Traditional gear hobbing tooling design heavily relies on accumulated experience and trial-and-error methods, often lacking systematic analytical approaches. This results in extended design cycles and increased costs. To address these challenges, this study focuses on a disc-type cylindrical involute helical gear, utilizing Finite Element Analysis (FEA) tools to develop a set of quick-change gear hobbing fixtures. The objective is to enhance the overall design level and mechanical performance of the gear hobbing fixtures. Initially, the fixture structure is designed based on the machining principles of cylindrical involute helical gears using a gear hobbing machine. Subsequently, simulation analysis is performed using ANSYS Workbench software. The analysis results indicate that the structural strength of the fixture meets the machining requirements; however, the equivalent stress value on the expansion sleeve exceeds the allowable stress by 24%. To improve the equivalent stress distribution on the expansion sleeve and enhance its service performance, a multi-objective optimization method based on a genetic algorithm is employed for its redesign. Following optimization, with both deformation and equivalent stress satisfying the required criteria, the fatigue life of the expansion sleeve is significantly increased.
The gear hobbing process is widely adopted in gear manufacturing due to its significant advantages in efficiency, precision, and economy. During gear hobbing operations, the stability, positioning accuracy, and changeover efficiency of the fixture directly determine the quality of gear machining and production efficiency. However, traditional gear hobbing tooling design faces several technical bottlenecks. On one hand, the design process overly relies on empirical accumulation and trial-and-error methods, lacking systematic analytical means, which leads to prolonged design cycles and increased costs. On the other hand, existing fixture structures are often complex, and the changeover process is cumbersome, making it difficult to adapt to the demands of multi-variety, small-batch production modes. Against this backdrop, achieving rapid fixture changeover, structural optimization, and performance enhancement through technological innovation has become an urgent technical challenge in the current field of gear manufacturing.
Finite element analysis technology provides a new solution for the design and optimization of fixtures and jigs. In this context, this study, based on the actual needs of a gear manufacturing enterprise, uses finite element analysis technology as the core support to carry out innovative design and multi-objective optimization research on a quick-change gear hobbing tooling system. The research object is a disc-type cylindrical involute helical gear, and the design is based on the YS3120CNC gear hobbing machine.
Structural Design of Gear Hobbing Tooling
Based on the geometric characteristics of the disc gear and the motion characteristics of the gear hobbing machine, the following tooling design scheme is formulated:
- According to the geometric features of the disc gear and the parameters of the YS3120CNC CNC gear hobbing machine, a dual-benchmark positioning system is established: the gear end face constitutes the axial positioning benchmark, and the high-precision mounting hole establishes the radial positioning benchmark, achieving complete six-degree-of-freedom constraint of the workpiece.
- Aiming at the positioning deviation caused by geometric accuracy defects of the workpiece inner hole, a multi-lobed elastic expansion sleeve mechanism is adopted. This mechanism achieves adaptive compensation through uniform radial deformation, effectively eliminating fit clearance and reducing tooth profile and pitch accumulation deviation.
- In view of the functional requirements of workpiece inner hole positioning and expansion, an external expansion mechanism is developed based on the cone surface coupling principle: the fixed expansion sleeve and the axially movable expansion sleeve pull rod are matched through the cone surface, driving the radial expansion of the expansion sleeve to form a reliable interference fit.
- Aiming at the φ34.7 mm workpiece inner hole and the structural limitations of the gear hobbing machine, a piston-type connecting pull rod is designed to realize the expansion sleeve expansion function through axial displacement transmission.
- The connection method and connection dimensions between the expansion sleeve and the tooling body are standardized to achieve quick replacement of the expansion sleeve when processing workpieces of different sizes.
According to the above scheme analysis, the final design of the gear hobbing tooling fixture is completed. The working principle of the fixture is as follows: the expansion sleeve pull rod generates an axial downward displacement driven by the machine tool hydraulic system, thereby applying pressure perpendicular to the cone surface to the expansion sleeve, prompting the expansion clamping section of the expansion sleeve to expand radially. This mechanical action generates radial expansion force, realizing the radial positioning of the workpiece.
Finite Element Simulation Analysis of Gear Hobbing Tooling
The materials used for making various parts of the tooling are all 20CrMnTi, and the hob material is S390. The mechanical parameters of the materials are shown in Table 1.
| Material | Density (kg/m³) | Elastic Modulus (GPa) | Poisson’s Ratio | Yield Strength (MPa) |
|---|---|---|---|---|
| 20CrMnTi | 7,860 | 212 | 0.289 | 835 |
| S390 | 7,880–8,040 | 220–240 | — |
To improve computational efficiency and the accuracy of calculation results, while truly reflecting the structural characteristics of each part and without affecting the structural characteristics of the assembly, the tooling model is simplified in the following aspects:
- Remove small fillets, chamfers, process holes, keyways, and relief grooves; remove small threaded holes directly; change larger threaded holes into counterbores.
- Remove connecting parts such as screws and bolts, as these parts only affect the local stress state of the structure.
- Simplify the hob and workpiece.
After the simplification is completed, the tooling model is processed for meshing. As the tooling part structure is relatively complex, before meshing, each part needs to be segmented, and then the segmented parts are meshed one by one.
During the gear hobbing process, the tooling mainly bears the action of three types of loads: the hobbing force, the pull rod tightening force, and the tailstock pressing force. This study is based on the law of energy conservation, and by extracting the machine tool spindle power data, the maximum tangential hobbing force $F_t$ is calculated to be 725.028 N. Then, the radial hobbing force and axial hobbing force are estimated using Equation (1). Adopting a conservative principle, the coefficients take the maximum values: radial hobbing force $F_r = F_t / 0.2 = 3,625.14$ N, axial hobbing force $F_a = 0.7 F_r = 2,537.6$ N.
$$ \begin{cases} F_a = (0.2 \sim 0.7) F_r \\ F_r = (0.2 \sim 0.6) F_t \end{cases} $$
The clamping and unclamping of the workpiece and the rising and falling of the tailstock are all driven by the machine tool hydraulic system. The output pressure of the hydraulic cylinder can be calculated by the following equation.
$$ F = P \times A \times \eta $$
Where: $F$ is the output pressure of the hydraulic cylinder, N; $P$ is the pressure, Pa; $A$ is the effective area of the hydraulic cylinder, m²; $\eta$ is the efficiency coefficient.
The theoretical value range of the efficiency coefficient is 0.85–0.95. This paper adopts the conservative design principle, taking the upper limit value of the efficiency coefficient $\eta = 0.95$ for calculation analysis. Then, by substituting the piston diameter and working pressure of the hydraulic cylinder into Equation (2), the tailstock pressing force is approximately 9,363 N, and the worktable hydraulic cylinder pulling force is approximately 3,581 N. The pressing force is applied to the upper end face of the pressure cover, direction downward; the pulling force is applied to the lower end face of the machine tool pull rod, direction also downward.
In addition, to simulate the constraint effect of the worktable on the tooling, a fixed constraint is applied to the lower end face of the tooling base.
The deformation results of each part of the gear hobbing tooling are analyzed. The maximum deformation of the tooling is 0.7909 mm, located at the bottom of the machine tool pull rod. This phenomenon is mainly caused by the deformation of the machine tool pull rod-piston-expansion sleeve pull rod transmission system and the downward axial displacement. The upper end face of the tray shows a uniform deformation of about 0.01 mm. This deformation amount has a negligible impact on machining accuracy, proving that the tooling has good support performance. The deformation amounts of the tooling base, body, and limit block are all small, with maximum deformation amounts of 0.00085 mm, 0.0025 mm, and 0.00023 mm, respectively. These deformations have a negligible impact on machining accuracy. The expansion sleeve deforms and opens under the radial extrusion of the expansion sleeve pull rod, forming a uniform radial displacement, with a maximum value of about 0.25 mm, located at the uppermost part of the expansion sleeve and decreasing axially downward.
The equivalent stress distribution of each part of the tooling is analyzed. The yield strength of 20CrMnTi material is 835 MPa. Based on the design requirement of a tooling safety factor of 1.5, the allowable stress is calculated to be 556 MPa. The analysis results show that the maximum equivalent stress appears at the expansion sleeve, which is 689.93 MPa, exceeding the allowable stress value by about 24%. This phenomenon may be related to the unreasonable structural design parameters of the expansion sleeve and improper empirical values of key dimensions, which need to be structurally optimized in the subsequent design. The maximum equivalent stress values of the other parts are far lower than the allowable stress value of the tooling.
Multi-objective Optimization of the Expansion Sleeve
Genetic Algorithm (GA) has significant advantages compared to Gradient Descent (GD), Particle Swarm Optimization (PSO), and Simulated Annealing (SA) methods. Firstly, GA has a strong global search ability, avoiding local optima through selection, crossover, and mutation, making it suitable for high-dimensional nonlinear problems, while GD relies on derivatives and is easily affected by initial values, making multi-objective processing difficult. Secondly, GA adopts a population evolution mechanism, which can efficiently generate Pareto optimal solution sets, while PSO may have insufficient solution set distribution. In addition, GA does not require the objective function to be derivable or continuous, supports discrete variables and complex constraints, and has better robustness than single-point methods such as SA. Genetic algorithm is an ideal choice for complex system optimization. This study uses genetic algorithm to perform multi-objective optimization on the expansion sleeve.
To reduce the equivalent stress of the expansion sleeve and improve its service performance, based on design experience, four key dimensions of the expansion clamping section of the expansion sleeve (slot width, neck height of the expansion sleeve, neck wall thickness of the expansion sleeve, bottom hole diameter) are selected as design variables, denoted as P1, P2, P3, P4, respectively.
In order for the key dimensions to be recognized as design variables by ANSYS Workbench, parametric modeling of the expansion sleeve is carried out in SolidWorks. The relevant dimension names are modified to a format starting with “DS_”, and the DesignModeler module in Workbench is embedded into SolidWorks to achieve bidirectional model synchronization update. The specific design variable parametric names and geometric parameter variation ranges are shown in Table 2.
| Design Variable | Parametric Name | Initial Value (mm) | Variation Range (mm) |
|---|---|---|---|
| P1 | DS_D1 | 18 | 13–23 |
| P2 | DS_D2 | 3.75 | 1.5–4 |
| P3 | DS_D3 | 2.5 | 1.5–3.5 |
| P4 | DS_D4 | 4 | 2–6 |
In the research on the structural optimization design of the expansion sleeve, a multi-objective optimization model is constructed. The maximum deformation P5, maximum equivalent stress P6, and minimum fatigue life P7 are selected as objective variables, and key geometric parameters are selected as design variables. At the same time, the allowable stress of the tooling is taken as a constraint condition. The optimization goal is to maximize the fatigue life while meeting the design requirements of the maximum stress value and maximum deformation. Based on this, an optimization mathematical model is established:
$$
\begin{aligned}
& \text{Find: } \mathbf{x} = [x_1, x_2, x_3, x_4]^T \\
& \text{Maximize: } f_1(\mathbf{x}) = Lf_{\min}(\mathbf{x}) \\
& \text{Minimize: } f_2(\mathbf{x}) = Df_{\max}(\mathbf{x}) \\
& \text{Minimize: } f_3(\mathbf{x}) = Sf_{\max}(\mathbf{x}) \\
& \text{Subject to: } \\
& \quad f_2(\mathbf{x}) – \delta < 0 \\
& \quad 0.2 \leq f_2(\mathbf{x}) \leq 0.3 \\
& \quad f_3(\mathbf{x}) \leq [\sigma] \\
& \quad u_i \leq x_i \leq v_i \quad (i=1,2,3,4)
\end{aligned}
$$
Where: $Lf_{\min}(\mathbf{x})$ is the fatigue life of the expansion sleeve; $Df_{\max}(\mathbf{x})$ is the maximum deformation of the expansion sleeve, mm; $Sf_{\max}(\mathbf{x})$ is the maximum stress value of the expansion sleeve, MPa; $[\sigma]$ is the allowable stress, MPa; $x_i$ is the design variable parameter, mm; $u_i$, $v_i$ are the upper and lower limits of the design variable parameter, mm.
The experimental type adopts Central Composite Design (CCD), and the Face-Centered Cubic (FCC) design method is used to generate experimental samples. Finally, the obtained experimental design points are shown in Table 3 (partially), totaling 49 sets of design points, each containing 4 design variables and 3 objective variables.
| Point | P1 (mm) | P2 (mm) | P3 (mm) | P4 (mm) | P5 (mm) | P6 (MPa) | P7 (Cycles) |
|---|---|---|---|---|---|---|---|
| 1 | 13 | 2.75 | 2.5 | 4 | 0.56364 | 720.9 | 557.17 |
| 2 | 13 | 1.5 | 1.5 | 2 | 1.50729 | 1638.17 | 70.57 |
| 3 | 13 | 4 | 1.5 | 2 | 0.15674 | 305.81 | 6200.53 |
| … | … | … | … | … | … | … | … |
| 23 | 18 | 3.375 | 2.5 | 4 | 0.35845 | 473.52 | 1662.13 |
| 24 | 18 | 2.75 | 1.5 | 4 | 0.57015 | 791.41 | 437.11 |
| 25 | 18 | 2.75 | 2 | 4 | 0.59567 | 781.73 | 451.33 |
| … | … | … | … | … | … | … | … |
| 47 | 23 | 4 | 1.5 | 6 | 0.27243 | 399.54 | 2713.67 |
| 48 | 23 | 1.5 | 3.5 | 6 | 4.87546 | 3364.53 | 14.12 |
| 49 | 23 | 4 | 3.5 | 6 | 0.30349 | 388.77 | 2952.83 |
The Kriging model is an implicit statistical model based on Gaussian process, which describes spatial correlation through covariance function and provides predicted values and confidence intervals. It has advantages such as strong nonlinear fitting ability and high-dimensional adaptability. This paper uses the Kriging model to build a response surface fitting model.
After successfully building the response surface model based on the Kriging method in the response surface optimization module, the obtained goodness-of-fit curve diagram shows that the fitting degree of the objective variables is good, and the model is accurate and reliable.
According to the response surface optimization experimental design results and the constructed response surface model, multi-objective optimization solving is carried out. The solving objectives are set as follows: minimize the maximum deformation P5 (and constrain P5 ≥ 0.2 mm to ensure that the expansion sleeve has the minimum expansion amount required for effectively expanding and clamping the workpiece); the maximum equivalent stress P6 does not exceed the material allowable stress of 556 MPa; simultaneously maximize the minimum fatigue life P7. Using the multi-objective optimization method based on genetic algorithm, the optimization process sets the following parameters: initial sample size is 4000, iteration step size is 800 samples/time, the maximum proportion of Pareto front is set to 70%. The termination condition is to complete 20 generations of iterative calculation, and finally obtain 3 optimal candidate sample groups. The candidate points are shown in Table 4. The objective variables of the three candidate sample groups all meet the multi-objective optimization constraints.
| Parameter | P1 (mm) | P2 (mm) | P3 (mm) | P4 (mm) | P5 (mm) | P6 (MPa) | P7 (Cycles) |
|---|---|---|---|---|---|---|---|
| Initial Value | 18 | 3.75 | 2.5 | 4 | 0.2473 | 703.06 | 594.69 |
| Candidate Group 1 | 15.708 | 3.990 | 3.445 | 3.650 | 0.21031 | 312.304 | 6679.21 |
| Candidate Group 2 | 16.117 | 3.999 | 3.448 | 3.659 | 0.226 | 319.798 | 6679.67 |
| Candidate Group 3 | 15.868 | 3.989 | 3.480 | 3.714 | 0.210 | 317.307 | 6640.87 |
According to the optimization goal of obtaining the maximum fatigue life when the maximum stress value and maximum deformation meet the requirements, Candidate Group 1 is selected as the optimization result. The parameters corrected for this group are the final determined dimensions of the expansion sleeve, as shown in Table 5.
| Parameter | Initial Value (mm) | Optimized Value (mm) | Corrected Value (mm) |
|---|---|---|---|
| P1 | 18 | 15.708 | 15.5 |
| P2 | 3.75 | 3.990 | 4 |
| P3 | 2.5 | 3.445 | 3.4 |
| P4 | 4 | 3.650 | 3.7 |
The corrected values are input as final parameters into the previously established parametric model of the expansion sleeve. The comparison of the expansion sleeve model before and after optimization is shown. Using the final value of the corrected expansion sleeve dimension as the design variable, static analysis is performed again, and compared with the initial result before optimization. As shown in Table 6, after multi-objective genetic algorithm optimization, the maximum deformation of the expansion sleeve is reduced to 0.21755 mm, a decrease of 12.03% compared to the initial value; the maximum equivalent stress is reduced to below the allowable stress, which is 301.09 MPa, a decrease of 57.17% compared to the initial value; the fatigue life is significantly improved, increased from the initial 594.69 cycles to 6,666.3 cycles, an increase of 11.2 times.
| Objective Variable | Before Optimization | After Optimization | Change Amount |
|---|---|---|---|
| Deformation (mm) | 0.2473 | 0.21755 | 0.02975 |
| Stress (MPa) | 703.06 | 301.09 | 401.97 |
| Fatigue Life (Cycles) | 594.69 | 6666.3 | 6071.61 |
Conclusion
This study takes a disc-type gear as the research object and successfully develops a set of quick-change gear hobbing tooling systems using ANSYS Workbench finite element software. After completing the structural design of the tooling based on empirical design, through static analysis, it is found that under external loads, the overall structural strength of the tooling meets the machining requirements. Among them, the equivalent stress value on the expansion sleeve exceeds the allowable stress by 24%, while the stress levels of other parts are significantly lower than the allowable value. Based on this, a multi-objective optimization method based on genetic algorithm is used to optimize the design of the expansion sleeve structure. While ensuring that the deformation and equivalent stress meet the design requirements, the fatigue life of the expansion sleeve is increased from 594.7 cycles to 6,666.3 cycles. This research demonstrates the effectiveness of combining finite element analysis and multi-objective optimization in improving the performance and longevity of critical components in gear hobbing tooling systems used in gear hobbing machines.