FEM project # 2

Title: FEM Project # 2
Name: Li James
Due Date: 21 April 2016 @ 5:00 pm
Class: ME37100
Professor: Benenson, G.

Overview
The purpose of this project was to evaluate a solid model design of a pulley using Finite Element
Method (FEM) to analyze any potential failure and redesign of this pulley model. The way failure was analyzed
in this design was to locate the area of maximum stress. In the simulation, the pulley was connected to a
motorized shaft and an object was lodged into one of the gaps on the pulley. The pulley continued to rotate in
spite of the obstacle, causing stress and generating a potential failure area. The project description gave me a
few constraints. The first constraint is that the material is 1020 steel. The second constraint is that the torque is
set at 100 N*m at one end of the shaft. The third constraint was that the direction of the torque is rotated based
on “Axis 1” (see figure 1). The fourth constraint is that one of the inner rectangles of one of the pulley gap
would be restrained. The fifth constraint is that the safety factor is 2 (divided the maximum yield strength of the
material by 2). The pulley design is acceptable if the maximum stress caused by the obstruction is below the
maximum yield strength of the material (von mises stress will be used to analyze this model) with the safety
factor included.
Figure 1: the pulley model
Procedure:
Analysis with the initial constraints only
I selected my boundary conditions based on the given constraints (see figure 2). The shaft was rotating
counter-clockwise, when the torque was applied, due to a motor attached to the end of the shaft. The right inner
rectangle at the most gap of the pulley was where the restraint was applied; that restraint represents the obstacle
that is lodged into the gap and the stress was generated from the force applied against the obstruction. Since the
rotation was counter-clockwise, the force of the obstruction should be normal to rotational force. That is why I
applied the restraint to the right wall of the top-most gap; the rotational force was to the left of the wall and the
force applied to the right wall was normal to the rotational force.

Figure 2: Initial force constraints on the model
After I applied the constraints, I ran a simulation with the given constraints and then I displayed the
stress and displacement vector plots (see figures 3 and 4). I hypothesized that the maximum stress would be at
the connection point between the shaft and the pulley and that the maximum displacement would be at where
the torque was applied. In a real life scenario, the shaft will attempt to spin the pulley against the obstruction
and the force will cause the shaft to twist at the torque application point and the stress to be concentrated at the
connection point due to the change in area form the shaft to the bore. Based on my observation of the two plots,
I declared this simulation invalid due to where the maximum stress and displacement was located. The
maximum stress was located at a vertex of the right inner wall and the maximum displacement was located at
the bottom of the pulley. This means that the pulley is translating away from or towards another pulley. If the
pulley was allowed to translate, the system balance would be thrown off. If the pulley translation was allowed to
happen in actual operating conditions, the translation will cause the pulley to wobble in place and prevent the
pulley itself from transferring enough force to the belt that is attached to it; if the force transfer is insufficient,
the belt may not move properly and the entire pulley system would be stalled.
Figure 3: Stress Plot with initial constraints (10 mm second order global mesh)

Figure 4: Vector Plot with initial constraints (10 mm second order global mesh)
Analysis with the initial constraints and new boundary conditions
To solve the pulley translation issue, I added new boundary conditions to the simulation. I decided to
place the new boundary conditions by restraining the inner circular bore of the pulley as fixed hinges (see figure
5). I used an overhead pulley as inspiration for the new restraints (see figure 6), where the inner bores are held
in place with hinges. After I placed the restraints, I reran the simulations again to determine the location of the
maximum stress and displacement.
Figure 5: Restraints for the inner bores

Figure 6: Overhead pulley
After I reran the simulations, I reanalyzed the location of the maximum stress concentration and
displacement (see figures 7 and 8). This time, I deem the simulation valid. The maximum stress concentration
was near the connection point between the shaft and pulley and the maximum displacement was at where the
torque was applied, as per my predictions. There was negligible translation from the pulley meaning that most
of the force from the pulley would be transferred to the belt once the obstruction is removed and the pulley
system can run smoothly. As with real life, the simulation showed that the torque was highest at the application
area because the motor will deform the shaft at the application area as the shaft attempts to spin the pulley
against the obstacle and the stress concentration was highest near where the shaft and pulley connected due to
the area change between the cylindrical shaft and the circular bore.
Figure 7: Stress Plot with new boundary conditions (10 mm second order global mesh)

Figure 8: Displacement Plot with new boundary conditions (10 mm second order global mesh
Convergence testing via local h-refinement
After I ran the simulation with the new boundary condition, I tested for convergence in order to
determine whether or not the solution of the stress value was valid. I decided to use a local mesh (see figure 9)
on the area of highest stress concentration (near the shaft-bore connection) to determine the convergence
because I know where the area of maximum stress is (failure area) and a global mesh h-refinement takes too
much time to run and may crash the simulation if the meshing is too fine for the software to handle. The
convergence test data will be shown in the results section.
Figure 9: Local h-refinement with the area to be refined.

However, there was a re-entrant edge between the shaft and the bore, where the stress concentration was
the highest. The re-entrant edge causes a stress-singularity that will keep increasing the maximum stress
concentration as the mesh is refined. The following formula shows why the stress singularity keeps increasing
the maximum stress at the area of concentration (the mathematical model used in the FEM simulation, for the
model in figure 9, was based on the following formula because the torque was the applied force and the area of
concentration was at shaft-bore connection edge and those two variables were needed to solve for the stress):
𝜎 =
𝐹
𝐴
, Where: σ = Stress; F = force; A = Area
The stress singularity was generated due to an infinitesimally small area at the re-entrant edge. That negligible
area causes the stress to go up as the mesh is refined because the area is inversely proportional to the stress. As
the area approaches zero, the stress approaches infinity. This relationship prevents any convergence from the
local h-refinement on the model shown in figure 9. A solution to this problem would be to add a fillet at the re-
entrant edge to create a large enough area to eliminate the re-entrant edge. This may result in stress convergence
through local h-refinement at the fillet because the area is no longer infinitesimally small; the convergence test
will be shown in the results section. By eliminating the re-entrant edge, the stress-related hot zones around that
area are averted. The removal of the hot zones means that the stress concentration around that area is lower.
This increases the strength of the shaft connection and lowers the chance of failure.
Figure 10: Addition of a fillet
Results
Convergence testing via local h-refinement (continued)
Simulation Tests Trial 1 Trial 2 Trial 3 Trial 4 Trial 5 Trial 6
Maximum Stress (MPa) [von mises] 74.8 77.8 82.4 87.6 97.9 122.4
Maximum Displacement (mm) [URES] 0.02885 0.02889 0.02892 0.02896 0.02897 0.02901
Number of Elements 5854 6556 7446 9207 12622 22262
Number of Nodes 10040 11098 12795 14875 19712 33631
Degree of Freedom 30057 33231 38322 44562 59073 100830
Global Size (mm) 10 10 10 10 10 10
Local Size (mm) 3 2.5 2 1.5 1 0.5
Fillet Radius (mm) None None None None None None
Table 1: Simulation data for local h-refinement with the original model

Figure 11: Stress Analysis for the local h-refinement with the original model
As expected, we see that from figure 11, the results diverged as the mesh was refined. The boundary
conditions were set at the bores (see figure 5) and at the initial constraints (see figure 2). The reason the
simulation data diverged was due to an issue with the model that rendered mathematical model used for this
FEM simulation was invalid (explained in the procedure section: “convergence testing via local h-refinement”).
This means the results for this simulation test was meaningless and the model geometry was revised in order to
create a more reliable simulation (see figure 10).
Convergence testing via local h-refinement using a 1mm fillet
Maximum Stress (MPa) [von mises] 101.3 104.3 105 103.6 100.2 103.8
Number of Nodes 11286 12840 14542 16724 25530 43680
Global Size (mm) 10 10 10 10 10 10
Local Size (mm) 3 2.5 2 1.5 1 0.5
Fillet Radius (mm) 1 1 1 1 1 1
Stresspercentchange fromthe trial average 1.68 1.23 1.91 0.550 2.75 0.744
Table 2: Simulation data for local h-refinement with 1 mm fillet
Figure 12: Stress Analysis for the local h-refinement
0
20
40
60
80
100
120
140
0 5000 10000 15000 20000 25000 30000 35000 40000
Stress (MPa)
[von mises]
Number of Nodes
Convergence Test (No fillet)
0
15
30
45
60
75
90
105
120
0 10000 20000 30000 40000 50000
Stress (MPa)
[von mises]
Number of nodes
Convergence Test (1 mm fillet)

Figure 13: 1 mm fillet
Based on figure 12, the results of this FEM Simulation appeared to converge at around 103 MPa as the
number of nodes increases with the maximum stress at around 105 MPa concentrated at where the fillet is
located. I set the location of the local h-refinement at the fillet area (see figure 13) and boundary conditions
were the same as with the original model (see figures 2 and 5). The convergence in the data and the minimal
change in stress (less than 4 % from the average stress of 103.03 MPa for the 6 trials) showed that the solution
for this FEM simulation test study was valid.
Maximum Stress (MPa) [von mises] 85.5 82.9 83.1 84.8 85.1 87
Number of Nodes 11359 12409 14684 17285 25694 44009
Global Size (mm) 10 10 10 10 10 10
Local Size (mm) 3 2.5 2 1.5 1 0.5
Stresspercent change from the trial average 0.905 2.16 1.93 0.0787 0.433 2.68
0
10
20
30
40
50
60
70
80
90
100
0 5000 10000 15000 20000 25000 30000 35000 40000 45000 50000
Stress (MPa)
[von mises]
Number of Nodes

Same result as with “Convergence testing via local h-refinement using a 1 mm fillet", but with the stress
convergence at around 85 MPa, the maximum stress at 87 MPa, and the average stress at 84.73 MPa (see table 3
and figures 14 and 15)
Number of Nodes 11890 12704 14643 18126 30398 60021
Global Size (mm) 10 10 10 10 10 10
Local Size (mm) 3 2.5 2 1.5 1 0.5
Stress percent change from the trial average 3.73 1.92 0.237 0.668 2.48 2.74
0
10
20
30
40
50
60
70
80
90
0 30000 60000 90000 120000 150000 180000 210000
Stress (MPa)
[von mises]
Number of Nodes

Same result as with “Convergence testing via local h-refinement using a 1 mm fillet ", but with the stress
convergence at around 79 MPa, the maximum stress at 79.5 MPa, and the average stress at 77.38 MPa (see table
4 and figures 16 and 17)
Number of Nodes 11602 13225 14380 19191 28169 74625
Global Size (mm) 10 10 10 10 10 10
Local Size (mm) 3 2.5 2 1.5 1 0.5
Stress percent change from the trial average 1.47 0.383 0.383 0.0226 0.970 1.24
0
10
20
30
40
50
60
70
80
0 10000 20000 30000 40000 50000 60000 70000 80000
Stress (MPa)
[von mises]
Number of Nodes

Same result as with “Convergence testing via local h-refinement using a 1 mm fillet ", but with the stress
convergence at around 74 MPa, the maximum stress at 74.8 MPa, and the average stress at 73.38 MPa (see table
5 and figures 17 and 18)
Fillet radius effects on the maximum stress at the area of concentration
Simulation Study Fillet Radius (mm) Maximum von mises Stress (MPa) for each simulation study
1 None 122.4
2 1 105
3 2 87
4 3 79.5
5 4 74.8
Table 6: Stress vs. fillet radius per simulation
Based on table 6, adding a fillet to the model geometry lowers the maximum stress at the area of
concentration and the larger the fillet, the lower the maximum stress. As the fillet eliminates the re-entrant edge
and the hot zones of stress, it causes the maximum stress to concentrate onto the fillet because the stress was
highest near the re-entrant edge (see figure 7 and tables 2 through 5). As the fillet gets bigger, it dissipates more
of stress concentration by spreading it out towards a larger area. As a result, the maximum stress at the area of
concentration decreases. Since the simulations in this FEM study undergoes torsion loading, we can look at the
stress concentration factor for the fillet in order to determine the maximum von mises stress for the analytical
solution for comparison to the simulation data and to the safety factor addled yield strength of the material. This
will be shown in the next section

Analytical results and simulation data comparison to material yield strength
Figure 20: Torsion-based shaft and fillet analysis
The formulas needed to obtain the analytical solution are as following:
𝜏0 =
𝑇 ∗ 𝑐
𝐽
; 𝑐 =
𝑑
2
; 𝐽 =
𝜋 ∗ 𝑑4
32
𝜏 𝑚𝑎𝑥 = 𝐾𝑡𝑠 ∗ 𝜏0 =
𝜎 𝑣𝑜𝑛 𝑚𝑖𝑠𝑒𝑠
√3
𝜎 𝑣𝑜𝑛 𝑚𝑖𝑠𝑒𝑠( 𝑎𝑛𝑎𝑙𝑦𝑡𝑖 𝑐 𝑎𝑙) = 𝜏 𝑚𝑎𝑥 ∗ √3
𝑃𝑒𝑟𝑐𝑒𝑛𝑡 𝑐ℎ𝑎𝑛𝑔𝑒 (%) = |
𝜎 𝑣𝑜𝑛 𝑚𝑖𝑠𝑒𝑠 ( 𝑆𝑖𝑚𝑢𝑙𝑎𝑡𝑖 𝑜 𝑛) − 𝜎 𝑣𝑜𝑛 𝑚𝑖𝑠𝑒𝑠 ( 𝑎𝑛𝑎𝑙𝑦𝑡𝑖𝑐𝑎𝑙)
𝜎 𝑣𝑜𝑛 𝑚𝑖𝑠𝑒𝑠 ( 𝑎𝑛𝑎𝑙𝑦𝑡𝑖𝑐𝑎𝑙)
|∗ 100
Legend
𝜏0 = 𝑁𝑜𝑟𝑚𝑎𝑙 𝑠𝑡𝑟𝑒𝑠𝑠 ( 𝑀𝑃𝑎);
𝑇 = 𝑇𝑜𝑟𝑠𝑖𝑜𝑛𝑎𝑙 𝑓𝑜𝑟𝑐𝑒 ( 𝑁 ∗ 𝑚) = 100
𝑟 = 𝑓𝑖𝑙𝑙𝑒𝑡 𝑟𝑎𝑑𝑖𝑢𝑠 ( 𝑚) [𝑠𝑒𝑒 𝑓𝑖𝑔𝑢𝑟𝑒 20]
𝑑 = 𝑠ℎ𝑎𝑓𝑡 𝑑𝑖𝑎𝑚𝑒𝑡𝑒𝑟 ( 𝑚) = 0.025
𝐷 = 𝐵𝑜𝑟𝑒 𝑑𝑖𝑎𝑚𝑒𝑡𝑒𝑟 ( 𝑚) [𝑠𝑒𝑒 𝑓𝑖𝑔𝑢𝑟𝑒 20] = 0.05
𝐷
𝑑
[𝑠𝑒𝑒 𝑓𝑖𝑔𝑢𝑟𝑒 20] =
0.05
0.025
= 2
𝜏 𝑚𝑎𝑥 = 𝑀𝑎𝑥𝑖𝑚𝑢𝑚 𝑠ℎ𝑒𝑎𝑟 𝑠𝑡𝑟𝑒𝑠𝑠 ( 𝑀𝑃𝑎);
𝐾𝑡𝑠 = 𝑇𝑜𝑟𝑠𝑖𝑜𝑛 𝑠𝑡𝑟𝑒𝑠𝑠 𝑐𝑜𝑛𝑐𝑒𝑛𝑡𝑟𝑎𝑡𝑖𝑜𝑛 𝑓𝑎𝑐𝑡𝑜𝑟 (𝑛𝑜 𝑢𝑛𝑖𝑡𝑠)
𝜎 𝑣𝑜𝑛 𝑚𝑖𝑠𝑒𝑠( 𝑎𝑛𝑎𝑙𝑦𝑡𝑖 𝑐 𝑎𝑙) = 𝑀𝑎𝑥𝑖𝑚𝑢𝑚 𝐴𝑛𝑎𝑙𝑦𝑡𝑖𝑐𝑎𝑙 𝑣𝑜𝑛 𝑚𝑖𝑠𝑒𝑠 𝑠𝑡𝑟𝑒𝑠𝑠 (𝑀𝑃𝑎)
𝜎 𝑣𝑜𝑛 𝑚𝑖𝑠𝑒𝑠 ( 𝑆𝑖𝑚𝑢𝑙𝑎𝑡𝑖𝑜𝑛) = 𝑀𝑎𝑥𝑖𝑚𝑢𝑚 𝑆𝑖𝑚𝑢𝑙𝑎𝑡𝑖𝑜𝑛 𝑣𝑜𝑛 𝑚𝑖𝑠𝑒𝑠 𝑠𝑡𝑟𝑒𝑠𝑠 (𝑀𝑃𝑎)

Simulations (exclude the simulation with no fillet) 1 2 3 4
Radius of fillet (m) 0.001 0.002 0.003 0.004
Calculated Normal Stress (MPa) 32.59 32.59 32.59 32.59
r/d 0.04 0.08 0.012 0.016
Torsion stress concentration factor (Approximated from figure 20) 1.80 1.45 1.40 1.36
Calculated Maximum Shear Stress (MPa) 58.67 47.26 45.63 44.33
Maximum Analytical von mises Stress (MPa) 101.62 81.86 79.04 76.78
Maximum simulated von mises Stress (MPa) 105 87 79.5 74.8
Percentage difference between analytical and simulated results 3.22 5.91 0.58 2.65
Material Yield Strength of 1020 steel (MPa) [von mises] 175
Table 7: Comparison between the analytical results, the simulated results, and the material yield strength
Discussion
Overall, I found this FEM project to be a fairly effective learning experience for the failure analysis of a
pulley. I managed to gain new analytical techniques needed to predict how the pulley was going to when an
obstacle got lodged into one of the pulley holes by testing the model with the initial constraints and by adding
new constraints if the initial constraints were insufficient. When I ran the simulation with the initial constraints,
I expect the maximum stress to be at the joint between the shaft and the pulley bore and the maximum
displacement to be at where the torque was applied under the belief that the pulley would be spinning in place.
What I did not expect the pulley to wobble in place with the initial constraints when I animated it. When I
reanalyze the constraints, I realized that there was nothing holding the pulley in place besides the obstruction
and that this lack of restraints reflected in the simulation results. The wobbling threw off my prediction because
the maximum stress concentration was located at where the obstacle was fixed and the displacement was
highest at the bottom pulley wheel. This makes sense because there was nothing restraining the pulley besides
the obstruction; this means that the stress will be concentrated at where the obstruction was fixed due to the
torque spinning the pulley against the obstruction. The maximum displacement location also makes sense
because the pulley has a larger diameter than the shaft and thus has to spin faster to cover the distance from the
size difference to achieve in the same amount of time (formula for time: time = distance / velocity). However,
the reason the pulley’s displacement was highest only at bottom was because the obstruction limits the
displacement and it was at located at the top gap of the pulley; this meant that as you go closer to the obstacle,
the displacement decreases. Unfortunately the initial constraints alone are not enough to solve the simulation
because in real life, a wobbling pulley cannot transfer enough its force to the belt needed and run the pulley
system. This means that new boundary conditions should be added because the initial constraints, by
themselves, were non-indicative of how a pulley actually works.
I decided to add new boundary conditions at the two inner cylindrical bores of the pulley and set them as
fixed hinges and reran the simulations with these new constraints. I used an overhead pulley (see figure 6) as
inspiration for the new boundaries. For details about why I chose these boundary restraints, see procedure
section: “Analysis with the initial constraints and new boundary conditions”. Suffice to say these new restraints
met my hypothesis of how a real life pulley would behave when an obstacle gets caught in one of the pulley’s
gaps (see procedure section: “Analysis with the initial constraints only” for details regarding my hypothesis). I
decided to refine the meshing of the model simulation using a local h-refinement at the area of the highest stress
concentration to test for convergence to verify the validity of the solution because that is where the pulley will
most likely fail and a global refinement takes longer and is heavier on the computer system when compared to a
local refinement.

I ran the simulation with the local h-refinement 6 times at the shaft-bore connection point. I started with
a 3 mm local mesh then refined the local mesh by 0.5 mm for each subsequent trial. As I expected, the
refinement caused the stress analysis plot to diverge (see figure 11). I believed the divergence was caused by the
re-entrant edge at the shaft-bore connection that created a stress singularity (for further details about my
divergence analysis, see procedure section: “Convergence testing via local h-refinement” and result section:
“Convergence testing via local h-refinement (continued)”). I decided to add a fillet at the edge where the shaft
and bore connected and refine the mesh at that fillet to eliminate the re-entrant edge. I did this to try and get the
stress analysis plot to achieve convergence and to have minimal stress variations during refinement, so I can
validate the simulation for real world analysis.
After I added the fillet, I decided to run 4 simulations with 6 trials each. I started the first simulation
with a 1 mm radius fillet and increase the fillet radius by 1 mm for each subsequent simulation. The mesh
refinement for each trial was the same as with the simulation without the fillet. This time the stress analysis plot
converged (see figures 12, 14, 16, and 18) with little stress variation between each trial for each simulation. The
maximum stress concentration at the fillet decreases as I increase the fillet size (see Table 6); for further details,
see: result section: “Fillet radius effects on the maximum stress at the area of concentration”. Once I obtained
these results, I decided to compare it to the analytical solution and then to the material yield strength in order to
determine if the simulations were accurate for failure analysis and whether the new redesigns were acceptable
or not.
From table 7, we can see that the difference between the analytical and simulated solution is within
acceptable limits of each other (less than 6% deviation for each simulation). This, along with the validity of the
simulations, meant that the simulations for the failure analysis of the pulley were fairly accurate and can be used
for real life failure analysis of the pulley. For both solutions, the maximum von mises stress was well below that
of the yield strength of the material (1020 steel) for every fillet radius shown. This means the new geometry
redesigns for the pulley was acceptable when used with the material. The reason the simulation without the fillet
was not included was because it has no radius. If the radius is zero, then r/d = 0. As we can see from figure 20,
as the r/d approaches zero, torsion stress concentration factor ( 𝐾𝑡𝑠) approaches infinity for D/d = 2. The
maximum shear stress and von mises stress will approach infinity as well; this renders the analytical results for
that simulation invalid and the data divergence (see figure 11) means that the simulation for that particular
model cannot be trusted.
If I were to do this project differently, I would probably run more trials for the FEM simulation without
the fillet to show the divergence more clearly. The software itself produced fairly accurate simulations of how
the pulley would fail in real life and, in this case at least, I accepted that the simulations showed me reasonably
accurate data for failure analysis of the pulley.
Resources
1. http://web.mae.ufl.edu/nkim/eas4200c/VonMisesCriterion.pdf
2. Shigley (2010), Mechanical Engineering Design 9th edition, Pennsylvania, N.Y: McGraw-Hill Series

FEM project # 2

Recommended

Recommended

More Related Content

What's hot

What's hot (20)

Viewers also liked

Viewers also liked (12)

Similar to FEM project # 2

Similar to FEM project # 2 (20)

FEM project # 2