CN107563072B - Finite element modeling method for weld nut based on automobile fatigue simulation - Google Patents
Finite element modeling method for weld nut based on automobile fatigue simulation Download PDFInfo
- Publication number
- CN107563072B CN107563072B CN201710799957.0A CN201710799957A CN107563072B CN 107563072 B CN107563072 B CN 107563072B CN 201710799957 A CN201710799957 A CN 201710799957A CN 107563072 B CN107563072 B CN 107563072B
- Authority
- CN
- China
- Prior art keywords
- nut
- modeling
- finite element
- welding
- bolt
- Prior art date
- Legal status (The legal status is an assumption and is not a legal conclusion. Google has not performed a legal analysis and makes no representation as to the accuracy of the status listed.)
- Active
Links
Images
Landscapes
- Investigating Strength Of Materials By Application Of Mechanical Stress (AREA)
Abstract
The invention discloses a welded nut finite element modeling method based on automobile fatigue simulation, which comprises the following steps: a welded nut modeling step, namely establishing a solid unit grid of the welded nut and a base metal through point arrangement and projection; modeling a welding nut and base metal connecting surface, namely modeling a welding line and contact between the welding nut and the base metal; a bolt modeling step, namely modeling a bolt matched with the welding nut; a modeling step of assembling the welded nut and the bolt, wherein the connection between the bolt and the welded nut is modeled and the pretightening force of the bolt is set; and (4) finite element calculation, namely moving the established model into a fatigue finite element calculation model, and obtaining a stress mode of the finite element welded nut through simulation of a finite element program. The invention not only considers the connection structure of the welding position, but also considers the contact effect of the nut to the plate. The deformation behavior of the welding nut in fatigue simulation can be accurately simulated, and accurate plate stress distribution can be obtained.
Description
Technical Field
The invention relates to the field of automobile manufacturing, in particular to a simulation test method in an automobile manufacturing process.
Background
A weld nut is a nut that is adapted to be welded at the outer edge of the nut, and is typically made of a weldable material and is relatively thick and adapted to be welded. During welding, two separated parts are integrated, the metal is melted at high temperature and then mixed together for cooling, and alloy is added in the middle. The interior of the weld nut is generally stronger than the nut under the influence of molecular forces. The welded nut has the advantages of high strength, wide application range and proper thickness, but the connected part is deformed due to high temperature and cannot be disassembled, and some active metals are not suitable for welding by the method, such as aluminum, magnesium and the like, need shielding gas argon arc welding, and require high processing technology and precision.
Finite elements are a numerical technique in mathematics to approximate a solution to the problem of solving partial differential equations. When solving, the whole problem area is decomposed, each subarea becomes a basic unit, and the basic unit is called a finite element. The finite element method is suitable for computer programming, along with the development of computer hardware, the finite element method can grade the structural performance of parts and the whole vehicle as early as possible, find weak links of design quickly, put forward optimization and improvement suggestions, reduce the number of experimental sample vehicles and the number of tests, shorten the development time, reduce the development cost and improve the maturity of products.
No engineering personnel have studied the method of simulating weld nuts in finite element simulation to date. Even the existing finite element models of the welding nuts are established according to the mechanical properties of the bolts and the nuts and neglect the contact effect of the nuts or the bolts on the plates, the modeling modes of the welding nuts are roughly divided into two types, one type is to neglect the welding relation of the bolts and the nuts and directly connect the plates by rigid units. The other type is that the bolt is modeled physically, but the welding form of the nut and the contact relation between the nut and the plate are ignored. For automobile fatigue simulation, a region with large local stress is often required to be analyzed, a traditional modeling mode usually only can accurately analyze the stress outside a bolt connection region due to neglecting an actual stress mechanism of the connection region, the stress analysis of the connection is very inaccurate, and a large number of experiments prove that the connection region of a welding nut happens to be a common place where cracking occurs, so that a finite element modeling mode for the welding nut in the prior art has a remarkable defect.
Disclosure of Invention
The invention aims to provide a welded nut finite element modeling method based on automobile fatigue simulation, which comprises the following steps:
a welded nut modeling step, namely establishing a solid unit grid of the welded nut and a base metal through point arrangement and projection;
modeling a welding nut and base metal connecting surface, namely modeling a welding line and contact between the welding nut and the base metal;
a bolt modeling step, namely modeling a bolt matched with the welding nut;
a modeling step of assembling the welded nut and the bolt, wherein the connection between the bolt and the welded nut is modeled and the pretightening force of the bolt is set;
and (4) finite element calculation, namely moving the established model into a fatigue finite element calculation model, and obtaining a stress mode of the finite element welded nut through simulation of a finite element program.
In one embodiment, the weld nut modeling step comprises:
a point distribution step, namely uniformly distributing points on the lap joint surface of the welding nut by using a geometric processing module, distributing a welding area by using hard points according to the actual length and position of a welding line, and then projecting the hard points onto the surface of the base metal to enable the welding nut and the nodes generated on the surface of the base metal to be in one-to-one correspondence;
a welded nut grid generating step, namely dividing the outer surface of the welded nut by utilizing a shell unit, defining the welded nut as a closed shell as a body, and then generating a hexahedral solid unit grid by using a projection method;
a parent material grid generating step, wherein a hexahedron solid unit grid is generated by extracting from the middle surface of a parent material and using an offset method;
and a material parameter setting step of giving material parameters to the weld nut and the base material.
In one embodiment, the weld nut in the weld nut generating step is a quadrangular unit within the range of the base. In the parent material mesh generation step, the parent material is a quadrangular unit in the range of the base.
In one embodiment, the parameters set in the material parameter setting step include: density, modulus of elasticity, poisson's ratio.
In one embodiment, the step of modeling the weld nut to parent material joint face comprises:
a welding wire modeling step, namely bonding nodes in the lapping surface of a welding nut and a base metal in a welding wire area in a one-to-one correspondence manner to generate a common node unit;
and a contact modeling step, namely modeling the contact by taking a region except a welding seam on the lap joint surface of the welding nut and the base material as a contact region based on finite element analysis.
In one embodiment, in the contact modeling step, the contact area on the base material is used as a slave surface, the contact area on the weld nut is used as a main surface, the contact mode is surface-surface contact, the preset friction coefficient is provided, and the contact type is sport contact.
In one embodiment, the bolt modeling step models the bolt with a one-dimensional beam element, and the parameters of the interface and the material are set according to the model of the bolt.
In one embodiment, the step of modeling the weld nut and bolt assembly comprises:
modeling connection of a bolt and a welding nut, grabbing all nodes in an area of an internal thread of the welding nut by using a rigid unit to generate a first rigid unit, connecting a mass center point of the first rigid unit with one end of a one-dimensional beam unit, grabbing nodes in a range compressed by a nut of the bolt on the surface of a base material by using the rigid unit to generate a second rigid unit, and connecting the mass center of the second rigid unit with the other end of the one-dimensional beam unit;
and setting bolt pretightening force, and setting the pretightening force on the one-dimensional beam unit according to the bolt grade by using finite element analysis.
In one embodiment, the rigid connection elements are compared as simulations in the finite element calculation step.
Aiming at the defects of the prior art, the finite element modeling method of the welding nut based on the automobile fatigue simulation not only considers the connection structure of the welding position, but also considers the contact effect of the nut on the plate. The method can accurately simulate the deformation behavior of the welding nut in fatigue simulation, so as to obtain accurate plate stress distribution, is quick and effective, and is convenient for engineering technicians to master.
Drawings
The above and other features, properties and advantages of the present invention will become more apparent from the following description of the embodiments with reference to the accompanying drawings in which like reference numerals denote like features throughout the several views, wherein:
FIG. 1 discloses a flow chart of a weld nut finite element modeling method based on automotive fatigue simulation according to an embodiment of the present invention.
Fig. 2 discloses a schematic view of the weld nut.
Fig. 3 discloses a schematic view of the connection structure of the weld nut, the bolt and the base material.
Fig. 4 discloses a schematic diagram of weld nut "common node + contact" modeling.
Fig. 5 discloses a schematic diagram of the connection modeling of the weld nut, bolt and parent material.
Detailed Description
Referring to FIG. 1, FIG. 1 discloses a flow chart of a weld nut finite element modeling method based on automobile fatigue simulation according to an embodiment of the present invention. The weld nut finite element modeling method of the present invention is described below in connection with a specific example.
The example simulates the cracking of a tail pipe bracket with a welded nut in a certain development vehicle type in a fatigue test. The weld nut has a diameter of 18mm, the bolt is M8, class 6.8, and has three equal weld lines at its edges, as shown in fig. 2, and fig. 2 shows a schematic view of the weld nut of this example. The weight of the exhaust pipe and the muffler is 13.5 kg, the thickness of the tail pipe support is 1.5mm, the material is H260, the yield limit is 272MPa, the connection structure of the welding nut, the bolt and the base material in the example is shown in FIG. 3, and FIG. 3 discloses a schematic connection structure of the welding nut, the bolt and the base material. The tail pipe bracket for lifting the muffler and the adjacent part of the body-in-white were used as calculation models, and the load was set to be 4 times 540N of the weight of the muffler. The boundary condition is that the interception position of the part is restricted with six degrees of freedom. The analysis software is Abaqus, the bolt pretightening force is loaded in the first step, and 4 times of the weight of the silencer is loaded in the second step to be used as the external load. The finite element modeling process of the weld nut, namely the finite element modeling method of the weld nut based on the automobile fatigue simulation, is described in detail as follows, and the method comprises the following steps:
101. and a welded nut modeling step, namely establishing a solid unit grid of the welded nut and the base metal through point distribution and projection. In one embodiment, the weld nut modeling step 101 includes several substeps:
and a point distribution step, namely uniformly distributing points on the lap joint surface of the welded nut by using a geometric processing module, referring to engineering technical drawings, distributing a welding area by using hard points according to the actual length and position of a welding line, and then projecting the hard points onto the surface of the base metal, so that the welded nut and the nodes generated on the surface of the base metal are in one-to-one correspondence.
And a welded nut grid generating step of dividing the outer surface of the welded nut by using shell units, wherein the welded nut is a quadrilateral unit in the range of a base, the welded nut is a closed shell, the closed shell is defined as a body, and then a hexahedral solid unit grid is generated by using a projection (map) method.
And a parent material mesh generation step of extracting the parent material mesh from the middle surface of the parent material, and generating a hexahedral solid cell mesh by using an offset (offset) method, wherein the parent material mesh is a quadrilateral cell within the range of the base.
And a material parameter setting step of giving material parameters to the weld nut and the base material. In one embodiment, the parameters set in the material parameter setting step include: density, modulus of elasticity, poisson's ratio, and the like.
102. And modeling the connection surface of the welding nut and the base metal, namely modeling the welding line and the contact between the welding nut and the base metal. In one embodiment, the step 102 of modeling the weld nut to parent material joint face comprises:
and a welding line modeling step, namely bonding the nodes in the lapping surface of the welding nut and the base metal in the area where the welding line is positioned in a one-to-one correspondence mode to generate a common node unit.
And a contact modeling step, based on finite element analysis, taking a region except a welding seam on the faying surface of the welding nut and the base material as a contact region, and modeling the contact, wherein the contact region on the base material is taken as a slave surface, the contact region on the welding nut is taken as a main surface, the contact mode is surface-surface contact, the preset friction coefficient is realized, and the contact type is kinematic contact. In this example, the friction coefficient was set to 0.2.
The modeling step 102 of welding the connection surface of the nut and the base material realizes a mode of 'common node + contact' modeling, and referring to fig. 4, fig. 4 discloses a schematic diagram of 'common node + contact' modeling of the welded nut.
103. And a bolt modeling step, namely modeling the bolt matched with the welding nut. In the bolt modeling step 103, the bolt is modeled by a one-dimensional beam unit, and parameters of an interface and a material are set according to the model of the bolt.
104. And a modeling step of assembling the welded nut and the bolt, wherein the connection between the bolt and the welded nut is modeled and the pretightening force of the bolt is set. In one embodiment, the modeling 104 of the weld nut and bolt assembly includes:
modeling of connection of the bolt and the welding nut, grabbing all nodes in an area of an internal thread of the welding nut by using a rigid unit to generate a first rigid unit, connecting a mass center point of the first rigid unit with one end of a one-dimensional beam unit, grabbing nodes in a range compressed by a nut of the bolt on the surface of a base material by using the rigid unit to generate a second rigid unit, and connecting the mass center of the second rigid unit with the other end of the one-dimensional beam unit, wherein a schematic diagram for modeling of rigid connection of the welding nut, the bolt and the base material is disclosed in fig. 5, which is shown in fig. 5. In fig. 5, the first rigid unit and the second rigid unit are each represented by a rigid unit icon, and the first rigid unit, the second rigid unit, and the one-dimensional beam unit all belong to the modeling unit.
And setting bolt pretightening force, and setting the pretightening force on the one-dimensional beam unit according to the bolt grade by using finite element analysis. The bolt class can be referred to the instructions of the machine manual, in this example, the M8, class 6.8 bolt pretension is 17000N, as specified in the machine manual, using finite element analysis software, and the pretension is applied to the one-dimensional beam element.
105. And (4) finite element calculation, namely moving the established model into a fatigue finite element calculation model, and obtaining a stress mode of the finite element welded nut through simulation of a finite element program. In one embodiment, the rigid connection elements are compared as simulations in the finite element calculation step. In the finite element calculation step 105, the established weld nut model is moved into the finite element calculation model, and meanwhile, for the purpose of comparing simulation results well, rigid connection units which are most commonly used in automobile simulation calculation at present are introduced as models for simulation comparison in the example. And finally, a stress distribution result on the tail pipe support can be obtained through simulation of a commercial finite element calculation program Abaqus, and the stress distribution result is compared with a test result. By comparison, the stress distribution condition obtained by applying the calculation model of the technology is good in test goodness of fit, the maximum stress is generated at the welding edge of the welding nut, a triangle formed by the stress distribution in the stress distribution diagram is consistent with the shape of cracking in the test, and the maximum stress is 275MPa and is slightly larger than the yield strength of the base metal, namely 272MPa, so that the support is at risk of fatigue cracking. The result is obtained by using a conventional rigid connection calculation model, the rigidity of the welding seam is greatly increased by rigid connection between the nut and the base material, so that the stress at the original weak welding line is obviously reduced, the maximum stress is only 0.9MPa and is far less than the yield strength of the base material, the fatigue cracking risk is avoided, and the stress distribution pattern is also inconsistent with the cracking form of the test.
Because the stress distribution condition is the most key and direct basis and standard in the automobile fatigue simulation calculation, the 'common node + contact' modeling method provides a quick and correct finite element model for welding the nut, so that an automobile structure designer can be assisted to quickly and accurately evaluate the fatigue performance of the base material, and reliable CAE analysis support is provided for further optimization and improvement of parts.
The invention has the following advantages:
1. the modeling process is simple: the welded nut model can be transplanted to any automobile fatigue simulation model only by simple common-node bonding, contact pair setting and pre-tightening force applying material attribute setting, and parameters can be adjusted.
2. The simulation precision is high: the built welding nut model comprehensively considers the welding seam and contact between the nut and the plate, and the bolt applies pretightening force, so that the stress condition of the plate on the welding nut side is completely consistent with the real condition, and the mechanical behavior and the deformation mode of the welding seam under the action of fatigue load can be correctly simulated.
3. The simulation efficiency is high: solid modeling is adopted for the weld nut of the primary analysis and the base material on the same side, and a beam unit is adopted for the bolt of the secondary analysis.
4. The simulation stability is good: the weld nuts are in one-to-one correspondence with grids on the surface of the base metal, so that nodes on the main surface and the secondary surface which are in contact are completely corresponding, the problem of non-convergence in implicit calculation is solved, and the phenomena of unstable resolving such as shooting points, negative volumes and the like which often occur in a shell unit and a solid unit cannot occur in the weld nut model.
Aiming at the defects of the prior art, the finite element modeling method of the welding nut based on the automobile fatigue simulation not only considers the connection structure of the welding position, but also considers the contact effect of the nut on the plate. The method can accurately simulate the deformation behavior of the welding nut in fatigue simulation, so as to obtain accurate plate stress distribution, is quick and effective, and is convenient for engineering technicians to master.
The embodiments described above are provided to enable persons skilled in the art to make or use the invention and that modifications or variations can be made to the embodiments described above by persons skilled in the art without departing from the inventive concept of the present invention, so that the scope of protection of the present invention is not limited by the embodiments described above but should be accorded the widest scope consistent with the innovative features set forth in the claims.
Claims (8)
1. A weld nut finite element modeling method based on automobile fatigue simulation is characterized by comprising the following steps:
a welded nut modeling step, namely establishing a solid unit grid of the welded nut and a base metal through point distribution and projection, wherein the welded nut modeling step comprises the following steps:
a point distribution step, namely uniformly distributing points on the lap joint surface of the welding nut by using a geometric processing module, distributing a welding area by using hard points according to the actual length and position of a welding line, and then projecting the hard points onto the surface of the base metal to enable the welding nut and the nodes generated on the surface of the base metal to be in one-to-one correspondence;
a welded nut grid generating step, namely dividing the outer surface of the welded nut by utilizing a shell unit, defining the welded nut as a closed shell as a body, and then generating a hexahedral solid unit grid by using a projection method;
a parent material grid generating step, wherein a hexahedron solid unit grid is generated by extracting from the middle surface of a parent material and using an offset method;
a material parameter setting step of giving material parameters to the weld nut and the base material;
modeling a welding nut and base metal connecting surface, namely modeling a welding line and contact between the welding nut and the base metal;
a bolt modeling step, namely modeling a bolt matched with the welding nut;
a modeling step of assembling the welded nut and the bolt, wherein the connection between the bolt and the welded nut is modeled and the pretightening force of the bolt is set;
and (4) finite element calculation, namely moving the established model into a fatigue finite element calculation model, and obtaining a stress mode of the finite element welded nut through simulation of a finite element program.
2. A weld nut finite element modeling method based on automotive fatigue simulation as claimed in claim 1,
the welding nut in the welding nut generating step is a quadrilateral unit in the range of the foundation;
in the parent material mesh generation step, the parent material is a quadrilateral unit in the range of the base.
3. A weld nut finite element modeling method based on automotive fatigue simulation as claimed in claim 1, wherein said parameters set in said material parameter setting step include: density, modulus of elasticity, poisson's ratio.
4. A finite element modeling method for a weld nut based on automobile fatigue simulation as claimed in claim 1, wherein the step of modeling the weld nut-base material joint surface comprises:
a welding wire modeling step, namely bonding nodes in the lapping surface of a welding nut and a base metal in a welding wire area in a one-to-one correspondence manner to generate a common node unit;
and a contact modeling step, namely modeling the contact by taking a region except a welding seam on the lap joint surface of the welding nut and the base material as a contact region based on finite element analysis.
5. A finite element modeling method of a weld nut based on automobile fatigue simulation as set forth in claim 4, wherein in the contact modeling step, the contact area on the base material is used as a slave surface, the contact area on the weld nut is used as a master surface, the contact mode is surface-surface contact, the preset friction coefficient is provided, and the contact type is sport type contact.
6. A weld nut finite element modeling method based on automobile fatigue simulation as claimed in claim 1, wherein in said bolt modeling step the bolt is modeled by a one-dimensional beam element, setting the parameters of interface and material according to the model of bolt.
7. The finite element modeling method of weld nut based on automobile fatigue simulation as claimed in claim 6, wherein said step of modeling the assembly of weld nut and bolt comprises:
modeling connection of a bolt and a welding nut, grabbing all nodes in an area of an internal thread of the welding nut by using a rigid unit to generate a first rigid unit, connecting a mass center point of the first rigid unit with one end of a one-dimensional beam unit, grabbing nodes in a range compressed by a nut of the bolt on the surface of a base material by using the rigid unit to generate a second rigid unit, and connecting the mass center of the second rigid unit with the other end of the one-dimensional beam unit;
and setting bolt pretightening force, and setting the pretightening force on the one-dimensional beam unit according to the bolt grade by using finite element analysis.
8. A weld nut finite element modeling method based on automotive fatigue simulation as claimed in claim 1, characterized in that said finite element calculation step uses rigid connection elements as simulation comparisons.
Priority Applications (1)
| Application Number | Priority Date | Filing Date | Title |
|---|---|---|---|
| CN201710799957.0A CN107563072B (en) | 2017-09-07 | 2017-09-07 | Finite element modeling method for weld nut based on automobile fatigue simulation |
Applications Claiming Priority (1)
| Application Number | Priority Date | Filing Date | Title |
|---|---|---|---|
| CN201710799957.0A CN107563072B (en) | 2017-09-07 | 2017-09-07 | Finite element modeling method for weld nut based on automobile fatigue simulation |
Publications (2)
| Publication Number | Publication Date |
|---|---|
| CN107563072A CN107563072A (en) | 2018-01-09 |
| CN107563072B true CN107563072B (en) | 2020-05-01 |
Family
ID=60979540
Family Applications (1)
| Application Number | Title | Priority Date | Filing Date |
|---|---|---|---|
| CN201710799957.0A Active CN107563072B (en) | 2017-09-07 | 2017-09-07 | Finite element modeling method for weld nut based on automobile fatigue simulation |
Country Status (1)
| Country | Link |
|---|---|
| CN (1) | CN107563072B (en) |
Families Citing this family (11)
| Publication number | Priority date | Publication date | Assignee | Title |
|---|---|---|---|---|
| CN109086498B (en) * | 2018-07-17 | 2020-05-08 | 东风商用车有限公司 | Analysis method for fender bracket with rubber pad |
| CN109508486B (en) * | 2018-10-31 | 2023-04-14 | 中国运载火箭技术研究院 | Bolt-connected finite element high-precision simplified modeling method and system |
| CN109409021B (en) * | 2018-12-18 | 2022-09-13 | 安徽江淮汽车集团股份有限公司 | Bolt connection method in engine simulation analysis |
| CN109766624A (en) * | 2019-01-04 | 2019-05-17 | 北京航空航天大学 | A kind of prediction technique of cementing structure adhesive layer fatigue life under the conditions of high/low temperature cold cycling |
| CN111209707B (en) * | 2020-02-21 | 2023-06-23 | 山东交通学院 | Friction type bolt connection node under combined action of compression shear, method and system |
| CN111400948B (en) * | 2020-03-16 | 2022-10-28 | 中国航天空气动力技术研究院 | Finite element calculation method for stress borne by stress release bolt |
| CN111444654B (en) * | 2020-04-07 | 2022-04-01 | 中国汽车工程研究院股份有限公司 | Virtual simulation method for judging bolt fracture under collision working condition |
| CN113742954A (en) * | 2020-05-29 | 2021-12-03 | 株洲中车时代电气股份有限公司 | Interference contact structure, and finite element modeling and calibrating method and system of motor stator |
| CN112307582B (en) * | 2020-10-30 | 2023-06-16 | 滨州渤海活塞有限公司 | Finite element modeling method for forged steel piston |
| CN112270055B (en) * | 2020-11-11 | 2024-07-09 | 珠海格力智能装备有限公司 | Stress analysis method, stress analysis device and processor of robot |
| CN114626273B (en) * | 2022-03-31 | 2023-06-09 | 广州思茂信息科技有限公司 | Hexahedral mesh partitioned bolt and nut finite element parametric modeling method |
Citations (2)
| Publication number | Priority date | Publication date | Assignee | Title |
|---|---|---|---|---|
| JP2007218288A (en) * | 2006-02-14 | 2007-08-30 | Honda Motor Co Ltd | Welded nut |
| CN106202639A (en) * | 2016-06-29 | 2016-12-07 | 北京强度环境研究所 | A kind of MJ bolt and nut finite element grid modeling method |
-
2017
- 2017-09-07 CN CN201710799957.0A patent/CN107563072B/en active Active
Patent Citations (2)
| Publication number | Priority date | Publication date | Assignee | Title |
|---|---|---|---|---|
| JP2007218288A (en) * | 2006-02-14 | 2007-08-30 | Honda Motor Co Ltd | Welded nut |
| CN106202639A (en) * | 2016-06-29 | 2016-12-07 | 北京强度环境研究所 | A kind of MJ bolt and nut finite element grid modeling method |
Non-Patent Citations (1)
| Title |
|---|
| 起重机轨道压板螺栓连接焊缝的动力学特征研究;葛文豪;《中国优秀硕士学位论文全文数据库》;20170615(第6期);正文第1-17,38-47页 * |
Also Published As
| Publication number | Publication date |
|---|---|
| CN107563072A (en) | 2018-01-09 |
Similar Documents
| Publication | Publication Date | Title |
|---|---|---|
| CN107563072B (en) | Finite element modeling method for weld nut based on automobile fatigue simulation | |
| Govik et al. | Finite element simulation of the manufacturing process chain of a sheet metal assembly | |
| CN100561490C (en) | Assembly soldering plate welded seam finite element modeling method based on vehicle collision simulation | |
| US20040195224A1 (en) | Automated weld location system for vehicles | |
| CN113408055B (en) | Automobile frame structure optimization method | |
| CN108646689B (en) | Virtual production manufacturing method and system based on welding | |
| CN110348088A (en) | Lightweight body structure Multipurpose Optimal Method based on agent model | |
| CN101916322A (en) | Optimization design method for sagging problem of car door based on CAE (Computer Aided Engineering) structural analysis | |
| JP5418374B2 (en) | Method and program for analyzing stiffness contribution of spot weld to spot welded structure | |
| CN105740504A (en) | Modeling method as well as calculation method and apparatus for gas cylinder mounting strength of passenger vehicle | |
| CN105740551B (en) | A kind of weld fatigue life-span prediction method | |
| Masters et al. | Modelling distortion induced in an assembly by the self piercing rivet process | |
| CN112241568A (en) | Engine cover opening and closing endurance fatigue analysis method based on finite elements | |
| Tagade et al. | Optimization and finite element analysis of steering knuckle | |
| CN111539135B (en) | Finite element modeling method for fatigue cracking prediction of sheet metal connection area | |
| CN111745276B (en) | Rapid simulation method for resistance spot welding residual stress and deformation of complex sheet metal component | |
| CN109255141B (en) | Optimization method for cross section shape of forward conceptual design of automobile body | |
| CN112464401B (en) | Accurate modeling method for metal material welding spot | |
| CN112033795B (en) | Biaxial stretching fatigue test piece optimization design method with oblique welding seam | |
| CN107169194B (en) | Finite element modeling method for automobile exhaust pipe silencer | |
| Govik et al. | The effects of forming history on sheet metal assembly | |
| CN109086498B (en) | Analysis method for fender bracket with rubber pad | |
| Osborne et al. | Finite element concept modelling methodologies for pickup truck boxes | |
| Huang et al. | Sensitivity Study of Self-Piercing Rivet Insertion Process Using Smoothed Particle Galerkin Method | |
| CN113901589B (en) | White car body baking deformation simulation analysis method |
Legal Events
| Date | Code | Title | Description |
|---|---|---|---|
| PB01 | Publication | ||
| PB01 | Publication | ||
| SE01 | Entry into force of request for substantive examination | ||
| SE01 | Entry into force of request for substantive examination | ||
| GR01 | Patent grant | ||
| GR01 | Patent grant |