FINITE ELEMENT ANALYSIS OF DEBONDED SANDWICH BEAMS UNDER
COMPRESSION
By
MANICKAM NARAYANAN
A THESIS PRESENTED TO THE GRADUATE SCHOOL OF THE UNIVERSITY OF
FLORIDA IN PARTIAL FULFILLMENT OF THE REQUIREMENTS FOR THE
DEGREE OF MASTER OF SCIENCE
UNIVERSITY OF FLORIDA
1999
ACKNOWLEDGMENTS
I would like to acknowledge the support and guidance of Dr. Bhavani Sankar, who has
been my advisor, sponsor and friend during my stay at the University of Florida. He is truly
an intelligent and kindhearted man from whom many have and will continue to learn.
I would also like to thank Mr. Juan Cruz, from NASA Langley Research Center, who has
supported this grant and has coordinated the cooperation between the University of Florida
and NASA Langley Research Center, Hampton VA.
TABLE OF CONTENTS
ACKNOW LEDGM ENTS ..............................................
A B ST R A C T . . . . . . . . . . . . . . . . . . . . . . . . . . . .
CHAPTERS
1 INTRODUCTION ...............
Literature Review ..............
M materials Systems ..............
Manufacturing Process ...........
Testing Equipment ..............
Inplane Compression Test Results .
Scope of Present Study ..........
2 FINITE ELEMENT ANALYSIS ....
Geometric Modeling ... . . .....
Finite Element Modeling .........
Loads and Boundary Conditions . .
M material M odeling . . . . . ...
Analytical Sandwich Beam Model .
Finite Element Simulation . . . ..
Riks Algorithm ................
The JIntegral .................
3 RESULTS AND DISCUSSIONS . .
Linear Buckling Analysis . . . ...
Postbuckling Analysis ...........
Energy Release Rate ............
Stress Analysis .................
Effects of Core Plasticity .........
. . . . . . . . . . . . . . . . . . 1 2
. . . . . . . . . . . . . . . . . . 1 4
. . . . . . . . . . . . . . . . . . 1 5
. . . . . . . . . . . . . . . . . . 1 7
. . . . . . . . . . . . . . . . . . 1 9
. . . . . . . . . . . . . . . . . . 2 0
. . . . . . . . . . . . . . . . . . 2 1
. . . . . . . . . . . . . . . . . . 2 3
. . . . . . . . . . . . . . . . . 2 4
. . . . . . . . . . . . . . . . . . 2 8
. . . . . . . . . . . . . . . . . . 3 2
. . . . . . . . . . . . . . . . . . 3 3
. . . . . . . . . . . . . . . . . . 3 7
page
...............................
...............................
...............................
...............................
...............................
...............................
4 CONCLUSIONS AND FUTURE WORK ................................ 49
APPENDICES
A BRIEF OVERVIEW OF ABAQUS . . . ....................... . 55
B RESULTS FROM POSTBUCKLING ANALYSES ....................... 59
LIST OF REFEREN CES .............................................. 78
BIOGRAPHICAL SKETCH ..................................... 80
iv
Abstract of Thesis Presented to the Graduate School of the University of Florida in Partial
Fulfillment of the Requirements for the Degree of Master of Science
FINITE ELEMENT ANALYSIS OF DEBONDED SANDWICH BEAMS UNDER
COMPRESSION
By
Manickam Narayanan
December 1999
Chairman: Dr. Bhavani Sankar
Major Department: Aerospace Engineering, Mechanics and Engineering Science
This thesis highlights research aimed at predicting the compressive failure of sandwich
beams with interfacial delaminations. A nonlinear finite element analysis was performed to
simulate axial compression of the debonded sandwich beams. The loaddeflection diagrams
were generated for a variety of specimens used in a previous experimental study. The energy
release rate at the crack tip was computed using the Jintegral, and plotted as a function of
the displacement and load. A detailed stress analysis was performed and the critical stresses
in the face sheet and the core were computed. Further, the core was modeled as a elastic,
perfectly plastic material and a nonlinear postbuckling analysis was performed. For this
model, loaddeflection curves, energy release rate plots and von Mises stress plots were
generated. By comparing the experimental failure load and the finite element analysis results,
the conclusions were reached and the scope of future research in this project was defined.
CHAPTER 1
INTRODUCTION
There is a renewed interest in using sandwich construction in aerospace structures mainly
driven by the possibility of reducing weight and cost. Fiber composites such as
graphite/epoxy are favored as the facesheet material because of their high stiffness and ability
to be cocured with many core materials. In the field of aerospace structural engineering,
sandwich constructions find application in wing skins and fuselage among other structures.
Debonding of the facesheet from the core is a serious problem in sandwich constructions.
This may occur during the fabrication process due to inadvertent introduction of foreign
matter at the interface or due to severe transverse loads as in foreign object impact. The
debonded sandwich panels are susceptible to buckling under inplane compressive loads,
which may lead to the propagation of the delamination, and/or core and facesheet failure.
Hence there is a need for a systematic study to understand how the core and facesheet
properties affect the compression behavior of a debonded sandwich composite.
Literature Review
There are many works concerning buckling of delaminated composite beams and plates.
These models were later extended to sandwich beams. Simitses et al. (1985) and Yin et al.
(1986) developed analytical models to study the effects of delamination on the ultimate load
capacity of beamplates. The latter paper included the postbuckling behavior as well as
2
energy release rate calculations to predict delamination growth. Chen (1993) included the
transverse shear effects on buckling, postbuckling and delamination growth in one
dimensional plates. A nonlinear solution method was developed by Kassapoglou (1988) for
buckling and postbuckling of elliptical delaminations under compressive loads. This method
employs a series solution approach in conjunction with the perturbation technique to solve
the laminated plate equations for large deflections. Experiments were performed on sandwich
panels containing delaminated facesheets (note that the delaminations were in between layers
of the facesheet; the facesheet/core interface did not contain delaminations). The nonlinear
models were able to predict the onset of delamination and failure loads in the experiments.
Minguet et al.(1987), studied the compressive failure of sandwich panels with a variety
of core materials including honeycomb core. They observed three types of failure modes 
core failure, debond and facesheet fracture. Based on the test results they developed a
nonlinear model to predict these failures using appropriate failure criteria for each failure
mode. Sleight and Wang (1995), compared various approximate numerical techniques for
predicting the buckling loads of debonded sandwich panels, and compared them with plane
finite element analysis. They concluded that 2D plane strain FE analysis is necessary in order
to predict the buckling loads accurately. Hwu and Hu (1992), extended the work of Yin et
al. (1986), for the case of debonded sandwich beams. They developed formulas for buckling
loads in terms of sandwich beam properties and debond length. Kim and Dharan (1992), used
a beam on elastic foundation model and computed the energy release rate in debonded
sandwich panels. Based on fracture mechanics they predicted critical debond lengths for crack
3
propagation. They used their model to predict failure in plasticfoam core sandwich panels.
An extensive experimental study was conducted by Kardomateas (1990), to understand the
buckling and postbuckling behavior of delaminated Kevlar/epoxy laminates. The
experimental program documented the loaddeflection diagrams, deformation shape in post
buckling and growth of delamination.
From this literature survey it is clear that a systematic study of compression behavior of
sandwich panels with debonded facesheets, especially failure in the postbuckling regime, is
overdue. Any modeling should be preceded by a testing program to understand the effects of
various parameters such as facesheet stiffness, core stiffness and core thickness, and debond
length on the buckling and postbuckling behavior. In a previous experimental study (Avery,
1998 and Avery and Sankar, 1999) compression tests were performed to understand the
effects of core and facesheet properties, and delamination length on the compression strength
of debonded sandwich composites. In the present study, an attempt is being made to use finite
element simulation of the compression tests to explain the failures observed in the
experiments. For the purpose of completeness a brief description of the experimental program
is presented in the following sections.
Materials System
The sandwich composites tested during the experimental study have two components: two
sets of facesheets to carry the majority of the load and the core material that is sandwiched
between them. The facesheet was made from Fiberite carbon fiber/epoxy plainwoven
prepregs (Product no: HMF 5322/97714AC). Some manufacturer listed properties are
shown in Table 1.1.
Table 1.1 Manufacturer's data for the graphite/epoxy facesheet material
Compressive Strength 77 ksi
Tensile Strength 97 ksi
Tensile Modulus 7.7 msi
Tensile strength (max. strain) 12, 658 gi&
Flatwise Tensile Strength 693 psi
Precured Resin Content 41.0 %
w
JL
Figure 1.1 Principal directions of the Nomex honeycomb
5
The core material used was the Nomex7 honeycomb manufactured by EuroComposites.
This material is made from an aramid fabric bonded together to form small hexagonal cells.
This structure is then coated with a phenolic resin. The honeycomb structure has orthotropic
properties and its principal directions are denoted by L, W, and t. The principal directions are
shown in Fig. 1.1. The Wdirection is in the general plane of the material and is perpendicular
to the Ldirection. The tdirection is the throughthethickness direction (perpendicular to the
plane of this paper). The core properties can be found in Avery (1998).
Manufacturing Process
The manufacturing of the sandwich composite for these tests was to simulate the actual
construction of a sandwich composite panel for an aircraft wing. The curing procedure was
designed to allow large wing sections of an aircraft to be manufactured at a reasonable cost.
Since an autoclave this size would substantially increase the cost of production, it was decided
to use only vacuum bag layups. Also, the panels were cocured to reduce the cost and time
to manufacture the specimens. That is, the facesheets and core material were bonded while
the skins were being cured. The majority of the panels manufactured for these experiments
use only the excess epoxy from the facesheets to bond to the core material. Each set of
specimens was manufactured from a flat sandwich plate. Artificial delaminations were
introduced into the specimens by inserting nonporous Teflon' strips between the prepreg and
the honeycomb. After curing, the plate was cut into individual specimens with a water
injecting, diamond coated masonry saw. Each specimen was then dried, labeled, and
measured to prepare it for testing.
6
Testing Equipment
The compression tests were performed on a 12,000 pound capacity Tinius Olsen testing
machine. The loading was controlled using a personal computer based controller. A Schaevitz
4inch stroke, Model 2000HR, Linear Variable Differential Transformer (LVDT), was used
to measure the displacement of the specimen. One of the LVDT brackets was mounted
directly above the load cell, eliminating errors from load cell deflections. The other LVDT
bracket was mounted above the loading fixture. A Sensotec 15,000 pound capacity load cell,
Model RM/767203, was used for the load measurements. The load and displacement data
were measured using data acquisition cards installed on the computer. The load, crosshead
deflection, relative time and displacement of the LVDT were recorded by the data acquisition
software.
Inplane Compression Test Results
The compression tests were conducted in a displacement controlled mode. Rectangular
sandwich specimens of length 4 inches and width 2 inches were clamped at the ends and
subjected to axial compression. The tests were stopped after substantial load reduction due
to catastrophic failure of the specimen. A sample compression test is illustrated by actual test
photographs in Fig. 1.2. Sixteen different types of specimens were used to understand the
effects of core thickness, core density, face sheet thickness and delamination length on the
compressive load carrying capacity of the sandwich beam column. Six repeat tests were
conducted for each specimen type. The experimental results are summarized in Table 1.2.
7
In Table 1.2, the facesheet thickness, core thickness, core density and delamination length
for each set of specimens are provided. The maximum load at which the specimen failed is
listed in the 6th column. The mode shape of each specimen attained during loading is given in
the last column. The facesheet thickness is expressed in terms of the number of plies in each
facesheet. The thickness of each ply is 0.0087 in. The failure load is given as load per unit
width of the specimen (lb/in).
Scope of Present Study
In this chapter, the other research that has been done on sandwich composites was
discussed and the previous experimental study was described. In the following chapter, the
various steps involved in the finite element modeling, such as the modeling of the geometry,
defining the material properties, applying the loads and boundary conditions and the finite
element simulation are described. Also, the analytical model of Hwa and Hu (1992), the
nonlinear solution strategy used for the postbuckling FE analysis and the Jintegral evaluation
are explained. In Chapter 3, the results from the linear buckling analysis is discussed. These
results are compared to the experimental results and the results from the analytical model
(Hwa and Hu, 1992). These results are found to be inadequate in explaining the failure
behavior observed in the tests. Then, the results of the postbuckling nonlinear analysis are
presented and the loaddeflection relationship, the stresses in the facesheets and the core, the
energy release rate calculations and the effect of the elastoplastic modeling of the core are
discussed. These results appear to provide a direction for future work in the study of
8
debonded sandwich beams. The conclusions from the results and discussions are summarized
in Chapter 4 and the scope of future work is discussed.
Figure 1.2 Compression test for Specimen 1: local antisymmetric buckling
I CIM,
Table 1.2. Dimensions and configuration of the sandwich beams and their failure loads in
the compression tests
Specimen Plies per Core Core Delamination Experimental Mode
Number facesheet Thickness Density Length Failure load Shape
(in.) (lb./ ft3) (in.) (lb/in)
1 1 0.250 1.8 0.5 98 LA
2 1 0.375 3.0 1.0 162 LS
3 1 0.500 3.0 1.5 164 LS
4 1 0.375 6.0 2.0 194 LS
5 3 0.375 3.0 0.5 1210 LS
6 3 0.250 6.0 1.0 497 LS
7 3 0.375 1.8 1.5 361 LS
8 3 0.500 3.0 2.0 439 LS
9 5 0.375 3.0 0.5 2528 GS
10 5 0.500 1.8 1.0 1215 GA
11 5 0.375 6.0 1.5 1385 GA
12 5 0.250 3.0 2.0 893 GS
13 7 0.500 6.0 0.5 4528 FF
14 7 0.375 3.0 1.0 2319 GA
15 7 0.250 3.0 1.5 1688 GS
16 7 0.375 1.8 2.0 1583 GA
LA: Local Antisymmetric, LS: Local Symmetric, GS: Global
symmetric, FF: Facesheet material failure
Symmetric, GA: Global Anti
CHAPTER 2
FINITE ELEMENT ANALYSIS
The finite element analysis was used to (a) estimate the linear buckling loads and mode
shapes of the delaminated sandwich beams and (b) simulate the actual compression tests by
performing a nonlinear postbuckling analysis of the sandwich beam under axial compression.
As will be seen later the results from the linear buckling analysis are needed for the post
buckling analysis also. The postbuckling analysis simulated the compression tests (Avery,
1998) as closely as possible.
The FE analysis was performed using the FE package ABAQUSTM. First, a geometric
model of the specimen was created using the FE preprocessor MSC/PATRANC. This was
converted to a finite element model by meshing the surfaces of the geometric model to create
nodes and elements. In the next stage, the material properties of the structural components
of the specimen were defined. This was followed by specifying the loads and boundary
constraints that would simulate the conditions of an actual compression test. Finally, the
input file was generated with this information and the analysis was performed using
ABAQUS. A brief introduction to the ABAQUS finite element package is presented in
Appendix A. The various stages of the FE analysis are discussed in detail in this chapter.
11
Geometric Modeling
This stage of the FE analysis involved the creation of a geometric model that would
represent the shape and dimensions of the test specimen (Fig. 2.1). The sandwich composite
specimen was 4 inches long and 2 inches wide. The thickness of the specimen was dependent
on the number of facesheet plies and the height of the core. Each facesheet ply was 0.0087
inches thick. The core was of three different thicknesses: 0.25, 0.375 or 5.0 inches. The
delamination was of four different lengths: 0.5, 1.0, 1.5 or 2.0 inches. The complete
dimensions of each design set are listed in Table 1.2 in Chapterl. The geometry and the finite
element model were created using the preprocessing software, MSC/PATRANC. The
sandwich composite specimen was modeled as a 2D or plane solid.
SCore
Facesheet
Figure 2.1 Sandwich composite specimen approximated as a 2D or plane solid model
First, points were created using the spatial coordinates that defined the outer boundary
of the 2D rectangular solid (in Fig. 2.1) and these points were then joined by curves. Next,
surfaces were created using these curves as the surface boundaries. Finally, three 2D solids
were created using these surfaces two of these solids representing the top and bottom face
sheets and the other solid forming the central NomexTM core. As mentioned earlier, the
12
honeycomb core was modeled as a continuum with equivalent mechanical properties. The
delamination is created in the FE modeling stage and will be discussed in the following
section.
Finite Element Modeling
The development of the FE model involved meshing of the surfaces of the geometric
model and resulted in the creation of approximately 800 isoparametric elements with 2500
nodes. Eightnode, biquadratic, plane strain elements were used to mesh the model. The
*ELEMENT command and the *NODE command in ABAQUS were used to create the
elements and nodes. The detailed set of commands and procedures used in the finite element
modeling are described in Appendix A.
After meshing the surfaces, duplicate nodes were removed using the "equivalence"
command in PATRAN. To create the delamination at the interface between the top facesheet
and the core, the nodes on the crack were excluded during the equivalence process. This
omission of the nodes along the crack creates a free edge at the interface simulating the
behavior of an interfacial delamination. The number of nodes thus excluded depended on the
length of the delamination in the specimen. The mesh in the vicinity of the cracktips were
modeled differently from the rest of the geometry to create a mesh fine enough to capture the
cracktip singularities. Bimaterial fracture mechanics studies (Zak and Williams, 1963, Rice,
1988, Hutchinson, 1990) have indicated that the stresses in the vicinity of an interfacial crack
tip at the interface between dissimilar materials are singular and vary as
U ~r (2.1)
13
where r is the distance from the cracktip of points where the stresses are calculated and ais
the bimaterial parameter (Dundurs, 1969) that depends on the elastic constants of the face
sheet and core
Figure 2.2 Finite element mesh in the vicinity of the cracktip
materials. FE modeling of such bimaterial interfacial crack problems has been studied by
several researchers, e.g., Charalambides,1990. These studies have suggested that a self
focusing mesh as shown in Fig 2.2 is very efficient in capturing the aforementioned singular
behavior at the cracktip.
I'
I
N: 
2 __________________
N
/ A'
',
,~rX ~ >
xx
L
14
Loads and Boundary Conditions
The compression testing of the sandwich composite specimen involved the loading of the
specimen in the axial direction under displacement control (Avery, 1998). The fixture used
in the test is shown in Fig. 2.3. To simulate the compressive loading under displacement
control, a multipoint constraint was created at one end of the sandwich beam. This multi
point constraint established a linear relationship between 'u' degreeoffreedom of one of the
nodes on the loading end of the beam (Fig. 2.3) and those of the remaining nodes at the same
end. A unit displacement in the axial direction was imposed on this node. This displacement
will be distributed among the remaining nodes appropriately so as to produce a constant
displacement at all the nodes on the loading face. This is accomplished by the multipoint
constraint imposed among the nodes.
Figure 2.3 Modeling of the boundary conditions of the compression test
15
Also, in the experiments the fixture acted like a clamp around the specimen for a length of
0.5" at both the ends. To simulate this in the finite element model, zerodisplacement was
imposed in the appropriate directions on the nodes along this clamped length of the beam as
shown in Fig. 2.3.
Material Modeling
The facesheet was modeled as a homogeneous linear elastic orthotropic material
throughout this study. It should be mentioned that in the tests graphite/epoxy plainweave
composite laminates were used as facesheets. This assumption is justified as the facesheet
did not undergo any delamination or other significant failure. The dominant failure
mechanisms of interest are the core failure and the interfacial fracture. The properties used
for the facesheet material are given in Table 2.1. The homogeneous properties were derived
from the data provided by the manufacturer (FiberiteTM) of the plainweave composite. The
1direction is parallel to the longitudinal beam axis and the 2direction is the thickness
direction of the sandwich beam. A state of plane strain is considered in the 12 plane, and the
beam width in the 3direction is assumed to be unity.
Although honeycomb core was used in the experimental study, it was decided to model
the core as a homogeneous continuum. This assumption is justifiable only if the characteristic
dimensions of the problem are much larger than the cell size. For example, in the current
problem the crack length is much larger than the cell size. Also, as one of the objectives was
to understand the effect of core properties on the buckling and postbuckling behavior, it was
16
decided that it was not necessary to model the microstructure of the core in detail at this
stage.
There were two core models used in the study. In the first part of the study wherein our
interest was in the energy release rate at the cracktip, the core was modeled as a linear elastic
orthotropic material. In the second part of the study our interest was in understanding the
effects of the core's elastoplastic nonlinear behavior on the postbuckling of the sandwich
beam. In that case the core was modeled as an isotropic elasticperfectly plastic material. The
two sets of properties are listed in Tables 2.1 and 2.2, respectively. The orthotropic material
properties were estimated based on the test results of Avery (1998) and the manufacturer's
(Nomex) material data. The isotropic elastoplastic material properties were chosen
arbitrarily, but representative of the core properties.
Table 2.1 Properties of facesheet and core materials used in the FE analysis. The Young's
moduli (E) and shear moduli (G) are in psi. i 's are the Poisson's ratios. The core density fi
is in lb/ft3.
Material Ell E22 E33 i 12 i 23 i31 G12 G23 G31
Facesheet 7.70E6 1.55E6 7.70E6 0.37 0.37 0.13 6.30E5 6.74E5 6.30E5
fi=1.8 336.00 181.09 15.1E3 0.01 0.01 0.01 3.9E3 3.9E3 3.9E3
C
o fi=3.0 560.00 301.82 27.1E3 0.01 0.01 0.01 7.0E3 7.0E3 7.0E3
r
e
fi=6.0 1121.0 603.64 51.0E3 0.01 0.01 0.01 13.9E3 13.9E3 13.9E3
Table 2.2 Properties of the core material as an isotropic elastic perfectly plastic material,
while the facesheet properties remain the same. Ec is the Young's modulus, 6y is the
maximum yield stress beyond which the stressstrain curve is parallel to the xaxis, and i is
the Poisson's ratio.
Analytical Sandwich Beam Model
A buckling model for delaminated sandwich composites by Hwu and Hu (1992) was
found to predict satisfactory results for specimens failing in a global buckling mode. This
model uses a combination of laminate theory and shear deformation theory. The facesheet
is assumed to be thin and carry no outofplane shear forces, while the core carries shear. The
core is also assumed to be infinitely stiff in the thickness direction, which is reasonably valid
for the Nomex honeycomb core material. Hwu and Hu (1992) presented the following
equation to predict a critical unit failure load:
[ 
P r (D + D D a + ka + a (2.2)
Lcr + 1tan 1(1 a) 2 tan 2a A3 tan 3a
where,
k 2 1 2 k 2 ( k)P (2.3)
S+ A 3 D (I P S (2.3)
2 3 2 3
Set Ec 6y i
Core EP1 1200 12 0.25
Core EP2 12000 120 0.25
Also,
A B, D,= D B 12,3 (2.4)
S(A), (B All
where A,,, B1, and D,, are the extensional stiffness, coupling stiffness and bending stiffness
of the laminated composite. The symbol a represents half the crack length. Each of the ith
terms represents a section of the composite beam, as shown in the figure below.
h" 
a
3
1 2
Figure 2.5 Delaminated sandwich model in Hwa and Hu (1992)
The equations above were solved iteratively until the critical buckling loads for various
modes were found. A FORTRAN program was written that stepped through loads until the
equations where satisfied. This model was modified from the Hwu and Hu model by adding
an inplane core stiffness. This additional stiffness slightly increased the critical loads but was
almost negligible. The results from the Hwa and Hu model were compared with the linear
19
buckling results by FEA and the experimental results. These results will be discussed in
Chapter 3.
Finite Element Simulation
As mentioned earlier the FE analysis was performed using the commercial software
ABAQUS. The analyses performed can be broadly classified into two parts: Linear buckling
analysis and nonlinear postbuckling analysis. The main purpose of the linear buckling
analyses was to understand the effects of core thickness, core density, facesheet thickness
and delamination length on the buckling loads and corresponding mode shapes. Further, as
will be explained later, the linear buckling mode shapes are required in specifying the
imperfections needed to trigger postbuckling during the nonlinear analysis. It should be
mentioned that no gap elements (contact elements) were used in between the nodes on the
delaminated surfaces. Thus interpenetration of the crack surfaces was not prevented in the FE
analysis. However it will be shown that there was no interpenetration in the first buckling
mode shapes, and hence the use of gap elements was not pursued. The results of the linear
buckling analysis are presented in Chapter 3.
The nonlinear postbuckling analysis was performed to simulate the compression tests on
the sandwich specimens. The nonlinear analysis consists of the following steps:
1. An eigenvalue buckling analysis was performed on the "perfect" model to obtain the
possible buckling modes.
2. In the second step of the analysis, an imperfection in the geometry was introduced by
adding a fraction of deflections from the eigen modes (buckling mode shapes) to the
"perfect" geometry to create a perturbed mesh. The choice of the scale factors of the
20
various modes was dependent on the facesheet thickness. Usually, 10% of the facesheet
thickness was assumed to be the scale factor for the major buckling mode. In the present
study only the first mode shape was included in the imperfection.
3. Finally, a geometrically nonlinear loaddisplacement analysis of the structure was
performed using the Riks method (Riks, 1979, Crisfield, 1981). A brief explanation of the
Riks method is presented in the next section.
During the postbuckling analyses the following quantities were computed at each load step:
(a) total load and displacement (end shortening), (b) stresses 6,x, 6y and ky in the facesheets,
(c) stresses 6,x, 6y and ky in the core and (d) Jintegral around one of the crack tips. These
results are discussed in Chapter 3. The Jintegral is a widely accepted quasistatic fracture
mechanics parameter used to study the onset of cracking for linear material response and,
with limitations, for nonlinear material response. A brief description of the Jintegral and its
relevance to the present study is presented in Section 2.8.
Riks Algorithm
The Riks algorithm is an incremental iterative solution strategy to solve geometric
nonlinear problems of buckling and postbuckling analysis. An incremental iterative approach
is based on the NewtonRaphson method of iterations. The modified NewtonRaphson
method is more accurate and minimizes computation time and hence it is preferred in
nonlinear finite element analysis. The equilibrium equations are obtained by applying the
minimum potential energy principles at each load increment. But these equilibrium equations
at the target point are algebraically equivalent to those equations that are obtained by applying
the second variation to the total potential at the known initial point of the load increment. The
21
resulting algebraic equations are solved by the Gauss elimination method to get a converged
solution for each load increment. The Newton method is good in its convergence, if the initial
solutions used for iteration are close to the solution paths. In order to obtain the approximate
initial solution, a known adjacent point is usually required. Thus the approach to solve the
problem is a process to follow the equilibrium paths step by step, starting from a known point
which is usually the unloaded state of the structure.
In general, an ideal nonlinear solution technique has to trace the entire pre and post
critical static load path of the structure under loading including the instability points.
Conventional algorithms are carried out at a constant load level, and hence at the limit points
(instability points), when the tangent stiffness matrix becomes singular, these iterations cannot
traverse them. To overcome this, Riks algorithm uses the load magnitude as an additional
unknown; it solves simultaneously for loads and displacements. Therefore another quantity
must be used to measure the progress of the solution. This quantity is the "arc length" 1, along
the static equilibrium path in loaddisplacement space. This approach provides solutions
regardless of whether the response is stable or unstable.
The JIntegral
The Jintegral is usually used in rateindependent quasistatic fracture analysis to
characterize the energy release associated with crack growth. It can be related to the stress
intensity factor if the material response is linear. The Jintegral is defined in terms of the
energy release rate associated with crack advance. In fact, it can be shown that the Jintegral
is equal to the energy release rate G in elastic materials and also in inelastic materials as long
as there is no unloading. The Jintegral is computes as
J = Uonx nu )ds i= 1,2 j= 1,2 (2.5)
F
where F is the path around which the integral is evaluated.
The Jintegral evaluations are possible at each location along the crack front. In a finite
element model each evaluation can be though of as the virtual motion of a block of material
surrounding the crack tip. Each such block is defined by contours; each contour is a ring of
elements completely surrounding the crack tip. ABAQUS automatically finds the elements
that form each ring from the node sets given as the crack tip. Each contour provides an
evaluation of the Jintegral. The command used for a Jintegral evaluation is *CONTOUR
INTEGRAL. This command and the associated procedure is discussed in Appendix A.
The Jintegral should be independent of the domain used, but Jintegral estimates from
different rings may vary because of the approximate nature of the finite element solution.
Therefore, there is a need for mesh refinement near the crack tip. Numerical tests suggest that
the estimate from the first ring of elements abutting the crack tip does not provide a high
accuracy result. Also, due to the facesheets being very thin in the specimens, later Jintegral
paths would also give erroneous results as they might traverse out of the geometry of the
specimen. In the present study, the Jintegral was computed along 20 contours around the
crack tip. The value of the energy release rate from the 7th, 8th or the 9th contour was used
in the analysis and discussions (Chapter 3) due to the above reasons.
CHAPTER 3
RESULTS AND DISCUSSION
The FE simulation of a compression test was performed on 16 models, by varying the
following parameters: facesheet thickness, core thickness, core density and delamination
length. Also, this set of 16 FE runs was repeated for three different material models of the
core (a) an orthotropic linear elastic model with properties as listed in Table 2.1 and (b) two
elastic perfectly plastic models with different values of elastic moduli and yield stress with
properties as listed in Table 2.2.
The results from these finite element analyses are discussed in the following sections. The
linear buckling analyses are presented first and compared with the experimental results and
the results from the analytical model of Hwa and Hu (1992). Next, the postbuckling
nonlinear analyses results are presented and the critical loads are compared with the
experimental failure loads. The stresses obtained from the postbuckling analyses are
tabulated and their relevance to the failure phenomena is discussed. This is followed by an
explanation of the results from the energy release rate calculations. The plastic material model
results are presented next and the effects of nonlinear elastic constitutive properties of the
core on the load carrying capacity of the sandwich beams is discussed.
24
Linear Buckling Analysis
The results of the linear buckling analysis are presented in Table 3.1. The specimen
numbers correspond to those given in Table 1.2 in Chapter 1. The properties of the face sheet
and the core, and the specimen dimensions are also given in Table 1.2. The buckling loads
presented in Table 3.1 are loads per unit width (1 inch) of the beam. The results include
buckling loads and mode shapes for the first three buckling modes. A sample mode shape for
Specimen 8 is shown in Fig.3.1. In some of the specimens penetration between the core and
the delaminated face sheet occurred, especially in second and third modes, and hence they do
not represent realistic buckling loads. This penetration behavior in Specimen 1 is shown in
Figs. 3.2 and 3.3.
The experimental failure loads are given in the last column of Table 3.1. The purpose of
the linear buckling analysis was to see if the specimens failed near the lowest buckling load.
Further, the FE results for buckling loads can be compared to those obtained from sandwich
beam models (Hwa and Hu, 1992) to see if the specimens can be modeled as sandwich beams.
A comparison of FE results for the lowest buckling loads and the corresponding
experimental failure loads in Table 3.1 lead to the following conclusions. There seems to be
no correlation between the linear buckling loads and the ultimate compressive strength as
measured by the tests. When the buckling loads are smaller, as is the case with longer
delaminations, the experimental failure load is higher than the buckling load indicating that
the beam goes under postbuckling. When the buckling loads are higher, as in beams with
shorter delmainations and/or thicker face sheets, the experimental failure load is closer to the
25
buckling load. The cases wherein the experimental failure load is lower than the buckling load,
indicate that other factors such as core failure, core instability, delamination propagation
would have played a role in the failure, and lowered the failure load below the buckling load.
In one of the beams (Specimen 13) with thick face sheets and high density core, the load
carrying capacity was limited by the facesheet failure which cannot be predicted by a linear
buckling analysis. It should be reminded that the properties of the core used are the best
estimates of the actual core properties, and further the cellular core is assumed to be a linear
elastic continuum in both the analytical and FE models.
Another interesting observation from the results in Table 3.1 is the comparison of the FE
and analytical results (Hwa and Hu, 1992) for the buckling loads. Since both models use the
same material properties, the differences can only be attributed to the applicability of
sandwich beam models to the present problem. The FE model, which uses plane solid
elements, is applicable irrespective of the core thickness or delamination length. Further the
boundary conditions can be modeled exactly in the FE analysis. Thus the results can be
thought of as an evaluation of the beam model in the present context.
The analytical and FE buckling loads have reasonable agreement when the face sheets are
thin (Specimens 14) or when the beam undergoes global buckling (short delamination,
thicker facesheets as in specimens 9 and 13). In most other cases the analytical buckling load
was greater than the FE results indicating the beam model is much stiffer, and a plane model
is required for accurate prediction of buckling loads. No comparison was made for the second
and third buckling loads as the analytical model considered only symmetric modes whereas
the FE analysis considered the full beam. Further, we did not use gap elements between the
delaminated surfaces, and interpenetration of the delaminated surfaces occurred in these
modes (see Figs. 3.2 and 3.3) invalidating the results.
Table 3.1 Buckling loads per unit width for first three modes. Analytical results are from
Hwu and Hu (1992)
Mode 1 Mode 2 Mode 3 Expt. Error % Error % of
Set Failure ofFEA Analytical
Method Method Method Method
FEA of Hwa FEA of Hwa FEA of Hwa Load compared compared to
and Hu and Hu and Hu (lb/in.) to test FEA
1 111 142 177 567 278 700 98 13 28
2 32 36 67 143 138 320 162 80 11
3 15 16 31 63 64 142 164 91 6
4 8 9 17 36 34 80 194 96 6
5 1280 2465 1631 2600 2926 2615 1210 6 93
6 712 956 1101 1480 1259 3133 497 43 34
7 304 426 540 654 582 1441 361 16 40
8 193 240 392 736 640 961 439 56 25
9 2545 2551 3422 2614 4531 2621 2528 1 0
10 1699 1928 1762 1947 2738 1948 1215 40 13
11 1389 1969 2308 2773 2551 5098 1385 0 42
12 789 1103 972 1176 1487 1743 893 12 40
13 6678 6752 8724 6919 10897 6937 4528 47 1
14 3756 2591 4012 2620 6225 2622 2319 62 31
15 2489 1728 3661 1747 3825 1748 1688 47 31
16 1647 1456 2141 1462 3133 1462 1583 4 12
Figure 3.1. First buckling mode for Specimen 8
Figure 3.2. Second buckling mode for Specimen 1
Figure 3.3. Third buckling mode for Specimen 1
28
PostBuckling Analysis
As described in Chapter 2, a geometrically nonlinear analysis of the sandwich beam was
performed using the Riks algorithm. The purpose of the analysis was to see if the
experimental failure loads correspond to the maximum loads attained in the postbuckling
analysis. Sample loaddeflection curves for Specimens 4, 5 and 9 are shown in Figs. 3.4
through 3.6. From Fig. 3.4 it can be seen that the load reaches a plateau for Specimen 4, and
this maximum load seems to correspond to the failure load. However this was not the case
for all specimens. For example in Specimen 9 (Fig. 3.5) the plateau occurs at a load of about
3,200 lb/in, but the specimen failed at 2,528 lb/in.
250
200
150
o 100
50
0 
0.00 0.01 0.02 0.03 0.04 0.05
Displacement (in.)
Figure 3.4. Postbuckling loaddisplacement curve for Specimen 4
4000
3500
3000
2500
2000
1500
1000
500
0"
0.00
0.01 0.02 0.03
0.04
Displacement (in.)
Figure 3.5. Postbuckling loaddisplacement curve for Specimen 9
2500 
2000 ...,v
1500 
1000 
500
0
0.00 0.01 0.01
0.02 0.02 0.03 0.03
Displacement (in.)
Figure 3.6. Postbuckling loaddisplacement curve for Specimen 5
30
Thus we find that the maximum postbuckling load cannot be considered as the ultimate
load in compression. Further as seen in Fig. 3.6 some specimens do not exhibit a clear plateau
at least in the range of load steps used in the analysis indicating the maximum postbuckling
load could be much higher than the experimental failure load. Thus, there are three types of
loaddeflection behavior associated with the postbuckling of the delaminated sandwich
specimens: Type 1 when the load reaches a plateau and corresponds to the experimental
failure load, Type 2, when the load reaches a plateau but does not correspond to the
experimental failure load, and Type 3 when there is no clear plateau and the postbuckling
load might be higher than the experimental failure load. The postbuckling loaddeflection
plots for all the 16 specimens used in the experimental study are presented in Appendix B.
The summary of maximum loads attained in the FE analysis are presented in Table 3.2. The
FE postbuckling loads are compared to the experimental failure load by computing the
percentage difference and it is presented in the last column of Table 3.2.
From Table 3.2 the following observation can be made. The maximum load predicted by
the FE postbuckling analysis is approximately equal to or higher than the experimental failure
load. The values are closer in specimens 4, 8, 11, 12 and 16. In these specimens the
delamination length was either 1.5 inches or 2.0 inches. That is, when the delamination length
is longer post buckling will occur relatively sooner, and the postbuckling analysis is able to
predict the load carrying capacity with reasonable accuracy. However in other specimens the
actual failure occurred earlier than the postbuckling instability indicating that some other
failure mechanisms triggered the collapse of the specimens. It should be noted that in the case
31
Table 3.2 Results of postbuckling analysis
Set Delamination Pcr by FEM Pcr by experiment Error
(in.) (lb.) (lb.) (%)
1 0.5 91.0 98.5 8
2 1 270.0 161.7 67
3 1.5 330.0 163.8 101
4 2 191.0 193.6 1
5 0.5 1182.0 1210.0 2
6 1 985.0 496.6 98
7 1.5 430.0 361.0 19
8 2 404.0 439.1 8
9 0.5 3200.0 2528.0 27
10 1 1860.0 1215.0 53
11 1.5 1406.0 1385.0 2
12 2 815.0 892.6 9
13 0.5 8100.0 4528.0 79
14 1 3637.0 2319.0 57
15 1.5 1744.0 1688.0 3
16 2 1643.0 1583.0 4
of Specimen 13, which has thickest facesheets, thickest highdensity core and short
delamination, the postbuckling load is the highest (8,100 lb/in.). However its face sheets
failed at a much lower load (4,528 lb/in.). This is because the facesheets failed in
compression even before the specimen went into the postbuckling regime.
32
In summary, the postbuckling instability alone cannot be used to predict the compression
failure of the debonded sandwich beam specimens. Before the beam goes into the post
buckling regime other failure mechanisms can initiate failure leading to catastrophic failure
of the specimen. These failure mechanisms, for example, include delamination propagation,
core failure (especially near the cracktip) and facesheet failure. These mechanisms will be
investigated in the following sections.
Energy Release Rate
From early on it was suspected that the compressive failure in a debonded sandwich beam
will occur due to delamination buckling followed by catastrophic failure due to unstable
delamination propagation. However a postmortem analysis of failed specimens indicated that
there was no or little crack propagation in most of the failed specimens. In order to check
this, the energy release rate at the crack tip was computed using the Jintegral at each load
step of the postbuckling analysis. A typical graph showing the variation of energy release rate
with the load is presented in Fig. 3.7. The energy release rate at the experimental failure load
for each specimen is given in Table 3.3.
In the same table the interfacial fracture toughness for the corresponding specimen is also
given. This fracture toughness was measured using DCB specimens in the experimental study
(Avery, 1998). The amounts of crack extension (increase in the length of delamination) are
also given in the same table. From the results it is clear that the G was considerably lower
than G, in most specimens and delamination propagation could not have been the trigger
mechanism that caused the failure.
2.0
1.5
1.0
S0.5
SAn n
0 100 200 300 400 500
Load (lb.)
Figure 3.7. Energy release rate as a function of load for Specimen 8
Stress Analysis
The stresses in the face sheet and the core were computed at each load step of the
nonlinear analysis. These stresses were compared with corresponding strength values to check
if they could have initiated the failure. Sample plots of stress distribution through the
thickness of the core are presented in Figs. 3.8 and 3.9.
The stresses in Fig. 3.8 are in the vicinity of the cracktip, whereas Fig. 3.9 shows stresses
at the center of the specimen. The maximum compressive stresses in the face sheet and the
core corresponding to the experimental failure load are presented in Table 3.3. It must be
noted that the core stresses presented in the table are values either at the midspan of the
Table 3.3. Comparison of interfacial fracture toughness G, and maximum energy release
rate Gmax, and maximum core and facesheet stresses with corresponding strength values at
experimental failure load
Interfacial fracture Core Facesheet
Delam. Crack Core Max. core Max. Face
b/.) (b/.) length extension Strength stress (psi) sheet stress
(in.) (in.) (psi) & location* (ksi)
1 1.71 0.07 0.5 0.125 2.75 2.30 (CT) 19.4
2 1.43 0.21 1.0 0.000 6.10 8.77 (CC) 17.6
3 1.22 0.08 1.5 0.000 6.10 6.50 (CC) 18.9
4 1.05 Gmax>Glc 2.0 0.125 22.9 65 (CC) 21.1
5 4.99 1.65 0.5 1.000 6.10 10.2 (CT) 63.4
6 3.31 0.05 1.0 1.000 22.9 3.9 (CT) 13.9
7 6.59 0.14 1.5 0.625 2.75 3.5 (CT) 20.0
8 4.26 1.95 2.0 0.000 6.10 32 CC) 24.6
9 7.17 0.29 0.5 0.250 6.10 4.3 (CT) 32.9
10 8.05 0.11 1.0 0.125 2.75 2.9 (CT) 55.3
11 5.25 2.12 1.5 0.250 22.9 22.5 (CC) 65.2
12 6.47 Gmax>Glc 2.0 0.000 6.10 11 (CT) 23.4
13 4.96 0.12 0.5 0.000 22.9 15 (CT) 54.1
14 7.94 0.13 1.0 0.875 6.10 6.5 (CT) 25.9
15 7.16 4.70 1.5 0.125 6.10 25 (CT) 53.3
16 10.5 1.70 2.0 0.750 2.75 7.5 (CT) 28.4
The strain energy release rate values increase rapidly when the load reaches the plateau.
* The core stresses were monitored at two locations, CT: below the cracktip; CC: center of
the beam.
Compressive strength of graphite/epoxy face sheet material is 77 ksi.
35
specimen or in the vicinity of the crack tip. The compressive strength of the graphite/epoxy
face sheet material is given as 7.7x 106 psi by the manufacturer. The core compressive strength
varied from specimen to specimen depending on the core density.
In Table 3.3, the maximum stresses developed in the face sheet are presented in the
last column. Comparing with the face sheet strength provided by the manufacturer, it is clear
that the face sheet stresses were much lower than the corresponding strength values. But the
compressive stresses in the core (Column 7) exceeded the compressive strength of the core
(Column 6) indicating that core failure could have triggered the specimen failure. To
understand the relation between core instability and the failure of the sandwich beam
specimen, it was decided that a thorough investigation of the core was necessary. In a
subsequent experimental study of the core material, it was found that the core exhibited
properties similar to an elasticperfectly plastic material as shown in the stressstrain plot in
0)
.2
El
LU
14
12
10
" 8
4
2
8
15 10 5 0
Stress (psi)
Figure 3.8. Throughthethickness 6x stress distribution in the core in the
vicinity of the cracktip (Specimen 5) for a compressive load of 1078 lb/in
36
Fig. 3.10. In the next section, the results of the inelastic constitutive modeling of the core are
presented and the effects of such a model on the load carrying capacity are discussed.
0)
.2
'a
0"
40 30 20 10
Stress (psi)
Figure 3.9. Throughthethickness 6, stress distribution in the core at the
center of the beam (Specimen 8) for a compressive load of 391 lb/in
45
30
n
0.008
0.016
0.024
Strain
Figure 3.10 Stressstrain curve for a core specimen with f = 6.0 pcf
and height = 0.25 in.
A
1 2L
8
4
E) 4
37
Effects of Core Plasticity
As discussed in the two previous sections neither the energy release rate nor the stress
field in the beam could explain the instability of the sandwich beam and provide an estimate
of the maximum load the beam can carry. Further, inspection of the failed specimens and
evaluation of G corresponding to the failure load indicated that delamination initiation was
not the trigger mechanism for failure. Hence the effects of plasticity of the core on the
instability of the beam was investigated.
In this part of the study, the core was modeled as an isotropic elasticperfectly material
using two different set of core properties, Core EP1 and Core EP2 (see Table 2.2 in Chapter
2). Sample loadend shortening diagrams for both sets of core are presented in Figs.3.11
through 3.14.
250
200
S150
100 _ 
50
5 0 _ _ _ _ __
0
0.00E+00 2.00E02 4.00E02 6.00E02 8.00E02 1.00E01
Displacement (in.)
Figure 3.11. Postbuckling loaddisplacement curve for Specimen 5 with
Core EP1
1200 
1000 
800 _ 
o 600
400
200 
0
0 _
0.OOE+00 5.00E03 1.00E02 1.50E02
Displacement (in.)
Figure 3.12. Postbuckling loaddisplacement curve for Specimen 15 with
Core EP
1000
800
600
400
0 1  
0.OOE+00 5.00E02 1.00E01 1.50E01 2.00E01 2.50E01
Displacement (in.)
Figure 3.13. Postbuckling loaddisplacement curve for Specimen 5 with
Core EP2
1400 
1200 
1000
800 
600 
400 
200 
0
0.OOE+00 2.00E03 4.00E03 6.00E03
Displacement (in.)
8.00E03 1.00E02
Figure 3.14. Postbuckling loaddisplacement curve for Specimen 15 with
Core EP2
The maximum loads before failure for different specimens are presented in Table 3.4 for
Core EP1 and in Table 3.5 for core EP2. The contour plot of von Mises stresses in the core
are presented in Figs. 3.15 and 3.16.
From the von Mises stress plots and the loaddeflection diagrams the following
conclusions can be reached. As the beam is loaded, the deboned face sheet buckles and
creates a stress concentration at the crack tip. The core material yields at these high stresses
forming a small plastic zone or yield zone around the crack tip. As the load increases the
plastic zone size also increases. When the plastic zone size reaches a critical value, the
yielding spreads thorough the entire width of the core making the specimen unstable and
causing a large drop in the load. At this stage the load carrying capacity of the beam is
40
primarily determined by the facesheet stiffness as the core becomes ineffective in carrying the
load.
From figures 3.11 through 3.14 it may be noted that there are two distinct types of failure
are possible. In the first type the load drops suddenly before the beam goes into the post
buckling regime (Figs.3.11, 3.13). In the second type there is no distinct load drop but the
beam goes into postbuckling as shown in Figs. 3.12 and 3.14. The amount of load drop is
computed as follows. The deflection corresponding to the maximum load, Fmax, is noted in
each case and this deflection is designated as af (failure deflection). Then the load
corresponding to 1.1 af is determined from the loaddeflection diagrams and this is designated
as Fmn. The factor 1.1 was arbitrarily chosen in order to maintain consistency among the load
deflection diagrams of various specimens. The load drop AF is defined as the difference
between Fmax and Fmjn. Values of Fmax, Fmn and AF for each specimen are given in Tables 3.4
and 3.5. The value of energy release rate corresponding to Fmax are also provided.
From Tables 3.4 and 3.5, it is clear that both Fmax and Fmn. are a strong function of the face
sheet thickness and the core yield strength. Further, the values of Fmn. have a stronger
correlation to the face sheet thickness, indicating that after the core yields the load carrying
capacity depends mainly on the face sheet stiffness. An inspection of energy release rate G at
Fmax show no correlation between G and the failure load. This indicates that small scale
yielding near the crack tip could not explain the instability of the specimens. Hence future
studies should focus on the size of the plastic at the point of failure and its relation to
delamination length and core thickness.
MSUPATRAN Versin 35 11Spgg 145 7:;E
Frirge: DeauiJt, Sepl .TatiTrneUJUM: Str=, CornpenIts(NDLAYER ED I) (VI
De'lrnm: De'!iALt, Step 1,Tdo arirne. o n: Dei, rradcn, Disphboanerts
I I
I I I
I 43
A.44i
.140 I
.027'3
detuit_Frirnge :
Mm 1.741 lJld 112
Mn =res7aNd 1iO4
deriut _Delbrnlion :
Mmn mUm 0ld 19T
Figure 3.15 (a) von Mises stresses in the entire beam for Specimen 10 with Core EP1 before failure
1 .741
1.Ci3S
1512
.9413
.71130
Lx
MSGPATRAN Versin 35 11Sepg 1!31: 12
Fringe: DetaiJt,G1epl ToriTrneOfl 35 : St e "ss,ConpertsNOlLAYER EED (VQMaI
De'lrnm: Deaint, St l 1.ta l irne. Jo I e: De'krrnmtlicn, Disawemrnts
12 .Il
11 24
10 .4A
9.7 13
3.199
7.42
I F 4 I LtI II . i I
I I I
4.377
3JS. 15
2S3 I.
ZJ.93
1.32
deLiJt _Frirg e :
Mm 12 .u fjNd a
Min 5C m JMd3213
deiiat Delornilion :
Mm. ,rn N Jld Iui3
Figure 3.15 (b) von Mises stresses in the entire beam for Specimen 10 with Core EP1 after failure
Lx
MSC/PATRA N Ve ricn 8.5 11Sep9 15 03:42
Fringe: DNauI, Scp ,TollTirmO.0017e5: Sircm=, Comrponirdr (1i D L.A ERED) (VO )O
Delorrn: Dea ull, S1ep 1,Tot rrime0 .00 175: Detrma bion, DpblacrnmentE
_______ Kw.K.
I I
3
I I
2.589
2243
1.798
1 353 1
' I 3aIj _F I. i.e
.l _,aLJd LD l,,:, r. ,, 1,' :
1.aX, ,.l '4 :.r I 1 i
Figure 3.16 (a) von Mises stresses in the vicinity of the left crack tip for Specimen 10 with Core EP1 at 480 lb. The
maximum load was at 529 lb.
6j606
6251 L
5 B05
5360
4.9 15
4 470
4 .024
3579
3.134
MSCPIATFRAN Version 8.5 11Sep99 1503:48
Fringeo DlcduI, ScpToIallTirTnB0.002975: Sirar CDrTponncniNJ OLAVEFRIED) (VOM JL
Delorn: Delaul, SiepF 1Tota inimne=0 0027: Delo rnalion, D pislace rnnel
10.40
9j607
9.8 12
8.0 17
72222
6.42
4 939
4j044
3249
2.454
2<.K, __________
t __________________________________________________________________________________________________
Ix 1
1 BJ6
1701
.PI3un _F..iae
Fja 11 w ,.,r, 1 1[ '
r.*. 37T .7* IJ 1:4:1
l3 ui X De. : I rrIl." :
F/3n ,,. 1 ,,r.,i 1;Hf
Figure 3.16 (b) von Mises stresses in the vicinity of the left crack tip for Specimen 10 with Core EP1 at 529 lb.
2K
MSV PATFRAN Version 8.5 11Sep99 150354
Fringe: Dcdiul1, Slp1,'ToilTirnB0.004Ee25: S9rEwc, CompFon nr (OIJ .AVEF D) (VOlWM)
Delorrn: Deiull, Siep1,Toa lTime=0.0045625: Delcrmalbin, DiEplacemeni
11 0
8.S11 1
8.0 14
72 17
6.420
5j623
1 j637 L
I 1.., ..4 r
I
I
P. I3uM i ',, E
Sx i : .. j.r.a 1j.r 1
rIii,, i .7.rjJ .:h :
A'iufl 7..I.rk3 I, n
Figure 3.16 (c) von Mises stresses in the vicinity of the left crack tip for Specimen 10 with Core EP1 at 490 lb.
, 1
IS1FCPATIRAN Version 8.5 11Sep99 1504 .00
 rings, Dciul1, SBop1,Toi lTir 0.00709g7: S9rB=, CompFon rrrle(NOtJ. .AVEF D) (VOIIM)
Delorrn: Delul, Siep 1,Toa nlTime=0.0070937: Delormalio,r DEplbacmenis
3
I 2.722
I
+
1 949
SI f
IeI3ufFi \.e
ra 1:5 ..jrjd1 I.X;'
re.,i. ,cI :;.idJ 17:0
,el3u _eI .I.cT,",i :
=,,,, 0CI;? ,T'I" 1."v,5
Figure 3.16 (d) von Mises stresses in the vicinity of the left crack tip for Specimen 10 with Core EP1 at 470 lb.
12.0M
1 1.
7.361
6 88
15K
47
Table 3.4 Maximum load and drop in load after maximum load for various specimens with
different core thickness, delamination length, and face sheet thickness. The core properties
are those of Core EP1 as listed in Table 2.2
Maximum Load at Drop in
Set hf(in.) (in.) (in.) (lb./in.) Load 1.1 af Load
(in.) (in.) (lb./in.) ( ( (
(lb.) (lb.) (lb.)
1 0.0087 0.250 0.50 .07370 73 49 24
2 0.0087 0.375 1.00 .06827 93 47 46
3 0.0087 0.500 1.50 .04640 126 45 81
4 0.0087 0.375 2.00 .01667 80 39 41
5 0.0261 0.375 0.50 .00749 216 177 39
6 0.0261 0.250 1.00 .01039 198 160 38
7 0.0261 0.375 1.50 .04860 194 190 4
8 0.0261 0.500 2.00 .05640 207 179 28
9 0.0435 0.375 0.50 .00573 584 509 75
10 0.0435 0.500 1.00 .02590 529 526 3
11 0.0435 0.375 1.50 .06460 445 442 3
12 0.0435 0.250 2.00 .06710 482 478 4
13 0.0609 0.500 0.50 .07013 1067 1062 5
14 0.0609 0.375 1.00 .03387 1165 1165 0
15 0.0609 0.250 1.50 .06900 956 956 0
16 0.0609 0.375 2.00 .04195 1175 1175 0
The load at 1.1 af, where af is the displacement at the maximum load
48
Table 3.5 Maximum load and drop in load after maximum load for various specimens with
different core thickness, delamination length, and face sheet thickness. The core properties
are those of Core EP1 as listed in Table 2.2
hf hc a Maximum Load at Drop in
Set (in.) (in.) (in.) G (lb./in.) Load (lb.) 1.1af Load (lb.)
1 0.0087 0.250 0.50 1.8460 360 154 206
2 0.0087 0.375 1.00 0.3977 419 144 275
3 0.0087 0.500 1.50 0.2491 517 190 327
4 0.0087 0.375 2.00 0.0696 413 151 262
5 0.0261 0.375 0.50 1.3850 966 485 481
6 0.0261 0.250 1.00 1.0180 628 417 211
7 0.0261 0.375 1.50 1.3780 862 352 510
8 0.0261 0.500 2.00 1.2110 1162 1146 16
9 0.0435 0.375 0.50 0.0343 2216 743 1473
10 0.0435 0.500 1.00 1.3060 1526 1089 437
11 0.0435 0.375 1.50 1.1690 1063 1014 49
12 0.0435 0.250 2.00 0.4365 794 780 14
13 0.0609 0.500 0.50 0.1854 2163 1632 531
14 0.0609 0.375 1.00 0.3191 2182 1813 369
15 0.0609 0.250 1.50 0.9628 1186 1186 0
16 0.0609 0.375 2.00 1.8280 1766 1662 104
The load at 1.1 af, where af is the displacement at the maximum load
CHAPTER 4
CONCLUSIONS AND FUTURE WORK
A finite element analysis was performed to simulate axial compression of debonded
sandwich beams. A linear buckling analysis was performed to determine the buckling loads
and corresponding mode shapes. The nonlinear analysis modeled the postbuckling behavior
of the sandwich beams. The loaddeflection diagrams were generated for a variety of
specimens used in a previous experimental study. The energy release rate at the crack tip was
computed using the Jintegral, and plotted as a function of endshortening and the load. A
detailed stress analysis was performed and the critical stresses in the face sheet and the core
were computed. Further, the core was modeled as a elasticperfectly plastic material and a
nonlinear postbuckling analysis was performed. For this model, loaddeflection curves,
energy release rate plots and von Mises stress plots were generated.
By comparing the experimental failure load and the FEA results the following conclusions
can be reached. The linear buckling analysis is inadequate in predicting the load carrying
capacity of debonded sandwich beams. The specimens go well into postbuckling regime
before failure. From the nonlinear analysis it was found that failure occurs before the
maximum load is attained in postbuckling. Thus the failure has to be initiated by the debond
propagation or stresses in the core and/or facesheets. However the energy release rate was
considerably lower than the interfacial fracture toughness thus eliminating interface failure as
50
a mechanism for the specimen failure. The stress analysis results show that the face sheet
stresses were much lower than the corresponding strength values. But the compressive
stresses in the core exceeded the compressive strength indicating that core failure could have
triggered the specimen failure.
From the results of the FE analysis of the specimens with an elasticperfectly plastic core,
it is clear that both Fmax (the maximum load) and Fmn. (the load at 1.1 af, where af is the
displacement at Fmax) are strongly dependent on the face sheet thickness and the core yield
strength. Further, the values of Fmn. have a stronger correlation to the face sheet thickness,
indicating that after the core yields the load carrying capacity depends mainly on the face
sheet stiffness. An inspection of the energy release rate G at Fmax show no correlation between
G and the failure load. This indicates that small scale yielding near the crack tip could not
explain the instability of the specimens. The von Mises stresses in the core before and after
Fmax indicate that the plastic zone size around the crack tip might have an effect on the failure
of the core. The plastic zone size needs to be quantified for the various specimens and a
relation between the plastic zone size and the failure load needs to be established. Currently
the core is being modeled as a 3D structure with each honeycomb cell being modeled as a
hexagonal solid with 6 faces (Figs. 4.1 4.3). This model will be used to understand the
elastoplastic material behavior of the core material to establish this relation between the core
instability and the failure of the sandwich specimen.
Figure 4.1 (a) Top view of the core in 2D
Figure 4.1 (a) Top view of the core in 2D
Figure 4.1 (b) Hexagonal cellular structure of the core in 2D
z
Y X
Figure 4.2: (a) Hexagonal solid structure of the honeycomb cells in the 3D FE model of core material
Figure 4.2 (b) Each cell is modeled using 6 plates and each of these plates has 4 plate elements
APPENDIX A
BRIEF OVERVIEW OF ABAQUS
A. 1 Introduction
ABAQUS is one of the leading commercial FE packages available for industrial and
academic use. The ABAQUS finite element system used in this study includes
ABAQUS/Standard, a general purpose finite element program and ABAQUS/Post, an
interactive postprocessor that provides XY plots, animations, contour plots, and tabular
output of results from ABAQUS/Standard. In order to run a finite element analysis, an input
file is required. An ABAQUS input file is an ASCII data file that can be created by using a
text editor like vi or pico. The input file consists of a series of lines containing ABAQUS
options and data. Most input files have the same basic structure. There are two maj or sections
in an ABAQUS input file the model data section and the history data section.
A.2 Model Data
After the heading, the input file usually contains a model data section to define the nodes,
elements, materials, initial conditions, etc. The following model data must be included in an
input file to define the finite element model:
Geometry: The geometry of a model is described by elements and their nodes. The
rules and methods for defining the nodes and elements are described in Section 2.3.
Crosssections for structural elements (such as beams) must be defined.
56
Material definitions: A material type must be associated with most portions of the
geometry. The materials used are described in Section 2.5.
Boundary conditions: Zerovalued boundary conditions (including symmetry
conditions) can be imposed on individual solution variables such as displacements or
rotations. The definition of boundary conditions is discussed in Section 2.4.
A.3 History Data
After the model data section, the input file contains history data to define the analysis
type, loading, output requests, etc. The STEP option divides the model data from the history
data in the input file. The following history data must be included in an input file to define an
analysis procedure:
Response type: An option to define the analysis procedure type must appear
immediately after the *STEP option. ABAQUS can perform many types of analyses 
linear or nonlinear, static or dynamic, etc. The type of analysis used in this study is
discussed in Section 2.6.
Loading: Usually some form of external loading is defined. For example, concentrated
or distributed loading can be applied, temperature changes leading to thermal
expansion can be prescribed or contact conditions can be used to apply loads. The
loading is discussed in Section 2.4.
The input file containing the model and the history data sections is then processed by the
"solver input file processor" prior to executing the appropriate solver (in this study,
ABAQUS/Standard). The functions of the solver input file processor are to interpret the
57
ABAQUS options, perform the necessary consistency checking, and prepare the data for the
solver. After the analysis is completed by ABAQUS/Standard, the results are postprocessed
using ABAQUS/Post.
A.4 Element and Node definition
The syntax for the commands to define elements and nodes are shown below:
To create an element, the following command is used:
*ELEMENT, TYPE, ELSET
The first line after the above command contains the following information:
1. Element number
2. First node number forming the element
3. Second node number forming the element
4. Etc., up to 15 node numbers
TYPE This parameter is set to equal the element type. The element type used was CPE8
which corresponds to continuum plain strain element with 8 nodes
ELSET This parameter is set to equal the element set to which these elements will be
assigned. For e.g., if the element is to be part of the core, then ELSET = CORE
To create a node, the following command was used:
*NODE, NSET
The first line after the command contains the following information:
1. Node number
2. First spatial coordinate of the node
3. Second spatial coordinate of the node
4. Third spatial coordinate of the node
NSET This parameter is set to equal the name of the node set to which these nodes will be
assigned
A5. Contour Integral
The *CONTOUR INTEGRAL output option is used to compute contour integral
estimates in fracture mechanics studies. ABAQUS automatically finds the elements that form
each ring from the node sets given as the crack tip.. Each contour provides an estimate of the
Jintegral. The number of evaluations possible is the number of such rings of elements. The
user must specify the number of contours to be used in calculating the Jintegrals by using the
CONTOURS parameter on the *CONTOUR INTEGRAL option. The TYPE parameter i
sused to select the type of contour integral to be calculated. The default is to calculate the J
integral. It should be noted that the contour integral evaluations can be performed only in two
or three dimensions and can be used only with quadrilateral elements or brick elements.
APPENDIX B
RESULTS FROM POSTBUCKLING ANALYSES
The load deflection plots from the postbuckling analysis of the debonded sandwich beam
specimens are presented in this section. First, the plots of the analyses with the core as an
elastic orthotropic material are presented. This is followed by the plots from the analyses with
the core as an elasticperfectly plastic material.
60
Figure B1. Loaddisplacement plots with the core as an elastic orthotropic material
Set 1
200
150
100
50
0 0.002 0.004 0.006 0.008 0.01
End shortening (in.)
Set 2
400
300
* 200
100
0
0 0.005 0.01
0.015 0.02
End shortening (in.)
0.025
Set 3
0 0.005 0.01 0.015 0.02 0.025 0.03
End shortening (in.)
Set 4
0.01 0.02 0.03 0.04
0.05
End shortening (in.)
400
350
300
250
200
150
100
50
0
250
200
150
100
50
0
Set 5
2500
2000
. 1500  
o 1000 
500 
5 0 0 _ __
0 ______
0 0.005 0.01 0.015 0.02 0.025 0.03
End shortening (in.)
Set 6
600
500 
400 
o 300 
6 200 
2100
j 100 ________
0
0 0.002 0.004 0.006 0.008
End shortening (in.)
Set 7
1200
1000 
. 800 ,
600 _ 
o 400 ____
S 200 
0 _ _
0 0.005 0.01 0.015 0.02
End shortening (in.)
Set 8
500
400 ...........
, 300
" 200
o 100
0
0 0.005 0.01 0.015
End shortening (in.)
Set 9
4000
3000
o 2000
o
1000
0
0.01
0.02
End shortening (in.)
Set 10
0.005
0.01
End shortening (in.)
0.03
0.04
2500
2000
1500
1000
500
0
0.015
0.02
Set 11
0.005
0.01
End shortening (in.)
Set 12
0.005
0.01
0.015
End shortening (in.)
2000
1500
1000
500
0.015
800
700
600
500
400
300
200
100
0
0.02
Set 13
10000
8000
6000
4000
2000
0
0
0
0.02 0.04
End shortening (in.)
Set 14
4000
3000
o 2000
o
1000
0
0 0.005 0.01 0.015
End shortening (in.)
0.02 0.025
i_ 1e< *
'K
0.06
Set 15
0.005
0.01
End shortening (in.)
Set 16
0 0.01 0.02
End shortening (in.)
2000
1500
1000
500
0.015
2000
1500
1000
500
0.03
Figure B2. Loaddisplacement plots with the core as an elasticperfectly plastic material
(Core EP 1)
70
Set 1
0 0.005
0.01
0.015
0.02
End shortening (in.)
Set 2
End shortening (in.)
0.025
0.03
100
0 0.005 0.01 0.015 0.02 0.025 0.03
Set 3
150
 100
o 50
0
0 0.02 0.04 0.06
End shortening (in.)
Set 4
100
S80
60 _
 40 _
20
20 _ _ ____
0 0
0 0.02 0.04 0.06 0.08
End shortening (in.)
Set 5
250 
200
8 150 
o 100 _
J
50 
0
0 0.05 0.1 0.15 0.2
End shortening (in.)
Set 6
250
200 
8 150 ______+ +
o 100 
50
0 /
0 0.002 0.004 0.006 0.008
0 0.002 0.004 0.006 0.008
End shortening (in.)
Set 7
250
200
S150 _
m 100
50
0
' 50 __
0 _
0 0.005 0.01 0.015 0.02 0.025
End shortening (in.)
Set 8
250
200
. 150 _
o 100 _'
J t
50 _
0
0 0.01 0.02 0.03 0.04 0.05 0.06
End shortening (in.)
Set 9
0 0.005 0.01 0.015 0.02
End shortening (in.)
Set 10
600
500 
.6 400 
"0 300 
o 200
j
100 
0 A,
0 0.002 0.004 0.006 0.008
End shortening (in.)
Set 11
500
400
300
200
100
0
0.000
0.005
0.010
0.015
0.020
End shortening (in.)
Set 12
600
500   , 
400 
300
200
100 ,
0
0.000 0.010 0.020 0.030 0.040 0.050 0.060
End shortening (in.)
Set 13
0.000 0.050 0.100 0.150 0.200 0.250 0.300
End shortening (in.)
Set 14
End shortening (in.)
1200
1000
800
600
400
200
0
1400
1200
1000
800
600
400
200
0
0 0.002 0.004 0.006 0.008 0.01 0.012
Set 15
1200
1000
800
600
400
200
0
0 0.005 0.01 0.015
End shortening (in.)
Set 16
1400
1200
1000
800
600
400
200
0
0 0.05
0.1 0.15 0.2 0.25
End shortening (in.)
0.02
0.3
LIST OF REFERENCES
ABAQUS/Standard User's Manual, 1998. Hibbitt, Karlsson & Sorensen, Inc. Pawtucket, RI.
Avery, J.L., and B.V. Sankar, 1999. "An Experimental Study of Postbuckling Behavior of
Debonded Sandwich Composites," J. Composite Materials (under review).
Avery, J.L., 1998. "Compressive Failure of Delaminated Sandwich Composites," Master of
Science thesis, Department of Aerospace Engineering, Mechanics & Engineering Science,
University of Florida, Gainesville, Florida.
Charalambides, P.G., H.C.Cao, J.Lund, and A.G.Evans, 1990. "Development of Test Method
for Measuring the Mixed Mode Fracture Resistance of Bimaterial Interfaces," Mechanics of
Materials, 8: 268283.
Chen, H.P., 1993. "Transverse Shear Effects on Buckling and Postbuckling of Laminated
and Delaminated Plates," AIAA Journal, 31(1):163169
Crisfield, M.A., 1981. "A Fast Incremental/Iterative Solution Procedure That Handles Snap
Through", Comput. Struct., 13: 5562.
Dundurs, J., 1969. "EdgeBonded Dissimilar Orthogonal Elastic Wedges," J. Appl. Mech. 36:
650652.
Hutchinson, J.W., 1990. "Mixed Mode Fracture Mechanics of Interfaces," MetalCeramic
Interfaces (M.Ruhle, A.G. Evans, M.F. Ashby, and J.P. Hirth, eds.), Pergamon Press, New
York, pp. 295306.
Hwu, C., and J.S. Hu., 1992. "Buckling and Postbuckling of Delaminated Composite
Sandwich Beams," AIAA Journal, 30(7): 19011909.
Kardomateas, G.A., 1990. "Postbuckling Characteristics in Delaminated Kevlar/Epoxy
Laminates: An Experimental Study." J. Composites Technology & Research, 12(2): 8590.
Kassapoglou, C., 1988. "Buckling, Postbuckling and Failure of Elliptical Delaminations in
Laminates under Compression," Composite Structures, 1 9:139159
Kim, W.C., and C.K.H. Dharan, 1992. "FaceSheet Debonding Criteria for Composite
Sandwich Panels Under InPlane Compression," Engineering Fracture Mechanics,
42(4):642652.
Minguet, P., J. Dugundji and P.A. Lagace, 1987. "Buckling and Failure of Sandwich Plates
with GraphiteEpoxy Faces and Various Cores," J. Aircraft, 25(4):372379.
Rice, J.R., 1998. "Elastic Fracture Concepts for Interfacial Cracks," J. Appl. Mech., 55: 98
103.
Riks, E., 1979. "An Incremental Approach to the Solution of Snapping and Buckling
Problems," Int. J Solids. Struct., 15: 529551.
Sankar, B.V., M.Narayanan, and J.L.Avery, 1999. "Postbuckling Behavior of Debonded
Sandwich Composite Beams Under Compression," Paper No. AIAA991295, AIAA SDM
Conference, St Louis, MO, April.
Simitses, G.J., S. Sallam and W.L. Yin, 1985. "Effect of Delamination of Axially Loaded
Homogeneous Laminated Plates," AIAA Journal, 23(9): 14371444.
Sleight, D.W., and J.T. Wang, 1995. "Buckling Analysis of Debonded Sandwich Panel Under
Compression," NASA Tech Memorandum 4701.
Yin, W.L., S.N. Sallam and G.J. Simitses, 1986. "Ultimate Axial Load Capacity of a
Delaminated BeamPlate," AIAA Journal, 24(1):123128.
Zak, A.R., and Williams, M.L., 1963. "Crack Point Singularities at a Bimaterial Interface,"
J. Appl. Mech. 30: 142143.
BIOGRAPHICAL SKETCH
I was born in the city of Madras (now known as Chennai), India, on November 2, 1973.
I was the first of two sons born to my parents who are both professors at the University of
Madras. My younger brother named Elaya Manickam has just completed his Master of
Science degree in computer applications from Anna University, Madras, and is now working
as a software developer in Madras. I have been married to Aarthi Rao since January 1999.
She is working as a software developer in Cincinnati, Ohio.
I attended schools in Madras throughout my precollege life and then I attended the Birla
Institute of Technology and Science at Pilani, India. After earning a bachelor's degree in civil
engineering and a minor in physics, I joined the National Aerospace Laboratory, Bangalore,
India, as an engineertrainee in the Structures Division. I was part of a team that was
developing an inhouse finite element analysis package. After a year at Bangalore, Ij oined the
Aerospace Engineering Department at the University of Florida for my graduate studies. After
two years of research on delaminated sandwich composites, I defended my master's thesis in
September 1999.
I am looking forward to a new phase in my life. I hope to join the engineering industry
and be successful in all my endeavors.
