Structural optimization method for prolonging fatigue life of crankshaft of marine diesel engine

Abstract

The invention discloses a structure optimization method for prolonging the fatigue life of a crankshaft of a marine diesel engine. The structure optimization method comprises the following steps: developing a single-throw crankshaft modeling analysis plug-in; design parameters are selected, a three-dimensional geometric model of the single-throw crankshaft is dynamically constructed, and finite element analysis is carried out; developing a graphical interface for the dialog box script; seamless connection between the plug-in and the ABAQUS software is realized through development of the registration script; adopting optimal Latin hypercube sampling in a defined range to obtain a pre-calculation sample, developing a batch processing file and a Python script, and using an instruction to drive a single-throw crankshaft modeling analysis plug-in; a Pareto graph is adopted to analyze parameter sensitivity, a pre-calculation sample is screened, a high-precision Kriging proxy model is built, and then the optimal maximum bending stress value of the single-throw crankshaft and the corresponding optimal structure size are searched in combination with a particle swarm algorithm. According to the invention, the problem of low efficiency caused by frequent man-machine interaction when large samples are processed in the prior art is solved.

Description

Technical Field

[0001] The present invention relates to the technical field of crankshaft size optimization, and in particular to a structural optimization method for improving the fatigue life of a marine diesel engine crankshaft. Background Art

[0002] Since marine diesel engine crankshafts are subjected to a variety of complex loads in a complex working environment and due to their special structural characteristics, fatigue life analysis usually relies on simulation and experimental verification. Although fatigue verification experiments on marine diesel engine crankshafts have high accuracy, they usually take several days or even longer to complete. The finite element analysis method has become a common means of fatigue life assessment because it can realize numerical visualization of temperature, stress, and deformation, and can accurately simulate and calculate the stress magnitude and fatigue life of the crankshaft during the design phase. However, the existing technology still has the following problems in the research on fatigue optimization of traditional marine medium-speed diesel engine crankshafts:

[0003] (1) When dealing with large quantities of similar samples, the traditional finite element analysis method is inefficient due to the repetitive operations of modeling and parameter setting, making it difficult to meet the rapid iteration requirements in engineering design.

[0004] (2) Existing crankshaft fatigue optimization research mostly relies on a single finite element analysis software and lacks support for multi-software collaborative calculations;

[0005] (3) In the crankshaft fatigue optimization process, traditional methods often ignore the dimensional coordination and dynamic influence of adjacent components, resulting in the optimization results possibly triggering the need to redesign other components.

[0006] Therefore, the above problems need to be solved urgently. Summary of the Invention

[0007] Purpose of the invention: The purpose of the present invention is to provide a structural optimization method for improving the fatigue life of a marine diesel engine crankshaft. This method can address the complexity of the crankshaft structure and the large number of sample calculations required for fatigue life analysis, thereby solving the problem of low efficiency of traditional finite element methods when processing large samples due to frequent human-computer interaction.

[0008] Technical solution: To achieve the above objectives, the present invention discloses a structural optimization method for improving the fatigue life of a marine diesel engine crankshaft, comprising the following steps:

[0009] (1) Develop a single-throw crankshaft modeling and analysis plug-in to implement parametric modeling and bending stress analysis based on the ABAQUS API;

[0010] (1.1) Select the design parameters of the single-throw crankshaft modeling and analysis plug-in, which include six structural dimension parameters, material parameters, and finite element analysis setting parameters;

[0011] (1.2) Dynamically construct a three-dimensional geometric model of a single-throw crankshaft based on design parameters and perform finite element analysis, and generate a kernel code;

[0012] (1.3) Develop a graphical interface for the plug-in dialog script using the Tkinter library. The graphical interface integrates the design parameter input, the single-throw crankshaft 3D geometry model, and the finite element analysis parameter module;

[0013] (1.4) Achieve seamless integration of the single-throw crankshaft modeling and analysis plug-in with the ABAQUS software main program through the development of a registration script. That is, through modular development and object-oriented programming, the core code of the single-throw crankshaft modeling and analysis plug-in and the functions of the dialog script are encapsulated in a unified operation interface;

[0014] (2) Use optimal Latin hypercube sampling to obtain pre-calculated samples within the defined range, develop batch processing files and Python scripts, and use command-driven single-bend crankshaft modeling and analysis plug-in to obtain the maximum bending stress value of each pre-calculated sample;

[0015] (3) The Pareto chart is used to analyze the parameter sensitivity, the pre-calculated samples are screened to form training samples, a high-precision Kriging proxy model is built, and then the particle swarm algorithm is combined to find the minimum maximum bending stress value of the single-bend crankshaft and the corresponding optimal structural size in the design space.

[0016] Optionally, the structural dimension parameters in the step (1.1) are selected from the six structural dimension parameters that have the greatest impact on the bending stress in the single-throw crankshaft, the six structural dimension parameters including the crank pin diameter D1, the crank pin length L1, the crank pin fillet radius R1, the main journal diameter D2, the main journal length L2 and the main journal fillet radius R2; the material parameters include material density, elastic modulus and Poisson's ratio; the finite element analysis setting parameters include incremental step, load parameter, mesh size and finite element operation naming.

[0017] Optionally, the crank and crank pin parts in step (1.2) are specifically modeled as follows:

[0018] Define the Z-axis symmetry plane of the single-throw crankshaft as the XY reference plane, and the X-axis symmetry plane of the single-throw crankshaft as the YZ reference plane;

[0019] Using the XY datum plane as the sketch plane, draw six positioning circles of part size within the sketch plane. Parts 2, 3, and 4 should be mirrored on the axis where the centers of parts 1 and 5 are located. The size of the positioning circles is determined by the size of the crankshaft crank. Based on the shape of the crank-crankpin connection surface of the single-throw crankshaft, trim off the excess line segments to obtain the crank-crankpin connection surface. Then, axially stretch the obtained crank-crankpin connection surface. The stretching length is determined by the distance from the crankpin center to the crank-main journal connection surface. The stretching direction is opposite to the Z axis.

[0020] Use the XY datum plane as the sketch plane, and draw the crankpin circle and the cutting circle on the sketch plane. The center of the cutting circle should coincide with the center of the crankpin circle. The radius should be greater than the distance from the center of the crankpin circle to the lowest point of the crank-crankpin connection surface in the Y direction. The area between the two circles is the cutting area, and the extrusion is performed with a length of half the crankpin length. Use the YZ datum plane as the sketch plane for the bevel section of the crank top, draw the bevel section of the crank top, and then perform a rotational cut around the center axis of the main journal. The cutting angle and direction parameters are determined according to the design requirements of the crankshaft crank.

[0021] Use the crank-crankpin connection surface as the sketch plane, and draw the crankpin boss circular surface on the sketch plane. The center of the boss circular surface coincides with the center of the crankpin circular surface. The radius is determined according to the actual size of the boss circular surface. The area between the crankpin circular surface and the boss circular surface is the stretching area. Create the boss part of the crankpin through stretching operation. The stretching length is the height of the boss.

[0022] Optionally, the spindle neck position modeling in step (1.2) is specifically as follows:

[0023] Use the crank-main journal connection surface as the sketch plane, and draw a circle on the sketch plane as the cross-section sketch of the main journal. The radius of the circle is determined by the radius of the main journal. Then perform an extrusion operation, and the extruded thickness is the length of the main journal.

[0024] Use the crank-main journal connection surface as the sketch plane and draw the main journal boss circular surface on the sketch plane. The center of the boss circular surface coincides with the center of the main journal circular surface. The radius is determined based on the actual size of the boss circular surface. The area between the main journal circular surface and the boss circular surface is used as the extrusion area. Create the main journal boss part through extrusion operation. The extrusion length is the height of the boss.

[0025] Using the YZ datum plane as the sketch plane, draw a circular sketch on the sketch plane to create the main journal oil hole. Use an extrude and cut operation to form the main journal oil hole. The size of the circle is determined by the main journal oil hole radius, and the extrude and cut length must completely penetrate the main journal oil hole. Save the sketch after completion. Then copy the previously saved main journal oil hole sketch on another sketch plane, use an extrude and cut operation to form the other side of the main journal oil hole, and fillet the edge of the main journal oil hole.

[0026] The crankpin mid-axis surface of the crankshaft is used as the mirror plane to mirror the part, and the original part is retained; at the same time, the crankpin, crankpin boss, main journal, and main journal boss of the crankshaft are chamfered, and the size of the fillet is determined according to the actual crankshaft fillet radius.

[0027] Optionally, the specific steps of performing finite element analysis in step (1.2) are:

[0028] Obtain material parameters through querying and define them in the single-throw crankshaft 3D geometric model. The material parameters include material density, elastic modulus, and Poisson's ratio. Create a homogeneous solid section in the material assignment module and assign the defined material properties to the entire area of the crankshaft component through the created homogeneous solid section. Then, import the created single-throw crankshaft 3D geometric model into the assembly.

[0029] In the analysis step module, first create a static analysis step and select the Static-General analysis step. Based on the interaction definition, create a reference point in the assembly. Use coupling constraints to associate the reference point with the left and right end faces of the single-throw crankshaft main journal to define the interaction relationship in the model. Apply a concentrated force load to the reference point of the assembly to calculate the nominal bending moment of the single-throw crankshaft. The nominal bending moment is the maximum bending moment the crankshaft can withstand during operation. Convert the bending moment into a load. Then, in the finite element model, constrain the nodes used for the clamping end to the center point using a coupling mode. Then, apply an axial load along the cylindrical surface of the single-throw crankshaft main journal. A fixed constraint is applied to the right surface of the single-throw crankshaft main journal, fixing all nodes on the right side of the main journal. After setting the loads and constraints, mesh the crankshaft and set the appropriate mesh size. Generate a suitable mesh by setting mesh control, selecting the element type, and adjusting the seed size parameters. Select the weakest node of the crankshaft to create an output node set. Create a job and set the job name, model, and type parameters. After all settings are completed, submit the job for finite element analysis.

[0030] Optionally, the graphical interface in step (1.3) is divided into two modules according to function, namely, a "Model" module and a "Pre" module; the "Model" module is divided into two areas, the left "Structural Parameter" area contains six structural parameters: crankpin diameter D1, crankpin length L1, crankpin fillet radius R1, main journal diameter D2, main journal length L2, and main journal fillet radius R2; the right "Crankshaft" area contains a schematic diagram marking the position of each structural dimension in the single-throw crankshaft;

[0031] The "Pre" module is divided into six areas according to different functions. The "Material" area contains three material parameters: mass density, Young's modulus and Poisson's ratio; the "Step" area contains an input box for setting the incremental step size; the "Load" area is used to enter the set bending load size; the "Mesh" area is used to enter the mesh size; the "Job" area is used to name a finite element analysis; the "Stress Display" area covers a schematic diagram of the position where the bending load is applied in a single-throw crankshaft.

[0032] Optionally, the specific method of optimal Latin hypercube sampling in step (2.1) is:

[0033] Determine the number of parameters that need to be sampled and the value range of each parameter, divide the value range of each parameter into a corresponding number of intervals according to the number of sampling points, and ensure that each interval has equal probability; randomly select a sample point in each interval to form an initial Latin hypercube sample set; the sample points are evenly distributed in each parameter space, and the initial Latin hypercube sample set is optimized and adjusted by minimizing the distance metric between sample points. During the optimization process, a simulated annealing optimization algorithm is used to continuously try to adjust the position of the sample points until the set optimization goal is achieved, thereby obtaining the optimal Latin hypercube sample set that meets the optimization criteria.

[0034] Optionally, step (2) includes the following specific steps:

[0035] (2.1) Six structural dimension parameters are selected as the design variables of the single-throw crankshaft. The variable constraint ranges of the single-throw crankshaft design variables are determined based on the tolerance ranges between the various dimensions. Optimal Latin hypercube sampling is used within the variable constraint ranges of the six design variables to obtain several sets of pre-calculated samples, each set of pre-calculated samples including six design variable values.

[0036] (2.2) The instruction drives the single-bend crankshaft modeling and analysis plug-in to perform finite element analysis to obtain the maximum bending stress values of the single-bend crankshaft corresponding to several groups of pre-calculated samples.

[0037] Optionally, step (3) includes the following specific steps:

[0038] (3.1) The sensitivity of the structural parameters is analyzed using a Pareto chart. The main journal diameter D2 and main journal length L2 are removed from several sets of pre-calculated samples to form training samples. The training samples include the four structural parameters and the maximum bending stress value of the single-throw crankshaft.

[0039] (3.2) Build a Kriging proxy model and use the data set composed of training samples to build the Kriging proxy model. The input of the Kriging proxy model is 4 structural parameters. The output of the Kriging proxy model is the maximum bending stress value of the single crankshaft. The determination coefficient R is used to calculate the maximum bending stress of the single crankshaft. 2 Evaluate the accuracy of the Kriging surrogate model, i.e. R 2 Is it close to 1? 2 When R<0.95, increase the sample size and retrain the Kriging surrogate model until R 2 ≥0.95;

[0040] (3.3) The particle swarm optimization algorithm is used to find the minimum single-turn crankshaft maximum bending stress value and the corresponding optimal structural dimensions in the design space. The optimal structural dimensions are input into the single-turn crankshaft modeling and analysis plug-in, where the main journal diameter D2 and the main journal length L2 are set as the initial values. The corresponding maximum bending stress value is obtained and compared with the maximum bending stress value obtained by optimization to calculate the error. If the error is within 1%, the current optimal structural dimension parameters are output; if the error value is greater than 1%, the relevant parameters of the particle swarm optimization algorithm are adjusted, and the particle swarm optimization algorithm is reused to find the optimal output response in the Kriging proxy model until the error is less than 1%.

[0041] Optionally, in the step (3.1), a Pareto chart is used to analyze the sensitivity of the structural parameters to obtain that the crankpin fillet radius R1, the main journal diameter D2 and the main journal length L2 have a negative effect on the fatigue life of the crankshaft, among which the negative effect of the crankpin fillet radius R1 is the largest, and the negative effects of the main journal diameter D2 and the main journal length L2 are smaller, and the main journal diameter D2 and the main journal length L2 are eliminated; the crankpin diameter D1, the crankpin length L1 and the main journal fillet radius R2 have a positive effect on the fatigue life of the crankshaft.

[0042] Beneficial effects: Compared with the prior art, the present invention has the following significant advantages: the present invention adopts a crankshaft fatigue life optimization method that combines parametric modeling and instruction-driven finite element method, which can calculate the large number of samples required for the complexity of the ship diesel engine crankshaft structure and fatigue life analysis, and solve the problem of low efficiency of traditional finite element method when processing large samples due to frequent human-computer interaction; the present invention uses structural parametric modeling and instruction-driven finite element method to achieve rapid modeling, automatic assignment of material properties, mesh generation and rapid realization of crankshaft bending analysis, significantly improving calculation efficiency and reducing manual operation time; the parametric modeling of the present invention combined with the instruction-driven finite element method can achieve seamless docking of multiple software, and realize full-process calculation and analysis through automated scripts, especially in the case of structural diversity and dynamic load complexity, and can better adapt to the complex working conditions of the crankshaft; the present invention uses parametric modeling and instruction-driven finite element method to simultaneously consider the collaborative design of the crankshaft and adjacent components during the optimization process, ensure the integrity and compatibility of the optimization scheme, thereby reducing the need for subsequent design adjustments; the present invention takes into account the two key issues of complex stress conditions during crankshaft operation and dimensional matching during optimization, and improves the accuracy of structural optimization. BRIEF DESCRIPTION OF THE DRAWINGS

[0043] Figure 1 Schematic diagram of the crankshaft model in the present invention;

[0044] Figure 2 This is a schematic diagram of the staggered angles of the cranks in the present invention;

[0045] Figure 3 Schematic diagram of a single-throw crankshaft model in the present invention;

[0046] Figure 4 This is the ABAQUS secondary development flow chart in the present invention;

[0047] Figure 5 This is a schematic diagram of the interface of the parameterized model of the L6 single-throw crankshaft in the present invention;

[0048] Figure 6 Schematic diagram of the modeling part of the single-throw crankshaft in the present invention Figure 1 ;

[0049] Figure 7 Schematic diagram of the modeling part of the single-throw crankshaft in the present invention Figure 2 ;

[0050] Figure 8 Schematic diagram of load boundary conditions for finite element analysis in the present invention;

[0051] Figure 9 Schematic diagram of mesh division for finite element analysis in the present invention;

[0052] Figure 10 Schematic diagram of simulation results of finite element analysis in the present invention;

[0053] Figure 11 SN curve diagram of 34CrNi3MoA in the present invention;

[0054] Figure 12 This is a flow chart of the present invention using ABAQUS combined with ISIGHT instruction drive;

[0055] Figure 13 The Pareto diagram of the six structural dimensions of the L6 crankshaft in the present invention;

[0056] Figure 14 Schematic diagram of error analysis of the sample set by the Kriging proxy model in the present invention;

[0057] Figure 15 It is a schematic diagram of the iteration curve and optimal parameter verification of the particle swarm optimization algorithm in the present invention. DETAILED DESCRIPTION

[0058] The technical solution of the present invention will be further described below with reference to the accompanying drawings.

[0059] The present invention discloses a structural optimization method for improving the fatigue life of a marine diesel engine crankshaft, comprising the following steps:

[0060] (1) Figure 4As shown in the figure, a plug-in for modeling and analysis of the L6 single-throw crankshaft was developed, implementing parametric modeling and rapid bending stress analysis based on the ABAQUS API. During the development process, the structural characteristics of the L6 single-throw crankshaft were analyzed to accurately identify key structural dimensional parameters and material performance parameters, laying the foundation for the plug-in's functionality. The plug-in utilizes the ABAQUS API to achieve parametric modeling of the crankshaft model. Users can flexibly input and adjust model parameters through the plug-in interface. The plug-in also features rapid stress analysis capabilities that automatically generate loading conditions and perform finite element calculations.

[0061] like Figure 1 、 Figure 2 and Figure 3 As shown in the figure, the test object is a CHD416 L6 crankshaft with a specification of Φ115×300mm and a material of 34CrNi3MoA steel. The L6 crankshaft consists of six crank throws, a front shaft, and a rear shaft, which are symmetrically distributed along the axial center plane. Each crank throw consists of two symmetrical cranks and crankpins, and each crank throw is staggered by 120°. During diesel engine operation, the actual operating conditions of each crank throw are less affected by the adjacent crank throws. To save calculation time and cost, a single-throw crankshaft model is selected for finite element analysis.

[0062] The secondary development process of the L6 single-throw crankshaft modeling and analysis plug-in in ABAQUS involves several key steps, aiming to achieve functional expansion and interface parameterization through kernel code, dialog scripts, and registration scripts. As the core of the plug-in, the kernel code directly interacts with the underlying calculation engine of ABAQUS to define basic simulation components such as the crankshaft's structural model, material properties, loading conditions, and boundary conditions. The parametric development of the L6 single-throw crankshaft modeling and analysis plug-in requires writing an application programming interface (API) to achieve model generation, material property definition, and loading condition setting. For example, when modeling the main journal, it is necessary to create a circular contour through the kernel code and stretch it by projecting it onto the sketch to form the three-dimensional structure of the main journal. The kernel code needs to interact closely with the underlying calculation engine of ABAQUS to ensure the accuracy of the simulation results.

[0063] In terms of interface parameterization, dialog scripts are used to provide a user-friendly interactive interface, allowing users to customize the crankshaft geometry and simulation settings by inputting parameters. Dialog scripts are usually written in Python and are used to automate the graphical user interface (GUI) operations of ABAQUS. The interface development of the L6 single-throw crankshaft modeling and analysis plug-in requires the creation of command objects and the definition of corresponding parameters for them. For example, commands are defined by creating AFXGuiCommand objects, and floating numerical parameters such as D1 are defined using tools such as AFXFloatKeyword. Dialog scripts allow users to control the modeling process by inputting parameters through the GUI without directly writing code, such as setting parameters such as the journal diameter and length, thereby realizing operations such as model creation, material property settings, and boundary condition definitions.

[0064] To integrate custom functionality into ABAQUS, you need to write a registration script. This script is automatically executed when ABAQUS starts up and is used to register custom plug-ins, set environment variables, define shortcuts, or add custom buttons to the toolbar. For example, you can create a GroupBox to organize parameter input and use a VerticalAligner to enhance the interface layout. By customizing ABAQUS's initialization behavior through a registration script, custom plug-ins are automatically loaded at software startup, providing a more convenient user experience.

[0065] By expanding the functionality of the kernel code, designing a parameterized interface for dialog scripts, and customizing initialization behavior for registration scripts, developers can implement a parameterized interface for the L6 single-throw crankshaft modeling and analysis plug-in, thereby simplifying the crankshaft modeling and simulation process and improving work efficiency.

[0066] (1.1) Select the design parameters of the single crankshaft modeling analysis plug-in

[0067] The design parameters of the single-throw crankshaft modeling and analysis plug-in include structural size parameters, material parameters, and finite element analysis setting parameters;

[0068] The six structural dimension parameters that have the greatest impact on bending stress in a single-throw crankshaft are selected as the structural dimension parameters. The six structural dimension parameters include crankpin diameter D1, crankpin length L1, crankpin fillet radius R1, main journal diameter D2, main journal length L2, and main journal fillet radius R2.

[0069] Material parameters include material density, elastic modulus, and Poisson’s ratio;

[0070] Finite element analysis setting parameters include increment step, load parameters, mesh size and finite element operation naming;

[0071] (1.2) Dynamically construct a three-dimensional geometric model of the crankshaft based on the structural dimensions and finite element analysis parameters and perform finite element analysis;

[0072] (1.2.1) Figure 6 and Figure 7 As shown in the figure, the three-dimensional geometric model of the L6 single-throw crankshaft includes the modeling of the crank and crankpin parts and the main shaft neck part.

[0073] The modeling of the crank and crank pin includes the following steps:

[0074] The Z-axis symmetry plane of the single-throw crankshaft is defined as the XY reference plane, and the X-axis symmetry plane of the single-throw crankshaft is defined as the YZ reference plane.

[0075] Take the XY datum plane as the sketch plane, and draw positioning circles of six part sizes in the sketch plane. Parts 2, 3, and 4 should be mirrored on the axis where the centers of parts 1 and 5 are located. The size of the positioning circle is determined according to the size of the crankshaft crank; according to the shape of the crank-crankpin connection surface of the single-throw crankshaft, cut off the redundant line segments to obtain the crank-crankpin connection surface; then axially stretch the obtained crank-crankpin connection surface, and the stretching length is determined according to the distance from the crankpin center to the crank-main journal connection surface, and the stretching direction is opposite to the Z axis.

[0076] Use the XY datum plane as the sketch plane, draw the crankpin circular surface and the cutting circular surface on the sketch plane. The center of the cutting circular surface coincides with the center of the crankpin circular surface. The radius must be larger than the distance from the center of the crankpin circular surface to the lowest point in the Y direction of the crank-crankpin connection surface. The area between the two circles is the cutting area for stretching and cutting, and the length is half the length of the crankpin; use the YZ datum plane as the sketch plane for the bevel section of the crank top, draw the bevel section of the crank top, and then perform rotational cutting around the center axis of the main journal. The cutting angle and direction parameters are determined according to the design requirements of the crankshaft crank.

[0077] Use the crank-crankpin connection surface as the sketch plane, and draw the crankpin boss circular surface on the sketch plane. The center of the boss circular surface coincides with the center of the crankpin circular surface. The radius is determined according to the actual size of the boss circular surface. The area between the crankpin circular surface and the boss circular surface is the stretching area. Create the boss part of the crankpin through stretching operation. The stretching length is the height of the boss.

[0078] The spindle neck modeling specifically includes the following steps:

[0079] Take the crank-main journal connection surface as the sketch plane, and draw a circle on the sketch plane as the cross-section sketch of the main journal. The radius of the circle is determined by the radius of the main journal. Then perform the stretching operation, and the stretching thickness is the length of the main journal.

[0080] Take the crank-main journal connection surface as the sketch plane, and draw the main journal boss circular surface on the sketch plane. The center of the boss circular surface coincides with the center of the main journal circular surface. The radius is determined according to the actual size of the boss circular surface. The area between the main journal circular surface and the boss circular surface is the stretching area. The boss part of the main journal is created through stretching operation. The stretching length is the height of the boss.

[0081] Use the YZ reference plane as the sketch plane, draw a circular sketch on the sketch plane to create the main journal oil hole, and form the main journal oil hole through stretching and cutting. The size of the circle is determined by the radius of the main journal oil hole, and the stretching and cutting length must be completely through. Save the sketch after completion; then copy the previously saved main journal oil hole sketch on another sketch plane, form the other side of the main journal oil hole through stretching and cutting, and chamfer the edges of the main journal oil hole.

[0082] The crankpin mid-axis surface of the crankshaft is used as the mirror plane to mirror the part, and the original part is retained; at the same time, the crankpin, crankpin boss, main journal, and main journal boss of the crankshaft are chamfered, and the size of the fillet is determined according to the actual crankshaft fillet radius.

[0083] After all modifications are completed, all features of the part are regenerated to ensure the integrity and accuracy of the model; to simplify subsequent operations and observations, all reference surfaces in the part are hidden to make the model more concise.

[0084] (1.2.2) The specific steps for finite element analysis of the crankshaft three-dimensional geometric model are as follows:

[0085] like Figure 8 、 Figure 9 and Figure 10 As shown in Table 1, the crankshaft is made of 34CrNi3MoA alloy steel. The mass density, elastic modulus and Poisson's ratio of the material are obtained by querying. The material density ρ is 7850 kg / m 3 , elastic modulus E = 210 GPa, Poisson's ratio μ = 0.3; material parameters are defined in the three-dimensional geometric model of the single-throw crankshaft, and the material parameters include material density, elastic modulus and Poisson's ratio; the specific parameter values of the material parameters are determined according to the material used in the crankshaft.

[0086] Table 1 Basic property parameters of 34CrNi3MoA material

[0087]

[0088] In the material assignment module, a homogeneous solid section is created, and the defined material properties are assigned to the entire area of the crankshaft component through the created homogeneous solid section; then the created crankshaft 3D geometry model is imported into the assembly.

[0089] The nominal bending moment of the L6 single-throw crankshaft is the maximum bending moment the crankshaft is subjected to when in working condition, that is, the bending moment the crankshaft is subjected to under maximum explosion pressure. The specific expression is as follows:

[0090]

[0091] Where: M -1 is the nominal bending moment, D is the cylinder diameter, L1 is the distance from the center of the crank connecting rod to the center of the main journal, G is the distance from the center of the crank arm to the center of the main journal, P is the cylinder explosion pressure, K is the support coefficient, and L is the distance between the centers of two adjacent main journals.

[0092] According to the parameters required for the bending moment calculation in Table 2, the nominal bending moment M of the single-throw crankshaft is calculated. -1 = 10500 N·m. Considering the difficulty of directly adding bending moments in the simulation platform, the bending moments were converted into loads. In the finite element model, the nodes at the clamping end were constrained to the center using a coupled mode. A load was then applied axially along the cylindrical surface of the single-throw crankshaft main journal. To simulate the bending conditions of the crankshaft, a fixed constraint was applied to the right surface of the single-throw crankshaft main journal, fixing all nodes on the right side of the main journal. Mesh size significantly affects crankshaft stress results. Extensive simulation comparisons have shown that a 4mm mesh provides more accurate crankshaft stress calculations.

[0093] Table 2 Parameters required for bending moment calculation

[0094]

[0095] In the analysis step module, first create a static analysis step and select the static-general analysis step; according to the definition of interaction, create a reference point in the assembly; associate the reference point with the left and right end faces of the single-throw crankshaft main journal through coupling constraints to define the interaction relationship in the model; apply a concentrated force load to the reference point of the assembly and apply a fixed constraint to the other reference point to simulate the mechanical behavior under actual working conditions; after completing the load and constraint settings, it is necessary to mesh the part and generate a suitable mesh by setting mesh control, selecting element type and adjusting seed size parameters; select the nodes of the part to create an output node set; create a job and set the job name, model and type parameters; after all settings are completed, submit the job for finite element analysis.

[0096] (1.3) The Tkinter library is used to develop a graphical interface for the dialog script, which integrates parameter input, model generation and finite element analysis modules.

[0097] like Figure 5As shown, the graphical interface divides the dialog box into two modules according to the function, the "Model" module and the "Pre" module; the "Model" module is divided into two areas. The "Structural Parameter" area on the left contains six structural parameters: crankpin diameter D1, crankpin length L1, crankpin fillet radius R1, main journal diameter D2, main journal length L2 and main journal fillet radius R2; the "Crankshaft" area on the right is a schematic diagram that marks the position of each structural dimension in the single-throw crankshaft.

[0098] The "Pre" module is divided into six areas according to different functions. The "Material" area contains three material parameters: mass density, Young's modulus and Poisson's ratio; the "Step" area contains an input box for setting the incremental step size; the "Load" area is used to enter the set bending load size; the "Mesh" area is used to enter the mesh size; the "Job" area is used to name a finite element analysis; the "Stress Display" area covers a schematic diagram of the position where the bending load is applied in a single-throw crankshaft.

[0099] (1.4) The development of registration scripts enables seamless integration of custom modeling functions with the ABAQUS software main program. Specifically, through modular development and object-oriented programming, the functions of the kernel code and dialogue scripts are encapsulated in a unified operating interface.

[0100] When developing a single-throw crankshaft modeling and analysis plug-in in ABAQUS, define a class that inherits from AFXForm. In the class initialization part, set the commands associated with the kernel code functions of the single-throw crankshaft modeling and analysis plug-in and the keyword variables used to pass parameters; define methods to obtain the corresponding dialog box instance to display the operation interface; set the inspection mechanism and the logic for canceling the operation; finally, obtain the plug-in toolset, register a button, bind the class instance to the button operation, and specify the kernel initialization string, so as to integrate the functions of the kernel code of the single-throw crankshaft modeling and analysis plug-in and the functions of the dialog box script into an operation interface. Users can perform operations related to crankshaft bending stress analysis by clicking a button.

[0101] (2) Optimal Latin hypercube sampling is used within the defined range to obtain pre-calculated samples, batch processing files and Python scripts are developed, and the command-driven finite element method is used to automate crankshaft fatigue parametric modeling and large-sample finite element analysis. Based on the optimal Latin hypercube sampling method, pre-calculated samples are automatically generated within the specified parameter range. This method ensures the uniform distribution and representativeness of the samples in the parameter space, thereby supporting subsequent large-sample analysis and model construction. Subsequently, ABAQUS batch processing files were developed for crankshaft fatigue parametric modeling and large-sample analysis, and an efficient Python script processing process was established. Combined with the command-driven finite element method, batch modeling and analysis of several groups of crankshaft samples were achieved, significantly improving the efficiency of finite element calculations.

[0102] (2.1) Optimal Latin Hypercube Sampling

[0103] The single-throw crankshaft design variables are selected as crankpin diameter D1, crankpin length L1, crankpin fillet radius R1, main journal diameter D2, main journal length L2, and main journal fillet radius R2. The variable constraint range of the single-throw crankshaft design variables is determined based on the tolerance range of each dimension.

[0104] The tolerance ranges between the various dimensions of the L6 crankshaft were precisely defined at the outset of its design, ensuring precise fit with other components in the diesel engine. Setting constraints for L6 crankshaft dimensional optimization based on these tolerances prevents post-optimization dimensions from exceeding tolerances and causing mismatches with associated components. Table 3 shows the constraints for the design variables.

[0105] Table 3 Constraint range of single-throw crankshaft design variables

[0106]

[0107] The optimization of the L6 crankshaft is a single-objective optimization. Although there is no need to consider interaction effects and nonlinear responses, each additional objective can improve the accuracy of the agent model. According to the empirical formula

[0108] N=4(n+1)(n+2)

[0109] Where N is the number of samples, n is the number of input design variables, n = 6, and 224 groups of samples are generated according to the formula.

[0110] Optimal Latin hypercube sampling is used within the variable constraints of the six design variables to obtain several groups of pre-calculated samples. Each group of pre-calculated samples includes six design variable values. The specific method of optimal Latin hypercube sampling is as follows:

[0111] Determine the number of parameters that need to be sampled and the value range of each parameter, divide the value range of each parameter into a corresponding number of intervals according to the number of sampling points, and ensure that each interval has equal probability; randomly select a sample point in each interval to form an initial Latin hypercube sample set; the sample points are evenly distributed in each parameter space, and the initial Latin hypercube sample set is optimized and adjusted by minimizing the distance metric between sample points. During the optimization process, a simulated annealing optimization algorithm is used to continuously try to adjust the position of the sample points until the set optimization goal is achieved, thereby obtaining the optimal Latin hypercube sample set that meets the optimization criteria.

[0112] (2.2) The command drives the single crankshaft modeling analysis plug-in to perform finite element analysis.

[0113] like Figure 11 As shown in the figure, analysis of the SN curve shows that the stress level of the crankshaft is negatively correlated with its fatigue life: greater stress means shorter fatigue life, and vice versa. Since the overall fatigue life of a crankshaft is determined by its most vulnerable portion, measuring the stress in this portion alone can determine its minimum fatigue life. However, the complexity of the modeling process and computational cost often pose significant challenges when performing crankshaft fatigue analysis and finite element simulation in ABAQUS. While specialized plug-ins exist that allow for direct operation and solution within the ABAQUS interface, this process is often time-consuming and expensive. Furthermore, this approach requires a large number of prediction samples, making manual modifications to material parameters and job submissions within the software particularly difficult. To address these issues, a set of batch processing files and Python scripts were developed. Combined with ISIGHT software, this automated process for crankshaft fatigue parametric modeling and sample finite element stress analysis was achieved. Calculating the output for all samples took approximately 200 hours.

[0114] like Figure 12 As shown in the figure, the specific steps are as follows: assign six structural dimension parameters to the crankshaft structure, including crankpin diameter D1, crankpin length L1, crankpin fillet radius R1, main journal diameter D2, main journal length L2 and main journal fillet radius R2, call the single-throw crankshaft modeling and analysis plug-in of ABAQUS, submit 224 groups of samples after optimal Latin hypercube sampling, generate 224 groups of finite element calculation result files, and obtain the key stress data of each group of input samples by extracting the parameter file of the maximum bending stress of the single-throw crankshaft. Then, complete the crankshaft fatigue life analysis of the 224 groups of input samples and obtain the fatigue life prediction results of each group of samples.

[0115] (3) The sensitivity of parameters was analyzed using the Pareto chart, and a Kriging proxy model was built and combined with the particle swarm algorithm to optimize the crankshaft structure. The L6 single-bend crankshaft modeling and analysis plug-in was used for calculation, and the fatigue life of the initial structure was compared to verify the correctness of the fatigue life optimization method. The sensitivity of each key parameter was analyzed by the Pareto chart, and the main parameters that had a significant impact on the fatigue performance of the crankshaft were clearly identified. At the same time, the secondary parameters with lower sensitivity were eliminated, effectively optimizing the complexity of the model. Based on the input and output data of the high-precision calculation sample, the Kriging proxy model was constructed, and the accuracy of the model was verified by the determination coefficient to meet the requirements of engineering applications. Finally, based on the Kriging proxy model combined with the particle swarm algorithm for multi-objective optimization, the optimal solution of the crankshaft size parameters under the stress minimization condition was obtained, and the feasibility and effectiveness of the solution were verified by finite element simulation.

[0116] (3.1) Pareto chart analysis of sensitivity revealed that the crankpin fillet radius R1, main journal diameter D2, and main journal length L2 had negative effects on the fatigue life of the L6 crankshaft, with the crankpin fillet radius R1 having the greatest negative effect. The crankpin diameter D1, crankpin length L1, and main journal fillet radius R2 had positive effects on the crankshaft fatigue life. The main journal diameter D2 and main journal length L2 were removed from the 224 pre-calculated samples to form training sample points. The training sample points included four structural parameters and the maximum bending stress value of the single-throw crankshaft.

[0117] Based on 224 groups of samples and the corresponding maximum bending stress calculated by finite element, a Pareto chart is used to identify the contribution of different dimensions to the crankshaft stress. The Pareto chart shows the relative importance of different factors on the results according to the Pareto principle, and sorts the factors according to their contribution to the output response, so as to intuitively show which factors play a dominant role. The blue column in the Pareto chart represents a factor that has a positive effect on the response variable, that is, when the factor increases, the fatigue life of the crankshaft increases; on the contrary, the red column represents a negative effect, that is, the increase in the factor leads to a decrease in fatigue life. The results show that the crankpin fillet radius R1 has a strong negative effect on the fatigue life of the L6 crankshaft and is the main dimensional factor affecting the fatigue life of the crankshaft. In addition, only the crankpin diameter D1, crankpin length L1 and main journal fillet radius R2 have a positive effect on the fatigue life of the L6 crankshaft, that is, the life of the crankshaft will be improved when the size increases, such as Figure 13 shown.

[0118] (3.2) Kriging surrogate model

[0119] The optimization process usually requires multiple iterations to gradually approach the optimal solution. Faced with complex simulations, each run may consume a lot of time and computing resources. Using a surrogate model can make iterations execute more quickly, allowing for rapid evaluation. Among various surrogate models, the Kriging surrogate model is very suitable for situations where high prediction accuracy is required because of its excellent efficiency and ability to provide accurate predictions based on the same samples. The Kriging surrogate model is based on the Kriging interpolation algorithm, and its expression is:

[0120]

[0121] Where: is the estimated value, w is the optimal coefficient, and y is the true value.

[0122] The calculated output value of the function expression obtained by fitting the sample data by the least squares method and used to approximately describe the relationship between the dependent variable and the independent variable is described as the weighted linear superposition of the samples. As long as the optimal coefficient w is found so that the estimated value The difference with the true value y(x) is the smallest, and If the unbiased estimation is satisfied, the model training is considered complete, so the improved Kriging interpolation algorithm expression can be obtained as follows:

[0123]

[0124] Where: E(*) is the mathematical expectation of the variable value.

[0125] In the above formula, w (i) Solve the following system of equations:

[0126]

[0127] Where: μ represents the Lagrange multiplier, x i 、x j Represent different groups of input variables; for the covariance Cov(x0,x i ), a variation function is introduced as an alternative, and the most widely used is the Gaussian model;

[0128]

[0129] like Figure 14 As shown, the specific process of building the Kriging proxy model is as follows:

[0130] First, the data set consisting of training sample points is divided into a training set and a test set, usually divided at a ratio of 70%-30%. The training set is used for model construction, and the test set is used to evaluate model performance. Then, for the sample points in the training set, four structural dimension parameters are identified as input variables, and stress values are used as output variables. When constructing the Kriging proxy model, a Gaussian function is selected to describe the correlation between the input variables and the output variables, and the unknown parameters in the Gaussian function are determined based on the sample point data. Using the Gaussian function with determined parameters, the sample points in the training set are fitted to construct a preliminary Kriging proxy model. Then, the test set is used to verify the model, and the coefficient of determination R is used to determine the unknown parameters in the Gaussian function. 2 Indicators evaluate the prediction accuracy of the model. Generally speaking, R 2 The larger the value, the better. 2 The closer it is to 1, the smaller the error between the maximum bending stress value of the single-bend crankshaft predicted by the proxy model and the maximum bending stress value of the single-bend crankshaft obtained by simulation is, and R 2 The approximate model is considered to be credible if the value of is greater than 0.95. 2 A value greater than or equal to 0.95 is a usable high-precision Kriging proxy model. If the proxy model has a very low precision, the optimal Latin hypercube sampling method is used to double the number of samples on the basis of 224 groups of samples. The finite element analysis is performed in combination with the command-driven single-bend crankshaft modeling and analysis plug-in to obtain the maximum bending stress value of the single-bend crankshaft corresponding to all samples. The Kriging proxy model is rebuilt using all new and old samples and R is calculated. 2 Repeat the above steps until R 2 The value is greater than or equal to 0.95. The final Kriging surrogate model has an R 2 The value is 0.971, which has a good degree of fitting and high credibility. It can be used to predict stress values under new size parameter combinations, reduce dependence on finite element calculations, and improve calculation efficiency.

[0131] The constructed Kriging proxy model replaces the time-consuming calculation process for different input samples in finite element simulation, and can quickly obtain the output response values corresponding to all possible input sample combinations in the design space. Therefore, simply input the input samples to be calculated into the Kriging proxy model, that is, four fixed structural dimensions, to quickly obtain the output response for this set of samples, namely the maximum bending stress value of the single-throw crankshaft.

[0132] (3.3) Particle Swarm Optimization

[0133] Crankshaft optimization, with stress as the sole objective, is a single-objective optimization analysis. For this type of analysis, the particle swarm optimization algorithm excels due to its high implementation and computational efficiency. It simulates the collaborative optimization behavior of a flock of birds, sharing information between individuals and the group to search for the global optimal solution, eliminating the need for complex adaptive adjustments and genetic manipulation. In the particle swarm optimization algorithm, each particle represents a potential solution and has two properties: position and velocity. Particles update their own velocity and position by tracking the individual optimal solution and the global optimal solution. The position and velocity update formulas are as follows:

[0134] V ij (n+1)=ωV ij (n)+c1r1[P Best (n)-X ij (n)]+c2r2[G Best (n)-X ij (n)]

[0135] X ij (n+1)=X ij (n)+V ij (n+1)

[0136] Where: V ij (n) and X ij (n) represent the velocity and position vector of particle i in j-dimensional space after n iterations; P Best (n) and G Best (n) represents the optimal solution of the particle individual and the optimal solution of the particle swarm obtained after n iterations respectively; c1 and c2 are learning factors; r1 and r2 are random numbers in the interval [0,1]; ω is the inertia factor.

[0137] After 500 iterations, the particle swarm optimization algorithm generated bending stresses for all selected L6 crankshafts. Table 4 lists 15 sample data sets, with 485 remaining. The iterative results show that the optimization results stabilize around 448 MPa, ultimately achieving an optimal solution of 448.3395 MPa.

[0138] Table 4 Sample dataset

[0139]

[0140] Combined with simulation to verify the optimal structural dimensions, the calculated maximum stress value is 446.9 MPa, with an error within 1%. Its minimum fatigue life is 7,862,984 times, which is an increase of 118% compared to the original model.

[0141] If the error value is greater than 1%, then return to the particle swarm algorithm optimization step, adjust the particle swarm algorithm's inertia weight, learning factor and other related parameters, and reuse the particle swarm algorithm to find the output response in the Kriging proxy model, that is, the sample point with the smallest maximum bending stress value of the single-knuckle crankshaft, that is, the combination of the four structural dimensions and the corresponding maximum bending stress value of the single-knuckle crankshaft. Then, the four single-knuckle crankshaft design variables and the two initial values of the main journal diameter D2 and the main journal length L2 in the newly found sample points are input into the L6 type single-knuckle crankshaft modeling analysis plug-in to obtain the corresponding maximum bending stress value, and compare it with the newly optimized maximum bending stress value to calculate the error; repeat this cycle until the calculated error is less than 1%, and the output maximum bending stress value is the optimized value, and the corresponding six single-knuckle crankshaft design variables are also the optimized results, such as Figure 15 As shown in the iterative graph, the optimization results stabilize near 448 MPa, ultimately achieving an optimal solution of 448.3395 MPa. The corresponding optimal structural dimensions are: crankpin diameter D1 is 99 mm, main journal radius D2 is 115 mm, crankpin length L1 is 51.5541 mm, main journal length L2 is 84 mm, crankpin fillet radius R1 is 5.1820 mm, and main journal fillet radius R2 is 7.1921 mm.

Claims

1. A structural optimization method for improving the fatigue life of a marine diesel engine crankshaft, characterized in that: The steps include: (1) Develop a single-throw crankshaft modeling and analysis plug-in to implement parametric modeling and bending stress analysis based on the ABAQUS API; (1.1) Select the design parameters of the single-throw crankshaft modeling and analysis plug-in, which include six structural dimension parameters, material parameters, and finite element analysis setting parameters; (1.2) Dynamically construct a three-dimensional geometric model of a single-throw crankshaft based on design parameters and perform finite element analysis, and generate a kernel code; (1.3) Develop a graphical interface for the plug-in dialog script using the Tkinter library. The graphical interface integrates the design parameter input, the single-throw crankshaft 3D geometry model, and the finite element analysis parameter module. (1.4) Achieve seamless integration of the single-throw crankshaft modeling and analysis plug-in with the ABAQUS software main program through the development of a registration script. That is, through modular development and object-oriented programming, encapsulate the core code of the single-throw crankshaft modeling and analysis plug-in and the functions of the dialog script in a unified operation interface; (2) Use optimal Latin hypercube sampling to obtain pre-calculated samples within the defined range, develop batch processing files and Python scripts, and use command-driven single-bend crankshaft modeling and analysis plug-in to obtain the maximum bending stress value of each pre-calculated sample; (3) The Pareto chart is used to analyze the parameter sensitivity, the pre-calculated samples are screened to form training samples, a high-precision Kriging proxy model is built, and then the particle swarm algorithm is combined to find the minimum maximum bending stress value of the single-bend crankshaft and the corresponding optimal structural size in the design space.

2. A structural optimization method for improving the fatigue life of a marine diesel engine crankshaft according to claim 1, characterized in that: In the step (1.1), the structural dimension parameters are selected from the six structural dimension parameters that have the greatest impact on the bending stress in the single-throw crankshaft, and the six structural dimension parameters include the crankpin diameter D1, the crankpin length L1, the crankpin fillet radius R1, the main journal diameter D2, the main journal length L2 and the main journal fillet radius R2; the material parameters include material density, elastic modulus and Poisson's ratio; the finite element analysis setting parameters include incremental step, load parameter, grid size and finite element operation name.

3. The structural optimization method for improving the fatigue life of a marine diesel engine crankshaft according to claim 1, characterized in that: The modeling of the crank and crank pin parts in step (1.2) is specifically as follows: Define the Z-axis symmetry plane of the single-throw crankshaft as the XY reference plane, and the X-axis symmetry plane of the single-throw crankshaft as the YZ reference plane; Using the XY datum plane as the sketch plane, draw six positioning circles of part size within the sketch plane. Parts 2, 3, and 4 should be mirrored on the axis where the centers of parts 1 and 5 are located. The size of the positioning circles is determined by the size of the crankshaft crank. Based on the shape of the crank-crankpin connection surface of the single-throw crankshaft, trim off the excess line segments to obtain the crank-crankpin connection surface. Then, axially stretch the obtained crank-crankpin connection surface. The stretching length is determined by the distance from the crankpin center to the crank-main journal connection surface. The stretching direction is opposite to the Z axis. Use the XY datum plane as the sketch plane, and draw the crankpin circle and the cutting circle on the sketch plane. The center of the cutting circle should coincide with the center of the crankpin circle. The radius should be greater than the distance from the center of the crankpin circle to the lowest point of the crank-crankpin connection surface in the Y direction. The area between the two circles is the cutting area, and the extrusion is performed with a length of half the crankpin length. Use the YZ datum plane as the sketch plane for the bevel section of the crank top, draw the bevel section of the crank top, and then perform a rotational cut around the center axis of the main journal. The cutting angle and direction parameters are determined according to the design requirements of the crankshaft crank. Use the crank-crankpin connection surface as the sketch plane, and draw the crankpin boss circular surface on the sketch plane. The center of the boss circular surface coincides with the center of the crankpin circular surface. The radius is determined according to the actual size of the boss circular surface. The area between the crankpin circular surface and the boss circular surface is the stretching area. Create the boss part of the crankpin through stretching operation. The stretching length is the height of the boss.

4. The structural optimization method for improving the fatigue life of a marine diesel engine crankshaft according to claim 1, characterized in that: The spindle neck part modeling in step (1.2) is specifically as follows: Use the crank-main journal connection surface as the sketch plane, and draw a circle on the sketch plane as the cross-section sketch of the main journal. The radius of the circle is determined by the radius of the main journal. Then perform an extrusion operation, and the extruded thickness is the length of the main journal. Use the crank-main journal connection surface as the sketch plane and draw the main journal boss circular surface on the sketch plane. The center of the boss circular surface coincides with the center of the main journal circular surface. The radius is determined based on the actual size of the boss circular surface. The area between the main journal circular surface and the boss circular surface is used as the extrusion area. Create the main journal boss part through extrusion operation. The extrusion length is the height of the boss. Using the YZ datum plane as the sketch plane, draw a circular sketch on the sketch plane to create the main journal oil hole. Use an extrude and cut operation to form the main journal oil hole. The size of the circle is determined by the main journal oil hole radius, and the extrude and cut length must completely penetrate the main journal oil hole. Save the sketch after completion. Then copy the previously saved main journal oil hole sketch on another sketch plane, use an extrude and cut operation to form the other side of the main journal oil hole, and fillet the edge of the main journal oil hole. The crankpin mid-axis surface of the crankshaft is used as the mirror plane to mirror the part, and the original part is retained; at the same time, the crankpin, crankpin boss, main journal, and main journal boss of the crankshaft are chamfered, and the size of the fillet is determined according to the actual crankshaft fillet radius.

5. The structural optimization method for improving the fatigue life of a marine diesel engine crankshaft according to claim 1, characterized in that: The specific steps of performing finite element analysis in step (1.2) are: Obtain material parameters through querying and define them in the single-throw crankshaft 3D geometric model. The material parameters include material density, elastic modulus, and Poisson's ratio. Create a homogeneous solid section in the material assignment module and assign the defined material properties to the entire area of the crankshaft component through the created homogeneous solid section. Then, import the created single-throw crankshaft 3D geometric model into the assembly. In the analysis step module, first create a static analysis step and select the Static-General analysis step. Based on the interaction definition, create a reference point in the assembly. Use coupling constraints to associate the reference point with the left and right end faces of the single-throw crankshaft main journal to define the interaction relationship in the model. Apply a concentrated force load to the reference point of the assembly, that is, calculate the nominal bending moment of the single-throw crankshaft. The nominal bending moment is the maximum bending moment that the crankshaft can withstand during operation. Convert the bending moment into a load. In the finite element model, constrain the nodes used for the clamping end to the center point using a coupling mode. Then, apply an axial load along the cylindrical surface of the single-throw crankshaft main journal. A fixed constraint is applied to the right surface of the single-throw crankshaft main journal, fixing all nodes on the right side of the main journal. After completing the load and constraint settings, mesh the crankshaft and set an appropriate mesh size. Generate an appropriate mesh by setting mesh control, selecting the element type, and adjusting the seed size parameters. Select the weakest node of the crankshaft to create an output node set. Create a job and set the job name, model, and type parameters. After all settings are completed, submit the job for finite element analysis.

6. The structural optimization method for improving the fatigue life of a marine diesel engine crankshaft according to claim 1, characterized in that: In step (1.3), the graphical interface is divided into two modules based on their functions: the "Model" module and the "Pre" module. The "Model" module is divided into two areas. The "Structural Parameter" area on the left contains six structural parameters: crankpin diameter D1, crankpin length L1, crankpin fillet radius R1, main journal diameter D2, main journal length L2, and main journal fillet radius R2. The "Crankshaft" area on the right contains a schematic diagram that marks the position of each structural dimension in the single-throw crankshaft. The "Pre" module is divided into six areas according to different functions. The "Material" area contains three material parameters: mass density, Young's modulus and Poisson's ratio; the "Step" area contains an input box for setting the incremental step size; the "Load" area is used to enter the set bending load size; the "Mesh" area is used to enter the mesh size; the "Job" area is used to name a finite element analysis; the "Stress Display" area contains a schematic diagram of the position where the bending load is applied in a single-throw crankshaft.

7. The structural optimization method for improving the fatigue life of a marine diesel engine crankshaft according to claim 1, characterized in that: The specific method of optimal Latin hypercube sampling in step (2.1) is: Determine the number of parameters that need to be sampled and the value range of each parameter, divide the value range of each parameter into a corresponding number of intervals according to the number of sampling points, and ensure that each interval has equal probability; randomly select a sample point in each interval to form an initial Latin hypercube sample set; the sample points are evenly distributed in each parameter space, and the initial Latin hypercube sample set is optimized and adjusted by minimizing the distance metric between sample points. During the optimization process, a simulated annealing optimization algorithm is used to continuously try to adjust the position of the sample points until the set optimization goal is achieved, thereby obtaining the optimal Latin hypercube sample set that meets the optimization criteria.

8. The structural optimization method for improving the fatigue life of a marine diesel engine crankshaft according to claim 1, characterized in that: The step (2) includes the following specific steps: (2.1) Six structural dimension parameters are selected as the design variables of the single-throw crankshaft. The variable constraint ranges of the single-throw crankshaft design variables are determined based on the tolerance ranges between the various dimensions. Optimal Latin hypercube sampling is used within the variable constraint ranges of the six design variables to obtain several sets of pre-calculated samples, each set of pre-calculated samples including six design variable values. (2.2) The instruction drives the single-bend crankshaft modeling and analysis plug-in to perform finite element analysis to obtain the maximum bending stress values of the single-bend crankshaft corresponding to several groups of pre-calculated samples.

9. The structural optimization method for improving the fatigue life of a marine diesel engine crankshaft according to claim 1, characterized in that: The step (3) includes the following specific steps: (3.1) The sensitivity of the structural parameters is analyzed using a Pareto chart. The main journal diameter D2 and main journal length L2 are removed from several sets of pre-calculated samples to form training samples. The training samples include the four structural parameters and the maximum bending stress value of the single-throw crankshaft. (3.2) Build a Kriging proxy model and use the data set composed of training samples to build the Kriging proxy model. The input of the Kriging proxy model is 4 structural parameters. The output of the Kriging proxy model is the maximum bending stress value of the single crankshaft. The determination coefficient R is used to calculate the maximum bending stress of the single crankshaft. 2 Evaluate the accuracy of the Kriging surrogate model, i.e. R 2 Is it close to 1? 2 When R<0.95, increase the sample size and retrain the Kriging surrogate model until R 2 ≥0.95; (3.3) The particle swarm optimization algorithm is used to find the minimum single-turn crankshaft maximum bending stress value and the corresponding optimal structural dimensions in the design space. The optimal structural dimensions are input into the single-turn crankshaft modeling and analysis plug-in, where the main journal diameter D2 and the main journal length L2 are set as the initial values. The corresponding maximum bending stress value is obtained and compared with the maximum bending stress value obtained by optimization to calculate the error. If the error is within 1%, the current optimal structural dimension parameters are output; if the error value is greater than 1%, the relevant parameters of the particle swarm optimization algorithm are adjusted, and the particle swarm optimization algorithm is reused to find the optimal output response in the Kriging proxy model until the error is less than 1%.

10. The structural optimization method for improving the fatigue life of a marine diesel engine crankshaft according to claim 9, characterized in that: In the step (3.1), the sensitivity of the structural parameters is analyzed using a Pareto chart, and it is found that the crankpin fillet radius R1, the main journal diameter D2, and the main journal length L2 have a negative effect on the fatigue life of the crankshaft, among which the crankpin fillet radius R1 has the largest negative effect, and the main journal diameter D2 and the main journal length L2 have a smaller negative effect, so the main journal diameter D2 and the main journal length L2 are eliminated; the crankpin diameter D1, the crankpin length L1, and the main journal fillet radius R2 have a positive effect on the fatigue life of the crankshaft.

Images