Air suspension guide arm simulation loading simulation analysis method

Abstract

The invention relates to the field of air suspension guide arm simulation analysis, in particular to an air suspension guide arm simulation loading simulation analysis method. According to the method, an axle is simplified into a circular tube, other models are built according to the actual size, and a CAD digital model of a vertical guide arm loading simulation model is built; importing into finite element analysis software to carry out grid division and endowing each material with attributes; respectively applying loads by adopting a scientific loading method and sequence; and finally, outputting a simulation result. Through system-level modeling and a scientific loading strategy, the real stress state of the guide arm in the whole vehicle is restored, the convergence difficulty is reduced, and high-precision simulation of the loading working condition of the guide arm is achieved.

Description

Technical Field

[0001] The present invention relates to the field of air suspension guide arm simulation analysis, and particularly to a method for simulating the installation of an air suspension guide arm for simulation analysis. Background Art

[0002] As a core component connecting the wheel and the vehicle frame, the automotive guide arm's core function is to constrain the movement trajectory of the wheel relative to the vehicle body, attenuate the vibration caused by the elastic system, and efficiently transmit the loads and torques from the longitudinal, vertical, and lateral directions. By elastically connecting the vehicle body and the wheel, the guide arm significantly reduces the transmission of ground impact to the vehicle body, thereby improving the ride comfort of the vehicle and the comfort of the occupants.

[0003] As a key component of the composite air suspension, due to the complex and variable geometric shape of the guide arm (such as features like the coil ear and the press-bending transition zone), it is difficult to use traditional calculation methods to predict its stress level. CAE simulation analysis can model the stress distribution of the guide arm at the initial stage of design, providing a basis for product design and development. However, currently, component-level analysis or single guide arm assembly analysis is generally used, which cannot accurately reflect the stress situation of the guide arm in the whole vehicle and has a large difference from the whole vehicle.

[0004] Furthermore, the simulation of installing the guide arm on the vehicle belongs to the analysis of a typical non-linear large deformation system, and its difficulty lies in multi-part contact and complex loads. If the contact parameters (such as the friction coefficient), loading sequence, or increment step are set improperly during modeling, it will not only greatly extend the calculation cycle but also may lead to simulation divergence or even failure, seriously affecting the development efficiency.

[0005] Therefore, there is an urgent need to develop a simulation analysis method for the guide arm to accurately predict its true stress distribution and improve the accuracy of the simulation analysis. Summary of the Invention

[0006] The present invention aims at the technical problems existing in the prior art and provides a method for simulating the installation of an air suspension guide arm for simulation analysis, which can reflect the true stress level of the guide arm in the whole vehicle and improve the accuracy of the simulation analysis.

[0007] The technical solution of the present invention to solve the above technical problems is as follows: A method for simulating the installation of an air suspension guide arm for simulation analysis includes the following steps: Step 1, establish the CAD digital model of the guide arm installation simulation model, simplify the axle as a circular tube, model it according to the size of the circular tube, and model the upper backing plate, lower backing plate, guide arm, U-bolt, gasket, and upper cover plate according to the actual size; Step 2, import the CAD digital model into the finite element analysis software, perform mesh division on the circular tube, upper backing plate, lower backing plate, guide arm, U-bolt, gasket, and upper cover plate, and assign each material property; Step 3: Apply an axial pre-tightening force to the U-bolt and gradually load it to the target axial force; apply loads to the guiding arm, including vertical load, longitudinal load, and lateral load respectively; Step 4: Output the simulation results.

[0008] Based on the above technical solutions, the present invention can be further improved as follows.

[0009] Further, the Step 3 includes the following steps: Step1: Apply an axial pre-tightening force of 20N - 100N to the U-bolt; Step2: Apply all axial forces according to the bolt torque-axial force relationship; Keep the bolt at a fixed length, apply vertical loads F1 and F2 to the center of the guiding arm ear, and apply vertical loads F6 and F7 to the center of the airbag at the end of the guiding arm; Keep the bolt at a fixed length, apply longitudinal loads F3 and F4 to the center of the guiding arm ear; Keep the bolt at a fixed length, apply lateral loads F5 and F6 to the center of the guiding arm ear.

[0010] Further, the initial increment step in Step1 and Step2 is set to 0.1, the initial increment step in Step3 is set to 0.01, and the maximum increment step is set to 0.2. [[ID=2,3]]

[0011] Further, in Step1 and Step2, the remaining degrees of freedom on both sides of the guiding arm, gasket, and upper cover plate are constrained, and only the vertical degree of freedom is retained.

[0012] Further, in Step 3, boundary conditions: both ends of the circular tube are fixed with all degrees of freedom, and the side degree of freedom constraints of the guiding arm, gasket, and upper cover plate on both sides are released.

[0013] Further, in Step 3, define interactions: set the circular tube and the upper backing plate, and the lower backing plate as bonded constraints; define all contacts between the guiding arm and the upper cover plate, the guiding arm and the gasket, and the gasket and the upper backing plate, and the friction coefficient is set to 0.2.

[0014] Further, when applying loads to the guiding arm in Step 3, apply vertical loads F1 and F2 to the center of the guiding arm ear, apply vertical loads F7 and F8 to the center of the airbag at the end of the guiding arm, and calculate according to the fact that F1, F2, F7, and F8 jointly bear 2 times the axle load; Apply longitudinal load F3 and lateral load F5 to the center of the guiding arm ear, and calculate according to the theory of 0.7g; Apply longitudinal load F4 and lateral load F6 to the center of the guiding arm ear, and calculate according to the theory of 0.4g.

[0015] Further, in Step 2, a hexahedral mesh is used, and the mesh is encrypted in the bending transition area of the guide arm. The mesh size is 2 mm; the mesh size in the remaining areas is 5 mm. The hexahedral mesh and the local encryption strategy can accurately capture the detailed responses in high stress gradient areas such as the bending transition area while ensuring the calculation efficiency.

[0016] Further, in Step 2, the finite element analysis software is Abaqus software, the solver is selected as implicit, and the contact algorithm is the penalty function.

[0017] Further, in Step 1, the guide arm loading simulation model for the vehicle includes a circular tube, an upper backing plate, a lower backing plate, a guide arm, a U-bolt, a gasket, and an upper cover plate; there are two guide arms on the circular tube. The circular tube and the guide arm are located in the U-shaped groove of the U-bolt and fastened by bolts. Upper and lower backing plates are respectively provided on the upper and lower surfaces of the circular tube located in the U-shaped groove, and a gasket is provided between the upper backing plate and the guide arm.

[0018] The beneficial effects of the present invention are as follows: 1. By establishing a vehicle-level guide arm loading simulation model, the present invention simplifies the axle into a circular tube and models other components based on the actual dimensions, solving the problem that the traditional component-level analysis cannot reflect the true stress state of the whole vehicle, improving the simulation accuracy, and shortening the test cycle.

[0019] 2. The present invention adopts a scientific loading method. The pre-tightening force is loaded step by step, from the initial force to the full pre-tightening force to ensure the smooth fit of the contact surface. The multi-directional loads are applied separately, vertically, longitudinally, and laterally, separating the stress contributions in each direction, which helps the calculation to converge and the loading to be stable; at the same time, the stress under a single-directional load can be obtained. By scientifically setting the contact parameters, loading methods, and sequences between parts, the difficulty of convergence can be reduced, and the efficiency and accuracy of the simulation can be improved. BRIEF DESCRIPTION OF THE DRAWINGS

[0020] Figure 1 It is a schematic diagram of the steps of the air suspension guide arm simulation loading and simulation analysis method described in the present invention; Figure 2 It is a schematic diagram of the steps of Step 3 in the embodiment of the present invention; Figure 3 It is a schematic diagram of the structure of the guide arm loading simulation model described in the present invention.

[0021] In the drawings, the list of components represented by each label is as follows: 1. Circular tube, 2. Upper backing plate, 3. Lower backing plate, 4. Gasket, 5. Guide arm, 6. Upper cover plate, 7. U-bolt. DETAILED DESCRIPTION OF THE EMBODIMENTS

[0022] Next, the technical solutions in the embodiments of the present application will be clearly and completely described in conjunction with the accompanying drawings in the embodiments of the present application. Obviously, the described embodiments are only a part of the embodiments of the present application, rather than all the embodiments. Based on the embodiments in the present application, all other embodiments obtained by those skilled in the art without creative efforts shall fall within the protection scope of the present application.

[0023] In the description of the present application, the terms "first" and "second" are only used for descriptive purposes, and cannot be construed as indicating or implying relative importance or implicitly specifying the quantity of the indicated technical features. Thus, the features defined with "first" and "second" may explicitly or implicitly include one or more of the described features. In the description of the present application, "a plurality" means two or more, unless otherwise specifically defined.

[0024] In the description of the present application, the term "for example" is used to mean "serving as an example, illustration, or explanation". Any embodiment described as "for example" in the present application is not necessarily construed as being more preferred or having more advantages than other embodiments. In order for any person skilled in the art to implement and use the present invention, the following description is given. In the following description, details are set forth for the purpose of explanation. It should be understood that those of ordinary skill in the art can recognize that the present invention can be implemented without using these specific details. In other instances, well-known structures and processes will not be elaborated in detail so as not to obscure the description of the present invention with unnecessary details. Therefore, the present invention is not intended to be limited to the embodiments shown, but is consistent with the broadest scope that conforms to the principles and features disclosed in the present application.

[0025] Embodiment An air suspension guide arm simulation loading and simulation analysis method includes the following steps: Step 1, establish a CAD digital model of the guide arm loading simulation model, simplify the axle into a circular tube 1, model according to the size of the circular tube 1, and model the upper backing plate 2, the lower backing plate 3, the guide arm 5, the U-bolt 7, the gasket 4 and the upper cover plate 6 according to the actual size; Specifically, the guide arm loading simulation model includes a circular tube 1, an upper backing plate 2, a lower backing plate 3, a guide arm 5, a U-bolt 7, a gasket 4 and an upper cover plate 6. There are two guide arms 5 on the circular tube 1. The circular tube 1 and the guide arm 5 are located in the U-shaped groove of the U-bolt 7 and are fastened by bolts. The upper and lower surfaces of the circular tube 1 located in the U-shaped groove are respectively provided with an upper backing plate 2 and a lower backing plate 3, and a gasket 4 is provided between the upper backing plate 2 and the guide arm 5.

[0026] Step 2: Import the CAD digital model into the finite element analysis software, perform mesh generation on the circular tube 1, upper backing plate 2, lower backing plate 3, guide arm 5, U-bolt 7, gasket 4, and upper cover plate 6, and assign material properties to each component. Specifically, the material of the guide arm 5 is spring steel. The mesh type used is hexahedral mesh, and the mesh is refined in the bending transition area of the guide arm 5, with a mesh size of 2 mm, and the mesh size in the remaining areas is 5 mm. In the embodiment of the present application, the finite element analysis software is Abaqus software, the solver is selected as implicit, and the contact algorithm is the penalty function.

[0027] Step 3, Step 1: Apply an axial pre-tightening force of 100 N to the U-bolt 7; Step 2: Apply the full axial force according to the bolt torque-axial force relationship; Step 3: Keep the bolt at a fixed length, apply vertical loads F1 and F2 to the center of the guide arm ear, and apply vertical loads F7 and F8 to the center of the airbag at the end of the guide arm; Step 4: Keep the bolt at a fixed length, apply longitudinal loads F3 and F4 to the center of the guide arm ear; used to simulate the emergency braking condition; Step 5: Keep the bolt at a fixed length, apply lateral loads F5 and F6 to the center of the guide arm ear; used to simulate the turning lateral force.

[0028] In this embodiment, swapping the order of Steps 3, 4, and 5 does not affect the implementation of the solution of the present invention. Only in the embodiment, the loads are applied in the order of Steps 3, 4, and 5. Applying the loads separately helps with the calculation convergence and smooth loading; at the same time, the stress under unidirectional loads can be obtained.

[0029] Among them, in order to smoothly apply the bolt force, in Steps 1 and 2, the remaining degrees of freedom on both sides of the guide arm 5, gasket 4, and upper cover plate 6 are constrained, and only the vertical degree of freedom is retained.

[0030] In order to achieve calculation convergence, the initial increment step and the maximum increment step need to be set accordingly. The initial increment step in Steps 1 and 2 is set to 0.1, and the initial increment step in Steps 3, 4, and 5 is set to 0.01, and the maximum increment step is set to 0.2.

[0031] Specifically, in Step 3 of this embodiment, the boundary conditions are as follows: both ends of the circular tube 1 are fixed with all degrees of freedom, and the lateral degree of freedom constraints on both sides of the guide arm 5, gasket 4, and upper cover plate 6 are released. Simulate the installation of the axle in the vehicle.

[0032] In Step 3, define the interactions: A bonded constraint is set between the circular tube 1, the upper backing plate 2, and the lower backing plate 3; all of the guide arm 5 and the upper cover plate 6, the guide arm 5 and the gasket 4, and the gasket 4 and the upper backing plate 2 are defined as contacts, and the friction coefficient is set to 0.2 for all of them.

[0033] In Step 3, the basis for load numerical calculation: When applying loads to the guide arm, a vertical load F1 and F2 are applied to the center of the guide arm ear, and a vertical load F7 and F8 are applied to the center of the airbag at the end of the guide arm. It is calculated according to the condition that F1, F2, F7, and F8 jointly bear 2 times the axle load to simulate the full load condition. A longitudinal load F3 and a lateral load F5 are applied to the center of the guide arm ear, and it is calculated according to the theoretical gravitational acceleration of 0.7g. A longitudinal load F4 and a lateral load F6 are applied to the center of the guide arm ear, and it is calculated according to the theoretical gravitational acceleration of 0.4g. By quantifying the loads, it is ensured that the simulated loads are consistent with the actual vehicle conditions, improving the engineering applicability of the results.

[0034] Step 4: Output the simulation results.

[0035] In summary, the present invention solves the problems of low accuracy and difficult convergence in the traditional simulation of the guide arm 5 through vehicle-level modeling, step-by-step loading strategy, parametric constraints, and contact definition.

[0036] Although the embodiments or examples of the present disclosure have been described with reference to the accompanying drawings, it should be understood that the above methods, systems, and devices are merely exemplary embodiments or examples. The scope of the present invention is not limited by these embodiments or examples, but is only defined by the authorized claims and their equivalent scope. Various elements in the embodiments or examples can be omitted or replaced by their equivalent elements. In addition, the steps can be executed in an order different from that described in the present disclosure. Further, various elements in the embodiments or examples can be combined in various ways. Importantly, with the evolution of technology, many elements described herein can be replaced by equivalent elements that appear after the present disclosure.

Claims

1. A simulation analysis method for the air suspension guide arm in the vehicle-mounted state, characterized in that It includes the following steps: Step 1: Establish a CAD digital model of the loading simulation model of the guiding arm. Simplify the axle as a circular tube and model it according to the size of the circular tube. Model the upper backing plate, lower backing plate, guiding arm, U-bolt, gasket and upper cover plate according to the actual size; Step 2: Import the CAD digital model into the finite element analysis software, perform mesh division on the circular tube, upper backing plate, lower backing plate, guiding arm, U-bolt, gasket and upper cover plate, and assign material properties to each; Step 3: Apply an axial pre-tightening force to the U-bolt and gradually load it to the target axial force; Apply loads to the guiding arm, and apply vertical load, longitudinal load and lateral load respectively; Step 4: Output the simulation results.

2. The air suspension guide arm simulation loading and simulation analysis method according to claim 1, wherein The following steps are included in Step 3: Step1: Apply an axial pre-tightening force of 20N - 100N to the U-bolt; Step2: Apply all axial forces according to the bolt torque-axial force relationship; Step3: Keep the bolt at a fixed length, apply vertical loads F1 and F2 to the center of the guiding arm ear, and apply vertical loads F7 and F8 to the center of the airbag at the end of the guiding arm; Keep the bolt at a fixed length, apply longitudinal loads F3 and F4 to the center of the guiding arm ear; Keep the bolt at a fixed length, apply lateral loads F5 and F6 to the center of the guiding arm ear.

3. The air suspension guide arm simulation loading and simulation analysis method according to claim 2, wherein In Step1 and Step2, the initial increment step is set to 0.1; In Step3, the initial increment step is set to 0.01, and the maximum increment step is set to 0.

2.

4. The air suspension guide arm simulation loading and simulation analysis method according to claim 2, wherein In Step1 and Step2, constrain the remaining degrees of freedom on both sides of the guiding arm, gasket and upper cover plate, and only retain the vertical degree of freedom.

5. The air suspension guide arm simulation loading and simulation analysis method according to claim 2, characterized in that, In Step 3, fix all degrees of freedom at both ends of the circular tube, and release the side degree of freedom constraints on both sides of the guiding arm, gasket and upper cover plate.

6. The air suspension guide arm simulation loading and simulation analysis method according to claim 2, wherein In Step 3, set the binding constraints between the circular tube and the upper backing plate and the lower backing plate; Define all contacts between the guiding arm and the upper cover plate, the guiding arm and the gasket, and the gasket and the upper backing plate, and set the friction coefficient to 0.

2.

7. The air suspension guide arm simulation loading and simulation analysis method according to claim 2, characterized in that When applying loads to the guiding arm, apply vertical loads F1 and F2 to the center of the guiding arm ear, apply vertical loads F7 and F8 to the center of the airbag at the end of the guiding arm, and calculate according to the common bearing of 2 times the axle load by F1, F2, F7 and F8; Apply longitudinal load F3 and lateral load F5 to the center of the guiding arm ear, and calculate according to the theory of 0.7g; Apply longitudinal load F4 and lateral load F6 to the center of the guiding arm ear, and calculate according to the theory of 0.4g.

8. The air suspension guide arm simulation loading and simulation analysis method according to claim 1, characterized in that, In Step 2, use hexahedral mesh as the mesh type, and perform mesh encryption in the bending transition area of the guiding arm. The mesh size is 2mm; The mesh size of the remaining areas is 5mm.

9. The air suspension guide arm simulation loading and simulation analysis method according to claim 1, wherein In Step 2, the finite element analysis software is Abaqus software, the solver is selected as implicit, and the contact algorithm is the penalty function.

10. The air suspension guide arm simulation loading and simulation analysis method according to claim 1, characterized in that In Step 1, the loading simulation model of the guiding arm includes a circular tube, an upper backing plate, a lower backing plate, a guiding arm, a U-bolt, a gasket and an upper cover plate; There are two guiding arms on the circular tube. The circular tube and the guiding arm are located in the U-shaped groove of the U-bolt and are fastened by bolts. Upper backing plates and lower backing plates are respectively arranged on the upper and lower surfaces of the circular tube located in the U-shaped groove, and the gasket is arranged between the upper backing plate and the guiding arm.

Images