V1
2...

El)

.51

a... $2.

, fik.f_
wkwfimmwvfi fig.
, :1 . .4 . ,

 

,zi. Janka
J...

.
.5...

4
~
.A

A ..
A???” 51
.v I.

Suwumi...n.~ ,% . 5.

; in? 3...”.le

.4... EM?“ .
It!

Ln :1
3.5.21.1
u...“ .v

d! 4.!32 .. . g
snark. 3.1. 171.2359 4.

E... 3.5~ g: 13.5.
74)] {chin £3.19 .

 

. spew
.... ,. v
(HWHJnn

.1... . .13.».
a3; ..

...v.
in. ..

. . . . ‘02KTRWh36.
. 42...}: . . . . n :3 a 441.. .3 . , , ”firm” . :94»... 13...;
‘33 73M fiflfiniw ...:.. .3 IfiRfi. “aw—WWW , . .t .2 .. .. 1.4.3.. .. . . .

 

 

 

.1 - LIBRARY
.100 f Mid'ligan Sm
Umrersrly

 

 

This is to certify that the
thesis entitled

THREE-DIMENSIONAL STRAIN ANALYSIS OF SINGLE-LAP
BOLTED JOINTS IN THICK COMPOSITES USING FIBER-
OPTIC STRAIN GAGES AND FINITE ELEMENT METHOD

presented by

GABRIEL A. ISAICU

has been accepted towards fulfillment
of the requirements for the

MS. degree in Mechanical Engineering

 

 

Azami

Major Professor’s Signature
3 1%; a») 2 no 4.

Date

MSU is an Affirmative Action/Equal Opportunity Institution

 

 

PLACE IN RETURN BOX to remove this checkout from your record.
To AVOID FINES return on or before date due.
MAY BE RECALLED with earlier due date if requested.

 

DATE DUE

DATE DUE

DATE DUE

 

 

 

 

 

 

 

 

 

 

 

 

 

 

2/05 p:lC|RC/DateDue.indd-p.1

 

THREE-DIMENSIONAL STRAIN ANALYSIS OF SINGLE-LAP
BOLTED JOINTS IN THICK COMPOSITES USING FIBER-
OPTIC STRAIN GAGES AND FINITE ELEMENT METHOD

BY

Gabriel A. Isaicu

A THESIS

Submitted to
Michigan State University
in partial fulfillment of the requirements
for the degree of

MASTER OF SCIENCE
Department of Mechanical Engineering

2006

ABSTRACT
THREE-DIMENSIONAL STRAIN ANALYSIS OF SINGLE-LAP BOLTED JOINTS IN
THICK COMPOSITES USING FIBER-OPTIC STRAIN GAGES AND FINITE ELEMENT
METHOD
BY

Gabriel A. Isaicu

Bolted joints involving composite plates used to be almost entirely
dedicated to aero—space applications. As the need for energy conservation
increases, the field of composite bolted joints finds new application in ground
armored vehicles. Thick panels able to withstand large in-plane and impact loads
are critical. This study was concerned with the evaluation of strain fields in thick
composite plates used in single-lap bolted joints. The area of interest was the
bearing plane region close to the bolt hole. Both experimental and finite element
analyses were performed to evaluate possible failure causes and three-
dimensional effects present in thick composite bolted joints. Experiments were
performed for pin connection and bolted joint configurations. Experimental data
for the pin connection and the bolted joints were recorded by embedded fiber-
optic strain gages. The fiber-optic strain gages were embedded in the bearing
plane of the composite plate. The numerical analysis was performed using both
ANSYS and LS-DYNA finite element codes. The finite element analysis correlated

reasonably well with the experiments.

to my beloved parents, Ligia and Aurel Isaicu

ACKNOWLEDGEMENTS

I would like to gratefully acknowledge Professor Gary L. Cloud for his
continuous and determined support, sound advice and the opportunity to work
on this project. I would like thank Dr. Dahsin Liu and Farhang Pourboghrat for
their interest in this research. I would also like to thank my colleague, Dr.
Gaetano Restivo, for the help, advice and efforts during this project. Last but not
least I would like to thank my brother, Adrian, and my wife, Dominique, for all

their patience, love and support. To all of the above, THANK YOU!

TABLE OF CONTENTS

List of Tables ......................................................................................................... vii
List of Figures ......................................................................................................... viii
Key to Symbols ...................................................................................................... xii
Chapter 1 ..................................................................................................... 1
1.1 LITERATURE REVIEW ........................................................................... 3
1.1.1 Purely Experimental Studies ............................................................ 3
1.1.2 Combined Experimental and Finite Element Analysis Studies .............. 9
Chapter 2 ................................................................................................... 13
Chapter 3 ................................................................................................... 17
3.1 FIBER-OPTIC STRAIN GAGES .............................................................. 18
3.2 MATERIAL PROPERTIES VALIDATION .................................................. 24
3.2.1 Volume Fraction Determination ..................................................... 25
3.2.2 Experimental Validation of Material Properties ................................ 26

3.3 CLAMPING FORCE DETERMINATION ................................................... 35
3.4 EXPERIMENTAL ANALYSIS .................................................................. 40
Chapter 4 ................................................................................................... 47
4.1 FINITE ELEMENT MODEL DESCRIPTION .............................................. 49
4.1.1 ANSYS Finite Element Models ........................................................ 50
4.1.2 LS-DYNA Finite Element Models .................................................... 63

V

Chapter 5 ................................................................................................... 72

5.1 RESULTS FOR TYPE 1 SPECIMENS ...................................................... 72
5.2 RESULTS FOR THE TYPE 2 SPECIMEN ................................................. 78
Chapter 6 ................................................................................................... 90
Chapter 7 ................................................................................................... 94
7.1 FIBER-OPTIC STRAIN GAGE ERRORS .................................................. 94
7.2 FINITE ELEMENT MODELING .............................................................. 95
7.3 MACRO-MECHANICAL PROPERTIES ..................................................... 96
7.4 FRICTION COEFFICIENTS ................................................................... 97
Chapter 8 ................................................................................................... 98
APPENDIX 1 ............................................................................................... 99
REFERENCES ............................................................................................. 117

vi

LIST OF TABLES

Table 3.1 E-glass and epoxy resin properties ................................................. 24
Table 3.2 Composite laminate material properties. ......................................... 27
Table 3.3 Readings from the R56 rosettes and fiber-optic strain gages ............ 32
Table 3.4 Material properties validation ......................................................... 34
APPENDD( 1

Table A.1 Mold dimensions. ........................................................................ 102

vii

LIST OF FIGURES

Figure 1.1 Single-lap bolted joint. ................................................................... 2
Figure 1.2 Basic failure modes. ...................................................................... 4
Figure 1.3 FRP specific failure modes. ............................................................. 4
Figure 3.1 Light paths through generic optical fiber. ...................................... 19
Figure 3.2 Typical Fabry-Perot strain sensor. ................................................. 20
Figure 3.3 Typical Extrinsic Fabry-Perot Deployment. ..................................... 20
Figure 3.4 Cross correlation using Fizeau interferometer. ............................... 21

Figure 3.5 Fiber-optic strain gage (FOSG) glued to the E-glass weave with

schematics of the FOSG ............................................................................... 23
Figure 3.6 Sample attachment of fiber-optic strain gages to E-glass weave. ..... 29
Figure 3.7 Optical fiber attachment point. ..................................................... 30
Figure 3.8 Tensile test specimen and strain gage layout. ................................ 30
Figure 3.9 Tensile test loading setup and data acquisition equipment. ............. 31
Figure 3.10 Tensile test result comparison. ................................................... 33
Figure 3.11 Load cell transducer ................................................................... 36
Figure 3.12 Transducer calibration. .............................................................. 37
Figure 3.13 Clamping force variation for successive 25lb-in bolt torque

applications. ............................................................................................... 38
Figure 3.14 Clamping force relaxation. .......................................................... 39

Figure 3.15 Type 1 Specimens: (a) Fiber-optic strain gage attached to the E-
glass weave; (b) schematics of the sensor locations; (c) sensor locations and
identification ............................................................................................... 42

Figure 3.16 Specimen dimensions for the Type 1 specimens. .......................... 43

viii

Figure 3.17 Dimensions for the aluminum plate and Type Zspecimen. ............ 44

Figure 3.18 Fiber-optic strain gage locations in the Type Zspecimen ............... 45
Figure 3.19 Loading frame schematics. ......................................................... 46
Figure 3.20 Bolted joint with transducer — loading frame position .................... 46
figure 4.1 Validation scheme. ...................................................................... 48
Figure 4.2 Tensile specimen model with applied boundary conditions. ............. 51
Figure 4.3 Longitudinal (top) and transverse (bottom) strains for 50lb load ..... 52
figure 4.4 Meshed bolted joint. .................................................................... 53
Figure 4.5 Symmetry expansion mesh. ......................................................... 54
Figure 4.6 Close-up view of selected elements around the bolt hole. ............... 55
figure 4.7 Bolt, washer and nut assembly. .................................................... 56
Figure 4.8 Bolt pretension scheme ................................................................ 58

figure 4.9 Contact surfaces (element shrinkage used for better visualization). . 59

figure 4.10 Finite element model of the bolted joint with boundary conditions

and load ..................................................................................................... 62
Figure 4.11 LS-DYNA pin connection model. .................................................. 64
Figure 4.12 LS-DYNA pin connection model: close-up view. ............................ 66
Figure 4.13 LS-DYNA bolted joint model. ...................................................... 69
figure 4.14 LS-DYNA bolted joint model: close-up view .................................. 70
Figure 4.15 LS-DYNA bolted joint model: symmetry expansion. ...................... 71

Figure 5.1 Results comparison for Type 1 specimens: sxx (25lb-in bolt torque) -
one sample experiment. .............................................................................. 73

figure 5.2 Type 1 specimens: 3,0. strain map for 150lb load and 25 lb-in bolt
torque ........................................................................................................ 74

ix

Figure 5.3 Type 1 specimens: symmetry expansion of the sxx strain map for
150lb load and 25lb—in bolt torque. ............................................................... 75

figure 5.4 Type I specimens: Shear stress ox, at 150lb load and 25Ib-in bolt
torque. ....................................................................................................... 76

Figure 5.5 Type 1 specimens: von Mises stress map in the fastener at 150lb load
and 25lb-in bolt torque. ............................................................................... 77

Figure 5.6 2,0. strain map of the bolted joint for 150lb load and 25lb—in bolt
torque ........................................................................................................ 77

Figure 5.7 Equivalent positions of the fiber-optic sensors for Type Zspecimen. 79

Figure 5.8 Results comparison for Type Zspecimen: exx for the pin connection
case ........................................................................................................... 80

figure 5.9 Pin connection: a,“ strain map for Type Zspecimen at 200lb load.... 81

figure 5.10 Pin connection: a,“ strain map with visible secondary contact point at
200lb load. ................................................................................................. 82

Figure 5.11 Pin connection: Type Zspecimen exx strain map at 200lb load. ...... 83

Figure 5.12 Results comparison for the Type 2 specimen: a,“ for the 25lb—in bolt
torque case. ............................................................................................... 84

figure 5.13 Type 2 specimen: Assumed bulge representation compared with FEA

results. ...................................................................................................... 86
Figure 5.14 Type Zspecimen: ex, strain map at 200lb load and 25lb-in bolt

torque ........................................................................................................ 88
Figure 5.15 Type Zspecimen: a,“ strain map at 200Ib load and 25lb-in bolt

torque ........................................................................................................ 89
figure 7.1 Fiber optic strain gage embedded in composite plate. .................... 95
Figure 7.2 Simplified fastener finite element model. ....................................... 96

Appendix 1

figure A.1 Specimen dimensions. ................................................................ 102
figure A.2 Mold shape. ............................................................................... 103
Figure A3 The mold: before cutting the side channel to accommodate the side

exiting sensor. ........................................................................................... 104
Figure A.4 Fiber-optic sensors positions. ...................................................... 105
figure A.5 Fiber optic sensor bearing shrink wrap tubing ............................... 107
figure A.6 Sensor positioning. ..................................................................... 109
figure A] Sensor position on the E-glass weave. ......................................... 108
figure A.8 Special tool for mold releasing ..................................................... 113
figure A.9 Composite plate trimming. .......................................................... 115

xi

KEY TO SYMBOLS

E - Young's elasticity modulus
v — Poisson ratio

v - Volume

V - Volume fraction

G - Shear modulus

T - Installation torque

K - torque coefficient

D - nominal bolt diameter

P - clamping load

a - strain

0 - stress

xii

Chapter 1

INTRODUCTION

“The field of composite materials is both old and new. Is old in the sense
that most natural objects, including human body, plants, animals are composite.
It is new in the sense that only since the early 19605 have engineers and
scientists exploited seriously the vast potential of fabricated fibrous composite

materials“ (1998).

Fastening composite structures induces yet another problem in the search
for a complete understanding of their behavior. The simplest methods to fasten
composites are bolting, riveting and bonding. Bonding and riveting do not allow
for easy removal or replacement of damaged parts and inspection under limited-
space conditions. Bolting composites, however, proves to be a very inexpensive
and efficient solution. Parts can be easily removed and replaced, and structural
integrity can be evaluated with ease. A standard single-lap bolted joint is shown

in Figure 1.1.

 

Figure 1.1 Single-lap bolted joint.

Many composite structures have been designed to be used in applications
such as aerospace, ship building, sports equipment and circuit boards. These
structures use mostly single or double-lap bolted joint configurations, and they
are generally multi-fastened. Composite plates used for these applications are

usually thin to moderately thick.

In the past few years, new applications that require increased strength
are driving composite structures into new and innovative fields such as general
automotive parts and ground armor transport vehicles. For these fields, a solid
balance between strength and weight is needed. Strength is needed to safely
replace current designs, and reduced weight is required for improved vehicle

handling, fuel efficiency and, last but not least, fast deployment.

1.1 LITERA TURE REVIEW

Past and present research dedicated to bolted joints of composite
structures is channeled in two main directions: experimental studies on failure
and damage propagation and, the newest trend, numerical simulations.
Advances made in computing power in the past decade influenced the
development of powerful computer programs capable of simulating mechanical
interactions such as contact between three-dimensional surfaces and dynamic

contact between mechanical components.

1.1.1 Purely Experimental Studies

To take advantage of Fiber Reinforced Polymers (FRP) composite
structures, complete analyses of stress and strain distributions in the composite
structure are needed. The influence of stress concentration factors such as the
bolt hole, bolt hole to plate edge distance, hole diameter, and bolt-to-hole

clearance have to be fully understood.

The most common types of failure in composite structures are shown in

Figure 1.2.

 

 

 

 

 

 

Net-section

CZ:

 

 

 

 

O»

Shear-out

 

 

 

 

Bearing

 

 

Cleavage

Figure 1.2 Basic failure modes.

Specific failure modes in FRP composites are shown in Figure 1.3.

 

 

Hr

Kinking

ll

Fiber failure

l-l
lll

Matrix cracking

=5
7.—

_
Delamination

Figure 1.3 FRP specific failure modes.

In an extended experimental study on damage development in
mechanically fastened laminate composites, Ireman et al. (2000) used
graphite/epoxy laminates in an attempt to characterize damage development
close to the bolt hole. The laminate configurations in test specimens were quasi-
isotropic: [(i45/0/90)4]s and [(1:45/0/90)eIs; and zero-dominant
[(145/90/02/90/02)2]s. The thicknesses of the composite plates used in this study
were 4.16mm and 8.32mm, corresponding to 0.16in and 0.32in, respectively.
The study used both single and multi-bolt configurations of single-lap joints in
conjunction with a special fixture to eliminate the bending moment caused by
the eccentric load path (secondary bending). Both countersunk and protruding
head bolts were used. Damage development was assessed using resistance
strain gages, acoustic emission, X-ray, and by microscopic examinations.
Destructive examination was performed, as the specimens were cut and polished
and then examined under the microscope. The specimens were loaded a number
of times (six or seven) and monitored by acoustic emission. When acoustic
emission showed that some damage occurred to the specimen, the loading was
stopped and the specimen was examined by X-ray and microscope. The study
concluded that the specimens tend to experience the whole palette of FRP failure
modes before total failure is reached. As the load increases the specimens show

matrix cracking, fiber failure, delamination and kinking followed by total failure.

Hou and Liu (2003) studied the effects of size and thickness on the
composite joints. Glass/epoxy specimens with [0,90] stacking sequence of 9, 17
and 34 plies were employed in a double-lap pin joint configuration. Specimens
were 0.13in, 0.25in and 0.5in thick. On the effect of joint length on the
composite joint, the study concluded that as the ratio between the length from
the hole to the clamped end over the width passed 4, the joint strength remains
fairly constant. Investigations of three-dimensional size effects revealed that the
ratio of thickness over the hole diameter was found to be a critical value for the
composite joint. The effect of pin-hole clearance values over the joint was clear,
with the joint strength decreasing as the clearance increased. As the loading rate
increased, an increase in the joint strength was observed. The study also
concluded that as the FRP plate thickness increased, a decrease in strength was
observed. This result was compared to the Weibull theory. All specimens except
the one with 34 plies and 0.5in thickness experienced bearing damage. The

0.5in thick specimen experienced total net-section failure.

Lawlor, McCarthy and Stanley (2002) did an experimental study concerned
with the effects of clearance on single-lap single-bolt composite joints. The
specimens were made of carbon fiber/epoxy with the thickness between 0.11in
and 0.2in having two different stacking sequences: one quasi-isotropic and one
zero-dominated. Bolts used were aerospace grade titanium alloy with 8mm

(0.31in) nominal diameter. Both protruding head and countersunk fasteners were

used along with steel washers and nuts. The bolt torques applied were “finger
tight” and 141 lb-in. Clearance was obtained by using constant nominal diameter
bolts and by varying hole diameter. The study concludes that the main effects of
clearance were concentrated in stiffness and ultimate strain variation with little
effect on strength. An expected delay in load take-up and better load distribution

were experienced with high clearance value specimens.

An experimental study on fatigue resistance of composite joints using
protruding head bolts, written by Starikov and Schon (2002), employed carbon
fiber/epoxy plates with quasi-isotropic and 0-degree lay-ups. Specimens were
used in single and double-lap multi-bolt configurations. All specimens had the
same thickness of 3.12mm (0.12in). Bolts used in this study were titanium with
protruding heads (hexagon type). The single-lap configuration used 6 bolts
evenly distributed in 3 lines. Bolts were tightened with 80lb—in torque. Fatigue
tests were performed by loading and unloading the specimen. The number of
cycles used was in the range 103-106, depending on when failure of the bolted
joint occurred. Measurements were done using resistance strain gages to analyze
strain distribution and load transfer between bolt rows. Extensometers were used
to evaluate relative displacement between composite plates. The plates were
loaded using two approaches: additional plates glued to the specimen or lateral
supports with Teflon lubrication. Both approaches are used to avoid secondary

bending. The study concluded that there is a linear dependence between the

fatigue resistance and the number of bolts used in the joint. Bolt failure was the
dominant cause of joint failure. However, the joints supporting the highest loads

failed in two modes.

Tong (2000) studied the bearing failure of composite bolted joints with
non-uniform bolt-to-washer clearance. The study focused on the relative
positions of the bolt and washer on the bearing failure of the bolted joint.
Composite plates were made of carbon/epoxy using a quasi-isotropic stacking
sequence. The specimens were set to have 8 plies of plain carbon weave adding
up to 1.72mm (0.068in) in thickness. Steel bolts, nuts and washers were used
for the joining of the composite panel to two steel plates in a double lap
configuration. A piezoelectric load cell transducer was used to measure clamping
loads. Experimental results were compared to analytical results based on a
modified model of Herrington and Sabbaghian. The author observed good
agreement for the case when the washer is offset in the loading direction and
poor agreement for the case when the washer is offset opposite to the loading
direction. Possible causes that may influence the agreement between
experimental and analytical results are listed. The study concludes that the
extreme positions of the washer to the bolt shank slightly affects the initial

failure load but has no significant influence on the ultimate failure load.

Herrera-Franco and Cloud (1992) did an experimental study concerning
the stress and strain distributions in the vicinity of single-pin lap joints. The study
presented options for reducing stress concentrations by use of hole inserts. The
specimens used were made of thirteen layers of regular symmetric cross-ply
glass/epoxy having a 0.14in thickness. The specimens were loaded in a double-
lap single-bolt configuration. Measurements of surface stress and strain fields in
the neighborhood of the hole were performed by means of moiré interferometry.
Measurements were taken for no insert, a hard insert (aluminum) and a soft
insert (epoxy) in an isotropic material and in the glass/epoxy composite. High
sensitivity moiré interferometery was used to measure surface strains within the
insert ring. One of the conclusions reached by the authors was that a 50%
reduction in bearing strains for the case of a soft insert ring, compared with the
no-insert case in the composite plate. Also, approximately 50% reduction of the
shear strain in the bearing region is observed. For the case of the hard insert,
there was a 90% reduction of the bearing stress at the edge of the hole

compared to the no-insert case.

1.1.2 Combined Experimental and Finite Element Analysis Studies

Previous finite element models built to simulate bolted joints were mainly

conducted only two-dimensional analyses. Few of the studies conducted with the

9

help of the Finite Element Analysis (FEA) modeled the bolted joint as a three-

dimensional model.

One of first studies concerned with three-dimensional stress analysis of a
composite laminate bolted joint was developed by Chen, Lee and Yah (1995).
The study reports on a general method of evaluating contact stresses generated
by the bolt-hole interaction using an incremental variational principle formulation
and the transformation matrix derived from three-dimensional contact kinematic
conditions. The numerical results obtained were compared with experimental
results from a double-lap bolted joint. The composite plates used in the
experiment were thin graphite/epoxy with [i45/0/90]s quasi-isotropic lay-up and
thick glass/epoxy of various stacking sequences. The effects of friction,
clearance, bolt elasticity, stacking sequence and clamping on the contact
tractions around the bolted joint were included in the analysis. Clamping force
was modeled as pressure and it was determined analytically. Good agreement
between the numerical results and the referenced experimental results was

reported.

Another study by Chutima and Blackie (1996) looked into the effects of
pitch distance, row spacing, end distance and bolt diameter on multi-fastened
composite joints. The authors limited their study to a multi-bolt double-lap

configuration of the bolted joint. The study used a two-dimensional finite

10

element model to calculate contact stresses and load distribution. The study
reported that friction at the bolt-hole interface exerted a considerable effect on

the local contact stress distribution around the holes.

Camanho and Matthews (1997) wrote a review of the investigations that
have been made on the stress and strength analysis of bolted joints in FRP
composites. The review highlighted different methods used to predict failure in
single or multi-fastener joints, numerical approaches that include two and three-
dimensional models as well as an assessment of the effects of clearance, friction
and geometry. The authors concluded that in order to include important aspects
of the joint’s behavior and strength the use of three-dimensional models is

necessary.

Ireman (1998) did a three-dimensional stress analysis of bolted single-lap
composite joints. A three-dimensional finite element model of the composite
bolted joint was developed to determine non-uniform stress distributions through
the thickness of composite laminates in the proximity of the bolt hole. The finite
element models were created using IDEAS and solved using ABAQUS, a
commercially available finite element software. Added supports were used to
eliminate secondary bending due to offset boundary conditions. One coefficient
of friction was used for all contact surfaces due to software limitations.

Numerical results were compared against strain gage measurements.

11

Kermanidis et al. (2000) developed a three-dimensional progressive
damage model to simulate damage accumulation in single-lap bolted joints.
Stress analysis was performed using ANSYS software and the model was
incorporated in the ANSYS solving routine. The model was based on the Hashin-
type criteria and contained a set of degradation rules. FEA results were then

compared to experimental results from Ireman’s study (1998).

Whitney et al. (2004) studied singular stress fields near contact
boundaries in composite bolted joints. The study focused on the singular stresses
arising in the vicinity of contact surfaces induced in laminated orthotropic plates
by mechanical fastening. The investigations were done using local asymptotic
solutions and full-field numerical analysis. Frictionless contact conditions were
assumed. The bolted joint numerical model considered symmetry with respect to

the contact plane between the two plates forming the bolted joint.

A study conducted by Iancu et al. (2004) studied bolted joints of an
isotropic material and aluminum. A three-dimensional numerical model was built
and results were compared against photoelasticity and resistance strain gages
(RSG) experimental results. The model boundary conditions were such that
secondary bending was eliminated. Good agreement between experimental and

numerical results was reported.

12

Chapter 2

RESEARCH OBJECTIVES

As mentioned in Chapter 1, most of the past studies concentrated on two-
dimensional finite element numerical models, and just a few studies approached
the three-dimensional finite element numerical models. From the three-
dimensional finite element models one can observe that most of them are
concerned with either double-lap bolted joints or single-lap bolted joints modified
such that the bending caused by the eccentric loading path is not included in the

analysis.

Previous studies contained experimental data from resistance strain gages
applied on the surface of the composite plate. This approach does not allow
measurements very close to the bolt hole, nor on the bearing plane of the
specimen. One study included resistance strain gages inside an isotropic
specimen with fairly good results. Using resistance strain gages inside a laminate
composite plate would not be desirable because it could alter the mechanical

properties of the composite plate in a significant manner.

13

Since “traditional applications” of laminate composite materials have
mostly been concentrated in the aerospace and electronics related fields,
composite plates generally have low thickness value. The importance of such
applications led researchers into studying thin composite plates. But, as
omposite engineering evolves and more and more fields require the balance
between strength and weight that the laminate composites offer, more
investigations are necessary to characterize the behavior of thicker, more

complex composite materials.

This research studied a single-lap bolted joint between a thick laminate
composite plate and an aluminum plate. The bolted joint was modeled
numerically using finite element analysis and it included the fastening parts:
washers, nut and bolt. The numerical results were then compared with
experimental data coming from fiber-optic strain gages (FoSG) embedded in the
thick composite plate. Since most of the damage supported by the laminate is
bearing damage, as shown in Figure 1.2, this analysis concentrated on
measurements in the bearing plane of the laminate composite plate. The position

and magnitude of the stress and strains in the specimen were reported.

The finite element analysis provides a complete three-dimensional map of
stresses and strains. The experimental data obtained through the thickness of

the composite plate provides valuable information from within the specimen. The

14

investigations were done on glass reinforced epoxy plates. Future studies will be

concentrated on very thick sandwich composite materials.

The methods used in this research were chosen based on some very
important factors. The finite element analysis is able to provide three-
dimensional data map that is practically impossible to obtain with a reasonable
number of sensors. Finite element analysis proves to be a very inexpensive tool
in the study of fiber reinforced composite materials. With all the advantages of
the finite element method, the numerical model has to be first tested so that
accuracy of results can be evaluated. Improvements to the model are then
possible so that the numerical model can be used with confidence to obtain

qualitative as well as quantitative results.

Fiber-optic strain gages were chosen for their miniscule dimensions
without jeopardizing accuracy. These sensors can be embedded in the specimen
at the time of fabrication and they do not significantly affect the material
properties of the thick composite laminate plate. The data stream coming from
the sensors can be used at any given time for validation purposes, as well as for

health monitoring of the composite joint during its service life.

From here on, this thesis is structured as follows: Chapter 3 deals with

experimental setup, specimen characteristics and composite material property

15

validation. Chapter 4 presents the main points of the finite element model and
will present reasons why certain settings were chosen. Chapter 5 gives an
overview of the results obtained and results comparison. Chapter 6 provides
conclusions drawn from this study. Chapter 7 focuses on possible error causes

and suggestions.

The most challenging part of the finite element analysis is modeling the
contact involved in the bolted joint. This task proves to have a large influence on
the numerical results and it needs to be carefully addressed. Another crucial
factor is correct determination of the clamping force for bolted joints. Also,
material properties have to be correctly determined, such that the input
parameters of the finite element model are in accordance with the experiment.
The details on the modeling of the contact surfaces is included in Chapter 4.
Details about the determination of the clamping load and material properties

calibration, as well as the studied load cases, are covered in Chapter 3.

16

Chapter 3

EXPERIMENTAL ANALYSIS

Experimental analysis for this research is a means of validating the finite
element analysis that gives valuable insight into the strain and stress

distributions in thick laminate composite plates in single-lap bolted joints.

The method of choice for experimental investigations was using fiber-optic
strain gages. The fiber-optic sensors were used to measure strains inside the
composite plate, in the bearing plane. These readings were not sufficient for the
finite element analysis and other experiments were done to gather the necessary
data for input into the finite element model. Material properties and clamping

force were important parameters that needed to be accurately determined.
Experimental investigations for material properties validation and some of

the bolted joint experiments were done in collaboration with Xu Ding and

Gaetano Restivo, as part of the comprehensive research program.

17

3.1 FIBER-OPTIC STRAIN GAGES

A brief outlook over the theory behind fiber-optic sensors, with accent on
the fiber-optic strain sensors, is necessary for understanding the use and

usefulness of these new-generation sensors.

What is a sensor? A sensor is any a device which converts a physical
property of interest into a different form of energy which can be transmitted,
processed and correlated to the physical property. In our case, the sensor is a
Fabry-Perot cavity and the form of energy that transmits the signal is an optical

signal.

The medium that carries the signal to and from the sensor is the optical
fiber. The optical fiber is made of a very thin silica core surrounded by a silica
cladding that has a lower refractive index than the core. The obtained effect is
that the light is guided through the core from the source to the other end of the
optical fiber as it can be seen in Figure 3.1. The core and the cladding are then
protected by a silicon coating followed by buffer jacket, strength members and
outer polyurethane jacket. These protection coatings can differ depending on the

application.

18

Glass Cladding Glass Core

 

 

Figure 3.1 Light paths through generic optical fiber.

The Fabry—Perot sensor consists of two partially reflective mirrors
separated by a cavity. In the intrinsic form, the mirrors are fabricated within the
fiber, thus the cavity is actually the fiber itself. In the extrinsic version of the
Fabry-Perot sensors, as shown in Figure 3.2, the two mirrors are separated by an
air gap. The light traveling through the fiber is partially reflected back by the first
mirror. The remaining light enters the cavity and is reflected back and forth
between the mirrors. Interference occurs between the light beams resulting in a

phase shift due to the additional optical path.

19

Fabry-Perot Cavity

Micro-capillary Tube I Optical Fiber

Partially Reflective Mirrors

Gage Length

 

 

 

Figure 3.2 Typical Fabry-Perot strain sensor.

The interrogator, patented by Bellville and Duplain (1993; 1995) is based

on a white-light Fizeau interferometer shown in Figure 3.3.

 

Lens Wedge
Fabry-Perot

 

Coupler -2”

-:_—-§ (— ”T": CCD sensor

 

 

 

 

4.
White Light

 

 

Interrogator

 

Figure 3.3 Typical Extrinsic Fabry-Perot Deployment.

The light from a broadband source is sent along one of the fiber branches.

It arrives in the coupler where it is transmitted along the fiber branch bearing

20

the sensor. The light is bounced by the two mirrors and reflected back to the
signal conditioner. The modulated light is then passed through a cylindrical lens
and then projected on a wedge. The wedge acts a cross-correlator with the
position of the light on the wedge as a function of the cavity length. The light
corresponding to 0' pm of cavity length will be projected on the wedge at the
point where the wedge thickness is 0’ pm. Cross-correlation is obtained
instantaneously by passing the light through the glass wedge. The light then falls
on a linear CCD array for which each pixel corresponds to a specific correlated

cavity length (1993).

Pixel Pixel

 

 

 

 

 

 

 

 

Lens Wedge Unstrained Strained

Figure 3.4 Cross correlation using Fizeau interferometer.

Some of the advantages fiber-optic sensors offer are: small size, easy

embedment, low transverse load sensitivity, small gage length, EMI/RFI

21

interference immunity, ability to implement in hostile environments without

fearing corrosion and mechanical strength, to name a few.

For the purpose of this research, fiber-optic sensors brought a novel
approach for the characterization of strain fields inside the laminate material. As
mentioned before, most of the research done in this field used surface mounted
resistance strain gages to validate numerical models. By embedding even
miniscule foil gages into laminate specimens, the material properties of the

laminate would most likely suffer alterations that affect the experiment.

All fiber-optic strain gages used in this research are non-compensated
type gages having a 2mm gage length as manufactured by FISO Technologies.
The outer diameter of the strain gage is 230pm. Schematics of the fiber-optic

gage used in this research is shown in Figure 3.5.

22

.....
‘~
~
‘~

 

 
  
    

~- ~~~~~~~~~~~~ 4 3mm + 1. 0mm """""""""
___________________ ‘nl—‘ I jfi—i . '!
Ii‘g;.gtgt‘t :vag‘

‘ fi‘sg

 
  

v
a t s. 3%.!
I%g§_"¥;‘-£ “In ‘1» '

     

   

figure 3.5 Fiber-optic strain gage (FOSG) glued to the E-glass weave with

schematics of the FOSG.

23

3.2 MATERIAL PROPERTIES VALIDATION

The objective of this part of the research work was validation of two
important mechanical properties of the laminate composite material used in the
single-lap bolted joint structure. Also, by comparing the measured results of
strain obtained from resistance strain gages and fiber-optic strain sensors, the

efficiency of the fiber-optic sensors can be evaluated.

To be consistent with proceeding research work, Epoxies, Etc... 20-3302
epoxy resin and E-glass fiber weave were used. Epoxies, Etc... 20-3302 is a two-
component, ultra-clear, epoxy system designed for LED. (Light Emitting Diode)
encapsulation, fiber optics, and any potting or adhesive application requiring

optimum clarity. Material properties are shown in Table 3.1.

 

E-glass fiber E(PSI) 10.5e6 v 0.22

 

Epoxy E(PSI) 0.5e6 v 0.37

 

 

 

 

 

 

 

Table 3.1 E-glass and epoxy resin properties

In order to obtain the desired thickness of 0.5in, 60 plies of E—glass weave
were used for each specimen. The plain weave had 18warp/in and 18fill/in fiber

counts.

24

3.2.1 Volume Fraction Determination

Volume fraction. determination was needed to determine the macro-
mechanical material properties of the composite plate. Since macro-mechanical
properties were to be used in the finite element analysis, an accurate

determination was necessary.

Volume fraction calculations were performed on one of the first specimens
used in this research study. The same materials were used for all specimens
included in the study thus the change in volume fraction, from one specimen to
another, was considered to be negligible. Dimensions of the specimen used for
determining the volume fraction are 4.35inx3.91inx0.5in (Length x Width x

Height). The specimen had 60 plies of plain weave style 3733.

The volume of the plate can be expressed in terms of the volumes
occupied by the fiber and the matrix. The void content of the plate is assumed to

be negligible at this time.

vplate = v fiber + Vmatrix 3'1

Dividing the above equation by the plate volume , we obtain the volume

fraction relationship:

25

V v .
__ fiber matnx _
1 — V + V — Vfiber + Vmatrix 32

plate plate

The plate volume was calculated based on the plate dimensions and it

was found to be vp/m: 8.50in.

The weight of the plain weave was recorded for a stack of 60 plies and it
was found to be 4.46602. The density of E-glass fiber is 0.093 lbm/in3 (1998).
Thus, the volume occupied by the fibers is Vp/ate‘=3.00in3. Dividing the volume
occupied by the fibers by the total volume of the plate, the volume fraction of

the specimen is VfibeF0.35.

3.2.2 Experimental Validation of Material Properties

The finite element model can use layered elements to represent the
stacking of E-glass fibers and epoxy. Then it can use a homogenization scheme
to calculate the effective material properties for the laminate plate. This step was
avoided due to heavy calculation volume. It is also an error-prone scheme due to
the fact that fiber lay-up is not a pure [0/90]s because of undulations of the

woven fibers.

26

Material properties were then acquired from a model by Dasgupta et al.
(1996). This model accounted for the undulations in the weave and it provided
the necessary data to determine homogenized mechanical properties of the
laminate as a whole. The determined orthotropic material properties were then
included into the finite element numerical model. Material properties of the

laminate are shown in Table 3.2.

 

 

Ex E, El ny G,..=(i,,z
Component ny sz=Vyz
(psi) (psi) (psi) (96') (Psi)
Composite
2.46e6 2.46e6 4.78e5 0.38 0.14 4.2e5 2.72e5
plate

 

 

 

 

 

 

 

 

 

 

Table 3.2 Composite laminate material properties.

The advantages of using orthotropic material properties for the finite
element numerical models are not insignificant. Calculation time is greatly
reduced because of the use of lower order elements having a lower number of
degrees of freedom (DOFs). Convergence problems are also avoided due to the

simplified model.

After the determination of the material properties of the laminate,
validation of the material properties was necessary to prove the accuracy of the

determinations and to provide a solid base for the numerical model. For

27

validation, a specimen having the same lay-up scheme and volume fraction was

used in a tensile test.

For the tensile test, a combination of Micro-Measurements EA-13-12012-
120 0-90° resistance strain gage rosettes and FISO fiber-optic strain gages was
used. By using both methods, the conventional and well known resistance strain
gages and the new generation of sensors, the fiber-optic strain sensors, a

validation of the fiber-optic sensors was possible.

Two fiber-optic sensors were attached to the 30m E-glass layer prior to
specimen fabrication. Attachment of the sensors to the weave is necessary in
order to preserve the sensor’s position during fabrication. Sensor repositioning
would be impossible after the epoxy cures. Two small blobs of Devcon Aluminum
Liquid (F-2) metal-filled epoxy secured the naked fiber to the weave. The metal
filled epoxy would be an advantage for X-ray localization of multiple fiber-optic

strain gages.

A sample attachment of a fiber optic sensor to the E-glass weave can be
seen in Figure 3.6. The portion of the fiber where the strain gage is located is
not glued at this point. During fabrication the epoxy secures the sensor within

two consecutive layers of E-glass weave.

28

“Heat shrinkf
A’ tubing

E-glass
plain weave

Metal-filled

epoxy

Fiber-optic
outer jacket

r

e
.0
fl
m
.m

t

p
O

 

Figure 3.6 Sample attachment of fiber-optic strain gages to E-glass weave.

A microscopic view of a fiber-optic strain gage attachment point is shown

in Figure 3.7.

29

‘ I

0 25 mm

 

Figure 3.7 Optical fiber attachment point.

The two 0-90° resistance strain gage rosettes were attached to opposite
faces of the specimen. The rosettes provided valuable data for avoiding bending
during testing and material properties validation. The tensile test specimen, as

shown in Figure 3.8, was 10in long, 2.25in wide and 0.5in thick.

 

‘—_ 10in >

2 R86 axial\ / FOSG transverse 0.5in

_./ tel: ‘/ 5f},
F [d’ 7 2.25in
T

To 5i?

Figure 3.8 Tensile test specimen and strain gage layout.

 

 

 

30

The tensile test specimen was set up in the load frame as seen in Figure
3.9. The RSGs were connected to Measurements Group P—3500 Strain Indicator
setups in half-bridge configuration with temperature compensation gages
mounted on an unloaded specimen. The FISO fiber-optic strain gages were
connected to an 8-channel FISO UMI-8 signal conditioner that provided a data

stream to a portable laptop computer.

 

Figure 3.9 Tensile test loading setup and data acquisition equipment.

To minimize any effect of bending caused by misalignment of loading
fixture, the loading setup was adjusted until matching readings were obtained

from the two RSG rosettes within 10% variation. The tensile specimen was

31

loaded from 0 to 200 lbs. Readings were taken at 5 minutes after each loading.

Strain readings are shown in Table 3.3.

 

 

 

 

 

 

 

 

 

Axial RSG Transverse RSG Axial FOS Transverse FOS
Load(Lb) She-s05!)

(W3) (us) (He) (#8)
25 21.7 8 -2 8 -O.5
50 43.4 17 -3 16 -1.5
75 65.2 25 -4 24 -2.5
100 86.94 34 -5 33.5 -3
125 108.6 42 -7 41.5 -4
150 130.4 52 -8 51 5.5
175 152.1 60.5 -9 59 -6
200 173.9 70 -10 68.5 -6.5

 

 

 

 

 

 

 

 

Table 3.3 Readings from the RSG rosettes and fiber-optic strain gages.

In parallel with the experiment, a finite element model numerical analysis
was performed. The numerical model of the tensile specimen with analytically
calculated material properties was simulated under the same load conditions as
in the experiment. A comparison between the finite element numerical results,
results from the fiber-optic strain gages and from RSG rosettes is shown in

figure 3.10.

32

 

 

 

Tensile Test Results

 

 

 

  
 
 
 
    

 

 

 

 

 

80

70 «~ +Axial Strain RSG
+Axial Strain FOS

60 -- ‘ Axial Strain Numerical
—+(—-Tran5\erse Strain RSG

50 ~~-—« +Transuarse Strain FOS
+Transwrse Strain Numerical

 

 

 

 

 

 

 

 

 

Strain (microstrain)
8

 

 

 

 

.{9 .9 .{o o ,{9 .3? ((0 '90

Load (LB)

 

 

 

Figure 3.10 Tensile test result comparison.

Numerical results, resistance strain gage results and fiber-optic strain
gage results show very good agreement for the longitudinal strains. Good
agreement between numerical results and resistance strain gage results is shown
for the transverse strains, with some discrepancies for the fiber-optic results. A
possible reason for the difference in results is the very low value of strain for the
transverse direction and the resolution difference for the two experimental

techniques. The Measurements Group P-3500 Strain Indicator has a resolution of

33

1 pa and the F150 UMI-8 has a resolution of 0.5 pg. Error sources are addressed

in more detail in Chapter 7.

Table 3.4 shows a comparison between the analytical and experimental

determinations of the Poisson ratio VI; and the elastic modulus along the

 

 

 

direction of the fibers.
Analytical RSG result FOSG result
E1 (e6 PSI) 2.466 2.47 2.62
V]; 0.14 0.15 0.11

 

 

 

 

 

 

Table 3.4 Material properties validation.

Overall the results show generally a good agreement that prove that the
material properties used in the finite element numerical model are accurate.
Also, the fiber-optic strain gages proved to be a solid and efficient tool in

studying composite laminates strain fields.

34

3.3 CLAMPING FORCE DETERMINATION

A torque wrench was used to apply a preset torque on the bolt head. This
torque has to be converted to clamping force. The clamping force is one of the
most important parameters in this study and represents the force exerted by the
bolt on the two plates that form the bolted joint, holding them together. This
parameter has to be introduced into the finite element model and its value

greatly influences the analysis.

In the “Standard handbook of fastening and joining” (1989) the following

formula is given:

T=K-D-P 3.3

where T=installation torque (lb-in)
K=torque coefficient
D=nominal bolt diameter (in)

P=clamping load (lb)

In the formula above the only variable is the torque coefficient. This
coefficient varies with a multitude of parameters including finishes, wear,
lubricant coatings, etc. The variation of the torque coefficient can only be

35

determined experimentally. For some of the standard fasteners statistic analysis
was used to determine the range in which the torque coefficient is most likely to

fall.

For the purpose of this research, accurate determination of the clamping
load was performed by using Transducer Techniques THC-lK-T 1000lb thru-the-
hole type load cell transducer, as shown in Figure 3.11. The transducer is used in
combination with a Hewlett-Packard 6200B DC power supply and a Hewlett-

Packard 3468A multi-meter.

 

...L... .

Figure 3.11 Load cell transducer.

The load cell calibration was checked using shunt resistors, and calibration
data was compared against the manufacturer's supplied calibration sheet. The
comparison between the two calibration curves is shown in Figure 3.12. The

measured difference between the calibration values was less than +/-0.3%.

36

 

 

 

 

 

 

 

 

 

 

 

 

——_—7‘ TT . . T'T f—l
Transducer Calibration
0.025
0.02 --— +FactoryCalibration (V) /
+Readi s
2 0.015 . "g M __
3
5 0.01 T-——-- - - -—
0.005
0 / r j
0 463.83 927.66
Load (LB)

 

 

 

Figure 3.12 Transducer calibration.

A series of forty successive load-unload cycles were performed with a
0.5in shoulder bolt used in the analysis. The torque applied by means of a torque
wrench was set to be 25lb-in. Although the torque wrench was set to a specific
value, the converted clamping force was not the same for two or more
consecutive tightenings. Torque wrench release timing and wear of the nut and

bolt threads are just two of the factors greatly influencing the results.

A few tests were done concerning the clamping load. The transducer was
mounted on a similar specimen using the same nut and bolt as used in the
single-lap joint. The bolt was tightened using the torque wrench and the
clamping load values were read after a five minute interval. After the reading the

bolt was released and then a new tightening was performed with the same

37

parameters. Forty such cycles were done for each test. A sample result is shown

in figure 3.13.

 

 

{_,__ ,_ _ __ _ ._.____

Clamping Force

 

 

i 180.0 1— - - - » --
k 160.0 « ~
140.0 «

120.0

100.0
80.0
60.0

l 40.0

\ 20.0

l

l

|

+ Clam ping force

 
   

 

 

 

 

— Linear (Clamping force)

 

 

 

 

 

 

Load (LB)

 

 

 

 

0.0 I T Tj— TTT—T T'TT TT IIIIII T I T T T I F I I - I I fiT’T I T 1
1 3 5 7 9111315171921232527293133353739
Load-unloadcycies

l
L r
u

 

 

Figure 3.13 Clamping force variation for successive 25lb-in bolt torque

applications.

This development led to modifications in the way the experiment was run.
A longer bolt was used to allow mounting of the load cell transducer directly on
the bolted joint. This change provided the means to read the clamping force in a
direct manner during the load-up sequence. A special configuration was
necessary to ensure that the bolted joint configuration would not be influenced

by the addition of the transducer.

38

Experiments performed with the modified setup to accommodate the
transducer showed a pattern in clamping force variation or relaxation. The
relaxation was attributed, in principal, to the soft nature of the composite matrix.
Readouts from two experiments are shown in

Figure 3.14. The experiments were conducted in such manner as to allow
sufficient time for material relaxation between two consecutive experiments. Two

very important conclusions were drawn:

° Initial clamping load varies at the same torque setting;

° Clamping force relaxes over the duration of the experiment.

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

Clamping Load Relaxation
180.0 -,..-__,__.________-___ ._
160.0
A 140.0
m
3 120.0
8
3 100.0
E 80.0 .. _
Q
g 60.0 i e_*
a . §+Sample 1 .
400 +— H -« —--—— ni+Sample2F —
20.0
0.0 —~—-———:— ------ T - ~ T -. , ,
5 10 15 20 25 30 35
Time (min)

 

 

 

Figure 3.14 Clamping force relaxation.

39

3.4 EXPERIMENTAL ANALYSIS

As stated in the Research Objectives, one of the goals of this research
study was to obtain through-the-thickness strain measurements that would
validate the finite element analysis. In turn, the finite element model, validated
by experimental data, delivers the locations of the maximum shear stress and of

the possible failure of the composite plate.

The supporting plate was made of aluminum 2024-T4 with the following material
properties:
E = 1.01e7 psi

v = 0.34

The aluminum plate used in the investigations was 8inx4inx0.5in (Length

x Width x Height).

Fiber-optic strain gages were embedded in the composite specimens at
the time of fabrication. The detailed process and guidelines for fabricating such

specimens can be found in Appendix 1.

Experiments performed in this study used specimens that incorporated
different numbers of fiber-optic strain gages. One of the first specimens

40

contained only one fiber-optic strain gage and it was built to assess whether or
not fiber-optic strain gages can deliver results from an area that has very high
strain gradient. Another reason was to make an initial qualitative assessment of
the experimental data coming from a composite plate used in a bolted joint. The
initial assessment validated the use of fiber-optic strain gages placed close to the
bolt hole. Since the results obtained from the specimen having only one fiber-

optic strain gage were only qualitative, they were not presented in this thesis.

The next step was molding specimens that had more measurement points
so that the strains in the bearing plane of the composite plates can be compared
with the finite element models. The decision made was to use three fiber-optic
strain gages embedded in the bearing plane of each composite plates at safe
distances from the bolt hole and the surfaces. All specimens in this first batch
had three embedded fiber-optic strain gages and will be named Type 1
Specimens from now on. One of the fiber-optic strain gages attached to the E-
glass weave is shown in Figure 3.15a. The approximate position of the sensors is
shown in Figure 3.15b and the specific location and strain gage identification are

shown in figure 3.15c.

Problems experienced during experiments performed with the Type 1
specimens included strain gage damage during hole drilling or manufacturing,

precise strain gage positioning and optical fiber shear at the exit point from the

41

specimen. All these issues were fixed for the specimen used in the final stage of

the research.

 

 

 

 

    

 

 

.E —'
‘ OI _ \ BOIt
‘T
‘ Hole
5% I K A
N
ositions B
P C .

 

 

(a) (b) (C)
Figure 3.15 Type 1 Specimens: (a) Fiber-optic strain gage attached to the E-
glass weave; (b) schematics of the sensor locations; (c) sensor locations and

identification.

The dimensions of the Type 1 specimens are shown in Figure 3.16. As is
can be observed, the specimens were 5in long. This created problems because of
the insufficient space to route the optical fiber coming out of the specimens. A
lower corner radius had to be used for the fiber, creating unnecessary stress on
the fiber at the specimen interface. The additional stress lead to fiber rupture in

a few cases.

42

 

 

 

1.5in

 

5in

 

 

 

 

2 Y: 05in ——JL
4in '—> *—

 

 

 

 

 

Figure 3.16 Specimen dimensions for the Type 1 specimens.

The composite specimen used in the final stage of this research study was
8inx4inx0.5in (Length x Width x Height). This specimen will be referred to as

Type 2 specimen. Material properties for the composite plate were identical as

the first batch specimens and were presented in subchapter 3.2. Detailed

dimensions of both aluminum and composite plates are show in Figure 3.17.

43

 

 

 

 

 

 

 

 

2
.E
N- G 0.5 in
.JL_ . .- -_ E
1.5 in _
4 r
. __L
3 l" 0.5 In

 

 

 

 

 

 

Figure 3.17 Dimensions for the aluminum plate and Type Zspecimen.

The experience gained with the Type 1 specimens proved to be very
useful when new specimens were fabricated. Precise location of the fiber-optic
strain gages is very important and special techniques were used to improve
sensor positioning such that hole drilling did not affect the sensors. Details about
sensor positioning are found in Appendix 1. Protection measures were added to
ensure the integrity of the optical fiber at the specimen interface. Shrink wrap
tubing was added to the vulnerable part of the optical fiber for protection. One

such installation was shown in Figure 3.6.

The locations of the five sensors embedded in the specimen are shown in

Figure 3.18.

 

 

 

 

 

 

 

 

 

2 in 0.1in
C
33.
OJ! Q 0.5in
“xi-.5—
H .—.-
e . .
A .5
0. Hill
H I ’1 I I I 0.1in

 

 

 

 

 

 

 

 

 

0.1in

 

 

 

Figure 3.18 Fiber-optic strain gage locations in the Type Zspecimen.

The bolted joint was subjected to axial load on a loading frame as shown
in Figure 3.19 and Figure 3.20. The axial loading was performed by adding dead
weights on the loading hanger. The loading frame has a mechanical advantage
factor of 5. For each pound of deadweight on the loading hanger, a load of 5lb is
exerted on the bolted joint. The bolted joint equipped with the transducer and in

loading position is shown in Figure 3.20.

45

A/ Main lever

 

( Loading

Aluminum

plate / Weights

Composite

plate .
/ Loading frame

 

Figure 3.19 Loading frame schematics.

 

Figure 3.20 Bolted joint with transducer — loading frame position.

A comparison and discussion of the results obtained from experiments

performed with both Type I and Type Zspecimens are presented in Chapter 5.

46

Chapter 4

FINITE ELEMENT MODELS

Finite Element Analysis (FEA) is one powerful tool that researchers are
using with success to solve complex problems. Mathematical models are used to
represent real-life phenomena and results obtained by solving the models
represent approximate solutions to the given problem. FEA is used in numerous
fields of research such as chemistry, electro—magnetics, fluid mechanics, solid

mechanics, forming, crashworthiness, composite structures, and so on.

With the advance in computing performance, FEA becomes more and
more important to the extent that it sometimes replaces expensive experiments.
FEA is not recommended to be used as a whole means of obtaining results as it

is, as previously stated, an approximation of the real life phenomena.

This research project combines experiments and Finite Element Analysis.
The interaction between the two fields is mandatory for better understanding of
localized phenomena and for validating results. As shown in Figure 4.1, finite

Element Analysis was used in close connection with the experiments. Feedback

47

from both methods provided enhancements and revealed possible causes of
errors. The Finite Element Model was improved numerous times to better
approximate the experiment conditions. In return, the Finite Element Analysis

dictated improvements to the experiments including fiber-optic strain gage

 

 

 

 

 

 

 

 

 

 

 

positioning.
Initial Conditions
Assumptions \
[ FEA ] Feedback Experiment ]
\ Results ] /

 

 

Figure 4.1 Validation scheme.

48

4.1 FINITE ELEMENT MODEL DESCRIPTION

Finite Element Analysis is a three step process. First a finite element
model has to be built and load conditions applied. Second, the model is solved
using one of the available algorithms. And finally, the third step is the processing

and interpretation of the results.

During this research the software used for FEA simulations were ANSYS
v9.0 — implicit finite element commercial code, and LS-DYNA V970 Rev5434 —
explicit/implicit finite element commercial code. ANSYS is an all-in-one finite
element software. It has built-in modeling capabilities, a powerful set of solvers
that can handle diverse problems, and it also includes a built-in post-processor
for result evaluation and interpretation. ANSYS can solve a wide range of
problems including thermal, electro-magnetic, static (linear and non-linear),
vibration, optimization and, with the LS-DYNA add-on module, dynamic
problems. LS-DYNA is a very capable finite element code that can solve multi-
physics problems including solid mechanics, crashworthiness, fluid dynamics,

metal forming, heat transfer and others.

Both ANSYS and LS-DYNA were used in this research study. Initially, the
FEA was performed exclusively in ANSYS. As the study matured, the need to
implement special bolted joint characteristics, such as bolt-to-hole clearance, led

49

to the FE model migration from ANSYS to LS-DYNA. The reasons behind the
migration are discussed further in this chapter. Both finite element models are

discussed in detail.

4.1.1 ANSYS Finite Element Models

Initially, for this project, non-linear static analysis was required. Only
implicit code was used due to the static nature of the problem. For dynamic
calculations that take into account clearance and other complex factors, the
model had to be migrated to use explicit code that can handle rigid body motion

and large displacements.

One of the first models created was the tensile specimen used in
validating the material properties and testing the fiber-optic strain gages.
Material properties, once validated, were used in the bolted joint finite element

model.

All models used SOLID45 three-dimensional structural solid elements. The

tensile specimen was modeled using 750 SOLID45 elements of different

dimensions. Coarse mesh was used at the ends of the coupon and finer mesh

50

was used in the center, where the area of interest was. Five elements were used

for the thickness.

The boundary conditions were equivalent to the ones used in the
experiment. The nodes on one end face were fixed and on the opposite end face
nodal loads were applied. The model and the applied boundary conditions are

shown in Figure 4.2.

 

Figure 4.2 Tensile specimen model with applied boundary conditions.

Sample results obtained using the finite element model for the tensile

specimen can be seen in Figure 4.3.

A comparison between finite Element Analysis, fiber-optic strain gages and

resistance strain gages was presented in Chapter 3.

51

 

 

 

L-fi’l‘f‘FIE ” W‘ 'T:*“' .
.2718-04' .3503~04 .4298-04
.3113-04 .3908-04 .4698-04

AN

 

 

 

 

 

   

 

 

   

 

~.878E-05 -. 6822-05 -.486E-OS -.290£-05 -.946£—06
- . 7BOE-OS - . SB‘lZ-OS - . 38811-05 - . 1933-05 . 3273-07

Figure 4.3 Longitudinal (top) and transverse (bottom) strains for 50lb load
anammg.

With preliminary determinations finished the finite element model of the

bolted joint was prepared.

52

The bolted joint was modeled using SOLID45 8-node elements. Special
attention was dedicated to the meshing process. This step is very important

because of significant impact it has over calculations.

Since the bolted joint has a plane of symmetry, the model created was
half of the bolted joint. Symmetry boundary conditions were used on the

symmetry plane. A typical mesh is shown in Figure 4.4.

 

 

 

 

 

Figure 4.4 Meshed bolted joint.

53

One of the most important advantages of working with only half the
model is the reduction in the number of elements. This leads to a direct
reduction of the number of equations which translates into greatly reduced
computational time. The model can be expanded symmetrically to represent a
full-shape model. A symmetry expansion of the half-model is presented in Figure

4.5.

 

 

 

 

 

Figure 4.5 Symmetry expansion mesh.

54

Each plate was split into separate volumes for easier and more accurate
meshing. The split-volume technique helped in reducing and eliminating shape-
violating elements. Another fact worth mentioning is meshing the high strain
gradient regions with smaller elements and lower gradient regions with larger
size elements. This led to a better distribution of the number of elements and not
only reduced the size of the model but provided good indication of contact issues
arising from mesh generation gaps and penetrations. A close-up view of the

mesh around the hole is shown in Figure 4.6.

 

 

 

 

 

Figure 4.6 Close-up view of selected elements around the bolt hole.

55

To reduce the number of contact surfaces included in the model, and for
simplification reasons, the bolt, nuts and washers were all modeled as a single
volume. The bolt, nut and washer assembly is shown in Figure 4.7. The bolt hole
diameter has the same value as the bolt shank to simulate a snug fit. This was

also important because of contact convergence constraints.

 

 

 

 

 

 

Figure 4.7 Bolt, washer and nut assembly.

Since the finite element model is used to simulate both pin connection and
bolt connection, pretension had to be introduced. There are multiple ways to

simulate bolt pretension using finite element models. Most common methods

56

are: thermally induced pretension, washer/nut pressure and pretension by
special elements. The latter uses specially designed elements that achieve the
desired pretension by creating a virtual section within the bolt shank. The virtual
section splits the bolt in two and then it brings them together using the desired
clamping force value. The pretension effects needed to be calculated in the first
loading step of the simulation. No other external loads were introduced during
this step to ensure model convergence and accuracy. Once the displacement
map was calculated it was used as initial condition for the next loading step. The

subsequent loading steps were used to apply load on the bolted joint.

The pretension section is meshed using special elements. In ANSYS the

pretension elements are PRETSl79. The location of the section cut (pretension

mesh) was specified as a fixed value on the bolt shank.

A simplified scheme on how the pretension was achieved using PREl’Sl79

elements is shown in Figure 4.8.

57

  
 

Pretenslon Load

Figure 4.8 Bolt pretension scheme.

ANSYS introduces a new way of modeling contact by laying the contact
elements on top of the solid mesh. The contact elements used were selected
based on the three-dimensional characteristics of the model and also based on
the nature of surfaces coming in contact. Elements having surface-to-surface
capabilities were used to model the contact surfaces. In ANSYS, contact surfaces
are designated as Target and Contact surfaces. This is analogous to the
master/slave scheme. Target surfaces are the equivalent of slave surfaces and
contact surfaces are equivalent to master surfaces. Each target and contact

surface coming in contact forms a contact pair. All contact pairs were modeled as

58

flexible-to-flexible contact pairs. Contact surfaces for the expanded model are

shown in Figure 4.9.

 

 

 

 

 

Figure 4.9 Contact surfaces (element shrinkage used for better visualization).

59

° Contact pairs were formed as follows:
° Washer to plate (2 pairs)
° Bolt to hole (2 pairs)

° Plate to plate (2 pairs)

Some clarifications are necessary for the number of contact pairs. Contact
between each washer and the small cylindrical volume under the washer is
modeled as one contact pair. The bolt surface and the hole of each plate
constitute one contact pair. Because of the split volume nature of the model,
there are two pairs of surfaces coming into contact between the two plates, thus

forming two contact pairs.

Elements used to model the contact surfaces are CONTA174. These
elements are three-dimensional, have 8 nodes, and are used for surface-to-
surface contacts. The target surfaces were meshed using TARGE170. These
elements are three-dimensional and take the number of nodes of the element

upon which they are laid .

The contact method of choice was the Augmented Lagrange Method. This
method is basically the same as the Penalty method with enhanced penetration
control. The reason behind the choice was the better conditioning and decreased

computation time of the method, capability to handle large displacements and

60

the handling of contact surfaces coming in and out of contact. The behavior of
the contact pair was set to standard. The option to automatically close gaps and
reduce penetration was enabled. The option to exclude initial penetration was

enabled.

Fiction coefficients were assigned separately for each contact pair. The
friction coefficient for steel-aluminum contact was set to 0.3. The friction
coefficient for both aluminum and steel with the composite plate was set to 0.48.
The influence of friction coefficients on the FEA results is discussed in Chapter 7.
Contact surface status was checked before each simulation to reveal gaps or
penetrations. ANSYS can automatically offset surfaces so they come in contact if

the gap in a contact pair is reasonably low.

The boundary conditions applied to the finite element model simulated in
detail the experimental conditions. The composite plate was fixed to the free
end. Symmetry conditions were applied for all parts on the symmetry plane.
Clamping force was simulated as pretension in a separate loading step. The
aluminum plate had all nodes from the free surface coupled to simplify load
application and to avoid unwanted edge deformation. A master node was
assigned and a single force was applied to it. Multiple load steps were necessary

to obtain the necessary results to match the experimental loading conditions.

61

The final finite element model incorporated 4723 elements and it is shown

with applied boundary conditions in Figure 4.10.

 

 

 

 

 

Figure 4.10 Finite element model of the bolted joint with boundary conditions

andload.

Results and discussion on the results obtained with the ANSYS finite

element model are presented in the next chapter.

62

4.1.2 LS-DYNA Finite Element Models

LS-DYNA was used as a useful tool to bridge the gap between the
limitations of the ANSYS models and the real-life situations. LS-DYNA handled
problems where ANSYS could not converge due to implicit code limitations.
Change in surface contact status (on/off) and bolt-to-hole clearance were just
two very important real-life situations that could not be implemented using
ANSYS alone. The ANSYS models were migrated to LS-DYNA and rigid body
motion, change in contact status and clearance were handled without additional
spring elements, very soft materials or other improvisations. The mesh was
exported from ANSYS using the ANSYS/LS-DYNA module. With the mesh in
place, the models were then imported in Altair HyperMesh v7.0 modeler where

contact, boundary conditions, loads and all other necessary LS-DYNA “keywords

(commands) were introduced.

Two cases were modeled in LS-DYNA. The first model simulated a pin
connection. This case was simulated because the only load present was the load
applied to the joint. This step was necessary to avoid any possible problems

caused by the clamping force.

63

1.5-D YIVA Pin Connection Model

The pin connection model consisted of three parts: the aluminum plate,
the composite plate and the pin. All parts were modeled using SOLID elements.
SOLID elements were required because of the three-dimensional nature of the
problem. SHELL elements would not have sufficed because they cannot
accurately simulate the contact between the plates and the pin. The LS-DYNA pin

connection model is shown in Figure 4.11.

   

AZ/
y x
Figure 4.11 LS-DYNA pin connection model.

The pin connection model had 5138 nodes in 4020 elements. All elements
were considered deformable, including the pin. Material properties for the

aluminum plate and the pin were defined using *MAT_ELASTIC card. Because

64

during the experiments the loads used were not causing any plastic deformation
to the joint components, plasticity was not considered. The composite plate was

modeled using *MAT_ORTHOTROPIC_ELASTIC card.

The mesh was refined for both plates in the area around the bolt hole.
The pin mesh was adapted to the hole mesh such that there were equal
numbers of elements for the hole and the circumference of the bolt. This was

important to minimize node-to-element penetrations during the contact.

Contact between the two plates and between the two plates and the bolt
was simulated. The contact option used for the model was chosen based on the
nature of the contact. *CONTACT_SURFACE_TO_SURFACE_ID was preferred.
This way, contact surfaces were defined using SEl‘_SEGMENT and then pairs
were formed to create the full contact definition. Three contact pairs were

created as follows:

° aluminum plate to composite plate,
° pin to composite plate,

° pin to aluminum plate.

All contact pairs were governed by the master-slave principle. The

surfaces belonging to the stiffer material were considered master contact

65

surfaces. The friction coefficient for steel-aluminum contact was set to 0.3. The
friction coefficient for both aluminum and steel with the composite plate was set

to 0.48. This was consistent with the ANSYS model.
Since there were no rigid elements present, all parts were considered
deformable and a more accurate representation of the physical interactions

present in the bolted joint was obtained.

A close-up view of the region around the pin is shown in Figure 4.12.

 

X

Figure 4.12 LS-DYNA pin connection model: close-up view.

Bolt-to-hole clearance was set for both the aluminum and the composite
plates. Diametric bolt-to-hole clearance values were set to 0.01in for the

aluminum plate and 0.005in for the composite plate. The clearance values were

66

selected for reasons explained in Chapter 5. No clearance was modeled for the
contact between the two plates. The initial penetration check option was
activated in the contact definitions to verify that no nodes or elements were

penetrating the opposing contact surface.

Boundary conditions were defined using three node sets. The node sets

were useful because they simplified the load definitions in the LS-DYNA input file.

The far end of the composite plate was set to have zero translation for all
three axes. Rotation was permitted around any axis, similar to the experiment

conditions.

A half model approach was used to take advantage of the symmetry plane
present in the pin connection model. Symmetry boundary conditions were
applied to all nodes in the symmetry plane. The load was applied to the far end
of the aluminum plate by means of a load curve with predefined points for
specific load values, similar to the experiment loading conditions. No additional
loads were applied. Except for the mentioned nodal constraints and symmetry

conditions, no other nodal constraints were present.

67

1.5-D YNA Bolted Joint Model

The second LS-DYNA model was used to simulate the bolted joint case.
The model was created in a similar manner as the pin connection model. The

differences and similarities between the two models are explained below.

The bolted joint was modeled using 4496 nodes in 3290 elements. All
elements were SOLID type similar to the pin connection model. Material

properties were the same as for the pin connection case.

The bolt, washers and nut representing the bolt assembly were modeled
as a single part, to minimize the number of contact surfaces and processing

time.

In addition to the three contact pairs present in the pin connection model,
two more contact pairs were needed to account for the two washer-plate
interactions. These surfaces were modeled similar to the existing three pairs,
using the *CONTACT_SURFACE_TO_SURFACE_ID contact card. The LS-DYNA

bolted joint model is shown in Figure 4.13.

68

 

Figure 4.13 LS-DYNA bolted joint model.

The bolt pretension was obtained using a newly introduced option in LS-
DYNA 970 Rev 5434. This option defines an initial stress section in a selected
part set. The initial stress section acts in a similar manner as the ANSYS
pretension mesh. A part set is defined and it can contain one or more parts. The
part set is virtually separated with a plane defined in
*DATABASE_CROSS_SECI’ION_PLANE card. The two portions of the part set will
then be forced to come together and in this way the pretension is obtained. A
stress curve with zero origin and the desired maximum value needs to be applied
to the part set. When the end of the stress curve is reached, the pretension

initialization stops and the joint load can be applied.

69

 

Figure 4.14 LS-DYNA bolted joint model: close—up view.

The initial stress section option is similar to the ANSYS pretension mesh
but it differs in the way the pretension value is defined. The ANSYS pretension is
achieved by specifying a load value whereas the LS-DYNA pretension is achieved
by specifying a desired stress value. Since the experimental values for pretension
are in terms of clamping force, a transformation from force to stress is necessary

to achieve a similar result.

A full model of the bolted joint created by symmetry expansion is shown

in Figure 4.15.

70

 

Figure 4.15 LS-DYNA bolted joint model: symmetry expansion.

The boundary conditions for the bolted joint were set similarly to the ones
defined for the pin connection model. The far end of the composite plate was
constrained for translation along all axes and free to rotate. Symmetry boundary
conditions were applied to the nodes in the symmetry plane and the axial load is
applied using a load curve. The load curve was set so that it was zero until the

pretension stage ended.

71

Chapter 5

RESULTS COMPARISON AND DISCUSSION

Results from experiments and Finite Element Analysis are compared in
this chapter. Results for the pin connection and the bolted joint are presented.

Results are presented separately for Type 1 and Type Zspecimens.

5.1 RESUL TS FOR TYPE 1 SPECIMENS

Type I specimens provided useful data in the first stages of this research.
Experiments conducted with these specimens recorded data for positions A, B
and C, as shown in Figure 3.15. No pin connection data was compiled for Type 1
specimens. The optical fibers of the embedded sensors in Type 1 specimens
were damaged during various stages of the experiments and data was available
only for the 25lb-in bolt torque. Fiber-optic sensors were not reset after the
torque was applied. A comparison between finite element results and

experimental results for the 25lb—in bolt torque is shown in Figure 5.1.

72

 

25 lb-in Bolt Torque

0 25 50 75 100 125 150

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

.E .
g 33.20
9 8
g E40 ‘
3 €60 V:
450 —I-—A-EXP —-t-B-EXP —O-C-EXP
100 —n-A-FEA —A—B-FEA -0-C-FEA
Load (LB)

 

 

Figure 5.1 Results comparison for Type I specimens: a,“ (25lb-in bolt torque) -
one sample experiment.

The results for the Type 1 specimens show a fairly good correlation for
strain gages in positions A and C. The strain gage in position B showed a fairly
large discrepancy compared with the finite element results. Also, experimental
data showed a slightly different trend than was obtained with finite elements.
Multiple experiments were performed and initial strain scatter appeared after the
bolt torque was applied. The differing trends and the initial strain scatter were
caused by visco-elastic effects in the composite plate matrix. These effects were

mentioned in subchapter 3.3 Clamping Force Determination.

73

A strain map of the axial strain (8,“) obtained from FEA is shown in Figure
5.2. The maximum compression strain occurs at the initial contact point which is
on the edge of the hole. The ANSYS model does not have any bolt-to-hole

clearance, but clearance is actually present in the experiment.

    
     

Maximum tension

 

Maximum
compression

 

 

 

z

v\1//
x

Figure 5.2 Type 1 specimens: sxx strain map for 150lb load and 25 lb-in

bolt torque.

A full size strain map of the axial strain (exx) at 150lb load is shown in
Figure 5.3. The full size map was created by symmetry model expansion within
the ANSYS post processor. The advantage of the full symmetry expansion is that
it creates a full picture of the strains sustained by the object. A half size model is
also useful because, in our case, it shows the strain distribution in the bearing

plane.

74

Maximum
compression

 

Figure 5.3 Type 1 specimens: symmetry expansion of the sxx strain map for

150lb load and 25lb-in bolt torque.

A shear stress map of the ox, shear stress at 150lb load is shown in Figure
5.4. The maximum shear stress aw in the composite plate provides indication on
where initial delamination will first occur if the specimen is overloaded. The
failure is likely to develop at an angle of approximately 45° from the x-direction.

This is a very important factor in safety calculations for such joints.

75

    
    

Positive Shear
Stress

Negative Shear
Stress
Figure 5.4 Type 1 specimens: Shear stress 0,, at 150lb load and 25lb-in bolt

torque.

The von Mises stress distribution in the bolt assembly reveals a maximum
stress occurring on the composite plate side of the built-in washer, as shown in
Figure 5.5. This is expected as the bolt tilts under the load. The maximum von
Mises stress on the composite plate occurs on the side of the bolt hole in the

area with maximum tensile strain.

76

  
 

 

Max. von Mises
Stress

 

 

 

Figure 5.5 Type 1 specimens: von Mises stress map in the fastener at 150lb load

and 25lb-in bolt torque.

A complete strain map of the bolted joint for Type 1 specimens showing

the axial strain at 150lb load and 25Ib-in bolt torque is shown in Figure 5.6.

composite

   
    
 

aluminum

Y \Z:
x
Figure 5.6 exx strain map of the bolted joint for 150lb load and 25lb—in bolt

torque.

77

5.2 RESUL 129 FOR THE TYPE 2 SPECIMEN

Experiments with the Type 2 specimen, although the same in nature as
the experiments with Type 1 specimens, followed different procedures. These
procedures were implemented out of the need to overcome problems related to
clamping force relaxation, creep, and strain scattering. These procedures were
improved as more experiments were performed. The procedures included the
use of a conical spring washer to compensate for the clamping force relaxation,
accelerated load/unload process and strain gage resetting. All finite element

results for the Type Zspecimens were extracted using LS-DYNA.

In order to eliminate undesired effects of the strain components created
by the clamping force, the results for the pin connection experiments and LS-
DYNA pin connection model were compared. The schematics and the labels of
the equivalent positions of the fiber-optic strain gages in the finite element
model are shown in Figure 5.7. The locations and labels are valid for the pin

connection case as well as the 25lb-in bolt torque case.

78

X

 

Figure 5.7 Equivalent positions of the fiber-optic sensors for Type Zspecimen.

A comparison between the finite element results and the experimental
data is shown in Figure 5.8. The experimental data were recorded for multiple
experiments and then averaged. The graph shows the averaged experimental

data.

79

 

 

 

 

 

 

 

 

 

 

 

 

 

 

Pin Connection
0 50 100 150 200
100 f-
O ‘ —. —— Il‘ — — — — — — —- "— — _ -°
l\:~ ,- ~~~ ~~~~

A ‘ \
.E 7100 -— -
g I \ x ‘ 7’5 ‘- —.
a 200 a s ‘ A
2 l \ 4.
o
"E -300 l \f\
V I l —o—-F085 \
.E -400 ——l —I—-—FOS1 A‘
g l ‘ —-.—Fosz \
'l’ ”—3, —o— FEMS \
x I ; —D— FEM1 \

-600 -. -—a— FEM2 W- .. _2_ -

. ——><-- FEM3
-700 l .__ 7 I . "7,2
Load (lb)

 

 

 

Figure 5.8 Results comparison for Type Zspecimen: a». for the pin connection

case.

Fiber-optic strain gage number 4 was damaged during the fabrication
process, therefore results for that particular location were not available. Since no
correlation can be made between the finite element results at the FOS#4
location and the experimental data for FOS#4, finite element results for FOS#4

were not compiled.

The experimental data and the finite element results for the pin
connection agreed reasonably well. The maximum strains present at the edge of
the composite specimen bolt hole were successfully characterized. A slightly

larger difference was observed for the other locations.

80

The maximum axial strain, in the bearing plane of the composite plate,
was recorded by FOS#1 and the value was -662 pa. The finite element model
results showed -653 pa for the same position. The difference between the

experiment and the finite element analysis is lower than 1.5%.

 
    

VJ/y
x
Figure 5.9 Pin connection: exx strain map for Type Zspecimen at 200lb load.

Axial strains of the pin connection for 200lb load are shown in Figure 5.9.
The plates were modeled as being in contact at the start of the finite element
simulation. As the load increased, the plates were forced out of contact until total

separation was achieved. This observation was consistent with experiments.

81

Another important factor that needed attention was the value of the bolt-
to—hole clearance. Initially, clearance values were set to be the same for both the
aluminum and the composite plates. This contradicted the experiments which
were showing compression strains present at the location of FOS#S. The LS-
DYNA model was modified accordingly to allow the pin to have a secondary

contact point on the composite plate.

   
    
 

aluminum

composite

Figure 5.10 Pin connection: a,“ strain map with visible secondary contact point at

200lb load.

A close-up view of the pin connection showing axial strains at 200lb load

is shown in Figure 5.10. The picture shows the two regions of contact for the

82

composite plate and the total separation of the plates under load. The aluminum
plate was found to be controlling the motion of the pin and the contact between

the pin and the composite plate.

A stand-alone view of the composite plate strain field of axial strains at
200lb load is shown in Figure 5.11. The maximum strains occur at the edge of
the plate where the pin contact patch begins. Tension strains present on the
sides of the hole are caused by the axial load being mainly supported by only

one side of the hole.

 

Figure 5.11 Pin connection: TypeZspecimen exx strain map at 200lb load.

Changes in bolt-to-hole clearance in the pin connection finite element

model were propagated to the bolted joint model.
83

Fiber-optic strain gages were reset to zero after the bolt torque
application. Undesired strains caused by visco-elastic effects were minimized this

way.

A comparison between the finite element results and the experiments is
shown in Figure 5.12. The bolted joint was loaded from 0lb to 200lb and data
from multiple experiments were averaged. The experimental results shown in the
graph are averaged results. Good validation for the maximum strain in the

bearing plane can be observed.

 

25 in-Ib Torque

 

 

 

 

 

 

 

 

 

 

 

 

0 50 100 150 200
100 . X
50 “—W—P—g -—-
1? ’ ’T
E o _ __ .2 f at —x
E '50 "L“ —x—Foss -‘\“
I? -100 -l. +FOS1\\ Eh;
v + \ 3
c 450 +— F032 ;\\ x ,
'3 —0—FOS3
. \ \ n
? -200 J—l —X_FEM5 — - x ,
" -250. —U—FEM1
—-A—FEM2 X
-300 4 —<>-FEM 3

 

 

 

Load (lb)

 

 

 

Figure 5.12 Results comparison for the Type 2 specimen: a,“ for the 25lb-in bolt

torque case.

84

The maximum strain in the bearing plane was recorded by FOS#2 and the
value was -269pe whereas the finite element analysis reported -274 pa for the
same point. The error between the finite element prediction and the experiment

was approximately 2%.

An interesting observation for the Type 2 specimen was that FOS#2
recorded higher strains than FOS#1. This was not observed with other
specimens used in past research and initial finite element models were
contradicting the experimental values. The reason for such results was assumed
to be a small bulge on the inside of the hole close to the location of FOS#2. The
pin connection case did not reveal such results and it was believed that the bulge
was caused by the clamping force. The clamping force initiated a larger
deformation amplified by either pockets of air trapped during the molding
process or a matrix-rich area in the specimen. The bulge caused a shift in
contact surface and an unexpected jump in strain for the plate regions monitored

by FOS#2 and FOS#3.

Bearing damage of composite plates in single-lap bolted joints is
commonly found on the edge of the hole. As the load increases, the bearing
damage propagates further from the edge of the hole. This is consistent with the

findings of McCarthy et al. (2002).

85

 

 

l‘r

In a normal situation, and consistent with results obtained with Type 1
specimens, the edge of the hole coincides with the first point of contact. In the
case of an unforeseen matrix-rich area, air pocket or manufacturing defect that
can create a bulge in hole wall, the bearing damage sustained by the composite
plate is expected start at the location of the first point of contact, which is
shifted. The shift may lead to different failure modes than expected. The
assumed bulge was represented in the finite element model by a reduced
regional bolt-hole clearance. The assumed bulge position and the finite element
results are shown in Figure 5.13. Corrections to the finite element model to
account for the bulge validated the assumed existence of a bulge in the hole

wall.

 

 
   

 

Aluminum

 

 

 

 

Figure 5.13 Type 2 specimen: Assumed bulge representation compared with FEA

results.

 

 

The results show a reasonably good correlation between finite element
analysis and experiments in the bearing region of the composite plate. On the
opposite side of the hole, however, FOS#S recorded very low strains during
experiments. The finite element model showed tensile strains increasing
immediately after load was applied on the joint. A possible cause would be the
lack of a secondary contact point on the region monitored by FOS #5. The
secondary contact point was missing because the bolt is constrained by the

washer and clamping force.

The axial strains in the area around the fastener are shown in Figure 5.14.

clearance is also visible as well as bending caused strains in the far-field region

of the composite plate.

87

 

    

composite

Figure 5.14 Type Zspecimen: exx strain map at 200lb load and 25lb—in bolt

torque.

A closer view of the axial strain map of the composite plate, as shown in
Figure 5.15, reveals the shifted contact point between the bolt shank and the
composite plate. There is no secondary contact point visible. Tension strains on
the side of the hole are also a bit shifted, most likely because of the change in

contact patch location.

88

 

Figure 5.15 Type Zspecimen: sxx strain map at 200lb load and 25lb—in bolt

 

torque.

89

Chapter 6

CONCLUSIONS

This study was concerned with the evaluation of strain fields in thick
composite plates used in single-lap bolted joints. The area of interest was the
bearing plane region close to the bolt hole. Both experimental and finite element
analyses were performed to better evaluate possible failure causes and three-

dimensional effects present in thick composite bolted joints.

The materials used for the two plates forming the bolted joint were
aluminum 2024-T4 and style 3733 E-glass/epoxy. The composite plate had 60
plies and 0.35 volume fraction. Macro-mechanical properties for the composite
plate were taken from the literature and validated by experiments. The validation
was performed against experimental data recorded with surface-mounted

resistance strain gages and embedded fiber-optic strain gages.

Experimental data for the pin connection and the bolted joints were

recorded by embedded fiber-optic strain gages and a through-the-hole type load

90

transducer. The fiber-optic strain gages were embedded in the bearing plane of
the composite plate for both Type 1 and Type 2 specimens. For Type 2
specimens one sensor was also placed inside the composite plate on the opposite
side of the hole from the bearing plane. The numerical analysis was performed
using both ANSYS and LS-DYNA commercially available finite element codes.
Experimentally validated material properties were used for the composite plate. A
comparison between finite element analysis and experiments was performed for
each load case and specimen type. The finite element analysis correlated
reasonably well with the experiments. Three-dimensional effects present in the

single-lap bolted joints, such as secondary bending, were accurately determined.

A fiber-optic strain gage installation method and safety procedures were

developed.

The maximum strains present in the bearing plane were experienced for
the pin connection case. This case is analogous to a loose or missing nut in the
bolted joint. In the 25-lb-in bolt torque case, the maximum recorded strains were
significantly lower compared to the pin connection case. An optimum bolt torque

value needs to be determined in future research.

91

 

Visco-elastic effects have a major influence on experimental results. Such
effects were minimized during experiments by use of conical spring washers,

torque application techniques and experiment procedures.

In the case of the pin connection the maximum strain resulting from the
finite element analysis was -653 pa while the experimental data at the same
point showed -662 us. This corresponds to less than 1.5% difference between

the finite element and the experiments.

For the 25lb-in case, the finite element analysis reported a maximum
strain of -274 pa in the bearing plane. The experimental data recorded for the
same point showed a value of -269 us. The difference between the experiments

and the finite element analysis was approximately 2%.

Type 2 specimen exhibited a different strain field in the bearing plane
than Type I specimens. The different behavior was assumed to be produced by
a localized bulge in the hole wall. Finite Element Analysis models modified
accordingly, to account for the localized bulge, successfully validated the

assumption.

For both the pin connection and the 25lb-in bolt torque cases the

maximum strains were successfully determined both experimentally and

92

numerically with the lower strains showing fairly good agreement between
experimental and numerical analysis. Further investigations are necessary to
accurately determine variable bolt-to-hole clearance effects, explore a wide
range of bolt-torque cases with optimum bolt-torque values and visco-elastic
effects. These effects are known to produce results scattering and have a

negative impact on the service life of the composite bolted joint.

93

 

Chapter 7

ERROR SOURCES

Error sources in this study are found in experimental as well as numerical

analyses. Sources of error are:

° fiber-optic strain gages,
° finite element modeling,
° composite material mechanical properties,

° friction coefficients.

7.1 FIBER-OPTIC STRAIN GAGE ERRORS

During fabrication, the fiber-optic strain gages, although small, can create
a localized matrix-rich region between the immediately adjacent plies. The visco-
elastic effects present in the matrix during loading are amplified in the matrix-
rich region thus influencing results. A matrix-rich region around an embedded

optical fiber is shown in Figure 7.1.

94

._ I _.:‘-‘ I, .(f' 1:" :4. _'»
. ,; Warp strand . 3 .

. t. .
. V, ‘ w " .4:
(£5 ' "
. . . .
" ’ 2H 1' '
. I.

J .

. .

 

Figure 7.1 Fiber optic strain gage embedded in composite plate.

7.2 FINITE ELEMENT MODELING

Finite element errors influencing results are caused by material properties
input, geometrical approximations, simplified fastener representation, friction
coefficient and bolt-to-hole clearance values. Each probable cause has an

influence on the results depending on the load case.

The simplified fastener approach, as shown in Figure 7.2, proved to be a
good representation of the bolt assembly, but it does not account for washer-to-
bolt head or washer-to—nut interactions. The impact of these interactions, along
with washer-bolt clearance effects, needs to be further evaluated.

95

 

Figure 7.2 Simplified fastener finite element model.

 

7.3 MACRO-MECHANICAL PROPERTIES

Macro-mechanical properties of the E-glass/epoxy plate were taken from
the literature and validated by experiments. The inherent errors of approximating

the composite plate macro—mechanical properties from constituent material

 

properties are therefore present.

The hand lay-up method used to fabricate the specimens creates the
possibility for air-pockets within the composite plate. The particular epoxy used
can dissipate air pockets quite efficiently. Nevertheless, some air pockets are still

present and they are visible in Figure 7.1 as dark round spots.

96

7.4 FRICTION COEFFICIENTS

The values of the friction coefficients directly influence the FEA results.
The largest surfaces coming in contact for the bolted joint and the pin
connection were the overlapped plate surfaces. The friction coefficient between
the composite and the aluminum had the biggest impact on the results. In the
case of the Type 2 specimen, a change in value from 0.45 to 0.48 in the
composite-to-aluminum and composite-to steel friction coefficient resulted in a
20% reduction in maximum strain obtained with FEA for the FOS#2 position.
Mold release, oxidation and other surface contaminants may produce wide

variations in friction coefficients.

97

 

1P“

Chapter 8

FUTURE WORK

Taking into consideration the large spectrum of variables and parameters
involved in studying single-lap single-bolt thick composite joints, more work is
needed to fully characterize the behavior of such bolted joints. The following

research directions should be considered in the future:

° Experimental and FE Analyses characterizing the use of conical spring
washers in the bolted joint,

° Implementation of Bragg grating fiber-optic strain gages for far-field
strains and structural health monitoring of such regions,

° Experimental determination of friction coefficients of composite joint
parts,

° Optimization of the bolt torque value,

° Experimental and FE Analyses of strain reduction methods such as hole
inserts,

° Experimental and FE Analyses of thicker sandwich-type composite

materials in single-lap bolted joints.

98

 

APPENDIX 1

99

APPENDIX 1

Fabrication of E-glass/Epoxy Plate with Embedded

Fiber Optic Sensors

OBJECTIVE

The objective of this research work was to analyze strains in the bearing
plane of a “thick" composite plate in a single-lap bolted joint. The sensors used
are non-compensating fiber-optic strain gages as manufactured by FISO
Technologies. These sensors were embedded in the plate at the time of
fabrication. The fabrication steps listed below can be used as guidelines for

future specimen fabrication.

STEP1

This step included the initial measurements, the manufacturing of the

mold and the cutting of the E-glass weave to the preset dimensions.

100

 

Tools and materials:

. Calculator (optional)

. Marker

. Ruler

. Melamine sheet

. Card board (cellulose based)
. Circular saw

. Staple gun or solid stapler

. Silicone sealer or tacky tape
. Pair of clamps

0 Protection glasses

. Protection breathing mask (for cutting E-glass weave and melamine)
o Scissors

. E-glass weave (for this experiment, E-glass style 3733 was used)

1. Initial measurements

The desired specimen dimensions, used in this research work, are shown
in Figure A.1. Based on these dimensions, the size of the mold was set to be
larger than the specimen. This allowed us to trim the edges in order to obtain
consistent material properties throughout the plate because edges are

particularly rich in matrix.

101

 

 

 

 

 

L 2in
r i

1

4m

 

 

 

 

|
I<

 

3 in —0.5 in

 

 

 

 

 

 

Figure A.1. Specimen dimensions.

The mold was done by cutting each side of the mold from a melamine

sheet. The dimensions of the mold components are shown in Table A.1.

Table A.1. Mold dimensions.

 

 

 

 

 

 

 

No. of Pieces Length (in) Height (in) Thickness (in)
1 10 5 3/4
1 5 2 3/4
2 10 3/4 2 3/4
1 9 5/8 4 5/8 3/4

 

 

 

 

 

After the components were cut to the preset dimensions, they were

assembled with one handed bar clamps. Then they were joined together with

staples. The small gaps at the joints were filled with tacky tape (silicone can be

102

‘m' _...__._...___- .

 

used as well). Cardboard was used for the side of the mold where the bearing

plane sensors were set to come out of the plate.

A sketch of the mold and a picture with the mold and the bar clamps can

be seen in Figure A.2 and Figure A.3, respectively.

 

 

Figure A.2. Mold shape.

103

 

Figure A3. The mold: before cutting the side channel to accommodate the side

exiting sensor.

2. Sensor position

Specimen was set to have five fiber optic sensors embedded at fabrication
time. Positioning the sensors required exact calculations so that the tip of the
sensor was not to close to the hole wall. Figure A.4 shows the position of each
fiber-optic sensor. The distance between each of the four sensors in the bearing

plane is equal to 0.1in.

104

 

  

WV?

 

 

 

 

 

 

 

 

 

 

 

 

 

 

 

. '1 Q 0.5in
.E
A .E
3 0.1in
1
”LL I 0.1in

Figure A.4. Fiber-optic sensors positions.

Shrink wrap tubing was attached to the PVC coating of the fiber-optic

sensors to protect the naked fibers that come out of the specimen.

STEP 2

Tools and materials:
. Fiber-optic sensors

. 1/16” heat-shrink tubing (or smaller diameter)

. Soldering iron or small heat gun

105

1. Attaching Shrink Wrap Tubing

The shrink wrap tubing was cut to 1 inch per segment. Each segment was
then positioned such that it was overlapping the PVC jacket. The shrink wrap
tubing was heated up by means of a soldering iron. The fiber and the shrink
wrap were rotated above the soldering iron, ensuring that there was a small gap
between the hot solder iron and the shrink wrap. Once this operation was
completed, the shrink wrap needed repositioning due to axial shrinkage to
ensure a proper placement with respect to the end of the fiber. One end of the
tubing was overlapping and squeezing the PVC jacket (about 1/3in) and the
other end had to be close enough to the tip of the sensor so that it would be
fixed in the specimen during lay-up (about 1/8"). A sensor with the shrink wrap

tubing attached to it is shown in Figure A5.

106

. .—.—\ ., . . ,7,

. - 7..-.HT-371W-IIII
\IV \~-,
.\

,fis,

Shrink wrap tubing

 

Figure A.5. Fiber optic sensor bearing shrink wrap tubing.

In order to maintain the position of the sensor during lay-up and curing
processes, the fiber-optic sensors were attached to the fiber glass cloth. Each of
the fiber-optic sensors was taped to a ruler for safety and positioning purposes.
The ruler allowed for precise positioning of the tip of the sensor and also kept

the fiber from moving.

STEP3

Tools and materials:

. Previously cut E-glass weave

. One ruler for each gage

107

0 Tape
. Erasers to hold the tip of each gage in place

0 Epoxy or aluminum filled epoxy

Two small drops of DEVCON Aluminum Liquid (F-2) were used to attach
each sensor to the fiber glass cloth. The sensors were positioned such that they
would blend between two longitudinal E-glass fiber strands, as shown in Figure

A.7 and Figure A.6.

Fiber-optic

Sensor E-glass Weave

 

Figure A.6. Sensor position on the E-glass weave.

During this step the mold was coated with successive layers of mold

release agent and let to dry as per manufacturer instructions.

108

 

Figure A.7. Sensor positioning.

STEP 4

Tools and materials:

Latex gloves or similar

Mold release agent and applicator

Epoxy and hardener

E-glass with attached sensors

Mold

Small cups to temporarily store the epoxy and the curing agent
Weigh scale

Spoon or wood tongue depressor
109

9. Foam roller

10.Tray to wet the foam roller

1. Mold Release Agent Application
The mold release agent application should follow the manufacturer
instructions closely. LOCTIT E Frekote 55-NC mold release agent was used for the

specimen. This mold release agent features a drying time of less than a minute.

The mold release was applied at room temperature by means of a small
folded E-glass cloth (any lint free cloth can be used). Three successive base
coats were applied at five minutes intervals followed by a final coat that was let

to dry for thirty minutes before the lay-up process began.

2. Epoxy and hardener mixing

Once the epoxy is mixed together with the curing agent, the pot life does
not allow a long lay-up period. It is practically impossible to lay-up all 60 layers
in the pot life. Because of this fact, multiple pairs of small pots were used to
temporarily hold epoxy and hardener separately. Pots forming a pair were
weighed to fit manufacturer recommended mixing ratio. Each pair was then

mixed as the need for more epoxy occurred during lay-up.

110

Optically clear epoxy 20-3302 as manufactured by Epoxies, Etc... was

used, to be consistent with previous research.

3. Lay-up Process
Final position of the fiber-optic sensors on the vertical axis is directly
influenced by the thickness of the plate. The number of layers was previously set
to be 60. The number of fiber-optic sensors in the bearing plane was set to four.
One sensor shared the same E-glass weave layer with the one on the opposite
side of the hole. Every 12‘“ E—glass weave layer had a sensor (two for the layer

bearing both bearing plane and opposite side sensors).

Before starting the lay-up, the surface of the mold was wet with epoxy
using the roller. Then the first layer was laid in the mold and then pressed and
wet with the roller. This procedure was repeated for each layer that did not
contain any sensors. Special care was paid for the layers having sensors attached
to them.

As a recommendation, any sensor bearing layer should have an extra
layer laid on top before wetting. This prevents accidental damage to the sensors

by pressing with the roller directly on the sensors.

111

STEP5

This step involved removing the plate from the mold, drilling the hole and

trimming the edges to the desired dimensions.

Tools and equipment:

. Flat tip screwdriver

. Special flat plate sharpened aluminum tool (explained below)
0 Ruler

. Pencfi

. Press drill

. Circular saw

. 1/4" diameter drill bit

. 15/32" diameter drill bit

. 31/64” diameter chucking reamer
. 1/2” diameter chucking reamer

. Thin blade hand saw

. Flat hand file

. Sand paper

112

Special tool

This tool is very useful for removing the mold parts that eventually stick to
the composite plate after curing. It is very simple to do from a 1/8" thick
aluminum sheet (or similar). It is bent at one end such that it forms an L-shape
and it is sharpened at the other end by filing (or similar). Approximate

dimensions for the tool used in the project are shown in Figure A.8.

2in .
8m

 

 

 

0.5 in

 

l‘

 

 

 

1/8 in

 

Figure A.8. Special tool for mold releasing.

1. Removing the plate from the mold

Parts of the mold that were sticking to the plate were removed using a
combination of flat tip screwdriver and the special tool. The special tool is sharp
enough to be inserted between the plate and the mold and then punched down

until the plate separated from the mold.

113

2. Drill hole

The position of the hole needed to be calculated first. Special attention
was devoted to ensure that any of the tools used to drill the hole would not
come closer than expected to the sensor tips. Practice on a similar material as

the specimen is recommended.

After the center of the hole was identified the plate was fixed to the
workbench so that it would not move during the drilling process. Press drill
rotational speed was set to 200rpm and small feed was used throughout the

process. These steps were followed in the order listed below:

a. Drill hole with 1/4” drill bit
b. Enlarge hole with 15/32” drill bit
c. Reaming using 31/64” chucking reamer

d. Reaming using 1/2” chucking reamer

114

 

3. Trim edges

The cardboard was easily cut after the plate cured and the integrity of the
sensors was preserved. The trimmed region is shown in Figure A.9. The other
edges needed to be cut by means of circular saw and hand saw. The hand saw
was used to precision cut the slack material close to the side exiting sensor.

Filing and sanding were done as needed for a smooth finish.

Cut-off
region

Final plate
shape

@

 

 

Figure A.9. Composite plate trimming.

115

REFERENCES

116

REFERENCES

ANSYS v8.0 Documentation - ANSYS Inc.,
Belleville, C. and G. Duplain (1993). Fabry—perot optical sensing device for
measuring a physical parameter. U. S. Patent. 5,202,939.

Belleville, C. and G. Duplain (1993). "White-light interferometric multimode fiber-
optic strain sensor." OPTICSLETTERS 18(1): 78-80.

Belleville, C. and G. Duplain (1995). Fabry—Perot optical sensing device for
measuring a physical parameter. U. 8. Patent. 5,392,117.

Camanho, P. and F. Matthews (1997). ”Stress analysis and strength prediction of
mechanically fastened joints in FRP: A review." COMPOSITES PART A-
APPLIED SCIENCE AND MANUFACTURING 28(6): 529-547.

Chawla, K. K. (1998). Commsite materials : science and engineering. New York,
Spfingen

Chen, W. H., S. S. Lee, et al. (1995). "II-Dimensional contact stress-analysis of a
composite laminate with bolted joint." Composite Structures 30(3): 287-
297.

Chutima, S. and A. P. Blackie (1996). ”Effect of pitch distance, row spacing, end
distance and bolt diameter on multi-fastened composite joints.”
Composites Part A-Applied Science And Manufacturing 27(2): 105-110.

Dasgupta, A., R. K. Agarwal, et al. (1996). "Three-dimensional modeling of
woven-fabric composites for effective thermo-mechanical and thermal
properties." COMPOSITES SCIENCE AND TECHNOLOGY 56(3): 209-
223.

Herakovich, C. T. (1998). Mechanics of fibrous composites. New York, John
Wiley & Sons, Inc.

Herrera-Franco, P. J. and G. L. Cloud (1992). "Strain-relief inserts for composite
fasteners - An experimental-study." Journal Of Comsite Materiafi 26(5):
751-768.

Hou, L. and D. S. Liu (2003). ”Size effects and thickness constraints in composite
joints.” Journal Of @mposite Materials 37(21): 1921-1938.

117

 

Iancu, F., X. Ding, et al. (2004). Three-D photoelasticity. RSG. and finite element
investigation of thick single lap bolted ioints. SEM X International
Congress & Exposition.

Ireman, T. (1998). "Three-dimensional stress analysis of bolted single-lap
composite joints." Composite Structures 43(3): 195-216.

Ireman, T., T. Ranvik, et al. (2000). "On damage development in mechanically
fastened composite laminates." Composite Structures 49(2): 151-171.

Kermanidis, T., G. Labelas, et al. (2000). Finite element modeling of damage
accumulation in bolted composite joints under incremental tensile loading. I

European Congress on Computational Methods in Applied Sciences and
mn—eemg-

Lawlor, V., M. McCarthy, et al. (2002). "Experimental study on effects of
clearance on single bolt, single shear, composite bolted joints." PLASTICS ;
RUBBER AN_D COMPOSITE_S 31(9): 405-411. I

 

McCarthy, M., V. Lawlor, et al. (2002). "Bolt-hole clearance effects and strength
criteria in single-bolt, single-lap, composite bolted joints." COMPOSITES
SCIENCE AND TECHNOLOGY 62(10-11): 1415-1431.

Parmley, R. O. (1989). Standard hadbook of fastening8: joining. New York,
McGraw-Hill Publishing Company.

Starikov, R. and J. Schon (2002). "Experimental study on fatigue resistance of
composite joints with protruding-head bolts." Composite Structures 55(1):
1.

Tong, L. (2000). "Bearing failure of composite bolted joints with non-uniform bolt-
to-washer clearance." Qommsites Part A: Applied Science and

Manufacturing 31(6): 609.

Whitney, T. J., E. V. Iarve, et al. (2004). "Singular stress fields near contact
boundaries in a composite bolted joint.” lntemational Jopmal ofgflids and
Structures 41(7): 1893.

118