Development of a Durable Automotive Bushing with fe-safe/rubber

Transcription

1 Development of a Durable Automotive Bushing with fe-safe/rubber Jing Bi, Gergana Dimitrova, Sandy Eyl Dassault Systemes Simulia Corp 1301 Atwood Ave, Suite 101W, Johnston RI Abstract Fatigue life prediction is critical to assure the safety and reliability of automotive bushings. Bushings are usually made of rubber type materials that act as cushions between rigid members and are often of complex shape. The stiffness characteristic of the bushings is sensitive to the multi-body dynamics, noise and vibration of a vehicle. Given that an experimental program to evaluate bushing performance may cost between 20k to $200k USD, developing a durable automotive bushing can be challenging. In this paper, fatigue life prediction methodologies provided by fe-safe/rubber combining with finite element analyses, and optimization methods were utilized to develop a durable automotive bushing made of natural rubber. The proposed geometric design of the automotive bushing was obtained by a parametric optimization with the use of Abaqus finite element analyses ensuring the stiffness compliances in multiple loading directions. This procedure was automated by the process automation capability of Isight. The stresses and strains at critical locations from the finite element analysis of the proposed geometric design were then incorporated with the surface algorithm in fe-safe/rubber enforcing a plane stress condition and the Lake-Linley fatigue model. The fatigue life prediction was driven iteratively by the Tosca non-parametric optimization in order to find the more durable designs. Keywords: rubber bushing; fatigue life prediction, durability, parametric optimization; nonparametric optimization; Finite Element Analysis (FEA). Introduction Rubber bushings are used in vehicle designs to avoid metal-to-metal direct contact. They are widely adopted in the body mount, control arm mount, stabilizer bar mount and etc. systems of a vehicle for vibration control. The design of a rubber bushing must meet the preferred compliance and reduce vehicle noise and vibration [1]. In addition, rubber bushings need to survive multiaxial, variable amplitude load histories and meet the warranty life. Designing rubber bushings can be time consuming and expensive. A bushing test program including mold development, prototype production, multi-axial servohydraulic component testing, 4-poster testing and fleet testing could cost from 20,000 up to 200,000 US dollars [2]. Fatigue life and stiffness prediction are critical to assure the compliance and reliability of automotive bushings. In this paper, fatigue life prediction methodologies provided by fe-safe/rubber [3][4] combining with finite element analyses, and optimization methods were utilized to develop a durable automotive bushing made of natural rubber. The proposed geometric design of the automotive bushing was obtained by a parametric optimization with the use of Abaqus finite element analyses ensuring the stiffness compliances in multiple loading directions. This procedure was automated by the process automation capability of Isight. The stresses and strains at critical locations from the finite element analysis of the proposed geometric design were then incorporated with the surface

2 algorithm in fe-safe/rubber enforcing a plane stress condition and the Lake-Linley fatigue model. The fatigue life prediction was driven iteratively by the Tosca [5] non-parametric optimization in order to find the more durable designs. The final design satisfies the preferred stiffness compliance and improved durability targets. Finite element modeling In order to accurately analyze the bushing behavior under multi-axial variable amplitude loadings, FEA is adopted. The commercial FEA code Abaqus/Standard [6] is used in this study. The geometry of rubber bushings can become very complicated depending on application and purpose. For illustration purpose, the rubber bushing analyzed in this paper is one that connects a cylindrical inner metal to an outer metal housing with a cylindrical inner geometry. It is assumed that the geometry of the inner metal and outer metal housing are pre-determined in previous design stages and that the inner and outer radius of the rubber bushing cannot be changed. It is also assumed that the adhesive area of the bushing to the inner metal and outer metal housing is also pre-determined and fixed. The analyst is left to change the free surfaces of the bushing including the curved external surfaces of the bushing and shape/size of the voids to achieve a desired bushing behavior. The FEA model of the rubber bushing is modeled using hyperelastic material and hybrid solid elements (C3D4H or C3D8H) provided in Abaqus/Standard. For precise stress and durability analyses hexahedral mesh is used. A membrane section is modeled on the top free surface of the rubber bushing for accurate strain representation of the plane stress condition. The membrane section shares common nodes with the free surface of the rubber bushing and has a very small thickness so that the model stiffness is not affected. The stress strain history data are subsequently used in the fatigue analysis for precise fatigue life calculation. Due to symmetry, only the upper half of the bushing is modeled and symmetric boundary conditions are placed on the middle plane. The inner metal and outer metal housing are modeled as rigid bodies. Tie constraint is used to connect the rigid bodies and the deformable bushing. Loading is applied to the reference node of the inner metal rigid body in both translational (x, z) and rotational (y) directions. The effects of manufacturing processes such as cool down and swaging, on the stress strain responses tend to cancel out each other [7] and are therefore ignored in this study for simplicity. However, these can be included in multi-step Abaqus analysis if their effects are determined to be significant. Two bean shaped voids are symmetric. The rubber bushing exhibits varying stiffness response due to the material properties and the closing of these voids when highly deformed and contacted. Automatic general contact is used between the rubber bushing and itself when the void closes. The FEA model of the rubber bushing component is illustrated in Figure 1. Parametric optimization In this study, we allow the shape of the voids to be adjusted to achieve the preferred bushing compliance. As an example, it is assumed that the void is bean shaped consisting of two arcs cocentered at the center of the cross section and two small half circles at the two sides (Figure 2). The width of the void w, the distance from the center of the void to the center of the bushing r, and the span angle θ are the design parameters. The design range of each parameter is chosen

3 as shown in Table 1. A Python script is developed to generate the finite element model of the rubber bushing given any values of the design parameters within the defined design space. The script does the geometry/part creation, material and section definition and assignment, assembly creation, boundary condition and constraint application, partition, seeding and meshing, loading and step definitions automatically. Among all these steps, the sketching, partitioning, and meshing need special care during scripting so that models can be generated with any given values of the design variables. The modeling time is reduced from hours to 1 minute via a command line. The script allows effective use of Isight iterative optimization processes. The Isight workflow includes five components (Figure 3): A Simcode component that runs a Python script to generate the parameterized finite element model of a rubber bushing in Abaqus/CAE and writes the Abaqus input file; A Simcode component that runs the input file using Abaqus/Standard to solve for the nonlinear problem of the bushing loaded under multi-axial loads with self-contact; A Simcode component that runs a second Python script to extract the reaction force/moment and displacement/rotation and generate the stiffness response curves; A data matching component that compares the difference between the stiffness responses of the current design to the preferred targets; An optimization component that solves for the geometric parameters of the next proposed design and feeds the new design parameters to the first component. The first Simcode component runs an Abaqus python script without using a GUI. The python script includes lines defining 3 design variables. These are chosen as input parameters for the Simcode component and are mapped to the optimization component as a dataflow. The Python script is used as the input file for the Simcode component. The component generates the parameterized finite element model of the rubber bushing and writes the Abaqus input file to the working directory. The second Simcode component includes a command line to run the input file using the Abaqus/Standard solver and generates the output database (.odb file) to the working directory. The third Simcode component runs another Python script that extracts the reaction force/moment and displacement/rotation history output of the measuring point and writes the data into a text file. This text file as well as a text file that defines the target stiffness curves are defined as the input for the data matching component which then compares the sum of absolute differences between the stiffness curves of the current design and the target stiffness curves. The sums of differences of the 3 loaded directions are mapped to the optimization component. The Downhill Simplex optimization technique is adopted in the optimization component and is proved to obtain satisfactory optimum results with matching stiffness compliances. Downhill Simplex is an exploratory technique that samples the design space across a sub-region and moves from the worst point in the direction of the opposite face of the simplex toward better solutions. In this study, we used an initial simplex size of 0.1 (10% of design domain as the size of the starting simplex) and max iterations of 40. There are 3 design variables in this optimization as indicated above (w, r and θ) and the design objective is to minimize the sum of the absolute difference between the stiffness curves from the current design and the target stiffness curves in

4 the 3 loaded directions. Each loading direction is given a weighting factor of 1. The Isight workflow set up is shown in Figure 3. Optimum geometry is reached at r = mm, θ = 43.36º, w = 7.21 mm. Figure 4 shows the stiffness curves in the 3 loaded directions of the initial design, optimum design and preferred target. It is shown that the optimum design exhibits the required stiffness compliance. Non-parametric shape optimization based on fatigue life prediction Tosca non-parametric shape optimization allows for detail oriented improvement to an existing design, and is typically used at the end of the design process to fine tune a response such as stress or fatigue life. The surface geometry can be iteratively changed, using a minimization technique to achieve stress homogenization for instance. For rubber materials, this can usually be achieved by minimizing the max principal stress of the free surface [8]. fe-safe/rubber may then be used to quickly assess the fatigue life improvement of the elastomers in the bushing. However, in this paper, we take advantage of the combined use of fe-safe/rubber and Tosca to improve the worst life of the rubber component directly. The benefit of this approach is that the optimization is based directly on the fatigue life of each node on the free surface instead of maximum principal stress, which may not represent the worst life location in complex load conditions [9]. Abaqus/Standard is used to solve for the stress and strain distribution and history on the free surface of the bushing. Tosca drives the Abaqus and fe-safe jobs, reads the nodal fatigue results given by fe-safe and iteratively optimizes the shape of the free surface to maximize the fatigue life. The process starts with an Abaqus/Standard model, and sequentially runs the fe-safe analysis given the output.odb database from Abaqus. fe-safe writes nodal fatigue life data to the.csv database. Tosca then reads the life data and writes the new Abaqus input file with slightly revised free surface shapes. This workflow is iterated until the maximum number of iterations is reached (Figure 5). The controller approach is adopted to reduce stress concentration and reduce damage value/increase fatigue life. The design area is the free surface that includes the top curved surface and the surfaces on the two voids (Figure 6). All highlighted nodes are design nodes which Tosca modifies in order to find an optimal shape. Stamping constraint is applied to the voids to ensure manufacturability. Planar symmetry constraints are applied to all the design nodes to ensure that during the surface modification the symmetry of the bushing and the openings will be preserved. Freeze constraint is applied to nodes that are tied to the inner metal and outer metal housing. Mesh smoothing condition is applied to all of the elements of the rubber bushing. The purpose is to adjust not only the position of the nodes on the design surface, but also adjust underlying nodes accordingly to avoid mesh distortion. The optimization objective is to minimize the damage value defined as below: = 1 log where N is the number of cycles to fatigue failure.

5 Due to the severe deformation, the stresses and strains vary widely throughout the design area. Setting manually a reference damage value helps exercise special control on how the surface is modified based on the damage field distribution. The surface is moved outwards at areas where the damage is higher than the reference value and inwards at areas with damage lower than the reference value. Thus the reference value outlines a contour on the surface around which the surface grows or shrinks. The reference damage value also serves as target value around which the damage is homogenized thereby ensuring that each optimum design will have similar level of fatigue life improvement. In this example a reference damage value is chosen as 150% increase in number of cycles. This becomes important later when stiffness targets need to be adjusted. fe-safe/rubber is used as the fatigue life solver for the rubber bushing. The fatigue material definition is chosen as the natural rubber material from the Endurica material database (NR_GUM). Mooney Rivlin hyperelastic material is defined with the following modulus: Bulk modulus K = 3000 MPa; C01 = 0.1 MPa; C10 = 2.0 MPa. The algorithm comes from the fesafe/rubber plug-in, and is a surface algorithm, applied to the membrane elements defined on the surface of the finite element model, enforcing a plane stress condition. This algorithm calculates the number of cycles from an assumed initial crack length to final crack length using the cracking energy density criterion with a critical plane approach to determine crack direction. The load is applied as a sequence of stresses and strains from the Abaqus simulation result. The fatigue life is calculated based on the number of repeats of a single load step. This is regarded as a simplified loading for relative durability comparisons of different designs. For more accurate life prediction, load cycle data should be obtained from road load test data and included in the fesafe analysis through customized load data file. Environmental temperature effect is ignored here but can be included as well in fe-safe/rubber. An fe-safe macro was developed that contains macro command lines to read the necessary variables from the frames in the Abaqus results, select analysis groups, load fe-safe/rubber plugin and run the analysis. An fe-safe project definition file was also created that contains all the project definitions such as FEA model units, material data, fatigue algorithm, output format. Tosca calls the fe-safe macro and drives fe-safe analysis in each iteration of the shape optimization. No manual fe-safe job set up is necessary during the optimization. Figure 7 shows the damage values at the critical location two ends of the bean shaped voids before and after the shape optimization. It can be observed that damage value is only slightly reduced. However, if converted to worst life in number of cycles, the fatigue life increases from 9101 to (Figure 8). This is a ~77% increase of number of cycles to fatigue. A maximum number of 12 iterations are performed. And the optimum design is found at the 8 th iteration. The total optimization cost is 2 hr on a single CPU. Validation runs in Abaqus and fe-safe are performed to confirm the optimization results. Figure 9 shows the log of life from the validation run in fe-safe and results match with the optimization results after conversion from damage value to log life. Stiffness correction The fine tuning of the external free surface shapes during the shape optimization may slightly change the bushing stiffness compliance. In this research, it is found that the new stiffness curves

6 are about 10% lower than the preferred curves. In order to correct the stiffness decrease and precisely achieve the preferred stiffness compliance, the two optimization steps are repeated once with elevated preferred stiffness compliance. The reference damage value in the 2 nd shape optimization is chosen the same as the 1 st shape optimization: 150% fatigue life increase. This helps ensure that the optimum design after the 2 nd shape optimization has comparable level of stiffness decrease. A higher stiffness (110% original target) is now preferred and achieved during the parametric optimization and used as the initial design during the non-parametric optimization. Figure 10 shows the resulting stiffness responses in each loading direction. The stiffness curves of the optimum design from the 2 nd shape optimization matches well with those of the original design target. Figure 11 shows the worst life in number of cycles increases from 6833 to 13662, which is a ~100% fatigue life improvement. A maximum number of 12 iterations are performed. And the optimum design is found at the 6 th iteration. The total optimization cost is 2 hr 23 min on a single CPU. Validation runs in Abaqus and fe-safe are performed and the log life contour matches with the optimization results, as shown in Figure 12. Conclusions In this study, an automated workflow is presented for the design engineers to obtain an optimum design of the rubber bushing that satisfies the preferred stiffness compliance and improves fatigue life by approximately two times. The workflow combines the usage of numerical fatigue analysis of elastomers and optimization methodology with FEA. First a Python script is developed to generate the parameterized FEA model of the rubber bushing given a set of design parameters. This script was used by Isight to carry out a parametric optimization. The parametric optimization effectively catches the optimum design that exhibits matching stiffness compliance in all 3 loaded directions. This is followed by a non-parametric shape optimization to maximize the fatigue life of the bushing. The non-parametric shape optimization improves the fatigue life by 77%. It is found that the non-parametric shape optimization reduces the stiffness compliance slightly by 10%. This is corrected by repeating the two optimization procedures while increasing the initial stiffness targets by 10%. The final optimum design satisfies the stiffness requirements accurately while exhibit a 100% longer fatigue life comparing to the parametrically optimized design. References [1] Kim, J.J., Kim, H.Y., Shape Design of an Engine Mount by a Method of Parameter Optimization, Computers & Structures, Vol. 65, No. 5, 1997, pp [2] Sarkar, M. and Mars, W.V., Choosing the right material in a rubber bushing operating under variable amplitude loading, Simulia Central RUM Minneapolis MN, Sept 25, [3] fe-safe 6.5 User Manual, Dassault Systèmes Simulia Corp., [4] fe-safe/rubber 2.22 Manual, Endurica LLC, Findlay, OH, USA, [5] SIMULIA Tosca Structure Documentation 8.1, Dassault Systèmes Simulia Corp., May 2014.

7 [6] Abaqus Analysis User s Guide, Abaqus 6.14, Dassault Systèmes Simulia Corp., [7] Paige, R. E., Cooper Standard Automotive, FEA in the Design Process of Rubber Bushings, ABAQUS Users' Conference, Newport, Rhode Island, May 2002, pp [8] Flamm and Weltin, Lifetime prediction of multiaxially loaded rubber springs and bushings, Proceedings of the thrid European conference on constitutive models for rubber, London, England, Sept 15-17, 2003 [9] Zarrin-Ghalami, T., Fatemi, A., Multiaxial fatigue and life prediction of elastomeric components, International Journal of Fatigue, Vol. 55, 2013, pp

8 Figure 1 Finite element model of a rubber bushing

9 Figure 2 Geometric design parameters

10 Figure 3 Isight parametric optimization workflow

11 Isight target Initial design Optimum design Reaction force RF Displacement U1 4a. Displacement U1 vs. reaction force RF1

12 0-500 Isight target Initial design Optimum design Reaction force RF Displacement U3 4b. Displacement U3 vs. reaction force RF3

13 7 x Isight target Initial design Optimum design Reaction moment RM Rotation UR2 4c. Rotation UR2 vs. reaction moment RM2 Figure 4 Stiffness responses of each loaded direction

14 Figure 5 Tosca shape optimization workflow

15 Figure 6 Design surface of shape optimization

16 7a. Contour plot of damage values before the non-parametric shape optimization

17 7b. Contour plot of damage values after the non-parametric shape optimization Figure 7 Contour plot of damage value

18 Damage Value Iteration Number 8a. Worst life in damage value

19 1.7 x Number of cycles Iteration Number 8b. Worst life in number of cycles Figure 8 Worst life vs. iteration number 1 st shape optimization

20 Figure 9 Validation fe-safe runs before and after the 1 st shape optimization

21 Reaction force RF Target Shape optimization 1 Modified target Shape optimization Displacement U1 10a. Displacement U1 vs. reaction force RF1

22 0-500 Target Shape optimization 1 Modified target Shape optimization 2 Reaction force RF Displacement U3 10b. Displacement U3 vs. reaction force RF3

23 Reaction moment RM2 7 x Target Shape optimization 1 Modified target Shape optimization Rotation UR2 10c. Rotation UR2 vs. reaction moment RM2 Figure 10 Stiffness responses of each loaded direction

24 Damage Value Iteration Number 11a. Worst life in damage value

25 1.4 x Number of cycles Iteration Number 11b. Worst life in number of cycles Figure 11 Worst life vs. iteration number 2 nd shape optimization

26 Figure 12 Validation fe-safe runs before and after the 2 nd shape optimization

27 Table 1 Design range of each parameter Lower limit Upper limit w 6 mm 12 mm r 22 mm 25 mm θ 30 60