вход по аккаунту


The Response of Cranial Biomechanical Finite Element Models to Variations in Mesh Density.

код для вставкиСкачать
THE ANATOMICAL RECORD 294:610–620 (2011)
The Response of Cranial Biomechanical
Finite Element Models to Variations in
Mesh Density
Department of Earth Sciences, University of Bristol, Wills Memorial Building,
Queens Road, Bristol, United Kingdom
Finite element (FE) models provide discrete solutions to continuous
problems. Therefore, to arrive at the correct solution, it is vital to ensure
that FE models contain a sufficient number of elements to fully resolve
all the detail encountered in a continuum structure. Mesh convergence
testing is the process of comparing successively finer meshes to identify
the point of diminishing returns; where increasing resolution has marginal effects on results and further detail would become costly and
unnecessary. Historically, convergence has not been considered in most
CT-based biomechanical reconstructions involving complex geometries
like the skull, as generating such models has been prohibitively time-consuming. To assess how mesh convergence influences results, 18 increasingly refined CT-based models of a domestic pig skull were compared to
identify the point of convergence for strain and displacement, using both
linear and quadratic tetrahedral elements. Not all regions of the skull
converged at the same rate, and unexpectedly, areas of high strain converged faster than low-strain regions. Linear models were slightly stiffer
than their quadratic counterparts, but did not converge less rapidly. As
expected, insufficiently dense models underestimated strain and displacement, and failed to resolve strain ‘‘hot-spots’’ notable in contour plots.
In addition to quantitative differences, visual assessments of such plots
often inform conclusions drawn in many comparative studies, highlighting that mesh convergence should be performed on all finite element
models before further analysis takes place. Anat Rec, 294:610–620,
C 2011 Wiley-Liss, Inc.
2011. V
Key words: finite element analysis;
biomechanics; feeding
The use of finite element analysis (FEA) in biomechanics has been steadily increasing over recent decades.
It is now a powerful investigative tool in applied medical
and academic research where quantification of skeletal
stresses and strains is desired. As a computational technique, FEA offers a repetitive means of mechanically
testing complex 3D geometries of multiple materials
under a variety of physiological or destructive loading
conditions. Orthopedic models are often developed from
CT scans, allowing for generalized reconstructions to
predict mechanical behaviour (Roth et al., 2010), or subject-specific representations of an individual’s bones
for precise reconstructions, which can non-invasively
predict how a patient may respond to complex surgical
Additional Supporting Information may be found in the
online version of this article.
Grant sponsor: Natural Environment Research Council
(NERC) studentship; Grant number: NE/F007310/1.
*Correspondence to: Jen A. Bright, Department of Earth Sciences University of Bristol, Wills Memorial Building, Queens
Road, Bristol BS8 1RJ, United Kingdom. Fax: 0117-925-3385.
Received 18 October 2010; Accepted 22 December 2010
DOI 10.1002/ar.21358
Published online 2 March 2011 in Wiley Online Library
treatment (Remmler et al., 1998). In comparative studies, FEA is being used to investigate the wider association between function and form, by testing the
mechanical response to certain loads (Dumont et al.,
2005; Bourke et al., 2008; Moazen et al., 2008; Moreno
et al., 2008), and by using the fact that morphologies
can be manipulated within the computer to isolate the
effects of specific features on the strain environment
(Rayfield et al., 2007; Strait et al., 2007; Farke, 2008;
Tanner et al., 2008). FEA is also gaining popularity with
palaeontologists, for whom it offers a rare opportunity to
elucidate mechanically feasible behaviours, and ideally,
to address broader ecological and evolutionary questions
in fossil organisms (Rayfield, 2005, 2007; McHenry
et al., 2007; Wroe et al., 2007; Wroe, 2008; Tseng, 2009).
The decreasing cost of computer resources and wide
availability of software have made finite element modelling easily accessible. However, as with all modelling,
FEA describes a version of reality based on several simplifying assumptions. In skeletal biomechanics, this usually means the exclusion of soft tissues, or using bone
material properties from a related species in the absence
of data for the animal under investigation. An incomplete
understanding of how these assumptions affect the results
can make it possible to build inaccurate models, or models
laden with inappropriate assumptions. Thus, while FE
models can potentially yield vast amounts of important information, it is vital to ensure that they provide a precise
and accurate approximation of the scenario they have
been designed to address. Practices for the construction of
successful biomechanical models have been outlined, highlighting the importance of mesh verification and validation
(Viceconti et al., 2005; Anderson et al., 2007). Verification,
often referred to as precision, is concerned with the underlying mathematics of the model, ensuring that the correct
equations are being solved, and that the model contains
sufficient elements to approximate a continuum solution
(known as mesh convergence). Validation, often referred to
as accuracy, is concerned with ensuring that the model is
providing a realistic simulation by assigning appropriate
boundary conditions. The distinction between the two is
important: a model may be mathematically precise, but if
it has made incorrect assumptions about the boundary
conditions, then it will only be providing a precise answer
to the wrong question.
Unfortunately, although crucial, both steps are frequently overlooked by FE users, particularly in studies
of animal morphology. Commercial software verifies the
equations it uses, but the responsibility of performing a
mesh convergence test lies with the modeler. Convergence tests require the production of meshes with successively smaller element size, refining the model until
enough elements are used to demonstrate that increasing the resolution does not alter stress, strain, or displacement values calculated at the same region of the
structure. Biomechanical FE meshes are often based off
stereolithography (.stl) files that reconstruct internal
and external surface geometries using triangular facets.
The production of even one complex 3D mesh by this
method has historically been an incredibly time-consuming exercise. Stereolithography surfaces are often composed of facets whose shapes are of poor finite element
quality (e.g., high aspect ratio), or too fine to solve on a
normal desktop computer. As either problem requires
that the facets be completely remeshed, rather than
just simply subdivided, and the boundary conditions
reapplied to the new mesh, convergence testing is rarely
performed. When this is coupled with the fact that more
refined meshes frequently require prohibitively high
computer power, convergence tests often only compare
two or three successive meshes (Jones and Wilcox,
2007). These may be misleading as they only capture a
small portion of the convergence curve, which would
ideally show a rapid initial increase in strain or displacement followed by a plateau once convergence was
achieved. In reality, convergence curves may not behave
smoothly and important details could be lost (Schmidt
et al., 2009).
The vertebrate skull has a highly curved and complicated geometry, with numerous, interconnected internal
cavities and multidirectional loading regimes. It is of
particular interest to zoologists and palaeontologists as
it houses the sensory organs and feeding apparatus,
thus characterising many of the interactions an animal
will have with its environment. Although a number of
papers have been published on the convergence of
biomechanical models, these are often concerned with
medical models of the interaction between bones and
prosthesis (Schmidt et al., 2009), or with the relatively
simple geometries of the long bones (Ramos and Simões,
2006), phalanges (Richmond, 2007), pelvis (Anderson
et al., 2005), or vertebrae (Crawford et al., 2003; Jones
and Wilcox, 2007). These studies are not directly relevant to those interested in the behaviour of the whole
skull, such as is often the case in vertebrate morphology.
Thankfully, the falling cost of computer power and the
continuing improvement of mesh generating software
are now making convergence testing on highly complex
geometries like the skull a reasonable step in model
The aim of this study was to perform convergence testing on a complex skull geometry, to gauge what resolution of FE-mesh was required to achieve convergence
and at what rate different regions of the skull converged, and why. Convergence tests were performed on
specimen-specific finite element models of a modern
domestic pig skull by comparing strains and displacements in increasingly refined meshes. In particular it
was predicted that areas of the skull that experience
high strain gradients would converge at higher mesh
densities than regions of the skull with low strain gradients, as the position of high strain gradients would be
better resolved in meshes with greater precision. These
locations are not discernable a priori, but were expected
to occur in close proximity to loads and constraints. It
was also expected that areas of complex geometric detail
would require higher resolutions to appropriately resolve
strain than simple geometries.
Mesh Generation
The skull of a modern domestic pig (Large White
breed, age 6 months; skull dimensions 247 141 133 mm) was CT-scanned at the Royal Veterinary College on a Picker PQ5000 medical scanner (0.55 mm pixel
size, 1 mm slice thickness, 120 kV, 200 mA). The CT slices were imported into Amira 4.1 (Mercury Computer
Systems), and the bony and dental structures were segmented out and used to reconstruct a stereolithography
Fig. 1. Examples of (A) low (4 mm); (B) medium (2 mm); and (C) high (0.92 mm) density meshes, illustrating the loss of geometric details at lower mesh resolution. D: Locations of strain gauges used as convergence points in the study, and details of boundary conditions. Note that the applied loads are
asymmetrical. TMJ ¼ temporomandibular joint; M1 = 1st molar tooth; G ¼ gauge.
(.stl) file. This was then imported into HyperMesh 10.0
(Altair Engineering) for finite element pre-processing.
A series of successively refined 2D shell meshes were
generated using the HyperMesh ‘‘shrink-wrap’’ function,
which fits a 2D shell as tightly as possible over an existing geometry, with a user-controlled modal average element size. This results in meshes of homogeneously
sized elements with good aspect ratios, and also retains
internal geometries, such as the brain and sinus cavities. In instances where the desired element size is too
large to fit to the local curvature, the shrink-wrap function may adopt a slightly smaller element size to capture
fine details (e.g., cusps on the teeth), however, with the
very coarsest meshes, a certain degree of ‘‘smoothing
out’’ of the finer geometric details is unavoidable
(Fig. 1A–C). These 2D shells then formed the starting
point for an automated, surface-based tetrahedral meshing algorithm to generate a series of 3D FE meshes. Initially, five meshes of element sizes 1, 2, 3, 4, and 5 mm
were generated, then 13 subsequent finer meshes were
created post hoc, 11 with element sizes between 1 and
2 mm. The number of elements in a model increases
rapidly with decreasing element size, therefore a
large increase in the number of elements was encountered between 1 and 2 mm, necessitating additional
models to appropriately capture convergence detail. This
resulted in a total of 18 meshes, with modal average
element sizes between 5 and 0.83 mm (Supporting Information 1).
Boundary Conditions
Once the 3D meshes had been constructed, we applied
boundary conditions that mimicked the set-up of an in
vitro strain experiment that was being used to validate
the model as part of a wider study. This set-up utilized
loads totaling 755 N applied to the masseter and
temporalis muscle attachment sites, which pulled the
specimen down on to supports located bilaterally at the
first molars and temporomandibular joints (TMJ) on a
custom built-testing rig. This provided a reasonable
approximation of a biting scenario that was repeatable
and easy to model (Fig. 1D; Supporting Information 2).
Loads were applied to the FE-model via rigid body elements (RBE3 in HyperMesh) and constraints were
defined to prevent translation in the Y axis at the teeth
(dorso-ventral motion) and the XYZ axes at the TMJ, to
mimic the experimental loading rig. Loads were initially
applied to the original .stl import and then, using this as
a guide, were used to place the loads on to all the subsequent meshes to ensure repeatability of load positions.
Although every effort was taken to ensure that the
boundary conditions applied were as consistent as possible amongst models, the changing resolution of the
meshes meant that the exact locations on the original
mesh did not always match with a node on the shrinkwrapped meshes. In these instances, the nearest node
was used to apply the loads, however this meant that, in
the coarsest meshes, the positioning of loads and constraints may have been in error by up to 3.5 mm. In the
finer meshes, this error was <1 mm. Given that the
shortest dimension (height) of the specimen measured
133 mm, the maximum placement error of <3% was
deemed to be acceptable. At this stage, node sets
corresponding with the location of sixteen 45 mm2
planar rosette strain gauges (C2A-06-062LR-350; Vishay
Measurements Group UK, Basingstoke, UK) applied to
the experimental pig were defined, again initially on the
original .stl and then on the other meshes (Gauges 1–16,
Fig. 1D). Defining the node sets at this stage ensured
consistency amongst the models, and allowed for strain
data to be queried in these exact locations once the analyses were complete. Inevitably, as the mesh resolution
increased, so did the number of data points queried
per gauge in each subsequent analysis (Supporting
Information 3).
In the absence of material properties data on pig bone,
all models were assigned the properties of adult human
cranial bone (E ¼ 12.5 GPa, m ¼ 0.35, Peterson and
Dechow, 2003). Bone was assumed to be isotropic and
homogeneous, and the teeth were also assigned the
material properties of bone. Cranial sutures were not
considered in these models. Although investigation continues into the sensitivity of biomechanical FE models to
these assumptions, and their effects on model validity
(Ross et al., 2005; Strait et al., 2005; Kupczik et al.,
2007; Panagiotopoulou et al., 2010, 2011; Rayfield,
2011), the convergence test seeks only to verify, not
All models were exported with both linear 4-noded
(TET4), and quadratic 10-noded (TET10) tetrahedral elements, resulting in a total of 36 models: 18 with TET4
and 18 with TET10. The size of the elements in a given
model remains the same, but TET10 quadratic elements
have additional nodes located at the mid-point of
the edges of each element, allowing more complex
deformation to be modeled. TET4 elements are traditionally considered to be overly stiff (Mac Donald, 2007),
and so observing both types of element would determine
any difference in ‘‘convergence rates’’ (i.e., whether
convergence would be achieved earlier in lower resolution meshes in one element type compared to the
Finite Element Analysis
The 36 models were solved in Abaqus 6.8.2 (Dassault
Systèmes Simulia, Providence RI) on a desktop PC (Windows 64-bit Vista Business, Intel Xeon x5450 3.00 GHz
CPU, 64 GB RAM). At this specification, the lowest resolution model (5 mm TET4) ran in 7 sec, and the highest
resolution model (0.83 mm TET10) ran in 10.6 hr.
For each model, maximum (emax) and minimum (emin)
principal strain and displacement (U) values were
exported from each of the 16 node sets representing the
strain gauges, and contour plots of the models were visually inspected. Strain and displacement values from
nodes under each gauge site were averaged, and plotted
against the number of elements in the mesh. Nodes
selected only considered element apex nodes, and did
not include midpoint nodes from quadratic models, to
ensure consistency when comparing with linear models.
The error between successive models was calculated as
the percentage difference in strain or displacement magnitudes between the current mesh and the previous (less
refined) mesh (Schmidt et al., 2009) at each gauge location. We chose to identify the convergence where <10%
or <5% change in strain or displacement magnitudes
was found between successive meshes. To our knowledge, there appears to be no standard criterion of convergence, although <5% is often quoted (Anderson et al.,
2005; Schmidt et al., 2009). Ultimately, the target level
of convergence that is considered appropriate, be it 10%
or 0.1% change, is left to the user, who must decide
whether these errors are acceptable within the remit of
their analysis.
The highest density model (0.83 mm, TET10) was the
most precise, and was therefore used to determine the
strain and displacement ranges (max.–min. value) under
each gauge site, thus indicating the gradients encountered. Distorted elements (defined by Abaqus as
having Tetrahedral Quality Measure <0.02; Supporting
Information 1) were identified for each model, and
made up <0.01% of the total elements per model on
average [greatest value at 5 mm mesh (32,000 elements)
¼ 0.025% distorted elements, see Supporting Information 1].
TET4 Elements
All element numbers quoted in the text are rounded to
the nearest 10,000. For actual values please see Supporting Information 1. The results displayed in Fig. 2A–
C (see Supporting Information 4 for numerical values)
show that, by 1.05 mm (1,250,000 elements), all TET4
gauge sites have converged to within 10% change in values from meshes with successively smaller element size,
with two exceptions: emax G7 (12%) and displacement G2
(11%). By 0.92 mm (1,750,000 elements), almost all variables are converged to within 5%, with the following
exceptions: emax G4, G7, G9; emin G2, G3, G7; displacement G1, G2. This indicates that different locations in
the skull are converging at different rates, with some
reaching the target of 10% convergence at far lower
mesh densities than others: emin G8, for instance,
achieves 5% convergence in a mesh as coarse as 2.1 mm
(250,000 elements) (Fig. 2B).
Fig. 2. Distribution of convergence in the series of models for (A) emax; (B) emin; and (C) displacement.
Dark gray indicates convergence within 5%, light gray within 10%, and white >10%. Anomalous points
are marked as ‘‘x.’’
TET10 Elements
The TET10 models, as expected, are less stiff than their
4-noded counterparts (Fig. 3). Although both types of element generally follow the same convergence curve, with
the TET10 results plotting with slightly higher values of
strain (except G5; see Fig. 3) and displacement, the differences between TET4 and TET10 models are not consistent. In extreme examples, the TET10 models may give
anomalously high peaks of strain, evident as clear outliers
(marked by ‘‘x’’ in Fig. 2A,B; Fig. 3: G2, G12, G13, G14,
G16; bold numbers in Supporting Information 4), which
are absent in the TET4 results. We defined anomalies as
wherever convergence could be demonstrated to within
10% between two or more successive models on either side
of the anomalous point, or wherever the change in strain
between two models was over 100% more than the change
between the models preceding it.
The positions of these anomalous peaks are inconsistent: for instance, at 1 mm (1,500,000 elements) peaks
are present in G16, but not G15, to which it is directly
adjacent (Fig. 1D). Nor are all anomalous peaks in the
same model (e.g., G2 shows peaks at 1.05 mm, rather
than 1 mm as in the previous example). Removal of the
anomalous points and recalculation of the percentage
change based on the previous model (along with qualitative observation of the convergence plots) suggests that,
without these anomalies, 5–10% strain convergence
would be obtained by 1.05 mm or earlier (Fig. 4A,B). In
all models without clear anomalies, 10% convergence is
achieved by 0.92 mm, with the following exceptions: emax
G7; displacement G1, G2, G4, G6, G7. Displacement
results therefore appear to be less stable than those of
strain using TET10 elements, with no gauges achieving
5% convergence by the highest resolution model (0.83
mm), whereas 14 out of 16 gauges reach this by 1.05
mm using TET4 (Table 1).
Relationship with Strain Gradients
We predicted that regions with the highest strain gradients would take longer to converge than low strain
Fig. 3. Convergence plots of strain (solid lines) and displacement (dashed lines) at all gauge sites (G1–
G16) for TET4 (closed markers) and TET10 (open markers) models.
Fig. 3. (Continued)
Fig. 4. Distribution of convergence in the series of models following the removal of anomalous points
(marked by ‘‘x’’), for (A) emax and (B) emin. Dark gray indicates convergence within 5%, light gray within
10%, and white >10%.
TABLE 1. Number of gauges out of a total of 16 achieving convergence
by 0.92 mm (1,749,149 elements)
gradient regions. Strain ranges predicted by the highest
resolution model (0.83 mm, TET10) were obtained from
each gauge site, and are presented in Table 2. G5 and
G8 have the highest strain ranges and G2 has the lowest. This was expected, given their proximities to loading
on the zygomatic arch (Fig. 1D). Contrary to predictions,
however, G5 and G8 converged very rapidly, whereas G2
was one of the slowest gauges to converge (Fig. 2A–C).
Association with Geometry
The convergence locations we chose were equivalent to
the positions of strain gauges in an associated in vitro
validation study. The placement of strain gauges
requires that the bones be relatively flat and featureless,
and so curvature of the bones should not be affecting the
convergence results. However, G7, which fails to achieve
convergence within 10%, is directly adjacent to a prominent groove in the thin anterior frontal bone, associated
with a large blood vessel (Fig. 1D). No other gauges are
in such close proximity to notable geometric features.
Consideration of Contour Plots
Most paleontological use of finite element analysis is
concerned not with the absolute values generated by the
models, but a more qualitative comparison of the contour
plots they produce. Such comparisons allow conclusions
to be drawn about the relative performances of two different structures (Rayfield et al, 2007; Jasinoski et al.,
2009). Qualitative observations of the contour plots produced by the convergence test show how these change
with increasing model resolution. Low resolution models
tend to underestimate values and miss ‘‘hot-spots’’ of
higher strain (Fig. 5). By 1 mm element size, minor differences in the location of high strains are still discernable, but contour plots have generally settled on a stable
pattern (Fig. 5P,H0 ). Contour plots for displacement are
more homogeneous, but differences in the rostrum are
still apparent even in the highest resolution models
(compare Fig. 5A00 –B00 ).
The results show that in most areas of the skull, TET4
models converge to within 5% and TET10 to within 10%
by 0.92 mm (1,750,000 elements). The relatively poor performance of the TET10 models was surprising, as they often failed to converge as rapidly as their TET4
counterparts. When strain is the variable of interest, this
apparently poor performance can be attributed to the
TABLE 2. Predicted strain ranges at each gauge
site in the highest resolution model (0.83 mm TET10)
Gauge site
Displacement (mm)
Bold normal type numbers indicate the highest values and
bold italics indicate the lowest values for each variable.
presence of anomalously high strains at certain locations
(‘‘x’’ in Fig. 2A,B; anomalous peaks in Fig. 3; bold numbers
in Supporting Information 4). The reason for the anomalous peaks is unclear, given that the only difference
between TET4 and TET10 models is whether the elements are linear or quadratic, and by the stage of mesh
refinement that most anomalies appear (1 mm), the maximum possible discrepancy in boundary condition application point between models was < 1 mm. As the percentage
of distorted elements was low (< 0.01%) and bad elements
were located away from the gauge sites, element distortion is unlikely to be responsible. If the anomalous data
points are disregarded, TET10 models converge to within
5% relative difference at element sizes equal to or larger
than the TET4 models (compare Fig. 2A,B with Fig.
4A,B). However, it can be reasonably demonstrated that,
by 0.92 mm element size, both the TET4 and TET10 models are converged in regards to principal strain to within
5% at all locations except G7 (emax 12–13%, emin 7–8%). As
noted above, the G7 site is close to an area of complex
geometry, which may be responsible for this failure to
converge satisfactorily.
Fig. 5. TET4 contour plots of emax (A–R), emin (S–J0 ), and displacement (K0 –B00 ) in order of increasing
When displacement is the variable of interest, most
TET10 model locations converge to within 10% by 0.92
mm element size (1,750,000 elements), but none to
within 5%. This is an unexpected result, as displacement
is often demonstrated to converge at lower mesh densities than strain (Mac Donald, 2007). Conversely, in
TET4 models 13 gauges achieve 5% convergence by this
stage (Table 1). One would expect that the increased resolution offered by TET10 elements should improve the
results of these models, but perhaps the greater degree
of deformation permitted by TET10 elements slows their
rate of displacement convergence.
We note that the convergence curves, and consequently the magnitudes of relative error, are not smooth.
In all gauges, even those that ultimately achieve convergence, successive models may report a relative error of
<5%, only to jump up to higher errors in the next model
in the sequence (Supporting Information 4). This is a
similar observation to that of Schmidt et al. (2009), who
found that Von Mises stress sometimes increased in
their models after a period of apparent convergence.
These periods of apparent convergence followed by
jumps in strain present a dilemma: how can we be certain that convergence has been achieved in our finest
models when further resolution increases may show
another strain jump? In the two finest meshes modelled
(0.92–0.83 mm), a decrease of <0.1 mm element size
resulted in a model with nearly 450,000 more elements.
Conversely, a size decrease of 0.125 mm for models earlier in the analysis (1.500–1.375 mm) gives element
gains of only 130,000. Because of the greater range of
mesh densities represented towards the end of the analysis, and that stable plateaus are observed in the length
of the convergence curve that we have covered, we are
confident that, in gauges we have deemed converged,
further jumps are unlikely. Of course, as finite element
models represent discretizations of continuous problems,
the only way to be certain that smaller element sizes
would not see jumps in their results would be to increase
mesh resolution ad infinitum, although in practice this
is clearly not possible. Our results therefore support
Schmidt et al.’s (2009) assertion that mesh convergence
studies comprising only two or three mesh densities may
be insufficient. For instance, the peaks of anomalously
high strain identified in this study would not have been
apparent without the wider assessment of error that
identified them as outliers, nor could we confidently predict that further element increases will not result in
strain jumps.
Predictions that gauge sites subjected to higher strain
gradients would be slower to converge were shown to be
incorrect. The gauge sites with the highest gradients
(G5 and G8) in fact showed the fastest convergence
rates. These sites were located on the zygomatic arch,
close to the application of the loading. On further consideration, this result is perhaps not that surprising. The
sites closest to the loading experience the highest absolute strains in the model. Consequently, to produce a
variation of 5% requires more absolute change in strain
values at these locations than at sites with lower average strain values. Similarly, sites with lower average
strains will be very sensitive to small changes in the
model, and thus require higher resolution meshing to
achieve convergence. However, depending on the nature
of the question being addressed, it is possible that
regions of low strain are not of interest to the investigator. If this is the case and absolute values are unimportant, then perhaps lows strains can be ignored. Then, it
is sufficient only to resolve the model so that (i) areas of
high strain converge and (ii) areas identified as low
strain are indeed areas of low strain (rather than an
artefact of the model being under-converged; Fig. 5).
The meshes used in this study can be thought of as homogeneous in terms of element size. Although this
approach is ideal for a convergence study of the whole
skull, the observation that different locations converge at
different rates indicates that element size homogeneity is
not the most efficient meshing method: some gauges converge at lower mesh densities than others and do not
require the computationally expensive high resolution
forced upon them by homogeneous high-density meshes.
Similarly, even regions that require a high mesh density
to converge, such as some of the low strain areas identified in this study, may be of little interest to the investigation. As these regions would not require the most
precise solution, a coarser mesh may suffice in such locations. Gauge 7 was unable to show 10% emax convergence
even at the highest mesh density considered here. Adaptive re-meshing, where troublesome areas are re-meshed
with finer elements after identifying them by the homogeneous approach described above, is the solution to this efficiency dilemma. However, this is currently difficult to
put into practice using the automated meshing software
utilized by most morphologists attempting to capture
complicated and highly curved 3D structures. Surfaces
generated from .stl files automatically apply smaller triangular facets to capture highly curved geometry, but
conversely, use larger facets for flat areas. As these local
variations in facet density are dictated by geometry and
not strain, it cannot be assumed that a direct conversion
of these facets into elements will give a model that is
appropriately converged: for instance, strains developed
in flatter regions may not be fully resolved by large elements the size of the original facet (all locations in this
analysis were relatively flat, due to the need to attach
strain gauges). In addition, errors may arise from the
close proximity of very large to very small elements that
may be generated in an .stl.
Despite its qualitative nature, the fact that contour
plots also show sensitivity to mesh density is important.
Low resolution meshes underestimated strain and failed
to resolve strain ‘‘hot-spots’’ in the contour plots. This
may significantly alter an interpretation of structural
behaviour, or mislead comparisons with a validation
dataset. In palaeontology, comparative studies often
focus on the response of morphologies to idealised loads
and interpret differences in contour plots because absolute values cannot be validated. In such studies, different morphologies will likely converge at different rates
and as such, verification of all morphologies being considered is particularly crucial so that inappropriate
mesh resolutions do not confound the true effects of differences in morphology.
For most locations, convergence in this study can be
said to have been successful by element sizes of 1 mm.
It is important to emphasize that the specifics of this
convergence study are unique to this particular model
set-up. Convergence tests should ideally be performed in
all finite element analyses, and the current study highlights mesh verification as an important step before any
validation or interpretation of models of the skull can
occur. If validation cannot be performed and only contour patterns are of interest, convergence is still vital to
ensure that the correct patterns have been resolved.
The authors thank Daniel Nieto (Altair UK) for his
extensive help and advice on mesh generation, Chris
Lamb (Royal Veterinary College) for scanning the specimen, and Michael Fagan (University of Hull) for his assistance in resolving early mesh errors, as well as two
anonymous reviewers for their constructive comments.
Anderson AE, Ellis BJ, Weiss JA. 2007. Verification, validation and
sensitivity studies in computational biomechanics. Comput Meth
Biomech 10:171–184.
Anderson AE, Peters CL, Tuttle BD, Weiss JA. 2005. A subject-specific finite element model of the pelvis: development, validation
and sensitivity studies. J Biomech Eng 127:364–373.
Bourke J, Wroe S, Moreno K, McHenry C, Clausen P. 2008. Effects
of gape and tooth position on bite force and skull stress in the
dingo (Canis lupus dingo) using a 3-Dimensional Finite Element
approach. PLoS ONE 3:e2200.
Crawford RP, Rosenburg WS, Keaveny TM. 2003. Quantitative computed tomography-based finite element models of the human lumbar vertebral body: effect of element size on stiffness, damage,
and fracture strength. J Biomech Eng 125:434–438.
Dumont ER, Piccirillo J, Grosse IR. 2005. Finite-element analysis of
biting behaviour and bone stress in the facial skeletons of bats.
Anat Rec 283A:319–330.
Farke AA. 2008. Frontal sinuses and head-butting in goats: a finite
element analysis. J Exp Biol 211:3085–3094.
Jasinoski SC, Rayfield EJ, Chinsamy A. 2009. Comparative feeding
biomechanics of Lystrosaurus and the generalised dicynodont
Oudenodon. Anat Rec 292:862–874.
Jones AC, Wilcox RK. 2007. Assessment of factors influencing finite
element vertebral model predictions. J Biomech Eng 129:898–903.
Mac Donald BJ. 2007. Practical stress analysis with finite elements.
Dublin: Glasnevin Publishing.
McHenry CR, Wroe S, Clausen PD, Moreno K, Cunningham E.
2007. Supermodeled sabercat, predatory behaviour in Smilodon
fatalis revealed by high-resolution 3D computer simulation.
PNAS 104:16010–16015.
Moazen M, Curtis N, Evans SE, O’Higgins P, Fagan MJ. 2008.
Combined finite element and multibody dynamics analysis of biting in a Uromastyx hardwickii lizard skull. J Anat 213:499–508.
Moreno K, Wroe S, Clausen P, McHenry C, D’Amore DC, Rayfield
EJ, Cunningham E. 2008. Cranial performance in the Komodo
dragon (Varanus komodoensis) as revealed by high-resolution 3-D
finite element analysis. J Anat 212:736–746.
Panagiotopoulou O, Curtis N, O’Higgins P, Cobb SN. 2010. Modelling
subcortical bone in finite element analyses: a validation and sensitivity study in the macaque mandible. J Biomech 43:1603–1611.
Panagiotopoulou O, Kupczik K, Cobb SN. 2011. The mechanical
function of the periodontal ligament in the macaque mandible:
a validation and sensitivity study using finite element analysis.
J Anat 218:75–86.
Peterson J, Dechow PC. 2003. Material properties of the human
cranial vault and zygoma. Anat Rec 274A:785–797.
Ramos A, Simões JA. 2006. Tetrahedral versus hexahedral finite
elements in numerical modelling of the proximal femur. Med Eng
Phys 28:916–924.
Rayfield EJ. 2005. Using finite-element analysis to investigate
suture morphology: a case study using large carnivorous dinosaurs. Anat Rec 283A:349–365.
Rayfield EJ. 2007. Finite element analysis and understanding the
biomechanics and evolution of living and fossil organisms. Annu
Rev Earth Pl Sc 35:541–576.
Rayfield EJ. 2011. Strain in the ostrich mandible during simulated
pecking and validation of specimen-specific finite element models.
J Anat. 218:47–58.
Rayfield EJ, Milner AC, Xuan VB, Young PG. 2007. Functional morphology of spinosaur ‘‘crocodile-mimic’’ dinosaurs. J Vertebr Paleontol 27:892–901.
Remmler D, Olson L, Ekstrom R, Duke D, Matamoros A, Matthews
D, Ullrich CG. 1998. Pre-surgical CT/FEA for craniofacial distraction: I. Methodology, development, and validaton of the cranial
finite element model. Med Eng Phys 20:607–619.
Richmond BG. 2007. Biomechanics of phalangeal curvature. J Hum
Evol 53:678–690.
Ross CF, Patel BA, Slice DE, Strait DS, Dechow PC, Richmond BG,
Spencer MA. 2005. Modeling masticatory muscle force in finite
element analysis: sensitivity analysis using principle coordinates
analysis. Anat Rec 283A:288–299.
Roth S, Raul J-S, Willinger R. 2010. Finite element modelling of
paediatric head impact: global validation against experimental
data. Comput Meth Prog Biol 99:25–33.
Schmidt H, Alber T, Wehner T, Blakytny R, Wilke H-J. 2009. Discretization error when using finite element models: analysis and evaluation of an underestimated problem. J Biomech 42:1926–1934.
Strait DS, Richmond BG, Spencer MA, Ross CF, Dechow PC, Wood
BA. 2007. Masticatory biomechanics and its relevance to early
hominid phylogeny: an examination of palatal thickness using
finite element analysis. J Hum Evol 52:585–599.
Strait DS, Wang Q, Dechow PC, Ross CF, Richmond BG, Spencer
MA, Patel BA. 2005. Modeling elastic properties in finite-element
analysis: how much precision is needed to produce an accurate
model? Anat Rec 283A:275–287.
Tanner JB, Dumont ER, Sakai ST, Lundrigan BL, Holekamp KE.
2008. Of arcs and vaults: the biomechanics of bone-cracking in
spotted hyenas (Crocuta crocuta). Biol J Linn Soc 95: 246–255.
Tseng ZJ. 2009. Cranial function in a late Miocene Dinocrocuta
gigantea (Mammalia: Carnivora) revealed by comparative finite
element analysis. Biol J Linn Soc 96:51–67.
Viceconti M, Olsen S, Nolte L-P, Burton K. 2005. Extracting clinically relevant data from finite element simulations. Clin Biomech
Wroe S. 2008. Cranial mechanics compared in extinct marsupial
and extant African lions using a finite-element approach. J Zool
Wroe S, Clausen P, McHenry C, Moreno K, Cunningham E. 2007.
Computer simulation of feeding behaviour in the thylacine and
dingo as a novel test for convergence and niche overlap. Proc R
Soc B 274:2819–2828.
Без категории
Размер файла
1 150 Кб
model, elements, cranial, mesh, response, finite, variation, density, biomechanics
Пожаловаться на содержимое документа