Optimization of dental implant using genetic algorithm

Abstract

The subject of the present work is optimization of the modern implant system Osteoplant, which was created and is still developed by Founda-tion of University of Medical Sciences in Poznań. Clinical observations point to the occurrence of both early and late complications in the case of all two-component implant systems. In many cases, these problems are caused by mechanical fractures of the implants themselves. The ob-tained results of the previous studies focused on necessary changes of the implant mechanical behavior, which helped to achieve the required long-term strength. However, modifications of the present dental implant system are not obvious. In this paper, an optimization of the Osteoplant dental implant system, with the use of FEA and genetic algorithms is discussed.

Full text

JOURNAL OF THEORETICAL
AND APPLIED MECHANICS
47, 3, pp. 573-598, Warsaw 2009
OPTIMIZATION OF DENTAL IMPLANT USING
GENETIC ALGORITHM
Tomasz Łodygowski
Krzysztof Szajek
Marcin Wierszycki
Poznań University of Technology, Institute of Structural Engineering, Poznań, Poland
e-mail: tomasz.lodygowski@put.poznan.pl
The subject of the present work is optimization of the modern impla nt
system Osteoplant, which was created and is still developed by Founda-
tion of University of Medical Science s in Poznań. Clinical observations
point to the o c c urrence of both early and late complications in the case
of all two-component implant systems. In many cases, these problems
are caused by mechanical fractures of the implants themselves. The ob-
tained results of the previous studies focused on necessary changes of
the implant mechanical behavior, which helped to achieve the required
long-term strength. However, modifications of the present dental implant
system are not obvious. In this paper, an optimization of the Osteoplant
dental implant system, with the use of FEA a nd genetic algorithms is
discussed.
Key words: design optimization, genetic algorithm, dental implant
1. Introduction
The use of implants is the commonly applied treatment method of dental re-
storations. The modern implant system Osteoplant was created and has been
developed by Foundation of University of Medical Sciences in Poznań since
over 10 years. The Osteoplant is a two-component implant system. It consists
of the abutment an d root, which are connected by a titanium screw. Clini-
cal observations point to the occurrence of both early and late complications
in the case of all two-component implant systems (Goodacre et al., 2003).
In many cases, these problems are caused by mechanical fractures of the im-
plants themselves (Hędzelek et al., 2004; Kąkol et al., 2002; Zagalak et al.,

574 T. Łodygowski et al.
2005). One of the most dangerous complications is fracture and cracking of
the dental implant parts. Damage of dental implant components makes further
treatment very difficult. The previous studies (Wierszycki, 2007; Wierszycki
et al., 2006a,b,c) confirmed fatigue as a reason of implant damage. The obta-
ined results of previous studies focused on necessary changes of the implant
mechanical beh avior, which helped to achieve the required long-term strength.
However, modifications of the present dental implant system are not obvious.
To find out a better design of the implant system, an optimization procedures
based on FEA must be used. In this paper, the optimization of the Osteoplant
dental implant system, with the use of FEA, genetic algorithms is discussed.
Fig. 1. Dental implant Osteoplant
Genetic algorithms (GAs) have received wide popularity as optimization
techniques during the last decades, in particular, for very complex designs
and they can successfully compete with gradient-based approaches in many
areas (Goldberg, 1989). GAs are stochastic search app roaches which rely on
the principle of survival of th e fittest in natural selection. Unlike conventional
optimization techniques, GAs explore simultaneously the entire design space
and, therefore, are likely to reach the global minimum. An improvement of
the global search process can be performed by incorporating neural networks
(NN) in optimization, which can learn and adapt changes over time. In general,
GAs require a lot computations (structural analyses in our case) and hence
high performance computing id eally addresses their needs, especially w hen
combined with NN.
In the created tool, the existing open source libraries have been used:
Galileo (for GA) and ffnet (for NN). The whole optimization procedure was
implemented with the use of Py th on scripting language. The FE model, nu-
merical analysis and post-pro cessing of results were performed with the use
of the Abaqus Unified FEA product suite from SIMULIA. The integration of
the GA and NN libraries with the FE tools was done by using the Abaqus
Scripting Interface (ASI).

Optimization of dental implant... 575
2. Model
The learning of a genetic algorithm and neutral n etwork needs a huge number
of an alyses to be carried out. For this reason, the crucial characteristic of
the numerical model of imp lant, which is used in optimization process, is
performed. In practice, the time of calculation can not exceed s everal dozen
minutes. This limitation causes that a fully three-dimensional m odel of an
implant and typical modeling approaches can not be used (Wierszycki et al.,
2006a). For this study, a special approach was proposed. A m odeling approach
described in detail below enables us to carry out a nonlinear, 3D simulation
of a dental implant in an acceptable time with a satisfactory level of accuracy
of the results.
Fig. 2. Numerical models of the implant: axisymmetric (a) and 3D (b)
A three-dimensional model of the implant has been created by revolving
an axisymmetric mod el ab out its axis of symmetry. The s ymmetric model
generation capability of Ab aqus/Standard enables one to create automatically
a three-dimensional model (Abaqus..., 2007a). The nodes, elements, section
definitions, material and contact definitions of the three-dimensional m odel
are created automatically based on the axisymmetric model description. Only
kinematic constraints and boundary conditions must be redefin ed . In order
to reduce the time of calculation, the asymmetric deformation of the three-
dimensional model was assumed to be symmetric w ith respect to the radial –
symmetry axis plane at an angle equal to 0 or 180
◦
. The symmetric results
transfer capability of the program and it was used to transfer the results from
the axisymmetric simulation of the assembly to the final three-dimensional
model (Abaqus..., 2007a).

576 T. Łodygowski et al.
2.1. Geometry
The geometry of the numerical model was simplified to the axisymmetric
description (Fig. 2). The internal threads of the implant body and screw were
simplified to axisymmetric, parallel rings. Because the main goal of this study
is the optimization of the screw connection, the external thread of implant bo-
dy was omitted. The parametric Abaqus/CAE m odel of the implant consists of
three axisymmetric parts. The shape of each of them corresponds to the cross-
section of dental implant components: abutment, body and screw. The 2D
sketches of this parts have fully parametric geometry description and are fully
constrained. These constraints with the dimensions and parametric equations
added to the sketch enable us to automatically modify the shape of implant
components (Abaqus..., 2007b). The six global independent parameters were
defined:
• screw head diameter,
• screw head conic surface opening angle,
• screw head height,
• hexagonal slot diameter,
• hexagonal slot height,
• hexagonal slot conic surface opening angle.
All parts share the same parameters, so the instances of the parts are
always consistent. The parameters are further coded in GA as gens (see Sec-
tion 3.2.2.).
The geometry of the three-dimensional model of the implant was not defi-
ned directly. The FE three-dimensional model is automatically created based
on the axisymmetric model (see Section 3.3.4).
2.2. Material
All components of an implant are made of medical alloys of titanium. For
general stress-strain analyses, isotropic and non-linear elastic-plastic charac-
teristics of material models were taken into account. The material properties
were based on the Certificates of Conformity and on literature (Wang, 1996).
The mechanical properties of titanium alloys are shown in Table 1. For fati-
gue calculations, the model of material has to be simplified to a linear elastic
description.
The material models and characteristic geometry definitions are automa-
tically trans ferred from the axisymmetric to three-dimensional model durin g
realization of the symmetric model generation p rocedure (Abaqus..., 2007a).

Optimization of dental implant... 577
Table 1. Mechanical properties of implant materials
Implant body Abutment Screw
Young’s modulus [MPa] 105 200 105 200 105 200
Poisson ratio 0.19 0.19 0.19
Yield [MPa] 615.2 832.3 802.8
Tensile Yield [MPa] 742.4 1004.0 970.4
2.3. Assembly and contact
The assembly is done at the first axisymmetric stage of creation of the
implant model. The three two-dimensional instances of implant parts were
positioned relative to each other in a global coordinate system. Relative posi-
tion constraints were applied to align with:
• conic surface of hexagonal slot and outside of abutment,
• conic surface of screw head and inside of abutment.
Fully relative position constraints of implant part instances make possible
automatic redefinition of the implant model assembly (Abaqus..., 2007a). The
assembling simulation involves solving a contact problem (Wierszycki et al.,
2006b). For this pu rpose, it is necessary to define three contact areas, between:
• root and abutment,
• root and screw,
• abutment an d screw.
This contact conditions produce typical assembly problems, so we decided
to use a standard small-sliding contact formulation. In order to minimize the
dependence on mesh density, the surface-to-surface contact discretization was
used. Significant penetrations of master nodes into the slave surfaces do not
occur with the used space discretization. Moreover, surface-to-surface d iscre-
tization provides more accurate stress and pressure results, especially in the
cases of contacts at corners like on the threads. In some situations, the surface-
to-surface discretization approach can generate additional solution costs (Aba-
qus..., 2007a). The reason for this is that more nodes per each constraint are
involved. In this particular application, the surface-to-surface discretization
approach significantly reduces the solution cost. For a three-dimensional mo-
del with two cylindrical elements in 180
◦
segment, the node-to-surface di-
scretization causes a double increase in the number of increments and sever
discontinue iterations. There are no significant differences in time of calcula-
tion depending on th e method of contact constraint enforcement. The penalty

578 T. Łodygowski et al.
method as the contact constraint enforcement method was selected for both
normal and tangential directions. Tangential surf ace behavior was defined as
the classical isotropic Coulomb friction model. The friction coefficient is the
same for all contact pairs and amounts to 0.19. The definitions of contact pa-
irs are automatically transf erred from the axisymmetric to th ree-dimensional
model in the symmetric model generation procedure (Abaqus..., 2007a).
2.4. Loads
The loading of the implant model is a two-step pr ocess. The first step
corresponds to simulation of a tightening process. In this step, both model and
its response are axisymmetric. Th is simulation can be carried out with the use
of the axisymmetric model. The second step is bending, which is caused by
the worst component of service load, perpendicular to the axisymmetric axis.
In this case, the model which can describe asymmetric deformation is needed.
For a two-component implant, one of the most crucial aspects of numeri-
cal mo deling is simulation of the mechanical assembly subject to tightening
of the implant screw (Lang et al., 2003; Wierszycki et al., 2006c). For the
axisymmetric or a simplified three-dimensional model, tightening s imulations
cannot be performed as a real physical p rocess. A work-around of this ap-
proach is necessary. For simulation of tightening, a prescribed assembly load
has been used. The middle part of the s crew was defined as pre-tension sec-
tion. The tightening load (150 N) was applied to the pre-tension section as a
concentrated load. During calculation, the screw length was reduced in this
pre-tension section to achieve th e assumed tightening force. T he implant body
and abutment were tightened as results of the change of screw length. The
value of axial force in the tightened s crew was calculated from the empirical
formulation (Bozkaya and M¨uf¨ut, 2005; Lang e t al., 2003; Merz et al., 2000). I t
depends on the friction coefficient and torque. This assumption and procedure
of tightening were verified during full simulation of screw tightening with the
help of a fully three-dimensional FE model of an implant (Wierszycki e t al.,
2006c). The results obtained in the axisymmetric simulation were transf ered
into th e final thr ee-dimensional model. The second step was bending of the
tightened implant. The bending force was applied to the tip of ab utment by
means of the concentrated load (10 N) perpendicular to the axisymmetric axis
of the implant.
2.5. Mesh
For all parts of the model, a quad-dominated shape of elements was used.
At each edge of the mesh region, the seed (approximated node locations) has

Optimization of dental implant... 579
been defined to control mesh d en s ity. Correct mesh density must be ensured for
different geometry configurations. The seeds have been defined by s pecifying
average element sizes along the edges. To ensure the proper mesh density
for d ifferent geometry configurations, the seed densities have been partially
constrained. Th is app roach ensured that even if the number of elements along
the edge was changed its size remained such as had been defined (Abaqus...,
2007b).
The mesh of the three-dimensional model was generated automatically in
the symmetric m odel generation procedure. In whole model of implant, CCL9
and CCL12 elements were used (Abaqus..., 2007a). The cylindrical elements
available in Abaqus/Standard use standard isoparametric interpolation in the
radial-symmetry axis plane, combined with trigonometric interpolation fu nc-
tions with respect to the angle of revolution. Cylindr ical elements can span
angles between 0 and 180
◦
. The cost of calculation was significantly reduced
by this fact itself. The number of cylindrical elements along the circumf eren -
tial dir ection is the compromise between time of calculation and accuracy of
the results. Five tests were carried out to evaluate which number of elements
is optimal. The models with three-dimensional solid element C3D8 and C3D6
were used as reference solutions. In the models, 32 and 16 elements per 180
◦
segment were used. The maximum values of the equivalent Mises stress at
characteristic n otches and global bending stiffness of the whole implant struc-
ture were used to compare the results. T he comparison of computations for
different models are shown in Fig. 3. Detailed results of comparable studies are
shown in Table 2. Because there are no significant differences in the results for
two- and four-cylindrical elements, two elements were used in the optimization
process. This approach enabled us to describe nonlinear asymmetric deforma-
tion for axisymmetric geometry and simultaneously s ignificantly reduced size
of the prob lem (ca. 94 000 dof) in comparison with the fully three-dimensional
model (ca. 600 000 dof).
Fig. 3. The Wallclock time for 3D analyses with the use of cylindrical (CCL-x) and
3D s olid ele ments (C3D-x)

580 T. Łodygowski et al.
Table 2. S elected parameters of comparable 3D simulations with the use of
cylindrical (CCL-x) and 3D solid elements (C3D-x)
Float. point Minimum Required Number Number Number Wall-
operations memory disks- of equa- of incre- of itera- clock
per itera- required diskspace tions ments tions time
tion [–] [MB] [MB] [–] [–] [–] [s]
CCL-1 6.51 · 10
9
47.31 150.73 56226 7 40 160
CCL-2 2.81 · 10
10
87.25 366.96 93588 7 45 401
CCL-4 1.61 · 10
11
176.93 1034.24 168312 9 62 1565
C3D-16 9.48 · 10
11
447.38 2969.60 317760 13 104 8730
C3D-32 5.15 · 10
12
1157.12 8427.52 616656 13 109 47685
3. Dental implant optimization
The optimization of the presented dental implant is a very complex problem.
The m odel, which is the basis (starting point) for the optimization, is well
developed. It estimates the implant behavior giving consideration to material
nonlinearity, complex contact definition and prestress of the assembly screw.
The level of complexity and large number of design parameters result in many
local minima in the design space. Thus, the optimization algorithm has to
search for the optimal solution globally, based on a limited set of solutions
in the design space. Moreover, a few problems with FE analysis can occur
and should be taken into account. The most frequent ones are rebuilding and
no-convergence problems. The complexity of geometry and large number of
design parameter combinations makes it impossible to predict all problems
with the geometry. As a consequence, for some configurations of the design
parameters which are in the feasible region, the proposed shape is incorrect.
Additionally, the problem with mesh generation can occur, which can be also
treated as a rebuild problem. Reasons for no-convergence are usually caused by
too large plastic strain or contact problems. Both can occur for points in the
feasible region of the design space and have to be expected during optimization
process.
One of the optimization algorithms which can fulfill all these requirements
is a genetic algorithm. In th e presented optimization, a classic binary form
with two genetic operators: crossover and mutation is used.

Optimization of dental implant... 581
3.1. Genetic algorithm (GA)
The genetic algorithm has been inspired by evolutionary biology and in-
corporates techniques such as inheritance, mutation, selection and crossover to
find a better solution. The most important advantages of the genetic algorithm
over classic methods of optimization is that it works basing on the problem
solution instead of analytical relations. It can optimize linguistic variables and
use parallel computing by nature. Despite being a powerful optimization tool,
the genetic algorithm uses simple rules, which makes it easy to implement. In
the module presented in this work, the galileo (GPL) library was used.
Fig. 4. Scheme of genetic algorithm processing
A genetic algorithm operates on individuals which are abstract represen-
tations of a real solution. Each individual contains a set of encod ed design
variables, which is called a chromosome. The binary enco ding is a very classic
one and is also u sed here. The range and number of bits was set for each de-
sign parameter. The string repr esenting a chromosome was constructed over
the alphabet {0, 1} and can be symbolically represented as follows
A = a
1
a
2
a
3
. . . a
i
. . . a
l
(3.1)
In equation (3.1), a
i
represents a particular bit, an element from alphabet,
at the position i, and l denotes the total string length. In order to collect
chromosomes with similar features, we can introduce a schema. The schema is
constructed over an extended alphabet of three symbols {0, 1, ∗}, where ∗ is
do not care symbol. The schema can be symb olically r ep resented as fallows
H = h
1
h
2
h
3
. . . h
i
. . . h
l
(3.2)
h
i
denotes a particular element from the extended alphabet at the position i,
and l represents the schema length. Th e order of schema H, denoted by o(H)

582 T. Łodygowski et al.
represents the number of fixed positions, in this case, 0’s and 1’s, whereas
length, denoted by δ(H) is the distance between the first and the last fixed
position. The chromosome matches the s chema if for i ∈ h1, li, h
i
= a
i
or
h
i
= ∗. Each schema H can be described by the order and the length.
The main idea of GA processing consists in generation of a set of initial
solutions and use of evolutionary operators to improve them in successive
iterations, called generations. An initial set of individuals, called the initial
population, is usually randomly created. Every new population is subjected
to evaluation. The evaluation process consists of assigning a fitness value to
each individual. The fitness value describes solution quality and is calculated
according to an objective function and results of FE analyses.
Denoting the fitness value of th e j-th individu al matching the schema H
by f
H
j
and their number after t-th iteration by m(H, t), the average fitness
value for the schema H after t -th iteration can be represented as follows
f(H, t) =
P
f
H
j
m(H, t)
(3.3)
whereas the average fitness value of entire population may be given by
f =
P
f
j
n
(3.4)
The population size and j-th representation of individuals is denoted by n
and f
j
, respectively.
Fitness values are the b asis for the selection process. The selection mecha-
nism watches over the improvement of the next population quality. During
selection, statistically only the most fitted individuals are chosen in order to
allow them to take part in creation of the next population. The probability
of choosing the particular in dividual in a single trial using the wh eel-roulette
selection method can be given by the following equation
p
i
=
f
j
P
f
j
(3.5)
Assuming that the numb er of a s elected individual has to be equal to the po-
pulation size, the expected number of in dividuals which match the schema H
in the t + 1 population is as follows
m(H, t + 1) = m(H, t)
f(H, t)
f
(3.6)
The number of schema H representatives in the next population grows with
the ratio of the average value of the schema to the average fitness of the entire

Optimization of dental implant... 583
population. Thus, the s chema with a higher average fitness is more strongly
promoted. Moreover, one should expect that the number of individuals mat-
ching the schema will grow if their average value is higher than the whole
population average value.
In the next stage, the selected individuals are subj ected to crossover and
mutation. The operators use selected chromosomes in order to create new
design parameter configurations. The primary function of crossover is to m ix
the parent individual chromosomes and create a n ew couple of offsprings. The
crossover proceeds with a probability defined by th e crossover rate p
c
. The
moderation of crossover prevents premature convergence getting stuck in a
local minimum. I n a classic form, crossover consists of sampling a chromosome
partition point, dividing parent chromosomes and swapping obtained parts
between them. The crossover improves the population d iversity but on the
other hand reduces individuals, which match the schema H regardless of their
fitness. The probability of survival of the scheme H, in spite of crossover, can
be defined as follows
p
s
= 1 − p
c
δ(H)
l − 1
(3.7)
In the equation above, l denotes the chromosome length.
Mutation is responsible for random distortion of chromosomes. Random
distortions keep diversity of the population on a sufficient level and help to
escape from a local minimum. In binary encoded chromosomes, mutation sam-
ples a gene and changes its value to the opposite. The intensity of mutation
is controled with the mutation rate p
m
. Similar to crossover, mutation can
destroy individuals matching the schema H. In the case of mutation, the pro-
bability of H schema representative survival can be given by the equation
p
s
= 1 − o(H)p
m
(3.8)
Summing up the effect of three operators: selection, mutation and cros-
sover, the expected number of representatives of the schema H in the next
population can be given as follows
m(H, t + 1)  m(H, t)
f(H, t)
f
h
1 − p
c
δ(H)
l − 1
− o(H)p
m
i
(3.9)
In the last stage, the n ew population rep laces the previous one. Usually,
the genetic algorithm ends when either the maximum fitness value for the
best fitted individual is obtained or the maximum number of generations is
achieved. A general chart-flow of the genetic algorithm is presented in Fig. 4.

584 T. Łodygowski et al.
3.2. Definition of the optimization problem
3.2.1. The goal
The present study is expected to find a new dental implant shape. The
shape should lead to lower principal stresses in comparison with the curren-
tly encountered values. In the presented FE model, geometry and material
properties are similar to a real dental implant. The loads which were app lied
come from (Zagalak, 2003) and are recognized as test loads. For the presented
configuration, the maximum principal stresses are greater than 625 MPa and
are localized in the screw corner (Fig. 5).
Fig. 5. Huber-Mises stress in the initial design of a dental implant
In spite of looking for a new proposal of shape, an other goal is verification
of the used numerical method. The study should provide an answer to the
question wether this methodology can be used in further improvement of the
dental implant design.
The genetic algorithm tries to find the most fitted individual with the h i-
ghest fitness value. In the case of minimization problem, the obj ective function
has to be modified in order to evaluate individuals. In the present work, the
fitness function was defined according to the equation
f(X) =

1
σ
max
maxPrinc

2
c (3.10)
where X = [A, B, C, D, E, F ] and c = 10
9
.
The value of σ
max
maxPrinc
represents the maximum principal stress in the
upper part of the implant and the vector X denotes configuration of design

Optimization of dental implant... 585
parameters. An additional multiplier c was used in order to prevent obtaining
values smaller than machine precision.
3.2.2. Design parameters
Geometry of the presented two-component implantology system is qu ite
complex and the choice of correct design parameters is crucial. The thread
was excluded from consideration at this stage of the study. Six geometrical
parameters were defined as real variables (Fig. 6). All of them refer to the
upper part of the imp lant.
Fig. 6. Design para meters
The design parameters were encoded into a binary string. There were d e-
termined for each design parameter range and number of bits for encoding.
The ranges come from both th e geometry limitations and manufacture requ-
irements, and are listed in Table 3.
The larger numb er of bits for encod ing, th e better accuracy. On the other
hand, however, the total time of optimization substantially increases. The
decision on the number of bits is always a compromise between time and
required accuracy. In the present case, for angle variables four-bit strings were
constructed, whereas for all the rest only three bits were used. The choice of
particular design parameters was based on th e range and expected influence
on final results. The obtained resolution of the design parameter d, can be
calculated as follows
d
π
=
d
max
− d
min
2
n
− 1
(3.11)

586 T. Łodygowski et al.
Table 3. Range and number of bits for design parameter encoding
Name Symbol
Min Max
Range Bits
Reso-
value value lution
Screw head diameter A 0.95 1.6 0.65 3 0.093
Screw head conic
B 0.0 80.0 80.0 4 5.33
surface openin g angle
Screw head height C 1.5 6.4 4.9 3 0.7
Screw diameter D 1.0 1.5 0.5 3 0.071
Hexagonal slot height E 0.05 2.65 2.6 3 0.371
Hexagonal slot conic
F 11.0 90.0 79.0 4 5.27
surface openin g angle
where d
max
, d
min
denotes the maximum and minimum limit for the variable
for string length equal to n .
All th e binary strin gs reference to the design variables and are joined in a
chromosome. In the present work a twenty bit string is used as below
ch
i
= [g
A
1
, g
A
2
, g
A
3
|g
B
4
, g
B
5
, g
B
6
, g
B
7
|g
C
8
, g
C
9
, g
1
0
C
|g
1
1
D
, g
1
2
D
, g
1
3
D
|
(3.12)
g
1
4
E
, g
1
5
E
, g
1
6
E
|g
1
7
F
, g
1
8
F
, g
1
9
F
, g
2
0
F
]
The superscripts denote design parameters s ymbols in accordance with Ta-
ble 3.
3.2.3. Constraints
The material used in the FE model s imulates the elasticplastic behavior.
To some extent, it is allowed to exceed the plastic stress limit in the dental
implant but the plastic strain can not be too large. In FE analysis, it is assumed
that the maximum equivalent of plastic strain can not be higher than 10%.
The equivalent plastic strain can be calculated as
ǫ
pl
= ǫ
pl


0
+
t
Z
0
r
2
3
˙ǫ
pl
: ˙ǫ
pl
dt (3.13)
where ǫ
pl


0
denotes initial equivalent strain, which was equal zero, whereas
˙ǫ
p
l denotes the equivalent plastic strain rate. The principal stress red uction,
which was set as the goal, directs ch anges in in dividual in the opposite direction
to this constraint. Thus, no stress or plastic strain constraints were necessary.
In the case of rebuild or convergence problem, the death penalty method is
applied. The individual is eliminated fr om further processing.

Optimization of dental implant... 587
3.2.4. The genetic algorithm
In the evaluation of a single individual, the FE model of the dental imp lant
which is timeconsuming significantly limits the population size. On the other
hand, the population has to be large enough to provide suffi cient diver sity and
represent the design space properly. In the pr esent work, a forty-individual
population was used. The number of epochs was not limited a priori. The
optimization was stopped , based on monitored results. The signal to brake the
procedure was sent after a few epochs without any new proposal for better
solution.
The first population was randomly created. Moreover, because of the death
penalty method constraints, individuals in the first population were genera-
ted and checked as long as the whole population of correct individuals was
not achieved. The procedure prevents starting from individuals, which will be
eliminated in the second generation.
The ranking-based method of selection was used. T his type of selec-
tion consists in sequential arrangement of individuals accor ding to their fit-
ness and assigning to each i-th individual in the range from r
min
i
to r
max
i
where
r
min
0
= 0 r
min
i
= r
max
i−1
r
max
i
= r
min
i
+
p
i
P
n
j=0
p
j
r
max
n
= 1.0
(3.14)
In the above equations p
i
and n denote the position in the ranking and the
population size, respectively. During the selection, a value between 0 and 1 is
randomly generated and indicates the individual which refers to the range in
which the value is included. In contrast to the classic method of selection, i.e.
roulettewheel, this method sets probability of being selected according to th e
position in the ranking instead of the fitness. As a consequence, the probability
of choosing an individual w ith much lower fitness than the maximum one
increases and results in higher diversity in the late stage of the optimization
process.
The onepoint crossover method is applied. The selected individuals are
joined into couples, their chromosomes are divided into three substrings at
random positions and swapped between parent ind ivid uals. A new couple
of offsprings r ep resents combinations of both parent features. In order to
keep diversity on a sufficient level during the optimization process, not all
couples are subjected to crossover. The intensity of crossover is determined
with the crossover rate, which is constant and equal to 0.75 in the present
work.

588 T. Łodygowski et al.
In the last stage of recombination, random distortions are introduced to
chromosomes. The probability of each gene distortion is controlled by the
mutation rate. In the present work, the constant value of 0.02 during th e
whole optimization process was kept. When a gene is selected to mutation its
value is changed to opposite one, from 0 to 1 and vice versa.
The classic form of population replacement was used. The whole previous
population was replaced w ith the new one completely. This method allows for
increasing the diversity and search through the design space more extensively
in comparison with alternative methods, e.g. steadystate replacement. Unfor-
tunately, at the same time, it moderates the convergence and increases the
number of necessary FE analyses. The small population size, which was used,
limited the variation of the design parameters, therefore the diversity was an
important factor.
3.3. Incorporation of the genetic algorithm into Abaqus/CAE
The genetic algorithm processes chromosomes which represent various
combinations of design parameters. Each new chromosome has to be evalu-
ated in order to assess its quality. A great advantage of the genetic algorithm
is that the evaluation process can be fully elaborated in an exterior proce-
dure. The procedure return s fitness values based on chromosomes. The tool
employed in the evaluation procedure has to provide possibility to rebuild the
FE model for any design parameter configuration. Moreover, some procedures
like meshing has to be created automatically. Thus, the reliability and capa-
city of the rebuilding tool are crucial. In the present work, the Abaqus/CAE
environment in cooperation with Abaqus/Standard code is used.
3.3.1. Optimization module for Abaqus/CAE
Abaqus/CAE provides an efficient environment for user scripting. The
object-oriented scripting language, called python is available. The user can
add new procedures into the kernel and graphical user interface (GUI) as well.
In order to carry out the dental implant optimization, a new mod ule has been
created with a fully functional graphical user interface (Fig. 7).
The optimization driver was imported as an external library into Aba-
qus/CAE environment. The open source library called galileo was used. The
implemented module was divided into two main sections. The first one orga-
nizes genetic optimization and employes galileo library mostly, whereas the
second provides a tool for chromosome evaluation.

Optimization of dental implant... 589
Fig. 7. Optimization module for Abaqus/CAE
3.3.2. Individual evaluation
Every chromosome created in the reprod uction process is a starting point
for the evaluation procedure. In the first stage, each i-th chromosome is di-
vided into substrings w hich refer to the design parameters. Next, each binary
substring is decoded into an integer value e
j
and i-th design parameter is
calculated with the given equation
d
j
= e
j
d
max
j
− d
min
j
2
n
− 1
(3.15)
In the equation above, the symbol n denotes the substring length. Finally,
a set of real design parameter values is obtained and provides the basis for
model rebuilding.
All design parameters refer to geometry of the dental implant. Aba-
qus/CAE kernel script is created and run in order to change them in the
model. The obtained geometry is controlled and if the shape is invalid, the
rebuild error is raised. The weakest point of the procedure is the creation of
a mesh. The mesh is generated automatically and due to the large number of
analyses it is not possible to control it manually. It is assumed that any er-
ror in the mesh result in higher principal s tresses and eliminates the solution
during selection. Based on the modified geometry, the FE analysis definition
is created and sent to the Abaqus/Standard solver. In the case of the pre-
sent work, an additional analysis has to be carried out to provide results for

590 T. Łodygowski et al.
the axisymmertic model. The spatial dental FE model was built based on the
results for axisymmetric one and add itional data such as lateral force magnitu-
de. The module waits for analysis termination until the maximum time is not
exceeded. In the case of too long analysis, the solver stops an d no convergence
error is raised. This limitation can also eliminate well fitted solutions but is
necessary to proceed the optimization.
The analysis resu lts and all information abou t its proceeding is stored in
an output database, which can be read with the use of the python script. All
necessary information is extracted from the output database and the objective
function is calculated . Finally, the fitness value returns to th e optimization
driver. The whole flow chart of the individual evaluation procedure is presented
in Fig. 8.
Fig. 8. I ndividual evaluation procedure
In the case of the rebuild error, the zero fitness value is returned for an
individual. The zero fitness value guarantees that invalid solution will be eli-
minated during the selection process.
3.3.3. Parallelization
Genetic processing generates a large number of s olutions that have to be
checked. Taking into account the time of a single FE analysis, the total time of
optimization (compu tations) is a frequent limitation. The sin gle analysis of the
presented FE model took 5 to 40 minutes and a large spread was caused by the
nonlinear behavior. Because the time of analysis is significant, the algorithm
was modified to support parallel analyses. During the evaluation stage, the
optimization d river waits for fitness values of all individuals. T he population
is divided into s ubgroups according to available resources. In the work, an

Optimization of dental implant... 591
eight-processors mach ine was us ed to determine the number of individuals,
which were evaluated simultaneously. For each ind ividual in a group, an FE
analysis defi nition is prepared. Next, all analyses are submitted simultaneously
and the longest one determines the time which is necessary for evaluation of
the whole group. T he obtained results are the basis of fitness calculation. They
are returned to the optimization driver. The procedure is presented in Fig. 9.
Fig. 9. Scheme of genetic algorithm evaluation processing
3.3.4. Procedure of building of an FE implant model during the optimization process
The procedure of building of an FE imp lant model during the optimization
process is schematically show n in Fig. 10. At the beginning of the optimization,
the Ab aqus/CAE file with the fully parametric axisymmetric model of the im-
plant is opened. This model was described in details before (Section 2). When
the optimization loop is started, the axisymmetric model of the implant is
modified. The Abaqus/CAE creates an INP file with a modified axisymmetric
model of the implant and the Optimization Module sub mits jobs. The results
of these axisymmetric simulations are assembled in the implant structure. In
the next step, the optimization module generates PARAM files and simul-
taneously runs three-dimensional jobs. The INP file of the three-dimensional
model contain the definition of symmetric model generation procedure, and
the second step of implant simulation is manually prepared. The PARAM files
are created based on inf ormation from axisymmetric ODB fi les and options
which are defined at the beginning of the optimization procedure. These files
contain parameters of three-dimensional models of th e implant:
• segment angle thr ough which the cross-section is to be revolved,
• number of elements to be used in the segment,

592 T. Łodygowski et al.
• offset for element numbering,
• offset used for node numbering,
• global number of node in the axisymmetric model.
Fig. 10. The procedur e of building of an FE implant model during the optimization
process
Finally, th e results of three-dimensional simulations are read from ODB fi-
les and the Optimization Module can start the Genetic Algorithm process. This
procedure must be repeated for each population. The described modeling ap-
proach with the use of axisymmetric geometry description and semi-analytical
discretization enable us to carry out a large number of implant simulations in
a realistic time period and to carry out the optimization.
3.4. Results
The optimization was performed using 8 cpus in computations (Fujitsu-
Siemens PRIMERGY TX300 S3). During the whole optimization process over
1600 FEA analyses were curried out. The total time of optimization was ca.
250 hours.
The evolution of the optimization process is presented in Fig. 11. It shows
changes of the maximum principal stresses in the upper part of the implant

Optimization of dental implant... 593
screw for successively generated solutions. The average value of the principal
stress is drawn by the solid curve. It can be observed that the designs are
being improved - the maximum principal stress is decreasing. Starting with an
value of 625 MPa, the principal stress is reduced dow n to 150 MPa. The graph
does not consist of the first stage when th e initial population was established.
More than 320 FE analyses were necessary to find forty correct individuals.
Starting with the fir s t population of r an dom individuals yields better solution.
Moreover, the reduction of pr incipal stress is meaningful and equals 475 MPa,
what is more th an 75% of the initial value. In the next generations, the design
parameters from the best solution (peaks) were promoted stronger and thu s
they strongly influenced the population improvement. It r esulted in constant
decreasing of both average and minimum value of principal stresses. After the
20th generation, the best solution was established and no furth er essential
reduction of stress was observed. Because of the chosen reproduction strategy,
the diversity within population was kept on a sufficient level and even in the
last monitored population the individu als represented a wide range of fitness
value.
Fig. 11. Fitness value for sucessively g e nerated individuals
Two proposals of new shapes are shown in Fig. 12. The lowest principal
stress was obtained for shape (b) and equaled 150 MPa. The next proposal
(Fig. 12c) provides reduction down to 180 MPa but still has a hexagonal slot
instead of the most optimal solution. The haxagonal slot plays an important
role in preventing screw loosening, thus solution (b) will not be considered
in further analyses. T here are a few clear tendencies easy to observe. In the
first place, the screw head is wider than the initial one and the opening angle

594 T. Łodygowski et al.
of the screw head conic surface is moderated. Together w ith modification of
the opening angle of the hexagonal slot, the conic surface makes clamping
of the abutment and the body more efficient. Moreover, moderation of the
opening angle of the screw head conic surface reduces stress concentration in
the interior corner of the screw.
Fig. 12. Initial (a) and new (b, c) shapes of dental implant
All the modifications make the joint stiffer and reduce relative rotation
between the abutment and the body. The implant starts to behave as a canti-
lever (Fig. 13). The final implant incorporates a body to carry the lateral load.
As a result, the displacement of points in the upper edge is reduced almost
twice from 0.085 mm down to 0.045 mm.
The change of dental implant behavior results also in a more uniform stress
distribution (Fig. 14). The contact p ressure is realized on the whole contact
surface in contrast to the initial implant. Consistently, the screw is less bent.
All the proposals of new shapes were verified with the use of the full three-
dimensional FE model. The results confirmed that the FE m odel built with
cylindrical and solid elements pr ovides compatible values and can be used for
further optimization.
4. Conclusions
The present app roach successfully incorporates an FE solver into a genetic
optimization procedure. T he complex dental implant model was optimized
based on FE analyses. The s tu dy and the final results give evidence that the

Optimization of dental implant... 595
Fig. 13. Deformation of the initial (a) and final (b) dental implant (displacement
scaled up 40 times)
Fig. 14. Mises stress in the initial (a) and final (b) dental implant
presented method is efficient and can be used for f urther analyses. Moreover,
the FE model built with cylindrical and solid elements was validated and no
meaningful differences with the full three-dimensional solid FE mo del were
observed.
A new shape was found which provided a solution with substantial redu c-
tion in principal stresses and displacemens. The joint between the abutment
and the body was much stiffer. It made the implant behave more as a cantile-
ver than a two-element s y s tem. As a consequence, the obtained dental implant

596 T. Łodygowski et al.
transmitted stress from the abutment to the body more s moothly and the ma-
ximum displacement was reduced twice. In comparison with the optimal dental
implant it is visible that the initial one behaved more as a hinge where the
screw is bent. The obtained reduction of the principal stress allowed also for
assumming a significant extension of long-life strength of the implant.
Fatigue damage of implant components is not a common phenomenon but
it makes fu rther treatment very difficult. One of the main final goals of dental
implant optimization is the minimization of fatigue damage of the implant.
The obtained level of principal stress in the key parts of th e implant connec-
tion enable us to reduce or even eliminate the risk of fatigue damage. It should
be noted that despite the level of principal stress reduction only a part of it
can be obtained in the real p roduct. In the first place, the limitation comes
from manufacturing requirements. The dimensions have to be adopted to the
given m anufacture facility. The second limitation refers to the screw loose-
ning. The shape of the hexagonal slot which connects the root of the implant
with the abutment plays the key role in kinematic behavior of th e implant.
The final geometry of screw connection mu s t protect against screw loosening
phenomenon as well. The final shape of this part must also ensure easiness of
in-vivo assembling of the implant. On the one hand, the hexagonal slot must
safely trans fer torsional load during implant fixing and abutment assembling,
on the other hand the dentist sh ou ld easily place the abutment in the slot.
As shown above, the real implant must consider many mentioned limita-
tions. The obtained results of the optimization procedure cannot be directly
adopted in implant systems used at present, but can be a start point for new
designs of such systems. However, the presented approach of optimization can
be used in further studies and designing of modified and new dental implants.
The primary disadvantage of the pr esented numerical approach is the num-
ber of FE analyses, which are necessary to b e carry out in the procedu re.
Despite the total time of the analysis can be shortened usin g parallel com-
putations, it is still a considerable limitation. Thus, it is an important goal
of the stud y to modify the procedure in order to reduce the number of time-
consuming analyses. The first study with the use of a neural network as a
surrogate model has been already elaborated, and the obtained results seem
to be promising.
Acknowledgment
The support of Poznan University of Technology grant DS 11-034/09 as well as
the possibility of using the computational environment of Poznan Supercomputing
and Networking Ce ntre are kindly acknowledged.

Optimization of dental implant... 597
References
1. Abaqus Analysis User’s Manual, 2007a, SIMULIA, Pawtucket
2. Abaqus/C AE User’s Manual, 2 007b, Pawtucket
3. Bozkaya D., M
¨
uf
¨
ut S., 2005 , Mechanics of the taper integrated s crewed-in
(TIS) abutments used in dental implants, Journal of Biomechanics, 38, 8797
4. Burczyński T., Długosz A., Kuś W., 2006, Parallel evolutionary algorithms
in shape optimization of heat radiators, Journal of Theoretical and Applied
Mechanics, 44, 2, 351-366
5. Burczyński T., Kuś W., Długosz A., Orantek P., 2004, O ptimizatio n
and defect identification using distributed evolutionary alg orithms, Engineering
Applications of Artificial Inteligence, 17, 4, 337-3 44
6. Chao H.K., Rowlands R.E., 2007, Reducing tensile stress concentration
in performed hybrid laminate by genetic alg orithm, Composites Science and
Technology, 67, 13, 2877-2883
7. Goldberg D.E., 1989 , Genet icAlgorithm in Search, Optimization and Machi-
ne Learning, 1st Ed., Addison-Wesley Professio nal
8. Goodacre C.J., Bernal G., Rungcharassaeng K., Kan J.Y., 2003, Cli-
nical co mplication with implants and implant pros these s, International Journal
of Prost hodontics, 90, 121-129
9. Hędzelek W., Zagalak R., Łodygowski T, Wierszycki M., 2004, Ba da-
nia biomechaniczne elementów protetycznych implantów z zastosowaniem me-
tody elementów skończonych, Protetyka Stomatologiczna, 51, 1, 23- 29
10. Kąkol W., Łodygowski T., Wierszycki M., 2002, Numerical analysis of
dental implant fa tigue, Acta of Bioengineering and Biomechanics, 4, 1, 79 5-796
11. Lang L.A., Kang B., Wang R.F., Lang B.R., 2003, Finite element analy-
sis to determine implant preload, The Journal of Prosthetic Dentistry, 90, 6,
539-546
12. Merz B.R., Hunenbart S., Belser U.C., 2000, Mechanics of the implant-
abutment connection: an 8- degree tap e r compared to a butt joint connection,
The International Journal of Oral and Maxillofacial Implants, 15, 4, 519-526
13. Michalewicz Z., Schoenauer M., 1996, Evolutionary algorithms for c on-
strained parameter o ptimizatio n problem, Evolutionary Computation, 4, 1, 1-32
14. Natali A.N., 2003, Dental Biomechanics, Taylor & Francis
15. Szajek K., Kąkol W., Łodygowski T., Wierszycki M., 2008, Optimi-
zation module for Abaqus/CAE based on Genetic Algorithm, Abaqus U sers’
Conference, Newport, USA, 447-462

598 T. Łodygowski et al.
16. Wang K., 1996, The use of titanium for medical applications in the USA,
Materials Science and Engineering, A213, 134-137
17. Wierszycki M., 2007, Numeryczna analiza wytrzymałościowa wszczepów uzę-
bienia oraz s egmen tu kręgosłupa ludzkiego, PhD Thesis, Poznań
18. Wierszycki M., Kąkol W., Łodygowski T., 2006a, Fatigue algorithm
for dental implant, Foundations of Civil and Environmental Engineering, 7,
363-380
19. Wierszycki M., Kąkol W., Łodygowski T., 2006b, Numerical comple-
xity of selected bio mechanical problems, Journal of Theoretical and Applied
Mechanics, 44, 4, 797-818
20. Wierszycki M., Kąkol W., Łodygowski T., 2 006c, The scre w loosening
and fatigue analyses of three dimensional dental implant model, ABAQ US
Users’ Conference 2006, Boston MA
21. Zagalak R., 2003, Evaluation of Mechanical Properties of Two Dental Im-
plants Osteoplant, PhD Thesis, University of Medical Sciences in Poznań [in
Polish]
22. Zagalak R., Hędzelek W., Łodygowski T., Wierszycki M., 2005,
Wpływ za niku kości i gęstości na ryzyko złamań implantów - badania metodą
elementów skończonych, Implantoprotetyka, 6, 1, 3-7
Optymalizacja wszczepu stomatologicznego z wykorzystaniem
algorytmu genetycznego
Streszczenie
Przedmiotem pr e zentowanej pracy jest problem optymalizacji systemu implanto-
logicznego Osteoplant, k tóry został opracowany i wciąż jest ulepszany przez Fundację
Uniwersytetu Medycznego w Poznaniu. Obserwacje kliniczne potwierdzają występo-
wanie powikłań zarówno we wczesnej, jak i późnej fazie użytkowania implantu. Do-
ty chczas otrzymane wyniki wskazują, że wydłużenie bezawaryjnego okresu użytko-
wania implantu wymaga wprowadzenia z mian w jego pracy mechanicznej. Jednakże,
ustalenie szczegó ł ów mo dy fikacji nie jest ocz ywiste. W artykule została opisana proce-
dura optymalizacji systemu implantologicznego Osteoplant z użyciem analizy metodą
elementów skończonych oraz algorytmu genetycznego.
Manuscript received Febru ary 11, 2009; accepted for print April 8, 2009