A tire forming tread rolling process simulation method, application and computer program product
By building a tire molding model using the ABAQUS simulation method, the problem of difficult to accurately predict material distribution during the tire molding process was solved, which reduced costs and shortened cycles, and improved tire quality.
Patent Information
- Application Number
- CN202310050159.3
- Authority / Receiving Office
- CN · China
- Patent Type
- Patents(China)
- Current Assignee / Owner
- Filing Date
- 2023-02-01
- Publication Date
- 2025-09-30
- Estimated Expiration
- 2043-02-01
AI Technical Summary
During the tire building process, it is difficult to accurately predict the material distribution of the finished tire, resulting in time-consuming and labor-intensive design adjustments with large errors.
A tire building tread rolling process simulation method based on ABAQUS is used to construct a tire building model and predict material distribution through finite element meshing, material property assignment, wire element embedding, component assembly, contact condition creation, and boundary condition definition.
Reduce the cost of new tire R&D, shorten the R&D cycle, improve the accuracy of material distribution prediction, and improve problems such as zero-degree streaking and shoulder bubbles.
Smart Images
Figure CN116127603B_ABST
Abstract
Description
Technical Field
[0001] The present invention relates to the technical field of tire production design, and in particular to a tire molding tread rolling process simulation method, application and computer program product. Background Art
[0002] Molding is one of the most critical steps in the tire design and manufacturing process. However, due to the high flow of rubber between components during the molding process, it is difficult to accurately predict the material distribution of the finished tire. For a long time, tire designers have relied on experience or references from similar tire structures to determine the dimensions of each component, repeatedly adjusting the design through trial and error to ensure tire quality. This method is not only time-consuming and labor-intensive, but the resulting material distribution often deviates significantly from the original design. Summary of the Invention
[0003] In order to solve the above technical problems, the purpose of the present invention is to provide a tire molding tread rolling process simulation method based on ABAQUS. This method can predict the material distribution of the tire tread according to the construction design drawings, build a bridge between the tread design and the tire manufacturing process, thereby reducing the R&D cost of new tires and shortening the new tire R&D cycle.
[0004] In order to achieve the above-mentioned purpose, the present invention adopts the following technical solutions:
[0005] A tire tread rolling process simulation method based on ABAQUS, the method includes the following steps:
[0006] 1) Finite element meshing and material property assignment
[0007] Draw the shape of the tire blank and the roller structure before tread rolling. Divide the tire blank shape into a grid, divide the rubber parts into quadrilateral units or triangular units, and divide the steel wires into line units.
[0008] Establish rubber material properties, define its density, elastic modulus, and Poisson's ratio, and assign these material properties to the rubber component unit; establish steel wire material properties, define the cross-sectional area, spacing, angle, and Poisson's ratio of the steel wire, and assign these material properties to the steel wire unit; export the file to inp format;
[0009] 2) Embedding of steel wire unit
[0010] Open the inp file generated in step 1) in Abaqus; select the Interaction module, create an embedding region in the constraint manager, and embed the steel wire element into the corresponding rubber element;
[0011] 3) Assembly of components
[0012] Assemble the tire blank model and the roller model into a calculation model;
[0013] 4) Create contact conditions
[0014] 4.1) Create contact surfaces and contact properties;
[0015] 4.2) Set the contact properties between the roller and the rubber and between the rubbers;
[0016] 5) Definition of boundary conditions
[0017] This includes the application of force and displacement and the setting of boundary conditions. Seven motion steps are created in the Step module. The first step is to inflate the tire blank; the second step is the pre-contact between roller one and the tread; the third step is the rolling process of roller one on the tread; the fourth step is the pre-contact between roller two and the tread; the fifth step is the rolling process of roller two on the tread; the sixth step is the pre-contact between roller three and the tread; and the seventh step is the rolling process of roller three on the tread. The loading conditions or motion conditions for steps one to seven are defined.
[0018] 6) Output calculation file
[0019] Output the set calculation model in the form of an inp file and calculate it; select the Job module, generate the calculation file in Create Job and output the calculation.
[0020] Preferably, in step 3), select the Assembly module, click Create instances, select the tire blank, roller 1, roller 2, and roller 3, assemble all components together, and create a calculation instance.
[0021] Preferably, the step 4.1) is as follows:
[0022] Select Surface in the tool options to create a contact surface;
[0023] Select the inner surface elements of the tire model and create an inflation contact surface named "inflation_surf"; select the outermost elements of the tread and create a contact surface named "TreadUp_surf"; select the elements below the tread and create a contact surface named "TreadLow_surf"; select the cells at the shoulder that will be in contact with the tread and create a contact surface named "Shoulder_surf"; select roller one and choose to create a contact surface on the geometry, select the outer surface of roller one as the contact surface between roller one and the tread, named "GL1_surf", select the outer surface of roller two as the contact surface between roller two and the tread, named "GL2_surf", select the outer surface of roller three as the contact surface between roller three and the tread, named "GL3_surf".
[0024] Preferably, the step 4.2) is as follows:
[0025] Select the Interaction module in Abaqus, create normal contact properties in the Interaction Property Manager and set the friction coefficient;
[0026] The contact properties between the roller and the rubber are named "IntProp-1", and the contact properties between the rubber and the rubber are named "IntProp-2".
[0027] In the Interaction Manager, select "Surface-to-surface contact", that is, surface-to-surface contact, set the contact between the lower surface of the tread and the surface at the shoulder, that is, "TreadLow_surf" and "Shoulder_surf" are in contact, and assign the contact property of "IntProp-2" to the contact pair; set "GL1_surf" and "TreadUp_surf" in contact, and assign the contact property of "IntProp-1" to the contact pair; set "GL2_surf" and "TreadUp_surf" in contact, and assign the contact property of "IntProp-1" to the contact pair; set "GL3_surf" and "TreadUp_surf" in contact, and assign the contact property of "IntProp-1" to the contact pair.
[0028] Preferably, the step 5) includes 7 movement steps, the first step is to inflate the tire blank, named "Inflation"; the second step is the pre-contact between roller one and the tread, named "GL1_contact"; the third step is the rolling process of roller one on the tread, named "GL1_dis1"; the fourth step is the pre-contact between roller two and the tread, named "GL2_contact"; the fifth step is the rolling process of roller two on the tread, named "GL2_dis2"; the sixth step is the pre-contact between roller three and the tread, named "GL3_contact"; and the seventh step is the rolling process of roller three on the tread, named "GL3_dis3".
[0029] The step 5) includes:
[0030] 5.1) Define the loading conditions for the first step, "Inflation." Inflate the inner contour of the tire blank to a shape close to that of the super-formed tire. Select "Pressure" for the loading type and "inflation_surf" for the loading surface. Set the pressure within a range of 0.1-0.3 MPa.
[0031] 5.2) Define the motion condition for the second step, "GL1_contact." This step requires Roller 1 to move a certain distance toward the tread, making contact with it. In Create Boundary Condition, select "GL1_contact" for the step and Displacement / Rotation for the type. Select Roller 1 as the geometry, check U2 and U1, and enter the displacement distance in the input box.
[0032] 5.3) Define the motion conditions for the third step, "GL1_dis1." This step applies a force perpendicular to the tread to Roller 1, and Roller 1 moves a specified distance from the center of the tread toward the edge. In Create Load, select Concentrated force for Type and Perpendicular to tread CF1 for Direction. Enter the force magnitude in the input box. In Create Boundary Condition, select "GL1_dis1" for Step, Displacement / Rotation for Type, Roller 1 for Geometry, and U2 for Displacement. Enter the displacement distance in the input box.
[0033] 5.4) Define the motion condition for step 4, "GL2_contact." This step requires roller 2 to move a certain distance toward the tread, making contact with it. In Create Boundary Condition, select "GL2_contact" for the step and Displacement / Rotation for the type. Select roller 2 as the geometry, check U2 and U1, and enter the displacement distance in the input box.
[0034] 5.5) Define the motion conditions for step 5, "GL2_dis2." This step applies a force to roller 2 at an angle of 20° to 30° to the tread. Starting from the position where roller 1 ends, roller 2 moves along the negative Y axis and stops at the edge of the running surface. In Create Load, select Concentrated force for Type. Decompose the force into two forces along the X and Y axes, respectively, based on their magnitude and direction. Select CF1 and CF2, and enter the corresponding force magnitudes in the following input boxes. In Create Boundary Condition, select "GL2_dis2" for Step, select Displacement / Rotation for Type, select roller 2 for Geometry, select U2, and enter the displacement distance in the following input box.
[0035] 5.6) Define the motion condition for step 6, "GL3_contact." This step requires Roller 3 to move a certain distance toward the tread, making contact with it. In Create Boundary Condition, select "GL3_contact" for the step and Displacement / Rotation for the type. Select Roller 3 as the geometry, check U2 and U1, and enter the displacement distance in the input box.
[0036] 5.7) Define the motion conditions for step 7, "GL3_dis3." This step applies a force to roller three at an angle of 65° to 75° to the tread. Roller three moves from the edge of the running surface in the negative X-axis direction to the bottom edge of the tread. In Create Load, select Concentrated force for the type. Decompose the force into two forces along the X and Y axes, respectively, based on their magnitude and direction. Select CF1 and CF2, and enter the corresponding force magnitudes in the following input boxes. In Create Boundary Condition, select GL3_dis3 for the step, select Displacement / Rotation for the type, select Roller three for the geometry, select U1, and enter the displacement distance in the following input box.
[0037] Furthermore, the present invention also discloses the application of the method in tire simulation.
[0038] Furthermore, the present invention also discloses a computer device, comprising a memory, a processor, and a computer program stored in the memory, wherein the processor executes the computer program to implement the method.
[0039] Furthermore, the present invention also discloses a computer-readable storage medium having a computer program or instruction stored thereon, which implements the method when the computer program or instruction is executed by a processor.
[0040] Furthermore, the present invention also discloses a computer program product, comprising a computer program or instructions, which implement the method when executed by a processor.
[0041] By employing the aforementioned technical solution, the present invention can predict the material distribution of a tire tread based on construction design drawings, building a bridge between tread design and tire manufacturing processes, thereby reducing the R&D cost and shortening the development cycle for new tires. The calculation results show that the tread in the calculated model has good fit and is similar to the actual tread profile after rolling, indicating that the model's calculation results are of reference value. Based on this calculation model, researchers can analyze the stress or strain of rubber or steel wire during rolling and improve issues resulting from tread rolling, such as zero-degree flare or shoulder bubbles. BRIEF DESCRIPTION OF THE DRAWINGS
[0042] Figure 1 This is the tread rolling calculation model.
[0043] Figure 2 The calculation completion status for the tread rolling model. DETAILED DESCRIPTION The following will be combined with the embodiments of the present invention to provide a complete and comprehensive description of the technical solutions in the embodiments of the present invention, and further explain the invention. Obviously, the embodiments described are only part of the embodiments of the present invention, not all of them. Given the embodiments of the present invention, all other embodiments obtained by ordinary technicians in this field without making creative efforts are within the scope of protection of the present invention.
[0044] 1. Finite element meshing and material property assignment
[0045] Use CAD to draw the tire shape and roller structure before rolling the tread, and save them in .dxf format. Import the tire shape into HyperMesh for meshing, dividing the rubber components into quadrilateral elements or triangle elements, and the steel wires into line elements.
[0046] Create rubber material properties, defining its density, elastic modulus, and Poisson's ratio, and assign these material properties to the rubber component elements. Create steel wire material properties, defining the cross-sectional area, spacing, angle, and Poisson's ratio of the steel wires, and assign these material properties to the steel wire elements. Export the file to inp format.
[0047] 2. Embedding of steel wire unit
[0048] Open the inp file generated in step 1 in Abaqus. Select the Interaction module and create an embedded region in the Constraint Manager. Embed the steel wire elements in the corresponding rubber elements.
[0049] 3. Assembly of components
[0050] Assemble the tire model and the roller model into a calculation model. Select the Assembly module, click Creatinstances, select the tire, roller 1, roller 2, and roller 3, assemble all the components together, and create a calculation instance, such as Figure 1 shown.
[0051] 4. Create contact conditions
[0052] Create contact surfaces and contact properties. Select Surface in the Tool option to create a contact surface. Select the inner surface elements of the tire blank model to create an inflation contact surface named "inflation_surf"; select the outermost elements of the tread to create a tread contact surface named "TreadUp_surf"; select the elements below the tread to create a contact surface named "TreadLow_surf"; select the cells of the shoulder that will be in contact with the tread to create a contact surface named "Shoulder_surf"; select roller one and choose to create a contact surface on the geometry. Select the outer surface of roller one to become the contact surface between roller one and the tread, named "GL1_surf", select the outer surface of roller two to become the contact surface between roller two and the tread, named "GL2_surf", and select the outer surface of roller three to become the contact surface between roller three and the tread, named "GL3_surf".
[0053] Set the contact properties between the roller and the rubber and between the rubber and the rubber. Select the Interaction module in Abaqus, create the normal contact properties in the Interaction Property Manager and set the friction coefficient. Name the contact properties between the roller and the rubber "IntProp-1" and the contact properties between the rubber and the rubber "IntProp-2". Select "Surface-to-surface contact" in the Interaction Manager, that is, surface-to-surface contact, set the contact between the lower surface of the tread and the surface at the shoulder, that is, "TreadLow_surf" and "Shoulder_surf", and assign the contact properties of "IntProp-2" to the contact pair. Set "GL1_surf" and "TreadUp_surf" in contact, and assign the contact property of "IntProp-1" to the contact pair; set "GL2_surf" and "TreadUp_surf" in contact, and assign the contact property of "IntProp-1" to the contact pair; set "GL3_surf" and "TreadUp_surf" in contact, and assign the contact property of "IntProp-1" to the contact pair.
[0054] 5. Definition of boundary conditions
[0055] It mainly includes the application of force and displacement and the setting of boundary conditions. First, create steps in the Step module, which mainly include 7 motion steps. The first step is to inflate the tire blank, named "Inflation"; the second step is the pre-contact between roller one and the tread, named "GL1_contact"; the third step is the rolling process of roller one on the tread, named "GL1_dis1"; the fourth step is the pre-contact between roller two and the tread, named "GL2_contact"; the fifth step is the rolling process of roller two on the tread, named "GL2_dis2"; the sixth step is the pre-contact between roller three and the tread, named "GL3_contact"; the seventh step is the rolling process of roller three on the tread, named "GL3_dis3".
[0056] Define the loading conditions for the first step, "Inflation." Inflate the inner contour of the tire to a shape close to the super-formed state. Select "Pressure" for the loading type, "inflation_surf" for the loading surface, and set the pressure (ranging from 0.1-0.3 MPa).
[0057] Define the motion condition for the second step, "GL1_contact." This step moves Roller 1 a certain distance toward the tread (negative X-axis direction) until it contacts the tread. In Create Boundary Condition, select "GL1_contact" for the step and Displacement / Rotation for the type. Select Roller 1 as the geometry, check U2 and U1, and enter the displacement distance in the input box.
[0058] Define the motion conditions for the third step, "GL1_dis1." This step applies a force perpendicular to the tread to Roller 1, moving it a certain distance from the center of the tread toward the edge. In Create Load, select Concentrated force for Type and Perpendicular to tread (CF1) for Direction. Enter the force magnitude in the input box. In Create Boundary Condition, select "GL1_dis1" for Step, Displacement / Rotation for Type, select Roller 1 for Geometry, select U2 for Displacement, and enter the displacement distance in the input box.
[0059] Define the motion condition for step 4, "GL2_contact." This step moves roller 2 a certain distance toward the tread, bringing it into contact. In Create Boundary Condition, select "GL2_contact" for the step and Displacement / Rotation for the type. Select roller 2 as the geometry, check U2 and U1, and enter the displacement distance in the input box.
[0060] Define the motion conditions for the fifth step, "GL2_dis2." This step applies a force to roller two at a certain angle (20°~30°) to the tread. Roller two starts at the end position of roller one and moves along the negative Y-axis to the edge of the running surface. In Create Load, select Concentrated force as the type, and decompose the force into two forces along the X-axis and Y-axis, respectively, based on their magnitude and direction. Check CF1 and CF2, and enter the corresponding force magnitudes in the input boxes at the rear. In Create Boundary Condition, select "GL2_dis2" as the step, select Displacement / Rotation as the type, select roller two as the geometry, check U2, and enter the displacement distance in the input box at the rear.
[0061] Define the motion condition for step 6, "GL3_contact." This step moves Roller 3 a certain distance toward the tread, making contact with it. In Create Boundary Condition, select "GL3_contact" for the step and Displacement / Rotation for the type. Select Roller 3 as the geometry, check U2 and U1, and enter the displacement distance in the input box.
[0062] Define the motion conditions for step seven, "GL3_dis3." This step applies a force to roller three at a certain angle (65°-75°) to the tread. Starting from the edge of the running surface, roller three moves along the negative X-axis and stops at the bottom edge of the tread. In Create Load, select Concentrated force as the type, and decompose the force into two forces along the X and Y axes, respectively, based on their magnitude and direction. Check CF1 and CF2, and enter the corresponding force magnitudes in the following input boxes. In Create Boundary Condition, select "GL3_dis3" as the step, select Displacement / Rotation as the type, select roller three as the geometry, check U1, and enter the displacement distance in the following input box.
[0063] 6. Output calculation file
[0064] Output the set calculation model in the form of inp file and calculate. Select Job module, generate calculation file in Create Job and output calculation. The calculation results are shown in Figure 2 .
[0065] 7. Results Analysis
[0066] The calculated results show that the tread conforms well to the model and is similar to the actual tread profile after rolling. This means the model's calculations are valuable for reference. Researchers can use this model to analyze the stress and strain of rubber or steel wire during rolling and improve tread rolling issues such as zero-degree flare and shoulder bubbles.
Claims
1. A tire tread rolling process simulation method based on ABAQUS, characterized in that: The method comprises the following steps: 1) Finite element meshing and material property assignment Draw the shape of the tire blank and the roller structure before tread rolling. Divide the tire blank shape into a grid, divide the rubber parts into quadrilateral units or triangular units, and divide the steel wires into line units. Establish rubber material properties, define its density, elastic modulus, and Poisson's ratio, and assign these material properties to the rubber component unit; establish steel wire material properties, define the cross-sectional area, spacing, angle, and Poisson's ratio of the steel wire, and assign these material properties to the steel wire unit; export the file to inp format; 2) Embedding of steel wire unit Open the inp file generated in step 1) in Abaqus; select the Interaction module, create an embedding region in the constraint manager, and embed the steel wire element into the corresponding rubber element; 3) Assembly of components Assemble the tire blank model and the roller model into a calculation model; 4) Create contact conditions 4.1) Create contact surfaces and contact properties Select Surface in the tool options to create a contact surface; Select the inner surface elements of the tire model and create an inflation contact surface named "inflation_surf"; select the outermost elements of the tread and create a tread contact surface named "TreadUp_surf"; select the elements below the tread and create a contact surface named "TreadLow_surf"; select the cells at the shoulder where the tread will contact the tread and create a contact surface named "Shoulder_surf"; select roller 1 and choose to create contact surface on the geometry. Select the outer surface of roller 1 as the contact surface between roller 1 and the tread and name it "GL1_surf", select the outer surface of roller 2 as the contact surface between roller 2 and the tread and name it "GL2_surf", and select the outer surface of roller 3 as the contact surface between roller 3 and the tread and name it "GL3_surf"; 4.2) Set the contact properties between the roller and the rubber and between the rubbers; 5) Definition of boundary conditions This includes applying force and displacement and setting boundary conditions. Seven motion steps are created in the Step module. The first step is inflating the tire blank; the second step is the pre-contact between roller one and the tread; the third step is the rolling process of roller one on the tread; the fourth step is the pre-contact between roller two and the tread; the fifth step is the rolling process of roller two on the tread; the sixth step is the pre-contact between roller three and the tread; and the seventh step is the rolling process of roller three on the tread. The loading conditions or motion conditions for steps one through seven are defined. 6) Output calculation file Output the set calculation model in the form of inp file and calculate; Select the Job module, generate the calculation file in Create Job and output the calculation.
2. The tire tread rolling process simulation method based on ABAQUS according to claim 1, characterized in that: Step 3) Select the Assembly module, click Create instances, select the tire blank, roller 1, roller 2, and roller 3, assemble all components together, and create a calculation instance.
3. The tire tread rolling process simulation method based on ABAQUS according to claim 1, characterized in that: Step 4.2) is as follows: Select the Interaction module in Abaqus, create normal contact properties in the Interaction Property Manager and set the friction coefficient; The contact properties between roller and rubber are named "IntProp-1", and the contact properties between rubber and rubber are named "IntProp-2". In the Interaction Manager, select "Surface-to-surface contact", that is, surface-to-surface contact, set the contact between the lower surface of the tread and the surface at the shoulder, that is, "TreadLow_surf" and "Shoulder_surf", and assign the contact property of "IntProp-2" to the contact pair; set "GL1_surf" and "TreadUp_surf" to contact, and assign the contact property of "IntProp-1" to the contact pair; set "GL2_surf" and "TreadUp_surf" to contact, and assign the contact property of "IntProp-1" to the contact pair; set "GL3_surf" and "TreadUp_surf" to contact, and assign the contact property of "IntProp-1" to the contact pair.
4. The tire tread rolling process simulation method based on ABAQUS according to claim 1, characterized in that: Step 5) includes 7 motion steps. The first step is to inflate the tire blank, named "Inflation"; the second step is the pre-contact between roller 1 and the tread, named "GL1_contact"; the third step is the rolling process of roller 1 on the tread, named "GL1_dis1"; the fourth step is the pre-contact between roller 2 and the tread, named "GL2_contact"; the fifth step is the rolling process of roller 2 on the tread, named "GL2_dis2"; the sixth step is the pre-contact between roller 3 and the tread, named "GL3_contact"; and the seventh step is the rolling process of roller 3 on the tread, named "GL3_dis3".
5. The tire tread rolling process simulation method based on ABAQUS according to claim 3, characterized in that: Step 5) includes: 5.1) Define the loading conditions for the first step, "Inflation." Inflate the inner contour of the tire blank to a shape close to that of the super-formed tire. Select "Pressure" for the loading type and "inflation_surf" for the loading surface. Set the pressure within a range of 0.1-0.3 MPa. 5.2) Define the motion condition for the second step, "GL1_contact." This step requires Roller 1 to move a certain distance toward the tread, making contact with it. In Create Boundary Condition, select "GL1_contact" for the step and Displacement / Rotation for the type. Select Roller 1 as the geometry, check U2 and U1, and enter the displacement distance in the input box. 5.3) Define the motion conditions for the third step, "GL1_dis1." This step applies a force perpendicular to the tread to Roller 1, and Roller 1 moves a certain distance from the center of the tread to the edge. In Create Load, select Concentrated force for the type and Perpendicular to tread CF1 for the direction. Enter the force magnitude in the input box. In Create Boundary Condition, select "GL1_dis1" for the step and Displacement / Rotation for the type. Select Roller 1 for the geometry, select U2 for the displacement, and enter the displacement distance in the input box. 5.4) Define the motion condition for step 4, "GL2_contact." This step moves roller 2 a certain distance toward the tread, making contact with it. In Create Boundary Condition, select "GL2_contact" for the step and Displacement / Rotation for the type. Select roller 2 as the geometry, check U2 and U1, and enter the displacement distance in the input box. 5.5) Define the motion conditions for step 5, "GL2_dis2." This step applies a force to roller 2 at an angle of 20° to 30° to the tread. Starting from the position where roller 1 ends, roller 2 moves along the negative Y axis and stops at the edge of the running surface. In Create Load, select Concentrated force for Type. Decompose the force into two forces along the X and Y axes, respectively, based on their magnitude and direction. Check CF1 and CF2, and enter the corresponding force magnitudes in the following input boxes. In Create Boundary Condition, select "GL2_dis2" for Step, select Displacement / Rotation for Type, select roller 2 for Geometry, check U2, and enter the displacement distance in the following input box. 5.6) Define the motion conditions for step 6, "GL3_contact." This step requires the roller to move a certain distance in three directions toward the tread and make contact with it. In Create Boundary Condition, select "GL3_contact" as the step, select Displacement / Rotation as the type, select Roller 3 as the geometry, check U2 and U1, and enter the displacement distance in the input box at the back; 5.7) Define the motion conditions for step 7, "GL3_dis3." This step applies a force to roller three at an angle of 65° to 75° to the tread. Roller three moves from the edge of the running surface in the negative X-axis direction to the bottom edge of the tread. In CreateLoad, select "Concentrated force" for the type and decompose the force into two forces along the X and Y axes, respectively. Select CF1 and CF2, and enter the corresponding force magnitudes in the following input boxes. In Create BoundaryCondition, select "GL3_dis3" for the step, select "Displacement / Rotation" for the type, select roller three for the geometry, select U1, and enter the displacement distance in the following input box.
6. Application of the method according to any one of claims 1 to 5 in tire simulation.
7. A computer device comprising a memory, a processor, and a computer program stored in the memory, characterized in that: The processor executes the computer program to implement the method according to any one of claims 1 to 5.
8. A computer-readable storage medium having a computer program or instruction stored thereon, characterized in that: When the computer program or instruction is executed by a processor, the method according to any one of claims 1 to 5 is implemented.
9. A computer program product comprising a computer program or instructions, characterized in that When the computer program or instruction is executed by a processor, the method according to any one of claims 1 to 5 is implemented.