometric processing, wherein the components include rotor laminations, magnetic steel and a rotor shaft; performing mesh division on the geometric models of the geometrically processed components to establish a rotor lamination strength finite element model; assembling the model based on predefined component connection relationships and defining material properties of each component; setting boundary conditions and loads, and defining static strength working conditions based on the boundary conditions and loads; performing solution calculation on the rotor lamination strength finite element model to obtain calculation results of the static strength working conditions, and generating rotor lamination strength analysis results according to the calculation results. The present application improves the strength calculation precision and simulation efficiency, and provides reliable basis for rotor lamination structure optimization design and lightweight.

Description

Technical Field

[0001] This application relates to the field of motor rotor strength simulation technology, and in particular to a method for simulation analysis of motor rotor lamination strength. Background Technology

[0002] The rotor laminations are the core force-transmitting and electromagnetic functional components of a drive motor. The rotor core is assembled from multiple layers of silicon steel laminations, supporting permanent magnets, balance plates, and other structures. It withstands the centrifugal loads generated by high-speed rotation and the torque transmitted by the shaft, thereby realizing the motor's energy conversion and power output to meet the performance requirements of the vehicle's power system. The rotor laminations are the most critical load-bearing component in the motor rotor assembly. Efficiently and accurately calculating their strength allows for timely optimization of the lamination structure design, which helps save R&D costs and shorten product development cycles.

[0003] In product design, two main techniques are typically employed to determine the strength of motor rotor laminations. The first is experimental techniques, which rely on physical prototypes and dedicated high-speed test benches. These methods have long testing cycles, lag behind product development, require the fabrication of multiple lamination samples and associated fixtures, resulting in high costs. Furthermore, they struggle to comprehensively cover multi-condition testing, including extreme speeds and high / low temperatures, thus failing to fully meet the needs of rapid product iteration. The second technique is simulation techniques. This involves building a finite element model of the rotor lamination strength and applying boundary conditions such as centrifugal loads and interference fit loads under rated operating conditions to perform simulation calculations and obtain the plastic strain distribution of the lamination structure. When the maximum plastic strain value is lower than the required material elongation threshold, the rotor lamination strength is considered to meet the requirements.

[0004] However, current calculations of rotor lamination strength have significant limitations. The analysis process generally ignores the effects of the material's plastic constitutive model and the interference fit between the lamination and the shaft. The linear elastic analysis assumptions have inherent limitations, and the effects of thermal stress and material property changes caused by temperature rise are not taken into account. Furthermore, the stress concentration effects of local features such as keyways, ventilation holes, and magnet slots further increase the difficulty of achieving fully parametric, refined modeling. Due to the combined effect of these factors, the rotor lamination strength results obtained using simplified models fluctuate significantly, resulting in low calculation accuracy.

[0005] For example, the paper "Motor Rotor Laminations and Their Simulation Verification Method" (CN120414954A) provides a method for simulating and verifying motor rotor laminations by establishing a finite element analysis model of rotor laminations. However, this method only uses linear elastic material constitutive model for simulation calculation and relies solely on the comparison between equivalent stress and preset performance thresholds for strength evaluation. It ignores the influence of stress redistribution and plastic deformation accumulation on the actual load-bearing capacity of the structure after the material yields and enters the plastic stage. The strength evaluation method is relatively simple, and the evaluation results deviate significantly from the actual mechanical behavior when the load is close to or exceeds the material yield limit.

[0006] The method provided by "A Strength Verification System for Motor Rotor Structure" (CN110736925A) is an experimental testing method. The testing cycle is long, and the cost of prototypes and tooling is high, which is not conducive to rapid verification of the scheme in the early stage of design, cost saving and shortening of the R&D cycle. Summary of the Invention

[0007] The purpose of this invention is to provide a simulation analysis method for the strength of motor rotor laminations, so as to solve the problems of low calculation accuracy, single strength evaluation method, and inability to truly consider the effects of elasto-plastic constitutive model and interference fit in the existing technology for rotor lamination strength simulation.

[0008] This invention provides the following solution: A simulation analysis method for the strength of motor rotor laminations includes: Obtain the geometric models of each component of the rotor assembly, and perform geometric processing on the geometric models of the components. The components of the rotor assembly include rotor laminations, magnets, and rotor shaft. Mesh the geometric model of the components after geometric processing, and establish a finite element model of rotor lamination strength; The rotor lamination strength finite element model is assembled based on the predefined component connection relationship, and the material properties of each component in the rotor lamination strength finite element model are defined. Set the boundary conditions and loads for the finite element model of the rotor lamination strength, and define the static strength condition based on the boundary conditions and loads; The rotor lamination strength finite element model is solved to obtain the calculation results of the static strength condition, and the rotor lamination strength analysis results are generated based on the calculation results.

[0009] In one optional implementation, the step of obtaining the geometric models of each component of the rotor assembly and performing geometric processing on the component geometric models includes: The geometric model of the rotor laminations, the magnets, and the rotor shaft is sliced ​​and cut so that the thickness of the sliced ​​geometric model is the thickness of a single layer of laminations. Based on the symmetrical characteristics of the rotor assembly, the geometric models of the rotor laminations, the magnets, and the rotor shaft after slicing are symmetrically cut. Using the contact area edge of the geometric model of the rotor laminations, the magnets, and the rotor shaft as a reference, the cutting is performed by translating a first preset distance along the normal direction of the contact area edge towards the non-contact area, so that a transition area is formed between the cutting line and the contact area edge.

[0010] In one optional implementation, the step of meshing the geometrically processed component geometric model and establishing a finite element model of the strength of each rotor lamination includes: Based on the symmetry characteristics of the rotor assembly, a hexahedral mesh of the 1 / 12 model is established, and a complete finite element model of the rotor lamination strength is established through symmetry. The mesh of the contact area of ​​the rotor laminations, the magnets and the rotor shaft is refined, the mesh of the non-contact area is coarsened, and the geometric surface enclosed by the edge line of the contact area and the cutting line is divided into a transition mesh to ensure the mesh quality of the transition area.

[0011] In one optional implementation, the mesh generation of the geometrically processed component geometric model further includes: Ensure that the grid nodes on the contact surfaces of the rotor laminations, the magnets, and the rotor shaft correspond one-to-one.

[0012] In one optional implementation, assembling the rotor lamination strength finite element model based on predefined component connection relationships includes: Based on the actual installation position of the rotor assembly, contacts are created between the rotor laminations and the rotor shaft, as well as between the rotor laminations and the magnets.

[0013] In one optional implementation, defining the material properties of each component in the rotor lamination strength finite element model includes: Define the density, elastic modulus, and Poisson's ratio of the rotor laminations, the magnets, and the rotor shaft; The magnet is defined as a linear elastic material; The rotor laminations and the rotor shaft are defined as elastoplastic materials. The nominal stress and strain data of the rotor laminations and the rotor shaft are converted into actual stress and plastic strain data, and respectively assigned to the rotor laminations and the rotor shaft in the finite element model of rotor lamination strength. When the plastic strain value of the rotor laminations or the rotor shaft is less than 1×10-5, the plastic strain value is taken as 0.

[0014] In one optional implementation, setting the boundary conditions and loads for the rotor lamination strength finite element model includes: The inner surface of the rotor shaft is fixed to simulate the interaction between the rotor shaft and the rotor laminations. When fixing the inner surface of the rotor shaft, constraints are applied using RBE3 units. The principal point of the RBE3 unit selects the element node of the inner surface of the rotor shaft, and the slave point selects the geometric center of the inner surface of the rotor shaft. All degrees of freedom of the slave point of the RBE3 unit are constrained.

[0015] In an optional implementation, setting the boundary conditions and loads for the rotor lamination strength finite element model further includes: A maximum radial interference load is applied to the contact surface between the rotor laminations and the rotor shaft. The overspeed centrifugal load is calculated based on the motor's maximum operating speed, and then applied to the rotor lamination strength finite element model.

[0016] In one optional implementation, defining the static strength condition based on the boundary conditions and the load includes: The static strength condition is composed of the boundary conditions of the inner surface of the fixed rotor shaft, the maximum single-sided interference load in the radial direction applied to the contact surface between the rotor laminations and the rotor shaft, and the overspeed centrifugal load calculated based on the highest operating speed of the motor.

[0017] In one optional implementation, the step of solving the finite element model of the rotor lamination strength to obtain the calculation results under static strength conditions, and generating rotor lamination strength analysis results based on the calculation results, includes: The finite element model of rotor lamination strength was solved using the ABAQUS / Standard solver. Select nodes at non-contact locations on the rotor laminations, extract the plastic strain values ​​of the nodes at the non-contact locations, and use the plastic strain values ​​of the nodes at the non-contact locations as the basis for static strength evaluation. When the maximum plastic strain value of the non-contact node is less than the material elongation, the strength of the rotor lamination is determined to meet the requirements; otherwise, the strength of the rotor lamination is determined to not meet the requirements.

[0018] The above scheme achieves the following beneficial technical effects: Obtaining and processing the geometric models of each component of the rotor assembly helps eliminate the adverse effects of local features on mesh quality, providing a suitable geometric basis for subsequent mesh generation. Meshing the geometrically processed component models and establishing a finite element model of rotor lamination strength enables refined modeling of the contact area, improving the calculation accuracy of critical regions. Assembling the model based on predefined component connection relationships and defining the material properties of each component allows for realistic simulation of the contact relationships between the rotor laminations, rotor shaft, and magnets, while considering the elasto-plastic constitutive properties of the materials, making it more consistent with actual stress conditions. Setting boundary conditions and loads and defining static strength conditions allows for simultaneous consideration of the combined effects of interference fit loads and overspeed centrifugal loads, realistically reproducing the stress state under high-speed conditions. Solving the model and generating rotor lamination strength analysis results yields high-precision plastic strain and deformation distribution, accurately evaluating rotor lamination strength and significantly improving the accuracy and engineering practicality of rotor lamination strength calculations. Attached Figure Description

[0019] Figure 1 A flowchart of a simulation analysis method for the strength of motor rotor laminations according to an embodiment of the present invention is shown; Figure 2 A schematic diagram of a rotor assembly structure according to an embodiment of the present invention is shown; Figure 3 A schematic diagram of a rotor assembly slice cutting according to an embodiment of the present invention is shown; Figure 4 A schematic diagram of the geometric cutting of various components according to an embodiment of the present invention is shown; Figure 5 A schematic diagram of the translational cutting of various components according to an embodiment of the present invention is shown; Figure 6 A schematic diagram of the grid division of the contact areas of each component according to an embodiment of the present invention is shown; Figure 7 A schematic diagram of the non-contact area grid division of each component according to an embodiment of the present invention is shown; Figure 8 A schematic diagram of an RBE3 unit established on the inner surface of a rotor shaft bore according to an embodiment of the present invention is shown.

[0020] Explanation of reference numerals in the attached figures: 1-Rotor laminations; 2-Magnet; 3-Rotor shaft; 4-Slice cutting surface; 5-RBE3 unit. Detailed Implementation

[0021] The technical solution of the present invention will now be clearly and completely described with reference to the accompanying drawings. Obviously, the described embodiments are only some, not all, of the embodiments of the present invention. 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.

[0022] The present invention will now be described in further detail with reference to the accompanying drawings and specific embodiments.

[0023] This invention provides a method for simulating and analyzing the strength of motor rotor laminations, referring to... Figure 1 The method includes the following steps S101-S105.

[0024] Step S101: Obtain the geometric models of each component of the rotor assembly and perform geometric processing on the component geometric models.

[0025] Reference Figure 2 The rotor assembly includes rotor laminations 1, magnets 2, and rotor shaft 3. Before conducting strength simulation analysis, geometric models of rotor laminations 1, magnets 2, and rotor shaft 3 are obtained. These geometric models can be CAD models or finite element preprocessing geometric models imported through preprocessing software.

[0026] The obtained geometric models of rotor lamination 1, magnet 2, and rotor shaft 3 are sliced ​​and cut respectively. (Refer to...) Figure 3 After slicing, the structural thickness of the geometric model is the thickness of a single-layer lamination, providing a geometric basis consistent with the actual structure for subsequent mesh generation and material property definition. In this embodiment, the thickness of the single-layer lamination is determined according to the thickness of the actual rotor lamination 1 silicon steel lamination, for example, it can be 0.3mm, 0.5mm, or other practically used lamination thicknesses.

[0027] Furthermore, based on the symmetry characteristics of the rotor assembly, the geometric models of the rotor laminations 1, magnets 2, and rotor shaft 3 after slicing are symmetrically cut. (Refer to...) Figure 4 Symmetrical cutting allows the axisymmetric features of the rotor assembly to be utilized, facilitating subsequent local modeling and grouping operations when defining material properties. The angle of symmetrical cutting can be determined based on the geometric features of the actual rotor assembly, such as the number of magnetic poles and slots. For example, for a 12-pole structure, a 1 / 12 sector can be cut out.

[0028] Furthermore, using the contact area edge of the geometric model of rotor laminations 1, magnets 2, and rotor shaft 3 as a reference, cutting is performed by translating a first preset distance along the normal direction of the contact area edge towards the non-contact area. (Refer to...) Figure 5 The cutting line is located within the non-contact area, forming a transition zone between it and the edge of the contact area. The first preset distance is 0.3 mm. This transition zone ensures the quality of the transition between the subdivided mesh in the contact area and the coarse mesh in the non-contact area during subsequent mesh generation, preventing abrupt changes in mesh size that could degrade mesh quality.

[0029] Step S102: Mesh the geometric model of the component after geometric processing and establish the finite element model of rotor lamination 1 strength.

[0030] Specifically, based on the symmetry characteristics of the rotor assembly, a hexahedral mesh of a 1 / 12 model can be established, and a complete finite element model of rotor lamination strength can be established through symmetric expansion. Using a 1 / 12 model for mesh generation can reduce the number of meshes and workload, while ensuring the consistency of the overall model.

[0031] During mesh generation, the contact area between rotor laminations 1, magnets 2, and rotor shaft 3 is meshed finely, while the non-contact area is meshed coarser. A transition mesh is then created for the geometric surface enclosed by the contact area edges and the cutting lines. (See also...) Figure 6 and Figure 7 The contact area is the region where the parts actually come into contact and fit together, and its stress gradient is relatively large. Therefore, it is necessary to refine the mesh to obtain higher accuracy. In contrast, the stress change in the non-contact area is relatively gentle, and a coarser mesh can be used to reduce the model size.

[0032] Furthermore, during the mesh generation process described above, it is ensured that the mesh nodes on the contact surfaces of rotor lamination 1, magnet 2, and rotor shaft 3 correspond one-to-one. Specifically, for the contact surfaces between rotor lamination 1 and rotor shaft 3, and between rotor lamination 1 and magnet 2, it is ensured that the two contacting surfaces have corresponding nodes at the same positions. This makes the contact calculation more stable and improves the solution accuracy when defining the contact relationships subsequently.

[0033] Step S103: Assemble the rotor lamination strength finite element model based on the predefined component connection relationship, and define the material properties of each component in the rotor lamination strength finite element model.

[0034] Specifically, based on the actual installation position of the rotor assembly, the contacts between rotor lamination 1 and rotor shaft 3, and between rotor lamination 1 and magnet 2, are created. Here, the contact between rotor lamination 1 and rotor shaft 3 is an interference fit, and the contact between rotor lamination 1 and magnet 2 is a mating contact between magnet 2 and magnet 2 slots. By creating these contact pairs, the components are assembled into a unified finite element model of rotor lamination 1 strength according to their actual installation relationships.

[0035] After assembly, define the material properties of each component in the finite element model of rotor lamination 1 strength.

[0036] Specifically, the density, elastic modulus, and Poisson's ratio of rotor laminations 1, magnets 2, and rotor shaft 3 are defined. These material mechanical parameters are primarily determined based on the measured results of standard uniaxial tensile tests; when no measured data is available, they can be selected by referring to national material standards and steel mill quality certificates. Density is used for subsequent centrifugal load calculations and mass matrix establishment, while elastic modulus and Poisson's ratio are used for the stress-strain relationship in the linear elastic stage.

[0037] Furthermore, magnet 2 is defined as a linear elastic material. Magnet 2 does not undergo significant plastic deformation under normal conditions, therefore it is not necessary to define its true stress-plastic strain relationship.

[0038] Furthermore, rotor lamination 1 and rotor shaft 3 are defined as elasto-plastic materials. Specifically, the nominal stress-strain data of rotor lamination 1 and rotor shaft 3 are converted into actual stress and plastic strain data, and assigned to rotor lamination 1 and rotor shaft 3 in the finite element model of rotor lamination 1 strength, respectively. During the conversion, when the plastic strain value of rotor lamination 1 or rotor shaft 3 is less than 1×10⁻⁶, the conversion is performed. 5 When the value of plastic strain is zero, the effect of the numerically small plastic strain on the calculation convergence and result stability is eliminated.

[0039] The nominal stress-strain data can be converted into actual stress and plastic strain data according to the following formulas (1) to (4): ; In the formula, For actual stress, To respond realistically, For nominal stress, In order to respond nominally, For plastic strain, Let E be the elastic strain and E be the elastic modulus. When the calculated plastic strain value is less than 1 × 10⁻⁶, the elastic strain is considered less than 1 × 10⁻⁶. 5 When the stress-plastic strain curves of rotor lamination 1 and rotor shaft 3 are obtained, they are directly set to 0. After obtaining the actual stress-plastic strain curves of rotor lamination 1 and rotor shaft 3, they are assigned to the corresponding finite element model.

[0040] Step S104: Set the boundary conditions and loads for the rotor lamination strength finite element model, and define the static strength condition based on the boundary conditions and loads.

[0041] Specifically, after completing the assembly and material definition, it is necessary to set boundary conditions and loads for the finite element model of rotor lamination 1 strength.

[0042] The boundary conditions are set as follows: the inner surface of the rotor shaft 3 is fixed to simulate the interaction between the rotor shaft 3 and the rotor laminations 1. When fixing the inner surface of the rotor shaft 3, constraints are applied using RBE3 elements. (Refer to...) Figure 8 The principal point of the RBE3 element is selected from the element nodes on the inner surface of the rotor shaft 3, and the slave point is selected from the geometric center of the inner surface of the rotor shaft 3. All degrees of freedom of the RBE3 element are constrained at the slave point. Through the RBE3 element, the degree of freedom constraints of the nodes on the inner surface of the rotor shaft 3 can be transferred to the geometric center point, thereby achieving uniform constraint on the inner surface.

[0043] The load setting process is as follows: apply a maximum radial interference load to the contact surface between rotor lamination 1 and rotor shaft 3. This load is used to simulate the interference fit between rotor lamination 1 and rotor shaft 3 in actual assembly; calculate the overspeed centrifugal load based on the highest operating speed of the motor, and apply the overspeed centrifugal load to the finite element model of the rotor lamination 1. The overspeed centrifugal load can be calculated using formula (5): ; In the formula, F is the overspeed centrifugal force load in N; m is the mass of the part in kg; r is the radius of gyration of the center of mass in meters; and n is the maximum operating speed of the motor in r / min. This centrifugal load is used to simulate the centrifugal force generated under overspeed rotation conditions.

[0044] After setting the boundary conditions and loads, a static strength condition is defined based on these conditions and loads. Specifically, the static strength condition is composed of the boundary conditions on the inner surface of the fixed rotor shaft 3, the maximum single-sided interference load in the radial direction applied to the contact surface between the rotor lamination 1 and the rotor shaft 3, and the overspeed centrifugal load calculated based on the motor's highest operating speed. This static strength condition is used to simulate the working state of the rotor lamination 1 under actual interference loads and overspeed centrifugal loads.

[0045] Step S105: Solve the finite element model of rotor lamination strength to obtain the calculation results of static strength condition, and generate rotor lamination strength analysis results based on the calculation results.

[0046] Specifically, the ABAQUS / Standard solver was used to solve the finite element model of rotor lamination 1 to obtain the calculation results under static strength conditions. These results include mechanical response information such as nodal displacements, element stresses, and plastic strains.

[0047] After obtaining the calculation results, it is necessary to select nodes at non-contact locations on rotor lamination 1, extract the plastic strain values ​​of these nodes, and use these values ​​as the basis for static strength evaluation. Using the plastic strain at non-contact locations for strength evaluation avoids the interference of local contact effects on the evaluation results.

[0048] The strength judgment criterion is as follows: when the maximum plastic strain value of the non-contact node is less than the material elongation, the strength of rotor lamination 1 is deemed to meet the requirements; otherwise, the strength of rotor lamination 1 is deemed not to meet the requirements. The material elongation can be obtained through a standard uniaxial tensile test or selected with reference to a material standard handbook. When the maximum plastic strain value reaches or exceeds the material elongation, it indicates that the lamination may experience local cracking or failure under this static strength condition, and the structure of rotor lamination 1 needs to be optimized or the material adjusted.

[0049] The motor rotor lamination strength simulation analysis method provided in this embodiment defines the contact nonlinear properties of each component by specifying the finite element mesh division rules of the motor rotor lamination, defining the boundary conditions on the inner surface of the rotor shaft, applying interference load and centrifugal load according to the actual operating conditions, simulating the mechanical evolution law of the lamination under high speed, defining the static strength calculation scenario, considering the correction effect of plastic deformation on stress redistribution after material yielding, and realistically reproducing the stress state of the rotor lamination at high speed, thus obtaining high-precision results of structural plastic strain and deformation distribution.

[0050] This embodiment uses a real geometric model of rotor laminations, rotor shaft, and magnets, and performs fine mesh processing on the contact areas of each component, assigning them different material elastic-plastic properties to minimize the calculation deviation from the real lamination structure, ensure mesh quality, and improve calculation accuracy.

[0051] In this embodiment, the rotor laminations, rotor shaft, and magnets are all modeled symmetrically. Each component is modeled using a hexahedral mesh, and face-to-face contact and interference contact are used to simulate the fit and contact relationship. This not only effectively ensures the calculation accuracy of the rotor lamination strength, but also shortens the preprocessing and solution calculation time and improves the simulation efficiency.

[0052] This embodiment provides a standardized and streamlined method for calculating the strength of motor rotor laminations, significantly reducing the problem of large deviations in calculation results caused by engineers' subjective judgment, reducing the time spent manually adjusting models and parameters, and improving simulation efficiency and result consistency. Rotor lamination strength calculation can be performed in the early stages of product development, supporting multiple rounds of structural optimization and improvement, enhancing structural mechanical performance and lightweighting, effectively ensuring the product passes testing on the first attempt, shortening the product development cycle, and reducing product development costs.

[0053] Obviously, the above embodiments of the present invention are merely examples for clearly illustrating the present invention, and are not intended to limit the implementation of the present invention. For those skilled in the art, other variations or modifications can be made based on the above description. It is impossible to exhaustively list all the implementation methods here. All obvious variations or modifications derived from the technical solutions of the present invention are still within the protection scope of the present invention.

Claims

1. A method for simulation analysis of the strength of motor rotor laminations, characterized in that, include: Obtain the geometric models of each component of the rotor assembly, and perform geometric processing on the geometric models of the components. The components of the rotor assembly include rotor laminations, magnets, and rotor shaft. Mesh the geometric model of the components after geometric processing, and establish a finite element model of rotor lamination strength; The rotor lamination strength finite element model is assembled based on the predefined component connection relationship, and the material properties of each component in the rotor lamination strength finite element model are defined. Set the boundary conditions and loads for the finite element model of the rotor lamination strength, and define the static strength condition based on the boundary conditions and loads; The rotor lamination strength finite element model is solved to obtain the calculation results of the static strength condition, and the rotor lamination strength analysis results are generated based on the calculation results.

2. The method for simulation analysis of motor rotor lamination strength according to claim 1, characterized in that, The process of obtaining geometric models of each component of the rotor assembly and performing geometric processing on the component geometric models includes: The geometric model of the rotor laminations, the magnets, and the rotor shaft is sliced ​​and cut so that the thickness of the sliced ​​geometric model is the thickness of a single layer of laminations. Based on the symmetrical characteristics of the rotor assembly, the geometric models of the rotor laminations, the magnets, and the rotor shaft after slicing are symmetrically cut. Using the contact area edge of the geometric model of the rotor laminations, the magnets, and the rotor shaft as a reference, the cutting is performed by translating a first preset distance along the normal direction of the contact area edge towards the non-contact area, so that a transition area is formed between the cutting line and the contact area edge.

3. The method for simulation analysis of motor rotor lamination strength according to claim 1, characterized in that, The process of meshing the geometrically processed component models and establishing finite element models for the strength of each rotor lamination includes: Based on the symmetry characteristics of the rotor assembly, a hexahedral mesh of the 1 / 12 model is established, and a complete finite element model of the rotor lamination strength is established through symmetry. The mesh of the contact area of ​​the rotor laminations, the magnets and the rotor shaft is refined, the mesh of the non-contact area is coarsened, and the geometric surface enclosed by the edge line of the contact area and the cutting line is divided into a transition mesh to ensure the mesh quality of the transition area.

4. The method for simulation analysis of motor rotor lamination strength according to claim 3, characterized in that, The mesh generation of the geometrically processed component geometric model also includes: Ensure that the grid nodes on the contact surfaces of the rotor laminations, the magnets, and the rotor shaft correspond one-to-one.

5. The method for simulation analysis of motor rotor lamination strength according to claim 1, characterized in that, The assembly of the rotor lamination strength finite element model based on predefined component connection relationships includes: Based on the actual installation position of the rotor assembly, contacts are created between the rotor laminations and the rotor shaft, as well as between the rotor laminations and the magnets.

6. The method for simulation analysis of the strength of motor rotor laminations according to claim 1, characterized in that, The definition of the material properties of each component in the rotor lamination strength finite element model includes: Define the density, elastic modulus, and Poisson's ratio of the rotor laminations, the magnets, and the rotor shaft; The magnet is defined as a linear elastic material; The rotor laminations and the rotor shaft are defined as elastoplastic materials. The nominal stress and strain data of the rotor laminations and the rotor shaft are converted into actual stress and plastic strain data, and respectively assigned to the rotor laminations and the rotor shaft in the finite element model of rotor lamination strength. When the plastic strain value of the rotor laminations or the rotor shaft is less than 1×10-5, the plastic strain value is taken as 0.

7. The method for simulation analysis of motor rotor lamination strength according to claim 1, characterized in that, The setting of boundary conditions and loads for the finite element model of the rotor lamination strength includes: The inner surface of the rotor shaft is fixed to simulate the interaction between the rotor shaft and the rotor laminations. When fixing the inner surface of the rotor shaft, constraints are applied using RBE3 units. The principal point of the RBE3 unit selects the element node of the inner surface of the rotor shaft, and the slave point selects the geometric center of the inner surface of the rotor shaft. All degrees of freedom of the slave point of the RBE3 unit are constrained.

8. The method for simulation analysis of the strength of motor rotor laminations according to claim 7, characterized in that, The setting of boundary conditions and loads for the rotor lamination strength finite element model also includes: A maximum radial interference load is applied to the contact surface between the rotor laminations and the rotor shaft. The overspeed centrifugal load is calculated based on the motor's maximum operating speed, and then applied to the rotor lamination strength finite element model.

9. The method for simulation analysis of the strength of motor rotor laminations according to claim 8, characterized in that, The definition of static strength conditions based on the boundary conditions and the loads includes: The static strength condition is composed of the boundary conditions of the inner surface of the fixed rotor shaft, the maximum single-sided interference load in the radial direction applied to the contact surface between the rotor laminations and the rotor shaft, and the overspeed centrifugal load calculated based on the highest operating speed of the motor.

10. The method for simulation analysis of the strength of motor rotor laminations according to claim 1, characterized in that, The finite element model of rotor lamination strength is solved to obtain the calculation results under static strength conditions, and the rotor lamination strength analysis results are generated based on the calculation results, including: The finite element model of rotor lamination strength was solved using the ABAQUS / Standard solver. Select nodes at non-contact locations on the rotor laminations, extract the plastic strain values ​​of the nodes at the non-contact locations, and use the plastic strain values ​​of the nodes at the non-contact locations as the basis for static strength evaluation. When the maximum plastic strain value of the non-contact position node is less than the material elongation, the strength of the rotor lamination is determined to meet the requirements; otherwise, the strength of the rotor lamination is determined to not meet the requirements.

Images