Method for improving simulation convergence of engineering tire through double-rim constraint model

Abstract

The invention relates to the technical field of tire simulation, in particular to a method for improving engineering tire simulation convergence through a double-rim constraint model. The method comprises the following steps: establishing a double-rim constraint model jointly constrained by a rigid rim model, a local seam allowance contact surface model and a local rim contact surface model, and establishing a constraint relationship between a tire and a rim; assembling and inflating the double-rim constraint model, analyzing the uniformly distributed pressure load of the rims and the inner surface of the tire under the action that the pressure of the tire is equal to that of the tire, and completing a two-dimensional axisymmetric inflation analysis result; and rotating the double-rim constraint model by 360 degrees along a symmetric center line, converting the double-rim constraint model into a three-dimensional grid model, transmitting a two-dimensional axial symmetry inflation analysis result into the three-dimensional grid model generated by rotational symmetry, and respectively applying different load values to the three-dimensional tire model to obtain a simulation calculation result of the tire under corresponding working conditions. According to the method, the convergence of finite element simulation calculation of the tire is improved through the double-rim constraint model.

Description

TECHNICAL FIELD

[0001] The present application relates to the field of tire simulation technology, in particular to a method for improving the convergence of engineering tire simulation by using a double-rim constraint model. BACKGROUND

[0002] Using finite element simulation calculation method to analyze tire performance can accurately obtain the stress and deformation of the tire under different air pressure, load and steering conditions, and can effectively obtain the stress and strain distribution of the tire under different working conditions. Finite element simulation calculation is an important means of tire product development and performance research. In tire simulation analysis, the rigid material rim is constrained on the tire by the contact between the rim and the tire bead portion sub-interface position, such as the conventional model shown in Figure 1 As shown in Figure 1 The conventional sub-interface contact surface 1 and the conventional rim contact surface 2 are filled with high-pressure gas inside the tire, and the tire bears a very high contact pressure and sliding tendency under high load conditions, and the contact state changes dramatically with load changes. This extreme nonlinear contact behavior is one of the main reasons why tire simulation analysis cannot be completed.

[0003] For example, Chinese patent publication No. CN115081291A discloses a finite element tire simulation fast convergence method using virtual rims, application and program product. This method uses a rigid sub-interface model completely, which improves the simulation calculation convergence and calculation efficiency, but the virtual rim control surface cannot deform, which causes the virtual rim model to be unable to accurately reflect the stress and deformation of the gradually established contact part between the tire sub-interface and the rim after the air pressure and load change. For high load and extreme steering conditions, the virtual rim model cannot accurately reflect the support state of the rim contact surface to the tire bead portion, such as the virtual rim model shown in Figure 2 which includes Figure 2 a rigid surface 3 that cannot deform freely, Figure 3 a boundary position of the air state defect 4 that is not reasonably distorted, Figure 4 and a side slip working condition simulation of the steering state defect 5 that is not reasonably distorted. Various virtual rim model defects cause the tire bead portion position to be unable to accurately simulate the contact between the tire and the rim under high load conditions and extreme steering conditions, resulting in poor simulation result accuracy.

[0004] Therefore, in the above conventional technology, it is not possible to improve the convergence difficulty of tire simulation calculation caused by the complex contact state of the bead seat position, and to improve the calculation accuracy caused by the complete use of rigid sub-interface model to improve convergence. SUMMARY

[0005] The technical problem to be solved by the present application is to overcome the shortcomings of conventional technology and provide a method for improving the convergence of engineering tire simulation by using a double-rim constraint model.

[0006] The technical scheme adopted by the present application is as follows: A method for improving convergence of engineering tire simulation by a double-rim constraint model, comprising the following steps: S1, establishment of a double-rim constraint model: a double-rim constraint model is established by establishing a rigid rim model, a local bead contact surface model and a local rim contact surface model to jointly constrain the double-rim constraint model, and a constraint relationship between the tire and the rim is established, comprising the following steps: S11, establishment of a rigid rim model; S12, establishment of a local bead contact surface model; S13, establishment of a local rim contact surface model; S2, inflation calculation of the double-rim constraint model: the double-rim constraint model is assembled and inflated, and under the action of the tire exerting an equal pressure to the tire air pressure, the uniform pressure load of the rim and the inner surface of the tire is analyzed, and the standard solver of the finite element software abaqus is submitted to solve the two-dimensional axisymmetric inflation analysis result; S3, calculation of tire simulation convergence: the double-rim constraint model is rotated by 360° along the symmetry line to convert into a three-dimensional grid model, the two-dimensional axisymmetric inflation analysis result is transmitted to the three-dimensional grid model generated by rotation symmetry, and different load values are applied to the three-dimensional tire model respectively, and the standard solver of the finite element software abaqus is submitted to solve and calculate, to obtain the simulation calculation result of the tire under the corresponding working condition.

[0007] The technical scheme improves the convergence of tire finite element simulation calculation by using rigid displacement of the rigid rim model to replace the contact pair of the tire and the rim; and accurately simulates the gradual establishment of the contact and deformation relationship of the tire in the process of pressure and load change through the local bead contact surface and the local rim contact surface. The technical scheme can not only improve the calculation convergence of the tire under harsh working conditions and ensure the completion of the calculation of the finite element model, but also improve the simulation calculation precision through the contact relationship between the bead and the local rim.

[0008] In addition, the method for improving convergence of engineering tire simulation by the double-rim constraint model according to the present application has the following additional technical features: According to one embodiment of the present application, in the step S1, the establishment of the double-rim constraint model is derived from a two-dimensional material distribution map of the engineering tire, and a two-dimensional axisymmetric finite element grid is defined by using the finite element grid definition software hypermesh to define the two-dimensional material distribution map describing the tire structure, to obtain a tire finite element grid model.

[0009] In the technical solution, the two-dimensional material distribution map directly shows the types, positions and relative distribution of different materials in the tire. For example, different materials are used in different parts of the tire, such as the tread, sidewall and belt. Hypermesh automatically or semi-automatically generates a high-quality two-dimensional axisymmetric finite element grid according to the two-dimensional material distribution map. When dividing the grid, the software considers the geometric characteristics and material properties of different parts of the tire to reasonably determine the size, shape and density of the grid. For example, in the stress concentration areas of the tire, such as the tread and belt, the grid is divided more finely to improve the calculation accuracy; in some areas with relatively small stress, the grid is appropriately sparse to reduce the calculation amount.

[0010] According to one embodiment of the present application, in step S1, the engineering tire is selected as a 460 / 95R25 specification mine wide-body dump truck tire.

[0011] In the technical solution, the engineering tire is a radial tire with a cross-sectional width of 460 mm, a cross-sectional height of 95% of the cross-sectional width, and an inner diameter of 25 inches. This engineering tire is only one tire scheme that can represent the effect of the technical solution, and is not a limitation of the present application.

[0012] According to one embodiment of the present application, the establishment of the rigid rim model in step S11 includes the following steps: S111, the finite element grid extending the left tire sub-portion bead toe to the upper side of the tire heel flush with the upper surface of the tire bead wire is defined as a left rigid rim unit; and the nodes of all rigid units in the left rigid rim unit are defined as left rigid rim nodes; S112, the finite element grid extending the right tire sub-portion bead toe to the upper side of the tire heel flush with the upper surface of the tire bead wire is defined as a right rigid rim unit; and the nodes of all rigid units in the right rigid rim unit are defined as right rigid rim nodes; S113, in the tire finite element grid model, the left rigid rim unit and the right rigid rim unit form a rigid rim unit constraint of the rigid rim model with the unit type set as RAX2, which is used to simulate the rigid rim constraint behavior of the rim on the tire.

[0013] In the technical solution, the finite element grid extending the left and right tire sub-portion bead toe to the upper side of the tire heel flush with the upper surface of the tire bead wire is defined as a rigid rim unit, which is used to simulate the actual contact and constraint area of the rim and the tire sub-port. By extending the definition, the constraint effect of the rim on the tire sub-port portion can be more accurately simulated. The rigid rim node is the main position of the interaction between the rim and the tire. By defining the node, the boundary conditions, loads and other conditions are accurately applied to simulate the constraint force and acting force of the rim on the tire.

[0014] According to one embodiment of the present application, the step S12 of establishing the local bead contact surface model comprises the following steps: S121, the upper unit of the left rigid bead unit is extended to the tire side direction until the finite element grid that may contact the tire bead area and the rim surface, defined as the left local bead contact surface; the left local bead contact surface does not coincide with the left rigid bead unit; S122, the upper unit of the right rigid bead unit is extended to the tire side direction until the finite element grid that may contact the tire bead area and the rim surface, defined as the right local bead contact surface; the right local bead contact surface does not coincide with the right rigid bead unit; S123, in the tire finite element grid model, the left local bead contact surface and the right local bead contact surface form a local bead contact surface constraint, which is used to simulate the local bead contact surface constraint behavior of the rim on the tire.

[0015] In the present technical solution, the upper unit of the left and right rigid bead unit is extended to the tire side direction until the finite element grid that may contact the tire bead area and the rim surface, defined as the left and right local bead contact surface, which is to more comprehensively and accurately simulate the actual contact between the tire and the rim. For example, when the tire bears a large load, the tire bead part will deform, causing the originally non-contacting bead peripheral area to contact the rim surface. By extending the definition, the potential contact area can be captured. The rigid bead unit is used to simulate the rigid constraint of the rim, and the local bead contact surface is used to simulate the contact behavior between the tire and the rim. The two do not coincide to avoid confusion in the calculation process, making the calculation and transmission of contact force more accurate. For example, when calculating the contact stress, the non-coincidence setting clearly distinguishes the rigid constraint force and the contact force, so as to obtain more accurate stress distribution results.

[0016] According to one embodiment of the present application, the step S13 of establishing the local rim contact surface model, in the contact analysis of the tire and the rim, only considers the rim flange part that may contact the local bead contact surface of the tire, and ignores the area that may contact the rigid bead position, defined as the local rim contact surface model, which is used to simulate the local rim contact surface constraint behavior of the rim on the tire.

[0017] In the present technical solution, the local rim contact surface model is the flange part of the complete rim contact surface model in the conventional simulation scheme, and the conventional rim contact surface model is the contact surface model containing the complete rim surface; the local rim model is the conventional rim contact surface model removing the area that may contact the rigid bead position and retaining the flange area that may contact the local bead contact surface.

[0018] According to one embodiment of the present application, the step S2 of the inflation calculation of the double-rim constraint model comprises the following steps: S21, control the left rigid rim node to move to the rim width position through displacement boundary conditions, and control the right rigid rim node to move to the rim width position through displacement control; S22, establish a contact relationship between the local bead contact surface model and the local rim contact surface model; S23, apply an inflation load to the tire, and submit the set analysis step to the standard solver of the finite element software abaqus for calculation.

[0019] In the technical solution, the control of the left and right rigid rim nodes to move to the rim width position through displacement boundary conditions is to accurately simulate the actual installation state of the rim in the finite element model. For example, if the rim position is not symmetrical during inflation, it may cause excessive force on one side of the tire, resulting in unrealistic stress neutralization and deformation. The tire will expand and contact the rim, and the contact surface will generate contact pressure and friction; through the contact relationship, the finite element model simulates this mutual influence, so that the deformation of the tire and the rim on the contact surface is coordinated, thereby obtaining more accurate calculation results.

[0020] According to one embodiment of the present application, the step S3 of the tire simulation convergence calculation applies different load values to the three-dimensional tire model respectively, and compares the convergence time of the normal model, the virtual rim model and the double-rim constraint model respectively.

[0021] According to one embodiment of the present application, the step S3 of the tire simulation convergence calculation, from the simulation calculation results, the double-rim constraint model has better simulation calculation efficiency and accuracy on the basis of overcoming the inflation state defects and the handling state defects of the virtual rim model.

[0022] Compared with the conventional technology, the present application has the following beneficial effects: By using rigid displacement of the rigid rim model to replace the contact pair of the tire and the rim, the convergence of the tire finite element simulation calculation is improved; through the local bead contact surface and the local rim contact surface, the contact and deformation relationship of the tire during the pressure and load change process is accurately simulated. The technical solution can not only improve the calculation convergence of the tire under harsh working conditions and ensure the completion of the finite element model calculation, but also improve the simulation calculation accuracy through the contact relationship between the bead and the local rim. BRIEF DESCRIPTION OF DRAWINGS

[0023] Figure 1 is a schematic diagram of a normal model.

[0024] Figure 2 is a schematic diagram of a virtual rim model.

[0025] Figure 3 This is a diagram showing the inflation state defects of a virtual rim model.

[0026] Figure 4 This is a diagram showing the handling defects of a virtual rim model.

[0027] Figure 5 This is a two-dimensional finite element mesh diagram of the tire model of the present invention.

[0028] Figure 6 This is a schematic diagram of the rigid rim unit of the present invention.

[0029] Figure 7 This is a schematic diagram of the rigid rim node of the present invention.

[0030] Figure 8 This is one of the schematic diagrams of a partial sub-port contact surface of the present invention.

[0031] Figure 9 This is the second schematic diagram of a partial sub-port contact surface of the present invention.

[0032] Figure 10 This is a schematic diagram of the double rim constraint position of the present invention.

[0033] Figure 11 This is a schematic diagram of a portion of the rim contact surface of the present invention.

[0034] Figure 12 This is a comparison diagram of the same defect under the double rim constraint model and the virtual rim constraint model.

[0035] In the diagram: 1. Conventional sub-rim contact surface; 2. Conventional rim contact surface; 3. Rigid surface that cannot undergo free deformation; 4. Inflation state defect; 5. Control state defect; 6. Left rigid rim unit; 7. Right rigid rim unit; 8. Left rigid rim node; 9. Right rigid rim node; 10. Left partial sub-rim contact surface; 11. Right partial sub-rim contact surface; 12. Rigid rim unit constraint; 13. Partial sub-rim contact surface constraint. Detailed Implementation

[0036] The technical solutions of the embodiments of the present invention will be clearly and completely described below with reference to the accompanying drawings. Obviously, the described embodiments are only some, not all, of the embodiments of the present invention. Based on the embodiments of the present invention, all other embodiments obtained by those skilled in the art without creative effort are within the scope of protection of the present invention.

[0037] Example 1 like Figures 5 to 12 As shown in the figure, this embodiment provides a method for improving the convergence of engineering tire simulation using a dual-rim constraint model, including the following steps: S1, establishment of a double-rim constraint model: a double-rim constraint model is established by establishing a rigid rim model, a local bead contact surface model and a local rim contact surface model, and a constraint relationship between the tire and the rim is established, including the following steps: S11, establishment of a rigid rim model; S12, establishment of a local bead contact surface model; S13, establishment of a local rim contact surface model; S2, inflation calculation of the double-rim constraint model: the double-rim constraint model is assembled and inflated, and the uniform pressure load of the rim and the inner surface of the tire under the action of the tire exerted with the tire pressure is analyzed, and the standard solver of the finite element software abaqus is submitted to solve the two-dimensional axisymmetric inflation analysis results; S3, calculation of the convergence of the tire simulation: the double-rim constraint model is rotated by 360° along the symmetry line to convert into a three-dimensional grid model, the two-dimensional axisymmetric inflation analysis results are transferred to the three-dimensional grid model generated by rotation symmetry, and different load values are applied to the three-dimensional tire model, respectively, and the standard solver of the finite element software abaqus is submitted to solve the calculation, and the simulation calculation results of the tire under the corresponding working condition are obtained.

[0038] The technical solution replaces the contact pair of the tire and the rim with a rigid displacement by the rigid rim model, improves the convergence of the tire finite element simulation calculation, and accurately simulates the gradual establishment of the contact and deformation relationship of the tire in the process of pressure and load change through the local bead contact surface and the local rim contact surface. The technical solution can not only improve the calculation convergence of the tire under harsh working conditions and ensure the completion of the finite element model calculation, but also improve the simulation calculation precision through the contact relationship between the bead and the local rim.

[0039] Example 2 The specific case will be analyzed below.

[0040] The tire model adopted in the embodiment of the application is a 460 / 95R25 specification mine wide-body dump truck tire.

[0041] According to the two-dimensional CAD design material distribution diagram of the 460 / 95R25 specification engineering tire, the tire material distribution diagram describing the tire structure is divided into a two-dimensional axisymmetric finite element grid by using the finite element grid division software hypermesh, and the finite element grid is as shown in Figure 5 .

[0042] In the tire finite element mesh model, rigid axisymmetric elements of type RAX2 are created at the left and right bezel positions of the tire, respectively, and a left rigid rim element 6 named rigid-rim-l and a right rigid rim element 7 named rigid-rim-r are placed there. The left rigid rim element 6 is created starting from the left tire bezel toe position in the tire finite element model and extends to the upper side of the tire heel, flush with the upper surface of the tire bead. Figure 6 As shown; the right-side rigid rim unit 7 is constructed from the right tire bead position to the tire heel, extending to a position flush with the upper surface of the tire wire bead, as shown. Figure 6 As shown.

[0043] For the left rigid rim unit 6 and the right rigid rim unit 7, respectively, a left rigid rim node 8 named rim-l and a right rigid rim node 9 named rim-r are created. The left rigid rim node 8 includes all the nodes of the rigid units in the left rigid rim unit 6 in step S2, such as... Figure 7 As shown, the right rigid rim node 9 includes all nodes of the rigid unit in the right rigid rim unit 7 in step S2, such as... Figure 7 As shown.

[0044] A left-side partial bead contact surface 10, named surf-rim-l, is established on the left side of the tire model. This left-side partial bead contact surface 10 begins at the upper unit of the left-side rigid rim unit 6 and extends towards the tire sidewall until it exceeds the area where the tire bead region may contact the rim surface, ensuring no overlap with the left-side rigid rim unit 6. Figure 8 As shown.

[0045] A right-side partial bevel contact surface 11 named surf-rim-r is established on the right side of the tire model. This right-side partial bevel contact surface 11 begins at the upper unit of the right-side rigid rim unit 7 and extends towards the tire sidewall until it exceeds the area where the tire and rim may contact, ensuring no overlap with the right-side rigid rim unit 7. Figure 9 As shown.

[0046] The dual-rim constraint model includes displacement constraints on the tire imposed by rigid rim elements of the steps, and the constraint control region is as follows: Figure 10 As shown; the dual-rim constraint model includes contact pair constraints composed of a local rim contact surface model and a local sub-rim contact surface. The areas where contact constraints may occur during simulation analysis are as follows: Figure 10 As shown, this constraint is used to accurately simulate the rim-tire binding behavior as the contact state changes with the load, ensuring the accuracy of simulation calculations under different working conditions.

[0047] The local rim contact surface model in the establishing step S6 is a local rim portion of a complete rim contact surface model in a conventional simulation scheme, the conventional rim contact surface model is a contact surface model containing a complete rim surface, as shown in Figure 1 The local rim model is a conventional rim contact surface model removing the area that may contact the rigid bead position, and retaining the rim area that may contact the local bead contact surface, Figure 11 as shown in.

[0048] The two-dimensional axisymmetric tire model inflation calculation is performed on the set two-dimensional axisymmetric grid model, and an assembly and inflation analysis step is set, wherein analysis step step1 controls the left rigid rim node 8rim-l to move-2.5mm in the local 2 direction to fix the rigid rim unit to the rim width position; controls the right rigid rim node rim-r to move+2.5mm in the local 2 direction to fix the rigid rim unit to the rim width position; analysis step step2 establishes the contact relationship of the local rim contact surface model surf-rim and the local bead contact surface surf-rim-l and surf-rim; analysis step step3 applies a uniform pressure load to the inner surface of the tire equal to the tire air pressure, completes the two-dimensional axisymmetric tire inflation calculation setting, and generates a calculation file; the generated calculation file is submitted to the standard solver of the finite element software abaqus to solve the finite element simulation calculation of the two-dimensional inflation condition.

[0049] The three-dimensional tire model loading calculation is performed on the two-dimensional axisymmetric grid model, which is rotated by 360° along the symmetry center line to convert it into a three-dimensional grid model, the two-dimensional axisymmetric inflation analysis result is transmitted to the three-dimensional grid model generated by rotation symmetry, and the three-dimensional tire model is respectively subjected to 12 tons, 24 tons and 30 tons of load, and the standard solver of the finite element software abaqus is submitted to solve the calculation, and the finite element simulation calculation result of the tire under the corresponding working condition is obtained. The calculation result and the calculation efficiency are shown in Table 1.

[0050] Table 1

[0051] Compared with the contact pair model of the conventional rim contact surface and the tire bead contact surface, the double-rim constraint model proposed in the application can effectively ensure the smooth completion of the simulation calculation under the conditions of 24 tons and 30 tons, and effectively improve the convergence of the simulation calculation. Compared with the virtual rim model mentioned in the patent authorization number CN115081291B, the simulation calculation efficiency is basically the same, and the double-rim model proposed in the application overcomes the defects of the left side Figure 12 The constraint is not accurate, and accurately reflects the contact relationship between the rim edge and the tire as Figure 12 shown on the right side, and the simulation calculation accuracy is higher.

[0052] Although the present application has been described in detail with reference to the preferred embodiments, it should be understood that the application is not limited to those preferred embodiments. Without departing from the spirit and scope of the application, one of ordinary skill can make various modifications and / or substitutions to the application. Any and all modifications made within the scope of the application disclosed herein are to be considered as falling within the scope of the application. Therefore, the scope of the application should be determined by the appended claims.

Claims

1. A method for improving the convergence of engineering tire simulation using a dual-rim constraint model, characterized in that, Includes the following steps: S1. Establishment of the dual-rim constraint model: By establishing a dual-rim constraint model jointly constrained by a rigid rim model, a local sub-rim contact surface model, and a local rim contact surface model, the constraint relationship between the tire and the rim is established, including the following steps: S11. Establishment of the rigid rim model; S12. Establishment of the local sub-port contact surface model; S13. Establishment of a local rim contact surface model; S2. Inflation calculation of the double rim constraint model: The double rim constraint model is assembled and inflated. The uniform pressure load on the rim and inner surface of the tire is analyzed under the action of applying tire pressure equal to the tire pressure. The two-dimensional axisymmetric inflation analysis results are obtained by submitting the standard solver of the finite element software Abaqus. S3. Calculation of tire simulation convergence: The double rim constraint model is rotated 360° along the centerline of symmetry to convert it into a three-dimensional mesh model. The two-dimensional axisymmetric inflation analysis results are transferred to the three-dimensional mesh model generated by rotational symmetry. Different load values ​​are applied to the three-dimensional tire model respectively. The solution is submitted to the standard solver of the finite element software Abaqus to obtain the simulation calculation results of the tire under the corresponding working conditions.

2. The method for improving the convergence of engineering tire simulation using a dual-rim constraint model as described in claim 1, characterized in that, In step S1, the establishment of the dual-rim constraint model is derived from the two-dimensional material distribution map of the engineering tire. The two-dimensional material distribution map describing the tire structure is defined into a two-dimensional axisymmetric finite element mesh using the finite element mesh definition software Hypermesh, thus obtaining the tire finite element mesh model.

3. The method for improving the convergence of engineering tire simulation using a dual-rim constraint model as described in claim 2, characterized in that, In step S1, the engineering tires are selected as 460 / 95R25 wide-body mining dump truck tires.

4. The method for improving the convergence of engineering tire simulation using a dual-rim constraint model as described in claim 2, characterized in that, The establishment of the rigid rim model in step S11 includes the following steps: S111. Define the finite element mesh extending from the left tire bead to the upper side of the tire heel, flush with the upper surface of the tire wire ring, as the left rigid rim element (6); and define the nodes of all rigid elements in the left rigid rim element (6) as the left rigid rim node (8). S112. Define the finite element mesh extending from the right tire bead to the upper side of the tire heel, flush with the upper surface of the tire wire ring, as the right rigid rim element (7); and define the nodes of all rigid elements in the right rigid rim element (7) as the right rigid rim node (9). S113. In the tire finite element mesh model, the rigid rim element (6) on the left and the rigid rim element (7) on the right form the rigid rim element constraint (12) of the rigid rim model with the element type set to RAX2, which is used to simulate the rigid rim constraint behavior of the rim on the tire.

5. The method for improving the convergence of engineering tire simulation using a dual-rim constraint model as described in claim 3, characterized in that, The establishment of the local sub-port contact surface model in step S12 includes the following steps: S121. Extend the upper element of the left rigid rim element (6) towards the tire side until it exceeds the finite element mesh where the tire bead area may contact the rim surface. Define this as the left local bead contact surface (10). The left local bead contact surface (10) does not coincide with the left rigid rim element (6). S122. Extend the upper element of the right rigid rim element (7) towards the tire side until it exceeds the finite element mesh where the tire bead area may contact the rim surface. Define it as the right local bead contact surface (11). The right local bead contact surface (11) does not coincide with the right rigid rim element (7). S123. In the tire finite element mesh model, the left local sub-contact surface (10) and the right local sub-contact surface (11) form a local sub-contact surface constraint (13), which is used to simulate the behavior of the rim on the tire's local sub-contact surface constraint (13).

6. The method for improving the convergence of engineering tire simulation using a dual-rim constraint model as described in claim 5, characterized in that, The establishment of the local rim contact surface model in step S13 involves considering only the rim flange portion that may contact the local bead contact surface of the tire in the contact analysis between the tire and the rim, while ignoring the area that may contact the rigid bead position. This is defined as the local rim contact surface model, which is used to simulate the local rim contact surface constraint behavior of the rim on the tire.

7. The method for improving the convergence of engineering tire simulation using a dual-rim constraint model as described in claim 6, characterized in that, The inflation calculation of the double rim constraint model in step S2 includes the following steps: S21. Control the left rigid rim node (8) to move to the rim width position through displacement boundary conditions, and control the right rigid rim node (9) to move to the rim width position through displacement control. S22. Establish the contact relationship between the local sub-jaw contact surface model and the local rim contact surface model; S23. Apply an inflation load to the tire and submit the set analysis step to the standard solver of the finite element software Abaqus for calculation.

8. The method for improving the convergence of engineering tire simulation using a dual-rim constraint model as described in claim 1, characterized in that, The calculation of tire simulation convergence in step S3 involves applying different load values ​​to the three-dimensional tire model and comparing the convergence times of the conventional model, the virtual rim model, and the double rim constraint model.

9. The method for improving the convergence of engineering tire simulation using a dual-rim constraint model as described in claim 8, characterized in that, The calculation of tire simulation convergence in step S3 shows that, based on the simulation results, the dual-rim constraint model has better simulation efficiency and accuracy by overcoming the deficiencies in inflation and handling states of the virtual rim model.

Images