Virtual Tests for Facilitating Steering Wheel Development SAE TECHNICAL PAPER SERIES

Transcription

1 SAE TECHNICAL PAPER SERIES Virtual Tests for Facilitating Steering Wheel Development Zane Z. Yang, Srini V. Raman and Deren Ma Delphi Corporation Reprinted From: Virtual Engineering and Development, Digital Modeling, and Rapid Prototyping (SP-97) 25 SAE World Congress Detroit, Michigan April -4, 25 4 Commonwealth Drive, Warrendale, PA 596- U.S.A. Tel: (724) Fax: (724) Web:

2 The Engineering Meetings Board has approved this paper for publication. It has successfully completed SAE s peer review process under the supervision of the session organizer. This process requires a minimum of three (3) reviews by industry experts. All rights reserved. No part of this publication may be reproduced, stored in a retrieval system, or transmitted, in any form or by any means, electronic, mechanical, photocopying, recording, or otherwise, without the prior written permission of SAE. For permission and licensing requests contact: SAE Permissions 4 Commonwealth Drive Warrendale, PA 596--USA permissions@sae.org Tel: Fax: For multiple print copies contact: SAE Customer Service Tel: (inside USA and Canada) Tel: (outside USA) Fax: CustomerService@sae.org ISSN Copyright 25 SAE International Positions and opinions advanced in this paper are those of the author(s) and not necessarily those of SAE. The author is solely responsible for the content of the paper. A process is available by which discussions will be printed with the paper if it is published in SAE Transactions. Persons wishing to submit papers to be considered for presentation or publication by SAE should send the manuscript or a 3 word abstract to Secretary, Engineering Meetings Board, SAE. Printed in USA

3 Virtual Tests for Facilitating Steering Wheel Development Copyright 25 SAE International Zane Z. Yang, Srini V. Raman and Deren Ma Delphi Corporation ABSTRACT A steering wheel is an indispensable component in an automobile. Although the steering wheel was invented about one hundred years ago and its structure has since become more and more complex with numerous innovations, documented analysis on steering wheel performance is very limited. Today, a steering wheel is not only a wheel that controls where your car goes; it also plays an important role in a vehicle occupant protection system. Therefore, many requirements have to be met before a steering wheel goes into production. With the development of computational mechanics and increasing computer capability, it has become much easier to evaluate the steering wheel performance in a totally different way. Instead of running prototype tests, steering wheel designs can be modeled virtually in various scenarios using finite element analysis, thus facilitating the development cycle. The objective of this paper is to give an overview of the modeling, simulation and challenges faced in the analysis of steering wheels. INTRODUCTION material can be urethane, leather, wood, or a combination thereof. Figure. A steering wheel at design stage A steering wheel is one of the most important components in a vehicle safety system. In addition to steering the vehicle, a steering wheel along with a steering column also supports the driver-side airbag that deploys during a severe frontal crash, thus reducing injuries to the driver. There have been a lot of publications on the analysis for safety systems and components such as airbags. Altenhof, et al [] has recently investigated the crash performance of steering wheel inserts during impact loading. However, little information about the study of steering wheel overall performance can be found in the literature including SAE publications. Molding Switches Insert Rim Spokes Hub Shroud A typical steering wheel assembly is comprised of a metal insert, a steel hub, and a layer of material (molding) to cover part of the insert (Figures and 2). Structurewise, a steering wheel can have 2, 3, or 4 spokes (Figure 3). Depending on design criteria, the cross-sections of the spokes and rim could be solid, tubular or u-channel. Commonly used insert materials include magnesium, aluminum and steel; and the cover Figure 2. Components of a typical steering wheel

4 The current engineering specification for steering wheels lists about 3 different physical tests to which each wheel must be validated. Additional tests may also be required by vehicle manufacturers. Of these tests, more than 5 are of the wheel structure while the rest are environment-related. These tests, if performed physically, cost a lot of money for a prototype wheel. Fortunately, many of the structural tests can be done virtually by steering wheel suppliers like Delphi using numerical methods such as the finite element analysis. Recommendations based on analysis results have helped Delphi in cost savings by shortening product lead-time and reducing the number of prototype tests. (a) The virtual tests for steering wheels can be categorized by nature into three types: modal analysis, static analysis, and impact analysis. This paper gives an overview of the simulation of the virtual tests for these analyses. Each of the analysis tests is briefly explained. Emphasis is placed on how to model the physical tests virtually under various conditions using finite element analysis. Analysis examples are given to illustrate how the virtual tests are set up. In addition, challenges and difficulties in the simulation process are addressed. In particular, model quality, contact problems, and material issues are discussed. MODAL ANALYSIS TEST Figure 3. Various steering wheel styles (a): 2-spoke; (b): 3-spoke; (c): 4-spoke (b) (c) The resonant frequency of a steering wheel is a very important design parameter. The current specification for most vehicle manufacturer s steering wheel calls for a minimum of 6 Hz for the resonant frequency. Much time is spent in the early phases of the design process to make sure that this specification is met. The resonant frequency issue is important because the steering wheel is a direct interface to the driver through the senses of touch and sight. No automobile manufacturer wants the driver to feel vibrations or see the wheel vibrating at idle while waiting in a traffic light. For these reasons, the resonant frequency should fall within a frequency range where the wheel will not be excited by vibrations coming up the steering column. Unfortunately, this is usually very difficult to achieve. Therefore, the frequency is chosen such that its value is away from the idle speed and also away from the cruising speeds such as 55, 65, or 7 mph. It should be in a speed range that is passed through quickly and not driven steadily. Note that vibrations could still be felt by the driver at other than the resonant frequency by direct transmission through the steering wheel. Therefore, mass dampers are sometimes added to steering wheels to damp out vibrations, which usually happen at idle speeds. The steering wheel can be simplified as a spring-mass system with the insert structure being the spring. The resonant frequency of such a system would be ω = k / m 2

5 where k is the spring constant and m the mass of the system including the molding, switches, leather-wrap, and airbag module. It is noted that there are only two variables that can affect the resonant frequency, namely, the stiffness and mass. As a consequence, in analyzing a steering wheel, care is to be taken to model the structure of the insert closely, thereby representing the correct stiffness. In the mean time the system mass as well as its distribution should also be accurately simulated. The resonant frequency of a steering wheel can be obtained from a modal analysis of a finite element model, which is usually carried out using the commercially available code, NASTRAN [2]. The frequencies of interest are the first two, which will be a rim-bending mode (fore/aft) and a wheel-bending mode (lateral) as per the normal requirements. Figure 4 shows the first and second bending modes of a steering wheel in the virtual test. RIM-ROLL FLEX TEST This test simulates a driver pushing repeatedly on the wheel with a concentrated load. The wheel is mounted on a rotating fixture with a dead weight roller resting on the rim. It must survive a number of rotations without fracturing or deflecting more than a specified amount, depending on the vehicle manufacturer s requirements. This test can be modeled with a linear finite element analysis by applying the load at the 2 o clock position of the rim. The analysis gives the maximum stress to the wheel because the upper loop of the rim has the largest moment arm. The design is modified if necessary until all stresses are below the tensile yield stress of the material. This virtual test is usually done using NASTRAN [2]. Figure 5 shows the virtual test setup. Load st mode 2nd mode BENDING TESTS Figure 5. Virtual rim-roll flex test setup Figure 4. First and second bending modes Generally, three different modal analysis models are required for a steering wheel. The first one is the insert frequency model with no molding mass added. The second model will have the molding mass and leather wrap and switches added. And the last model will be of the full wheel assembly with the airbag module added. The vehicle manufacturer is only interested in the last one while the other two models are analyzed to assist in model validation during the design process. A majority of the steering wheel assemblies have the first mode resonant frequencies of up to 75 Hz. In addition to the resonant frequency, the principal moment of inertia of a steering wheel with respect to its column also has to meet the specification. The moment of inertia can be calculated from the NASTRAN output data. STATIC ANALYSIS TESTS Many different types of static analyses under various loading conditions are to be provided by the vehicle manufacturers. Among them are the rim-roll flex test and the bending tests. The purpose of the bending tests is to determine the bending stiffness and deformed shape of a steering wheel when tested to a simulated driver frontal impact condition. The model is usually generated so that the rim at the 2 o clock or 6 o clock position will contact a rigid surface or a block. The block is comprised of a layer of rubber and a layer of steel as well. A displacement toward the steering wheel is applied to the block while the wheel hub is fixed. A load deflection curve has to be provided to the design engineer. This analysis involving both geometrical and material nonlinearities can be done in the commercially available finite element analysis code, ABAQUS [3]. Bending test at 2 o clock Figure 6 shows the lab test setup for the case of bending at the 2 o clock position, where the steering wheel is mounted so that the plane of the wheel rim is vertically positioned. Shown in Figure 7 is the corresponding virtual bending test setup, where a fixed boundary condition at the hub is presumed. The load-deflection curve for the wheel as well as the upper and lower limits set forth by the vehicle requirement from the vehicle manufacturer is plotted in Figure 8. The simulation curve based on analysis results has to fall between the lower 3

6 and upper limits. Figure 8 indicates that the wheel is well designed to the bending test requirement at 2 o clock. In the lab test, the block is free to move, while in the virtual test this is achieved by allowing no friction forces between the wheel and the block. It should be pointed out that the block length in Figure 7 really does not matter as long as the wheel is in contact with the block during the course of testing. Load (normalized).4 Upper limit Lower limit Simulation Deflection Figure 8. Load-deflection curve at 2 o clock position Figure 6. Lab bending test setup Load Rubber Deformed Steel Figure 9. Virtual bending test setup at 6 o clock position Load Upper limit Lower limit Simulation Undeformed Figure 7. Virtual bending test setup at 2 o clock position Load (normalized).4 Tip-load test at 6 o clock This bending test is performed while the wheel is tilted for 3 o to the original vertical plane of the wheel rim. Figure 9 shows the virtual test setup and Figure the load-deflection curve as well as the upper and lower limits in the specification. It is seen from Figure that the wheel is just a little too stiff at 6 o clock. As a consequence, design changes to weaken the lower loop of rim or spokes may be needed Deflection Figure. Load-deflection curve at 6 o clock position 4

7 IMPACT ANALYSIS TESTS Steering wheels are subject to impact testing because of their location in the vehicle. There are basically three impact requirements for wheels. Torso impact with the load distributed by an inflated airbag Torso impact at speeds below the airbag firing speed (or above the airbag firing speed as set forth in European and Japanese standards) [6] Head impact at speeds below the airbag firing speed V o V o These tests can be carried out on the steering wheel, which is rigidly mounted, mounted to a steering column, or mounted to an energy absorber. The finite element analysis package, LS-DYNA [4], is used to perform all these impact analysis tests. TORSO IMPACT In a torso impact test [5], the steering wheel is placed at its in-car position and impacted by a 75 lb (34 kg) torso at 5 mph (24 kph) at various rim locations (Figure ). The torso finite element model (Figure 2) was created based on the dimensions as specified in ECE-R2 [6]. An initial velocity, V o, is applied to the torso in the direction towards the wheel, which is fixed at its hub. This torso is sometimes replaced with a 5 lb (22.7 kg) steel block upon a vehicle manufacturer s request. Figure 2. Virtual torso impact test setup The analysis criteria are that no failure of material should occur in the metal insert and the resultant force exerted on the load cell mounted under the steering wheel hub should not exceed,2 N for 3 ms [6]. Figure 3 shows the animations of a virtual test example at 5 ms and ms after the initial impact, and Figure 4 the corresponding strain contour plots in critical areas of the steering wheel. As the time increases from 5 ms to ms, the deformation of the wheel increases significantly. In addition, the maximum strained area has shifted from the lower spoke to the hub area due to the change in contact between the torso and the wheel assembly. However, the maximum equivalent plastic strain is still below 9%, the material failure strain for this wheel, implying that there is no material failure during the impact test. t = 5 ms t = ms Figure 3. Deformed shape under torso impact Figure. Torso impact test setup 5

8 t = 5 ms t = ms Lower limit Upper limit Simulation Load (normalized) Deflection Figure 4. Strain contours in steering wheel Plotted in Figure 5 is the impact load versus time curve for a steering wheel at 3 different impact locations. It is clearly seen that the peak impact load for this wheel design occurs at 4 o clock position where the rim meets the spokes. It is clearly seen that the aforementioned maximum load requirement is well met by this wheel design. Some of the vehicle manufacturers may also be interested in the load-deflection curve, which should not go beyond the specified limits. Figure 6 shows the load-deflection curve for the wheel is already out of the specification range. Design improvement has to be made to meet this requirement. Load (normalized).4 4: 6: 2: Time Figure 5. Impact load on torso Figure 6. Load-deflection curve at 2: o clock HEADFORM IMPACT The head impact test was run with a 5 lb (6.8 kg), 6.5 (65 mm) steel hemispherical ball at 5 mph (24 kph) on a bungee cord propelled rotating arm. This has since been modified by using a lb (4.54 kg) FTSS free motion headform (FMH) [7] deployed from a linear accelerator. This test not only examines the integrity of the wheel but also assures minimizing harm to the occupant. The resulting deceleration on the headform should not exceed 8 g for 3 ms and the peak deceleration should be below 2 g [6]. Alternatively, a specification for the headform maxilla load should be met. A standard finite element model provided in LS-DYNA format of the FMH is available for use, which essentially provides the same accelerometer output as the real physical test device does. Figures 7 and 8 show the virtual headform test setup and resulting impact animations at 5 ms and ms for a steering wheel assembly with a magnesium insert, where the headform is launched at an initial speed of V o. Shown in Figure 9 are the strain contours of the magnesium insert. It is observed that the equivalent plastic train has increased by 6 times from the impact moment of 5 ms to that of ms though the magnitude is still quite low when compared to the failure strain of magnesium. The headform decelerations when impacted at the 4 o clock and 6 o clock positions are plotted in Figure 2, while the maxilla load is shown in Figure 2. It is seen from Figures 2 and 2 that the aforementioned requirements for both headform deceleration and maxilla load are met for this steering wheel design. 6

9 4: 6: V o Deceleration (normalized).4 V o Figure 7. Virtual headform impact test setup Time t = 5 ms t = ms Figure 2. Deceleration of headform Load (normalized).4 Figure 8. Deformed shape under headform impact t = 5 ms t = ms Time Figure 2. Maxilla load of headform DISCUSSION In order for a virtual test setup to be predictive, the finite element model for a steering wheel has to be validated by physical test data. Table shows the correlation level for each type of virtual tests. Table. Correlation level of virtual tests Virtual Test Type Modal Analysis Static Analysis Impact Analysis Figure 9. Strain contours of magnesium insert Correlation Level Very High High Moderate 7

10 Once the finite element model has been correlated, it can be used to predict the performance of the steering wheel design in various scenarios, thereby greatly facilitating the wheel development. However, there still are some issues that need to be addressed when using the virtual tests. MESH DENSITY OF WHEEL For a steering wheel assembly model, the global element size should be determined so that it is not too small to result in a huge model. But it is still small enough to capture the design features such that the steering wheel design is well simulated to represent its structural stiffness and mass distribution. In regions where there is a drastic change in the curvature of geometry, the mesh density may be increased. However, in the areas where impacts and contacts are expected, a fairly uniform mesh should be generated. CONTACT PROBLEMS Analysis involving contacts is still a very challenging topic for implicit solvers. In general, ABAQUS has been found to do a reasonable job dealing with the contact problems in static analysis. However, in difficult cases such as the aforementioned bending tests, the solution procedure may not converge. It has been found, generally, that the bending test at the 6 o clock position is more difficult to solve than that at the 2 o clock position. This is caused by the relative position of the elements in contact on the wheel and the block, thereby the relative position of the steering wheel and the block. The block is usually meshed coarsely so that it can be designated as the master surface in the contact definition. In impact analysis, care should be taken when choosing the contact types. MATERIAL PROPERTIES As mentioned earlier, the steering wheel insert is usually made of magnesium alloy or aluminum alloy because these materials are most cost-effective. In order to accurately simulate the response of a steering wheel, the material description should be close to reality. Unfortunately, a complete set of material data is still not available for these most commonly used materials. Also, stress-strain curves considering rate dependency cannot be found for use in LS-DYNA. On the other hand, the strain rate might be high enough to affect the behavior of a steering wheel subjected to an impact at up to 5 mph (24 kph). Therefore, in order for the results of virtual impact tests to be useful, more efforts are needed to obtain dynamic material properties. MODELING OF MOLDING The molding material is much softer than the insert metal. For example, urethane, a typical commercially available foam material, has a Young s modulus of 6 GPa, compared to that of a typical magnesium alloy, 42 GPa. As a consequence, the stiffness contributed by the molding to the stiffness of the whole structure is negligible in most cases. Its mass, however, should be considered in an impact test and represented by concentrated masses attached to appropriate nodes. In case the molding stiffness needs to be included, it can be modeled with solid elements, beam elements, or beam elements and null shells, which are used to describe the contact surface of the molding. CONCLUSION In this paper, the procedures of three major virtual structural tests for developing steering wheels were outlined. These tests involved modal, static and impact analyses. Examples were given to show how the virtual tests were set up. Emphasis was placed on the specific modeling techniques suited for each test. Difficulties and challenges in the modeling process were also addressed. Based on our experience at Delphi it can be concluded that The correlation level of a virtual test for steering wheels to its corresponding physical test using the currently available modeling technologies is acceptable for the automotive industry; and The virtual tests can significantly facilitate the development of steering wheels REFERENCES. W. Altenhof, B. Arnold, Z. Li, O. Nabeta and R. Turchi, A Comparison of the Crash Performance of Three-spoke and Four-spoke Steering Wheel Armatures during Impact Loading, Int. J. Vehicle Design, Vol. 35 (24), No. 3, pp MSC.Nastran 2 Quick Reference Guide, MSC. Software Corporation, ABAQUS Analysis User s Manual, Version 6.4, ABAQUS, Inc., LS-DYNA Keyword User s Manual, Version 97, Livermore Software Technology Corporation, FMVSS Impact Protection for the Driver from Steering Control System, ECE-R2 -- Impact Against Steering Mechanism, FTSS Free Motion Headform Model, Version 3.2, First Technology Safety Systems, Wayne A. Wilson and Zane Z. Yang, Steering Wheel Modeling Guidelines, Internal Document, Delphi Safety and Interior Systems, Wayne A. Wilson, Structural Analysis of Steering Wheels, Analytical Design Forum, Delphi Safety and Interior Systems,

11 CONTACT Zane Z. Yang is a Senior Safety Systems Analysis Engineer with the Division of Electronics & Safety, Delphi Corporation. He has a Ph.D. in Structures and Materials from Purdue University, W. Lafayette, IN. His expertise is in vehicle crashworthiness, engineering mechanics, and composites. zane.z.yang@delphi.com. Srini V. Raman is an Engineering Group Manager of the Safety Systems Analysis Group with the Delphi E&S Division. He holds a Masters degree in Mechanical Engineering from the University of Nevada, Reno, NV. srini.v.raman@delphi.com. Deren Ma is a Staff Product Engineer with the Delphi E&S Division. He received his Doctorate in Mechanical Engineering from the Wichita State University, Wichita, KS. His work includes systems engineering, CAE/math based engineering, vehicle occupant restraint systems and crashworthiness, multibody dynamics and finite element analysis. deren.ma@delphi.com. 9