Automobile dashboard armrest assembly strength cae analysis method
By considering the location and convergence angle of the weld line in the CAE analysis of the automotive sub-dashboard armrest assembly, the problem of not considering the influence of the weld line in the prior art is solved, which improves the analysis accuracy and product strength, reduces costs and risks, and enhances customer satisfaction.
Patent Information
- Application Number
- CN202310000175.1
- Authority / Receiving Office
- CN · China
- Patent Type
- Patents(China)
- Current Assignee / Owner
- Filing Date
- 2023-01-02
- Publication Date
- 2026-01-02
- Estimated Expiration
- 2043-01-02
AI Technical Summary
Existing technologies do not consider the influence of weld lines in injection-molded products in the strength analysis of automotive sub-dashboard armrest assemblies, resulting in insufficient analysis accuracy. This may lead to insufficient strength, abnormal noise, or parts coming off, increasing costs and customer complaints.
By obtaining the mechanical parameters of each component of the handrail assembly regarding the presence or absence of weld lines, the INP material model was edited, and the location and confluence angle of the weld lines were determined using Moldflow and HyperMesh software. CAE simulation analysis was then performed using Abaqus software, taking into account the influence of weld lines on material strength.
This improved the accuracy of strength analysis for automotive sub-dashboard armrest assemblies, reduced testing costs, shortened design cycles, avoided insufficient strength issues, and enhanced product quality and customer experience.
Smart Images
Figure CN115985426B_ABST
Abstract
Description
TECHNICAL FIELD
[0001] The present application relates to a method for analyzing the strength of an automobile component, in particular a method for analyzing the strength of a center console assembly of an automobile instrument panel.
[0002] The center console assembly of an automobile instrument panel not only has a storage function, but also has a decorative effect, and the soft covering gives a sense of comfort. If the strength of the center console assembly is insufficient, abnormal noise may occur during driving, which seriously affects product quality; or the local parts of the center console assembly are partially detached or broken, the opening of the center console is blocked, or even cannot be opened, causing user complaints and increasing customer complaints, and the cost of replacing parts also increases.
[0003] The material model is the basis of CAE analysis, and the material elastic modulus, yield stress, fracture stress and strain mechanical parameters are obtained through spline tensile test. However, the tensile spline with a weld line needs to be redesigned for the injection mold, and the strength of the material with a weld line is generally not tested. At present, during the engineering data design stage of the strength CAE analysis of the center console assembly of an automobile instrument panel, the influence of the weld line of the injection molded product on the material strength is generally not considered. According to the existing literature, the strength of the sample with a weld line is about 50% of the strength of the sample without a weld line. For the strength analysis of functional parts, if there is a weld line in the stress area, the strength of the functional part will decrease by about half. The present application introduces material parameters with different weld line convergence angles in the strength CAE analysis, which can greatly improve the analysis accuracy, avoid the risk of insufficient strength and fracture of the assembly, reduce the subsequent cost of changes, shorten the cycle, reduce the cost, improve the product quality, and enhance the customer's experience. SUMMARY
[0004] The purpose of the present application is to provide a method for analyzing the strength of a center console assembly of an automobile instrument panel, so as to improve the accuracy of the strength analysis of the center console assembly of an automobile instrument panel.
[0005] The method for analyzing the strength of a center console assembly of an automobile instrument panel according to the present application comprises the following steps:
[0006] Step 1: Obtain the mechanical parameters of the materials with and without weld lines of each part of the center console assembly, and edit the INP material model.
[0007] Step 2: Use the 3D data of the center console assembly provided by the product engineer to analyze the mold flow of the key parts of the center console assembly in the Moldflow software, and determine the position and convergence angle of the weld line of the parts.
[0008] Step 3: Convert the 3D data into a finite element model for analysis by modeling with the software HyperMesh.
[0009] Step 4: Perform CAE simulation analysis in the Abaqus software.
[0010] Step 5, analysis result confirmation.
[0011] Step 6, evaluation of the analysis result of Step 5, NO back to Step 3, YES product structure locking.
[0012] The Step 1 includes the following steps:
[0013] Step 1.1, making 1A dumbbell standard sample: making sample with fusion line convergence angle θ of 0°, 45°, 90°, 135° and no fusion line.
[0014] Step 1.2, sample tensile test: clamping 1A dumbbell standard sample on tensile testing machine, setting tensile rate at 1mm / min and 50mm / min respectively, performing tensile test to obtain stress-strain curve of the material.
[0015] Step 1.3, stress-strain curve processing: converting the test obtained engineering stress-strain curve into true stress-strain curve, calculating the elastic modulus, yield stress, breaking stress and plastic strain of the material.
[0016] Step 1.4, CAE simulation sample tensile test: drawing hexahedral mesh of the sample, assigning material parameters of Step 1.3, fixing one end of the sample and applying force on the other end, simulating sample tensile test to obtain CAE analysis stress-strain curve.
[0017] Step 1.5, comparing the coincidence of the two curves of sample tensile CAE analysis stress-strain curve and measured stress-strain curve, NO back to Step 1.1, YES proceeding to next step.
[0018] Step 1.6, editing and saving mechanical property parameters in Hypermesh, exporting INP material model for standby use.
[0019] The Step 2 includes the following steps:
[0020] Step 2.1, geometric model processing: removing free edges, small fillets and small steps in CADdoctor, exporting UDM file.
[0021] Step 2.2, importing the file exported by Step 2.1 into Moldflow, creating mesh model, analyzing and selecting the best gate location, determining the fusion line position and convergence angle.
[0022] The Step 3 includes the following steps:
[0023] Step 3.1, using modeling software HyperMesh, creating finite element mesh of each connecting component, drawing tetrahedron mesh for the handrail base, drawing hexahedron mesh for the metal rotating shaft, and drawing middle surface mesh for other parts.
[0024] Step 3.2, according to the welding line position and the convergence angle of step 2, using the material model obtained in step 1 and the material model in the material library, assigning the material parameters of each part of the automobile auxiliary instrument panel assembly and the material parameters of different welding line convergence angles to the finite element model.
[0025] Step 3.3, creating 1D connecting units connecting each finite element mesh.
[0026] Step 3.4, applying internal load on the handrail assembly and setting the boundary conditions of the auxiliary instrument panel assembly.
[0027] Step 3.5, setting the output and analysis steps.
[0028] Step 3.6, saving the above model and exporting the INP file.
[0029] The step 4 comprises the following contents: importing the INP file of the finite element model of the automobile auxiliary instrument panel assembly into the simulation analysis software Abaqus to run analysis, if the result is error or does not converge, returning to step 3.1 and step 3.3 to check the model, until the displacement and stress visualization cloud diagram is obtained.
[0030] The step 5 comprises the following contents: opening the analysis result ODB file in Abaqus Viewer, separately displaying the handrail outer cover plate, the handrail inner cover plate, the handrail base and the auxiliary instrument panel lower body four parts, checking the stress cloud diagram, and confirming the maximum stress of the corresponding part and the position where the maximum stress appears.
[0031] The step 6 comprises the following contents: comparing the measured stress result with the yield stress of each part of the material, if it is greater than the yield stress of the material, then the structure is optimized, the model is modified, and the step 3 is returned until the analyzed stress is less than the yield stress of the material; if it is less than the yield stress of the corresponding material, then the requirement is met, and the product structure is locked.
[0032] The present application has the following beneficial effects:
[0033] I. The tensile test is carried out on certain PP+EPDM_TD20, and the material strength of the welding line is compared as follows: the tensile strength of the material without welding line (the tensile strength of the material is the yield stress) is 24.3 MPa, the tensile strength of the welding line with a convergence angle of 45° is 12.39 MPa, and the tensile strength of the welding line with a convergence angle of 0° is 11.6 MPa. For the strength analysis of the functional part, if there is a welding line in the stress area, the strength of the functional part will decrease by about half. The CAE analysis method of the application introduces the material strength of the welding line, which can greatly improve the accuracy of the strength analysis of the automobile center console assembly.
[0034] II. Since the tensile sample with a welding line needs to be redesigned, the material strength with a welding line is not generally tested, so the conventional CAE analysis does not consider the influence of the product welding line on the material strength. The CAE analysis method of the application introduces the material model of the welding line into the finite element model, improves the reliability of the strength analysis of the automobile center console assembly, and basically replaces the late DV test of the strength of the center console assembly, thereby reducing the test cost.
[0035] III. The CAE analysis method of the application is applied to the strength analysis in the project data design stage, which can find the problem of insufficient strength of the center console assembly in advance, solve the problem in the early stage, avoid the risk of fracture of the center console, reduce the cost of later changes and shorten the rectification period. BRIEF DESCRIPTION OF DRAWINGS
[0036] Figure 1 The CAE analysis method of the automobile center console assembly of the application is a flow chart.
[0037] Figure 2 The explosion diagram of the automobile center console assembly.
[0038] Figure 3 The schematic diagram of the 1A dumbbell-shaped standard sample of the application.
[0039] Figure 4 The tensile test schematic diagram of the electronic universal testing machine involved in the application.
[0040] Figure 5 The schematic diagram of the material welding line convergence angle of the application.
[0041] Figure 6 The schematic diagram of the material welding line scanning section of the application.
[0042] Figure 7 The corresponding schematic diagram of the node at the shaft hole matching position of the automobile center console assembly.
[0043] Figure 8 The structure schematic diagram of the center console base and the metal shaft of the automobile center console assembly.
[0044] Figure 9 This is a detailed schematic diagram of the mesh refinement of the armrest base at the shaft hole mating point of the automotive sub-instrument armrest assembly.
[0045] Figure 10 This is a schematic diagram of the load loading on the automotive sub-dashboard armrest assembly. Detailed Implementation
[0046] The present invention will now be described in further detail with reference to the accompanying drawings.
[0047] like Figure 2 The model shown is a 3D model of the automotive sub-instrument assembly, including armrest assembly 1, rear air duct rear section assembly 2, sub-instrument left side accessory assembly 3, sub-instrument left side panel assembly 4, sub-instrument front connecting plate 5, sub-instrument lower body frame 6, sub-instrument upper body frame 7, sub-instrument right side accessory assembly 8, and sub-instrument right side panel assembly 9. The input data must include wall thickness, flange, reinforcing ribs, and installation positioning structure and distribution.
[0048] The accuracy of CAE analysis is related to the material model, finite element mesh model, internal connectivity, boundary conditions, and loading conditions. To improve analysis accuracy, each of these factors should be carefully considered to ensure the simulation closely approximates the actual state. Specific analysis methods are as follows:
[0049] Step 1: Obtain the mechanical parameters of each part of the armrest assembly with and without weld lines, and edit the INP material model.
[0050] Step 1.1: Prepare as shown in the attached document. Figure 3 The 1A dumbbell-shaped standard template 10 shown is obtained by arranging different gate positions when designing the stretch template for the injection mold to obtain weld line templates. After the mold is processed, the injection molding process is adjusted to obtain 1A dumbbell-shaped standard templates 10 with weld line confluence angles θ of 0°, 45°, 90°, 135° and no weld line.
[0051] Step 1.2, Spatial Tensile Test: Clamp the 1A dumbbell-shaped standard spatula 10 in the... Figure 4 On the tensile testing machine shown, an extensometer is placed at the gauge length of the specimen, and tensile rates of 1 mm / min and 50 mm / min are set to conduct tensile tests to obtain the stress-strain curves of the material.
[0052] Step 1.3, Stress-Strain Curve Processing: Based on the curve transformation formula, the experimentally obtained engineering stress-strain curve is transformed into a real stress-strain curve, and the elastic modulus, yield stress, fracture stress, and plastic strain of the material are calculated.
[0053] Step 1.4, CAE simulation tensile test of sample: using Catia software, according to the measured sample size, draw the 3D data of 1A dumbbell-shaped standard sample 10. Open HyperMesh software, import sample 3D data, draw hexahedral mesh, assign material parameters in step 1.3 to sample finite element mesh, fix one end of the sample and apply force to the other end, simulate tensile test of sample, and get CAE analysis stress-strain curve.
[0054] Step 1.5, compare the coincidence of the two curves of tensile CAE analysis stress-strain curve and measured stress-strain curve, NO go back to step 1.1, YES go to the next step.
[0055] Step 1.6, edit and save the mechanical property parameters obtained in step 1.3 in Hypermesh, export INP material model for future use.
[0056] Step 2, use the 3D data of automobile instrument panel assembly provided by product engineers to analyze the flow of mold in Moldflow software for each key part of the armrest assembly, and determine the position of the weld line and the convergence angle.
[0057] The material strength at the weld line is only about 50% of the actual strength of the material, or even lower. When two or more melts converge in the mold cavity, the temperature, pressure, and viscosity of each melt are different, and the melts cannot effectively mix and entangle, resulting in different convergence angles of the weld marks on the product, as shown in Figure 5 , a linear mark appears on the surface of the plastic part, and a V-shaped groove is formed in the cross section, as shown in Figure 6 .
[0058] Step 2.1, geometric model processing: open the 3D data of the armrest inner and outer cover plate, armrest base 14 and instrument panel lower body skeleton 6 in Catia software, and export the igs format file. Import igs file in CADdoctor, process free edge, small fillet and small step features, and export UDM file.
[0059] Step 2.2, import the file exported in step 2.1 into Moldflow, create a mesh model, analyze and select the best gate location, and determine the weld line position and convergence angle.
[0060] Step 3, modeling by software HyperMesh, convert 3D data to finite element model for analysis.
[0061] Step 3.1, use modeling software HyperMesh to create finite element mesh of each connection component, where the armrest base 14 is drawn as a tetrahedral mesh, the metal shaft 15 is drawn as a hexahedral mesh, and the other parts are drawn as a mid-surface mesh.
[0062] Metallic pivot 15 model units should be hexahedral elements, and the nodes of the metallic pivot 15 should correspond to the nodes of the hole positions of the handrail base 14, as shown in Figure 7 .
[0063] Because the cantilever of the handrail base 14 and the metallic pivot 15 is long, as shown in Figure 8 , the cantilever is likely to be broken under stress, and the stress distribution of the shaft hole matching position should be considered in the analysis, and the following points should be noted in the modeling:
[0064] a. The grid size of the handrail base 14 is 2mm, and the grid of the shaft hole matching position is refined, as shown in Figure 9 , with a size of 1mm.
[0065] b. The contact connection should be built at the hole matching position of the handrail base 14 and the metallic pivot 15, and the gap between the handrail base 14 and the metallic pivot 15 should be ensured to prevent the shaft from penetrating the base during rotation (the single-sided gap is controlled within 0.05mm), and the nodes correspond to each other.
[0066] Step 3.2, using the material model obtained in step 1 and the material model in the material library, assign the material parameters of each part of the automobile instrument panel assembly to the finite element model in HyperMesh software. For the fusion line area of the handrail base 14, the inner cover plate of the handrail and the lower body skeleton 6 of the instrument panel, according to the fusion line position and convergence angle obtained in step 2, assign the corresponding fusion line material model to the five rows of grids in the fusion line area.
[0067] Step 3.3, create 1D connection units connecting each finite element grid: view the installation point position relationship of each part of the instrument panel assembly in CATIA software, and establish connections in HyperMesh software according to the assembly relationship of each part.a. The installation structure is bolt / screw: 1D connection unit restricts 1-6 degrees of freedom;b. The installation structure is V-shaped card: 1D connection unit restricts 1-6 degrees of freedom, and other self-cards are released according to the actual assembly situation.
[0068] Step 3.4, apply internal load to the handrail assembly 1 and set the boundary conditions of the instrument panel assembly.
[0069] Load application: In HyperMesh software, apply Z-direction load to the middle area of the handrail outer cover plate, as shown by the arrow. Figure 10 .
[0070] Set boundary conditions: Fix 1-6 degrees of freedom of the instrument panel mounting bracket and the floor, and the connection point of the instrument panel assembly and CCB, release the X-direction translation freedom and Y-direction rotation freedom of the front end of the instrument panel assembly, and fix the freedom in other directions.
[0071] Step 3.5, setting output and analysis step.
[0072] Setting output: Set the node output as displacement U and the element output as stress S and plastic strain PE in HyperMesh software.
[0073] Setting analysis step: Select the analysis step solver parameter as Static static analysis in HyperMesh software, check the internal load, boundary condition options and output.
[0074] Step 3.6, save the above model and export INP analysis file.
[0075] Step 4, CAE simulation analysis in Abaqus software.
[0076] Import the INP file of the finite element model of the automobile auxiliary instrument panel assembly into the simulation analysis software Abaqus, run the analysis, if error or non-convergence occurs during the analysis, return to step 3.1 and / or step 3.3 to check the model, until the displacement and stress visualization cloud diagram is obtained.
[0077] Step 5, analysis result confirmation.
[0078] In Abaqus Viewer, open the analysis result ODB file, separately display the armrest outer cover plate, auxiliary instrument panel lower body skeleton 6, armrest base 14 and armrest inner cover plate four parts, view the stress cloud diagram, and confirm the maximum stress of the corresponding parts and the position where it appears.
[0079] Step 6, compare the stress results measured in step 5 with the yield stress of each part material, if greater than the yield stress of the material, then optimize the structure, modify the model, return to step 3.1 and / or 3.3 to modify the model, until the analyzed stress is less than the yield stress of the material; if less than the yield stress of the corresponding material, then it meets the requirements, and the product structure is locked.
Claims
1. A method for CAE analysis of strength of an automobile instrument panel armrest assembly, characterized in that, The method comprises the following steps: Step 1, obtaining the mechanical parameters of each part of the armrest assembly with or without a weld line, and editing an INP material model; Step 2, using the 3D data of the automobile auxiliary instrument panel assembly provided by a product engineer, performing mold flow analysis on the key parts of the armrest assembly in the Moldflow software to determine the position of the weld line and the convergence angle of the parts; Step 3, modeling by using the software HyperMesh, and converting the 3D data into a finite element model for analysis; Step 4, performing CAE simulation analysis in the Abaqus software; Step 5, confirming the analysis result; Step 6, evaluating the analysis result of Step 5, NO returning to Step 3, and YES locking the product structure; The step 1 comprises the following steps: Step 1.1, making 1A dumbbell-shaped standard samples: making samples with weld line convergence angles θ of 0°, 45°, 90°, 135° and without a weld line; Step 1.2, sample tensile test: clamping the 1A dumbbell-shaped standard sample on a tensile testing machine, setting the tensile rate to be 1 mm / min and 50 mm / min respectively, and performing tensile test to obtain the stress-strain curve of the material; Step 1.3, stress-strain curve processing: converting the engineering stress-strain curve obtained by the test into a true stress-strain curve, and calculating the elastic modulus, yield stress, fracture stress and plastic strain of the material; Step 1.4, CAE simulation sample tensile test: drawing a hexahedral mesh for the sample, assigning the material parameters of Step 1.3, fixing one end of the sample and applying force to the other end, simulating the sample tensile test, and obtaining the CAE analysis stress-strain curve; Step 1.5, comparing the coincidence of the CAE analysis stress-strain curve and the measured stress-strain curve of the sample tensile test, NO returning to Step 1.1, and YES proceeding to the next step; Step 1.6, editing and saving the mechanical property parameters in HyperMesh, and exporting the INP material model for standby use; The step 2 comprises the following steps: Step 2.1, geometric model processing: removing free edges, small fillets and small steps in CADdoctor, and exporting a UDM file; Step 2.2, importing the file exported in Step 2.1 into Moldflow, creating a mesh model, analyzing and selecting the best gate location, and determining the weld line position and convergence angle.
2. The automotive dashboard armrest assembly strength CAE analysis method of claim 1, wherein, The step 3 comprises the following steps: Step 3.1, using the modeling software HyperMesh to create a finite element mesh of each connecting component, wherein a tetrahedral mesh is drawn for the armrest base, a hexahedral mesh is drawn for the metal shaft, and a middle mesh is drawn for other parts; Step 3.2, according to the weld line position and convergence angle of Step 2, using the material model obtained in Step 1 and the material model in the material library, assigning the material parameters of each part of the automobile auxiliary instrument panel assembly and the material parameters of different weld line convergence angles to the finite element model; Step 3.3, creating 1D connecting units connecting the finite element meshes; Step 3.4, applying internal loads to the armrest assembly and setting the boundary conditions of the auxiliary instrument panel assembly; Step 3.5, setting the output and analysis steps; Step 3.
6. Save the above model, export INP file.
3. The automotive dashboard armrest assembly strength CAE analysis method of claim 1, wherein, The step 4 includes the following contents: The INP file of the finite element model of the automobile auxiliary instrument panel assembly is imported into the simulation analysis software Abaqus for analysis, if the result is error or does not converge, return to step 3.1 and step 3.3 to check the model, until the displacement and stress visualization cloud chart is obtained.
4. The automotive dashboard armrest assembly strength CAE analysis method of claim 1, wherein, The step 5 includes the following contents: In Abaqus Viewer, open the analysis result ODB file, respectively and individually display the armrest outer cover plate, armrest inner cover plate, armrest base and auxiliary instrument panel lower body four parts, view the stress cloud chart, and confirm the maximum stress of the corresponding part and the position where it appears.
5. The automotive dashboard armrest assembly strength CAE analysis method of claim 1, wherein, The step 6 includes the following contents: Compare the measured stress result with the yield stress of each part material, if it is greater than the yield stress of the material, then optimize the structure, modify the model, return to step 3, until the analyzed stress is less than the yield stress of the material; If it is less than the yield stress of the corresponding material, it meets the requirement, and the product structure is locked.