Parameter study of bodywork attachments influencing the chassis dynamics by vibration response analysis

Parameter study of bodywork attachments influencing the chassis dynamics by vibration

response analysis

A ^NIRUDH G ^URURAJ D ^ESHPANDE

Master of Science Thesis TRITA-ITM-EX 2018:369 KTH Industrial Engineering and Management

Machine Design SE-100 44 STOCKHOLM

J UNE 2018

Abstract

Master of Science Thesis TRITA-ITM-EX 2018:369

Parameter study of bodywork attachments influencing the chassis dynamics by vibration response analysis

Anirudh Gururaj Deshpande

Examiner Supervisor

Approved

2018- 06-11 Ulf Sellgren Ulf Sellgren

Commisioner Contact Person

SCANIA CV AB Martin Hede

The automotive sector is continuously evolving and the companies are well aware of the rising demands from customers with regard to driving comfort and experience. Trucks carrying heavy loads are often equipped with on-built bodywork, for example a box for pallets and goods, a garbage collector device or a supporting frame for carrying timber. SCANIA bodybuilding centre develops guidelines for selecting different types of bodywork, i.e. the type of supporting frame, design and number of attachment brackets, attachment points. The purpose of this master thesis is to develop a better understanding of how the supporting frame and its attachments in a truck influence the chassis frame dynamics and to propose improvements to these guidelines.

Major parameters influencing the chassis dynamics were identified and described from the outset. Physical vibration testing of the chassis-subframe assembly was carried out at road simulator. The frequency response functions from the measurements were used to determine the modal parameters. Several tests were performed by altering the parameters and recording the measurements. The results from the test cases were used to study and analyse the eigen frequencies, mode shapes and damping in the system. Also, a new method to build a dynamic finite element (FE) model of chassis and subframe is presented in this study. Modal analysis of the chassis-subframe assembly was done to study the eigen frequencies and mode shapes by FEM. The proposed method of coupling the chassis and the subframe is critically assessed by correlating the results from FE simulation with the experimental results. Based on the results from experiment and numerical simulation, new recommendations are proposed with regard to the bodywork attachments’ configuration in the truck.

Keywords: Eigen frequency, modal analysis, frequency response function, damping

Sammanfattning

Examensarbete TRITA-ITM-EX 2018:369

Parameterstudie av påbyggnadsanslutningar som påverkar chassidynamiken genom vibrationsresponsanalys

Anirudh Gururaj Deshpande

Examinator Handledare

Godkänt

2018- 06-11 Ulf Sellgren Ulf Sellgren

Uppdragsgivare Kontaktperson

SCANIA CV AB Martin Hede

Bilindustrin är i ständig utveckling och är väl medvetna om de ökande kraven från kunder med avseende på körkomfort och körupplevelse. Lastbilar med tunga laster är ofta utrustade med en påbyggnad, till exempel en låda för pallar och gods, en sopsamlare eller en stödram för bärning av timmer. SCANIA Bodybuilding Center utvecklar riktlinjer för val av olika typer av karosseri, dvs typ av stödram och antal , fästpunkter. Målet med detta arbete är att utveckla en bättre förståelse för hur det stödjande ramverket och dess infästningar i en lastbil påverkar rammens dynamik och sedan föreslå förbättringar till dessa riktlinjer.

Viktiga parametrar som påverkar chassisdynamiken identifierades och beskrivs från början.

Fysisk vibrationstestning av chassiet och påbyggnadsram med fasthållningsfäste utfördes vid i testrigg på Scania R&D. Frekvensresponsfunktionerna från mätningarna användes för att bestämma modala parametrar. Olika test utfördes genom att ändra parametrarna och upptagnin- gen av mätningarna. Testresultaten användes för att studera egenfrekvenser egna frekvenser, modifieringsformer och dämpning i systemet. Även en ny metod för att bygga en dynamisk finit element (FE) modell eller chassi och påbyggnadsram är presenterad i denna undersökning.

Modalanalys av chassi-påbygnadsramssystemet gjordes för att studera FEMs egna frekvenser och modeformer. Den föreslagna metoden för koppling av chassit och delramen i FEM är kritiskt bedömd genom att korrelera FE-simuleringen med de experimentella resultaten. Baserat på de utförda experimenten och den numeriska simuleringen föreslås från experiment och numerisk simulering, föreslås nya rekommendationer med avseende på påbyggnadsanslutningarnas kon- figuration i lastbil.

Nyckelord: Eigenfrekvens, modalanalys, frekvensresponsfunktion, dämpning

Foreword

This thesis work was carried out at SCANIA CV AB, Södertälje over a period of five months.

I’m very grateful to SCANIA for providing me an opportunity to work in their organization. It has been a wonderful learning experience and I had the unique opportunity to work at vägsimulator at RTCD, SCANIA. I would like to express my deepest appreciation to all those who provided me the possibility to complete this project.

I would first like to thank my thesis supervisor Martin Hede whose knowledge, expertise and insights throughout the project have been invaluable and has helped me stay on the right track. I would also like thank my manager, Mattias Borg for providing me with all the necessary facilities and tools to carry out the work. Since this project involved multiple departments-design, FEM simulation and physical testing, a steering group was formed to bring in the necessary knowledge and expertise from each of these departments. I would like to thank the all the members of the steering group who were involved in this project from the very beginning and provided me with valuable guidance and insights.

I wish to express my sincere thanks to Prof. Ulf Sellgren (my supervisor at KTH), who has always been available whenever I ran into trouble spot or had a question about my work and has provided me with a new perspective about approaching the problem.

Finally, I would like to express my very profound gratitude to my parents and friends for the continuous support and encouragement throughout my years of study and through the process of writing this thesis.

Anirudh Gururaj Deshpande

Stockholm, Sweden

vi

Nomenclature

ABBREVIATIONS

EM A Experimental Modal Analysis F EM Finite Element Method F F T Fast Fourier Transform F RF Frequency Response Function P SD Power Spectral Density R MS Root Mean Square NOTATIONS

ω Frequency

ω r Resonant frequency ζ Damping ratio

R _x Rotational degree of freedom in x-direction

R _y Rotational degree of freedom in y-direction

R _z Rotational degree of freedom in z-direction

U _x Transnational degree of freedom in x-direction

U _y Transnational degree of freedom in y-direction

U _z Transnational degree of freedom in z-direction

Table of Contents

Nomenclature vii

Page

List of Tables xi

List of Figures xiii

1 Introduction 1

1.1 Background . . . . 1

1.2 Purpose . . . . 1

1.3 Delimitations . . . . 2

1.4 Method . . . . 2

2 Frame of Reference 7 2.1 Chassis Frame Design . . . . 7

2.2 Subframe and Bodywork Attachments . . . . 8

2.2.1 Subframe . . . . 8

2.2.2 Bodywork Attachments: Design and Selection . . . . 9

2.3 Vibrations . . . . 10

2.3.1 Modal Analysis . . . . 10

2.3.2 Experimental Modal Analysis . . . . 11

2.3.3 Frequency response function (Transfer function) . . . . 12

2.3.4 Coherence . . . . 13

2.3.5 Random vibration . . . . 14

2.3.6 Power Spectral Density (PSD) . . . . 14

2.3.7 Damping . . . . 14

2.3.8 Measurement of Damping Ratio . . . . 15

2.4 Friction–vibration interactions . . . . 16

2.4.1 Friction in bolted joints . . . . 16

2.4.2 Friction Modeling and Simulation . . . . 17

3 Implementation 19 3.1 Description of Major Parameters . . . . 19

3.1.1 Number of Bodywork Attachments . . . . 19

3.1.2 Position of Bodywork Attachments . . . . 19

3.1.3 Design of Bodywork Attachments . . . . 19

3.1.4 Pretension/Bolt torque in Bodywork Attachments . . . . 20

viii

TABLE OF CONTENTS

3.2 Physical Vibration Testing . . . . 21

3.2.1 Experimental Setup . . . . 21

3.2.2 Test Objective and Plan . . . . 23

3.2.3 Measurement Equipment . . . . 24

3.2.4 Excitation signals . . . . 26

3.2.5 Data Acquisition and Processing . . . . 26

3.3 Finite Element Model Description . . . . 27

3.3.1 Scope and Method Development . . . . 27

3.3.2 Chassis and Subframe Model . . . . 28

3.3.3 Interface and Joints . . . . 30

3.3.4 Modelling the Bodywork Attachments . . . . 31

3.3.5 Material . . . . 32

3.3.6 Mesh . . . . 32

3.3.7 Boundary Conditions and Constraints . . . . 33

4 Results and Discussions 35 4.1 Physical Vibration Testing . . . . 35

4.1.1 Influence of Excitation Signal . . . . 35

4.1.2 Test Cases: Study and Comparison . . . . 39

4.2 FEM: Vibration Response Analysis . . . . 43

4.2.1 Modal Analysis of Chassis . . . . 43

4.2.2 Modal Analysis of Chassis-Subframe assembly . . . . 46

4.2.3 Correlating FE results with Experiments . . . . 48

4.2.4 Discussion on the FE method . . . . 49

5 Conclusions 51

6 Future Work 53

Bibliography 55

Appendix

A Supports and fixtures 57

B Modal analysis of beams 59

List of Tables

T ABLE Page

3.1 Test cases summary . . . . 24

3.2 Excitation Signal . . . . 26

3.3 Components of chassis and subframe . . . . 28

3.4 Material property of steel . . . . 32

3.5 Mesh details . . . . 33

4.1 Experiment result summary . . . . 39

4.2 Comparison of FE and Experimental results . . . . 49

A.1 Parts for vibration testing . . . . 57

List of Figures

F IGURE Page

1.1 Flowchart describing the methodology . . . . 3

2.1 Typical chassis frame in a truck . . . . 7

2.2 Typical subframe in a truck . . . . 8

2.3 Types of bodywork brackets [1] . . . . 9

2.4 Flat plate . . . . 10

2.5 Response of plate as a function of time . . . . 11

2.6 Summary of experimental modal analysis procedure . . . . 11

2.7 Bode Plot of Amplitude and Phase of a FRF function [16] . . . . 12

2.8 Plot: Green (Coherence) and Red (FRF) [16] . . . . 13

2.9 Typical power spectral density vibration testing specification . . . . 14

2.10 Bandwidth method of damping measurement . . . . 15

2.11 Normalized friction force vs slip velocity. (a) Coulomb,(b) Sticktion, and (c) Stribeck friction laws. . . . 17

3.1 (a) Rubber bushing bracket (b) Flexible bracket (c) Rigid bracket . . . . 20

3.2 Experiment Setup . . . . 21

3.3 Front Support . . . . 22

3.4 Rear Support . . . . 23

3.5 Test setup arrangement . . . . 25

3.6 Measurement Senors: (a) Accelerometers (b) Displacement sensor (c) Load cell . . . . 25

3.7 MATLAB tool for processing results . . . . 26

3.8 FE model method: (a) 1-D element connection (b) Contact (c) New material layer . . . 28

3.9 FE model: (a) Half model of chassis (b) Section showing the mesh . . . . 29

3.10 FE model: (a) Section showing mesh (b) Half model of subframe . . . . 29

3.11 Subframe: (a) Side and cross member interface (b) Front stop and side member interface (c)Bunk body and sidemember interface . . . . 30

3.12 Chassis: Interfaces and joints . . . . 30

3.13 Connector model for brackets . . . . 31

3.14 Example: Connector definition . . . . 32

3.15 (a) Front Support (b) Rear Support . . . . 33

4.1 Acceleration PSD : Test case 1 (Base Configuration) . . . . 36

4.2 Transfer function, Cyl acc. vs Frame acc. :Test case 1 (Base Configuration) . . . . 37

4.3 Acceleration PSD : Test case 11: All 11 brackets flex (20 Nm) . . . . 38

L IST OF F IGURES

4.4 Transfer function, Cyl acc. vs Frame acc.: Test case 11 (All 11 brackets flex (20 Nm)) . 38

4.5 Acceleration PSD: Test cases 1,2 and 3 . . . . 40

4.6 Acceleration PSD: Test cases 1, 10, 11 and 12 . . . . 41

4.7 Acceleration PSD: Test cases 14,15 and 16 . . . . 42

4.8 (a) Acceleration PSD: Test cases 6 and 7 (b) Flex bracket side view . . . . 43

4.9 Modal analysis of chassis (half model) . . . . 44

4.10 Modal analysis of chassis (full model) . . . . 45

4.11 Modal analysis of chassis (full model) . . . . 45

4.12 Modal analysis : Base configuration ; Modes 1,2 and 3 . . . . 46

4.13 Modal analysis : Test case 9;Modes 1,2 and 3 . . . . 47

4.14 Modal analysis : All 11 flex brackets (20Nm); Modes 1,2 and 3 . . . . 48

B.1 Mesh model with TIE connection . . . . 59

B.2 Modal analysis of beams (TIE connection) . . . . 60

B.3 Mesh model with CONN3D2 connection . . . . 60

B.4 Modal analysis of beams (CONN3D2 connection) . . . . 61

xiv

Chapter 1

Introduction

The automotive sector is continuously evolving and the companies are well aware of the rising demands from customers when it comes to driving comfort and experience. SCANIA CV AB being a major Swedish automotive industry manufacturer of commercial vehicles – specifically heavy trucks and buses, has made this a priority. The company has been a pioneer in developing premium vehicles where performance, robustness and ergonomics have a perfect blend.

1.1 Background

The design architecture of a Scania truck is unique which allows the company to manufacture large number of truck variants for different applications and load ratings. This is possible by adopting a modular architecture where one can produce different variants of trucks by an ideal combination of modular sub-systems which provides great deal of flexibility and also cost re- duction. However, it also brings new set of challenges as the sub-system being developed are required to meet a vast set of complex design requirements and functionality. One such challenge is optimizing the driving comfort irrespective of the truck variant.

Trucks carrying heavy loads are often equipped with on-built bodywork, for example a box for pallets and goods, a garbage collector device or a supporting frame for carrying timber.

SCANIA bodybuilding centre develops guidelines for selecting different types of bodywork, i.e. the type of supporting frame, design and number of attachment brackets, attachment points etc. For a rigid truck with a body work, the design of the supporting frame, the attachment brackets and the load itself, have a significant influence on the truck chassis dynamics. These guidelines are built on experience and analytic tools, as for example the chassis frame strength level, torsional rigidity class etc. These are categorizations which SCANIA has developed for its vehicles based on operating conditions and dynamic loads acting on the vehicle. However, it is possible that the general guidelines do not always fit a specific vehicle or application and complaints occur regarding undesired vibrations to the cabin which affects the driving comfort.

1.2 Purpose

The objective of this master thesis is to develop a better understanding of how the supporting frame and its attachments in a truck influence the chassis frame dynamics. Physical vibration testing would provide information on system’s eigen frequencies and damping characteristics.

The aim is to study and analyze the results from testing and understand how the change in the

CHAPTER 1. INTRODUCTION

system parameters affect the dynamic response of the chassis.

It is also the objective to utilize the extracted modal parameters to build a dynamic FE model of the chassis-subframe assembly which then can be used to study the vibration response of the system. This is to improve the existing design guidelines to reduce the risk of disturbing vibrations to the cabin by modifying the bodywork attachments.

Research Questions

• How does the supporting frame and its attachments in a truck influence the chassis frame dynamics?

• Is it possible to develop an FE model of the chassis-subframe assembly which can be used to study the dynamic response for any bodywork attachment configuration?

1.3 Delimitations

• Road induced vibrations/ disturbances are considered in the scope of this thesis. Other vibration sources such as tires/wheels, power train and wind are not part of this study.

• This thesis work focuses on the vibration characteristics of a specific sub-frame type and chassis

• Suspensions, wheels and chassis components are not part of this study to order to reduce complexity in FE modelling and analysis.

• The work is carried out on one type of wheel configuration i.e. 4x2 wheel configuration.

• The input signal for testing and FE simulations are not from real road measurement signals but instead a pre-defined random signal is used for excitation.

1.4 Method

The following section describes the methodology adopted in carrying out this thesis work. The flowchart shown in the figure 1.1 highlights the key steps which are elaborated further.

1. Perform a literature study to build understanding of mechanical vibrations, friction and damping in heavy vehicles. Measured data on a truck for timber transport exists and is used for better problem understanding.

Sources:

• Thesis reports

2

1.4. METHOD

Figure 1.1: Flowchart describing the methodology

• Research papers

• Text books

• Scania technical documents 2. Objective and definition

The objective of this master thesis is to develop a better understanding of how the support- ing frame and its attachments in a truck influences the chassis frame dynamics. Physical vibration testing would provide information on system’s eigen frequencies and damping characteristics. The aim is to analyse the results from testing and understand how the change in the system parameters affect the dynamic response of the chassis.

It is also the objective to utilize the extracted modal parameters to build a dynamic FE model of the chassis-subframe assembly which then can be used to study the vibration response of the system. This is to improve the existing design guidelines to reduce the risk of disturbing vibration to the cabin

3. Describe major parameters and how they influence the chassis dynamics Ex:

• Bracket type (design)

• Number of brackets

• Position of brackets

• Bolt pre-torque in brackets

CHAPTER 1. INTRODUCTION

4. Physical Vibration Testing:

• Testing to be carried out in road simulator

• Design of fixtures and parts for testing

• Preparation of test setup and manufacturing of the required parts

• Defining a test plan and output parameters for measurements

• Processing the outputs for future study and comparison 5. Create an FE model with simple beams to identify the best method

• Create beams with simple rectangular cross section which could be assumed as chassis and subframe

• Identify the scope of the FE Model.

• List possible ways of connecting the two beams which satisfies the requirement in this study

• Perform a modal analysis to study the eigen frequencies and mode shapes

• Select the best method which could be applied for building the global FE model 6. Create an FE model of chassis and subframe

• The CAD model of the chassis and subframe is to be imported from CATIA into the pre-processor

• Setup the assembly model with bodywork attachments

• FEM modelling in Hypermesh tool

• Appropriate loads and boundary conditions are to be applied to replicate test conditions

• Study the dynamic response of the assembly in free and forced vibration conditions

• Abaqus tool is to be used for performing the analysis 7. Vibration response analysis

• Modal characteristics of the assembly is to be studied and analyzed i.e. mode shapes, eigen frequencies and damping

• Response of the system to be studied under forced vibration e.g. random signal 8. Tune the Damping and Stiffness of bodywork attachments

• The stiffness value of brackets need to be estimated and tuned to match the experi- mental results.

4

1.4. METHOD

• An equivalent damping value has to be provided to represent the damping provided by a given bracket

9. Compare the model to performed tests

The results are compared based on the eigen frequencies, mode shapes and damping ratio.

10. The results would be analyzed and discussed on the following:

• Mode shapes and eigen frequencies of the chassis frame-subframe assembly

• Identifying trends with regard to the structural damping in the system

• Most suitable bodywork attachment design and configuration in terms of damping 11. Conclusions

• Report findings and propose new recommendations for bodywork attachments based on the study

• Comment on the validity and applicability of the FE model

12. Make proposals to future work Future work based on experiments and also on the FE

model

Chapter 2

Frame of Reference

This chapter elucidates the necessary concepts and background knowledge that is used in carrying out this thesis work. The chapter starts with introduction on chassis design, sub-frame and bodywork attachments followed by detailed description on mechanical vibrations which forms the core of the thesis. It also touches upon the friction-vibration interaction at the end of the chapter.

2.1 Chassis Frame Design

Figure 2.1: Typical chassis frame in a truck

Chassis frame is the structure which forms the backbone of any vehicle. It provides the necessary

strength to support the vehicle’s components and payload placed on it. The frame is designed to

withstand the loads from the road, suspension, drive train and steering system.The most common

type of frames used in trucks today is the C-channel frame. The steel C-channel frame exhibits

high strength and allows for easy modifications and adaptations for bodywork to be fitted on it

[2] . A typical chassis frame comprises of two side members or rails which are straight C-sections

CHAPTER 2. FRAME OF REFERENCE

or have a slight angle towards the front end. These side members are connected to each other by several cross members which provide the required strength and stiffness. In addition, the cross members also prevent the frame from twisting which in other words provides the necessary torsional rigidity to the chassis structure. Figure 2.1 shows a typical chassis frame of a truck.

2.2 Subframe and Bodywork Attachments

2.2.1 Subframe

Figure 2.2: Typical subframe in a truck

The subframe is an additional frame mounted on top of the truck chassis frame [2]. The subframe length can vary as it starts from the rear end of the cab and can extend to a short length or cover the entire chassis frame. Figure 2.2 shows an example of a typical subframe in a truck.

It is highlighted in blue. The primary purpose of the subframe is to protect the chassis frame by evenly distributing the load from bodywork. It also provides rigidity and reduces the stress in

8

2.2. SUBFRAME AND BODYWORK ATTACHMENTS

the rear overhang when needed for example in tipper trucks. In addition, it provides necessary clearance for wheels and other parts which protrude above the frame. The design architecture of the subframe is similar to the chassis frame which consists of two side members interfaced by few cross members. The subframe and chassis frame move relative to one another when driving on uneven roads.The friction between the chassis frame and subframe helps in damping the the movement [3].

2.2.2 Bodywork Attachments: Design and Selection

Body adaptation brackets are used as a system for attachment to connect the chassis frame with the subframe. Depending on the combination, the desired characteristics can be achieved, from rigid to flexible attachment [4]. Depending on the application and need, combination of rigid or flexible attachments are used accordingly. There are several types of bodywork attachments as shown in the figure 2.3. SCANIA Bodybuilding centre has general recommendations for selecting the design of subframe and bodywork brackets. As stated in chapter 1, the recommendations have been based primarily on frame strength level, torsional rigidity class and also previous experience. These are categories which SCANIA has developed for its vehicles based on operating conditions and dynamic loads acting on the vehicle.

Figure 2.3: Types of bodywork brackets [1]

1. Flexible attachment upwards and downwards.

2. Flexible attachment upwards and longitudinally, with angle brackets and compression springs.

3. Longitudinally flexible attachment with angle brackets.

4. Rigid attachment with angle brackets.

CHAPTER 2. FRAME OF REFERENCE

5. Rigid attachment with flat bracket.

6. Rigid attachment with flat bracket welded to the subframe.

2.3 Vibrations

Vibrations are oscillatory responses of dynamic systems. Mechanical vibrations occur as both free and forced responses in practical situations. Some of the vibrations are useful, and others are undesirable and should be suppressed. Developing an FE model serves as a useful tool in the design and development of mechanical systems [5]. This section provides some fundamental knowledge on study and analysis of vibrations including damping.

2.3.1 Modal Analysis

Modal analysis is simply the process of describing a structure in terms of its natural characteris- tics which are frequency, damping and mode shapes.

Figure 2.4: Flat plate

Consider a freely supported flat plate as shown in figure 2.4. If a force is applied on the plate with fixed amplitude and the rate of oscillations is slowly increased, then it is observed that the response amplifies as the rate of oscillation of applied force matches with the natural frequency (resonant frequency) of the system.This is depicted in figure 2.5. Also, the deformation patterns of the flat plate at these natural frequencies have different shapes depending on which frequency is used for excitation. These deformation patterns are referred to as mode shapes of the structure [6]. It is important to identify the natural frequencies and how it affects the response of the structure. A better understanding of the modes shapes is helpful during design of a mechanical system [7].

10

2.3. VIBRATIONS

Figure 2.5: Response of plate as a function of time

2.3.2 Experimental Modal Analysis

The specific purpose of an experimental modal analysis (EMA) is to determine the parameters of a physical model describing the vibrations of a structure [8]. EMA make use of measured frequency response functions between motion response and exciting forces. These functions do not depend on the excitation and are unique for each structure. Figure 2.6 shows a graphic summary of the experimental modal analysis procedure. In practice, a structure is discretised by a set of observation points. Then the frequency response functions are measured with respect to these discretisation points. An exciting force is applied to a discretisation point and the motion caused by this force, is measured. The frequency response functions between the measured force and motion signal is calculated. This process is repeated for all the points which yields a frequency response matrix with respect to observation points. Finally the measured functions are used to determine modal model parameters. There are many advantages of a modal model. For example, in automotive industry the modal model of a vehicle could be used to evaluate passenger comfort.

Figure 2.6: Summary of experimental modal analysis procedure

CHAPTER 2. FRAME OF REFERENCE

2.3.3 Frequency response function (Transfer function)

The frequency response is the ratio of output response of a structure to an applied force.The response is measured as displacement, velocity or acceleration. This time data is transformed from time domain to frequency domain using Fast Fourier Transform (FFT) using a signal analyzer and computer package [7]. In a Frequency Response Function (see figure 2.7) measurement the following can be observed:

• Resonances - Peaks indicate the presence of the natural frequencies of the structure under test

• Damping - Damping is proportional to the width of the peaks. The wider the peak, the heavier the damping

• Mode Shape – The amplitude and phase of multiple FRFs acquired to a common reference on a structure are used to determine the mode shape

Figure 2.7: Bode Plot of Amplitude and Phase of a FRF function [16]

12

2.3. VIBRATIONS

2.3.4 Coherence

Coherence is a function which indicates how much of the output is due to the input in the FRF. It is the indicator of the quality of the FRF [7]. It helps in evaluating the consistency of the FRF by indicating the repeatability of measurement.

The value of a coherence function (see figure 2.8) ranges between 0 and 1:

A value of 1 at a particular frequency indicates that the FRF amplitude and phase are very repeatable from measurement to measurement. A value close to 0 indicates that opposite – the measurements are not repeatable, which could possibly be due to one of the following reasons [9]:

• the presence of noise in measurements

• the non-linear relationship between output and input signal

• the response is due to other inputs than the applied input

Figure 2.8: Plot: Green (Coherence) and Red (FRF) [16]

CHAPTER 2. FRAME OF REFERENCE

2.3.5 Random vibration

Vibrations found in everyday life scenarios (a vehicle on a roadway, the firing of a rocket or an airplane wing in turbulent air flow) are not repetitive or predictable like sinusoidal wave forms [10]. When a typical ground vehicle is driven over the road, the vibration spectrum from the road loading is determined by the surface roughness and the speed of the vehicle. In this instance, the spectral pattern is typical of a random noise distribution [11]. In random vibration testing, all the frequencies of the structure are excited in the defined spectrum at any given instance of time.

Random vibration testing helps in identifying structure’s natural frequencies and also relative damping in the system.

2.3.6 Power Spectral Density (PSD)

Generally the random vibration spectrum profile is displayed as a power spectral density (PSD) plot. This plot shows the mean square acceleration per unit bandwidth. The shape of a PSD plot defines the average acceleration of the random signal at any frequency [10].

Figure 2.9: Typical power spectral density vibration testing specification

2.3.7 Damping

Damping is the phenomenon by which mechanical energy is dissipated (usually converted to internal thermal energy) in dynamic systems [5]. It is important to know the damping of a mechanical system to develop a dynamic model. The knowledge about damping in the system is also useful to make design modifications in the structure which does not meet certain accepted standard. There are three primary mechanisms of damping which are of interest in mechanical systems:

14

2.3. VIBRATIONS

• Internal damping (of material)

• Structural damping (at joints and interfaces)

• Fluid damping (through fluid structure interactions)

Structural damping is caused by rubbing action or relative motion between components at the joints and interfaces in a mechanical system. Usually internal damping is negligible compared to structural damping [5].

2.3.8 Measurement of Damping Ratio

Figure 2.10: Bandwidth method of damping measurement

There are three common means of estimating damping:

• The first is a time domain approach and is used to estimate the damping associated components’ fundamental frequency. This is called as the log decrement approach [12].

• The second approach is to extract the damping values based on phase angle response

around the resonance. This is a frequency domain approach.The slope of the phase angle

response at resonance is controlled by the damping in the system. This phase angle data

can also be used to estimate damping values [12].

CHAPTER 2. FRAME OF REFERENCE

• The third means of estimating damping is referred to as the half power band width method.

The bandwidth method of damping measurement is also based on frequency response. The method uses the bandwidth at resonance, obtained from the response modulus, to estimate damping [12].

In the present thesis work, the damping ratio which in other words corresponds to structural damping is estimated using this approach. The peak magnitude is given by equation for low damping. Bandwidth (half-power) is defined as the width of the frequency-response magnitude curve when the magnitude is p ¹

2 times the peak value [5]. This is denoted by ∆ ω . An expression for

∆ ω = ω 2 − ω 1 (2.1)

is obtained using equation:

|H( ω )| = ^ω

2 n

[( _ω ² _n − ω ² ) ² + 4 ζ ² ω ² n ω ² ]

(2.2)

The resulting solution for _ω is termed as the resonant frequency _{ω r} .

For low damping _ζ < 0.1, damping ratio can be estimated from the bandwidth using the relation :

ζ = 1 2

∆ ω ω r

(2.3)

2.4 Friction–vibration interactions

Friction and vibration interact with each other in a dynamical system with sliding interface.It is important to combine the aspects of mechanical vibrations and tribology to analyze vast amount of practical cases. Different friction models have been developed for individual conditions. This is mainly because friction is a complex process in which forces are transmitted, mechanical energy is converted, surface topography is altered, interface material can be removed or formed, and physical and chemical changes can occur [13].

2.4.1 Friction in bolted joints

The double beam is an academic example which demonstrates the main features of a friction damped system. The study basically deals with two superposed beams pressed together by one or more bolted joints. One end of the double beam is fixed. The friction between the beams is the dominant dynamical phenomenon. It influences the stiffness and the damping of the structure.

Experiments and simulations are performed for a simple laboratory structure consisting of two superposed beams with friction in the interface. With the concept of optimal placed bolted friction beams there will be an improvement of the damping characteristics, and through stiffness tuning, resonance problems will be avoided [14].

16

2.4. FRICTION–VIBRATION INTERACTIONS

2.4.2 Friction Modeling and Simulation

Figure 2.11: Normalized friction force vs slip velocity. (a) Coulomb,(b) Sticktion, and (c) Stribeck friction laws.

Many friction models contain a variety of nonlinear features such as discontinuities, hysteresis, internal dynamics, and other complications. These properties cause the friction models to be numerically stiff and therefore computationally cumbersome [15]. The basic problem is the numerical stiffness of such systems. Models of friction derived from the Coulomb friction paradigm suggest that the friction force changes “discontinuously” as the direction of interfacial slip changes.

The figure 2.11 shows some typical sketches of friction force versus slip velocity.

It should be noted that “sticking” of the frictional interface is characterized by zero slip velocity; therefore, it is not uncommon for the frictional interface to spend intermittent and finite periods of time at zero slip velocity, where the friction law is discontinuous. One approach is to proceed with the above friction models and smooth the curve at the region of discontinuity or work with other friction models. In reality, the physical friction process is not discontinuous.

Various models of friction have been proposed that address this shortcoming by refining the behavior of the interface when the slipping velocity is small or when it changes sign. For example,

“microslip” models allow small amounts of displacement to occur during sticking. Examples of

friction models with smooth microslip behavior include the Dahl model , the Valanis model , and

the Leuven model [15]. This thesis will not focus on developing detailed friction models defining

the contact between chassis and subframe or the friction in bolted joints of the bracket as it is

considered to be time consuming and complex.

Chapter 3

Implementation

This chapter describes major parameters influencing the chassis dynamics, the physical vibration testing and the dynamic FE model of chassis and subframe. The necessary details regarding the test plan, setup and excitation signals are elaborated. Thereafter, a new method for building a dynamic FE model is presented. Detailed description of the FE model is given in the chapter with regard to the mesh, material properties and boundary conditions.

3.1 Description of Major Parameters

This section describes the major parameters which have an influence on the chassis dynamics. It is necessary to identify the parameters in the beginning as they form the basis for the vibration test plan and also in defining the scope of the FE model.

3.1.1 Number of Bodywork Attachments

The number of bodywork attachments that go into a truck play a major role as the number of clamping points would greatly influence the dynamic behavior of the chassis. As the number of clamping points increase, system tends to become stiffer.

3.1.2 Position of Bodywork Attachments

The position of of the bodywork is another parameter which is of importance as it affects the stiffness of the chassis-subframe assembly which in turn has an effect on the dynamic behavior.

For a given design and set number of brackets, the placement of brackets will have an effect on how different sections of the chassis-subframe assembly would move.

3.1.3 Design of Bodywork Attachments

As discussed in section 2.2.2, there are several types of bodywork attachments(brackets) which

are used based on the need and applicability. However, in the current thesis work, only three

types of brackets are tested as they are recommended brackets for the chassis and subframe of

the truck- Pacer.

CHAPTER 3. IMPLEMENTATION

(a)

(b)

(c)

Figure 3.1: (a) Rubber bushing bracket (b) Flexible bracket (c) Rigid bracket

3.1.4 Pretension/Bolt torque in Bodywork Attachments

Another factor which plays a major role in influencing the dynamic behavior of the chassis is the pre-tension or bolt torque in the bodywork attachments. This is applicable to rubber bushing and flexible brackets as they have vertical screws/bolts which are tightened with a definite torque value.

20

3.2. PHYSICAL VIBRATION TESTING

3.2 Physical Vibration Testing

3.2.1 Experimental Setup

The physical vibration testing is carried out at road simulator which is a test facility at RTCD (Chassis Dynamics group), Scania. The following section will describe the experimental setup and also the support fixtures that are designed for the setup. Figure 3.2 shows the experimental setup that is used to carry out the testing. Typically, a vägsimulator is used for full vehicle testing and the rig has six hydraulic cylinders which are indicated as H1-H6 (see figure 3.2) on the floor base.The wheels of the truck rest on the hydraulic cylinder base. However, in the present experimental study the chassis and subframe were to be tested in isolation. In this regard, a modification had to be made to accommodate the chassis-subframe assembly.

Figure 3.2: Experiment Setup

All other chassis components such as suspension,fuel tank etc are not part of the setup and only basic chassis with subframe is used for the testing. The chassis-subframe assembly is moved to one side of the vägsimulator. The entire assembly rests on the support rods and blocks.

(a) Front Support

The front support acts as the excitation source as the hydraulic cylinder underneath excites the

chassis-subframe system. The front support (see figure 3.3) consists of a green base plate which

is secured firmly to the base surface of the hydraulic cylinder. Two load cells are placed on top of

the green plate and screwed in. Two new rectangular blocks are designed and manufactured for

CHAPTER 3. IMPLEMENTATION

Figure 3.3: Front Support

the purpose of providing support base. These blocks are designed considering the hole pattern in the load cell. A hole is provided in the centre of the block to accommodate an M16 threaded rod which is also manufactured for this setup. The two rods are very long which allows the front module of the chassis frame to be adjusted in height.

(b) Rear Support

The rear support (see figure 3.4) acts as the fixed support for the assembly. It consists of four main components which are the rear block, ball joint rod, two-end threaded rod and a spacer. The rear block is a rectangular block with two slots which are provided to match the hole pattern on the black hydraulic cylinder base. Four M12 bolts are used to fix the block to the base. An M30 hole is provided approximately at the centre of the blocks. The hole is positioned based on the distance between the spring brackets. One end of the threaded rod is screwed into the block and on the other end, a ball joint rod is screwed in. The entire assembly is locked by the spring bracket bolt which has the spacer to provide a tight fit. The purpose of using a ball joint rod is to have a revolute joint or a pin joint allowing rotation about spring bracket bolt axis. This will not constrain the bending motion of the chassis. The hydraulic cylinder is not actuated making the entire rear support fixed.

22

3.2. PHYSICAL VIBRATION TESTING

Figure 3.4: Rear Support

3.2.2 Test Objective and Plan

(a) Objective

The purpose of physical vibration testing or experimental modal analysis is to determine the parameters of a physical model describing the vibrations of a structure. The measured frequency response functions help in identifying eigen frequencies, mode shapes and damping in the system.

(b) Test plan

The chassis-subframe assembly is rigged with the necessary measurement sensors which would

be explained in the next section. All the parameters such as bracket type, position etc are noted

and a test matrix is prepared to make changes to these parameters in different test cases. A

random noise excitation is done to achieve the above stated objective. A detailed test plan is

prepared to list all the different test cases. A total of 17 test cases are carried out. Table 3.1 gives

the summary of these test cases. Figure 3.5 shows the test arrangement. Base configuration

implies the factory fitted configuration where the brackets 1-3 are rubber bushing brackets, 4 is a

flexible bracket and 5-11 are rigid brackets.

CHAPTER 3. IMPLEMENTATION

Table 3.1: Test cases summary Test Case Bodywork attachment configuration

1 Base configuration

2 Base config with 6mm compression in rubber bushing brackets (1,2,3)

3 Base config with 12mm compression in rubber bushing brackets (1,2,3)

4 Three brackets (2,3,4) detached (vertical screws off) and compression of 12 mm in bracket 1

5 Three brackets (2,3,4) detached (vertical screws off) and compression of 6 mm in bracket 1

6 Three brackets (2,3,4) detached (vertical screws off) and bracket 1 is set to original state

7 Three brackets (2,3,4) removed (chassis brackets removed) and bracket 1 is set to original state

8 Three brackets (2,3,4) removed (chassis brackets removed) and bracket 1 has 6mm compression

9 Three brackets (2,3,4) removed (chassis brackets removed) and bracket 1 has 12mm compression

10 All 11 brackets are flex brackets with 30Nm bolt torque 11 All 11 brackets are flex brackets with 20Nm bolt torque 12 All 11 brackets are flex brackets with 10Nm bolt torque 13 All brackets removed (subframe resting on chassis) 14 Only bracket 1 and 11 with 30Nm

15 Bracket 1 and 11 with 30Nm and bracket 5 is flex with 20Nm 16 Bracket 1 and 11 with 30Nm and bracket 5 is rigid

17 Only chassis frame

3.2.3 Measurement Equipment

In the current experimental study, accelerometers, displacement sensors and load cells are used to measure the data. A total of 14 accelerometers are used of which seven accelerometers are placed on chassis (left side) and six on the subframe (left side). An accelerometer is also placed on the excitation cylinder to record the cylinder acceleration. Each accelerometer had two channels to measure the components in x(horizontal) and z (vertical) directions. A displacement sensor is placed at the front end of the subframe to record any relative horizontal movement of subframe with respect to the chassis frame. Two load cells are used in the front support to capture the force exerted by the hydraulic cylinder on the assembly. Figure 3.6 shows all the measurement sensors that are used during the physical vibration testing.

24

3.2. PHYSICAL VIBRATION TESTING

Figure 3.5: Test setup arrangement

Figure 3.6: Measurement Senors: (a) Accelerometers (b) Displacement sensor (c) Load cell

CHAPTER 3. IMPLEMENTATION

3.2.4 Excitation signals

As stated earlier, a random signal is used to excite the system.The random signal is run for time period of 180 seconds. Table 3.2 provides information about the input excitation signal that is used during the testing. The excitation is provided as cylinder base displacement. For each test case, there were typically three sub test cases that are carried out. These sub-cases are performed to see the influence of the excitation signal amplitude on the response.

Table 3.2: Excitation Signal Excitation signal Max

Amplitude Frequency Subcase Percentage of Max Amp

Random signal 1mm 4-40 Hz

1 50%

2 25%

3 12.5%

3.2.5 Data Acquisition and Processing

Figure 3.7: MATLAB tool for processing results

SIRIUS is the data acquisition hardware which is used for recording the measurement data.

This data is then processed with the help of software called DEWESoft. It is primarily a data acquisition and storage software with some analysis capabilities as well. The data is then exported

26

3.3. FINITE ELEMENT MODEL DESCRIPTION

to a MATLAB environment. Scania developed MATLAB based plot tool is then utilized to plot the required output (PSD, transfer function etc). The tool is also used for plotting the running mode which helps in visualizing the mode shape. Figure 3.7 shows the graphic user interface (GUI) of the tool used for processing the results.

3.3 Finite Element Model Description

The finite element (FE) modelling and analysis is carried out in Hypermesh and Abaqus software.

Hypermesh is used to build the FE model and mesh. Abaqus is used for solving and Abaqus Viewer is used for post-processing the results.

3.3.1 Scope and Method Development

The parameters influencing the chassis dynamics as described in section 3.1 define the scope of the FE model. Three methods are identified in the beginning to build the FE model. These methods are described below briefly:

• Defining a contact between chassis and subframe

• Defining a 3rd surface (material layer) which has the properties of contact and connection type defined in it

• Connecting the chassis and subframe with 1-D elements

With the first method (defining contact), the major drawback is that during a modal analysis

or eigen frequency analysis in Abaqus, the contact is ignored and hence this approach will not

meet the desired objective. The second approach involves incorporating the properties of contact

between chassis and subframe and the bracket modal parameters in the form a new material

layer. Though this is a good method, the development of such a detailed model requires more time

and is beyond the scope of this thesis. The third approach serves as the best alternative among

the three as it very well fits into the scope of FE model which requires the major parameters

to be modelled and altered easily to check the response. The main idea behind this method is

to use 1D elements as the bodywork brackets and define the properties of the brackets in these

elements. A simple case study is done by performing modal analysis on two simple rectangular

steel beams of 2m length and (50*20)mm cross section. This is done in order to evaluate and

understand the behavior of different 1D elements such as TIE, GAPS, SPRINGS, RIGIDS, etc

and identify the best element which could fit the application. CONN3D2(connector element) is a

versatile connector element which allows the user to define the its stiffness and damping with

respect to 6 degrees of freedom. CONN3D2 is identified as the best element type which very well

serves the desired objective.

CHAPTER 3. IMPLEMENTATION

Figure 3.8: FE model method: (a) 1-D element connection (b) Contact (c) New material layer

3.3.2 Chassis and Subframe Model

A simplified model of chassis and subframe is imported from CATIA into Hypermesh. The model is split in the centre along XZ plane and it is decided to perform the FE analysis with half model by placing a symmetry constraint along the XZ plane. Figure 3.9 and Figure 3.10 show the meshed half model of chassis and subframe respectively. Working with the half model will not affect the bending modes and will save computational time. Table 3.3 provides details of the sub components which make the chassis and subframe. The modelling of interface and joints between these components is explained the next section.

Table 3.3: Components of chassis and subframe

Components (Chassis) Quantity Components (Subframe) Quantity

Side member 1 Side member 1

Cross member 8 Cross members 4

Front beam 1 Bunk bodies 2

Central beam 1 Front stop (sub-assembly) 4

Front side plate 1

Torque bracket 1

Base bracket 1

28

3.3. FINITE ELEMENT MODEL DESCRIPTION

Figure 3.9: FE model: (a) Half model of chassis (b) Section showing the mesh

Figure 3.10: FE model: (a) Section showing mesh (b) Half model of subframe

CHAPTER 3. IMPLEMENTATION

3.3.3 Interface and Joints

Figure 3.11: Subframe: (a) Side and cross member interface (b) Front stop and side member interface (c)Bunk body and sidemember interface

Figure 3.12: Chassis: Interfaces and joints

30

3.3. FINITE ELEMENT MODEL DESCRIPTION

Chassis and subframe are comprised of several sub-components. The interfaces of these compo- nents are modelled using extend resmesh, ruled mesh, and B31 (spider) for bolted joints. The extend remesh option is used to connect all the subframe cross memebers to its side member.Ruled mesh option is used to connect bunk bodies and front stop to the side member in subframe. All the bolted joints in chassis and subframe are modelled as spider connection with B31 elements.

These options are available in Hypermesh and will not be explained in detail. Figure 3.11 and Figure 3.12 show the interfaces and joints in subframe and chassis respectively.

3.3.4 Modelling the Bodywork Attachments

As discussed in section 3.3.1, the bodywork attachments are modelled as connector elements (CONN3D2). Figure 3.13 shows the connector model which represents the bodywork brackets.

The holes in the chassis and subframe provide an accurate position of the attachment points. 1D rigid beam elements are used to create a spider (shown in green) which connects all the nodes present on the circumference of the hole to its centre. Typically, each bracket uses three frame holes to be fixed on the frame.The corresponding middle hole from chassis and subframe is chosen for connecting the end points of the connector (shown in blue).

Figure 3.13: Connector model for brackets

CHAPTER 3. IMPLEMENTATION

Figure 3.14: Example: Connector definition

3.3.5 Material

The chassis and subframe components have been modelled with steel properties as shown in Table 3.4.

Table 3.4: Material property of steel

Property Value

Density 7.85e-9 ton/mm ³ Young’s Modulus 210e3 N/mm ²

Poisson’s ratio 0.3

3.3.6 Mesh

The choice of elements play an important role in the FE analysis as it affects not only the quality of results but also the computational time needed to perform the simulation. In the present study, the two main components of the FE model are the chassis frame and subframe. Since the the major components of chassis and subframe are quite long and have approximately uniform thickness , SHELL elements i.e. mixed mesh of TRIA and QUAD elements are used to mesh them.

However, for components with non-uniform thickness, SOLID elements are used for meshing. A coarse mesh has been applied to the model as the current study does not focus on stresses in the

32

3.3. FINITE ELEMENT MODEL DESCRIPTION

system but only on the eigen frequencies which are not affected by the element size. The details of the elements and corresponding properties for all the components are listed in Table 3.5

Table 3.5: Mesh details

Property Components (Chassis)

Components (Subframe)

Cross member-5 Torque bracket

Base bracket (Chassis)

Bolts Front rod

Rear rod

Bodywork Attachments

Element

type S4 and S3R S4 and S3R C3D10I B31 CONN3D2

Element

property SHELL SHELL SOLID BEAM

SECTION

CONNECTOR SECTION Element

size

1.5-15mm (Adaptive mesh)

1.5-15mm (Adaptive mesh)

0.8-30mm

(Adaptive mesh) - -

Material Steel Steel Cast steel Steel CONNECTOR

BEHAVIOR

Thickness 8mm 6mm - - -

3.3.7 Boundary Conditions and Constraints

Figure 3.15: (a) Front Support (b) Rear Support

Boundary conditions greatly influence the FE results and hence have to be modelled as close to

reality as possible. In the present FE model setup, there are two boundary conditions i.e. front

CHAPTER 3. IMPLEMENTATION

and rear support.

(a) Front support

The front support rod is modelled using a B31 element which is a 1D bar or beam element and takes the properties of the material defined by the user which in this case is steel. The bottom node of the B31 element is fixed or in other words has all 6 degrees of freedom constrained. The top node of the 1D bar is connected to central node underneath the chassis cross beam section. It represents the hole drilled in the front cross beam. The cross section of the beam is circular with a radius of 8mm.

(b) Rear support

The rear support rod is modelled using again a B31 element as in previous case. The rear support is quite complex compared to the front support as the ball joint rod provides a rotational degree of freedom along the spring bracket bolt axis. B31 elements (indicated in red colour) are modelled as spider connection from the two the spring bracket holes which results in creation of central node. The purpose of using B31 elements for the spider connection is that it introduces stiffness properties of steel in the bolted connection which is more realistic than modelling it as rigid connection. A revolute joint is created with the help of the CONN3D2 element . The rotational degree of freedom about y-axis (bolt axis) is made free by defining a very low stiffness value (k=1N/mm) in the CONN3D2 element. This connector forms the link between spider central node and the top node of B31 (support rod).The bottom node of the B31 element is fixed as in the previous case. The cross section of the support rod is circular with a radius of 15mm.

(c) Symmetry Constraint

Th symmetry plane for the assembly is XZ plane. FE simulation of half model (chassis and assembly), following constraint has been applied:

U _x = free U _y = zero U _z = free R _x = zero R _y = free R _z = zero

34

Chapter 4

Results and Discussions

This chapter presents the results from experimental vibration testing and the FE analysis (modal analysis). The results are first discussed separately to analyze the findings of physical testing, followed by FE results and correlation between the two.

4.1 Physical Vibration Testing

This section will focus on the results from the random vibration testing which gives information about the eigen frequencies, mode shapes and modal damping.

4.1.1 Influence of Excitation Signal

The influence of excitation signal amplitude on the output parameters is presented and discussed below. This is done by analyzing the results from acceleration PSD plot, transfer function plot and coherence plot. The legends in the PSD plot, transfer function plot and coherence plot given as random_ 50, random_ 25 and random_ 12 correspond to random excitation signal with 50%

25% and 12.5% of maximum displacement amplitude.

(a) Test case 1: Base configuration

It is observed from the PSD plot (shown in figure 4.1) that the eigen frequencies for the first mode are 9.37 Hz, 9.57 Hz and 9.57 Hz for 50% 25% and 12.5% amplitude random signal respectively.

For the second eigen mode the frequencies are 16.99 Hz, 17.38 Hz and 17.38 Hz for 50% , 25% and 12.5% amplitude random signal respectively. The values show that the input signal excitation has an affect on the eigen frequencies. The trend indicates that as the input signal excitation amplitude increases the eigen frequency value decreases for a given mode.´The bending stiffness of the assembly is higher when the two frame surfaces are sticking to one another. When a higher amount of energy is supplied to a coupled system which has non-linear effects, it could be possible that when a greater amount of energy (higher amplitude) supplied to the system, the contact between two surfaces may change from "sticking" to "slipping" making the frames and surfaces under bolt heads slide. This could result in reduced stiffness and thereby lower eigen frequency.

From the transfer function plot between frame acceleration and cylinder acceleration (shown

in figure 4.2), information is obtained on the amplification , phase angle and coherence in the

system. Amplification plot agrees well with eigen frequency values as the peaks denote response

CHAPTER 4. RESULTS AND DISCUSSIONS

amplification at eigen frequencies. The phase angle plot shows that there is 180 degree phase shift occurring at eigen frequencies further ascertaining the above observation. The 360 degree phase shift in the range of 25-40 Hz can be ignored as it is a mathematical feature in the post processing tool and does not have any physical significance. Interesting aspect to note from the coherence plot is the that the coherence values at resonances are close to 1 which indicates repeatability in measurement. However, the coherence value is very low (0.2) at around 13Hz and 35 Hz. This is because these points indicate the presence of anti-resonances. In general, anti-resonances occur between two resonances.

Figure 4.1: Acceleration PSD : Test case 1 (Base Configuration)

36

4.1. PHYSICAL VIBRATION TESTING

Figure 4.2: Transfer function, Cyl acc. vs Frame acc. :Test case 1 (Base Configuration)

(b) Test case 11: All 11 brackets flex (20 Nm)

Another test case results are presented to confirm the trends observed in the previous case.

From the PSD plot (shown in figure 4.3) the eigen frequencies for the first mode are 9.961 Hz, 10.16 Hz and 10.16 Hz for 50% , 25% and 12.5% amplitude random signal respectively. For the second eigen mode the frequencies are 17.77 Hz, 18.16 Hz and 18.36 Hz for 50% , 25% and 12.5%

amplitude random signal respectively. Again values indicate that the input signal excitation amplitude does affect the eigen frequencies. The trend shows that as the input signal excitation amplitude increases, the eigen frequency value decreases for the assembly configuration.

From the transfer function plot between frame acceleration and cylinder acceleration (shown in figure 4.4), information is obtained on the amplification , phase angle and coherence in the system. Amplification plot agrees well with eigen frequencies values as the peaks denote response amplification at eigen frequencies. The phase angle plot shows that there is 180 degree phase shift occurring at eigen frequencies further ascertaining the above observation. The findings from the coherence plot is the that the coherence values at resonances are close to 1 which indicates repeatability in measurement. However, the coherence value is very low (0.2) at around 12.5Hz.

This is because this point represents anti-resonance.

CHAPTER 4. RESULTS AND DISCUSSIONS

Figure 4.3: Acceleration PSD : Test case 11: All 11 brackets flex (20 Nm)

Figure 4.4: Transfer function, Cyl acc. vs Frame acc.: Test case 11 (All 11 brackets flex (20 Nm))

38

4.1. PHYSICAL VIBRATION TESTING

4.1.2 Test Cases: Study and Comparison

Comparison of different test cases is presented and discussed below. Since it is found that excitation signal amplitude does have an effect on the output, the results from all the test cases are with respect to 50% amplitude random signal measured at chassis frame position 3z. This will ensure fair comparison and the inferences from the experimental results will be more reliable.

The results i.e the eigen frequencies and modal damping ratio (%) are listed in table 4.1.

Table 4.1: Experiment result summary

Test Case Eigen Mode 1 (Hz)

Damping ratio (%)

Eigen Mode 2 (Hz)

Damping ratio (%)

1 9.375 2.66 16.8 1.48

2 9.570 1.95 17.58 1.99

3 9.766 1.28 17.58 1.19

4 9.570 3.13 17.19 1.74

5 9.180 2.72 16.8 1.33

6 8.984 2.22 16.6 1.26

7 8.203 2.43 16.21 1.29

8 8.398 3.57 16.8 1.78

9 9.375 4.26 17.19 2.32

10 9.961 1.50 17.97 1.25

11 9.961 1.90 17.77 1.68

12 9.570 2.19 17.38 1.72

13 9.180 4.35 15.04 2.32

14 9.570 2.09 14.65 1.57

15 9.570 2.61 17.38 2.44

16 9.375 2.66 16.6 2.16

17 10.550 0.85 20.9 1.91

(a) Comparison of Test cases 1, 2 and 3

Figure 4.5 shows the acceleration PSD plot of test cases 1, 2 and 3. These test cases corre- spond to the base(standard) configuration, standard configuration with compression of 6mm and 12mm in rubber bushing brackets numbered 1,2 and 3. It can be observed that as the compression increases, the eigen frequencies for the first and second eigen modes rise up. This can be attributed to the increased contact stiffness introduced because of greater clamping force (normal force) when the rubber bushing brackets are compressed.

With regard to damping, the damping ratio decreases as the compression in rubber bushing

brackets increases in case of the first eigen mode. For the second eigen mode, the damping ratio

increases and then there is sudden drop in the value with increase in compression. The overall

trend suggests that damping is more for the standard configuration which could also be observed

from the low acceleration amplification values from the plot. This could be due to the greater