A vehicle lateral stiffness analysis and optimization method for improving vehicle handling and a readable storage medium
By employing Admas handling performance analysis and vehicle lateral stiffness optimization methods, the problem of insufficient body stiffness in improving vehicle handling is solved, achieving accurate evaluation and optimization of vehicle handling, and applicable to various vehicle models.
Patent Information
- Authority / Receiving Office
- CN · China
- Patent Type
- Patents(China)
- Current Assignee / Owner
- CHONGQING CHANGAN AUTOMOBILE CO LTD
- Filing Date
- 2022-09-28
- Publication Date
- 2026-06-12
AI Technical Summary
Existing technologies, when improving vehicle handling, lack systematic analysis and optimization methods for vehicle stiffness, especially neglecting the impact of body stiffness on handling.
Admas's handling performance fundamental analysis was adopted, and the target lateral stiffness of the whole vehicle was set. A finite element analysis model of the lateral stiffness of the whole vehicle was established through the vehicle lateral stiffness optimization method. Lateral forces were applied and the center of mass was constrained. The lateral stiffness of the front and rear suspensions was calculated. The vehicle structure was strengthened according to the strain energy distribution. Finally, real vehicle verification was carried out.
It improves the evaluation and simulation accuracy of vehicle handling, breaks the traditional method of evaluating body-in-white stiffness, and is applicable to both traditional fuel vehicles and new energy vehicles, thus enhancing handling and simulation efficiency.
Smart Images
Figure CN115563731B_ABST
Abstract
Description
Technical Field
[0001] This invention relates to vehicle stiffness technology for improving vehicle handling, specifically to vehicle lateral stiffness analysis and design technology for improving overall vehicle handling. Background Technology
[0002] With the rapid development of the economy and the automotive industry, people's living standards have improved rapidly, and cars have gradually become a common means of transportation for ordinary families. As customers gain a deeper understanding of cars, their performance requirements are also increasing. Beyond meeting daily commuting needs, people are also placing new demands on the overall handling of the vehicle. Faced with increasingly fierce market competition, major automakers, in addition to meeting handling stability regulations, are paying more and more attention to the personalized driving experience for users, adding tests and evaluations beyond regulatory requirements, such as the moose test. Typically, major automakers mainly adjust chassis stiffness and structural design through KC analysis, roll analysis, pitch analysis, and yaw analysis to meet basic handling requirements, but they often overlook the impact of body rigidity.
[0003] Currently, vehicle body stiffness has detailed and clear evaluation indicators in the disciplines of durability, abnormal noise, and NVH (Noise, Vibration, and Harshness), but a complete evaluation system for overall vehicle handling is still lacking. For example, patent document CN201810368362.4 discloses a method and system for optimizing vehicle body stiffness, detailing the process from obtaining a CAD model of the vehicle body to converting it into a finite element model, then solving the body modal analysis, and optimizing areas with displacements greater than the error value through displacement cloud map comparison analysis until design requirements are met. It mainly describes the conversion of engineering data to finite element data and the optimization of the vehicle body structure using modal displacement cloud maps. Another example is patent document CN201210228196.0, which discloses a vehicle body stiffness estimation algorithm and device. By obtaining the relationship between vehicle body stiffness and the sensitivity of n sheet metal parts, it quickly estimates the contribution of each scheme to vehicle body stiffness, saving simulation calculation time. Both of these technologies directly or indirectly optimize vehicle body stiffness. Currently, regarding the improvement of overall vehicle handling performance, from the perspective of body stiffness analysis, most automakers have successful experience in controlling the bending and torsional stiffness of the body-in-white, but lack research on the overall vehicle stiffness. Summary of the Invention
[0004] This invention proposes a method for analyzing and optimizing the lateral stiffness of a vehicle to improve its handling performance. The aim is to break away from the traditional design of vehicle handling stability and the traditional handling analysis model that usually treats the vehicle body as a rigid body for analysis and optimization, and to establish a new alternative model and optimization approach.
[0005] The technical solution of the present invention is as follows:
[0006] The proposed method for analyzing and optimizing the lateral stiffness of a vehicle involves three steps: first, performing a basic analysis of Admas handling performance; second, outputting the target lateral stiffness of the vehicle; third, optimizing the lateral stiffness of the vehicle; and finally, conducting analysis verification and real-vehicle acceptance. The specific steps are as follows:
[0007] Step 1: Basic Analysis of Handling Performance
[0008] A basic vehicle control model is established in the Admas control software based on the chassis hardpoint parameters of the actual vehicle, and the basic analysis results are output.
[0009] ADAMS, or Automatic Dynamic Analysis of Mechanical Systems, is a virtual prototyping analysis software developed by MSC Corporation in the United States.
[0010] Step 2: Target output of vehicle lateral stiffness
[0011] Based on the target requirements for improved handling, the following constraints were set: total body roll gain, maximum lateral acceleration, rear axle lateral flexibility gradient, linear understeer gradient, yaw rate overshoot, acceleration pitch angle gradient, and braking pitch angle gradient. The following design variables were set: spring stiffness, yaw ratio, stabilizer bar diameter, damper damping value, toe-adjusting rod bushing stiffness, and lower control arm bushing stiffness. The overall vehicle lateral stiffness was set as the objective function. The optimal target value of the overall vehicle lateral stiffness was obtained through handling performance analysis software.
[0012] Step 3: Optimize the lateral stiffness of the entire vehicle
[0013] A finite element analysis model of the vehicle's lateral stiffness is established based on the vehicle's stress conditions analyzed by the Admas control software, and the vehicle's lateral stiffness is optimized based on the optimal value of the vehicle's lateral stiffness output in step 2.
[0014] This invention establishes an approximate model for analyzing and optimizing the lateral stiffness of the entire vehicle. Constraints and loading are applied to the finite element model based on the actual vehicle handling performance analysis conditions to approximately simulate the deformation of the entire vehicle. First, the finite element model of the entire vehicle is simplified. Then, lateral forces are applied at the front and rear wheel contact points, and the center of gravity of the entire vehicle is constrained, outputting the front and rear lateral stiffness respectively.
[0015] Step 3 specifically includes:
[0016] Step 3.1: Simplify the model:
[0017] The vehicle's lateral stiffness model mainly consists of an interior body model and simplified front and rear suspension models. The interior body finite element model comprises the body-in-white, door closures, interior and exterior trim, and electrical components. The chassis model consists of the steering system and simplified front and rear suspension models using rigid elements. For example, if the subframe is softly connected to the body, the subframe and body are connected via CBUSH elements.
[0018] S1, the front suspension model uses rigid element RBE2 and spring element CBUSH to simulate the actual force transmission path;
[0019] S2, the rear suspension model uses rigid element RBE2 and spring element CBUSH to simulate the actual force transmission path.
[0020] Step 3.2: Front Suspension Operating Conditions Settings
[0021] The front overhang condition is set up with the centroid 22 of the analysis model as the master node and the point on the floor projected from the centroid 22 along the Z direction as the slave node, creating an RBE2 element with 123456 degrees of freedom. The RBE2 master node is constrained using the SUPORT1 constraint type, with constrained degrees of freedom of 123456.
[0022] A load of 1000N is applied along the Y-axis of the vehicle coordinate system at the contact point 1 of the left front tire and the contact point 23 of the right front tire, respectively, and the front suspension condition is established. For details of the constraints and loading positions, please refer to [link to relevant documentation]. Figure 4 The operating conditions are set as follows:
[0023] $HMNAME LOADSTEP 1"FRONT"
[0024] SUBCASE 1
[0025] LABEL = FRONT
[0026] LOAD = 2
[0027] SUPORT1 = 1
[0028] ANALYSIS = STATICS.
[0029] Step 3.3: Rear Suspension Operating Conditions Settings
[0030] The rear suspension load condition is set by simultaneously applying a 1000N load along the Y-axis of the vehicle coordinate system at the left rear tire contact point 14 and the right rear tire contact point 24, with constraints consistent with the front suspension load condition. The rear suspension load condition is set as follows:
[0031] $HMNAME LOADSTEP 2"REAR"
[0032] SUBCASE 2
[0033] LABEL= REAR
[0034] LOAD = 3
[0035] SUPORT1 = 1
[0036] ANALYSIS = STATICS.
[0037] Step 3.4: Solver Setup
[0038] The NASTRAN static load analysis solver SOL101 is used to output lateral displacement. Specific PARAM control parameters are detailed below:
[0039] PARAM, AUTOSPC, YES
[0040] PARAM, BAILOUT, -1
[0041] PARAM, POST, -1
[0042] PARAM, INREL, -1.
[0043] Step 3.5: Result evaluation. Based on the calculation formula of suspension lateral stiffness K, calculate the front lateral stiffness and rear lateral stiffness of the whole vehicle respectively.
[0044]
[0045] In the formula:
[0046] D = (Y1 + Y2) / 2
[0047] Y1 — Displacement of the left front wheel in the Y direction;
[0048] Y2 — Right front wheel displacement in the Y direction;
[0049] F – the sum of the loads applied to the front wheel contact point.
[0050] Step 4: Based on the principle of strain energy superposition, strengthen the vehicle body structure at the locations where large strain energy is concentrated during vehicle deformation.
[0051] Strain energy is the energy generated when the vehicle body is subjected to lateral loads, resulting in structural deformation under the applied load. When the applied force passes through this displacement, the force has done work. This external work, due to the deformation of structural components under load, is stored as strain energy in each structural component.
[0052] To improve the lateral stiffness of a vehicle body, it is necessary to strengthen the beam sections or local structures with the highest strain energy. Increasing the moment of inertia by strengthening the beam sections is the most effective method. Then, finite element analysis is performed, which will result in a new stiffness prediction value and a different strain energy distribution. Therefore, this process continues iteratively until the improved overall vehicle lateral stiffness meets the target requirements. This process often requires multiple iterations and is frequently automated in finite element analysis software.
[0053] Step 5: Substitute the optimized vehicle lateral stiffness analysis value that meets the target into the vehicle handling analysis model for verification, and evaluate whether the various handling indicators have reached the expected values.
[0054] Step 6: Prototype fabrication and on-vehicle verification and evaluation.
[0055] In another aspect, the present invention provides a computer-readable storage medium storing computer-readable instructions that, when executed by a computer's processor, cause the computer to perform the steps of the vehicle lateral stiffness analysis and optimization method described in the first aspect above.
[0056] As can be seen from the above technical solutions, this invention establishes a novel evaluation system for the analysis and optimization of vehicle lateral stiffness to improve overall vehicle handling. Its main advantages are as follows:
[0057] 1. This invention establishes a whole-vehicle stiffness model, incorporating the stiffness of closures, interior trim, and connecting buffer elements into the analysis model, breaking away from conventional methods for evaluating body-in-white stiffness. 2. This invention establishes a new evaluation method for chassis handling performance, using whole-vehicle stiffness as the objective function for handling performance analysis, breaking away from the traditional design method that treats body stiffness as a constant value. 3. This invention simplifies the chassis structure model, avoiding the problem of repeatedly calculating chassis stiffness in handling simulation, and improving the accuracy of ADMAS simulation.
[0058] This invention is applicable not only to traditional gasoline-powered vehicles but also to new energy vehicles. It breaks away from the traditional handling analysis model that typically treats the vehicle body as a rigid body for analysis and optimization, establishing a new alternative model and optimization approach. The method of this invention can be used to evaluate handling performance for different suspension structures, demonstrating strong practicality and scalability. Attached Figure Description
[0059] Figure 1 Flowchart of the method for analyzing and optimizing the lateral stiffness of the whole vehicle;
[0060] Figure 2 Simplified front overhang model;
[0061] Figure 3Simplified left rear overhang model;
[0062] Figure 4 Schematic diagram of lateral stiffness loading;
[0063] Figure 5 Approximate model of front shock absorber;
[0064] Figure 6 Front subframe and steering approximation model
[0065] Figure 7 Approximate model of rear shock absorber;
[0066] Figure 8 Approximate model of rear suspension. Detailed Implementation
[0067] The invention will now be further described with reference to the accompanying drawings.
[0068] like Figure 1 The flowchart shown is a brand-new evaluation system for the analysis and optimization of vehicle lateral stiffness to improve vehicle handling. It includes basic analysis of Admas handling performance, output of vehicle lateral stiffness target, optimization of vehicle lateral stiffness, analysis and simulation verification to final vehicle acceptance.
[0069] Step 1: Basic Analysis of Admas Handling Performance
[0070] A basic vehicle control model is established in the Admas control software based on the chassis hardpoint parameters of the actual vehicle, and the basic analysis results are output.
[0071] The Admas software used in this invention is a mechanical system dynamics simulation and analysis software developed by MDI Corporation in the United States. It uses an interactive graphical environment and parts library, constraint library, and force library to create a fully parametric geometric model of a mechanical system. It is currently one of the most mainstream multibody dynamics analysis software in the world.
[0072] First, open the Admas software and select the Admas / Car module to model the mechanical system. Perform multibody modeling based on the chassis hardpoints, apply kinematic pairs and constraints, and apply loads. Next, perform simulation analysis, replay the simulation results, and plot the simulation curves. Then, verify the simulation results by checking the experimental curves to confirm the reliability of the simulation. If the results are within the error range, further optimization analysis can be performed.
[0073] Step 2: Target output of vehicle lateral stiffness
[0074] Based on the target requirements for improved handling, the following constraints were set: total body roll gain, maximum lateral acceleration, rear axle lateral flexibility gradient, linear understeer gradient, yaw rate overshoot, acceleration pitch angle gradient, and braking pitch angle gradient. The following design variables were set: spring stiffness, yaw ratio, stabilizer bar diameter, damper damping value, toe-adjusting rod bushing stiffness, and lower control arm bushing stiffness. The overall vehicle lateral stiffness was set as the objective function. The optimal target value of the overall vehicle lateral stiffness was obtained through handling performance analysis software.
[0075] Constraints:
[0076] j=1, ..., m
[0077] k=1, ..., m h
[0078] Design variables:
[0079] i=1, ..., n
[0080] Objective function (minimize):
[0081]
[0082] In the formula, g(X) is the inequality constraint function and h(X) is the equality constraint function. The constraints are designed reasonably according to the control performance required by the project. These are design variables. The "L" in the superscript indicates the Lower Limit, and the "U" in the superscript indicates the Upper Limit. The upper and lower limits of the design variables should be reasonably defined according to the vehicle model positioning. It is the objective function, which sets the lateral stiffness of the whole vehicle to be minimized. This ensures that the cost is minimized while improving handling. Stiffness is directly proportional to weight.
[0083] Step 3: Optimize the lateral stiffness of the entire vehicle
[0084] A vehicle lateral stiffness analysis model is established based on the vehicle stress conditions analyzed by the Admas control software, and the vehicle lateral stiffness is optimized based on the optimal value of vehicle lateral stiffness output in step 2.
[0085] This invention establishes an approximate model for analyzing and optimizing the lateral stiffness of the entire vehicle. Constraints and loading are applied to the finite element model based on the actual vehicle handling performance analysis conditions to approximately simulate the deformation of the entire vehicle. First, the finite element model of the entire vehicle is simplified. Then, lateral forces are applied at the front and rear wheel contact points, and the center of gravity of the entire vehicle is constrained, outputting the front and rear lateral stiffness respectively.
[0086] The following description, in conjunction with the accompanying drawings and examples, further illustrates this step.
[0087] Step 3.1: The vehicle lateral stiffness model mainly consists of the interior body model and simplified front and rear suspension models. The interior body finite element model consists of the body-in-white, closures, interior and exterior trim, and electrical components. The chassis model consists of the steering system and simplified front and rear suspension models using rigid elements. If the subframe is softly connected to the body, the subframe and body are connected via CBUSH elements.
[0088] S1, the front suspension model uses rigid element RBE2 and spring element CBUSH to simulate the actual force transmission path, such as Figure 2 As shown.
[0089] Create an RBE2 element with front wheel contact point 1 as the master node and front wheel center 2 as the slave node. Use the center node 3 of the front shock absorber support as the master node, and the surrounding slave nodes include the center node of two rows of nodes and three bolt holes (this node is the master node of RBE2, and the slave nodes are the nodes around the bolt holes). Couple all 6 degrees of freedom to create the front shock absorber connection RBE2 element.
[0090] Create nodes by installing center point 3 on the front shock absorber, center point 4 on the outer steering ball joint, and center point 5 on the swing arm ball joint.
[0091] Using the front wheel center point 2 as the master node, and the center points 3 of the front shock absorber support, 4 of the outer steering ball joint, and 5 of the swing arm ball joint as slave nodes, create an RBE2 element. The connection between the vehicle body and the center node 3 of the front shock absorber support is simulated using a zero-length CBUSH element. The CBUSH element is placed in the global coordinate system, and the stiffness in the X and Y rotation directions of the CBUSH is defined as infinitesimal. Figure 5 As shown.
[0092] Create a node at the center point 9 of the left inner steering ball joint, with the center point 4 of the outer steering ball joint as the master node and the center point 9 of the left inner steering ball joint as the slave node, and create the steering ball joint RBE2 element.
[0093] Create nodes at the center point 11 of the front swing arm bushing and the center point 8 of the rear swing arm bushing, with the center point 5 of the swing arm ball joint as the master node and the center point 11 of the front swing arm bushing and the center point 8 of the rear swing arm bushing as the slave node, and create the RBE2 element.
[0094] The ball joint of the swing arm is simulated using zero-length CBUSH elements. One end of the CBUSH element is connected to the wheel center RBE2 element, and the other end is connected to the swing arm RBE2 element. The CBUSH element is placed in the global coordinate system, and the stiffness of the CBUSH element in the X, Y, and Z rotation directions is defined as infinitesimal.
[0095] With the center point 11 of the front swing arm bushing as the master node and the two rows of nodes at the bolt mounting holes of the front swing arm attachment point as slave nodes, an RBE2 element is created. The front swing arm bushing is simulated using a zero-length CBUSH element. The CBUSH element is placed in the global coordinate system, and the stiffness of the CBUSH element in the X, Y, and Z rotation directions is defined as infinitesimal.
[0096] The rear swing arm bushing is simulated using CBUSH elements. The center point 11 of the front swing arm bushing is the origin. A local coordinate system is created with the positive Z direction pointing from the center of the front swing arm bushing to the center of the rear swing arm bushing. The CBUSH elements are placed in this local coordinate system, and the stiffness of the CBUSH elements in the X, Y, and Z rotation directions is defined as infinitesimal.
[0097] The outer steering ball joint is simulated using a zero-length CBUSH element. A local coordinate system is created with the center point 4 of the outer steering ball joint as the origin, pointing from the center of the outer steering ball joint to the center of the inner steering ball joint in the positive Z direction. The CBUSH element is placed in this local coordinate system, and the stiffness of the CBUSH in the X, Y, and Z rotation directions is defined as infinitesimal.
[0098] Create an RBE2 element with the left inner steering ball joint center point 9 as the master node and the inner surface node of the sleeve at the connection between the steering cross tube and the front subframe as the slave node. Create a steering cross tube RBE2 element with the left inner steering ball joint center point 9 as the master node and the right inner steering ball joint center point 10 as the slave node.
[0099] The inner steering ball joint is simulated using zero-length CBUSH elements. A local coordinate system is created with the center point 4 of the outer steering ball joint as the origin, pointing in the positive Z direction from the center of the outer steering ball joint to the center of the inner steering ball joint. The CBUSH element is placed in this local coordinate system, and the stiffness of the CBUSH element in the X, Y, and Z rotation directions is defined as infinitesimal. Figure 6 As shown.
[0100] S2, the rear suspension model uses rigid element RBE2 and spring element CBUSH to simulate the actual force transmission path, such as Figure 3 As shown.
[0101] Create nodes at the center point 18 of the rear trailing arm bushing, the center point 15 of the tie rod outer bushing, the center point 12 of the upper swing arm outer bushing, the center point 16 of the lower swing arm outer bushing, the center point 17 of the lower bushing of the rear shock absorber, the center point 13 of the rear wheel, and the center point 11 of the shock absorber support.
[0102] Create an RBE2 element with rear wheel contact point 14 as the master node and rear wheel center point 13 as the slave node. Create another RBE2 element with the center point 11 of the shock absorber support as the master node and the RBE2 master node created from the two bolt holes as the slave nodes.
[0103] Create an RBE2 element with the rear wheel center point 13 as the master node, and the following nodes as slave nodes: rear trailing arm bushing center point 18, tie rod outer bushing center point 15, rear shock absorber lower bushing center point 17, upper control arm outer bushing center point 12, and lower control arm outer bushing center point 16. Similarly, create an RBE2 element with the shock absorber lower bushing center point 17 as the master node and the shock absorber support center point 11 as the slave node. Figure 7 As shown.
[0104] The damper support is simulated using a zero-length CBUSH element. A local coordinate system is created with the center point 17 of the lower bushing of the damper as the origin, pointing from the center of the lower bushing to the center of the damper support in the positive Z direction. The CBUSH element is placed in this local coordinate system, and the stiffness of the CBUSH element in the X and Y rotation directions is defined as infinitesimal.
[0105] The lower bushing of the rear shock absorber is simulated using a zero-length CBUSH, which shares a local coordinate system with the shock absorber support CBUSH. The stiffness of the CBUSH in the X, Y, and Z rotation directions is defined as infinitesimal.
[0106] The rear trailing arm bushing is simulated using a zero-length CBUSH element, and the CBUSH stiffness parameters and coordinate system adopt the actual parameters of the whole vehicle.
[0107] Create a node at the center point 20 of the inner bushing of the tie rod. Create the tie rod RBE2 element with the center point 15 of the outer bushing of the tie rod as the master node and the center point 20 of the inner bushing of the tie rod as the slave node.
[0108] Create a node at the center point 21 of the upper swing arm inner bushing. Create the upper swing arm RBE2 element with the center point 12 of the upper swing arm outer bushing as the master node and the center point 21 of the upper swing arm inner bushing as the slave node.
[0109] Create a node at the center point 19 of the lower swing arm inner bushing. Create the lower swing arm RBE2 element with the center point 16 of the lower swing arm outer bushing as the master node and the center point 19 of the lower swing arm inner bushing as the slave node.
[0110] The outer bushing of the tie rod is simulated using zero-length CBUSH elements. A local coordinate system is created with the center point 15 of the outer bushing of the tie rod as the origin, pointing from the center of the outer bushing to the center of the inner bushing of the tie rod in the positive Z direction. The CBUSH elements are placed in this local coordinate system, and the stiffness of the CBUSH elements in the X, Y, and Z rotation directions is defined as infinitesimal.
[0111] The inner bushing of the tie rod is simulated using a zero-length CBUSH element, which shares a coordinate system with the outer bushing of the tie rod, and the stiffness of the CBUSH in the X and Y rotation directions is defined as infinitesimal.
[0112] The lower control arm outer bushing is simulated using zero-length CBUSH elements. A local coordinate system is created with the center point 16 of the lower control arm outer bushing as the origin, pointing from the center of the lower control arm outer bushing to the center of the lower control arm inner bushing in the positive Z direction. The CBUSH elements are placed in the local coordinate system, and the stiffness of the CBUSH elements in the X, Y, and Z rotation directions is defined as infinitesimal.
[0113] The lower control arm inner bushing is simulated using a zero-length CBUSH element, which shares a coordinate system with the lower control arm outer bushing CBUSH. The stiffness of the CBUSH in the X and Y rotation directions is defined as infinitesimal.
[0114] The upper swing arm outer bushing is simulated using zero-length CBUSH elements. Taking the center point 12 of the upper swing arm outer bushing as the origin, a local coordinate system is created with the positive Z direction pointing from the center of the upper swing arm outer bushing to the center of the upper swing arm inner bushing. The CBUSH element is placed in the local coordinate system, and the stiffness of the CBUSH element in the X, Y, and Z rotation directions is defined as infinitesimal.
[0115] The inner bushing of the upper swing arm uses a zero-length CBUSH element, which shares a coordinate system with the outer bushing of the upper swing arm CBUSH. The stiffness of the CBUSH in the X and Y rotation directions is defined as infinitesimal.
[0116] Step 3.2: Set the front overhang condition to create an RBE2 element with 123456 degrees of freedom, using the centroid 22 of the analysis model as the master node and the point projected from the centroid 22 along the Z direction onto the floor as the slave node. Constrain the RBE2 master node using the SUPORT1 constraint type, with a constraint degree of freedom of 123456.
[0117] A load of 1000N is applied along the Y-axis of the vehicle coordinate system at the contact point 1 of the left front tire and the contact point 23 of the right front tire, respectively, and the front suspension condition is established. For details of the constraints and loading positions, please refer to [link to relevant documentation]. Figure 4 .
[0118] The operating conditions are set as follows:
[0119] $HMNAME LOADSTEP 1"FRONT"
[0120] SUBCASE 1
[0121] LABEL = FRONT
[0122] LOAD = 2
[0123] SUPORT1 = 1
[0124] ANALYSIS = STATICS.
[0125] SUPORT1 is used to eliminate the degrees of freedom Ur of rigid body motion in static analysis. A set of constraints must be given, which can be single-point or multi-point constraints, or given according to the supports of the free body. Singularities can be eliminated by restricting a sufficient number of degrees of freedom Ur.
[0126]
[0127] in:
[0128] G—Grid point or scalar point identifier (integer, >0);
[0129] C — Component number (integer, 0≤C≤6)
[0130] The stiffness equation of set a can be written in block form:
[0131]
[0132] In the formula:
[0133]
[0134] The displacement set ur is given by the user according to the SUPORT 1 card and is set to zero. P is the set of all external forces acting on the degrees of freedom, therefore the second equation has
[0135]
[0136] Stiffness matrix Since it is a non-singular matrix, the displacement set ul can be obtained.
[0137] Step 3.3: The rear suspension load condition is set by simultaneously applying a 1000N load along the Y-axis of the vehicle coordinate system at the left rear tire contact point 14 and the right rear tire contact point 24, with constraints consistent with the front suspension load condition. The rear suspension load condition is set as follows:
[0138] $HMNAME LOADSTEP 2"REAR"
[0139] SUBCASE 2
[0140] LABEL= REAR
[0141] LOAD = 3
[0142] SUPORT1 = 1
[0143] ANALYSIS = STATICS
[0144] Step 3.4: Solver setup. The NASTRAN static load analysis solver SOL101 is used to output lateral displacement. Specific PARAM control parameters are detailed below:
[0145] PARAM, AUTOSPC, YES
[0146] PARAM, BAILOUT, -1
[0147] PARAM, POST, -1
[0148] PARAM, INREL, -1.
[0149] AUTOSPC, YES controls the automatic elimination of true singularities, that is, adding the identified singularities to the set. It is mainly used for those degrees of freedom that are freely determined at GRID points but are not related to the finite element model, which need to be eliminated. These include nonplanar states in planar problems, rotational degrees of freedom of thin films and blocks, and normal phase rotation of plates and shells.
[0150] POST, -1, typically used for preprocessing and post-processing data blocks, is stored in the database and converted into a processable format via the DBC module. These data blocks include input data related to geometry, connectivity, element and material properties, and static loads.
[0151] Where BAILOUT, -1 causes the program to continue processing approximate singularities; if the value is 0, the program exits when an approximate singularity is detected.
[0152] The main function of the INERL setting is to define the balance between external forces and inertial forces. When selecting a set of forces Pa and applying them to a set a representing the displacements of a non-equilibrium set, a condition must be defined to prevent the influence of inertial forces; this is called inertia elimination. In Nastran calculations, inertia elimination must be performed using SUPORT 1 and INREL, -1 together. The main steps are as follows:
[0153] 1. Select a specific set of support points, i.e., set r, which is defined in SUPORT 1 card. In this invention, it refers to the center of gravity 22 of the whole vehicle model.
[0154] 2. Determine the rigid body acceleration of set r based on the loads acting on set a of degrees of freedom.
[0155] 3. Calculate the acceleration of the set of degrees of freedom l;
[0156] 4. Subtract the inertial force generated by the acceleration of the free set l from the external load Pl, and solve for the displacement set obtained by the constraint set r. The reaction force of the set of degrees of freedom r will be zero.
[0157] After decomposing the set a into sets l and r (where the degrees of freedom in set r are just enough to eliminate rigid body motion), we can obtain the equations of motion containing inertia elimination. Therefore, sets l and r are linked by the defined rigid body transformation matrix. Thus, dividing the equations of set a into sets l and r, we obtain the simplified mass matrix:
[0158]
[0159] The simplified mass matrix is obtained through the following transformation:
[0160]
[0161] The transformation matrix has already linked set a with set r, and therefore can be represented by the rigid body transformation matrix as follows:
[0162]
[0163] The set of forces associated with set r can also be simplified in a similar way:
[0164]
[0165] Since the stiffness matrix of set r is all zero, the equations of motion become
[0166]
[0167] Now, we can determine that the acceleration of set r is
[0168]
[0169] The acceleration of set l becomes
[0170]
[0171] By partitioning the mass matrix, the inertial forces associated with set l can now be determined as follows:
[0172]
[0173] In the formula, ql is the inertial force. These forces can be expressed as follows using the above formula:
[0174]
[0175] When considering the effects of inertia elimination, the inertial force can be added to the set of loads acting on it.
[0176] Step 3.5: Result evaluation. Based on the calculation formula of suspension lateral stiffness K, calculate the front lateral stiffness and rear lateral stiffness of the whole vehicle respectively.
[0177]
[0178] In the formula:
[0179] D = (Y1 + Y2) / 2
[0180] Y1 — Displacement of the left front wheel in the Y direction;
[0181] Y2 — Right front wheel displacement in the Y direction;
[0182] F – the sum of the loads applied to the front wheel contact point.
[0183] Step 4: Based on the principle of strain energy superposition, strengthen the vehicle body structure at the locations where large strain energy is concentrated during vehicle deformation.
[0184] Strain energy is the energy generated when the vehicle body is subjected to lateral loads, resulting in structural deformation under the applied load. When the applied force passes through this displacement, the force has done work. This external work, due to the deformation of structural components under load, is stored as strain energy in each structural component.
[0185] To improve the lateral stiffness of the vehicle body, it is necessary to strengthen the beam sections or local structures with the highest strain energy. Increasing the moment of inertia by strengthening the beam sections is the most effective method. Then, finite element analysis is performed, which will result in a new stiffness prediction value and a different strain energy distribution. We continue this process iteratively until the improved overall vehicle lateral stiffness meets the target requirements. This process often requires multiple iterations and can be automated in finite element analysis software.
[0186] Step 5: Substitute the optimized vehicle lateral stiffness analysis value that meets the target into the vehicle handling analysis model for verification, and evaluate whether the various handling indicators have reached the expected values.
[0187] Step 6: Prototype fabrication and on-vehicle verification and evaluation.
[0188] The above description, using a specific case study of handling optimization for a particular vehicle model, is a detailed account of the present invention. It is provided to facilitate understanding and application of the analytical and design techniques by those skilled in the art, and should not be construed as limiting the specific implementation of the invention to these descriptions. Any variations or substitutions that can be easily conceived by those skilled in the art within the scope of the disclosed technology should be included within the protection scope of the present invention. Therefore, the protection scope of the present invention should be determined by the scope of the claims.
Claims
1. A method for analyzing and optimizing the lateral stiffness of a vehicle, characterized in that, include: Step 1: Basic Analysis of Handling Performance A basic vehicle handling model is established in the handling analysis software based on the chassis hard point parameters of the actual vehicle, and the basic analysis results are output. Step 2: Target output of vehicle lateral stiffness: Based on the target requirements for improving handling, constraints and design variables are set, and the vehicle lateral stiffness is used as the objective function to obtain the optimal target value of vehicle lateral stiffness through handling performance analysis software. Step 3: Optimize the lateral stiffness of the entire vehicle: A finite element analysis model of the vehicle's lateral stiffness is established based on the vehicle's stress conditions analyzed by the control analysis software, and the vehicle's lateral stiffness is optimized based on the optimal target value of the vehicle's lateral stiffness. Step 4: Strengthen the vehicle body structure, conduct finite element verification analysis, and iterate multiple times until the lateral stiffness of the whole vehicle meets the target requirements.
2. The method of claim 1, wherein, Also includes: Step 5: Analysis and Verification: Substitute the optimized vehicle lateral stiffness analysis value that achieves the target into the vehicle handling analysis model for verification, and evaluate whether the various handling indicators have reached the expected values. Step 6: Vehicle Acceptance: Prototype is made and verified and evaluated on a real vehicle.
3. The method of claim 1, wherein, Also includes: The handling performance analysis software used is Admas, Motionview, Carsim, or Vi-Grade.
4. The method of vehicle lateral stiffness analysis and optimization of claim 1, 2 or 3, wherein, In the target output of the vehicle lateral stiffness in step 2, the total body roll gain, maximum lateral acceleration, rear axle lateral flexibility gradient, linear segment understeer gradient, yaw rate overshoot, acceleration pitch angle gradient, and braking pitch angle gradient are set as constraints.
5. The method of vehicle side stiffness analysis and optimization of claim 1, 2 or 3, wherein, In the target output of the vehicle lateral stiffness in step 2, the spring stiffness, skew ratio, stabilizer bar diameter, shock absorber damping value, toe-in adjustment rod bushing stiffness, and lower control arm bushing stiffness are set as design variables.
6. The method for analyzing and optimizing the lateral stiffness of a vehicle according to claim 4, characterized in that, In step 2, Constraints: j=1, ..., m k=1, ..., m h Design variables: i=1, ..., n Objective function: In the formula, g(X) is the inequality constraint function and h(X) is the equality constraint function. The constraints are designed reasonably according to the control performance required by the project. These are design variables. L stands for lower limit, and U stands for upper limit. The upper and lower limits of the design variables should be reasonably defined according to the vehicle model positioning. It is the objective function, which sets the lateral stiffness of the entire vehicle to be minimized.
7. The method for analyzing and optimizing the lateral stiffness of a vehicle according to claim 1 or 2, characterized in that, The vehicle lateral stiffness optimization in step 3 is achieved by first simplifying the vehicle finite element model, then applying lateral forces at the front and rear wheel contact points respectively, constraining the vehicle's center of gravity, outputting the front and rear lateral stiffness respectively, and optimizing the vehicle lateral stiffness based on the optimal target value.
8. The method for analyzing and optimizing the lateral stiffness of a vehicle according to claim 7, characterized in that, Step 3 includes: Step 3.1: Simplify the finite element model of the whole vehicle: The model for the lateral stiffness of the whole vehicle includes the interior body finite element model and the chassis model; the interior body finite element model includes the body-in-white, closures, interior and exterior trim and electrical components; the chassis model includes the steering system and simplified front and rear suspension models with rigid elements. The front suspension model uses rigid element RBE2 and spring element CBUSH to simulate the actual force transmission path, and the rear suspension model uses rigid element RBE2 and spring element CBUSH to simulate the actual force transmission path. Step 3.2: Front suspension operating condition settings: Using the centroid of the analysis model as the master node and the point projected from the centroid along the Z-axis onto the floor as the slave node, create an RBE2 element with 123456 degrees of freedom; constrain the RBE2 master node using the SUPORT1 constraint type, with a constraint degree of freedom of 123456. Loads are applied along the Y-axis of the vehicle coordinate system at the contact points of the left front tire and the right front tire, respectively, and the front suspension condition is established. Step 3.3: Rear Suspension Operating Conditions Settings At the contact point of the left rear tire and the contact point of the right rear tire, loads are applied simultaneously along the Y direction of the vehicle coordinate system, and the constraints are consistent with the front suspension condition to establish the rear suspension condition. Step 3.4: Solver Setup: The static load analysis solver is used to solve the problem and output the lateral displacement. Step 3.5: Result Evaluation: Based on the formula for calculating the suspension lateral stiffness K, the front and rear lateral stiffness of the entire vehicle are calculated respectively: In the formula: D = (Y1 + Y2) / 2, Y1 is the Y-direction displacement of the left front wheel, Y2 is the Y-direction displacement of the right front wheel, and F is the sum of the loads applied to the front wheel contact point.
9. The method for analyzing and optimizing the lateral stiffness of a vehicle according to claim 1, characterized in that, In step 4, based on the principle of strain energy superposition, the vehicle body structure is reinforced at the location where the strain energy is concentrated due to large vehicle body deformation.
10. A computer-readable storage medium, characterized in that, It stores computer-readable instructions, which, when executed by the computer's processor, cause the computer to perform the steps of the vehicle lateral stiffness analysis and optimization method as described in any one of claims 1 to 9.