Method for improving convergence of engineering tire simulation by dual rim constraint model

Abstract

The present application relates to the field of tire simulation technology, and particularly relates to a method for improving convergence of engineering tire simulation by a double-rim constraint model. The present application comprises the following steps: establishing a double-rim constraint model by establishing a rigid rim model, a local bead contact surface model and a local rim contact surface model, and establishing a constraint relationship between the tire and the rim; assembling and inflating the double-rim constraint model, analyzing the uniform pressure load of the rim and the inner surface of the tire under the action of the tire exerting an equal pressure to the tire air pressure, and completing the two-dimensional axisymmetric inflation analysis result; rotating the double-rim constraint model along the symmetry centerline by 360° to convert it into a three-dimensional grid model, transferring the two-dimensional axisymmetric inflation analysis result to the three-dimensional grid model generated by rotation symmetry, and applying different load values to the three-dimensional tire model respectively to obtain the simulation calculation result of the tire under the corresponding working condition. The present application improves the convergence of the finite element simulation calculation of the tire by 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 defect models 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:

[0007] A method for improving convergence of engineering tire simulation by a double-rim constraint model, comprising the following steps:

[0008] 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:

[0009] S11, establishment of a rigid rim model;

[0010] S12, establishment of a local bead contact surface model;

[0011] S13, establishment of a local rim contact surface model;

[0012] 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, 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;

[0013] S3, calculation of convergence of 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 result is transmitted to the three-dimensional grid model generated by rotation symmetry, and different load values are respectively applied to the three-dimensional tire model, 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.

[0014] 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.

[0015] 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:

[0016] According to an embodiment of the present application, in the step S1, the double-rim constraint model is established from a two-dimensional material distribution map of the engineering tire, a two-dimensional axisymmetric finite element grid is defined by using a finite element grid definition software hypermesh to define the two-dimensional material distribution map describing the tire structure, and a tire finite element grid model is obtained.

[0017] 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, the sidewall and the 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 the grid is divided, 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 the belt, the grid is divided more finely to improve the calculation accuracy; and in some areas with relatively small stress, the grid is appropriately sparse to reduce the calculation amount.

[0018] According to an embodiment of the present application, in step S1, the engineering tire is selected as a 460 / 95R25 size mine wide-body dump truck tire.

[0019] 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.

[0020] According to an embodiment of the present application, the establishment of the rigid rim model in step S11 includes the following steps:

[0021] 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;

[0022] 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;

[0023] 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.

[0024] The finite element grid defined by extending the upper side of the left and right tire bead toe to the upper surface of the tire bead is defined as a rigid rim unit, which is an area for simulating the actual contact and constraint of the rim and the tire bead.

[0025] According to one embodiment of the present application, the establishment of the local bead contact surface model in step S12 includes the following steps:

[0026] S121, the upper side of the left rigid rim 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 rim unit;

[0027] S122, the upper side of the right rigid rim 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 rim unit;

[0028] 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 to the tire.

[0029] The present technical solution extends the upper side of the left and right rigid rim units 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 area will deform, causing the originally non-contacting peripheral area to contact the rim surface. By extending the definition, the potential contact area can be captured. The rigid rim 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.

[0030] According to one embodiment of the present application, the step S13 of establishing the local rim contact surface model, in the analysis of the contact between the tire and the rim, only considers the rim flange part that can be in contact with the local bead contact surface of the tire, and ignores the area that can be in contact with the rigid bead position, defines the local rim contact surface model for simulating the constraint behavior of the local rim contact surface of the tire on the rim.

[0031] In the technical solution, the local rim contact surface model is the rim flange part of the complete rim contact surface model in the conventional simulation solution, and the conventional rim contact surface model is a contact surface model containing a complete rim surface; and the local rim model is obtained by removing the area that can be in contact with the rigid bead position from the conventional rim contact surface model, and retaining the rim flange area that can be in contact with the local bead contact surface.

[0032] According to one embodiment of the present application, the step S2 of calculating the inflation of the double-rim constraint model comprises the following steps:

[0033] S21, control the left rigid rim node to move to the rim width position through the displacement boundary condition, and control the right rigid rim node to move to the rim width position through the displacement control;

[0034] S22, establish the contact relationship between the local bead contact surface model and the local rim contact surface model;

[0035] S23, apply the inflation load to the tire, and submit the set analysis step to the standard solver of the finite element software abaqus for solving and calculation.

[0036] In the technical solution, the control of the left and right rigid rim nodes to move to the rim width position through the displacement boundary condition is to accurately simulate the actual installation state of the rim in the finite element model. For example, if the rim position is asymmetric during inflation, it can 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.

[0037] According to one embodiment of the present application, the step S3 of calculating the convergence of the tire simulation applies different load values to the three-dimensional tire model respectively, and compares the convergence time of the conventional model, the virtual rim model and the double-rim constraint model respectively.

[0038] According to one embodiment of the present application, the step S3 of calculating the convergence of the tire simulation, 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.

[0039] Compared with the conventional technology, the present application has the following beneficial effects:

[0040] The rigid rim model uses rigid displacement to replace the contact pair of the tire and the rim, 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 scheme can improve the calculation convergence of the tire under harsh conditions, ensure the completion of the calculation of the finite element model, and improve the simulation calculation precision through the contact relationship between the bead and the local rim. BRIEF DESCRIPTION OF DRAWINGS

[0041] Figure 1 is a schematic diagram of a conventional model.

[0042] Figure 2 is a schematic diagram of a virtual rim model.

[0043] Figure 3 is a defect diagram of the inflated state of the virtual rim model.

[0044] Figure 4 is a defect diagram of the operating state of the virtual rim model.

[0045] Figure 5 is a two-dimensional finite element grid diagram of the tire model of the present application.

[0046] Figure 6 is a schematic diagram of the rigid rim unit of the present application.

[0047] Figure 7 is a schematic diagram of the rigid rim node of the present application.

[0048] Figure 8 is one of the schematic diagrams of the local bead contact surface of the present application.

[0049] Figure 9 is the second schematic diagram of the local bead contact surface of the present application.

[0050] Figure 10 is a schematic diagram of the double-rim constraint position of the present application.

[0051] Figure 11 is a schematic diagram of the local rim contact surface of the present application.

[0052] Figure 12 is a comparison diagram of the same defect under the double-rim constraint model and the virtual rim model.

[0053] In the figure: 1, conventional bead contact surface; 2, conventional rim contact surface; 3, rigid surface that cannot be deformed freely; 4, inflation state defect; 5, handling 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 bead contact surface; 11, right partial bead contact surface; 12, rigid rim unit constraint; 13, partial bead contact surface constraint. DETAILED DESCRIPTION

[0054] The technical solutions in the embodiments of the present application will be clearly and completely described below with reference to the drawings in the embodiments of the present application. Obviously, the described embodiments are some of the embodiments of the present application, rather than all the embodiments of the present application. Based on the embodiments in the present application, all other embodiments obtained by a person of ordinary skill in the art without creative work fall within the protection scope of the present application.

[0055] Embodiment 1

[0056] As shown in the figure, the embodiment provides a method for improving convergence of tire simulation by a double-rim constraint model, comprising the following steps: Figures 5 to 12

[0057] S1, establishment of the double-rim constraint model: a double-rim constraint model jointly constrained by a rigid rim model, a partial bead contact surface model and a partial rim contact surface model is established to establish a constraint relationship between the tire and the rim, comprising the following steps:

[0058] S11, establishment of the rigid rim model;

[0059] S12, establishment of the partial bead contact surface model;

[0060] S13, establishment of the partial rim contact surface model;

[0061] 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 exerted and the tire 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;

[0062] S3, calculation of convergence of 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 result is transmitted to the three-dimensional grid model generated by rotation symmetry, and different load values are respectively applied to the three-dimensional tire model, the standard solver of the finite element software abaqus is submitted to solve and calculate, and the simulation calculation result of the tire under the corresponding working condition is obtained.

[0063] ​The technical scheme replaces the contact pair of the tire and the rim with rigid displacement through 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 scheme can improve the calculation convergence of the tire under harsh working conditions, ensure the completion of the calculation of the finite element model, and improve the simulation calculation precision through the contact relationship between the bead and the local rim.

[0064] Embodiment 2

[0065] The following will be analyzed in combination with specific cases.

[0066] The tire model adopted in the embodiment of the application is a 460 / 95R25 specification mine wide-body dump truck tire.

[0067] According to the two-dimensional CAD design material distribution map of the 460 / 95R25 specification engineering tire, the tire material distribution map describing the tire structure is divided into a two-dimensional axisymmetric finite element grid using the finite element grid division software hypermesh, and the finite element grid is as shown in Figure 5 .

[0068] In the tire finite element grid model, the left bead position and the right bead position of the tire are respectively established as rigid axisymmetric elements with the element type of RAX2, and are respectively put into the left rigid rim element 6 named rigid-rim-l and the right rigid rim element 7 named rigid-rim-r. The left rigid rim element 6 is established from the tire bead toe position of the left tire bead to the position where the upper side of the tire heel is flush with the upper surface of the tire bead wire, as shown in Figure 6 . The right rigid rim element 7 is established from the right tire bead toe position to the position where the upper side of the tire heel is flush with the upper surface of the tire bead wire, as shown in Figure 6 .

[0069] The left rigid rim element 6 and the right rigid rim element 7 are respectively established as the left rigid rim node 8 named rim-l and the right rigid rim node 9 named rim-r. The left rigid rim node 8 contains all the nodes of the rigid elements in the left rigid rim element 6 in step S2, as shown in Figure 7 . The right rigid rim node 9 contains all the nodes of the rigid elements in the right rigid rim element 7 in step S2, as shown in Figure 7 .

[0070] A left local bead contact surface 10 named surf-rim-l is created on the left side of the tire model bead, which is created from the top surface of the left rigid rim segment 6, extending to the sidewall direction until the area where the tire bead can contact the rim surface, and ensuring no overlapping area with the left rigid rim segment 6, as shown in Figure 8 .

[0071] A right local bead contact surface 11 named surf-rim-r is created on the right side of the tire model bead, which is created from the top surface of the right rigid rim segment 7, extending to the sidewall direction until the area where the tire bead can contact the rim surface, and ensuring no overlapping area with the right rigid rim segment 7, as shown in Figure 9 .

[0072] The dual rim constraint model contains displacement constraints of the tire by the rigid rim segments, and the constraint control area is shown in Figure 10 . The dual rim constraint model contains contact pair constraints of the local rim contact surface model and the local bead contact surface model, and the area where the contact constraint can occur in the simulation analysis is shown in Figure 10 . This part of the constraint is used to accurately simulate the rim behavior on the tire with the contact state changing with the load, ensuring the simulation calculation accuracy under different working conditions.

[0073] The local rim contact surface model in step S6 is created, which is a local rim portion of the complete rim contact surface model in the 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 the conventional rim contact surface model removing the area where the rigid bead position can contact, and retaining the rim area where the local bead contact surface can contact, Figure 11 .

[0074] The two-dimensional axisymmetric tire model inflation calculation is performed on the set two-dimensional axisymmetric grid model to set an assembly and inflation analysis step, wherein analysis step step1 controls left rigid rim node 8rim-l to move in local 2 direction by -2.5mm to fix the rigid rim unit to the rim width position; controls right rigid rim node rim-r to move in local 2 direction by +2.5mm 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-r; analysis step step3 applies an action equal to the tire air pressure to the tire inner surface uniform pressure load to complete the two-dimensional axisymmetric tire inflation calculation setting and generate a calculation file; and the generated calculation file is submitted to the standard solver of the finite element software ABAQUS for solving to complete the finite element simulation calculation of the two-dimensional inflation condition.

[0075] The three-dimensional tire model loading calculation is performed on the two-dimensional axisymmetric grid model rotated by 360° along the symmetry center line to convert the two-dimensional axisymmetric grid model 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 applied with a load of 12 tons, 24 tons and 30 tons, and the standard solver of the finite element software ABAQUS is submitted for solving calculation to obtain the finite element simulation calculation result of the tire under the corresponding working condition. The calculation result and the calculation efficiency are shown in Table 1.

[0076] Table 1

[0077]

[0078] 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 with the 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 constraint inaccuracy, accurately reflects the contact relationship between the rim edge and the tire as shown on the right, and has higher simulation calculation precision. Figure 12 Figure 12

[0079] ​​Although the present application is described in detail through the preferred embodiments with reference to the attached drawings, the present application is not limited thereto. Various equivalent modifications or replacements made by those skilled in the art to the embodiments of the present application without departing from the spirit and essence of the present application shall be included in the scope of the present application. Any person skilled in the art within the technical scope disclosed by the present application can easily think of changes or replacements, which shall be included in the protection scope of the present application. Therefore, the protection scope of the present application shall be subject to the protection scope of the 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 convergence of tire simulation: 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 standard solver of the finite element software Abaqus is submitted to solve the calculation and obtain the simulation calculation results of the tire under the corresponding working conditions. 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. 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). 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.

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 1, 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.

5. 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.

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 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