# 11 Finite Element Analysis

Document Sample

```					Finite Element Analysis, Chassis
Now we have a chassis and structure design that looks great, leaves room for
every component, allows the axles to travel in exactly the same way, and provides
mountings for everything that needs to be mounted. This, however, is only part of the
structural requirements. The structure must also, as its name suggests, provide enough
structure and strength to support the loads that the robot can expect to see.
In order to determine this, we have used the ANSYS finite element analysis
(FEA) software package. The structure pictured above is a extremely highly non-
deterministic, interlaced truss structure which would incredibly impractical if not
impossible to solve in closed form. Fortunately for us, FEA software exists that can
approximate a solution in a very effective and accurate way.
Over the course of the following analysis, we were able to examine the structural
integrity of the chassis and axles that we had designed for the construction of this robot.
These structures must be capable not only of supporting the weight of the robot, which
may exceed 350 pounds, but also a significant payload. We have prepared eight different
load cases that we will use to test the chassis’ strength in a variety of different situations.
We will also apply two different load cases to the axle design to evaluate their strength.

Simplifying the Structure for Export
Pictured to the right is the
model which we wish to analyze
using the ANSYS FEA software
package. However, it is not as
simple as exporting the solid
model with an .iges file extension
and importing it into ANSYS.
First of all, we have modeled the
chassis with a very high level of
detail; each member of the chassis
is a square or rectangular tube with a wall thickness of one sixteenth of an inch.

76
This means that there are many, many places in this model where there is open
space that is completely enclosed by solid structure. While this is not a problem for
SolidWorks, ANSYS cannot handle it. If you attempt to import a solid object that
contains pockets of empty space, it generates an error to the extent of “Area set could
contain multiple volumes.” At this point, the volumes will fail to import into ANSYS,
and therefore cannot be analyzed.
Even if this were not the case, however, this model is simply too complicated.
Henry Cogswell College has made available to its students an educational edition of the
ANSYS software package, which has a maximum node count of 23,000. This number is
deemed sufficient, and will almost never be exceeded by any project a student would
have a need to analyze. This is one of the almost nevers. Though we cannot be sure,
judging from our experience with a previous, comparable problem and the CosmosXpress
FEA software package, our best guess puts this problem somewhere well in upwards of
200,000 nodes.
In order to solve this problem, it must be simplified. We spent several weeks
working on the best way to approximate the structure with simpler shapes, and eventually
determined that our best option was to use areas for the mesh rather than volumes. The
simplest volumetric element possible is a tetrahedron, which consists of four sides, for
vertices, and six edges. Filling a complex shape such as this chassis with such elements is
an extremely complicated task, and easily crests the 23,000 node limit, crashing the
ANSYS program altogether. However, if we fill in the tubes to create a solid bar chassis,
and then mesh the areas that define the volume with an element thickness of one
sixteenth of an inch, it may provide a reasonable approximation.
To test this, we tried a simple case of our problem. We performed an analysis of a
one foot long, one inch square steel tube with one sixteenth inch thick walls. For one
case, we modeled the volume in SolidWorks, imported it into ANSYS, and meshed it
using volume elements. For the other, we simply generated a one by one by twelve solid
bar, imported it into ANSYS, and meshed the four areas of interest using one sixteenth

77
1
NODAL SOLUTION
JUN     8 2004
STEP=1                                                                                     21:48:55
SUB =1
TIME=1
SEQV      (AVG)
DMX =.104596
SMN =4427
SMX =219043

MN

MX

Y
X       Z

4427                    52119           99812              147504            195197
28273           75966             123658            171350            219043

1
NODAL SOLUTION
JUN     8 2004
STEP=1                                                                                     21:54:10
SUB =1
TIME=1
SEQV      (AVG)
DMX =.099386
SMN =4613
SMX =204734

MX

MN

Y
X        Z

4613                    49084           93556              138027            182498
26849           71320             115791            160263            204734

78
The results do not match exactly, but there is a very clear correlation between them.
Using area elements to approximate a volume mesh provides results that are very useful.
Some things must be kept in mind while using this approximation for our
problem. First, it is only an approximation; the results provided are not exact and are only
close to the actual load case. Also, the model that we will be using is merely an
approximation of the physical chassis that we are building. By simplifying it for analysis,
we have significantly changed the structure. The wall thickness of any given tube where
it intersects any other tube is lost, meaning that we are modeling a structure that appears
very similar to our own, but lacks any internal structure that our chassis will have. Also,
the model’s dimensions will be slightly off, as the one sixteenth inch wall thickness will
be generated at the surface of the volumes, resulting in a misplacement of 1/32 of an inch.
Even with all of these simplifications, however, the model still will not mesh in
under 23,000 nodes. We do, however, have one more option that will allow us to proceed.
We have cut the model in half along its plane of symmetry. This means it will take
roughly half as many nodes as a full version, and we can apply a symmetric boundary
condition along to cut so that it will behave as if both halves are there. However, this
that would cause the plane of symmetry to deform cannot be accurately represented.
Fortunately, our eight load cases were designed with this in mind, so none of them must
be thrown out.
The final, simplified model is pictured below:

79
Importing the Model into ANSYS
The first steps of analysis should remain the same for each load case we want to
perform. First, the solid model created in SolidWorks must be saved with an .iges file
extension, and then that file must be imported into ANSYS. This results in the following:

1
VOLUMES
JUN 25 2004
TYPE NUM                                                                    21:19:42

Y
X
Z

You can see here many of the modifications we made to the structure in order to
simplify the meshing process. The most easily visible is along the bottom bar where two
cross members of the undercarriage of the robot intersect at the same point. We have
added volume to that point because of the abnormal concentration of nodes there when it
was left as it was. As you will see in the meshed model, there are still a large number of
small elements at that location, but it was even worse before the modification was added.
Then, to set up the problem, we simply have to configure ANSYS for the analysis. We
set the filtering to structural, select a shell element with four nodes, set the area thickness
to 0.0625 units (inches in this case), set the modulus of elasticity to 29 million pounds per

80
square inch, and set Poisson’s ratio to 0.32 (these are the properties of low carbon,
structural steel). With all of these parameters set, we are ready to mesh the model.

Meshing the Model
To create the mesh, we will be meshing all areas. This is not strictly accurate, but
the cases where it is not exact are negligible. For example, the surfaces created where we
cut the model in half do not have a sixteenth inch thick wall along them, but because we
will be constraining those surfaces to create the symmetrical boundary condition, it will
not impact the results.
Issuing the mesh command causes a warning message to pop up that reads,
“Shape testing revealed that 368 of the 17548 new or modified elements violate shape
warning limits. To review test results, please see the output file or issue the CHECK
command.” This is just a warning, not an error, so we are still able to proceed with the
analysis. The meshed model can be seen below:

1
ELEMENTS
JUN 25 2004
21:44:37

Y
X
Z

81
Note: with some of the earlier iterations of this process, that number of shape
warnings we received was much higher. With our first attempts, the number of problem
elements was on the order of 700; through simplifying the model and adding volume to
assist the meshing process, we have almost halved the number of warnings generated
during meshing.

Applying the Boundary Conditions
We have eight different load cases that we wish to analyze over the course of this
project. For each of them, we will begin from this point, with a meshed model created in
exactly the same way as outlined above. We have saved our progress up until this point,
and will re-open this database file each time we wish to perform a new analysis.
Each of our load cases differs only in their boundary conditions. For each of the
eight cases, we will apply the symmetry conditions along the plane of symmetry, we will
apply loads to different nodes, and we will fix portions of the model that are appropriate
to have grounded. We will then examine the results produced in each of the eight cases,
checking for unacceptable deflection, stresses approaching half of the yield stress of steel,
or any other failures. If we discover any such failure, we will modify the chassis model,
and begin analysis of the new structure.

This is the simplest load case, and consists of the chassis loaded in static
equilibrium with the weight evenly distributed between the three axles on this side. To do
this, we will fix all degrees of freedom of the top surface, apply symmetric boundary
conditions along the plane of symmetry, and apply upward forces along where the axles
are mounted. This robot will weigh roughly 350 pounds, and it should be capable of
bearing the weight of a single passenger of any reasonable weight. To simulate the upper
bound of this loading, the total load applied to the chassis will be 700 pounds. Note that
this load is applied to only this half of the chassis; in effect, we are subjecting the chassis

82
In order to apply the force, we manually selected 150 nodes, each of which will
bear an equal portion of the force: 4.66667 pounds on each node in the positive y
direction. This results in the following:

1
ELEMENTS
JUN 29 2004
F                                                                         21:13:27

Y

Z       X

From here, applying the additional boundary conditions is simple. The top face of
the model is fully constrained, allowing none of its six degrees of freedom to change. The
middle face is the plane of symmetry. On this face, we constrain the translation in the z
direction, the rotation about the x-axis, and the rotation about the y-axis. This simulates a
condition that there is a mirror image of the model attached to this face under identical
boundary conditions. The fully constrained model is shown below:

83
1
ELEMENTS
JUN 29 2004
U                                                                        21:47:34
ROT
F

Y

Z       X

With all of the conditions set, we can issue a simple command to initiate the solution of
the load case. ANSYS takes a few moments to complete the solution for such a complex
problem.
The results of this static analysis can be viewed in the general postprocessor.
There are two major things that we are interested in: the deformed shape and the stress
plot. An exaggerated plot of the deformed shape can be seen below, with a dashed line to
indicate the initial shape:

84
1
DISPLACEMENT
JUN 29 2004
STEP=1                                                                 21:55:24
SUB =1
TIME=1
DMX =.002008

Y

Z       X

This looks very good, and tells us that the magnitude of the maximum displacement of
any node is just a hair over 0.002 inches, easily within acceptable limits. However, if we
zoom in on the back axle’s supports, we can clearly see the weak point in the design:
1
DISPLACEMENT
JUN 29 2004
STEP=1                                                                 21:58:32
SUB =1
TIME=1
DMX =.002008

85
This image is highly exaggerated; that point deflects only 0.002 inches under these
eye on this portion of the chassis, and if it shows high stresses or unacceptable deflection
under other loadings, this would be a good place to add a reinforcing member or two to
the chassis.
Another plot available to us is the von Mises stresses, shown below. The area of
concern is shown again here, to examine what kinds of stresses we can expect. High
deflection does not necessarily mean high stress, but we are keeping an eye on it just in
case:

1
NODAL SOLUTION
JUN 29 2004
STEP=1                                                                      22:04:46
SUB =1
MN
TIME=1
SEQV      (AVG)
DMX =.002008
SMX =7485

MX

0                     1663           3327          4990          6653
831.687           2495          4158          5822          7485

As you can see here, this is indeed a stress concentration, but the magnitude of the stress
is under 7.5 ksi. However, another area of interest cropped up in examining this plot. This
one is along the front axle:

86
1
NODAL SOLUTION
JUN 29 2004
STEP=1                                                                       22:08:10
SUB =1
TIME=1
SEQV      (AVG)
DMX =.002008
SMX =7485

0                     1663          3327          4990            6653
831.687          2495          4158          5822            7485

It doesn’t appear to be as bad as the back axle, but it is another area of interest. All in all,
however, the absolute highest stress concentration in the entire chassis is 7485 psi.
Structural steel has a yield stress of 36000 psi, giving us a safety factor of over 4.8. This
is acceptable; however, this is one of the easiest of our eight load cases.
We will watch these two locations for increased stresses in the following
analyses, and if our safety factor drops below 2, we will have to add reinforcements in
order to reduce the stresses.

87
Load Case #2: Focused Weight 1
For each of the focused weight load cases, we want to simulate a circumstance
where, due to dynamic loads or shifting weights, all of the weight of the previous case is
focused on a single axle. For this case, we will examine the front axle under a full 700
The solution is carried out as in the previous example. Again, we are concerned
with the deformed shape and the stresses in the chassis as a result of this load case. The
deformed shape is pictured below:

1
DISPLACEMENT
JUN 30 2004
STEP=1                                                                      20:23:19
SUB =1
TIME=1
DMX =.002171

Y
Z
X

This looks a like a significant deflection, but, again, it is exaggerated. The max deflection
in this case is only slightly higher than before, at 0.002171 inches. Furthermore, this
deflection occurs when the maximum load is entirely focused on one of the two front
wheels, or when double the safe load is taken on the front axle.

88
1
NODAL SOLUTION
JUN 30 2004
STEP=1                                                                    20:31:59
SUB =1
TIME=1
SEQV     (AVG)
DMX =.002171                              MX
SMX =12332
MN

Y
Z
X

0                 2741           5481           8222          10962
1370           4111           6851          9592           12332

Under these loads, the maximum total von Mises stress concentration that can be found in
this structure is 12332 psi. This is slightly higher than we are strictly comfortable with,
with a safety factor of only approximately 2.92, but in light of the loading under
consideration, it is acceptable. This indicates that in order to reach the yield strength of
steel, the front axle would need to be loaded with nearly six times the intended load
capacity of the entire robot.

89
Load Case #3: Focused Weight 2
This load case will simulate the exact same conditions as in the previous one,
except that the loads will be applied to the middle axle instead of the front one. The
deformed shape is pictured below:

1
DISPLACEMENT
JUN 30 2004
STEP=1                                                                20:56:14
SUB =1
TIME=1
DMX =.001538

Y
Z
X

Once again, note the max deflection of only 0.001538 inches, even less than in the
previous two cases.
The stresses are pictured below:

90
1
NODAL SOLUTION
JUN 30 2004
STEP=1                                                                        21:01:04
SUB =1
TIME=1
SEQV     (AVG)                                              MN
DMX =.001538                              MX
SMX =19752

Y
Z
X

0              4389           8779                 13168            17558
2195          6584            10973                 15363           19752

This shows higher stresses than we expected. This case showed less deflection than either
of the others, but it is the highest stress yet at 19.752 ksi, giving a safety factor of only
1.82. This stress concentration, however, occurs at node 2815, which is not at the
mounting point of the axle. It can be found at the top of the chassis, shown below:

91
1
NODAL SOLUTION
JUN 30 2004
STEP=1                                                                21:07:31
SUB =1
TIME=1
SEQV     (AVG)
DMX =.001538
SMX =19752

MX

0              4389          8779           13168           17558
2195          6584          10973           15363           19752

92
This is one of the areas that we adjusted in order to reduce the number of shape warnings
we got when solving load cases. It is clear from the pictures that the corner in question
buckled into the structure that was supposed to be supporting it. The shell elements used
to mesh this model are not interacting properly at this point, causing irregular geometry
and a high stress concentration.
By eliminating the top portion of the model from the selection, and re-listing the
stresses, we find that the maximum stress in the lower portion of the chassis is 8782.5 psi,
which suggests a much more acceptable safety factor of 4.1.
Even though we are reasonably sure that this stress concentration is not indicative
of a design flaw but rather an artifact of the simplification measures we had to take in
order to solve this problem, we will keep a close eye on the area in question. we see no
reason why this particular portion of the chassis should accumulate stresses of this
magnitude, but if they continue to do so in the following analysis, we will be forced to
either modify the model to more accurately represent the robot chassis, or reinforce the
design to eliminate the stress concentration.

Load Case #4: Focused Weight 3
This load case will examine the case where all of the weight of the chassis and
passenger is focused on the back axle. Because this was the biggest problem area in the
first load case, we expect this to be one of the most important analyses that we perform
using ANSYS. It is carried out, however, in exactly the same way as the previous two.
Pictured below is the deformed shape:

93
1
DISPLACEMENT
JUN 30 2004
STEP=1                                                                     21:31:06
SUB =1
TIME=1
DMX =.005262

Y
X       Z

Again, this shows an exaggerated view of the chassis deformation that looks very similar
to the aft portion of the chassis for the first load case. For this, however, the deflection is
on the order of two and a half times the deflection in the first case. That being said,
however, the deflection is still only 0.005262 inches, which is well within acceptable
limits. We would like to keep all possible deflections under one sixteenth of an inch, and
this is still less than one tenth of that.
In order to know if this load case produces unacceptable results, we must examine
the stresses, pictured below:

94
1
NODAL SOLUTION
JUN 30 2004
STEP=1                                                                       21:38:48
SUB =1
TIME=1
SEQV     (AVG)
DMX =.005262
SMX =19386

MN

Y
X
Z
MX

0              4308            8616             12924            17232
2154           6462             10770           15078            19386

Though it is difficult to get a good angle to see what is going on with these structures, we
do see here that 19386 is the maximum stress. This is a very high stress, giving us a
safety factor of only 1.857. Granted, this is an extreme load case, but with a possible
static safety factor of less than two, we will need to reinforce this portion of the chassis.

95
The fifth load case represents a situation where the chassis is loaded in a
completely different plane. Instead of being loaded in the normal, vertical direction, we
want to see how well the chassis will be able to withstand horizontal loads. This kind of
situation could be seen if the robot runs into an obstruction or is climbing a particularly
steep incline.
The procedure for this analysis is exactly the same as in previous, but with
different boundary conditions applied. Again, we have applied a force of 700 pounds to
the front axle. This is a very extreme case. This would only occur under dynamic shock
balanced on a single front wheel. The deformed shape and stress plot are pictured below:

1
DISPLACEMENT
AUG     3 2004
STEP=1                                                                     14:32:36
SUB =1
TIME=1
DMX =.011287

Y
X
Z

96
1
NODAL SOLUTION
AUG     3 2004
STEP=1                                                                          14:36:45
SUB =1
TIME=1
SEQV     (AVG)
DMX =.011287
SMX =69128

MX

0                 15362           30724           46085           61447
7681           23043           38404           53766             69128

This value of over 69 ksi is very troubling. However, upon closer inspection at the site of
this maximum, we see this:

1
NODAL SOLUTION
AUG     3 2004
STEP=1                                                                          14:35:55
SUB =1
TIME=1
SEQV     (AVG)
DMX =.011287
SMX =69128

MX

0                 15362           30724           46085           61447
7681           23043           38404           53766             69128

97
This is an area that we must have missed when we modified our SolidWorks model for
use in ANSYS. This is clearly a source of geometric problems. Because we have used
surface elements, these incredibly narrow surfaces have been modeled as incredibly thin
pieces of steel. In reality, the bars that make up this geometry will continue through the
surface and out to the side of the robot chassis, making a much stronger joint.
In order to gain a more accurate maximum stress estimate, excluding this
singularity for the analysis, we have adjusted the solid model constraints. With the front
of the chassis fully constrained and a 700 pound load applied to the back, we get the
following stress plot:

1
NODAL SOLUTION
AUG     3 2004
STEP=1                                                                            14:55:45
SUB =1
MX
TIME=1
SEQV     (AVG)
DMX =.056048
SMX =21421

Y
X
Z

MN

0                 4760          9520                14281           19041
2380          7140             11900             16661             21421

By eliminating that singularity from the analysis, the resultant stresses have been reduced
by a factor of more than three. They are still rather high, though, at 21 ksi, and our safety
factor is down to just over 1.7. Note, however, the location of the maximum stress. It is at
exactly the same location as the troublesome stress concentration from load case #3. We
still see stresses on the order of 15 ksi in the areas of interest, so this is an area to watch,
but the 21 ksi will not manifest itself in reality.

98
For our sixth load case, we want to examine a similar case to the previous one, but
with a z-direction load. We are going to be looking at the effects on the internal structure
here, so the loading will be applied to the side surface. The deformed shape and stress
distributions are included below:

1
DISPLACEMENT
AUG     3 2004
STEP=1                                                                       15:15:28
SUB =1
TIME=1
DMX =.003241

Y
Z
X

99
1
NODAL SOLUTION
AUG     3 2004
STEP=1                                                                              15:16:32
SUB =1
TIME=1
SEQV     (AVG)
DMX =.003241
SMX =11724

MN

Y
Z
X

MX

0                 2605               5211          7816               10422
1303              3908           6513          9119                  11724

These results are well within acceptable limits. A deflection of just over 0.003 inches and
a maximum stress of 11.7 ksi should be no problem for this design. For this loading, we
have a stress safety factor of over 3.

Load Case #7: Positive Bending Moment
This load case is designed to analyze how the general structure of the chassis
withstands a bending moment over its entire length. This type of loading will occur when
on uneven terrain or when the axles each bear a different amount of weight. In this case,
we will disregard any stress concentrations at the location of the application of the
loading, as that is not the concern here. Just as in the front load case, we are interested in
the reaction within the structure, not at the point of application.
Once again, the setup and analysis of this case is done exactly as in previous
cases. The deformed shape and stress plots are included below:

100
1
DISPLACEMENT
AUG     3 2004
STEP=1                                                                                15:51:05
SUB =1
TIME=1
DMX =.006405

Y
X
Z

1
NODAL SOLUTION
AUG     3 2004
STEP=1                                                                                15:54:34
SUB =1
TIME=1
SEQV     (AVG)
DMX =.006405
SMX =32898

YZ
X

MN

MX

0                 7311           14621               21932            29242
3655          10966               18277           25587                32898

101
Here we see a stress that very closely approaches the yield stress of steel. This max stress
occurs at the lower right of the plot above. We were surprised to see such a high stress in
that location, but, upon closer inspection (below), we again see that this is due to the
geometry of the problem.
1
NODAL SOLUTION
AUG     3 2004
STEP=1                                                                         15:53:40
SUB =1
TIME=1
SEQV     (AVG)
DMX =.006405
SMX =32898

MX

0                 7311           14621           21932           29242
3655          10966           18277           25587             32898

Once again we see the max stress at a sharp angle where the area elements become very
thin. These kinds of stress concentrations are largely due to the simplifications we were
forced to make in formulating this problem. Further, even were something like this to
manifest itself in the physical design, steel is a ductile material. Corners like this
represent theoretical infinite stress concentrations, but in practice, these points will

Load Case #8: Negative Bending Moment
For this load case, we will examine the response to a negative bending moment
using the same process we used in case 7. The deformed shape and stress plot are
included below:

102
1
DISPLACEMENT
AUG     3 2004
STEP=1                                                                          16:33:00
SUB =1
TIME=1
DMX =.003809

Y
X
Z

1
NODAL SOLUTION
AUG     3 2004
STEP=1                                                                          16:33:19
SUB =1
TIME=1
SEQV     (AVG)
DMX =.003809
SMX =11131

MN

Y
X
Z
MX

0                      2474          4947           7421          9894
1237               3710          6184           8658             11131

103
We are extremely happy with these results. No stress concentrations of significant
magnitude affected the results adversely, the deflection is well within acceptable limits at
less than 0.004 inches, and the stresses give us a safety factor of almost 3.25.
Furthermore, this is one of the load cases we expect to see the most often during normal
use. The center axle is positioned slightly lower than the other two to reduce the
“scrubbing” effect of turning with tank treads. This means that the vehicle will see this
negative bending moment during most driving conditions. These results are very
reassuring.

Summary of Chassis Analysis Results:
Over the course of analyzing the eight load cases discussed above, we have
learned a great deal about the weak points of this design. These are restated here for
discussion and mitigation:

This load case showed deflections and stresses well within acceptable limits. It
did indicate some weak points that were seen in greater detail in following load cases;
however, this load case did not expose any problems that required adjusting the design.

Load Case #2: Focused Weight 1
This load case showed deflections and stresses that were also within acceptable
limits. This was one of the locations we were watching after the results from case #1
were obtained, but this analysis shows that no problems should arise from this axle.

Load Case #3: Focused Weight 2
This load case showed acceptable deflections, but unacceptable stress levels.
Upon closer inspection, we found that the stress concentration was due to the
simplifications that we applied to the solid model. This stress concentration will not even
be present in the physical case. We kept this site under observation, but it showed no
further problems.

104
Load Case #4: Focused Weight 3
This load case showed unacceptable levels of stress. The mounting points for the
aft axle require reinforcement.

This load case showed high levels of stress. The supports for the far front, raised
axle will be re-evaluated. The stresses measured peaked at the location of the stress
concentration from load case #3, and can be discarded. However, the remaining stresses
are high enough to warrant reexamination.

This load case showed acceptable deflections and stress levels. No modifications
are necessary.

Load Case #7: Positive Bending Moment
This load case showed another point of unacceptable stress concentration. This
spot will be evaluated to determine if the stress concentration was due to the geometry
created during the simplification process, or if the structure needs to be modified.

Load Case #8: Negative Bending Moment
This load case showed acceptable deflections and stress levels. No modifications
are necessary.

Chassis Modifications:
After the results of the analysis described above, we have examined each of the
four locations of interest. Two of the sites contain stress concentrations that are of no
concern. They will not provide a significant problem once the physical chassis is
constructed; they are artifacts of theoretical stress concentrations due either to the original
geometry or the modifications that we have made to it for analysis. The third of the four
spots we have modified to reduce stresses, and the final spot we have examined and
decided to leave unmodified for reasons to be outlined below.

105
The two positions that will not create a problem are pictured below:

The picture on the left is the site of most of our troublesome stress concentrations.
You can see the small triangular chamfer that joins the two perpendicular members. This
chamfer was placed there to simplify the mesh that ANSYS had to create for this
problem, and will not exist when the chassis is constructed.
The picture on the right is the stress concentration that resulted from load case #7.
If you look closely at the image, you can see that one of the members is at a slightly
different angle than the other two, creating a singularity where the three intersect. This is
what caused the stress to spike during that load case. When the chassis is constructed, this
site will the ground flat, eliminating this singularity.
Furthermore, after examination of the forward portion of the chassis (pictured
below), I have determined that this area does not require modification.

106
There is an additional member at this location, which was not taken into account
previously. The axle that runs through the chassis here will support a significant amount
of load. Because, even without the axle present, this structure had a safety factor of more
than 2, there should be no problems in this area.
The final location to watch was the lower, aft portion of the chassis. This portion
did not have a geometric anomaly or stress concentration of direct concern. The stresses
were simply unacceptable because the structure was improperly supported. We have

Load Case #4: Focused Weight 3 (Revisited)
In order to evaluate the effectiveness of the added member, we will perform load
case #4 again on the revised model. This time, we must start over from the beginning of
the process, importing the new .iges file into ANSYS and meshing again from scratch.
Furthermore, we are going to need to manually re-select each of the nodes used
previously, as their numbers may have been altered in the meshing process.
The modified, imported, meshed, and constrained model had a mesh density that
was much lower than before. With the upgrade from ANSYS 7.1 to ANSYS 8.1, the
algorithms used for optimizing that matrices must have been tweaked. As a result, the

107
same model that was successfully meshed and was used for the previous analysis throws
a “divide by zero” error under the new version of the software. After some tweaking of
the mesh parameters (expanding the element size), we were finally able to achieve a
successful mesh and analysis.
Because we are only interested in the resulting stress for one simple analysis, this
mesh density should not pose a problem. After solving the system, we obtain the
following deformed shape and stress plots:

1
DISPLACEMENT
AUG 3 2004
STEP=1
20:13:08
SUB =1
TIME=1
DMX =.004013

Y
X       Z

108
1
NODAL SOLUTION
AUG 3 2004
STEP=1
20:13:55
SUB =1
TIME=1
SEQV     (AVG)
DMX =.004013
SMX =13139
MN

Y
X       Z

MX

0                 2920          5840          8759                 11679
1460          4380          7300          10219                  13139

This analysis results in a deflection of just a hair over 0.004 inches and a maximum stress
of just over 12 ksi, down from over 0.005 inches and 19 ksi before the addition of the
additional member. This ups our safety factor from 1.86 to 2.74. This brings the stress
levels in every part of the chassis under all eight load cases within acceptable limits.

Conclusions, Chassis Structural Analysis
The design under consideration here was a very sound one. After rigorous testing,
only four questionable points could be found. Three of these have been examined and
deemed acceptable. The last has been easily rectified. With the addition of a single, small
member at the bottom aft portion of the chassis, the design has passed all of the tests.
Even under extreme cases of static loading, our chassis always maintains a safety factor
of 2 or better, except in very special cases, which we are confident will not manifest
themselves in reality.
This chassis design is fully capable of everything we have tested. It can easily
support its full weight of 350 pounds plus an additional 350 pounds of payload, even
when that weight is focused on a single wheel. It can also support these kinds of loads

109
when oriented in other directions, as in the case of resting on its side or colliding with
another object. Furthermore, the structure is capable of supporting bending moments
applied to its entire length without unacceptable deflection or stress levels.
With the completion of this analysis and with the addition of the one modification
we have outlined above, we are confident that this chassis will meet our needs. Because
the structure had already been through numerous design iterations before the ANSYS
analysis, very few changes had to be made. This validation process has been the final
approval test for this structure. The chassis design is complete and ready to be built, as
pictured below:

110
Finite Element Analysis, Axle

Initial Steps: Designing the Axles
In addition to the chassis analysis and design, we would also like to use ANSYS
to analyze the axles for this robot. The wheels we want to use only have up to a ¾ inch
inside diameter, and a quick hand calculation shows that using a steel rod of this size will
result in unacceptable deflection and stresses.
These axles will be fixed, with the wheels mounted on bearings. This means that
the axles will be subjected to bending moments only, and they need not be axisymmetric
about any axis. After careful examination of the space available and the types of loads we
expect to see, we have come up with this design:

The primary goal of this design is to maximize the ability of this structure to support
bending moments in the vertical direction. It also had to have a thickness of less than one
inch to fit in the confined chassis. The short pegs perpendicular to the axle itself will be
used to constrain movement in the axial direction.

111
In order to mesh this piece for analysis, we went through much the same process
that we did with the chassis. First, we simplified the model by cutting it in half along its
plane of symmetry. We then exported it as an .iges file, and imported it into ANSYS. We
set the element type to a solid tetrahedron volume element. This means that this analysis
shouldn’t be subject to the inaccuracies present in the chassis due to surface meshes. The
meshed model is shown below:

1
ELEMENTS
JUL 27 2004
17:43:17

Y

Z       X

We are now ready to analyze the axles.

Applying the Boundary Conditions
Applying the boundary conditions to this problem was fairly difficult. This axle
will be subjected to a bending moment caused by a distributed load at the end and an
equal but opposite distributed load just in front of the peg. In the physical situation this is
designed to model, no parts of the axles are fully constrained. For this case, we have
opted to fix the cut surface at the plane of symmetry. Because no other points have their
displacements constrained, this should accurately model the real situation.

112
With that decided, we are ready to begin testing load cases. For this analysis, we
have only two such cases. The first is a simple bending moment in the y-z plane, with no
x components to any of the forces. This is the kind of loading we would expect to see
under normal use. The second is a less ideal case, where the force applied to the wheel
has an x component. This will represent a case where the wheel hits a bump at speed or
the robot is climbing a steep incline.

For this case, the bushings are not required to support any load. The wheel portion
of the axle is subjected to a loading in the positive y direction while the suspension is
subjected to a load in the negative y direction of equal magnitude.
case. The forces involved in this loading will have a magnitude of 350 pounds. This
represents the case where the robot is at full capacity of 700 pounds, all focused on a
single pair of wheels. Because this is only half of an axle, it will support half of that load.
The constrained and loaded model can be seen below:

1
ELEMENTS
JUL 27 2004
U
17:59:54
F

Y

Z       X

113
After solving the problem exactly as done in previous examples, we get the following
plots for deformed shave and stress distribution:
1
DISPLACEMENT
JUL 27 2004
STEP=1                                                                       18:04:51
SUB =1
TIME=1
DMX =.02081

Y

Z        X

1
NODAL SOLUTION
JUL 27 2004
STEP=1                                                                       18:09:43
SUB =1
TIME=1
SEQV     (AVG)
DMX =.02081
SMN =1.203
SMX =16672

Y

Z        X

MN

MX

1.203              3706           7410          11115           14819
1853           5558           9263           12967           16672

114
These are both very positive results. The deflection plot shows a maximum deflection of
only just over 0.02 inches. For the axles, an unacceptable level of deflection is much less
restrictive than for the chassis. A deflection of a quarter of an inch or more would not
significantly impact the design. The important part of this analysis is the stress analysis
As we can see from the plot above, the maximum stress is 16.7 ksi, and it occurs
exactly where we would expect. The maximum stress appears at the location where the
structure reduces to ¾ of an inch to thread into the wheel. Even with this stress
concentration, however, we see a safety factor of over 2.15, and this is under an extreme
One other observation of note can be seen from the above plot. Note that, unlike
many of the chassis loadings, most of this structure is not blue. The top and bottom of the
axles for most of their length all support a significant amount of load. This means that
there isn’t a lot of wasted material in this design. The exception to this is the large solid
portion just next to the maximum stress concentration. This portion is a clamp structure
that cannot be significantly reduced in size due to manufacturing limitations.
Overall, this load case shows that this axle design is very well suited for our
application.

We would like to do another load case to capture the result of a more complex
loading. In this case, the vertical force will be supported in the same way as the previous.
However, there will be a horizontal force as well, which will be supported at a different
location where the chassis structure will constrain the axle.
We will again load it under 350 pounds, but at this time, we will examine a case
where the force is applied at a 30-degree angle. This means that we will have a force in
the x direction with a magnitude of 175 pounds, and a force in the y direction with a
magnitude of 303.11 pounds.
We can now go through the exact same procedure to solve the system, and plot
the deformed shape as well as the stress distribution. Again, we are not overly concerned
with the deformed shape. So long as the deflections are not extremely high (on the order
of a quarter of an inch or more), they should not cause a problem. The main thing that we

115
am concerned about is stresses approaching the yield stress of steel. The plots are
included below:
1
DISPLACEMENT
JUL 27 2004
STEP=1                                                                     19:14:06
SUB =1
TIME=1
DMX =.047866                                                                        Y

Z       X

1
NODAL SOLUTION
JUL 27 2004
STEP=1                                                                     19:15:30
SUB =1                                                                       Y
TIME=1
SEQV     (AVG)                                                              Z       X
DMX =.047866
SMN =.483335
SMX =15792

MX

MN

.483335          3510          7019          10528           14037
1755          5264          8773           12283               15792

116
1
NODAL SOLUTION
JUL 27 2004
STEP=1                                                                     19:17:54
SUB =1
TIME=1
SEQV Y   (AVG)
DMX =.047866
X
SMN =.483335
Z
SMX =15792

MX

MN

.483335           3510          7019          10528           14037
1755          5264          8773           12283           15792

This tells us something very interesting. Our maximum stress concentration does not
increase with this, more severe loading. At first, this seems counter-intuitive, but it does
make sense. Note the position of the maximum stress concentration (denoted MX in the
image). This concentration is located along a circle, where the cylinder enters the clamp
device. Because this is a circle, we can expect the angle of the applied force to have little
impact on the magnitude of the maximum force. Indeed, that is the case we see here.
However, the maximum stress is not the only thing that we are concerned about.
Consider the previous case, with the ideal loading. The ¾ inch rods that make up the
length of the axle are subjected to a stress corresponding to somewhere around 6 ksi on
the key below the image. In this second case, we can see that the bands of brightest color
(indicating highest stresses) are shifted around the surface of the axle, and read as high as
9 or 10 ksi.
So, as a result of a non-ideal loading, we see two things: an increase in stress
along the length of the axle, and an increase in deflection (up from 0.02 inches to almost
0.05). The maximum stress in this part, however, is not greatly affected (changing from

117
16.7 ksi to 15.8 ksi). This non-ideal loading can be expected to result from several
different physical use cases, including accelerating and breaking, climbing hills, hitting
bumps, or even the effects of torque transmission through the tank-style tread that will be
wrapped around the wheels.

Conclusions
From these two load cases, we can conclude that this axle does not require
redesign. The axles, as pictured at the beginning of this analysis, are each capable of
statically supporting the entire weight of the fully loaded vehicle with a safety factor of
over two. This is within the acceptable limits.
Though these members can be expected to undergo shock loading, they are
suspended members, which will greatly reduce the impact of such a loading. Also, we
have considered an extreme case, giving us some additional elbow room. Through we can
entire weight of a fully loaded robot is borne by a single axle.
Furthermore, even given such an extreme and unlikely case of abuse, catastrophic
failure should not occur. The stress concentration that we have observed is localized at
what is technically an infinite stress concentration. Because steel is a ductile material,
upon reaching the yield strength at that point, the stress concentration will be reduced.
Because of these factors as well as the physical situation in which this axle will be
used, we can conclusively say that this design is fully capable of performing the required
task. An axle of this from will fit in the required space, constrain the proper degrees of
freedom while leaving the others free to vary, provide appropriate surfaces for mounting
wheels and bushings as required, and support the expected loads all without reaching half
of the yield stress of steel.

118

```
DOCUMENT INFO
Shared By:
Categories:
Tags:
Stats:
 views: 21 posted: 7/30/2012 language: English pages: 43
How are you planning on using Docstoc?