A method for analyzing durability of a rear towing device of an automobile

Abstract

The present application relates to a kind of automobile rear tow device durability analysis method, comprising the following steps: based on three-dimensional geometric data establishment white body finite element model and rear tow device finite element model, connect white body finite element model and rear tow device finite element model, intercept a part of white body, and rear tow device is installed on white body by bolt, and contact pair is formed in the sheet metal connecting area of white body and rear tow device durability finite element model;Constraint and target load are applied to the durability finite element model, and solving calculation is carried out, obtains stress result file, imports fatigue software into stress result file, and outputs fatigue result damage value;Compare fatigue result damage value and preset damage target value, and the fatigue result damage value that does not meet the requirement is optimized in combination with risk position.The present application can quickly, effectively and low cost predict the durability life of rear tow device body under dynamic, and the sheet metal, welding point and weld of white body installed.

Description

Technical Field

[0001] This invention relates to the field of computer-aided technology, and more specifically to a method for analyzing the durability of a car's rear towing device. Background Technology

[0002] With the continuous increase in per capita household income and consumption capacity in my country, domestic automobile sales are showing a sustained upward trend. Against this backdrop, the requirements for overall automobile performance are also increasing. Improving the overall safety performance of automobiles has become one of the most important research directions for automotive engineers. For automobiles, a rear-end towing device is installed at the rear of the vehicle for practical application. It consists of a mounting base, towing crossbeam, and towing ball joint, and is mainly used for towing RVs, motorboats, luggage compartments, and roadside assistance. Based on travel safety considerations, the reliability requirements for this device are extremely high. The state has issued relevant testing regulations, requiring high strength and durability of the rear-end towing device and its related mounting structures. Due to the long testing cycle, high cost, and limited visibility of products, with the maturity of finite element technology, the development of rear-end towing devices can be improved by using CAE simulation analysis to analyze its strength and durability performance during the design phase, allowing for structural optimization and iteration, thereby improving development efficiency.

[0003] For example, patent document CN108520118A discloses a method for analyzing the strength of a car tow hook. The method includes the following steps: performing a comprehensive scan of the car body and the tow hook; establishing a finite element model based on the scan data; calculating the target load corresponding to the tow hook under different working conditions according to a preset load formula; loading the target load into the finite element model and solving the finite element model to obtain the residual strain corresponding to the mounting point of the tow hook; and outputting the analysis data of the finite element model when the residual strain is determined to be within a preset strain range. This method for analyzing the strength of a car tow hook can ensure that the strength data of the tow hook meets preset standards, improving the overall safety factor of the product. However, this method only examines the static strength condition of the tow hook and is only a description of static load loading. The actual working state of the tow hook is dynamic, and ultimately, durability performance should be examined. Therefore, this method is not perfect.

[0004] Therefore, it is necessary to develop a new method for analyzing the durability of automotive rear-towing devices. Summary of the Invention

[0005] One of the objectives of this invention is to provide a method for analyzing the durability of a vehicle's rear towing device, which can quickly, effectively, and at low cost predict the durability of the rear towing device body and its mounted body-in-white sheet metal, weld points, and weld seams under dynamic conditions.

[0006] To achieve the above objectives, the present invention adopts the following technical solution: a method for analyzing the durability performance of a vehicle rear towing device, comprising the following steps:

[0007] S1. Based on three-dimensional geometric data, a finite element model of the body-in-white is established, and the weld points, structural adhesives, bolts and welds of the body-in-white are connected according to their actual positions.

[0008] S2, a finite element model of the rear towing device is established using three-dimensional geometric data, and the trailer ball joint, weld, bolts and the body of the rear towing device are connected according to the actual position;

[0009] S3, connect the finite element model of the white body and the finite element model of the rear towing device;

[0010] S4, cut off a part of the white body, install the rear towing device on the white body with bolts, and set contact pairs in the sheet metal connection area between the white body and the rear towing device to form a durability finite element model;

[0011] S5, apply constraints and target loads to the durability finite element model, solve the durability finite element model with applied constraints and target loads, obtain stress result files, import the stress result files into fatigue software, and output the fatigue result damage values ​​of sheet metal, weld points and welds respectively.

[0012] S6 compares the fatigue damage value with the preset damage target value, and optimizes the weld location, material grade, material thickness and sheet metal structure based on the risk location for fatigue damage values ​​that do not meet the requirements.

[0013] Based on the aforementioned technical methods, finite element simulation was used to establish and connect finite element models of the body-in-white and the rear towing device. Then, contact pairs were set up in the sheet metal connection area to form a durability finite element model, and constraints and target loads were applied. Fatigue results were solved and calculated. The results were compared with the target values ​​to see if they met the requirements. Thus, a rapid, effective, and low-cost method was achieved to predict the durability of the rear towing device body and its mounted body-in-white sheet metal, weld points, and weld seams under dynamic conditions.

[0014] Furthermore, S1 specifically includes: based on three-dimensional geometric data, extracting the mid-surface of the sheet metal structure of the body-in-white, dividing it into shell meshes to form an inp file, wherein the inp file includes mesh node information of sheet metal, weld points, weld seams, structural adhesive, and bolts.

[0015] Furthermore, S2 specifically includes:

[0016] S21, extract the middle surface of the sheet metal structure of the rear drag device and divide it into shell mesh;

[0017] S22, the trailer ball joint of the rear towing device is meshed using tetrahedral solid elements.

[0018] Furthermore, S3 specifically includes: the bolts, structural adhesive, weld points and welds in the finite element model of the white body and the finite element model of the rear towing device are simulated using RBE2 rigid elements, hexahedral elements + RBE3 flexible elements, shell elements - Bar elements - shell elements and shell elements, respectively.

[0019] Furthermore, S4 specifically includes: the sheet metal of the rear towing device as the main contact surface, the sheet metal of the body-in-white as the secondary contact surface, the sheet metal connection area between the body-in-white and the rear towing device is connected by a surface-to-surface contact pair, and a contact friction coefficient is set.

[0020] Furthermore, S5 specifically includes:

[0021] S51, constrains the degrees of freedom of the body-in-white section 123456;

[0022] S52, apply a cyclic load along the X direction of the body-in-white at the center point of the trailer ball joint, calculate and solve, and output the stress result file. The cyclic load is 0.6D.

[0023] S53 imports the stress result file and the inp file containing mesh node information of sheet metal, weld points, and weld seams into the fatigue software to solve for fatigue damage values.

[0024] Furthermore, the coefficient of contact friction between the body-in-white and the rear towing device is 0.15.

[0025] Furthermore, the body of the rear towing device is made of a nonlinear material with a stress-strain curve obtained from experiments.

[0026] Furthermore, S1 and S2 are modeled using Ansa or Hypermesh modeling software to establish finite element models.

[0027] Furthermore, the software used to solve the stress in the durability finite element model is Abaqus, and the fatigue software is Femfat.

[0028] The beneficial effects of this invention are as follows: By establishing separate finite element models of the body-in-white and the rear towing device, and then connecting the two models and extracting a portion of the body-in-white, the rear towing device is mounted on the body-in-white using bolts. Contact pairs are then established in the sheet metal connection area between the body-in-white and the rear towing device to form a durability finite element model. Constraints and target loads are applied to the durability finite element model, and the results are calculated to obtain stress result files. Fatigue damage values ​​of the sheet metal, weld points, and weld seams are output separately. This invention can quickly, effectively, and cost-efficiently predict the durability life of the rear towing device body and the sheet metal, weld points, and weld seams of the body-in-white under dynamic conditions. Attached Figure Description

[0029] Figure 1 This is a flowchart of the present invention; Detailed Implementation

[0030] The embodiments of the present invention will be described below with reference to the accompanying drawings and preferred embodiments. Those skilled in the art can easily understand other advantages and effects of the present invention from the content disclosed in this specification. The present invention can also be implemented or applied through other different specific embodiments, and various details in this specification can also be modified or changed based on different viewpoints and applications without departing from the spirit of the present invention. It should be understood that the preferred embodiments are only for illustrating the present invention and not for limiting the scope of protection of the present invention.

[0031] It should be noted that the illustrations provided in the following embodiments are only schematic representations of the basic concept of the present invention. Therefore, the drawings only show the components related to the present invention and are not drawn according to the actual number, shape and size of the components in the actual implementation. In the actual implementation, the form, quantity and proportion of each component can be arbitrarily changed, and the layout of the components may also be more complex.

[0032] See Figure 1 This embodiment provides a method for analyzing the durability of a vehicle's rear towing device, including the following steps:

[0033] S1. Based on three-dimensional geometric data, a finite element model of the body-in-white is established, and the weld points, structural adhesives, bolts and welds of the body-in-white are connected according to their actual positions.

[0034] S2, a finite element model of the rear towing device is established using three-dimensional geometric data, and the trailer ball joint, weld, bolts and the body of the rear towing device are connected according to the actual position;

[0035] S3, connect the finite element model of the white body and the finite element model of the rear towing device;

[0036] S4, cut off a part of the white body, install the rear towing device on the white body with bolts, and set contact pairs in the sheet metal connection area between the white body and the rear towing device to form a durability finite element model;

[0037] S5, apply constraints and target loads to the durability finite element model, solve the durability finite element model with applied constraints and target loads, obtain stress result files, import the stress result files into fatigue software, and output the fatigue result damage values ​​of sheet metal, weld points and welds respectively.

[0038] S6 compares the fatigue damage value with the preset damage target value, and optimizes the weld location, material grade, material thickness and sheet metal structure based on the risk location for fatigue damage values ​​that do not meet the requirements.

[0039] In this implementation, the preset damage target value is set to 0.5. If the fatigue damage value is less than 0.5, it is considered unacceptable and the structure needs optimization; otherwise, it is acceptable. The main optimization methods depend on the location of the risk, such as modifying local sheet metal features, increasing material thickness, upgrading material grade, and rearranging weld points. After optimization, steps S1 to S6 are repeated until the design requirements are met.

[0040] In this embodiment, S1 specifically includes the following steps:

[0041] Based on three-dimensional geometric data, the mid-surface of the sheet metal structure of the body-in-white is extracted and shell mesh is generated to form an inp file. The inp file includes mesh node information of sheet metal, weld points, weld seams, structural adhesive and bolts.

[0042] In this embodiment, S2 specifically includes the following steps:

[0043] S21, extract the middle surface of the sheet metal structure of the rear drag device and divide it into shell mesh;

[0044] S22, the trailer ball joint of the rear towing device is meshed using tetrahedral solid elements.

[0045] In this embodiment, S3 specifically includes the following steps:

[0046] Bolts, structural adhesive, weld points, and weld seams in the finite element models of the body-in-white and the rear towing device are simulated using RBE2 rigid elements, hexahedral elements + RBE3 flexible elements, shell elements - Bar elements - shell elements, and shell elements, respectively.

[0047] Preferably, the grid size of the rear towing device and the connection point with the body-in-white should not exceed 4mm. The grid size for the body-in-white is generally controlled at 8mm, primarily balancing computational efficiency and accuracy. A larger grid size results in fewer grid cells, thus leading to faster computation but lower accuracy. Conversely, a smaller grid size results in more grid cells, thus leading to slower computation but higher accuracy. Therefore, a grid size of 4mm is more suitable.

[0048] In this embodiment, S4 specifically includes the following steps:

[0049] The sheet metal of the towing device is the primary contact surface, and the sheet metal of the body-in-white is the secondary contact surface. The connection area between the sheet metal of the body-in-white and the towing device is connected by surface-to-surface contact, and a contact friction coefficient is set. Preferably, the contact friction coefficient between the body-in-white and the towing device is 0.15.

[0050] In this embodiment, S5 specifically includes the following steps:

[0051] S51, constrains the degrees of freedom of the body-in-white section 123456;

[0052] S52, apply a cyclic load along the X direction of the vehicle body at the center point of the trailer ball joint, calculate and solve the stress results file. Preferably, the cyclic load is 0.6D. The cyclic load here can be a static load specified in relevant standards or a dynamic load collected from experiments. There is no specific limitation.

[0053] S53 imports the stress result file and the inp file containing mesh node information of sheet metal, weld points and weld seams into the fatigue software to solve for fatigue damage values.

[0054] Additionally, in S2 and S3, it is important to import the stress result file distribution into FEMFAT, select the BASIC module, and choose upper and lower operating conditions. Then, check the Gaussian influence option within the software and check SPOT to start weld fatigue calculation. Define the weld type, set the output file format, and conduct fatigue analysis. This is common knowledge to those skilled in the art and will not be elaborated further.

[0055] In this embodiment, the body of the rear dragging device is made of a nonlinear material with a stress-strain curve obtained from experiments.

[0056] In this embodiment, the software used to build the finite element model is ANSA or Hypermesh. The software used to solve the stress in the durability finite element model is Abaqus, and the software used for fatigue is Femfat.

[0057] The sheet metal work described in this article is a comprehensive cold working process for thin metal sheets, including shearing, punching / cutting / compound cutting, bending, welding, riveting, splicing, forming, etc., such as the car body in this application, the main purpose of which is to distinguish the weld points from other metal parts.

[0058] In the description of this specification, references to terms such as "one embodiment," "some embodiments," "example," "specific example," or "some examples," etc., indicate that a specific feature, structure, material, or characteristic described in connection with that embodiment or example is included in at least one embodiment or example of the invention. In this specification, the illustrative expressions of the above terms do not necessarily refer to the same embodiment or example. Furthermore, the specific features, structures, materials, or characteristics described may be combined in any suitable manner in one or more embodiments or examples.

[0059] Although embodiments of the invention have been shown and described, those skilled in the art will understand that various changes, modifications, substitutions and alterations can be made to these embodiments without departing from the principles and spirit of the invention, the scope of which is defined by the claims and their equivalents.

Claims

1. A method for analyzing the durability performance of a vehicle's rear towing device, characterized in that, Includes the following steps: S1. Based on three-dimensional geometric data, a finite element model of the body-in-white is established, and the weld points, structural adhesives, bolts and welds of the body-in-white are connected according to their actual positions. S2, a finite element model of the rear towing device is established using three-dimensional geometric data, and the trailer ball joint, weld, bolts and the body of the rear towing device are connected according to the actual position; S3, connect the finite element model of the body-in-white and the finite element model of the rear towing device; the bolts, structural adhesive, weld points and welds in the finite element models of the body-in-white and the rear towing device are simulated using RBE2 rigid elements, hexahedral elements + RBE3 flexible elements, shell elements - Bar elements - shell elements and shell elements, respectively; S4, cut off a part of the white body, install the rear towing device on the white body with bolts, and set contact pairs in the sheet metal connection area between the white body and the rear towing device to form a durability finite element model; S5, apply constraints and target loads to the durability finite element model. The target load is a cyclic load applied along the X direction of the body-in-white at the center point of the trailer ball joint. Solve the durability finite element model with the applied constraints and target loads to obtain a stress result file. Import the stress result file into fatigue software and output the fatigue result damage values ​​of sheet metal, weld points, and weld seams respectively. S6, compare the fatigue result damage values ​​with the preset damage target values. For fatigue result damage values ​​that do not meet the requirements, optimize the weld point position, material grade, material thickness, and sheet metal structure in conjunction with the risk location.

2. The method for analyzing the durability of a vehicle's rear towing device according to claim 1, characterized in that, S1 specifically includes: based on three-dimensional geometric data, extracting the mid-surface of the sheet metal structure of the body-in-white, dividing it into shell meshes to form an inp file, wherein the inp file includes mesh node information of sheet metal, weld points, weld seams, structural adhesives and bolts.

3. The method for analyzing the durability of a vehicle's rear towing device according to claim 1, characterized in that, S2 specifically includes: S21, extract the middle surface of the sheet metal structure of the rear drag device and divide it into shell mesh; S22, the trailer ball joint of the rear towing device is meshed using tetrahedral solid elements.

4. The method for analyzing the durability of a vehicle's rear towing device according to claim 1, characterized in that, S4 specifically includes: the sheet metal of the rear towing device is the main contact surface, the sheet metal of the body-in-white is the secondary contact surface, the sheet metal connection area between the body-in-white and the rear towing device is connected by surface-to-surface contact, and a contact friction coefficient is set.

5. The method for analyzing the durability of a vehicle's rear towing device according to claim 2, characterized in that, S5 specifically includes: S51, constrains the degrees of freedom of the body-in-white section 123456; S52, apply a cyclic load along the X direction of the body-in-white at the center point of the trailer ball joint, calculate and solve, and output the stress result file. The cyclic load is 0.6D. S53 imports the stress result file and the inp file containing mesh node information of sheet metal, weld points, and weld seams into the fatigue software to solve for fatigue damage values.

6. The method for analyzing the durability of a vehicle's rear towing device according to claim 4, characterized in that, The coefficient of contact friction between the body-in-white and the rear towing device is 0.

15.

7. The method for analyzing the durability of a vehicle rear towing device according to any one of claims 1 to 6, characterized in that, The rear towing device body is made of a nonlinear material with a stress-strain curve obtained from experiments.

8. The method for analyzing the durability of a vehicle rear towing device according to any one of claims 1 to 6, characterized in that, The S1 and S2 models are established using Ansa or Hypermesh modeling software.

9. The method for analyzing the durability of a vehicle rear towing device according to any one of claims 1 to 6, characterized in that, The software used to solve the stress in the durability finite element model is Abaqus, and the software used to solve the fatigue problem is Femfat.

Images