Abstract:
The strength analysis and structural optimization of the flywheel bolt tightening reaction mechanism in a four-cylinder gasoline engine assembly line. Utilizing CATIA for 3D modeling and Hyperworks for mesh generation, the finite element analysis (FEA) was conducted in ABAQUS to assess the stress and displacement states under a 400N·m torque. The results indicate that while the reaction mechanism meets the strength requirements, the design of the gear shaping and limiting gear is overly complex, leading to material redundancy and poor economy. Therefore, an optimization of the limiting gear was carried out, and the new design was re-analyzed. The simplified gear shaping structure proved to meet the strength requirements while significantly improving economy, providing valuable insights for flywheel tightening process design and equipment selection.

1. Introduction
The flywheel, as a crucial component in engines, stores energy during the power stroke and provides rotational inertia. It is located at the power output end of the crankshaft, transmitting power through friction with the clutch. The quality of flywheel assembly has a significant impact on the overall performance of the engine. To ensure the quality of flywheel assembly, the tightening process of flywheel bolts is critical, necessitating the introduction of automated and digitalized tightening equipment to monitor the torque variation and attenuation during bolt tightening.
Simultaneously, a reaction mechanism is required at the front pulley of the engine to restrict the torque-induced rotation of the flywheel when four flywheel bolts are tightened simultaneously, ensuring that the bolts are tightened to the required torque specifications. Therefore, the use of CAE simulation software ABAQUS to analyze the structural strength of the flywheel bolt tightening reaction mechanism under a 400N·m bolt tightening torque provides an important basis for evaluating the feasibility and rationality of the reaction mechanism design and flywheel bolt tightening process.
2. Establishment of the Finite Element Model for the Flywheel Bolt Tightening Reaction Mechanism
2.1 3D Model Creation
The main function of the flywheel bolt tightening reaction mechanism is to insert a profiling block into the front pulley of the engine to form a fit and restrict the rotation of the flywheel caused by bolt tightening through a limiting gear, thereby safely and effectively tightening the eight flywheel bolts within the specified takt time. In this paper, the 3D model of the flywheel bolt tightening reaction mechanism was established in CATIA and converted into Step format. The Step format digital model was then imported into Hypermesh software for the creation of the finite element model.
2.2 Finite Element Model Creation
2.2.1 Geometric Model Cleanup
Utilizing Hypermesh, the non-critical fine features in the 3D model of the reaction mechanism, such as chamfers, fillets, small holes, and small bolt holes, were geometrically cleaned. These features, being far from the key analysis areas, have negligible impact on the simulation results but significantly affect mesh quality if not cleaned.
2.2.2 Simplification of Geometric Model Structure and Constraints
For complex assemblies like the reaction mechanism, the number of components is substantial. However, the primary focus is on whether the strength of the gear and V-shaped limiting gear meets the requirements. Considering the efficiency of finite element model creation and software calculation cycles, only the gear and V-shaped limiting gear were modeled in detail, while the base, servo motor, cylinder, drag chain, slide table, fixing bolts, cylinder bracket, etc., were not modeled. Additionally, the gear shaft and rectangular key used to transmit the tightening torque to the gear were not the focus of analysis and were therefore not modeled. The centroid of the gear was measured using CATIA, and a centroid Node was created in Hypermesh based on the centroid coordinates. The centroid Node was rigidly coupled to the nodes on the cylindrical surface of the gear inner hole using the RBE2 rigid element in the 1D panel, with all six degrees of freedom constrained. The torque was then applied to the centroid Node, equivalently replacing the torque transmitted by the gear shaft and rectangular key.
The slideway of the limiting gear is connected to the fixed plate by bolts, which are not the focus of detailed study but serve only to constrain the position of the slideway. Therefore, the RBE2 element in the 1D panel was used to create a rigid coupling of the nodes on the inner surface of the bolt holes, with the element type selected as COUP_KIN, otherwise, ABAQUS would not recognize it. In the ABAQUS Load module, an ENCASTRE (fixed support) boundary condition was created at the coupling point, fully constraining the six degrees of freedom, equivalently replacing the bolt fixation.
2.2.3 Mesh Generation
After simplifying the model, only the gear, limiting gear, and gear slideway components required meshing. Due to the special shape of the gear with 50 teeth, the Geometry panel in Hypermesh was used to split the gear, retaining only 1/50. A hexahedral mesh was applied to this 1/50 gear model, with a base mesh size of 1mm. The meshes of the remaining teeth were obtained by rotation, significantly improving meshing efficiency. The base mesh sizes for the limiting gear and slideway were set to 1mm and 2mm, respectively, with adjustments made to different parts of the model based on actual conditions. Quality control of key parameters such as maximum angle, minimum angle, twist, warp, and Jacobian was performed through mesh quality inspection to ensure that all elements met the calculation requirements. The simplified finite element model of the reaction mechanism. The model has 1,180,197 elements and 1,309,443 nodes, with hexahedral element type C3D8R. The mesh information of the model is summarized in Table 1.
Table 1: Mesh Information of the Model
Component | Number of Nodes | Number of Elements | Element Type |
---|---|---|---|
Gear | 816,750 | 759,200 | C3D8R |
Limiting Gear | 393,080 | 352,800 | C3D8R |
Gear Slideway | 99,513 | 68,197 | C3D8R |
2.2.4 Material Parameters
The material for the gear and gear slideway is 45 steel, while the material for the limiting gear is 40Cr. The material property data is shown in Table 2.
Table 2: Material Property Data
Component | Material Name | Elastic Modulus (MPa) | Poisson’s Ratio | Mass Density (t·mm^-3) | Yield Strength (MPa) |
---|---|---|---|---|---|
Gear | 45 Steel | 2.09×10^5 | 0.269 | 7.89×10^-9 | 355 |
Limiting Gear | 40Cr | 2.11×10^5 | 0.277 | 7.87×10^-9 | 785 |
Gear Slideway | 45 Steel | 2.09×10^5 | 0.269 | 7.89×10^-9 | 355 |
3. Load and Boundary Conditions
The function of the reaction mechanism is to engage the limiting gear with the driving gear, allowing the flywheel to be in a static equilibrium state when four bolts are tightened simultaneously. Therefore, relevant boundary conditions were created according to the static analysis method. The tightening of the flywheel bolts generates a 400N·m torque rotating in the positive X-axis direction. In the ABAQUS Load module, the torque is applied to the gear centroid coupling point, while the freedom of rotation around the X-axis of the centroid coupling point is released.
The primary function of the reaction mechanism in this study is to achieve a static equilibrium state for the flywheel when four bolts are tightened simultaneously by engaging the limiting gear with the driving gear. To simulate this in a finite element analysis (FEA), relevant boundary conditions and loads were created based on the static analysis method.
Loads
- Torque Application:
- The tightening of the flywheel bolts generates a torque of 400N·m rotating in the positive X-axis direction.
- This torque is applied to the gear centroid coupling point in the ABAQUS Load module.
- Simultaneously, the degree of freedom for rotation around the X-axis at the centroid coupling point is released to allow for torque application.
Boundary Conditions
- Fixed Constraints:
- The bolt holes connecting the limiting gear slideway to the fixed plate are not the focus of detailed study but serve to constrain the position of the slideway.
- Rigid body elements (RBE2) are used to couple the nodes within the bolt hole surfaces.
- ENCASTRE (fully constrained) boundary conditions are applied at the coupling points, constraining all six degrees of freedom, effectively replacing the bolt fixation.
- Friction Contact:
- Friction contacts are created between the engaging surfaces of the gear and limiting gear, as well as between the limiting gear and the slideway.
- The sliding formula selected is “Finite sliding,” with “Hard contact” for the normal direction and Coulomb friction for the tangential direction.
- The friction coefficient is set to 0.15, influencing the critical shear stress (τc) as per the formula: τc = μ × p, where μ is the friction coefficient and p is the normal contact pressure.
Analysis Scenarios
- Scenario: Gear subject to torque
- Torque: 400N·m
- Gravity Acceleration: -9800 mm/s² in the Y-direction (considering the effect of gravity)
Convergence and Loading Amplitude
- To ensure better convergence of the model, a custom loading amplitude curve is defined.
- A small initial load is applied in the first analysis step to establish a stable contact relationship.
- The analysis step is of the Static, General type, with a fully Newton-Raphson method selected for solving.
- Geometric nonlinearity (Nlgeom: On) is activated due to the involvement of friction contacts and nonlinear boundary conditions.
- Initial, minimum, and maximum increment sizes are set to 0.01, 1×10^-5, and 0.1, respectively.
By applying these loads and boundary conditions within the ABAQUS software, the stress and displacement states of the reaction mechanism under the specified torque can be accurately simulated and analyzed. This setup allows for the assessment of the structural integrity and performance of the reaction mechanism in the context of the flywheel bolt tightening process.