ANSYS-based automobile instrument drop simulation analysis method

Abstract

The invention discloses an ANSYS-based automobile instrument drop simulation analysis method, which comprises the following steps of: preprocessing a 3D model of an automobile instrument assembly, separating chips and pins on a PCB (Printed Circuit Board) in the 3D model, and carrying out common node connection; discretizing the preprocessed 3D model to draw an initial grid; a connection relation is established, and the chip pins are connected with the PCB through welding spots; mesh refinement is carried out on the 3D model of the automobile instrument assembly and all chips in the 3D model, an explicit linear mesh is adopted as the overall mesh of the 3D model of the automobile instrument assembly, and a hexahedral mesh is adopted at the corresponding contact position of each chip pin and a PCB; a local coordinate system is established, a rigid wall is established with the plane of the local coordinate system as the reference, and the rigid wall is used for simulating the ground; an initial speed and a gravity field when the 3D model falls to the rigid wall are applied to the preprocessed 3D model, then a stress result and a deformation result after the 3D model falls to the rigid wall are calculated in a simulation mode, and the initial speed is related to the falling height.

Description

Technical Field

[0001] The present invention relates to the technical field of drop simulation, and particularly to a method for analyzing the drop simulation of an automotive instrument based on ANSYS. Background Art

[0002] With the development of the technological process, electronic products are more widely used, more powerful in function, and smaller in volume. This means that the electronic components in them are smaller in size and more in number. However, there is an inevitable risk of dropping during product production, transportation, or daily use, which poses a significant test to the reliability of the products. For this reason, more and more manufacturers will verify the drop reliability of their products before leaving the factory.

[0003] Currently, there are mainly two methods for verifying the drop reliability of products: One is to conduct simulated drop tests on actual products under different scenarios (drop angles, heights, speeds, etc.), observe and detect whether the appearance and functions of the products are normal, and check whether the internal parts of the products are damaged after disassembly. Since this test often needs to be carried out repeatedly, the test cost is relatively high, and the products need to be disassembled after the test, resulting in a high time cost. Moreover, the product may be damaged secondarily during the disassembly process, making the test results unreliable. The second is to simulate the drop process of the product through a computer and analyze the product reliability through post-processing results. This method basically solves the problems of high cost, long time, and easy secondary damage of the first method. However, in view of the common simulation analysis methods on the market currently, most of the connections between electronic components and the main board use co-nodes, bindings, link pairs, or RBE2, and the meshes are mainly tetrahedrons. This ignores the problem of the soldering strength of the pins of the electronic components, resulting in a decrease in the accuracy of the results and unreliable results. Therefore, this method is not widely used in the field of automotive instruments. Summary of the Invention

[0004] Based on the above situation, the main purpose of the present invention is to provide a method for analyzing the drop simulation of an automotive instrument based on ANSYS, which can better simulate the soldering situation of the pins of the electronic components, reflect the true strength of the connection points, have good mesh quality, fast calculation and simulation speed for multiple times, save time costs, and improve the accuracy and universality of this method.

[0005] To achieve the above object, the technical solution adopted by the present invention is as follows:

[0006] A method for analyzing the drop simulation of an automotive instrument based on ANSYS, comprising the steps of:

[0007] S100, preprocess the 3D model of the automotive instrument assembly. Among them, separate each chip and pin on the PCB board in the 3D model and perform co-node connection;

[0008] S200, discretize the preprocessed 3D model to draw an initial mesh;

[0009] S300, establish a connection relationship, wherein the chip pins and the PCB board are connected by solder joints;

[0010] S400, refine the meshes of the 3D model of the automotive instrument assembly and each chip therein. Among them, the overall mesh of the 3D model of the automotive instrument assembly uses explicit linear meshes, and the corresponding contact positions between each chip pin and the PCB use hexahedral meshes;

[0011] S500, establish a local coordinate system, and establish a rigid wall based on the local coordinate system plane. The rigid wall is used to simulate the ground;

[0012] S600, apply the initial velocity and gravitational field when the preprocessed 3D model falls onto the rigid wall, and then simulate and calculate the stress results and deformation results of the 3D model after falling onto the rigid wall. Among them, the initial velocity is related to the height of the fall.

[0013] Preferably, the step S100 further includes:

[0014] Simplify the chamfers and excessive fillets with a diameter less than 1 mm of the plastic parts in the 3D model to make the 3D model interference-free and error-free.

[0015] Preferably, the step S200 further includes:

[0016] If the initial mesh generation fails and it is caused by the 3D model, return to the step S100 to process the model to confirm that the 3D model data meets the finite element analysis standard.

[0017] Preferably, for the solder joint connection between the chip pins and the PCB board in the step S300, the normal stress limit is 50 MPa, the shear stress limit is 30 MPa, the normal and tangential stress exponents are both 1, and the welding diameter is 0.8 mm.

[0018] Preferably, the step S300 further includes:

[0019] Use Bonding connection for the appearance parts connected by adhesive;

[0020] Use Bonding connection for the threaded parts of the components connected by bolts and insert the bolt pre-tightening force.

[0021] Preferably, for the Bonding connection of the appearance parts connected by adhesive, the maximum offset is 0.1 mm, and for the Bonding connection of the threaded parts of the components connected by bolts, the inserted bolt pre-tightening force is 85 N, and the duration is 0.3 s.

[0022] Preferably, in step S600, it is determined whether the parts of the 3D model are broken, whether the chip pins are broken, and / or whether the solder joint connection parts are de-soldered based on the stress result and the deformation result.

[0023] Preferably, step S600 further includes:

[0024] Determining whether the 3D model of the automotive instrument assembly is qualified based on the proportion of hourglass energy of the 3D model.

[0025] The present invention also discloses an electronic device, including a memory, a processor, and a computer program stored on the memory and executable on the processor. When the processor executes the computer program, the steps of any method of the present invention are implemented.

[0026] The present invention also discloses a computer-readable storage medium storing machine-executable instructions. When the machine-executable instructions are called and run by a processor, the machine-executable instructions cause the processor to run any method of the present invention.

[0027] The technical solution of the present invention aims at the problem of poor accuracy caused by the simplification of electronic components in existing simulations and the use of tetrahedral meshes for analysis. This patent uses separate modeling for ICs and pins and draws meshes with hexahedrons and tetrahedrons. Moreover, aiming at the problem that the connection method of electronic components in existing simulation technologies ignores the soldering strength of pins, solder joints are used for connection, and the true strength at the connection is reflected and the mesh quality is good. In this way, it not only solves the problems of high cost and easy secondary damage caused by manual disassembly in the prior art, but also solves the problem of poor accuracy. Since there is no need to test with actual products, the capital cost is saved; the variables in computer-aided calculations are controllable and the simulation conditions can be kept consistent for multiple times, so the variables are controllable; the simulation speed is fast for multiple calculations, saving time costs; the problems ignored by existing simulation technologies are improved, and the accuracy and universality of this method are improved. At the same time, by adjusting the position angle of the ground coordinate system and setting different initial velocities, the purpose of simulating the instrument falling from different heights and angles is achieved, and the calculation time is greatly shortened to save costs.

[0028] Other beneficial effects of the present invention will be described in the specific implementation manner through the introduction of specific technical features and technical solutions. Those skilled in the art should be able to understand the beneficial technical effects brought by the technical features and technical solutions through these introductions. BRIEF DESCRIPTION OF THE DRAWINGS

[0029] The preferred embodiments of the method for simulating the drop of an automotive instrument based on ANSYS according to the present invention will be described below with reference to the drawings. In the figures:

[0030] Figure 1Flowchart of the ANSYS-based automotive instrument drop simulation analysis method according to a preferred embodiment of the present invention;

[0031] Figure 2 Schematic diagram of the chip modeling method in the prior art;

[0032] Figure 3 Schematic diagram of the chip modeling method according to a preferred embodiment of the present invention;

[0033] Figure 4 Schematic diagram of the co - node connection between the chip pins and the chip IC according to a preferred embodiment of the present invention;

[0034] Figure 5 Schematic diagram of the projection of the chip pins onto the PCB board according to a preferred embodiment of the present invention;

[0035] Figure 6 Isotropic hardening curve diagram of the plastic material according to a preferred embodiment of the present invention;

[0036] Figure 7 Elastic modulus, Poisson's ratio, shear modulus, and bulk modulus curve diagrams of the plastic material according to a preferred embodiment of the present invention;

[0037] Figure 8 Final effect diagram of the 3D model mesh of the automotive instrument assembly according to a preferred embodiment of the present invention;

[0038] Figure 9 Final effect diagram of the chip model mesh according to a preferred embodiment of the present invention;

[0039] Figure 10 Position relationship diagram of the side where the automotive instrument is located in the height direction and the local coordinate system XOY plane according to a preferred embodiment of the present invention;

[0040] Figure 11 Schematic diagram of establishing a rigid wall based on the local coordinate system XOY plane according to a preferred embodiment of the present invention;

[0041] Figure 12 Schematic diagram of adding a standard gravity field in the local coordinate system XOY according to a preferred embodiment of the present invention;

[0042] Figure 13 Schematic diagram of setting the initial velocity of the 3D model in the local coordinate system XOY according to a preferred embodiment of the present invention;

[0043] Figure 14 Overall energy curve diagram of the 3D model drop process of the automotive instrument assembly according to a preferred embodiment of the present invention. Detailed implementation manner

[0044] Figure 1 The following is a flowchart of a method for ANSYS-based drop simulation analysis of an automotive instrument according to a preferred implementation manner of the present invention, including the steps:

[0045] S100. Preprocess the 3D model of the automotive instrument assembly. Among them, separate each chip and its pins on the PCB board in the 3D model and perform co-node connection.

[0046] For components such as chips that are only soldered to the surface of the PCB, the conventional modeling method is as shown in Figure 2 below. Simplify the pins. This method ignores the pin strength and the risk of pin breakage. The present invention adopts the modeling method as shown in Figure 3 below (the figure includes the PCB board, chip IC, and pins). Model the IC and pins separately, considering the strength difference caused by different materials of the IC and pins, and the product failure caused by pin breakage can be analyzed. As shown in Figure 4 below, the pins and the IC are connected by co-nodes.

[0047] S200. Discretize the preprocessed 3D model to draw the initial mesh;

[0048] S300. Establish the connection relationship. Among them, the chip pins and the PCB board are connected by solder joints. When welding between the pins and the PCB board, the pins need to be projected onto the board as shown in Figure 5 below.

[0049] S400. Refine the mesh of the 3D model of the automotive instrument assembly and each chip therein. Among them, the overall mesh of the 3D model of the automotive instrument assembly adopts an explicit linear mesh, and the hexahedron mesh is adopted at the corresponding contact positions of each chip pin and the PCB.

[0050] S500. Establish a local coordinate system, and establish a rigid wall based on the local coordinate system plane. The rigid wall is used to simulate the ground;

[0051] S600. Apply the initial velocity and gravitational field when the preprocessed 3D model drops onto the rigid wall, and then simulate and calculate the stress result and deformation result of the 3D model after dropping onto the rigid wall. Among them, the initial velocity is related to the dropping height.

[0052] Generally, before performing the simulation, it is necessary to clarify at what initial velocity, from what height, and at what angle the instrument lands, which will provide sufficient support for the subsequent calculation. In the detailed implementation manner, the landing velocity of the instrument can be calculated according to the following formula: V t = V0 + gt, Or m is the mass, g is the acceleration due to gravity, and h is the drop height. Specifically, the instrument can be dropped from a height of 1 m, and the calculated landing speed is 4.427 m / s.

[0053] The technical solution of the present invention aims at the problem of poor accuracy caused by the simplification of electronic components in existing simulations and the use of tetrahedral meshes for analysis. This patent uses separate modeling for the chip IC and pins and draws the mesh with hexahedrons plus tetrahedrons. Moreover, for the problem that the connection method of electronic components in existing simulation technologies ignores the soldering strength of pins, solder joints are used for connection, and the true strength at the connection is reflected and the mesh quality is good. In this way, it not only solves the problems of high cost and easy secondary damage caused by manual disassembly in the prior art, but also solves the problem of poor accuracy. Since actual products are not required for testing, capital costs are saved; computer-aided calculation variables are controllable and multiple simulation conditions can be kept consistent, and variables are controllable; multiple calculation simulations are fast, saving time costs; the problems ignored by existing simulation technologies are improved, and the accuracy and universality of this method are improved. At the same time, by adjusting the position angle of the ground coordinate system and setting different initial velocities, the purpose of simulating the instrument falling from different heights and angles is achieved, and the calculation time is greatly shortened and costs are saved.

[0054] In a preferred embodiment, step S100 further includes: simplifying the chamfers and excessive fillets with a diameter less than 1 mm of the plastic parts in the 3D model, so that the 3D model has no interference and no errors. For example, errors that occur during modeling or file conversion, etc.

[0055] In a preferred embodiment, step S200 further includes: if the initial mesh drawing fails and is caused by the 3D model, return to step S100 to process the model to confirm that the 3D model data meets the finite element analysis standard.

[0056] In a specific embodiment, a material library can also be established. For example, for the plastic materials in the automotive instrument assembly, an elastoplastic model can be selected, and relevant parameters are input according to different materials. For example, in the technical solution of the present invention, the density of the PC+ABS material is 1.109e-06 kg / mm 3 , the tensile ultimate strength is 45.17 MPa, the tensile yield strength is 35.06 MPa. In addition, the isotropic hardening curve is as Figure 6 shown, and the elastic modulus, Poisson's ratio, shear modulus, and bulk modulus are as Figure 7 shown.

[0057] In a preferred embodiment, the normal stress limit for the solder joint connection between the chip pins and the PCB board in step S300 is 50 MPa, the shear stress limit is 30 MPa, the normal and tangential stress exponents are both 1, and the welding diameter is 0.8 mm. By adjusting the normal stress limit, shear stress limit of the solder joint and the effective diameter parameter of the solder joint, the true strength of the welded part can be simulated well to simulate the soldering situation of the electronic component pins.

[0058] In a preferred embodiment, step S300 further includes: using Bonding connection for the appearance parts connected by adhesive; using Bonding connection for the threaded parts of the components connected by bolts and inserting the bolt pre-tightening force. Specifically, the maximum offset of the Bonding connection for the appearance parts connected by adhesive is 0.1 mm, the inserted bolt pre-tightening force of the Bonding connection for the threaded parts of the components connected by bolts is 85 N, and the duration is 0.3 s.

[0059] In a specific embodiment, the overall mesh of the 3D model of the vehicle instrument assembly adopts an explicit linear mesh. Among them, the element size is 3 mm, the growth rate is 1.5, the maximum size is 5 mm, the feature cleaning is turned on and the size is set to 0.5 mm, the curvature capture is turned on and the minimum curvature is set to 3 mm, the normal angle is 72°, the capture proximity minimum size is 3 mm, and the proximity gap factor is 3.0. The chip size is set to 1 mm, the cleaning feature size is 0.5 mm, the minimum size of the captured curvature and the minimum proximity size are 1 mm, and other parameters are the same as the overall mesh size. The hexahedral mesh is used to set the element size of 0.1 mm at the corresponding contact positions of the chip pins and the PCB. The final effect of the mesh of the 3D model of the vehicle instrument assembly is as Figure 8 shown, and the final effect of the mesh of the chip model therein is as Figure 9 shown.

[0060] In a specific embodiment, in step S500, a local coordinate system is established, which can make the vehicle instrument close enough to the XOY plane of the local coordinate system to save time cost. The plane of the vehicle instrument glass cover is perpendicular to the XOY plane of the local coordinate system, and the side in the height direction of the vehicle instrument forms an angle of 35° with the XOY plane of the local coordinate system (as Figure 10 ); a rigid wall is established based on the XOY plane of the local coordinate system to simulate the ground (as Figure 11 ); a standard gravity field is added, and the direction is vertically downward perpendicular to the ground (as Figure 12 ), and the initial velocity is set (as Figure 13 ). Different falling situations at different heights and angles can be simulated by setting different coordinate system positions and different initial velocities.

[0061] In a preferred embodiment, in step S600, it is determined whether the parts of the 3D model are broken, whether the chip pins are broken, and / or whether the solder joint connection parts are desoldered based on the stress results and deformation results.

[0062] In a preferred embodiment, step S600 further includes: determining whether the 3D model of the vehicle instrument assembly is qualified based on the ratio of the hourglass energy of the 3D model.

[0063] In a specific embodiment, the analysis duration is set to 0.03 s, the time step safety factor is 0.9, automatic mass scaling is turned on and the time step is set to 1.112E-07 s to control the mass scaling factor at the E-02 magnitude. The solution accuracy is selected as double precision. The appropriate number of CPUs and memory are allocated according to the computer configuration. In this patent, 32 cores and 2000000 MB are used. Standard LS-DYNA is used to control the hourglass, with an ID of 1 and an hourglass coefficient of 0.1. Monitor the overall energy curve as Figure 14 shown. The ratio of the hourglass energy is less than 2%, which is within the acceptable range, the results are reliable, the overall energy change tends to be stable in the later stage, and the result credibility is high.

[0064] The present invention also discloses an electronic device, including a memory, a processor, and a computer program stored on the memory and executable on the processor. When the processor executes the computer program, the steps of any method of the present invention are implemented.

[0065] The present invention also discloses a computer-readable storage medium storing machine-executable instructions. When the machine-executable instructions are called and run by a processor, the machine-executable instructions cause the processor to run any method of the present invention.

[0066] It should be noted that in the present invention, step numbers (letter or number numbers) are used to refer to certain specific method steps only for the purpose of description convenience and simplicity, and by no means to limit the order of these method steps by letters or numbers. Those skilled in the art can understand that the order of the relevant method steps should be determined by the technology itself and should not be unduly limited by the existence of step numbers.

[0067] Those skilled in the art can understand that, on the premise of no conflict, the above preferred solutions can be freely combined and superimposed.

[0068] It should be understood that the above embodiments are exemplary rather than restrictive. Without departing from the basic principles of the present invention, various obvious or equivalent modifications or substitutions made by those skilled in the art to the above details will be included within the scope of the claims of the present invention.

Claims

1. An ANSYS-based method for drop simulation analysis of automotive instrument panels, characterized in that Including the steps: S100, preprocess the 3D model of the vehicle instrument assembly. Specifically, separate each chip and its pins on the PCB board in the 3D model and perform co - node connection; S200, discretize the preprocessed 3D model to draw the initial mesh; S300, establish connection relationships. Specifically, the chip pins and the PCB board are connected by solder joints; S400, refine the meshes of the 3D model of the vehicle instrument assembly and each chip in it. Specifically, the overall mesh of the 3D model of the vehicle instrument assembly uses explicit linear meshes, and the corresponding contact positions between each chip pin and the PCB use hexahedral meshes; S500, establish a local coordinate system, and establish a rigid wall based on the local coordinate system plane. The rigid wall is used to simulate the ground; S600, apply the initial velocity and gravitational field when the preprocessed 3D model falls onto the rigid wall, and then simulate and calculate the stress results and deformation results of the 3D model after falling onto the rigid wall. Specifically, the initial velocity is related to the height of the fall.

2. The method for simulating and analyzing the drop of an automotive instrument based on ANSYS according to claim 1, wherein The step S100 further includes: Simplify the chamfers and excessive fillets with a diameter of less than 1 mm in the plastic parts of the 3D model to ensure that the 3D model has no interference and no errors.

3. The method for simulating and analyzing the drop of an automotive instrument based on ANSYS according to claim 1, wherein The step S200 further includes: If the drawing of the initial mesh fails and it is caused by the 3D model, return to step S100 to process the model to confirm that the 3D model data meets the finite element analysis standard.

4. The ANSYS-based method for drop simulation analysis of automotive instrument according to claim 1, characterized in that In the step S300, the normal stress limit for the connection between the chip pins and the PCB board by solder joints is 50 MPa, the shear stress limit is 30 MPa, the normal and tangential stress exponents are both 1, and the welding diameter is 0.8 mm.

5. The method for simulating and analyzing the drop of an automotive instrument based on ANSYS according to claim 1, wherein, The step S300 further includes: Use Bonding connection for the appearance parts connected by adhesive; Use Bonding connection for the threaded parts of the components connected by bolts and insert the bolt pre - tightening force.

6. The method for simulating and analyzing the drop of an automotive instrument based on ANSYS according to claim 5, wherein The maximum offset of the Bonding connection for the appearance parts connected by adhesive is 0.1 mm, and the inserted bolt pre - tightening force for the Bonding connection of the threaded parts of the components connected by bolts is 85 N, with a duration of 0.3 s.

7. The method for drop simulation analysis of automotive instrument based on ANSYS according to claim 1, characterized in that, In the step S600, judge whether the parts of the 3D model are broken, whether the chip pins are fractured, and / or whether the solder joint connection parts are de - soldered through the stress results and deformation results.

8. The method for drop simulation analysis of automotive instrument based on ANSYS according to claim 7, characterized in that The step S600 further includes: Judge whether the 3D model of the vehicle instrument assembly is qualified by the proportion of hourglass energy in the 3D model.

9. An electronic device, comprising a memory, a processor, and a computer program stored on the memory and executable on the processor, wherein, When the processor executes the computer program, it implements the steps of the method described in any one of claims 1 to 8 above.

10. A computer-readable storage medium, characterized in that, The computer - readable storage medium stores machine - executable instructions. When the machine - executable instructions are called and run by the processor, the machine - executable instructions prompt the processor to run the method described in any one of claims 1 to 8 above.

Images