A Description of the Anisotropic Material Behaviour of Short Glass Fibre Reinforced

A Description of the Anisotropic Material Behaviour of Short Glass Fibre Reinforced
Master's Degree Thesis
ISRN: BTH-AMT-EX--2006/D-01--SE
A Description of the Anisotropic
Material Behaviour of Short
Glass Fibre Reinforced
Thermoplastics Using FEA
Hamid Ghazisaeidi
Department of Mechanical Engineering
Blekinge Institute of Technology
Karlskrona, Sweden
2006
Supervisor:
Claes Hedberg, Docent, Ph.D Mech. Eng.
A Description of the Anisotropic
Material Behaviour of Short
Glass Fibre Reinforced
Thermoplastics Using FEA
Hamid Ghazisaeidi
Department of Mechanical Engineering
Blekinge Institute of Technology
Karlskrona, Sweden
2006
Thesis submitted for completion of Master of Science in Mechanical
Engineering with emphasis on Structural Mechanics at the Department of
Mechanical Engineering, Blekinge Institute of Technology, Karlskrona,
Sweden.
Abstract:
The aim of this work is to investigate and present a theoretical method to
describe the anisotropic material properties of short glass fibre
reinforced thermoplastics.
In this work, the injection moulding process simulation in SIGMASOFT
is combined with ABAQUS by a JAVA interface suggested, aiding a
micromechanical model, in order to simulate a steady state response of
short glass fibre reinforced thermoplastics under the application of a
harmonic force.
Keywords:
Anisotropic, Material properties, Injection moulding, SIGMASOFT,
ABAQUS, JAVA interface, Micromechanical model
Acknowledgements
This work was carried out at the institute of plastic processing (IKV),
RWTH-Aachen, Germany, under the supervision of Dr. Claes Hedberg
from Blekinge Institute of Technology (BTH), Prof. Dr.-Ing. Ernst
Schmachtenberg and Dipl-Ing.Tim Arping from Rheinisch Westfälische
Technische Hochschule Aachen (RWTH-Aachen).
I wish to express my sincere appreciation to Dipl-Ing. Tim Arping and for
his guidance and professional engagement throughout the work at the
institute of plastic processing (IKV) RWTH-Aachen. At the department of
mechanical engineering, Blekinge Institute of Technology (BTH), I wish to
thank Dr. Claes Hedberg for his valuable supports and suggestions.
Finally, I would like to thank Dipl-Ing. Marcel Brandt for his support
during the work.
Karlskrona, January 2006
Hamid Ghazisaeidi
2
Contents
1 Notation
6
2 Introduction, Motivation and Objectives
10
3 Theory
3.1 Short Glass Fibre Reinforced Thermoplastics
3.1.1 Classification of Composite Materials
3.1.2 Fibre Reinforced Composites
3.1.3 Thermoplastics
3.1.4 Injection Moulding (IM)
3.2 Anisotropy
3.2.1 Equations of General Anisotropic Elasticity
3.2.2 Micromechanical Model
3.3 Viscoelastic Behavior of Plastics
3.3.1 Application of Viscoelasticity to Describe the Behavior of
Plastics
3.4 Dynamic Mechanical Analysis (DMA)
3.4.1 Sinusoidal Oscillatory Test
3.5 Acoustic Analysis
3.5.1 Formulation of the Equations of Motion
3.5.2 Hamilton’s Principle
3.5.3 Lagrange’s Equations
3.5.4 Single Degree of Freedom System (SDOF)
3.5.5 Multiple Degree of Freedom System (MDOF)
3.6 Introduction to Finite Element Method (FEM)
3.7 Introduction to ABAQUS
3.8 Dynamic Response Analysis in ABAQUS
3.8.1 Step1 Natural Frequency Extraction
3.8.2 Step2 Direct Solution Steady State Harmonic Response
Analysis
3.9 Material Behavior Description
3.9.1 Frequency Domain Viscoelasticity
3.9.2 Material Damping (Rayleigh damping)
3.10 Introduction to SIGMASOFT
13
13
13
15
15
16
17
17
18
21
4 Simulations
4.1 Acoustic Simulation of a Viscoelastic Model Plate
4.1.1 Preprocessing
37
37
37
3
22
23
24
25
26
27
27
28
28
30
31
32
32
32
33
34
35
35
4.1.2 Postprocessing and Discussion
43
4.2 Acoustic Simulation of Short Glass Fibre Reinforced Model Plates
with Different Fibre Orientations
47
4.2.1 Introduction
47
4.2.2 Implementation into Software
48
4.2.3 Part Geometry in SOLIDWORKS
50
4.2.4 Injection Moulding Simulation in SIGMASOFT
51
4.2.4.1 Preprocessing
51
4.2.4.2 Postprocessing
54
4.2.4.3 Result Extraction (SIGMAlink)
60
4.2.5 JAVA Interface
60
4.2.6 Acoustic Simulation in ABAQUS
61
4.2.6.1 Preprocessing
61
4.2.6.2 Postprocessing and Discussion
63
5 Conclusion and Further Works
72
6 References
73
4
Appendices
A.
B.
C.
D.
ABAQUS input file for the polyamide model plate
ABAQUS input file for the PP GF 30 model plate 1
ABAQUS input file for the PP GF 30 model plate 2
Material Data in SIGMASOFT for the PP GF 30 model plates
5
75
80
85
90
1 Notation
A
Amplitude of the harmonic displacement
c
Damping matrix
c
Damping coefficient
cc
Critical damping coefficient
Cijkl
Elastic modulus tensor
E
Elastic modulus
Es
Storage elastic modulus
El
Loss elastic modulus
f
Frequency
F
Force matrix
F
Force
g (t )
Non-dimensional shear relaxation function
G*
Complex shear modulus
G
Shear modulus
Gs
Storage shear modulus
Gl
Loss shear modulus
G∞
Long term shear modulus
k
Stiffness matrix
k
Stiffness constant
K*
Complex bulk modulus
K
Bulk modulus
Ks
Storage bulk modulus
Kl
Loss bulk modulus
6
K∞
Long term bulk modulus
m
Mass matrix
m
Mass
t
Time
T
Kinetic Energy
T
Period
u
Displacement
u
Displacement vector
u&
Velocity vector
&&
u
Acceleration vector
U
Stiffness energy
V
Elastic strain energy
Wnc
Work done by non-conservative forces
ν
Poisson’s ratio
ω
Undamped angular natural frequency
ϖ
Damped angular natural frequency
τ
Shear stress
φ
Phase angle
φ
Eigenvector
γ
Shear strain
σ
Stress
δ
Phase lag angle
ε
Strain
ξ
Measure of reinforcement geometry
ξ
Damping factor
Φf
Fibre volume fraction
7
η
Viscosity
αR
Mass proportional Rayleigh damping factor
βR
Stiffness proportional Rayleigh damping factor
Indices
c
Composite
f
Fibre
m
Matrix
8
Abbreviations
CAE
Computer Aided Engineering
DMA
Dynamic Mechanical Analysis
DOF
Degree of Freedom
FEA
Finite Element Analysis
FEM
Finite Element Method
IM
Injection Moulding
MDOF
Multiple Degree of Freedom System
PP
Polypropylene
PP GF 30
Thirty Percent Short Glass Fibre Reinforced Polypropylene
SDOF
Single Degree of Freedom System
9
2 Introduction, Motivation and Objectives
Especially in the automotive field multitude of technical plastics parts are
used today. Since, the rising demands of the customers the technical plastic
parts have to also serve acoustic assignments, in addition to their usual
function. Designing these plastic parts already at an early stage of
development information about the acoustic behavior is needed.
Due their higher stiffness and strength short fibre reinforced thermoplastics
in contrast to unreinforced plastics may also be established for applications
that were particularly realized in metallic materials so far, e.g. applications
in automotive industry (Figure 2.1). Besides the low specific weight their
main advantage is cost-efficient large-lot production even of complex
shaped parts with high functionality by injection moulding.
[MANN+HUMMEL GmbH]
[BASF AG]
[Woco Industrietechnik GmbH]
[HEAD Deutschland GmbH]
[WILO AG]
[Robert Bosch GmbH]
Figure 2.1. Examples of complex technical injection moulded parts made of
short fibre reinforced thermoplastics.
The prediction of acoustic behavior of short fibre reinforced plastics is
supposed to be strongly dependent on the orientation of the glass fibres;
since there are major differences in the material properties in the fibre
direction and transverse to it (Figure 2.2). The orientation of the glass fibres
mainly results from the complex melt flow during filling of the mould
10
cavity. In addition to different local fibre orientation over the part fibre
orientation also varies in direction of wall thickness (Figure 2.3).
160
Stress [N/mm]
[N/mm
Stress
Stress
[N/mm2]
140
In flow direction
120
100
80
Transverse to flow direction
60
40
PA-GF 30 (dry)
Thickness: 2 mm
Temperature: 30 °C
20
0
0
1
2
3
4
Strain [%]
5
6
7
Figure 2.2. Dependency of the mechanical behaviour on fibre orientation
[10].
Orientation due to flow processes
V
Result: Anisotropic layer structure
Core layer:
⊥ to flow direction
(at frontal flow)
Edge layer:
inordinate orientation
V
Shear layer:
ll to flow direction
Figure 2.3. Development of fibre orientation due to flow processes [10].
11
The aim of the studies in this thesis is to predict the effects of anisotropic
material properties of the short glass fibre reinforced thermoplastics on the
acoustic part behavior. While doing this, the simulation of the acoustic
behavior should be improved on the knowledge of fibre orientation that is
completely dependent on the injection moulding process situations.
Regarding the acoustic FE-simulation of the plastic parts the established
characteristic values have to be placed in a precise way.
Therefore in this study, by using FEM, the effect of the fibre reinforcement
on the steady state dynamic responses of the plastic model plates under a
harmonic excitation is investigated. Plastic model plates of PP and PP GF
30 with different fibre orientations are studied.
In the first part of the work, a simple polyamide plate is designed using
SOLIDWORKS and meshed in ABAQUS (CAE), in order to study the
linear viscoelastic material modeling. Then the natural frequencies and the
steady state dynamic responses of the polyamide plate are extracted. The
aim of this part is to investigate the linear viscoelastic material model in
order to expand it to the modeling of anisotropic behavior in short glass
fibre reinforced thermoplastics.
After that in the second simulations, the acoustic behavior of a PP plate and
PP GF 30 model plates are studied for two months, where the motivation
for this work is to show that how the injection moulding process simulation
in SIGMASOFT can be combined to get the fibre orientation in order to put
them into the ABAQUS calculation finding anisotropic behavior.
12
3 Theory
3.1 Short Glass Fibre Reinforced Thermoplastics
Fibre reinforced polymer composite systems have become increasingly
important in a variety of engineering fields. The rapid growth in the use of
composite materials in structures has required the development of structure
mechanics for modelling the mechanical behaviour and the analysis of
structural elements made of composite material as laminate or sandwich
beams, plates, shells and injection moulded short glass fibre reinforced
thermoplastic [1].
3.1.1 Classification of Composite Materials
Summarizing the aspects defining a composite as a mixture of two or more
distinct constituents or phases it must be considered that all constituents
have to be present in reasonable proportions that the constituent phases
have quite different properties from the properties of the composite
material. Man-made composites are produced by combining the
constituents by various means. Figure 3.1 demonstrates typical examples of
composite materials. Composite can be classified by their form and the
distribution of their constituents (Figure 3.2). In the fibre reinforced
plastics, the arrangement and the orientation of long or short fibres
determine the mechanical properties of composites and the behavior ranges
between a general anisotropy to an isotropy. Fibre reinforced composites
are very important and in consequence this thesis work will essentially deal
with modeling and analysis of elements composed of fibre reinforced
material.
The most advanced composites are polymer matrix composites. They are
characterized by relatively low costs, simple manufacturing and high
strength. Their main drawbacks are the low working temperature,
sometimes high coefficient of thermal and moisture expansion and, in
certain directions, low stiffness. Polymer matrix composites are usually
reinforced by fibres to improve such mechanical characteristics as stiffness,
strength, etc. Fibres can be made of different materials (glass, carbon,
aramid, etc). Glass fibres are widely used because their advantages include
high strength, low costs and high chemical resistance [1].
13
Figure 3.1. Examples of composite materials with different forms of
constituents and distributions of the reinforcements. a. Laminate with unior bidirectional layers, b. Irregular reinforcement with long fibre, c.
Reinforcement with particles, d. Reinforcement with plate strapped
particles, e. Random arrangement of continuous fibres, f. Irregular
reinforcement with short fibres, g. Spatial reinforcement, h. Reinforcement
with surface tissues as mats, woven fabrics, etc. [1].
Composite
particle reinforced
fiber reinforced
preferred
orientation
random
orientation
continuous fiber reinforced
discontinuous fiber reinforced
(long fibers)
(short fibers)
unidirectional
reinforced
bidirectional
reinforced
special
reinforced
random
orientation
random
orientation
Figure 3.2. Classification of composites [1].
The fibre length, their orientation and their material behaviors are main
factors which contribute to the mechanical performance of a composite
material. Although matrices by themselves generally have low mechanical
properties (as) compared to fibres (except damping), they play following
several important roles:
14
•
Conduction of forces to fibres,
•
Protection of fibres from environmental effects,
•
Supporting of fibres under compression loads,
•
Responsibility of damping in composite.
3.1.2 Fibre Reinforced Composites
The economic application of plastics materials to mass-produced precision
engineered components has become possible largely as a result of the
development of short fibre reinforced composites.
•
Short fibre reinforced materials
Short fibre reinforced materials are the most commercially important
materials and the ones that exhibit the most significant development and
growth.
Some suppliers offer “long fibre” or “short fibres” reinforced thermoplastic
material. As defined by long fibre compound suppliers materials contain
fibre reinforcements that average 10 to 15 mm in length, while “short fibre”
compounds contain fibre reinforcements that are something less than this,
but average about 3 mm in length (Before injection moulding). After
injection moulding process fibres length are about 0.1~1 mm [1].
•
Glass Fibres
Reinforcements primarily give strength and stiffness to the composite. The
predominant fibres used for reinforcement are made of glass. But there are
a lot of kinds of fibres such as carbon (graphite), metal ceramic and etc.
Glass fibres are the most widely used form of reinforcement for plastic
materials. Advantages of glass fibres over other reinforcements include a
favorable cost/performance ratio with respect to dimensional stability,
corrosion resistance, heat resistance, and ease of processing [1].
3.1.3 Thermoplastics
Thermoplastics are polymers that can be melted more than once as the
molecular chains of these polymers do not crosslink and remain essentially
unchanged (except for some shortening) each time they are processed. This
15
is in contrast to thermosets, which undergo a chemical reaction when
processed, and hence cannot be remelted. Thermosets, however, generally
have greater dimensional stability and heat and chemical resistance than
thermoplastics. Paying attention to recycling issues; thermoplastics are
superior compare to thermosets, for short fibre reinforced thermoplastics
often are used as the matrix materials what needs need to an easy
producibility in the injection moulding process [13].
3.1.4 Injection Moulding (IM)
Although many fabricating processes are employed to produce unreinforced
plastic products, at least 50 % by weight of short fibre reinforced plastics
go through injection moulding machines. For smaller lot quantities,
however, other processes can compete with injection moulding (IM),
among them being compression moulding, transfer moulding, casting, and
thermoforming [2].
The IM process basically involves introducing the material into a
cylindrical heating chamber by a rotating screw where the compound is
melted under heat transfer and shearing. Then the melt is injected under
high pressure into a matched metal cavity. The part then solidifies into its
intended shape. With thermoplastic compounds, solidification occurs by
cooling the polymeric melt, but with thermoset compounds, solidification
occurs by heating the melt in the mould cavity to achieve polymerization
and cross-linking. The next step involves ejecting the part from the mould.
As shown in Figure 3.3, four basic mechanical units are combined to
perform injection moulding: the mould, a plasticizing unit, a mould
clamping unit and a control system unit [3].
Schließeinheit
Clamping Unit
Steuer- und
Werkzeug Plastifiziereinheit
Plasticizing Unit Control
System
Mold
Regeleinheit
Machine Base
Maschinenbett
Figure 3.3. The elements of an injection moulding process [3].
16
3.2 Anisotropy
Composites are mostly anisotropic. The properties of anisotropic materials
depend on the direction, whereas isotropic materials have no preferred
direction. Short glass fibre reinforced composites are classified in
anisotropic materials; therefore have some knowledge about anisotropy is
necessary for analyzing their behaviors.
3.2.1 Equations of General Anisotropic Elasticity
The constitutive equation, Hooke's law, states that the stress is linearly
proportional to strain [4],
σ ij = Cijkl ε kl ,
(3.1)
with Cijkl as the elastic modulus tensor. There are 81 components of Cijkl ,
but taking into account the symmetry of the stress and strain tensors, only
36 of them are independent. If the elastic solid is describable by a strain
energy function, the number of independent elastic constants is reduced to
21 by virtue of the resulting symmetry [15]
Cijkl = C klij .
(3.2)
This is the maximum number of independent elastic constants for any
material symmetry. If the symmetry properties imposed by the microscopic
nature of the material are considered, the number is typically less than 21.
An elastic modulus tensor with 21 independent constants describes an
anisotropic material with the most general type of anisotropy, triclinic
symmetry [5]. Orthotropic symmetry is characterized by three mutually
perpendicular mirror symmetry planes and twofold rotational symmetry
axes perpendicular to these planes [4].
17
⎡ C11
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎣⎢
C12
C 22
C13
C 23
0
0
0
0
C 33
0
0
C 44
0
sym.
C 55
0 ⎤
0 ⎥⎥
0 ⎥
⎥.
0 ⎥
0 ⎥
⎥
C 66 ⎦⎥
(3.3)
Materials with axisymmetry, also called transverse isotropy or hexagonal
symmetry, are invariant to 60 o rotation about an axis and describable by
five independent elastic constants [9],
⎡ C11
⎢
⎢
⎢
⎢
⎢
⎢
⎢
⎢⎣
C12
C 22
C12
C 23
0
0
0
0
C 22
0
0
C 44
0
sym.
C55
0 ⎤
0 ⎥⎥
0 ⎥
⎥,
0 ⎥
0 ⎥
⎥
C55 ⎥⎦
(3.4)
with C 44 = (C 22 − C 23 ) / 2 .
For example, a unidirectional fibre reinforced composite may have
orthotropic symmetry if the fibres are arranged in a rectangular packing or
transverse isotropy if the fibres are packed hexagonally [6]. Isotropic
materials with properties independent of direction are described by two
independent elastic constants [15].
3.2.2 Micromechanical Model
As mentioned, Hooke’s law written in tensor notation that describes the
relation between stress and strain (Chapter 3.2.1) provides the basis for the
calculation of the elastic behavior of plastics. If there are three orthogonal
planes of symmetry in the material - as it can be found for short fibre
reinforced thermoplastics - the material behavior is denoted orthotropic
(orthogonal anisotropy) with nine elements in elasticity modulus tensor
[10].
18
A comprehensive survey of different micromechanical models for the
determination of the elastic properties of short fibre reinforced composites
is given in [7]. At present from the multitude of published theories the
equation sets of Tandon-Weng [8] and Halpin-Tsai [9] achieved the widest
prevalence in commercial software.
The Halpin-Tsai equations are used in this thesis therefore they are
explained in more details in the following.
•
Halpin-Tsai Equations
The Halpin-Tsai equations are a simplified form of Hill’s generalized selfconsistent model results with engineering approximation to make them
suitable for the designing of the composite materials. Hill assumed a
composite cylinder model in which the embedded phase considered
continuous and perfectly aligned cylindrical fibres. Both materials were
assumed to be homogeneous and elastically transversely isotropic (Eq. 3.4)
about the fibre direction [9].
The Halpin-Tsai equations are tabulated in Table 3.1 for engineering
constants where E , G and K represent elastic, shear and bulk modulus,
respectively. ξ is a measure of reinforcement geometry and also ν and
Φ are Poisson ratio and fibre volume fraction, respectively. The indices f
and m stand on fibre and matrix respectively for all the parameters in the
Table 3.1.
Fibre volume fraction is calculated by Eq. 3.5;
Φ=
VF AF
=
=
VC AC
1
,
1− Ψ ρ f
1+
⋅
Ψ ρm
(3.5)
where
Ψ = fibre weight fraction
VF = volume of fibre
VC = volume of composite
AF = section area of fibre
AC = section area of composite
19
ρ f = density of fibre
ρ m = density of matrix.
Table 3.1. Halpin-Tsai equations [9].
E11 = Em
E22 = Em
1 + ξηΦ
1 − ηΦ
Ef
−1
Em
η=
Ef
+ξ
Em
ξ =2
1 + ξηΦ
1 − ηΦ
Ef
−1
Em
η=
Ef
+ξ
Em
ξ =2
l
d
ν 21 = ν 12
1 + ξηΦ
1 − ηΦ
Gf
−1
Gm
η=
Gf
+ξ
Gm
ξ =1
ν 31 = ν 21
1 E22
−1
2 G23
ν 23 = ⋅
G12 = G13
G23 = Gm
1 + ξηΦ
1 − ηΦ
E22
E11
ν 13 = ν 12
E33 = E22
G12 = Gm
ν 12 = Φν f + (1 − Φ)ν m
Gf
−1
Gm
η=
Gf
+ξ
Gm
ξ=
Km
Gm
Km
+2
Gm
ν 32 = ν 23
In Table 3.1, l and d stand on the length and diameter of the fibre,
respectively.
The relations between stiffness and engineering constants in Halpin-Tsai
equations are tabulated in Table 3.2.
20
Table 3.2. Relation between stiffness tensor and engineering constants in
Halpin-Tsai equations [9].
Cij
Engineering constants
(C 22 + C23 ) / 2
E22
2(1 −ν 23 − 2ν 12ν 21 )
C12 = C13
ν 21 E11
ν 12 E22
=
(1 − ν 23 − 2ν 12ν 21 ) (1 − ν 23 − 2ν 12ν 21 )
C11
(1 −ν 23 ) E11
(1 −ν 23 − 2ν 12ν 21 )
C 44
G23
C55 = C66
G12
C12 /(C 22 + C 23 )
ν 12
⎛ 2C122 ⎞
⎟⎟
C11 ⎜⎜
C
C
+
22
23
⎠
⎝
E11
[C11 (C22 + C23 ) − 2C122 ](C22 − C23 )
C12C22 − C122
E22
3.3 Viscoelastic Behavior of Plastics
It is observed that a plastic, at specific temperature and molecular weight,
may behave viscose as a liquid or solid depending on the speed (time scale)
at which its molecules are deformed. This behavior, which ranges between
liquid and solid, is generally referred to as the viscoelastic behavior or
material response. If the deformations are small the modeling is linear
viscoelastic. Non-linear viscoelasticity is required when modeling large
deformations so that the material deformation is dependent on the grade of
deformation. In this thesis work all simulations are assumed to be in the
linear domain.
In linear viscoelasticity the stress relaxation test is often used, along with
the time- temperature superposition principle [13] and the Boltzmann
21
superposition principle [12], to explain the behavior of plastics during
deformation.
3.3.1 Application of Viscoelasticity to Describe the Behavior of
Plastics
Most plastics exhibit a viscous as well as an elastic response to stress and
strain. This puts them in the category of viscoelastic materials. Various
combinations of elastic and viscous elements have been used to
approximate the material behavior of plastics. Most models are
combinations of springs and dash pots the most common one being the
Maxwell model [12].
E
η
σ
Figure 3.4. Schematic diagram of the Maxwell Model [12].
In the Maxwell model (Figure 3.4) the total strain, ε , in the model has an
elastic, ε e , and a viscous, ε v , strain contribution and can be represented as
follows:
ε = εe + εv .
(3.6)
Similarly, the strain rates are written as
ε& = ε&e + ε&v .
(3.7)
Assuming the spring follows Hookes law, the following relation holds
22
ε&e =
σ&
E
.
(3.8)
And the viscous portion, represented by the dash pot, is written as follows
ε&v =
σ
.
η
(3.9)
Combining the last three equations result in
σ=
η dσ
E dt
=η
dε
,
dt
(3.10)
which is often referred to as the governing equation for the Maxwell’s
model in differential form.
For more accurate estimate or realistic analysis the Maxwell model is not
sufficient. For a better fit with experimental data it is common to use
several spring-dash pot models in parallel. Such a configuration is often
referred as a generalized Maxwell model [13].
3.4 Dynamic Mechanical Analysis (DMA)
The Dynamic Mechanical Analysis (DMA) is a very important apparatus in
the modern polymer laboratory. DMA measures the mechanical properties
of materials for different thermoplastics while they are subjected to a
periodic stress, usually applied sinusoidally. An oscillating force is applied
to a sample of the material and the resulting displacement of the sample is
measured. From this the stiffness of the sample can be determined, and the
sample modulus can be calculated. Measuring the time lag in the
displacement compared to the applied sinusoidal force it is possible to
determine the damping properties of the material.
Most polymeric materials show a combination of both types of behavior i.e.
they react elastically, and flow to some extent at the same time
(viscoelasticity). The stress and strain curves are therefore out of phase by
an amount less than 90° [14].
23
3.4.1 Sinusoidal Oscillatory Test
In the sinusoidal oscillatory test, a specimen is excited with a low
frequency stresses input which is recorded along with the strain responses.
The shapes of the test specimen and the testing procedure vary significantly
from test to test [13].
If the test specimen in a sinusoidal oscillatory test is perfectly elastic, the
stress input and strain response would be as follows:
τ (t ) = τ 0 cos ωt ,
(3.11)
γ (t ) = γ 0 cos ωt .
(3.12)
For an ideally viscous test specimen, the strain response would lag π / 2
radians behind the stress input:
τ (t ) = τ 0 cos ωt ,
(3.13)
π
γ (t ) = γ 0 cos(ωt − ) .
(3.14)
2
Plastics behave somewhere in between the perfectly elastic and the
perfectly viscous materials and their responses is described by
τ (t ) = τ 0 cos ωt ,
(3.15)
γ (t ) = γ 0 cos(ωt − δ ) .
(3.16)
The shear modulus takes a complex form of
G* =
τ (t ) τ 0 e iδ τ 0
=
= (cos δ + i sin δ ) = Gs + iGl ,
γ (t )
γ0
γ0
(3.17)
which is graphically represented in Figure 3.5. Gs is usually referred to as
storage shear modulus and Gl as loss shear modulus. The ratio of loss
modulus to storage modulus is referred to as loss tangent or phase lag [13]:
tan δ =
Gl
.
Gs
(3.18)
24
G*
Gl
δ
Gs
Figure 3.5. Stress and strain vs. time t [13].
3.5 Acoustic Analysis
As this thesis work is dealing with acoustic analysis, the vibration theory
and finding appropriate method to set up the equations of motion is
interesting.
Vibration theory is concerned with the oscillatory motion of the physical
systems. The motions may be harmonic, periodic, or a general motion in
which the amplitude varies with the time. When the deformation is quite
small, the vibration is assumed linear.
Vibrations are the results of the combined effects of inertia and elastic
forces. Inertia of the moving parts can be expressed in terms of the masses,
moment of inertia, and the time derivatives of the displacements. Elastic
restoring forces can be expressed in the terms of the displacements and
stiffness of the elastic members.
While the effect of inertia and elastic forces tend to maintain oscillatory
motion, the transient effect dies out because of energy dissipation. The
process of energy dissipation is generally referred to as damping. Damping
in general, has the effect of reducing the amplitude of vibration. Plastics
materials are not perfectly elastic and they do exhibit damping, because of
the internal friction due to the relative motion between internal molecular
structures of the material during the deformation process. Such materials
are referred to as viscoelastic solids as viscoelastic thermoplastics which
are focused of this thesis work [16].
25
3.5.1 Formulation of the Equations of Motion
The success of mathematical analysis of vibration is dependent upon the
correct formulation of the equations of motion and is based on some
principles [17].
In order to obtain the equation of motion one may use the dynamic
equilibrium (using Newton’s second law of motion) or the principle of
virtual work (application of d’Alembert’s principle).
Considering the Newton’s second law for a dynamic system in equilibrium,
the equation of motion can be written
mu&& + cu& + ku = F .
(3.19)
In Figure 3.6 (for a single mass, spring damper system) the forces acting on
the mass consist of the externally applied force F , a restoring force ku due
to the spring and a damping force cu& due to the viscous damper and an
inertia force mu&& .
For multi degree of freedom systems:
[
]
r d
r
r
Fi − mi u&i + ci ui = 0,
dt
i = 1,2,K, N
(3.20)
where considering a system of N masses and dampers [17].
k
m
F(t)
u(t)
c
Figure 3.6. Single mass, spring, damper system [17].
Since, the problem of vectorial addition of forces when the structure to be
analysed is a complex one, this method is difficult to apply, therefore
Hamilton principle or Lagrange’s equation (more convenient form for a
discrete system) are more appropriate to use due to overcoming this
problem.
26
3.5.2 Hamilton’s Principle
Although the principle of virtual displacement overcomes the problem of
vectorial addition of forces, the virtual work itself is calculated from the
scalar product of two vectors, one representing a force and one a virtual
displacement. This disadvantage can be largely overcome by using
Hamilton’s principle. [17]
The mathematical statement of Hamilton’s principle is
t2
∫ (δ (T − V ) + δW ) dt = 0 ,
(3.21)
nc
t1
where
T = Kinetic Energy of the system,
V = Elastic Strain Energy of the system,
Wnc = Work done by non-conservative forces.
The application of this principle leads directly to the equations of motion
for any system. It can be applied to both discrete, multi-degree of freedom
systems and continuous systems. The advantage of this freedom
formulation is that it uses scalar energy quantities. Vector quantities may
only be required in calculating the work done by the non-conservative
forces.
3.5.3 Lagrange’s Equations
When Hamilton’s principle is applied to discrete systems it can be
expressed in a more convenient form as follows:
d ⎛ ∂T ⎞ ∂D ∂U
+
=F,
⎜
⎟+
dt ⎝ ∂u& ⎠ ∂u& ∂u
where T =
(3.22)
1
1
1
mu& 2 , U = ku 2 , D = cu& 2 .
2
2
2
Substituting this equation becomes same as the Eq. 3.19 [17].
27
3.5.4 Single Degree of Freedom System (SDOF)
In Eq. 3.19 with the assumptions of c = 0 and F (t ) = 0 , the equation
becomes mu&& + ku = 0 (undamped free vibration). The solution of this
equation is a pure time-harmonic oscillation and given by
u (t ) = A sin(ωt − φ ) ,
(3.23)
where the amplitude A and phase φ are determined by the initial conditions
k
. The solution describes
m
an oscillatory motion without damping. With F (t ) = 0 the equation
becomes
and ω is the undamped natural frequency ω =
mu&& + cu& + ku = 0.
(3.24)
This is the standard form of the second order differential equation of
motion that governs the linear vibration of damped single degree of
freedom systems. The solution of Eq. 3.24 is given by
u (t ) = A e−ξωt sin(ϖt + φ ).
(3.25)
where ξ is a dimensionless quantity. It is called as damping factor and
c
defined as ξ =
, while the critical damping coefficient c c is defined as
cc
cc = 2mω = 2 km , and ω is the system natural frequency defined
as ω =
k
. ϖ is the damped natural frequency (ϖ = ω 1 − ξ ² ).
m
The nature of the system’s motion depends on the value of ξ in Eq. 3.25
[18].
3.5.5 Multiple Degree of Freedom System (MDOF)
It is more convenient to use matrix notations to write the differential
equations of systems, which have more than one degree of freedom. For a
damped system with N degrees of freedom, the equation of motion can be
written in matrix form as:
28
&& + cu& + ku = F(t ) ,
mu
(3.26)
&& are the vectors of displacements, velocity and
where u, u& and u
accelerations defined as:
⎡u1 ⎤
⎡u&1 ⎤
⎡u&&1 ⎤
⎢u ⎥
⎢u& ⎥
⎢u&& ⎥
⎢ 2⎥
⎢ 2⎥
⎢ 2⎥
&& = ⎢. ⎥ ,
u = ⎢. ⎥, u& = ⎢. ⎥, and u
⎢ ⎥
⎢ ⎥
⎢ ⎥
⎢. ⎥
⎢. ⎥
⎢. ⎥
⎢u N ⎥
⎢u& N ⎥
⎢u&&N ⎥
⎣ ⎦
⎣ ⎦
⎣ ⎦
and m, c and k are the mass matrix, damping matrix and stiffness matrix
respectively and are given as:
... m1N ⎤
⎡ c11
⎢c
⎥
... m2 N ⎥
, c = ⎢ 21
⎢ ...
... ... ⎥
⎥
⎢
... m NN ⎦
⎣c N 1
⎡ m11
⎢m
m = ⎢ 21
⎢ ...
⎢
⎣m N 1
m12
m22
⎡ k11
⎢k
k = ⎢ 21
⎢ ...
⎢
⎣k N 1
k12 ... k1N ⎤
k 22 ... k 2 N ⎥⎥
.
... ... ... ⎥
⎥
... ... k NN ⎦
...
...
c12
c22
...
...
... c1N ⎤
... c2 N ⎥⎥
and
... ... ⎥
⎥
... c NN ⎦
(3.27)
The coefficients mij (i, j = 1,2,...N ) , cij (i, j = 1,2,...N ) and kij (i, j = 1,2,...N )
are termed mass, damping and stiffness matrix, respectively.
In the simplest theoretical case of N -DOF vibrations, there is no damping
and no forcing (undamped free vibration), and the equations of motion are:
&& + ku = 0 .
mu
(3.28)
Assuming the solution to be time-harmonic u(t ) = φ cos ωt , one obtains an
eigenvalue problem for the determination of ω and φ
(k − ω m )φ = 0 ,
2
(3.29)
29
where ω 2 is an eigenvalue and φ is the associated eigenvector. For
nontrivial solutions φ ≠ 0 to exist, the determinant of the coefficient matrix
must vanish, i.e.
k − ω2 m = 0 .
(3.30)
Expanding the determinant one obtains an n-degree polynomial in ω 2 , this
solution called frequency-equation. The N degrees of this polynomial
2
provide a set of eigenvalues ωi , i = 1,2,..., N , and the corresponding values
ω i are the un-damped natural frequencies. Substituting each ω i into Eq.
3.29 one obtains the associated eigenvectors φ i , i = 1,2,..., N , also termed
natural modes or mode shapes [18].
3.6 Introduction to Finite Element Method (FEM)
In the field of engineering design we come across many complex problems,
the mathematical formulation of which is tedious and usually not possible
by analytical methods. At such instants engineers often resort to the use of
numerical techniques. Here lies the importance of FEM, which is a very
powerful tool for getting the numerical solution of a wide range of
engineering problems. The basic concept is that a body or structure may be
divided into smaller elements of finite dimensions called as “Finite
Elements”. The original body or structure is then considered as an assembly
of these elements connected at a finite number of joints called as “Nodes”
or “Nodal Points”. The properties of the elements are formulated and
combined to obtain the properties of the entire body.
The equations of equilibrium for the entire structure or body are then
obtained by combining the equilibrium equation of each element such that
the continuity is ensured at each node. The necessary boundary conditions
are then imposed and the equations of equilibrium are solved to obtain the
variables required such as stress, strain, temperature distribution or velocity
depending on the application.
Thus, instead of solving the problem for the entire structure or body in one
operation, in the FEM, attention is mainly devoted to the formulation of
properties of the constituent elements. A common procedure is adopted for
combining the elements, solution of the equations and evaluation of the
30
variables required in all fields. Thus, the modular structure of the method is
well exploited in various disciplines of engineering.
The method is not exact, but it can be very accurate if used wisely. The
results, which are predicted by an experienced modeler, can be taken to be
exact to engineering accuracy, being limited more by lack of precise
knowledge of material properties, loads and the boundary condition than by
the errors of numerical method. While interpreting the result of an FEA the
engineer should be always aware of possible inaccuracy depending on these
errors. The software ABAQUS is based on Finite Element Analysis to solve
many engineering problems and is used in this thesis work.
3.7 Introduction to ABAQUS
ABAQUS is an engineering simulation program based on the finite element
method, which can solve problems ranging from relatively simple linear
analyses to the most challenging non-linear simulations. ABAQUS contains
an extensive library of elements that can model virtually nearly, any
geometry and most material properties. It has an equally extensive list of
material models that can simulate the behavior of most typical engineering
materials including metals, rubber, plastics, composites, reinforced
concrete, crushable and resilient foams, and geotechnical materials such as
soils and rock combined with the other material properties like density,
specific heat capacity and etc. Designed as a general-purpose simulation
tool, ABAQUS can be used to study more than just structural (stressdisplacement) problems. It can simulate problems in such diverse areas as
heat transfer, mass diffusion, thermal management of electrical components
(coupled thermal-electrical analyses), acoustics, soil mechanics (coupled
pore fluid-stress analyses), and piezoelectric analysis [19].
ABAQUS is simple to use even though it offers the user a wide range of
capabilities. For example, problems with multiple components are modeled
by associating the geometry defining each component with the appropriate
material models. In most simulations, even highly nonlinear ones, the user
needs only to provide the engineering data such as the geometry of the
structure, its material behavior, its boundary conditions, and the loads
applied to it. In a nonlinear analysis ABAQUS automatically chooses
appropriate load increments and convergence tolerances. Not only does it
choose the values for these parameters, it also continually adjusts them
during the analysis to ensure that an accurate solution is obtained
31
efficiently. The user rarely has to define parameters for controlling the
numerical solution of the problem [19].
3.8 Dynamic Response Analysis in ABAQUS
ABAQUS offers several methods for performing dynamic analysis of
problems which can be divided into two major groups: 1-Modal dynamics
and 2-Complex harmonic oscillations.
All simulation in this thesis are dealing with two steps in which in the first
step the natural frequency is extracted by Lanczos eigen-solver and the
second step by providing a direct steady-state dynamic analysis, the
responses of the system under harmonic excitation are determined.
3.8.1 Step1 Natural Frequency Extraction
The natural frequencies of a system can be extracted using eigenvalue
analysis (“Natural frequency extraction”) (See Chapter 3.5).
The frequency extraction procedure performs an eigenvalue extraction to
calculate the natural frequencies and the corresponding mode shapes of a
system. There are two methods to solve the eigenvalue matrix the Lanczos
and the subspace iteration method. The Lanczos method is generally faster
when a large number of eigenmodes is required for a system with many
degrees of freedom. The subspace method is faster when only a few
eigenmodes are needed.
The structural eigenvalue problem has received considerable attention since
the advent of finite element models. Ramaswami [20] summarizes available
methods for this problem. The most attractive one appears to be the
Lanczos method that is used in the simulations of this thesis in order to find
the natural frequencies.
3.8.2 Step2 Direct Solution Steady State Harmonic Response Analysis
There are three ways of steady state analysis: Direct, Mode and Subspace
based steady-state dynamic analysis. In the direct method the steady-state
harmonic response is computed directly in terms of the physical degree of
freedom of the model. The mode based analysis is based on modal
32
superposition techniques and the subspace analysis is based on a subspace
projection method. For computing the steady-state response of simulations
in this thesis the direct method is used, as it is more accurate than the other
two methods especially when viscoelastic material behavior is present in
the structure. However, it is more time consuming than the others.
The steady-state harmonic response of a system can be calculated in
ABAQUS/Standard directly in terms of the physical degrees of freedom of
the model (“Direct-solution steady-state dynamic analysis.”). The solution
is given in-phase (real) and out-of-phase (imaginary) components of the
solution variables (displacement, velocity, stress, etc.) as functions of
frequency. The main advantage of this method is that frequency-dependent
effects (such as frequency-dependent damping) can be modelled. The direct
method is the most powerful and accurate but also the most expensive
steady state harmonic response procedure. The direct method can also be
used if non-symmetric terms in the stiffness are important or if the model
parameters depend on frequency.
As mentioned, steady-state dynamic analysis provides the steady-state
amplitude and phase of the response of a system due to harmonic excitation
at a given frequency. Usually such analysis is done as a frequency sweep by
applying the loading at a series of different frequencies and recording the
long term steady state response in ABAQUS/Standard the direct-solution
steady-state dynamic procedure conducts this frequency sweep.
Therefore the direct steady-state dynamic analysis is chosen in the
following problems;
• for nonsymmetric stiffness,
• when any form of damping other than modal damping must be included,
• when frequency dependent viscoelastic material properties must be taken
into account.
3.9 Material Behavior Description
In order to describe the material behaviour (stiffness and damping) several
methods are available. The most accurate method is using viscoelasticity
theory and defines the mechanical behaviour of the plastic by data extracted
from DMA.
33
3.9.1 Frequency Domain Viscoelasticity
A viscoelastic model can be used to specify frequency or time-dependent
material behaviour. In the first simulation of this thesis work (Chapter 4.1)
the material behavior is modeled by assuming a viscoelastic polyamide
plate which is modeled in the frequency domain.
For modelling the viscoelastic behaviour of the plastic materials, the
frequency domain modelling can be used. Frequency dependent shear and
bulk moduli are used to include the dissipative part of the material
behaviour.
•
Determination of the viscoelastic material parameters
The dissipative part of the material behavior is defined by giving the real
and imaginary parts of g * and k * as functions of frequency. Where g * (ω )
is the Fourier transform of the non-dimensional shear relaxation
G (t )
function g (t ) = R − 1 . Expression for bulk relaxation function is similar
G∞
to shear relaxation function. The moduli can be defined as functions of the
frequency in the following three ways: by a power law, by tabular input or
by a Prony series expression for the shear and bulk moduli [19]. In the first
simulation of this thesis tabular frequency dependent data for input of
material modeling is used.
•
Tabular frequency dependence
The frequency domain response can alternatively be defined in tabular from
on the data lines by giving the real and imaginary parts of ωg * and ωk * ,
where ω is the circular frequency. The parameters are declared in the
command line as:
ω Re( g * ) , ω Im(g * ) , ω Re(k * ) , ω Im(k * ) and f ( Hz )
where
ω Re( g * ) = Gl G∞ , ω Im( g * ) = 1 − Gs G∞ , ω Re(k * ) = K l K ∞ , (3.31)
ω Im(k * ) = 1 − K s K ∞ , G∞ = G (t = ∞) and K ∞ = K (t = ∞)
34
This declaration was used to define the viscoelastic option in the ABAQUS
program for analyzing the steady state response (Chapter 4.1).
3.9.2 Material Damping (Rayleigh damping)
In direct steady state dynamic analysis, it is very often to define the energy
dissipation mechanisms (dashpots) as part of the basic model. ABAQUS
provides “Rayleigh” damping for this purpose. Rayleigh damping can be
used in direct-solution steady-state dynamic analyses to get quantitatively
accurate results, especially near natural frequencies.
To define Rayleigh damping, two Rayleigh damping factors should be
specified; α R for mass proportional damping and β R for stiffness
proportional damping. In general, damping is a material property specified
as part of the material definition.
For a given mode i the damping factor, ξ i , can be expressed in terms of the
damping factors α R and β R as:
ξi =
α R β Rωi
+
,
2ωi
2
(3.32)
where ωi is the natural frequency at this mode. This equation implies that,
generally speaking, the mass proportional Rayleigh damping, α R , is
damping for the lower frequencies and the stiffness proportional Rayleigh
damping, β R , damping at the higher frequencies.
The Rayleigh damping model is used in the following simulation of a short
glass fibre reinforced thermoplastic plate (Chapter 4.2).
3.10 Introduction to SIGMASOFT
SIGMASOFT is a tool for the investigation of the filling and cooling/curing
processes for thermoplastics, elastomers and thermoset materials. This
program has an integrated geometry modeler. Modeling a running system
in 3D provides the base for the numerical computations. A wide range of
modeling functions allows also the preparation of geometries in the
software itself. Furthermore, it facilitates accurate importing and
35
subsequent modification of CAD data via the different interface available.
Automatic meshing of the geometry in SIGMASOFT is a further important
key for rapid, accurate and flexible operation.
SIGMASOFT is based upon MAGMASOFT which is a simulation
software for the metal casting process which has been used for more than
ten years by more than 400 companies worldwide.
With SIGMASOFT the user can optimize the part and the tool with respect
to optimal part quality and cycle times.
SIGMASOFT is based on 3D volume elements. Parts with varying wall
thickness can be simulated in a physical correct manner. Inserts and the tool
are part of the model, both are calculated in 3D.
This engineering program allows the calculation of filling, cooling and
residual stresses in 3D volume elements also for fibre reinforced materials.
In this thesis work, SIGMASOFT was used to calculate the fibre orientation
in the modeled part, which affect its mechanical behavior [21].
36
4 Simulations
4.1 Acoustic Simulation of a Viscoelastic Model Plate
The simulation of the acoustic behavior of a polyamide model plate was
done in ABAQUS. The main goal of this task is the study of the material
modeling by data from DMA in the frequency domain, and obtaining the
result needed for comparison in the following study.
In order to simulate an isotropic model plate after defining the part
geometry, the material was modeled by the frequency dependent data
obtained from DMA measurements. The goal of this study is finding the
behavior of the specimen as responses for displacement, velocity and
acceleration with respect to frequency under the application of a 1 N
amplitude harmonic force.
4.1.1 Preprocessing
In this stage the model of the physical problem was defined and an
ABAQUS input file (Study_1, Appendix-A) was created.
•
Part Geometry
The model plate was created in SOLIDWORKS, the CAE software, and
imported as a “stl” file to ABAQUS. As it is shown in Figure 4.1, it is a
plate in feature of 112.5 mm length, 110.5 mm width and 2 mm thickness
in which two corners of the plate are filleted by a radius of 12 mm. this part
geometry corresponds to an actual model geometry which is available at
IKV that was the reason for choosing and modeling this model plate. In
further works, it will be possible to carry out validation measurements for
the simulation results of this part.
37
R12 mm
98.50 mm
88
.5
0m
m
m
2m
Figure 4.1. Part geometry of the specimen.
•
Material Modeling
In the property module the plate was termed as Polyamide which has a long
term elastic modulus of 380 MPa, a density of 1.144 g/cm3 and a Poisson’s
ratio of 0.28 and also the material was assumed to be isotropic and linear.
The chosen units were consistent and in SI (mm) form. The density of the
material was necessary to define the mass matrix as eigenmodes and
eigenfrequencies depend on it.
The main aim of the study is to get the steady state dynamic response of the
model plate under harmonic excitation considering frequency dependent
stiffness and damping behaviors of plastics. To get the damping effect in
the response, viscoelasticity associated with the plastic model plate had
been declared by using tabular frequency dependence of the material
property as discussed in Chapter 3.9.
The frequency domain viscoelasticity was used to characterize the
frequency dependent viscoelastic material properties, including the losses
38
caused by the ‘‘viscose’’ (internal damping) nature of the polymer (plastic).
The frequency domain viscoelastic material model describes the frequencydependent material behavior for small steady-state harmonic oscillations.
The frequency dependent data extracted from DMA measurements were
used as frequency tabular data in order to complete the model plate material
modeling.
From DMA measurements, the storage and loss elastic modulus ( Es and El )
can be derived for the interesting frequency interval (see Figure 4.2).
1.E+03
[Mpa]
[Mpa]
8.E+02
6.E+02
Es
El
4.E+02
2.E+02
0.E+00
0.001
0.01
0.1
1
10
100
1000
10000
Frequency [Hz]
Figure 4.2. Storage and loss elastic modulus obtained from DMA.
Using Eq. 4.1 and 4.2, the values of G s , Gl , K s and K l are obtained;
Gs =
Es
El
, Gl =
,
2(1 + v)
2(1 + v)
(4.1)
Ks =
Es
El
, Kl =
.
3(1 − 2v)
3(1 − 2v)
(4.2)
Figure 4.3 shows the frequency dependency of the storage and loss shear
modulus Polyamide.
39
[Mpa]
4.E+02
3.E+02
3.E+02
2.E+02
2.E+02
1.E+02
5.E+01
0.E+00
0.001
Gs
Gl
0.01
0.1
1
10
100
1000
10000
Frequency [Hz]
Figure 4.3. Storage and loss shear modulus obtained from
Eq. 4.1 and 4.2.
Considering Eq. 3.31; the parameters required, used as inputs in the
frequency tabular data, ω Re( g * ) , ω Im(g * ) , ω Re(k * ) and ω Im(k * ) were
calculated.
•
Enmeshment and Element type
The model plate is not a complex geometry and does not have different
structural elements. Because of this a single meshing for the whole part is
possible. As the simulation is considering shear stress, the solid
(continuum) element type was assigned to the part.
The linear hexahedral solid element type C3D8 is assigned to the model
plate in the mesh module. The first letter of this element’s name indicates to
continuum (solid) element family the element belongs.
In order to verify the element numbers, the first step (Natural frequency
extraction) was performed 7 times with different element numbers. As
Figure 4.4 shows, by increasing the element numbers; the first, second and
third natural resonance frequencies were obtained more accurately. Due to
going to quite suitable result by applying more than 2000 nodes; 2691
nodes were chosen for all simulations of this thesis.
40
Freq. [Hz[Hz]
Frequency
100
90
80
70
60
50
40
30
20
10
0
1st resonance freq.
2nd resonance freq.
3rd resonance freq.
0
2000
4000
6000
8000
10000
Element Numbers
Figure 4.4. Accuracy in the result by increasing the element numbers.
•
Steps involved in the modeling
Steps involved for the simulation were frequency extraction and direct
steady state dynamic analysis.
In the first step the natural frequencies were calculated by using Lanczos
eigensolver by assigning a frequency interval of 1 to 10000 Hz
The direct steady-state dynamic analysis was assigned for the second step
of this study in which provides the steady-state amplitude and phase of the
response of a system due to harmonic excitation at a given frequency. The
analysis was done as a frequency sweep by applying the loading at a series
of different frequencies and recording the response. The frequency range of
interest was selected from 1 to 10000 Hz and the number of frequencies at
which results were required in this range was specified to 10000 on the data
lines of the *STEADY STATE DYNAMICS command. The frequency
spacing is linear.
41
•
Load and boundary conditions
To define the boundary conditions one end of the plate was fixed and it was
assigned with zero degrees of freedom by means of encastre option in the
boundary condition command for all steps (Figure 4.5).
The concentrated harmonic load of 1 N amplitude was applied on the
corner point of the plate which is highlighted in Figure 4.5. In the steady
state dynamics step it is automatically considered as of sinusoidal nature
and only the value of the amplitude has to be assigned. The frequency of
the force is automatically adopted with the frequency sweep.
fixed end
Harmonic force with 1 N (amplitude)
Figure 4.5. Load and boundary conditions.
42
4.1.2 Postprocessing and Discussion
In the first part of this section natural frequencies and associated modes of
vibration are discussed, which give the deformation behavior of the system
on corresponding eigenmode. While, in the analysis of the steady state
dynamics response, the effect of the harmonic force on the displacement
and velocity responses are investigated.
•
Analysis done in step-1 (Frequency extraction)
The first four mode shapes of the natural frequency extraction step with
corresponding undamped natural frequencies are shown in the Figure 4.6
and also the first ten undamped natural frequencies are tabulated in Table
4.1. The contour plots of the deformed plate show how the plate is
deformed relatively. Figure 4.6 shows that opposite regions are more
deformed than the regions near by the fixed end. And also there are other
regions with zero deformation depending on the corresponding eigenform
at each mode shape.
Table 4.1. Natural Resonance Frequencies (Hz).
Mode No.
1
2
3
4
5
6
7
8
9
10
…
Frequencies (Hz)
14.55
46.90
89.82
127.98
156.90
253.88
282.59
284.67
328.12
457.54
…
43
Mode1
Mode3
at 14.55 Hz
at 89.82 Hz
Mode2
Mode4
at 46.90 Hz
at 127.98 Hz
2
3
1
Figure 4.6. Deformation of the polyamide model plate at the undamped
resonance frequencies.
•
Analysis done in step-2 (Steady state dynamics)
In this analysis, beside the calculation of the natural frequencies also after
the result values like the displacement, the velocity and the acceleration can
be determined. In this section the steady state dynamics response of the
polyamide model plate including material damping is achieved and the
displacement, velocity and acceleration responses obtained at the node of
the application of the harmonic force are extracted.
The first ten damped resonance frequencies are tabulated in Table 4.2, and
the corresponding deformation of the model plate is shown in Figure 4.7 for
the first four damped resonance frequencies.
44
Table 4.2. Damped Resonance Frequencies (Hz).
Mode No.
1
2
3
4
5
6
7
8
9
10
…
Frequencies (Hz)
17
53
109
151
185
334
399
578
620
708
…
Regarding the material definition (Chapter 4.1), the stiffness value changes
by frequency, so the stiffness value is not constant like the case of natural
frequency extraction. From the comparison between the undamped natural
frequencies and the corresponding damped ones; it is found that the
damped resonance frequency values shifted from the undamped natural
frequencies to the higher values. For example the first mode of undamped
natural frequency is situated at 14.55 Hz, while in the damped case the first
resonance peak lies on 17 Hz (comparison between Table 4.1 and 4.2).
Because the stiffness value is considered constant in the first step of the
simulation where the natural frequencies are extracted using the
eigensolver, however considering viscoelastic frequency dependent
material definition in the second step, the stiffness and damping values are
changing corresponding to frequency increment. This proves the fact that
any changing in material stiffness leads to higher or lower frequency
shifting. It stands on this fact that the higher stiffness value leads to higher
resonance frequencies and lower stiffness goes to lower resonance
frequencies.
From the other point of view the effect of changing damping on the model
plate response is performed at the peak value magnitudes.
45
at 17 Hz
at 53 Hz
at 151 Hz
2
3
1
Figure 4.7. Deformation of the polyamide model plate at the peak values of
the damped frequencies.
Figure 4.8 illustrates the displacement, velocity and acceleration responses
of the polyamide model plate to the harmonic force in a frequency interval
between 1 to 1000 Hz. In this figure and in all three responses, the peaks
are laid on the damped resonance frequencies and the effect of damping on
the magnitude of the responses is based on the natural phenomenon of
damping effects.
46
Response
point
1.E+07
1.E+06
1.E+05
1.E+04
1.E+03
1.E+02
1.E+01
1.E+00
1.E-01
1.E-02
Dis. [mm]
1
10
100
1000
Vel. [mm/s]
Acc. [mm/s2]
Frequency [Hz]
Figure 4.8. Displacement, velocity and acceleration responses vs.
frequency for the polyamide model plate.
4.2 Acoustic Simulation of Short Glass Fibre
Reinforced Model Plates with Different Fibre
Orientations
4.2.1 Introduction
Basic requirement for a precise acoustic simulation of injection moulded
parts made of short-fibre reinforced thermoplastics using FEA is
information about the local fibre orientation in the part.
The properties of a unidirectional reinforced fibre/matrix-composite
constitute the basis for the description of the local part stiffness of fibre
reinforced plastics (Figure 4.9). They can be calculated by means of
micromechanical models from the individual characteristics of fibre and
matrix (e.g. Halpin-Tsai equations in Chapter 3.2.2). As input parameters
the elastic properties of fibre and matrix, the fibre volume fraction and the
47
fibre geometry are needed (Table 3.1). On the other hand, the short fibres
orient to a state between complete disorientation and perfect unidirectional
alignment. Therefore, the stiffness properties have to be adjusted to the
actual state of orientation.
1. Fiber and Matrix
properties
Matrix
Em , νm
Fiber
E f ,ν f
Fiber volume fraction
Micromechanics
(Halpin/Tsai)
2. Properties of
unidirectional
composite
Transversely Isotropic
E1 , E2 , ν12 , G12 , G23
Orientation Averaging
(Advani/Tucker)
3. Properties of
real composite
Orthotropic
E1 / 2 / 3 , ν1 / 2 / 3 , G/ 1 / 2 / 3
Figure 4.9. Determination of the local stiffness of short fibre reinforced
thermoplastics.
4.2.2 Implementation into Software
The complete procedure as it was realised at the Institute of Plastic
Processing (IKV), Aachen, Germany, is shown in Figure 4.10. First of all a
complete 3D-calculation of the injection moulding process is carried out
using the SIGMASOFT package. In this context the geometry description
of the part geometry description of the part may be a CAD-model (e.g. *.stl
from SOLIDWORKS used in this thesis) or an adequate volumetric FEmesh. The results of this simulation step, i.e. fibre orientation, are then
mapped onto the FE-mesh for the acoustic analysis using the interface
SIGMAlink (Part of SIGMASOFT). Finally a routine called,”3D-
48
SIGMAmeetsABAQUS” which is developed at the IKV is used to calculate
the local anisotropic mechanical properties dependent on the local fibre
orientation and the measured material data concerning stiffness.
Material testing (stiffness
data of fiber and matrix)
CAD-Model
Micromechanical model
FE-Model 1
Properties of the unidirectional
reinforced composite
Adjustment according to
the state of orientation
Fiber orientation
link
Material model
CAD-Model
FE-Model 2
Acoustical
analysis in
ABAQUS
3D-SIGMAmeetsABAQUS
User-Subroutines for ABAQUS/Standard
Dynamic response
Figure 4.10. Concept for the complete 3D-design of short fibre reinforced
injection moulded parts.
To carry out the acoustic simulations ABAQUS/STANDARD was used as
the FEA program. However, a special user subroutine is needed to realize
the anisotropic stiffness analysis. Acoustic analyses were applied in
ABAQUS for the model plates.
49
4.2.3 Part Geometry in SOLIDWORKS
Two models consisting of the part, runner, inlet and mould were designed
in SOLIDWORKS. In the first model the runner is situated in the middle of
the smaller side of the plate as a “fish tail distribution system” (Figure 4.11)
while in the second model the melt runs to the mould by runner from one of
the corners of the model plate (Figure 4.12). This diversity in the position
of the runner leads to a very different melt flow in the models and therefore
leads to different fibre orientations in the model plates after injection
moulding.
(The models were saved in “stl” file format, which is a format readable in
SIGMASOFT.)
B
A
A= Part
B= Runner
C
C= Inlet
A= Part
B= Runner
C= Inlet
Figure 4.11. Model 1 designed in SOILDWORKS.
50
B
C
A
A= Part
B= Runner
A= Part
B= Runner
C= Inlet
C= Inlet
Figure 4.12. Model 2 designed in SOILDWORKS.
4.2.4 Injection Moulding Simulation in SIGMASOFT
As it is mentioned; the information about the local fibre orientation in the
part is the basic requirement for a precise acoustic design of injection
moulded parts made of short-fibre reinforced thermoplastics using the FEA.
In this section SIGMASOFT was used to simulate the injection moulding
process.
4.2.4.1 Preprocessing
•
Part Geometry
At first two projects were created, and then corresponding models,
geometries were imported to SIGMASOFT as “stl” files. Then the different
geometries were renamed to part, runner, inlet and mould. Afterwards the
materials were assigned to the different geometries each project. Then the
projects were ready for generating the meshes.
51
•
Enmeshment
In the advanced tab of the mesh generation of the enmeshment module in
SIGMASOFT, the plates were separated to the advanced meshing part
because the results on the model plates are more important than for the
mould, inlet or runner. Therefore the element number of the parts should be
bigger compared to the rest of geometries. In order to have a fine enough
enmeshment, the parameters for the accuracy, wall thickness, element size
and smoothing in option part was filled by appropriate values. The meshed
model plates with their runner and inlet parts are shown Figure 4.13 and
Figure 4.14 for the model 1 and 2, respectively. The number of elements for
the model plate 1 and 2 are about 278,000 and 168,000, respectively.
3
1
Figure 4.13. The enmeshment stage in SIGMASOFT for the model 1.
(278,264 part elements)
52
2
3
1
2
Figure 4.14. The enmeshment stage in SIGMASOFT for the model 2.
(168,181 part elements)
•
Simulation
The calculation can be started including the injection face of packing and
cooling and with the preparation for fast postprocessing.
•
Material definition
The material for the mould was selected from the standard library as steel
with the temperature of 70 o C . In order to assign the material for the part,
runner and inlet as a 30 % short glass fibre reinforced polypropylene
(POLYFORT-FPP 30 GF-C, Schulman, Kerpen- Germany), a material was
defined, due to the fact that this material is not available in the
SIGMASOFT library.
With the aid of the databases CADMOULD and MC-BASE the data
required for the material definition (30% Short Glass Fibre reinforced
Polypropylene) was extracted. MC-BASE is a material data base program
and CADMOULD is also an injection moulding simulation process
program which has a vast material database. These parameters include
rheological data, thermal properties and pvT properties which can be found
in the Appendix-D.
53
After defining and assigning the material to respected parts, the models
were ready to start the process simulation.
4.2.4.2 Postprocessing
After finishing the simulation the result can be checked in the
postprocessing module. The most interesting result is the fibre orientation
in the model plates that is not just unidirectional as the glass fibres are
distributed in different local fibre orientations, even in the wall thickness
direction.
The temperature filling stages are shown in Figure 4.15 for the model plate
1 and Figure 4.16 for the model plate 2.
40% filled
60% filled
80% filled
100% filled
3
1
2
Figure 4.15. Temperature filling stages of the model 1.
54
40% filled
60% filled
80% filled
100% filled
3
2
1
Figure 4.16. Temperature filling stages of the model 2.
The fibre orientation for the model plate1 is shown in Figure 4.17 and 4.18
in the middle and the outer layer of the wall thickness, respectively,
similarly Figure 4.19 and 4.20 illustrate the fibre orientation for the model
plate 2 in core and edge layers, respectively.
Figure 4.17. Fibre orientations in the core layer of the model plate 1.
55
Figure 4.18. Fibre orientations in the edge layer of the model plate 1.
Figure 4.19. Fibre orientations in the core layer of the model plate 2.
56
Figure 4.20. Fibre orientations in the edge layer of the model plate 2.
To have a better view Figures 4.21 and 4.22 show the section view of the
model plate 1 in thickness direction for fibre orientations in 1 and 2
direction, respectively. Considering Figure 4.21, most fibres are not laid in
1 direction and there are some regions in the middle of the wall thickness
that about 30 percent of fibres are turned in 1 direction.
Figure 4.22, proves this fact that most of the fibres in the shear layer tend to
lie parallel to the melt flow direction(more than 95 percent in 2 direction) in
contrast to the core layer in which the tend to turn to normal direction to the
melt flow (about 70 percent in 2 direction).
Studying the model plate 2 is also leads to the fact that the orientation of
the glass fibres mainly results from the complex melt flow during filling of
the mould cavity. In addition to different local fibre orientation over the
part fibre orientation also varies in the wall thickness direction.
Figures 4.23 and 4.24 illustrate the fibres orientation in 1 and 2 directions
for the model plate 2, respectively.
57
A
A
3
2
1
Figure 4.21. Fibre orientation in 1 direction of the model 1
(Section view AA).
A
A
3
1
2
Figure 4.22. Fibre orientation in 2 direction of the model 1
(Section view AA).
58
A
A
3
2
1
Figure 4.23. Fibre orientation in 1 direction of the model 2
(Section view AA).
A
A
3
2
1
Figure 4.24. Fibre orientation in 2 direction of the model 2
(Section view AA).
59
4.2.4.3 Result Extraction (SIGMAlink)
Before importing the results from SIGMASOFT, an ABAQUS input file is
required for each model that must consist of the geometry of the meshed
part.
Using SIGMAlink interface to translate data from SIGMASOFT to
ABAQUS and store this information based on ABAQUS input file.
In order to import data from SIGMASOFT, the ABAQUS input file was
prepared just for the plate, so just the data related to the plate must be
transferred with the same coordinate system in SIGMASOFT and
ABAQUS.
What is required from SIGMASOFT is the fibre orientation for the
completely filled stages, so all components of the orientation tensor were
imported. For translating data from SIGMASOFT elements to ABAQUS,
there are two methods in SIGMAlink. The first one is using the element
center that means only one result is written out for each element. The
second method is aiding the Gauss integration points, which is more
precise. For example , in hexahedral elements (our case) there are eight
Gauss integration points, therefore eight different results for each element
are written out, so that there is given a quite accurate orientation profile
over the element. On the other hand for hexahedral elements eight times
more RAM is required to store the orientation values in contrast to only one
result for each element.
4.2.5 JAVA Interface
After translating data into the ABAQUS plate geometry format, the next
interface is a JAVA execution program “ABAQUSmeetsSIGMA” that was
written in the IKV. The first part of the program is based on Halpin-Tsai
equation (Chapter 3.2.2) for calculating the stiffness tensor for the plate.
The input data required for the JAVA program are tabulated in Table 4.3.
The fibre volume fraction Φ f is calculated by Eq. 3.5.
60
Table 4.3. Data required for Halpin-Tsai equations.
E glass
fiber
E polypropylene
ν glass
72000 [Mpa]
1500 [Mpa]
0.2
fiber
ν polypropylene
0.35
Φf
0.129
So, at first the JAVA program calculates the stiffness parameters of a
unidirectional fibre reinforced composite by using the micromechanical
Halpin-Tsai equations (Table 3.2) and store them in a text file. Then using
Advani-Tucker orientation averaging method [11] the parameters in the
stiffness matrix of unidirectional fibre oriented composite are adjusted to
the degrees of fibre orientation for each Gauss integration point (for each
element).
This way the data required for the ABAQUS user material subroutine is
prepared, and can be used in the material definition part of preprocessing.
This data consist of the direction of the local coordinate system and the
stiffness coefficient that matches to the local coordinate system for each
Gauss integration point.
4.2.6 Acoustic Simulation in ABAQUS
As mentioned earlier, the acoustic simulation of the model plates can be
performed in ABAQUS. The simulation was done for three models: an
unreinforced polypropylene plate, model plate 1 and model plate 2.
4.2.6.1 Preprocessing
In this stage the models of the physical problems were defined and
ABAQUS input files (Appendix B and Appendix C) were created.
61
•
Part Geometry
The model plate is created in SOLIDWORKS and imported as a “stl” file to
ABAQUS (similar to the job done in Chapter 4.1.1). As it is shown in
Figure 4.1, it is a plate in feature of 112.5 mm length, 110.5 mm width and
2 mm thickness in which two corners of the model plate are filleted by a
radius of 12 mm.
•
Material Modeling
The user subroutine was written for ABAQUS in FORTRAN. The user
subroutine is based on the local coordinate systems and needs the stiffness
coefficient that matches to the local coordinate system for each Gauss
integration point. This information is stored in two different text files.
During the acoustic simulation in ABAQUS, the FORTRAN user
subroutine is called, in order to set up the local stiffness matrix for each
Gauss integration point.
Due to the fact that there was no method found for defining and applying
the local damping behavior for short fibre reinforced composites (at the
time of writing this thesis report), the value six is chosen and assigned as
the mass proportional damping factor (Alpha). In further studies this value
has proven suitable to define damping for plastic materials. The stiffness
proportional damping is not applicable together with a user material
subroutine definition in ABAQUS, so the Beta value has to be kept zero.
•
Enmeshment and Element type
The enmeshment and element type chosen are the same as those used in the
previous simulations (Chapter 4.1.1).
•
Step involved in the modeling
Two steps are assigned for this task:
1-Natural frequency extraction (by Lanczos eigensolver in the frequency
interval of 1~2000 Hz)
2-Steady-state dynamic response analysis (in the frequency interval of
1~2000 Hz)
62
•
Load and boundary conditions
The load and boundary conditions applied are similar to those used in
Chapter 4.1.1.
4.2.6.2 Postprocessing and Discussion
In the first part of this section natural frequencies and associated modes of
vibration are discussed, which give information about the deformation
behavior of the system corresponding to the eigenmodes. While in the
analysis of the steady state dynamics response, the effect of the harmonic
force on the displacement and velocity responses is investigated.
•
Analysis done in step-1 (Frequency extraction)
The first four mode shapes of the natural frequency extraction step with
corresponding undamped natural frequencies are shown in Figures 4.25,
4.26 and 4.27 for the PP plate, PP GF 30 model plate 1 and 2, respectively.
And also the first ten undamped natural frequencies are tabulated in Table
4.4 for these three plates.
Table 4.4. Natural resonance frequencies (Hz).
Mode No.
1
2
3
4
5
6
7
8
9
10
…
PP
48.642
88.742
300.49
341.78
370.34
597.05
843.20
852.03
915.28
1076.3
…
PP GF 30 Model1
70.029
117.16
380.40
447.47
511.13
754.93
958.25
1220.8
1229.3
1314.2
…
PP GF 30 Model2
54.684
104.88
340
425.83
477.64
750.74
955.31
1023
1235.9
1319.1
…
As it is obvious in Table 4.4, the undamped natural frequencies are shifted
to higher values from the PP plate to the model plate 2 and the the model
63
plate 1. For example the mode shape for the PP plate is laid on 48.642 Hz
in contrast to 54.684 Hz for the model plate 2 and 70.029 Hz for the model
plate 1. It declares the fact that for the first seven resonances the model
plate 1 behaves stiffer than the two others. The effect of reinforcement with
glass fibres on the stiffness tensor of the model palte1 and 2 is clear.
On the other hand, the contour plots of the deformed plate show how the
plate is deformed relatively. Figure 4.25 shows that opposite regions are
more deformed than the regions near by the fixed end. And also there are
other regions with zero deformation depending on corresponding
eigenform. The first and second mode shapes are similar in some ways but
the differences are started from the third mode shape where the third mode
shape for the PP plate is totally differed from the model plate 1 (Figure
4.26) and also this differences started for the model plate 2 from the fourth
mode shape (Figure 4.27).
Mode1
Mode3
at 48.642 Hz
at 300.49 Hz
Mode2
Mode4
at 88.742 Hz
at 341.78 Hz
2
3
1
Figure 4.25. Deformation of the PP model plate at the undamped
resonance frequencies.
64
Mode1
Mode3
at 70.029 Hz
at 380.40 Hz
Mode2
Mode4
at 117.16 Hz
at 447.47 Hz
2
3
1
Figure 4.26. Deformation of the PP GF 30 model plate 1 at the undamped
resonance frequencies.
Mode1
Mode3
at 54.684 Hz
at 340 Hz
Mode2
Mode4
at 104.88 Hz
at 425.83 Hz
2
3
1
Figure 4.27. Deformation of the PP GF 30 model plate 2 at the undamped
resonance frequencies.
65
•
Analysis done in step-2 (Steady state dynamics)
In this section the steady state dynamics response of the model plates
including material damping is achieved and the displacement, velocity and
acceleration responses obtained at the node of the applying of the harmonic
force are extracted.
The first four deformations of the PP plate, PP GF 30 model plate 1 and 2
at peak values of damped resonance frequencies are shown in Figure 4.28,
4.29 and 4.30 for the first four damped resonance frequencies.
at 301 Hz
at 49 Hz
at 89 Hz
at 342 Hz
Figure 4.28. Deformation of the PP model plate at the peak values
of the damped resonance frequencies.
66
at 380 Hz
at 70 Hz
at 117 Hz
at 448 Hz
2
3
1
Figure 4.29. Deformation of the PP GF 30 model plate at the peak values
of the damped resonance frequencies.
at 377 Hz
at 59 Hz
at 118 Hz
at 439 Hz
2
3
1
Figure 4.30. Deformation of the PP GF 30 model plate2 at the peak values
of the damped resonance frequencies.
67
Figure 4.31, 4.32 and 4.33 shows the displacement, velocity and
acceleration responses of the PP plate, PP GF 30 model plate 1 and 2 to the
harmonic force, respectively.
1.E+09
1.E+07
Response
point
1.E+05
1.E+03
1.E+01
1.E-01
1.E-03
Dis. [mm]
1
10
100
1000
Vel. [mm/s]
Acc. [mm/s2]
Frequency [Hz]
Figure 4.31. Displacement, velocity and acceleration responses vs.
frequency for the PP model plate.
1.E+09
1.E+07
Response
point
1.E+05
1.E+03
1.E+01
1.E-01
1.E-03
Dis. [mm]
1
10
100
1000
Vel. [mm/s]
Acc. [mm/s2]
Frequency [Hz]
Figure 4.32. Displacement, velocity and acceleration responses vs.
frequency for the PP GF 30 model plate 1.
68
1.E+09
1.E+07
Response
1.E+05
point
1.E+03
1.E+01
1.E-01
1.E-03
Dis. [mm]
1
10
100
1000
Vel. [mm/s]
Acc. [mm/s2]
Frequency [Hz]
Figure 4.33. Displacement, velocity and acceleration responses vs.
frequency for the PP GF 30 model plate 2.
In Figure 4.34, the effect of short glass fibres in reinforcing the plastic is
clearer precisely, where in the velocity response of the three models to the
harmonic force is compared. The first resonance frequency is shifted from
49 Hz for the PP plate to higher values for the model plate 2 and 1 with 55
Hz and 70 Hz, respectively.
For a better comparison between the model plate 1 and 2 responses, Figure
4.35 shows the velocity responses of the model plate 1 and 2 in the linear
scaling for the x axes. In this Figure, two resonance peaks are focused; at
the first resonance peak the model plate 2 is pursuing the model plate 1
with 15Hz frequency lag in contrast to the sixth resonance peak in which
the velocity peak in the model 1 is situated at 755 Hz while the same peak
response for the model 2 is laid on 790 Hz. These differences come from
the mode shape and the corresponding element of stiffness tensor of the
composite model that some times the model plate 1 shows stiffer than the
other and sometimes vice versa. So the fibre orientations play an important
role for the harmonic response of parts
Figures 4.36 and 4.37 compare the deformation of the first and sixth
response peak, respectively for the model plate 1 and 2.
69
1.E+05
Response
1.E+04
point
1.E+03
1.E+02
1.E+01
1.E+00
1
PP
10
100
1000
Model1
Frequency [Hz]
Model2
4.34. Comparison between the PP model plate, PP GF 30 model plate 1
and 2 velocity responses.
Resonance 6
Resonance 1
1.E+05
1.E+04
1.E+03
1.E+02
1.E+01
1.E+00
Model1
Model2
0
200
400
600
800
Frequency [Hz]
4.35. Comparison between the PP GF 30 model plate 1
and 2 velocity responses.
70
1000
Modelplate1
Modelplate2
at 70 Hz
at 49 Hz
2
3
1
Figure 4.36. Comparison of the deformation at the first resonance peak for
the model plate 1 and 2.
Modelplate1
Modelplate2
at 755 Hz
at 790 Hz
2
3
1
Figure 4.37. Comparison of the deformation at the sixth resonance peak for
model plate 1 and 2.
71
5 Conclusion and Further Works
The effect of anisotropy on the simulations of this thesis work shows that it
is possible to regard the local stiffness affected by the fibre orientation.
However due to lower damping behavior in the fibre orientation and higher
damping behavior in the transverse fibre direction, there is no precise
method for describing this damping behavior of short glass fibre reinforced
thermoplastics, at the time of writing this report.
Finite element method is a useful numerical method for modeling the
composites and also ABAQUS is suitable for modeling the steady state
dynamic analysis and extracts probably a more accurate result if the
injection moulding process is taken to account. This can be done by
simulation of the fibre orientations in a process simulation tool like
SIGMASOFT and exporting the resulting stiffness data to an ABAQUS
user material subroutine using micromechanical models.
Further work could take into consideration the following points;
•
Some experimental analysis can be done on the real specimens
that are available at IKV, in order to check and verify the results
from the simulations of this thesis.
•
Viscoelastic theory should be more refined to consider the
frequency dependent composite material behavior for stiffness
and damping.
•
A material model should be established that makes possible the
anisotropic simulation in ABAQUS.
72
6 References
1. Altenbach H., Altenbach J. and Kissing W., (2004), Mechancis of
Composite Structural Elements, Springer-Verlag Berlin Heidelberg.
2. Jones, Roger F., (1998), Guide to Short Fibre Reinforced Plastics,
Hanser Gardner publication.
3. Michaeli, W., (1999), Einführung in die Kunststoffverarbeitung.
München, Wien, Carl Hanser Verlag.
4. Auld, B. A., (1990), Acoustic Fields and Waves in Solids, Malabar
Krieger Publishing Company.
5. Fung, Y. C., (2001), Classical and Computational Solid Mechanics.
Singapore, World Scientific.
6. Norris, A. N., (1988), On the acoustic determination of the elastic
moduli of anisotropic solids and acoustic conditions for the existence of
planes of symmetry. Quarterly Journal of Mechanics and Applied
Mathematics. Vol. 42.
7. Tucker III, C.L. and Liang, E., (1999), Stiffness predictions for
unidirectional short-fibre composites, Review and evaluation,
Composite Science and Technology 59, S. 655 – 671, 1999.
8. Tandon, G.P. and Weng, G.J., (1984), The Effect of Aspect Ratio of
Inclusions on the Elastic Properties of Unidirectionally Aligned
Composites, Polymer Composites, Vol. 5, No. 4 S. 327 – 333, 1984.
9. Halpin, J.C. and Kardos, J.L, (1976), The Halpin-Tsai Equations: A
Review. Polymer Engineering & Science 16 5, S. 344 – 352, 1976.
10. Schmachtenberg E. Brandt M., (2005), Mechnische Auslegung von
kurzfaserverstärkten Spritzgussbauteilen vollständig in 3D.
11. Advani, S.G. and Tucker, C.L., (1987), The Use of Tensors to Describe
and Predict Fibre Orientation in Short Fibre Composites. In, Journal of
Rheology 31 8, S. 751 – 784, 1987.
12. Ramasamy, M. G., (1996), Application of Constitutive Modeling to the
Linear and Nonlinear Viscoelastic Behavior of Nitrile Rubber, Ph.D.
Dissertation,
73
13. Osswald, Tin A. and Menges G., (2003), Materials Science of Polymers
for Engineers, Hanser Gradner Publications, Inc., Cincinnati.
14. http://www.anasys.co.uk/library/dma1.htm 12, (2005).
15. Lakes, Roderic S., (1998), Viscoelastic Solids, CRC press.
16. Shabana, A.A., (1991), Theory of Vibration, Volume An Introduction,
Springer Verlag.
17. Petyt, M., (1998), Introduction to Finite Element Vibration Analysis,
Cambridge University Press.
18. Singh,A. G., (2003), Investigation of the Effect of Material Properties
on the Simulated Acoustic Behavior of Plastics Parts, RWTH-Aachen.
19. ABAQUS-6.5, DOCUMENTATION, 2005.
20. Ramaswami, S., (1979), Towards Optimal Solution Techniques for
Large Eigenproblems in Structural Mechanics, Ph.D. Dissertation, MIT,
1979.
21. SIGMASOFT Help Version 4.3, 2005.
74
A. ABAQUS input file for the polyamide
model plate
**Input file for Acoustic Simulation of a polyamide Model
Plate
*Heading
** Job name:polyamideAcoustic Sim:polyamidePlate
**
**PART Module **********************************************
**
*Part, name=PA Plate
*Node
1,
56.,
9.42900467,
0.
2,
56.,
46.,
0.
3,
5.1550765,
11.1808453,
0.
.,
.,
.,
..
.,
.,
.,
..
.,
.,
.,
..
3578,
-44.5250053,
51.9863625,
2.
3579,
-48.3500023,
51.9909096,
2.
3580,
-52.1749992,
51.9940681,
2.
*Element, type=C3D8
1,
31,
154,
11,
1,
2,
30,
155,
154,
3,
29,
156,
155,
926, 1049,
906,
896
31,
925, 1050, 1049,
926
30,
924, 1051, 1050,
925
.,
.,
.,
.,
.,
.,
.,
..
.,
.,
.,
.,
.,
.,
.,
..
.,
.,
.,
.,
.,
.,
.,
..
2512, 1930, 1929, 2684, 2683, 2825, 2824, 3579, 3578
2513, 1929, 1928, 2685, 2684, 2824, 2823, 3580, 3579
2514, 1928, 1800, 1927, 2685, 2823, 2695, 2822, 3580
*Nset, nset=_PeakedSet9, internal, generate
1,
3580,
1
*Elset, elset=_PeakedSet9, internal, generate
75
1,
2514,
1
** Region: (Section-1:Peaked)
*Elset, elset=_PeakedSet9, internal, generate
1,
2514,
1
** Section: Section-1
*Solid Section, elset=_PeakedSet9, material=Plastic
1.,
*End Part
**
**
** ASSEMBLY Module *****************************************
**
*Assembly, name=Assembly
**
*Instance, name=PA Plate, part=PA Plate
*End Instance
**
*Nset, nset=_PeakedSet4, internal, instance=Plate-1
2691,
*Nset, nset=_PeakedSet5, internal, instance=Plate-1
9,
10, 111, 112, 113, 114,
119, 120, 121, 122, 123, 124
115,
116,
117,
118,
.
.
.
2803, 2804, 2805, 2806, 2807, 2808, 2809, 2810, 2811, 2812,
2813, 2814, 2815, 2816, 2817, 2818
2819, 2820, 2821, 2822
*Elset, elset=_PeakedSet5, internal, instance=Plate-1
406, 422, 438, 454, 470, 486,
566, 582, 598, 614, 630, 646
502,
518,
534,
550,
.
.
.
2210, 2226, 2242, 2258, 2274, 2290, 2306, 2322, 2338, 2354,
2370, 2386, 2402, 2418, 2434, 2450
76
2466, 2482, 2498, 2514
*End Assembly
**
** Property Module *****************************************
** MATERIALS
**
*Material, name=PA Plastic
*Density
1.144e-09,
*Elastic, moduli=LONG TERM
380., 0.28
*Viscoelastic, frequency=TABULAR
0.0490263, -0.0609153,
0.0487705, -0.0557973,
0.001
0.0838516,
-0.409142,
0.0509866, -0.0549427,
10.011
0.0874009,
-0.444305,
0.0743564, -0.0806033,
20.021
.,
.,
.,
.,
.,
.,
.,
.,
.,
.,
.,
.,
.
.
.
0.235659,
-1.05676,
0.23572,
0.23578,
0.0844816,
-0.057756,
9979.98
-1.0572,
0.0845022, -0.0573199,
9989.99
-1.05765,
0.0845228, -0.0568842,
10000.
** --------------------------------------------------------**
** Step Module *********************************************
** STEP: FIND THE NATURAL FREQUENCY
**
*Step, name="FIND THE NATURAL FREQUENCY", perturbation
FIND THE NATURAL FREQUENCY
*Frequency,
eigensolver=Lanczos,
acoustic
coupling=on,
normalization=displacement, number interval=1, bias=1.
, 1., 10000., , ,
**
** Load Module *********************************************
77
**
** BOUNDARY CONDITIONS *************************************
**
** Name: CLAMPED Type: Symmetry/Antisymmetry/Encastre
*Boundary
_PeakedSet6, ENCASTRE
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field
*Node Output
A, U, V
**
*End Step
** --------------------------------------------------------**
** STEP: APPLYING STEADY STATE DYNAMICS
**
*Step, name="APPLYING STEADY STATE DYNAMICS", perturbation
*Steady State Dynamics, direct, frequency scale=LINEAR
1., 10000., 10000, 1.
**
** Load Module *********************************************
**
** BOUNDARY CONDITIONS
**
** Name: CLAMPED Type: Symmetry/Antisymmetry/Encastre
*Boundary
_PeakedSet5, ENCASTRE
**
** LOADS
78
**
** Name: CLOAD
Type: Concentrated force
*Cload, load case=1
_PeakedSet4, 3, 1.
**
** OUTPUT REQUESTS
**
**
** FIELD OUTPUT: F-Output-2
**
*Output, field
*Node Output
A, U, V
**
** HISTORY OUTPUT: H-Output
**
*Output, history
Model output
GA, GV
*End Step
79
B. ABAQUS input file for the PP GF 30
model plate 1
**Input file
ModelPlate1
for
Acoustic
Simulation
of
the
PP-GF-30-
*Heading
** Job name: PP-GF-30-Acoustic-Sim-model1: PP-GF-30-Plate
**
** PART Module *********************************************
**
*Part, name= PP-GF-30-Plate
*End Part
**
**
** ASSEMBLY Module *****************************************
**
*Assembly, name=Assembly
**
*Instance, name= PP-GF-30-Plate-1, part= PP-GF-30-Plate
*Node
1,
112.5,
40.102066,
2.
2,
66.465416,
43.9353981,
2.
3,
67.2839279,
0.,
2.
.,
.,
.,
.,
.,
.,
.,
.,
.,
.,
.,
.,
3462,
53.3212395,
102.945633,
0.
3463,
57.3190689,
102.886826,
0.
3464,
61.3423729,
102.828407,
0.
*Element, type=C3D8
1,
52,
149,
11,
2,
149,
150,
3,
150,
151,
1,
918, 1015,
877,
867
12,
11, 1015, 1016,
878,
877
13,
12, 1016, 1017,
879,
878
80
.,
.,
.,
.,
.,
.,
.,
.,
.
.,
.,
.,
.,
.,
.,
.,
.,
.
.,
.,
.,
.,
.,
.,
.,
.,
.
2428, 2180, 2181, 2597, 2596, 3046, 3047, 3463, 3462
2429, 2181, 2182, 2598, 2597, 3047, 3048, 3464, 3463
2430, 2182, 1785, 1786, 2598, 3048, 2651, 2652, 3464
*Nset, nset=_PeakedSet2, internal, generate
1,
3464,
1
*Elset, elset=_PeakedSet2, internal, generate
1,
2430,
1
** Region: (Section-1:Peaked)
*Elset, elset=_PeakedSet2, internal, generate
1,
2430,
1
**
*ORIENTATION, SYSTEM=USER, NAME=ORI
**
** Section: Section-1
*Solid Section, elset=_PeakedSet2, material=PP_30_GF_Model1,
ORIENTATION=ORI
1.,
*End Instance
**
*Nset,
nset=_PeakedSet19,
instance=ModelPlate1_Assem-1
3,
39,
40,
internal,
4,
9,
32,
33,
34,
41,
42, 109, 110
35,
36,
37,
38,
.
.
.
2633, 2634, 2635, 2636, 2637, 2638, 2639, 2640, 2707, 2708,
2709, 2710, 2711, 2712, 2713, 2714
2715, 2716, 2717, 2718, 2719, 2720, 2721, 2722
*Elset,
elset=_PeakedSet19,
instance=ModelPlate1_Assem-1
121, 122, 123, 124, 125, 126,
131, 132, 352, 379, 380, 381
81
127,
internal,
128,
129,
130,
382, 383, 384, 385, 386, 387,
392, 393, 394, 931, 932, 933
388,
389,
390,
391,
.
.
.
1747, 1748, 1749, 1750, 1751, 1752, 1972, 1999, 2000, 2001,
2002, 2003, 2004, 2005, 2006, 2007
2008, 2009, 2010, 2011, 2012, 2013, 2014
*End Assembly
**
** Property Module *****************************************
**
** MATERIALS
**
*Material, name=PP_30_GF_Model1
*Damping, alpha=6.
*DENSITY
1.14E-9
*USER MATERIAL, CONSTANTS=0
**
*DEPVAR
10
** --------------------------------------------------------**
** Step Module *********************************************
** STEP: FIND THE NATURAL FREQUENCY
**
*Step, name="FIND THE NATURAL FREQUENCY", perturbation
FIND THE NATURAL FREQUENCY
*Frequency,
eigensolver=Lanczos,
acoustic
coupling=on,
normalization=displacement, number interval=1, bias=1.
, 1., 2000., , ,
**
** Load Module *********************************************
**
** BOUNDARY CONDITIONS *************************************
82
**
** Name: CLAMPED Type: Symmetry/Antisymmetry/Encastre
*Boundary
_PeakedSet6, ENCASTRE
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field
*Node Output
A, U, V
**
*End Step
** --------------------------------------------------------**
** STEP: APPLYING STEADY STATE DYNAMICS
**
*Step, name="APPLYING STEADY STATE DYNAMICS", perturbation
*Steady State Dynamics, direct, frequency scale=LINEAR
1., 2000., 2000, 1.
**
** Load Module *********************************************
**
** BOUNDARY CONDITIONS
**
** Name: CLAMPED Type: Symmetry/Antisymmetry/Encastre
*Boundary
_PeakedSet5, ENCASTRE
**
** LOADS
**
** Name: CLOAD
Type: Concentrated force
83
*Cload, load case=1
_PeakedSet4, 3, 1.
**
** OUTPUT REQUESTS
**
**
** FIELD OUTPUT: F-Output-2
**
*Output, field
*Node Output
A, U, V
**
** HISTORY OUTPUT: H-Output
**
*Output, history
Model output
GA, GV
*End Step
84
C. ABAQUS input file for the PP GF 30
model plate 2
**Input file
ModelPlate2
for
Acoustic
Simulation
of
the
PP-GF-30-
*Heading
** Job name: PP-GF-30-Acoustic-Sim-model2: PP-GF-30-Plate
**
** PART Module *********************************************
**
*Part, name= PP-GF-30-Plate
*End Part
**
**
** ASSEMBLY Module *****************************************
**
*Assembly, name=Assembly
**
*Instance, name= PP-GF-30-Plate-1, part= PP-GF-30-Plate
*Node
1,
112.5,
40.102066,
2.
2,
66.465416,
43.9353981,
2.
3,
67.2839279,
0.,
2.
.,
.,
.,
.,
.,
.,
.,
.,
.,
.,
.,
.,
3462,
53.3212395,
102.945633,
0.
3463,
57.3190689,
102.886826,
0.
3464,
61.3423729,
102.828407,
0.
*Element, type=C3D8
1,
52,
149,
11,
2,
149,
150,
3,
150,
151,
1,
918, 1015,
877,
867
12,
11, 1015, 1016,
878,
877
13,
12, 1016, 1017,
879,
878
85
.,
.,
.,
.,
.,
.,
.,
.,
.
.,
.,
.,
.,
.,
.,
.,
.,
.
.,
.,
.,
.,
.,
.,
.,
.,
.
2428, 2180, 2181, 2597, 2596, 3046, 3047, 3463, 3462
2429, 2181, 2182, 2598, 2597, 3047, 3048, 3464, 3463
2430, 2182, 1785, 1786, 2598, 3048, 2651, 2652, 3464
*Nset, nset=_PeakedSet2, internal, generate
1,
3464,
1
*Elset, elset=_PeakedSet2, internal, generate
1,
2430,
1
** Region: (Section-1:Peaked)
*Elset, elset=_PeakedSet2, internal, generate
1,
2430,
1
**
*ORIENTATION, SYSTEM=USER, NAME=ORI
**
** Section: Section-1
*Solid Section, elset=_PeakedSet2, material=PP_30_GF_Model2,
ORIENTATION=ORI
1.,
*End Instance
**
*Nset,
nset=_PeakedSet19,
instance=ModelPlate1_Assem-1
3,
39,
40,
internal,
4,
9,
32,
33,
34,
41,
42, 109, 110
35,
36,
37,
38,
.
.
.
2633, 2634, 2635, 2636, 2637, 2638, 2639, 2640, 2707, 2708,
2709, 2710, 2711, 2712, 2713, 2714
2715, 2716, 2717, 2718, 2719, 2720, 2721, 2722
*Elset,
elset=_PeakedSet19,
instance=ModelPlate1_Assem-1
121, 122, 123, 124, 125, 126,
131, 132, 352, 379, 380, 381
86
127,
internal,
128,
129,
130,
382, 383, 384, 385, 386, 387,
392, 393, 394, 931, 932, 933
388,
389,
390,
391,
.
.
.
1747, 1748, 1749, 1750, 1751, 1752, 1972, 1999, 2000, 2001,
2002, 2003, 2004, 2005, 2006, 2007
2008, 2009, 2010, 2011, 2012, 2013, 2014
*End Assembly
**
** Property Module *****************************************
**
** MATERIALS
**
*Material, name=PP_30_GF_Model2
*Damping, alpha=6.
*DENSITY
1.14E-9
*USER MATERIAL, CONSTANTS=0
**
*DEPVAR
10
** --------------------------------------------------------**
** Step Module *********************************************
** STEP: FIND THE NATURAL FREQUENCY
**
*Step, name="FIND THE NATURAL FREQUENCY", perturbation
FIND THE NATURAL FREQUENCY
*Frequency,
eigensolver=Lanczos,
acoustic
coupling=on,
normalization=displacement, number interval=1, bias=1.
, 1., 2000., , ,
**
** Load Module *********************************************
**
** BOUNDARY CONDITIONS *************************************
87
**
** Name: CLAMPED Type: Symmetry/Antisymmetry/Encastre
*Boundary
_PeakedSet6, ENCASTRE
**
** OUTPUT REQUESTS
**
*Restart, write, frequency=0
**
** FIELD OUTPUT: F-Output-1
**
*Output, field
*Node Output
A, U, V
**
*End Step
** --------------------------------------------------------**
** STEP: APPLYING STEADY STATE DYNAMICS
**
*Step, name="APPLYING STEADY STATE DYNAMICS", perturbation
*Steady State Dynamics, direct, frequency scale=LINEAR
1., 2000., 2000, 1.
**
** Load Module *********************************************
**
** BOUNDARY CONDITIONS
**
** Name: CLAMPED Type: Symmetry/Antisymmetry/Encastre
*Boundary
_PeakedSet5, ENCASTRE
**
** LOADS
**
** Name: CLOAD
Type: Concentrated force
88
*Cload, load case=1
_PeakedSet4, 3, 1.
**
** OUTPUT REQUESTS
**
**
** FIELD OUTPUT: F-Output-2
**
*Output, field
*Node Output
A, U, V
**
** HISTORY OUTPUT: H-Output
**
*Output, history
Model output
GA, GV
*End Step
89
D. Material Data in SIGMASOFT for the
PP GF 30 model plates
Material type
plastic
Initial Temperature
240 o C
Lambda
0.27 W/mK
1390 J/kgK
CP
No-Flow-Temperature
130 o C
8.92 e+06 Pa s
Zero Shear Rate (dyn.) Visc. P1
Rheology
5202.40 s
Reciprocal Trans. Shear Rate P2
(Carreau
Exponent P3
0.74
WLF)
Reference Temperature T0
240 o C
parameters
Standard Temperature Ts
96.72 o C
Low Temperature Region
59525.8 bar cm3 /g
PF1
0.49 bar cm3 /g K
3142.82 bar
67465.30 bar
PF2
PF3
PF4
Transition Region
pvT
Schmidt
Coefficients
2.32e-07 cm3 /g
PF5
0.098 1/K
PF6
2.5719e-03 1/bar
PF7
High Temperature Region
46632.30 bar cm3 /g
PS1
0.70 bar cm3 /g K
1258.03 bar
51093.70 bar
PS2
PS3
PS4
Limit Transition
PK1
PK2
Fibre
General
Properties
Aspect Ratio
Geometry Parameter
Weight Fraction
Interaction Coefficient
90
134 o C
0.0223 o C/bar
25
0.997
15.00 %
1.00e-02
Department of Mechanical Engineering, Master’s Degree Programme
Blekinge Institute of Technology, Campus Gräsvik
SE-371 79 Karlskrona, SWEDEN
Telephone:
Fax:
E-mail:
+46 455-38 55 10
+46 455-38 55 07
[email protected]
Was this manual useful for you? yes no
Thank you for your participation!

* Your assessment is very important for improving the work of artificial intelligence, which forms the content of this project

Download PDF

advertisement