The document summarizes a finite element analysis of a Hyperloop pod frame. Three loading scenarios were analyzed: initial acceleration, constant velocity, and power failure impact. The frame was modeled in CREO and analyzed in ANSYS. The maximum stress of 19.2 GPa occurred during a power failure impact scenario. A mesh independence study refined the mesh to 3.1 million elements. Reinforcements will be added to stress concentrations to ensure the frame withstands expected loads.

1. Finite Element Analysis of Mercury III Hyperloop Scale Model Pod Frame
by:
William Steppe
Michael Hamman
Philip Haglin
Jared Kobrieger
Mercury III Hyperloop Team

2. The pod has been designed for the Hyperloop Competition that is being hosted by SpaceX in late
August of 2016. A finite element analysis has been performed on the frame to estimate the forces that
will be applied during its operation. Three different loading scenarios were analyzed; the initial
acceleration from the pusher cart, constant velocity, and the initial impact on one wheel in the event of
a power failure. The frame was modeled using CREO 3.0 and analyzed with ANSYS 14.5. Von Mises
Stress and Total Deformation were observed during this test as 6061-T6 Aluminum, the material of the
frame, is a ductile material and therefore falls under the test specifications of Von Mises. To ensure an
accurate mesh, an independent mesh analysis and refinement was performed under the constant
velocity loading scenario as it was the scenario with the least number of forces and therefore the easiest
to run. The element size started at 1cm with 632,907 elements and ended at 2.5mm element size and
3,127,723 elements. The maximum displacement that was recorded was 0.153m and is under the
impact failure scenario at the front of the pod. The maximum stress was 19.2 GPa and was under the
same scenario.

3. Contents
Introduction ..................................................................................................................................................4
Methodology.................................................................................................................................................4
Analysis and Results: Constant Velocity.......................................................................................................5
Analysis and Results: Acceleration...............................................................................................................7
Analysis and Results: Power Failure...........................................................................................................10
Mesh Independent Study............................................................................................................................11
Conclusion...................................................................................................................................................13
Works Cited.................................................................................................................................................14

4. Introduction
The frame of the pod is the most important structure as all the subsystems mount to it. Because of this,
it needs to be analyzed to ensure that under large loading scenarios it will not frail from stress or
deformation. The analysis was performed using ANSYS 14.5, and was performed on a frame modeled in
CREO 3.0.
Methodology
The frame will be made out of 6061-T6 Aluminum since that material is light weight, strong, and
inexpensive, as well as easy to manufacture. The following material properties were used for the
analysis: Tensile Yield Strength is 276MPa, Ultimate Tensile Strength is 310MPa, Modulus of Elasticity is
68.9 GPa, and Poisson’s Ratio is 0.33. The model of the frame utilized for the analysis was designed as a
single part, utilizing sweeps and extrusions-to-face features to create all the tubes and stock. This was
done so that there would be no intersecting volumes and so there would be no spaces in between stock
that would get meshed poorly at a high refinement. All of the holes for mounting components were
added to the stock, so that the forces that those masses would create could be applied on them, which
will more accurately resemble the pod. The pod frame was cut in half down the symmetric plane and
symmetry was used to make the mesh smaller which shortened the time it took to mesh and solve the
analysis. The frame was then fixed in the locations where the two halves of the frame would have met
in the longitudinal direction to simulate no deformation and shared stresses and strains in the
aforementioned direction.
Figure 1: CREO modeled frame half
The analysis performed was static structural modeling function, which simplified the analysis of the
frame at the maximum loading scenarios, as those would be the points where the frame would fail.
There were three different scenarios that were decided to be ran as they were estimated to be the
maximum loading scenarios: the acceleration from the pusher cart, constant velocity, and the impact

5. force sent to one wheel if the entire pod were to lose power and land on it. The mesh of the frame
started at a 1cm element size. An independent mesh analysis/refinement was then performed on the
constant velocity scenario to get an accurate mesh size, as that scenario had the fewest forces applied
to it. Once the mesh size was deemed acceptable, the other two loading scenarios were ran.
Analysis and Results: Constant Velocity
The constant velocity scenario was the easiest scenario to run, and therefore was ran first so that the
mesh independent study could be run. The loads for the constant velocity would also be similar
amongst all the tests. The loads that were applied to the frame under this scenario were the masses of
all of the components that would sit on the frame. The masses applied were as follows: the liquid
nitrogen tank that would initially hold the nitrogen was 15.8kg, the liquid nitrogen tank reservoir was
9.167kg, the manikin seat assembly was 20kg, and the computer and electrical components was 40kg.
In restricting the degrees of freedom for the pod, the magnets were considered wheels and fixed in
position. The theory behind this is that once the levitation of the pod is static and the magnets are
under constant load they will counteract the effects of gravity and support the weight of the pod.
The total deformation experienced in the final iteration of the constant velocity analysis was 6.11e-5m,
and was located where the seat and electronic components would be situated, as shown in Figure 2 and
Figure 3.
Figure 2: Total deformation under constant velocity

6. Figure 3: Zoomed in location of total deformation under constant velocity
The maximum Von Mises Stress is around the same location, located specifically at the inner hole where
the computer and electronic components box will be mounted, shown in Figure 4 and zoomed in in
Figure 5 and Figure 6. The maximum Von Mises Stress is 8.29MPa.
Figure 4: Maximum Von Mises Stress under constant velocity

7. Figure 5: Zoomed in maximum Von Mises Stress under constant velocity
Figure 6: Hole that experiences maximum Von Mises Stress under constant velocity
Since 8.29MPa is well under the tensile yield strength of the aluminum, this stress is not a concern.
Analysis and Results: Acceleration
The only change from the constant velocity scenario and the acceleration scenario is that the
acceleration scenario will experience a load at the location of the interface for the pusher cart which is
equal to 2 times the mass of the pod multiplied by the acceleration of the pusher cart, which is 1g,
which creates a force of 19620N. The total deformation, shown in Figure 7 and Figure 8, is 0.18m at the
location of the interface.

8. Figure 7: Total deformation under acceleration
Figure 8: Zoomed in location of total deformation under acceleration
The maximum Von Mises Stress is 2.62GPa and is located at a weld joint where the longitudinal tube
that the pusher interface is welded to meets one of the primary latitudinal tubes, shown in Figure 9 and
zoomed in in Figure 10.

9. Figure 9: Maximum Von Mises Stress under acceleration
Figure 10: Zoomed in location of maximum Von Mises Stress under acceleration
Although the stress is much higher than the tensile strength that the Aluminum can support, this isn’t
too much of a concern. This acceleration force is applied assuming that the magnets are completely
resisting any movement, however that is an inaccurate description since they will allow the pod to move
freely with the applied force from the pusher cart. Since there is a stress concentration there a
triangular stock of aluminum will be welded there to allow the stress to be spread out more freely,
which should alleviate any concerns of stress from the force of the pusher cart.

10. Analysis and Results: Power Failure
The impact failure stress was estimated to be the highest as it entails the entire pod dropping all of its
mass from the maximum velocity onto one wheel, which equated to a force of 179,098.34N. This force
was split in half and applied to the two wheel mount locations at the front of the frame. The maximum
deformation, shown in Figure 11 and Figure 12, is 0.153m, and is at the front-most tube on the frame.
Figure 11: Total deformation under power failure
Figure 12: Zoomed in maximum deformation under power failure
The maximum Von Mises Stress, under power failure is 19.2GPa, shown in Figure 13 and Figure 14, and
is located at one of the magnet mounts. However, this could be an inaccurate representation of the
stress as the magnet was still considered to be the degree of freedom constraint. The new degree of
freedom constraint would be better represented as the wheels themselves which could then move to

11. the rectangular stock that the wheels sit in. However, the deformation and stress that the frame
experienced under this impact needed to be observed and a degree of freedom constraint cannot be
applied to a location with a stress, as there will be no deformation observed.
Figure 13: Von Mises Stress under power failure
Figure 14: Zoomed in image of maximum Von Mises Stress under power failure
Mesh Independent Study
The mesh independent study was performed to ensure that a proper mesh was utilized in the testing of
the loading scenarios. The constant velocity scenario was utilized to perform the independent study as
it had the least number of loads which would help the solver run faster. The element size started at 1cm
and was decreased until an equilibrium was started to be observed. The element size and the maximum

12. displacement were the variables that were observed in creating the mesh independent study. Table 1
shows the numerical results and Figure 15 shows the graph that was plotted.
Table 1: Numerical results of the mesh independent study
Figure 15: Mesh independent study results
As can be observed by the graph, equilibrium was starting to be observed at an element size of
0.0025m. The mesh refinement would have continued, to get an even more equilibrium graph, however
the computer did not have enough computing power to solve any refiner of a mesh. The final element
count was 3,127,723 elements throughout the frame at a mesh size of 0.0025m.
Test Number Element Size (m) Element Number Max Deformation (m) Max von Mises Stress (Mpa) Max Elastic Strain (m/m)
1 0.0100 632907 5.9200E-05 8.710 0.0001257
2 0.0095 632042 6.0063E-05 8.780 0.0001237
3 0.0090 635973 6.0138E-05 8.823 0.0001247
4 0.0085 643532 6.0130E-05 8.680 0.0001225
5 0.0080 664403 6.0485E-05 8.880 0.0001253
6 0.0075 680860 6.0700E-05 8.800 0.0001242
7 0.0070 697417 6.0800E-05 8.860 0.0001250
8 0.0065 719833 6.0750E-05 8.850 0.0001249
9 0.0060 760735 6.0851E-05 8.750 0.0001234
10 0.0055 818024 6.0910E-05 8.940 0.0001262
11 0.0050 873036 6.0900E-05 8.890 0.0001250
12 0.0045 977833 6.1000E-05 8.950 0.0001262
13 0.0040 1155823 6.1000E-05 8.900 0.0001260
14 0.0035 1407070 6.1000E-05 8.910 0.0001260
15 0.0030 1838293 6.1100E-05 8.960 0.0001265
16 0.0025 3127723 6.1100E-05 8.930 0.0001259

13. Conclusion
In conclusion, the stresses that the pod will experience shouldn’t be very high. The acceleration and the
power failure loading scenarios did show very high stress concentrations, however they should not be as
high as predicted as the loading of the frame will be different in real life and needed to be simplified for
the initial analysis. Reinforcement will be applied at stress concentrations and some of the tubes will be
enlarged in order to withdraw any doubt that the frame will fail under loading.

14. Works Cited
ANSYS INC, "ANSYS.com," ANSYS INC, 2015 . [Online]. Available: http://www.ansys.com/. [Accessed NA].
PTC, "PTC CREO," [Online]. Available: http://www.ptc.com/product/creo/new. [Accessed December
2015].