1. ME 404-01 Final Project
Summer 2014
8/20/14
Alex Powers Marley Miller

2. Executive Summary
This final project included modeled an Easton EC70 XC handlebar (see Figure 1 below) under a variety
of common loading cases in order to investigate the stresses, strains, and deflections at various locations
and to compare the uses of different materials. Rough hand calculations were performed for stresses and
deflections which provided ballpark estimates to be compared to the model results and prove validity.
Once the geometry was created in SolidWorks (see Figures 2,3,4,5,6), it was imported into ABAQUS for
the 3 different models (beam, solid, and shell elements). Each model was used with a cantilever end load
and a torque load to easily compare the different models as well as different materials. Each model was
used with Aluminum 6061-T6, 4130 Chromoly Steel, and a carbon fiber layup to compare the benefits
and drawbacks of each material. We also modeled a generic steel clamp in order to determine the effects
of contact stresses on the max loads that the bar could handle.
Figure 1. Easton EC70 XC Carbon Fiber Handlebar
The shell model proved to be the most accurate and easiest to run and therefore was used for final results
and analysis. Using the shell model for a variety of material configurations, we found that the carbon fiber
handlebars could be tuned to outperform the steel and aluminum variants in both bending and torsional
loading cases, depending of course upon the layup used. Of the configurations tested, we feel as though
the [0°/0°/+45°/-45°] layup offered the best characteristics out of all of the configurations tested,
requiring a 310 lbf end load or a 2620 lbf-in torque to break while still offering resistance to shattering in
the event of an impact. These results can be found in Table 2 below. We also tested each configuration
with the clamp integrated into the assembly; we found that the clamp made no appreciable difference in
the max loads each configuration could handle.
While we don't know the true layup schedule for the bar, we can assume that it is mostly composed of
unidirectional fibers arranged at 0° with respect to the bar length, as this construction provides the most
strength in bending (the primary loading case for the bar). However, the bar would also need several plies
arranged at other angles (like ±45°) to survive clamp stresses and resist torsion applied along the bar by
the user. This construction would also help keep the bar together in the event of a catastrophic crack or
fracture, as the interwoven plies would hold the bar together better. To provide even greater strength, the
wall thickness at various locations on the bar could be adjusted while maintaining similar weight levels.
While we have no way of being sure that our model is accurate, our comparisons to the real product and
to our hand calculations (see Attachment 1) lead us to believe that our model provides reasonably useful
results.

3. Introduction
Carbon fiber components are becoming increasingly popular today in both recreational and professional
biking scenes. While it is commonly agreed upon that such components offer superior performance
characteristics (such as strength and low weight) to those fashioned from metal alloys, it is less clear how
much of a difference they actually make. Unlike with an isotropic material, it isn't an easy task to
determine the strength of a composite component with hand calculations, and this means that finite
element methods must often be employed.
The objective of this project was to investigate the stresses, strains, and deflections at various locations on
the EC70 XC carbon fiber handlebar. Beam, solid, and shell element models were developed to test our
handlebar, and our results were compared with our rudimentary hand calculations for a far simpler model.
These models allowed us to accurately predict the maximum loads that the product can handle and to
quantitatively compare it to similar products with the same geometry but differing composition
(aluminum 6061-T6 and 4130 chromoly steel, for example). This analysis also allowed for weight and
strength comparisons between the different products. Before starting the project, we expected the carbon
formulation to be slightly stronger and lighter than comparable steel and aluminum alloy handlebars, but
also significantly less stiff and far more expensive.
To determine whether or not the results from our models made sense, we needed baseline figures to
compare them to. To get these figures, we made a very rough and conservative model of the handlebar to
determine ballpark figures for max stresses and deflections. Our rough model takes the shape of a
cantilever beam with a constant cross section (the small outer diameter of our more precise model) and
the same length (13.5") as half of the actual handlebar. This may seem like a very rough model, but it is
intentionally conservative compared to the more precise model and will give us a good indication of our
precise model's validity, as we would expect to see lower stresses and deflections in our precise model for
a given loading case. Using a lower-end value for Young's modulus for unidirectional carbon fiber and
our rough model, we calculated a max stress of about 75.1 ksi and a max deflection of about 0.524 inches
for a -200 lbf vertical end load; if the precise model had not posted smaller stresses or deflections than the
rough model, we would have known that there could be a problem with the precise model. We also
calculated a max von Mises stress of about 2410 psi for a torque loading of 100 lbf-in along the shaft of
our rough model. For more information on this rough model and the worked-out calculations, please see
Attachment 1.
Model Development
Our model development began with measurements and pictures being taken of the actual product on our
test bike. From these measurements and observations, our next step was the creation of a SolidWorks
model to get the geometry of the handlebar correct. We took advantage of symmetry and modeled only
half of the handlebar. This model was created using a 3D wire sketch (pictured in Figure 2) to capture the
angles in 3D space and multiple profiles so that a loft could be used to create the handlebar. The model
begins as a straight line 1.5 inches long extending out from the plane of symmetry at the center of the
handlebar. This portion is assigned the large diameter of the bar (1.255 inches). The model then tapers
over a 3 inch segment to the small diameter (0.87 inches) at an angle of 9° up from the horizontal. It then
stays constant at that smaller diameter, but changes direction to 5° up from the horizontal and 5 back from
the horizontal for the last 8.75 inches of length. These profiles were then used to create a loft that passes
through all the profiles along the wire sketch, and a shell operation was done to hollow out the model.
The wall thickness is a constant 0.08 inches. Three views of this model can be found in Figure 3, Figure
4, and Figure 5 below.

4. To simulate the effects of contact between the handlebar clamp and the bar, we needed to model a set of
clamps as well. We modeled one half of our clamping assembly with a 2D sketch in SolidWorks and then
mirrored the sketch along the x-axis, and the model was then extruded to become a 3D part. The clamp
doesn't really model any real-world clamp in particular, but it is the same width as the model on our test
bike. Because the performance of the clamp isn't what we are testing, we felt as though our simple model
would suffice for determining clamp stresses on our handlebar. The clamp can be seen below in Figure 6.
Figure 2. 3D sketch from SolidWorks used to create handlebar loft
Figure 3. Initial SolidWorks model, front view
Figure 4. Initial SolidWorks model, top view

5. Figure 5. Initial SolidWorks model, isometric view
We were then able to import these models into ABAQUS for analysis. For all models and loading cases,
we used an ENCASTRE boundary condition at the thick end of the bar to simulate the fixed condition
that exists at the middle of the whole bar where the clamp acts.
Figure 6. SolidWorks clamp model
For the clamp analysis, we determined the force applied by a single bolt in the clamp assembly with the
bolt tension equation 8-27 found in Reference 1 and then multiplied this number by 4 (the number of
bolts in the assembly) for a conservative loading estimate of the entire assembly. We modeled these
forces in ABAQUS as an equivalent clamping pressure load on the four faces of the clamp. To constrain
the clamp on the bar, first a face-to-face tie constraint was used between each inside clamp face and the
bar. Then we used a shell edge to face constraint between the edge of the bar at the end and the outside
vertical face of each clamp. As we will see later on, we only needed to use the clamp on the shell model

6. because the shell model was the most accurate for all cases and materials. The shell assembly with the
clamp can be found below in Figure 7.
Figure 7. Assembly of the shell model including the clamp
Due to a lack of information regarding the layup schedule of the handlebar, we had to make several
assumptions about the bar's construction and primary loading cases. To begin with, we assumed a
constant wall thickness of 0.080" throughout the bar, which corresponded to the measured wall thickness
of the end of the bar. As we found later, this was most likely a reasonable assumption, as it very
accurately predicted the weight of the real handlebar. Assuming a ply thickness of 0.005", we calculated
that there were 16 plies of unidirectional carbon fiber making up the thickness of the bar. We then chose
several layup schedules based on the assumptions that beam bending was the major loading case and that
the bar additionally had to withstand a non-insignificant amount of torsion. We created and tested three
main types of layups: the quasi-isotropic "black aluminum" type that is popular in aerospace applications
and has a [0°/90°/+45°/-45°] pattern, a layup composed of only 0° and 45° plies in a repeating
[0°/0°/+45°/-45°] configuration which is similar to the layups of composite boat masts, and a layup
consisting of only 0° plies (all plies laid end to end along the handlebar). Each pattern was made
symmetric about the center of the layup.
For the beam model, just the 3D wire sketch shown in Figure 2 was imported into ABAQUS so that pipe
profiles could be created and applied to the sketch. To model the bar's geometry, we used three different
sections for the three aforementioned wire sections in the sketch: one big section for the large diameter
region, one small section for the small diameter region, and a linear taper section that joined the two other
regions. We felt as though this was the best way to approximate the more complex geometry of the actual
component, as it allowed for the best accuracy without using a much more complex sketch and many
more beam sections making up the tapered portion.
For the solid model, the initial SolidWorks model of the bar shown in Figure 3 was imported and a solid
homogeneous section was assigned for use with the aluminum and steel models. We constrained the
entire cross-section surface at the middle of the bar with ENCASTRE boundary conditions to lock it into
place, and then created a reference point at the center of the end of the bar. This point was tied to the
cross-section surface at that end with rigid body ties in order to evenly distribute any point loads or
moments applied at that point to the entire end of the bar. The solid model assembly looks virtually
identical to the shell assembly pictured in Figure 7. Unfortunately, we found that we could not properly
assign layup sections to the solid model, which limited our use of the solid model to only the aluminum
and steel variants of the handlebar. This ultimately meant that the solid model could not be used for the
majority of the project.

7. For the shell model, a slightly modified version of the SolidWorks model was imported with smaller
outside diameters (to account for the width of the shell section when applied at midsection to the shell)
and homogeneous shell sections were used to model the aluminum and steel variants of the bar.
Meanwhile, the 3 different layups mentioned above were created as composite sections and applied to
model the carbon variants of the bar. As before with the solid model, the entire middle cross-section was
constrained with an ENCASTRE boundary conditions, and a reference point was created at the end of the
bar and tied to the shell edge with tie constraints. The completed shell model assembly is pictured above
in Figure 7.
Mesh Development and Convergence
We used mesh convergence studies to determine the optimal element size for each model. In all cases, a
200 lbf end load was applied to the end of the handlebar and the max stress was determined for each
element size. In addition, an isotropic test material (6061-T6 aluminum) was used for each model in order
to simplify the test and eliminate the effects of the layup on the stresses in the bar.
For the beam model, we used standard quadratic (B32) beam elements to mesh the wire sketch. We then
attempted to run a mesh convergence study but noted that the beam elements converged no matter how
few of them we used. Using one element per section (for a total of three elements) yielded the exact same
stresses as a simulation run with hundreds of elements along the length of the handlebar. While this
situation is odd and probably deserve a closer look in the future, we opted in any case not to use the beam
model results, so the impact of this issue is trivial.
We tested all three solid element types (tetrahedral, hexahedral, and wedge) with our solid models. For
each element types, we used standard quadratic elements for better accuracy. We found that the
hexahedral elements worked the best, taking less computational time and fewer elements to converge
upon a solution than the other types. However, all three types converged upon virtually the same stress
values, and none took a prohibitively long time (>1.5 minutes) to run. The results of the solid element
mesh convergence studies can be found in Attachment 2.
For the shell model, standard quadratic elements with reduced integration (S8R) were chosen for all
configurations in order to provide the highest accuracy. With these elements, the shell model converged
with an average element size of 0.05 inches, which equates to about 19500 elements throughout the
model. The model was meshed using a swept mesh technique which produced very even mesh. Despite
needing a large amount of elements in order to yield converged results, the model still ran acceptably
quickly, taking about a minute of computational time for each simulation.
Each model converged upon reasonably similar stresses for the given 200 lbf end load. Both the solid and
the shell models showed max stresses of about 51700 psi in the same spots on the handlebar (at the
beginning of the tapered section), whereas the beam model showed max stresses of 47600 psi and at a
different location (at the bottom of the tapered portion) than in the solid and shell models. We believe the
discrepancies between the solid/shell models and the beam model might be attributable to the fact that the
solid and shell models are modeling curved beam bending stresses for the complex geometry in the
tapered section of the bar, whereas the beam model is comprised of straight sections and cannot take these
factors into account. In any case, the solid and shell models both seemingly provide good results.
However, as mentioned earlier, we could not get the solid model to work while using laminate sections,
so we decided to use the shell model for the rest of this project.
The shell model was checked thoroughly to ensure that its mesh was refined properly and was free from
defects. The smallest angle on any element in the mesh was 76.44°, which is more than acceptable for our

8. purposes. The worst aspect ratio on any element was 1.75, which is far less than the cutoff ratio of 4.0.
We feel as though these results indicate that our shell model was meshed correctly.
Figure 8. Convergence plot for the aluminum shell model
FE Analysis
We encountered many technical issues during this project, but we were able to address most of them in a
satisfactory manner. Our biggest issue regarded implementing loads in our shell and solid models.
Initially, we used shell edge loads for the bending and torsion cases, but we found that they were
producing stresses many times larger than our rudimentary hand calculations were predicting and were
creating odd stress concentrations at the end of the bar. We addressed this by using a reference point at
the end of the handlebar and tying it to the surface or edge at the end of the bar; this had the effect of
spreading out the load to the entire end of the bar, reducing stress concentrations and ensuring that the bar
was loaded correctly. We also had issues getting our shell model to mesh evenly and consistently; we
found that enabling the swept mesh option in the mesh options generated excellent mesh.
We also had issues getting our solid model to accept a lamina section for the purposes of modeling the
carbon variants of the handlebar. We unfortunately were not able to get this issue resolved and ended up
not using the solid model (which was otherwise promising in its results for isotropic materials) in our
project. However, we feel as though we demonstrated the validity of the model, and we believe that
someone with better knowledge of ABAQUS could very likely get the model to produce good results.
Results
After convergence was verified for our shell model, we began our tests by observing the von Mises
stresses in the aluminum and steel shell models and strains for each carbon shell model in post
processing. To compare all models and materials, we determined the highest cantilever and torque loads
the models could take before failure stresses (for the metal alloy variants) or failure strains (for the carbon
fiber variants) were reached. We also looked at tip deflections to check the validity of our model by
comparing the results to our hand calculations. The different materials deflected as we would expect with
the steel deflecting least, the carbon models deflecting more as more layers of differing angles were
added, and aluminum deflecting more than two of the three carbon layups. The carbon layup with only 0°
plies deflected 0.4012 inches which is slightly less than the 0.524 inches that the conservative hand
4.500E+04
4.700E+04
4.900E+04
5.100E+04
5.300E+04
5.500E+04
10 100 1000 10000 100000
MaxStress(psi)
# of Elements

9. calculations predicted, which allowed us to accept the validity of our model. These results can be found
below in Table 1 and the hand calculations are included in Attachment 1.
Material Max Deflection (in)
Carbon: "Black Aluminum" layup 0.7812
Aluminum 6061-T6 0.6160
4130 Chromoly Steel 0.2053
Carbon: 0/0/+45/-45 for 16 layers 0.5434
Carbon: 0/0/0/0 for 16 layers 0.4012
Table 1. Deflection results to prove validity of shell model
To compare to the hand calculations, we ran each model first with a vertical -200 lbf end load for the end
deflections and then with a 100 lbf-in torque (placed at the reference point at the end of the bar as
mentioned previously) to test for maximum shear stress. The aluminum shell model produced a maximum
stress of 2686 psi compared to the 2407 psi predicted by the hand calculations so this was another
verification of our model. Each variant was tested without the clamp, as we will discuss below.
To test the carbon variants, we ran the carbon shell model with the appropriate load and layup to be tested
and then checked the longitudinal (both compressive and tensile), transverse (both compressive and
tensile), and shear strains for each ply in the layup. If any strains in any of the plies exceeded the max
allowable values given by the instructor for the unidirectional fiber material, then the handlebar failed that
loading condition. Iterating through different loads for each layup gave us a good estimate of the max
loads that each layup could handle. The metal variants were iteratively tested in a similar manner to
determine max loads for each material configuration, but von Mises stresses were checked and compared
to yield stresses instead of using failure strain methods. The results of these tests can be found below in
Table 2.
Material
Max End Load
(lbf)
Failure
Mode
Max Torque
(lbf-in)
Failure
Mode
Mass
(lbm)
Carbon: "Black
Aluminum" layup
210 E22 2950 E22 0.33288
Aluminum
6061-T6
150 von Mises 1600 von Mises 0.57232
4130 Chromoly
Steel
240 von Mises 2420 von Mises 1.65798
Carbon: 0/0/+45/-45
for 16 layers
310 E22 2620 E22 0.33288
Carbon: 0/0/0/0 for
16 layers
330 E22 1750 E12 0.33288
Table 2. Maximum load results, failure modes, and masses
For the clamped models, we observed stresses and strains in each model using the loading case mentioned
above in the Model Development section. The following figures represent the results when clamping our
models with a metal clamp modeled from the clamp on the actual handlebar. This clamp creates new
stresses in the bar at the location of the clamp interface with the bar as compared to the models without
the clamp, but the largest stresses in the bar remain almost exactly the same with only a very slight
increase or decrease depending on the model. The much larger stresses that result are only found in the

10. steel clamps which we are not concerned about and which are likely due to the way it is constrained.
When modeling the carbon bar without the clamp, the maximum stresses in bending with a 200 lbf end
load were found to be 134 ksi, while with the clamp the value was 133.8 ksi. The max strains did not
change in any noticeable way with the clamp included or grow to anything approaching dangerous levels
in the area of the clamp interface. The locations of the failure strains also remain unchanged. When
modeling the aluminum bar without the clamp, the maximum stresses were found to be 51.88 ksi, while
with the clamp the value was 53.17 ksi. The results for the clamped carbon bar were exactly the same as
those for clamped aluminum, so the pictures are not included for the sake of redundancy.
Figure 9. Isometric view of clamps in post processing

11. Figure 10. Isometric view of clamped bar in post processing
Discussion
For the most part, the results of our tests seem to confirm our original thoughts as to the advantages and
disadvantages of carbon fiber handlebar construction. Depending on the layup schedule, carbon fiber can
either be comparable to or can far exceed the performance of common cycling materials such as chromoly
steel or 6061 aluminum when judged using weight and strength metrics. In bending tests, the
[0°/0°/+45°/-45°] and [0°/0°/0°/0°] layup variants in particular offer nearly 50% better load-bearing
capacity than the alloy variants for the same shell thickness. This makes sense, as in these configurations
the carbon fibers are mostly arranged along the length of the handlebar, which allows for the most
strength in tension and compression. The carbon variants also [mostly] performed better in shear than the
metal variants. The "black aluminum" layup [0°/90°/+45°/-45°] in particular was especially good in the
torsion tests, as its 45° and 90° plies directly translated to a large amount of shear strength. The
[0°/0°/+45°/-45°] layup also offered good resistance to shear failure, while the [0°/0°/0°/0°] layup was
predictably weak in the torsion test.
It appears that this handlebar in particular is geared more toward minimal weight rather than absolute
strength. There are many other widely used carbon fiber bike handlebars available that weigh a significant
amount more, presumably due to greater wall thicknesses. This is due to more layers of carbon in the
carbon bars and just more material in steel and aluminum versions, which adds strength at the expense of
greater weight. So, in regards to what kind of handlebar someone would want to use, it comes down to
personal preference. If you are not worried about huge loads and big impacts, but would rather further
reduce the weight of your bike, then a handlebar like this one would be a good choice; however, if you
wanted something that will stay intact no matter the severity of the loads or impacts placed on it, then you
might want to go with a thicker-walled carbon model or even an aluminum or steel model if you want to
save some money. A carbon fiber model is going to be a lot more expensive than a comparable steel or
aluminum model, but it will offer a far superior strength-to-weight ratio than other construction methods.

12. While we don't have enough information on the product to definitively say what the layup schedule
must be, we would expect that Easton used a layup schedule with mostly 0° plies running along the
length of the bar due to how the primary loading condition is bending. The actual layup is likely
some proprietary arrangement of plies that is far too complex to back out with ABAQUS simulation;
however, we would expect it to be somewhat similar to the [0°/0°/+45°/-45°] or [0°/0°/0°/0°]
layups we tested, or something in between the two. We would expect at least a few ply layers to be
oriented at an angle with respect to the length of the bar in order to keep the bar from failing in
shear and to keep it together in the event of a sharp impact that would crack the bar. We found that
our shell model very accurately predicted the weight of the real handlebar, predicting a weight of 0.3329
lbf. This result is very comparable to the stated weight of 0.3395 lbf for the actual product, which leads us
to believe that our constant thickness assumption was reasonably valid. If we had to guess, we would
assume that Easton used a thicker section around the tapered portion of the bar (where the highest strains
are) and kept it thinner around the center (where the strains are relatively low). This would be a good way
to significantly increase the strength of the bar without increasing the overall weight.
Conclusions
Modeling of an Easton EC70 XC handlebar was done in ABAQUS to determine the maximum loads that
different material models could take and to do analysis on the weight and strength benefits of using
carbon fiber over traditional metal alloys. Beam, solid, and shell element models were created for each
material to determine which models would be most accurate for determining results. Deflections and
stresses were compared to rough hand calculations done to determine the validity of each model and a
mesh convergence study was completed to ensure the most accurate results. Using the shell model,
maximum loads were found for a cantilever end load and a torque load for Aluminum 6061-T6, 4130
Chromoly Steel, and three different carbon fiber layups to determine the strengths and weaknesses of each
model. We had to take a design approach to estimate the layup of the carbon fiber bar because we did not
have information regarding the actual layup schedule; however, we know that our geometry is accurate
and we believe that our results are accurate due to the comparisons between our results and hand
calculations. From these results (found in Table 2), we saw that steel is very strong in both cases but you
face the problem of greater weight. The aluminum was the weakest in both loading cases, but aluminum
is relatively light and inexpensive to produce. For the carbon layups, we see that the more 0° layers
(meaning the fibers are oriented along the length of the beam) there are, the more strength in bending
there is, but less resistance to torsion. We guessed that the most likely layup schedule for the bar is one
similar to our [0°/0°/+45°/-45°] layup, as it provides nearly as much bending strength as the
[0°/0°/0°/0°] layup but also would stay together better in rough use due to the crossing plies. Of
course, the actual layup schedule is likely to be far more sophisticated than our simple layups.
Attachments
1. Hand calculations and model estimates
2. Mesh convergence tables and plots for solid element model
References
1. Budynas, Richard G., J. Keith. Nisbett, and Joseph Edward. Shigley.Shigley's Mechanical
Engineering Design. New York: McGraw-Hill, 2011. Print.