The aim of the paper is to obtain a unified finite element model of a complex process, which makes it possible to obtain visual information related to the influence of the welding process parameters on the results of the process of wave strain hardening of the weld material. Modeling of sequentially executed technological processes of different physical nature - welding and hardening, makes it possible to obtain more general and objective visual information about the process as a whole. Modeling in the Ansys software package is performed in stages, with the output of an earlier stage of modeling acting as the input data of the subsequent stage. At the first stage, the problem of visualizing the process of forming a weld is solved with the possibility of calculating temperature fields, stress and strain fields during heating and cooling of the welded workpiece. At the second stage, the calculated data is imported into the finite element model of processing welds with a deformation wave. A finite element model makes it possible to build microhardness maps for selected (dangerous) sections and visually monitor the change in stresses and strains in welded workpieces, depending on the technological modes of hardening by a deformation wave. The obtained visual information allows for a qualitative and quantitative assessment of the result of a complex process, which contributes to an increase in the bearing capacity and performance of the product as a whole.
1
In the modern world, digital technologies are considered as a means of describing the complete life cycle of a product - from design and manufacture to operation and disposal. Science-intensive industries have been given a daunting task even before the product and its constituent parts are put into production, to create, manufacture and test mathematical models under operating conditions. The least developed from the point of view of modeling are the technological processes of manufacturing parts. The problems of their modeling are largely associated not only with a large number of technological factors, but also with a change in the shape and size of a part during processing, a continuously and dynamically changing stress-strain state of a product, and the need to take into account thermal processes. The solution to the problem of transferring information about the product during the transition from one operation to another is also quite difficult. Since various software tools have been developed and proposed to simulate different operations, the loss of some information is inevitable at the stage of inter operational transition. The problem is especially acute for the transfer of information between technological processes that differ in the physical nature of the effects on the material of the original workpiece.
The aim of the paper is to obtain a unified finite element model of a complex
process, which makes it possible to obtain visual information related to the influence of
the welding process parameters on the results of the wave strain hardening (WSH)
process of the weld material. Modeling of interconnected sequentially executed
technological processes of different physical nature - welding and hardening, makes it
possible to obtain more general and objective visual information about the process as
a whole. The known finite element models of the welding process do not imply the
modeling of subsequent effects on the weld [
The essence of WSH [
Modeling in the Ansys software package is performed in stages, with the output of an earlier stage of modeling acting as the input data of the subsequent stage. The choice of Ansys is based on the high reliability of the data obtained and a wide range of multidisciplinary calculation modules, combined on one platform. The use of a single platform greatly facilitates data exchange when solving multidisciplinary problems without loss of accuracy in calculations. In a complex formulation in relation to the indicated processes, the problem is solved for the first time.
Visualization of the Process of Processing Welds by a Deformation Wave 3 2
The development of a finite element model of the process of processing welds by a deformation wave consisted of two stages.
At the first stage, using the previously obtained data, a finite element model of the
weld was created. For this, in the "Transient Thermal" module, in the "Geometry"
section, the geometry of the welded specimen was created, and the weld was divided
into face and root elements (Fig. 1). In the "Engineering Data" section, the properties
of the processed material such as: yield stress, strength, density, thermal expansion
coefficient, Young's modulus, Punson's coefficient, thermal conductivity, specific
heat, tangential modulus, etc., were set. Some physical and mechanical properties
were determined depending on the temperature. Further, a finite element mesh was
formed in the welded workpiece. To solve thermal problems, the mesh was assigned
the "Explicit" type. The elements of the weld were heated using the heat flow set by
the “Heat Flow” function. The procedure for determining the value of the required
heat flux during welding is presented in various sources, for example [
The geometry of the welded product and the material model were transferred to the “Static Structural” module from the “Transient Thermal” module (Fig. 1). The finite element mesh was re-formed. The “Fixed Support” boundary condition was assigned to the ends of the welded workpiece. It secures the edges of the workpiece in space. The boundary condition "Frictionless Support" was applied to the bottom of the welded workpiece to ensure its normal restraint, with freedom in the tangential direction. The “Imported Load” function was used to import temperature fields from the “Transient Thermal” module. The adjustment of the calculation parameters "Analysis Setting" was carried out in the same way as in the "Transient Thermal"module, which is necessary for adequate transmission and use in the calculation of temperature fields in time. After solving the problem in the "Static Structural" module, it became possible to assess the stresses and strains that occur in the workpiece after welding.
The second stage was the combination of the data obtained as a result of modeling a weld with a strain wave hardening model into a single finite element model of the process of processing welds with a strain wave. For this, the “Transient Structural” module was used. Import from the previous calculations of the values of stresses and strains, the geometry of the workpiece changed as a result of welding, was carried out using the "External Data" and "Mechanical Model" modules, respectively (Fig. 1).
In the "Transient Structural" module (Fig. 1), to the previously created geometry of the weld, one more body is added - a rod roller, through which the impact energy is communicated to the processed surface of the welded workpiece. Preparation for the calculation of the "Transient Structural" module began with setting the contact in the "Connectoins" section, in which the contact type was defined as "Frictional" and the friction coefficient value was set. To simplify the organization of contact settings between bodies, the “Contact Tool” function was created and enabled. The direct transfer of weld stresses to the “Transient Structural” module was performed using the “Imported Initial Stress” function. Restriction of the roller movement along one of the axes was set by the introduction of the Displacement boundary condition. Fastening of the edges of the welded workpiece in space was ensured by the "Frictionless Support" boundary condition, which was applied to the ends of the workpiece. The movement of the workpiece in the process of wave strain hardening was carried out using the "Velocity" function, which provided the setting of the kinematic speed of the workpiece movement in the selected direction.
The law of deformation of the welded workpiece by the roller was set using the
"Force" function, which reflected the change in the impact force over time. The type
of dependence was determined from previously solved contact problems based on the
finite element model of a shock system with an intermediate link [
Setting up the “Analysis Setting” calculation parameters was reduced to turning on the “Auto Time Stepping” function and choosing the principle of calculating steps after a specified time, indicating the minimum and maximum time for calculating one step. After solving the problem, in the "Transient Structural" module it becomes possible to assess stresses, deformations, displacements, temperatures, etc. If it is necessary to study any other parameters or their combinations, they are activated before starting the calculation in the "Analysis Setting" or written in the command line.
As an example of using the developed technique, a unified finite element model of processing welds with a deformation wave was created. So the welded product consisted of two steel plates of 40X grade with dimensions of 150 * 70 * 10 mm (Fig. 2). Welding was carried out in two passes, semi-automatic, with the current strength of the root and face seam, respectively, 185 and 130A. The deposited material is steel 40X grade. Cutting the edges of welded workpieces was done in accordance with GOST 5264-80. WSH modes are: impact energy 70 J; overlap coefficient K = 0.3; rod roller tool 40 mm long and 10 mm in diameter.
Visualization of the Process of Processing Welds by a Deformation Wave 5
As an example, seven impacts of the tool on the surface of the welded workpiece were modeled. The adequacy of the data obtained as a result of modeling was established on the basis of its comparison with experimental data obtained under similar conditions. In the model of the welded workpiece, the microhardness distribution map in the surface layer before and after the WSH was compared, the sizes of individual indentations and the distribution of the hardness map under them were estimated. The values obtained as a result of modeling correspond to the results of the experiment with a confidence level of 0.95. welded workpieces, depending on the technological modes of hardening by a deformation wave.
The obtained visual information allows for a qualitative and quantitative assessment of the result of a complex process, which contributes to an increase in the bearing capacity and performance of the product as a whole.
The reported study was funded by RFBR according to the research project No. 18-3820066.