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.
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.