Finite element analysis method for horizontal five-axis machining center with tilting table

Abstract

The finite element analysis method of a flip plate horizontal five-axis machining center belongs to the technical field of machine tool structure analysis.The finite element analysis method of a flip plate horizontal five-axis machining center is provided, which is suitable for technical analysis of machine tool structure performance and analyzes the static structure rigidity of the whole machine through finite element software.The technical scheme adopted by the present application is as follows: a finite element analysis method of a flip plate horizontal five-axis machining center, characterized in that, comprising the following steps: step one: establishing three-dimensional models of main structural parts, linear guide rails and sliding blocks, and ball screws and nut, and performing simplification processing; step two: assembling the models according to the constraint conditions, importing them into Ansys Workbench software, and defining the material properties of each structural part.

Description

Technical Field

[0001] This invention proposes a finite element analysis method based on a flip-type horizontal five-axis machining center, belonging to the field of machine tool structure analysis technology. Background Technology

[0002] In recent years, large CNC machining centers have been increasingly widely used in the aerospace field. They are characterized by high speed, high acceleration, high precision, wide machining range, and large part size. Among them, the flip-plate horizontal five-axis machining center is a type of machine tool used to process large and complex surface structures. It has a large worktable, strong load-bearing capacity, and is an automatically interchangeable worktable with high machining efficiency. Therefore, it is receiving increasing attention in the aerospace field and has become an irreplaceable product.

[0003] With the continuous development and advancement of science and technology, computer simulation is increasingly being applied in the machine tool industry. Finite element analysis (FEM) is a crucial tool, theoretically analyzing the stiffness, stability, and stress of machine tool components under static, dynamic, and thermal conditions. Therefore, the theoretical results obtained from FEM can effectively guide structural design. Currently, for large-scale horizontal five-axis machining centers, there is no effective theoretical analysis method for product structure based on the actual conditions of the machine tool, nor is there an effective simulation of the force transmission relationships between structural components. Furthermore, there is no comprehensive method for describing the contact conditions of various mating surfaces. Therefore, it is necessary to establish a FEM method for horizontal five-axis machining centers to comprehensively evaluate the structural static stiffness of these products. Summary of the Invention

[0004] In view of the above-mentioned technical problems, the present invention proposes a finite element analysis method based on a flip-type horizontal five-axis machining center, which is suitable for the technical analysis of machine tool structural performance. The static structural rigidity of the whole machine is analyzed by using finite element software. The technical solution adopted by the present invention is as follows: A finite element analysis method for a flip-type horizontal five-axis machining center, characterized in that it includes the following steps: Step 1: Establish three-dimensional models of the main structural components, linear guide rails and sliders, ball screws and nuts and simplify them.

[0005] Step 2: Assemble the model according to the constraints, import it into Ansys Workbench software, and define the material properties of each structural component.

[0006] Step 3: Create a wire element model of the wire rope in Ansys Workbench software, and establish the connection and constraint relationships between the wire rope and the fixed pulley, carriage, and movable pulley on the pulley frame through constraint processing in the software.

[0007] Step 4: Establish contact constraints between various structural components, including contact constraints between kinematic pairs such as linear guides and sliders, and ball screws and nuts, and input contact stiffness values ​​and friction coefficients.

[0008] Step 5: Mesh the entire model, including mesh size and refinement of local meshes.

[0009] Step 6: Apply loads and boundary conditions, including gravitational acceleration, cutting forces in three directions applied to the spindle, and boundary conditions constraining the bed and the mating surfaces of the vertical bed and anchor bolts. Then, perform finite element static analysis on the main machine model.

[0010] Step 7: After solving, check the deformation and stress of each structural component, extract the location of the maximum deformation and stress, and comprehensively evaluate the static stiffness of the structural component.

[0011] Furthermore, the main structural components mentioned in step one include the main bed, main slide, column, carriage, ram, spindle, auxiliary slide, pulley frame, upright bed, and worktable.

[0012] Furthermore, the simplification process described in step one includes removing all threaded holes, small holes in non-stressed areas, fillets, and chamfers—features that have minimal impact on the overall finite element analysis results.

[0013] Furthermore, a model of the wire rope is established in the finite element software using the link10 element, and the connection and constraint relationships between the wire rope and the fixed pulley, slide plate and movable pulley on the pulley frame are established through contact features.

[0014] Furthermore, the mating surfaces between the main structural components are set to frictional contact, and the contact constraints between the mating surfaces are established by using bolt preload in finite element software; the contact stiffness between the linear guide and the slider, and between the ball screw and the nut, is obtained by finite element analysis to obtain the ball stiffness value, and the contact constraints of the kinematic pair are established by the spring unit system.

[0015] Furthermore, the main structural components, linear guide rails and sliders, ball screws and nuts are all simulated using solid element Solid187.

[0016] The beneficial effects of this invention are as follows: This invention provides reasonable constraints on the main machine model of the flip-type horizontal five-axis machining center, realizing the effective transfer of load. This not only improves the efficiency and accuracy of calculation, but also allows for a more precise analysis of the deformation and static stiffness of each structural component of the main machine, providing an effective method for the static stiffness analysis of the flip-type horizontal five-axis machining center.

[0017] This invention is not only applicable to flip-type horizontal five-axis machining products, but can also be adapted to other types of large machining center products after adjustments. Attached Figure Description

[0018] To more clearly illustrate the embodiments of the present invention, a detailed description will be provided below with reference to the accompanying drawings.

[0019] Figure 1 This is a schematic diagram of the main structure of the flip-plate horizontal five-axis machining center of the present invention.

[0020] Figure 2 This is a schematic diagram simulating the connection between a steel wire rope and its carriage, movable pulley, and fixed pulley.

[0021] Figure 3 This is a schematic diagram of the contact constraints between the various structural components.

[0022] Figure 4 This is a schematic diagram illustrating the stiffness analysis between the linear guide and the slider.

[0023] Figure 5 This is a schematic diagram of the contact constraint between the linear guide and the slider.

[0024] Figure 6 The front view shows the contact constraints between the ball screw and the nut.

[0025] Figure 7 Left view showing the contact constraint between the ball screw and the nut.

[0026] Figure 8 This is a flowchart of the finite element analysis method of the present invention. Detailed Implementation

[0027] The following example uses a large-scale horizontal five-axis machining center with a flip-type design, along with accompanying documentation. Figures 1-8 Detailed explanation of the specific implementation methods of this invention patent: Step 1: As follows Figure 1 As shown, first, a three-dimensional model of the main body of the flip-type horizontal five-axis machining center is established, including the main bed (1), main slide (2), column (3), slide (4), ram (5), spindle (6), auxiliary slide (7), pulley frame (8), vertical bed (9), worktable (10), etc. After the model of each structural component is established, it is assembled according to the actual constraint state. During the assembly process, the main slide, column, slide and ram should be located in the actual machining position to facilitate the accurate application of cutting force to simulate the actual machining process.

[0028] Step 2: Import the host model into Ansys Workbench, set the material parameters and element types. The models involved in this invention all use solid187 elements, and the main material parameter types are HT300, Q345B, GCr15, etc.

[0029] Step 3: As Figure 2As shown, the 3D model of the wire rope is simulated using Link10 elements in Ansys Workbench software. The cross-sectional parameters of the wire rope are set. At the same time, the wire rope is connected to the contact surfaces of the carriage and column by welding points in the software. The frictional contact constraint between the wire rope and the fixed pulley and the movable pulley on the pulley frame is set as line element and surface element. The above settings ensure that the wire rope has both natural and tensile states, which conforms to the actual situation of the wire rope.

[0030] Step Four: As Figure 3 As shown, the contact constraint relationship between each mating surface and kinematic pair is established, which mainly includes the following parts: (1) The mating surfaces between each structural component: First, calculate the magnitude of the bolt preload. According to the formula, we can obtain:

[0031]

[0032] In the formula, M is the bolt installation torque in N.mm, and d is the nominal diameter of the bolt in mm. The preload of each bolt can be calculated according to the formula. In Ansys Workbench software, the bolt preload magnitude and position are set by the Bolt Pretension command. At the same time, the mating surfaces between structural components are set to frictional form, that is, the mating surfaces between two structural components mainly transmit normal loads, and slight tangential loads may exist.

[0033] (2) Contact constraints between the linear guide and the slider kinematic pair: such as Figures 4-5 As shown, the main approach is to simplify the contact constraint of the linear guide and slider structure using spring elements through finite element software. Next, the normal and tangential stiffness of the springs are input. Specifically, the spring stiffness values ​​are obtained by first applying a force F1 in the normal direction of the slider using the finite element software, and then obtaining the deformation value X of each ball in the normal direction. 11 -X 41 According to formula K 刚度 The stiffness K of the ball bearing in the normal direction can be calculated by dividing F by X. 11 -K 41 This involves determining the normal stiffness of each ball bearing's equivalent spring. Then, by applying a force F2 in the tangential direction of the slider, the deformation of each ball bearing is obtained, allowing the calculation of the ball bearing's tangential stiffness K. 12 -K 42 That is, the tangential stiffness of the equivalent spring for each ball. Finally, the spring stiffness in the two directions is vectored to obtain the total equivalent spring stiffness K1-K4 for each ball. The contact constraint between the linear guide and the slider kinematic pair can then be completed by setting the finite element software.

[0034] (3) Contact constraints between the ball screw and the nut kinematic pair: such as Figures 6-7 As shown, similar to the contact constraint between the linear guide and the slider, the stiffness between the lead screw and the nut is first analyzed using finite element software. Specifically, the lead screw, nut, and ball are assembled, and then an axial force is applied to the nut to obtain the overall deformation of the nut, from which the stiffness value K5 can be calculated. Then, n springs are set between the lead screw and the nut, each with a stiffness of K5 / n, and arranged around the circumference of the lead screw and the nut. This simulates the contact constraint between the ball screw and the nut kinematic pair. In this example, four spring elements are used for simulation.

[0035] Step 5: Mesh the entire model, mainly including the size of the mesh for structural components and moving parts, and the refinement of local meshes, including the mesh between contact surfaces, the mesh at edge locations with stress concentration, etc.

[0036] Step 6: Apply loads and boundary conditions: including gravitational acceleration, applying cutting forces in three directions to the spindle, and boundary conditions constraining the mating surfaces of the main bed and vertical bed with the anchor bolts. Then, perform finite element static analysis on the main machine model to solve the problem.

[0037] Step 7: After solving, check the deformation and stress of each structural component, extract the location of the maximum deformation and stress, and comprehensively evaluate the static stiffness of the structural component.

[0038] In summary, this example demonstrates how flexible spring elements and linear elements are used to reasonably constrain the main body model of a flip-type horizontal five-axis machining center, achieving effective load transfer. This not only improves the efficiency and accuracy of calculations but also allows for a more precise analysis of the deformation and static stiffness of various structural components of the main body, providing an effective method for static stiffness analysis of flip-type horizontal five-axis machining centers.

[0039] It should be noted that this embodiment is only used to illustrate the technical solution of the present invention, and does not mean that this method is limited to flip-type horizontal five-axis machining center products. It is also applicable to other types of large machining center products. Any changes and modifications made based on the present invention patent should fall within the scope of this patent.

Claims

1. A finite element analysis method for a flip-type horizontal five-axis machining center, characterized in that, Includes the following steps: Step 1: Establish and simplify the three-dimensional models of the main structural components, linear guide rails and sliders, ball screws and nuts; the main structural components include: main bed (1), main slide (2), column (3), carriage (4), ram (5), spindle (6), auxiliary slide (7), pulley frame (8), vertical bed (9) and worktable (10); Step 2: Assemble the model according to the constraints and import it into Ansys Workbench software, defining the material properties of each structural component; Step 3: Create a wire element model of the wire rope in Ansys Workbench software, and establish the connection and constraint relationship between the wire rope and the fixed pulley, carriage, and movable pulley on the pulley frame through the constraint processing in the software; Step 4: Establish contact constraints between various structural components, establish contact constraints for kinematic pairs, including contact constraints between linear guides and sliders, and between ball screws and nutes, and input contact stiffness values ​​and friction coefficients; Step 5: Mesh the entire model, including mesh size and refinement of local meshes; Step 6: Apply loads and boundary conditions, including gravitational acceleration and cutting forces in three directions applied to the spindle. The boundary conditions are to constrain the bed and the mating surfaces of the vertical bed and the anchor bolts. Then, perform finite element static analysis on the main machine model to solve the problem. Step 7: After solving, check the deformation and stress of each structural component, extract the location of the maximum deformation and stress, and comprehensively evaluate the static stiffness of the structural component.

2. The finite element analysis method for a flip-type horizontal five-axis machining center according to claim 1, characterized in that: The simplification method described in step one includes removing all threaded holes, small holes in non-stressed areas, fillets, and chamfers, features that have little impact on the overall finite element analysis results.

3. The finite element analysis method for a flip-type horizontal five-axis machining center according to claim 1, characterized in that: In the finite element software, a model of the wire rope is created using the link10 element, and the connection and constraint relationships between the wire rope and the fixed pulley, slide plate and movable pulley on the pulley frame are established using contact features.

4. The finite element analysis method for a flip-type horizontal five-axis machining center according to claim 1, characterized in that: The mating surfaces between structural components are set to frictional contact, and the contact constraints between the mating surfaces are established by using the bolt preload in finite element software; the contact stiffness between the linear guide and the slider, and between the ball screw and the nut, is obtained by finite element analysis to obtain the ball stiffness value, and the contact constraints of the kinematic pairs are established by the spring unit system.

5. The finite element analysis method for a flip-type horizontal five-axis machining center according to claim 1, characterized in that: All structural components, linear guides and sliders, ball screws and nuts are simulated using Solid187 solid elements.

Images