Structural dynamic analysis of a Formula SAE vehicle

UNITN – Alessandro Luchetti, Marco Basilici – Modeling and design with finite elements
University of Trento – Departement of Industrial Engineering
Structural dynamic analysis of a Formula SAE vehicle
Mechatronics Engeneering Master Degree – Modeling and design with finite elements
Prof: Benedetti Matteo
Alessandro Luchetti (M. 180061)
alessandro.luchetti@studenti.unitn.it
Marco Basilici (M. 182716)
marco.basilici@studenti.unitn.it
Final Report
2017-2018
ABSTRACT
The goal of this project is to determine the dynamic structural behavior of a racing car for a Formula SAE
competition.
Thanks to this study it was possible to verify, under a real load history, the goodness of the structure in
terms of stiffness and so the handling of the vehicle.

UNITN – Alessandro Luchetti, Marco Basilici – Modeling and design with finite elements
Index
1 Introduction............................................................................................................................................... 1
2 Finite Element Model ................................................................................................................................ 2
2.1 Assumptions and simplifications adopted in the analysis.......................................................... 3
2.2 Chassis ........................................................................................................................................ 5
2.3 Suspensions................................................................................................................................ 6
2.4 Front steering axle.................................................................................................................... 10
2.5 Heaviest components............................................................................................................... 11
2.6 Meshing.................................................................................................................................... 13
2.7 Tires.......................................................................................................................................... 13
2.7.1 Assumptions and simplifications adopted in the analysis........................................................ 13
2.7.2 Tire model ................................................................................................................................ 14
2.8 Assembly .................................................................................................................................. 16
2.8.1 Kinematics ................................................................................................................................ 16
2.8.2 Tire connection......................................................................................................................... 17
3 Modal analysis......................................................................................................................................... 18
3.1 Problem approach.................................................................................................................... 19
3.2 Results ...................................................................................................................................... 19
3.2.1 Mode shape and natural frequencies of simple structure....................................................... 19
3.2.2 Convergence analysis ............................................................................................................... 20
3.2.3 Mode shape and natural frequencies of complex structure.................................................... 21
3.2.4 Mode participation factors....................................................................................................... 23
3.2.5 Modal stresses.......................................................................................................................... 23
4 Transient dynamic analysis...................................................................................................................... 24
4.2 Equivalent tire system.............................................................................................................. 24
4.2.1 Contact elements definition..................................................................................................... 25
4.2.2 Weight car distribution ............................................................................................................ 26
4.2.3 Transient tire analysis............................................................................................................... 27
4.2.4 Results ...................................................................................................................................... 29
4.2.5 Tire conclusions........................................................................................................................ 30
4.3 Boundary conditions ................................................................................................................ 32
4.4 Prestressed Static Nonlinear analysis....................................................................................... 32

UNITN - Alessandro Luchetti, Marco Basilici – Modeling and design with finite elements
4.5 Solution .................................................................................................................................... 32
4.6 Results ...................................................................................................................................... 34
4.6.1 Loads on tire............................................................................................................................. 34
4.6.2 Stress analysis........................................................................................................................... 35
4.6.3 Chassis torsion.......................................................................................................................... 37
4.6.4 Camber deformation................................................................................................................ 37
4.6.5 Steering deformation ............................................................................................................... 38
5 Validation Model ..................................................................................................................................... 39
5.2 Vehicle parameters .................................................................................................................. 40
5.3 Chassis torsional stiffness......................................................................................................... 40
5.4 Antiroll stiffness (ARS).............................................................................................................. 42
5.5 Static nonlinear analysis in Ansys............................................................................................. 43
5.6 Matlab analytical model calculation ........................................................................................ 44
5.7 Results ...................................................................................................................................... 46
6 Conclusions and future developments.................................................................................................... 48
6 References............................................................................................................................................... 49
7 APPENDIX................................................................................................................................................. 50
7.1 ANSYS code commands lists..................................................................................................... 50
7.1.1 Macro ....................................................................................................................................... 50
7.1.2 Accelerations data.................................................................................................................... 55
7.1.3 Basic model .............................................................................................................................. 56
7.1.4 Wheel model and transient analysis........................................................................................ 68
7.1.5 Modal analysis.......................................................................................................................... 72
7.1.6 Convergence analysis ............................................................................................................... 75
7.1.7 Static stiffness chassis massless ............................................................................................... 78
7.1.8 Transient analysis..................................................................................................................... 81
7.1.9 Validation model ...................................................................................................................... 88
7.2 MATLAB code commands lists ................................................................................................. 91
7.2.1 Load transfer distribution study as a function of the antiroll stiffness distribution................ 91
7.2.2 Load Transfer distribution study as a function of the antiroll stiffness distribution considering
different chassis stiffness......................................................................................................... 92

1
1 Introduction
The vehicle analyzed and tested in this report is the one studied and designed by UniTrento Eagle Racing
Team for the Formula SAE project.
The Formula SAE is a worldwide competition for teams of university students organized by the Society of
Automotive Engineers (SAE). It includes the design and the manufacturing of a racing car, evaluated during
series of tests based on its design quality and engineering efficiency.
It was analyzed with appropriate software, Ansys and Matlab, the strengths and weaknesses of the car
structure. Trying to predict the behaviour of the car, as close as possible to the reality, during the FSAE
dynamic tests.
Scheme of the work:
The work can be divided into four sections:
• the first, Finite Element Model, was developed thanks Ansys Mechanical APDL software to create
the model to analyze. Beams, masses, and springs were used to provide good insight into the
problem at minimal computational cost;
• the second, Modal analysis, found the modal shapes and natural frequencies of the structure. The
convergence analysis was done and it was useful also in the next sections;
• the third, Transient analysis, studied the structural dynamic behavior of the car over time;
• the fourth, Validation Model, tried to find a match between the Ansys model and the analytical one
implemented with a Matlab code.
Finite
Element
Model
•Chassis
•Suspensions
•Steering
•Heaviest components
•Meshing
•Tires
•Assembly
Modal
analysis
•Modal shapes
•Natural frequencies
•Mode partecipation factor
•Convergence analysis
Transient
analysis
•Equivalent tire model
•Loads on tire
•Stress analysis
•Chassis torsion analysis
•Camber deformation
•Steering deformation
Validation
Model

2
2 Finite Element Model
Starting with a simple structure was later improved in such a way it could approach as much as possible the
real physical structure. Creating a model as close as possible to reality is the basis to obtain valid and
extensible data to the real case.
Figure 1 - CAD model
Two models were developed for the different types of analysis: modal and transient analysis.
Each model can be decomposed into these subgroups:
• the chassis;
• the suspension groups;
• the steering axles;
• the heaviest components;
• the wheel groups.
The only difference between the two is given by the tire model. An equivalent one was used for the
transient analysis to simulate the contact given by the ground.
Figure 2 - ANSYS model for modal analysis Figure 3 - ANSYS model assumption for transient analysis
In the next sections, each subgroup will be analyze focusing on their realization and how they are
connected to each other.

3
2.1 Assumptions and simplifications adopted in the analysis
• Element type: BEAM189
The element is a quadratic three-node beam element in 3-D, is based on Timoshenko beam theory
which includes shear-deformation effects.
Figure 4 - BEAM189 Geometry
• Element type: MPC184
It comprises a general class of multipoint constraint elements that apply kinematic constraints
between nodes.
The elements are loosely classified here as “constraint elements” (rigid link, rigid beam, etc.)
Figure 5 - MPC184 Rigid Link/Beam geometry
and “joint elements” (revolute, universal, etc.).
Figure 6 – Spherical Joint Geometry Figure 7 - Revolute Joint Geometry

4
• Element type: COMBIN14
It is a 3-D longitudinal spring-damper without mass. No bending or torsion is considered.
Figure 8 - COMBIN14 Geometry
• Element type: MASS21
It is a point element having up to six degrees of freedom. A different mass and rotary inertia may
be assigned to each coordinate direction.
Figure 9 - MASS21 Geometry
The units of measurement used in the analysis are:
Forces [N]
Linear dimensions [mm]
Masses [Mg]
Young modulus [MPa]
Density [Mg/mm3
]
Frequencies [Hz]
Table 1 - Unit of measure

5
2.2 Chassis
The chassis geometry was imported as an IGES files from the Inventor software cad to the Ansys
Mechanical APDL software.
Figure 10 - Chassis model imported in ANSYS software as an IGES files from Inventor CAD version
The material used for all the chassis tubes is the stainless 304L.
Young’s modulus E = 200 000 [MPa]
Poisson’s ratio v = 0.3
Yield Strength σy = 305 [MPa]
Density δ = 7.85e-9 [Mg/mm3
]
Table 2 - Stainless 304 properties
The tubes that composed the chassis have different sections but all of them are circular:
Main hoop / Front hoop / Shoulder Harness Mounting D1 = 30 [mm], t1 = 2 [mm]
Side impact Structure SIS / main hoop bracing/ front hoop
bracing / main hoop bracing support/ tractive system
protection -Tail
D2 = 28 [mm], t2 = 1.5 [mm]
Front Bulkhead Support / upper tie-beam / rear interlocks /
harness bracing
D3 = 28 [mm], t3 = 1.2 [mm]
Front Bulkhead D4 = 34 [mm], t4 = 1.2 [mm]
Free rule tubes D5 = 20 [mm], t5 = 1.5 [mm]
Table 3 - Chassis sections parameters
Figure 11 - Chassis

6
2.3 Suspensions
The suspensions geometrical parameters were imported from an external file. They were used to build the
suspensions geometry through the Ansys APDL software.
Two different models of suspensions were adopted: one pull-rod type for the front suspensions and the
other pushrod for the rear ones. The main differences between the two types of suspensions are the
connection position points of the suspension elements with the chassis and with the up-right; the other
difference is given by a different inclination of the rod. This inclination affects the forces applied to the rod,
either traction or compression. The second one should be taken under control because when stressed, it
could have elastic instability problems.
Figure 12 - Suspensions geometries configuration
Figure 13 - Rear left line suspensions group (push-rod) Figure 14 - Front left line suspensions group (pull-rod)
The material used for all the suspensions tubes is in composite. Carbon fiber is known for its anisotropic
characteristics therefore it was necessary to calculate the young modulus in all the directions. It was
possible thanks to laboratory test results.
Figure 15 - Traction test Figure 16 - Compression test Figure 17 - Bending Test
Pull-rod Push-rod

7
-1
0
1
2
3
4
5
6
7
8
9
10
0 0,2 0,4 0,6 0,8 1 1,2 1,4 1,6 1,8
Force[KN]
Displacement [mm]
Traction test
-1
1
3
5
7
9
0 0,2 0,4 0,6 0,8 1 1,2 1,4 1,6 1,8
Force[KN]
Displacement [mm]
Compression Test
-0,1
0,1
0,3
0,5
0,7
0,9
1,1
1,3
1,5
1,7
0 1 2 3 4 5 6 7 8 9 10
Force[KN]
Displacement [mm]
Bending test

8
Thanks to the above test plots it was calculated the stresses “σ” and deformations “ε” necessary to find the
young modulus.
From the plot of the bending test it was found the young modulus in the radial “x-y” directions. Instead
from the traction test plot it was found the young modulus in the axial “z” direction.
The properties of the carbon/epoxy material are:
Young’s modulus x direction Ex = 41118.55 [𝑴𝑷𝒂]
Young’s modulus y direction Ey = 41510.629 [𝑀𝑃𝑎]
Young’s modulus z direction Ez = 6687.7 [𝑀𝑃𝑎]
Poisson’s ratio v = 0.3 []
Density δ = 1.55e-9 [Mg/mm^3]
Table 4 – carbon/epoxy properties
The young modulus in z direction it isn’t so high due to the bonding at the test ends which makes the
structure less stiff.
Figure 18 - Bonding joints
Also, the young modulus in the compression test is small due to the resin properties that during the
compression test have the best on carbon fiber.
Figure 19 - Front suspension group Figure 20 - Rear suspension group

9
The connections between the suspensions and the chassis were done with infinitely rigid beam elements.
They simulate the real connections made with the 3D printed joints. The same elements were used for the
rocker and for the connections between the suspensions points and the uprights. These elements permit to
maintain the points fixed each other.
The suspension groups configurations and the different elements used are schematized in these figures:
Figure 21 - Rear left suspension group CAD model Figure 22 - Rear left suspension group Ansys model
Figure 23 - Front left suspension group CAD model Figure 24 - Front left suspension group Ansys model
Line color Elements
BEAM189
MPC184 – Rigid beam
COMBIN14
Table 5- Legend of elements colors
Stiffness [N/mm] Damping [Ns/mm]
Front shock absorbers 20 1.5
Rear shock absorbers 26 1.5
Table 6 - COMBIN14 elements properties

10
The circular section is the same for all the tubes used for the suspensions with the same dimensions:
Suspension arms Ro = 9 [mm], t = 1.5 [mm]
Table 7 - Suspension section parameters
Figure 25 - Rear left suspension group ANSYS section Figure 26 - Front left suspension group ANSYS section
2.4 Front steering axle
To simulate the loads from the steering connections to the chassis.
The section of the steering central part is square, as it can be seen from figure 26, with the following
dimensions:
Steering axle dx = 30 mm, dy = 30 mm
Table 8 - Steering axles section parameters
The connections with the chassis were done with infinitely rigid elements.
The material used for the steering axles is the same used for the chassis: stainless 304L.

11
2.5 Heaviest components
The weights of the heaviest components were added to the model to make it closer to reality. The bigger
weights are mainly located on the back of the car.
They are composed by:
Figure 27 - CAD model of the main heavy car components
Figure 28 – Battery pack
Figure 29 - Electric motor (Emrax)
Figure 30 - Inverter
MASSX = 71.135*10^(-3) [Mg]
MASSY = 71.135*10^(-3) [Mg]
MASSZ = 71.135*10^(-3) [Mg]
Ixx = 4415609.399*10^(-3) [Mg mm^2]
Iyy = 4543320.659*10^(-3) [Mg mm^2]
Izz = 597338.389*10^(-3) [Mg mm^2]
MASSX = 9.4*10^(-3) [Mg]
MASSY = 9.4*10^(-3) [Mg]
MASSZ = 9.4*10^(-3) [Mg]
Ixx = 43761.612*10^(-3) [Mg mm^2]
Iyy = 30102.130*10^(-3) [Mg mm^2]
Izz = 30079.592*10^(-3) [Mg mm^2]
MASSX = 8.929*10^(-3) [Mg]
MASSY = 8.929*10^(-3) [Mg]
MASSZ = 8.929*10^(-3) [Mg]
Ixx = 49968.797*10^(-3) [Mg mm^2]
Iyy = 88303.976*10^(-3) [Mg mm^2]
Izz = 117058.036*10^(-3) [Mg mm^2]
Battery pack
Inverters Emrax

12
All these components were represented in Ansys thanks the element MASS21 which is defined by a single
node where the mass components and the rotary inertias are concentrated.
The connections between these points and the chassis were done with infinitely rigid beam elements. The
choice of the points where these masses discharged their weights on the chassis was taken from the cad
model.
Figure 31 - Ansys model with MASS21 elements
Once the MASS21 elements were put in the model, the total weight of the car is equal to: 140.12 [Kg].
The weight of the car is still low compared to the actual one because not all the weights are considered in
the model such as the steering, the pedal, the wiring, the firewall, the hydraulic system, the seat, the body.
Introducing a weight as close as possible to the real one allows to evaluate the real stress to which the total
structure is subjected.
The weight of the structure was increased changing the chassis tubes density. During this phase, also the
position of the center of mass has been kept under control to respect the real position.
The final car model weight is: 324 [Kg]
Figure 32 - Center of mass position Center of mass
Inverter
Battery pack
Emrax

13
2.6 Meshing
The number of the model’s lines with their associated properties is high. Therefore, they were divided into
some groups and subgroups to simplify their selections for the mesh and for the postprocessing analysis.
A parametric approach was used to select the number of the elements. It was useful in the convergence
analysis.
Figure 33 - Meshed model
2.7 Tires
Tires are the unsprung mass of the vehicle. They guarantee the contact with the ground of the structure, so
they heavily influence the performance of the machine. They reduce vibrations caused from unevenness in
the road surface.
The tires were modelled with the Ansys Mechanical APDL software and then they were implemented in the
previous final model to make it more realistic.
2.7.1 Assumptions and simplifications adopted in the analysis
• Element type: SOLID186
It is a higher order 3-D 20-node solid element that exhibits. The tire was modeled with this element.
Figure 34 - SOLID186 Homogeneous Structural Solid Geometry

14
• Element type: HSFLD242
It is used to model fluids that are fully enclosed by solids (containing vessels). The pressure in the
fluid volume is assumed to be uniform.
Figure 35 - HSFLD242 Geometry
The rubber used for the tire has the following characteristics:
Young’s modulus E = 6894.8 [𝐌𝐏𝐚]
Poisson’s ratio v = 0.3
Density δ = 2.67E-9 [Mg/mm^3]
Table 9 - Tire rubber properties
C10 5.51584 [𝐌𝐏𝐚]
C01 1.37896 [MPa]
D 0
Table 10 - Mooney-Rivlin Material Model constants
The air used as the inside fluid, modeled using a compressible gas model, has these properties:
Reference temperature 20.0 [°C]
Temperature offset 274 [°C]
Initial density 1.225E-13 [Mg/mm3
]
Table 11 - Air properties
2.7.2 Tire model
Create the model geometry and mesh
The structural analysis has been performed using Ansys Mechanical APDL software. The tire model
construction started defining a typical section of the tire.
Figure 36 - Tire section
Internal radius (diameter 10 inch) 254/2 [mm]
External radius (diameter 16 inch) 406.4/2 [mm]
width 152.4 [mm]
Table 12 - Geometrical tire data

15
The above areas were rotated around an axis defined by two keypoints. The tire is then meshed using
SOLID186 solid elements and the rubber material was associated to it. The results are:
Figure 37 - Revolution area result Figure 38 - Meshed area
Pneumatic pressures of the tire are not always constant during the time of work. It is generated by the
deformation caused by contact with the ground. These pressure variations due to geometric changes were
expressed defining a hydrostatic fluid element (HSFLD242) for the tire.
Figure 39 - Tire with hydrostatic fluid element
The fluid elements cover some undesired volumes for example the rim region. These elements must exist
only in the region where air should be present. Their pyramid shaped with common vertices at each
pressure node doesn’t allow it so to solve this problem was used hydrostatic fluid elements having a
negative volume in the undesired region, as shown in this figure:
Figure 40 - Example of negative volume

16
2.8 Assembly
2.8.1 Kinematics
The machine kinematics was recreated adding to the model all the joints in such a way to simulate the real
mechanism.
Figure 41 - Rear suspensions Figure 42 - Front suspensions
The element used to simulate the shock absorbers was the COMBIN14. This element has the property that
has only the translational degree of freedom fixed. The rotational DOF are free so it wasn’t necessary to
introduce a spherical joint to the element’s ends.
Instead other joints were introduced to recreate the motion of the mechanism:
For the revolute and the three spherical types of joints in the model was used the same element type
MPC184. What changes in the spherical joints is the value of the alpha angle that represents the maximum
possible inclination of the spherical bearings. The difference depends on the model of bearing.
Alpha [°]
Spherical joint SA 10 E 12
Spherical joint GE 10 C 12
Spherical joint GEH 10 C 18
Table 13 - Different values of maximum inclination angle for all the spherical joints models
Spherical joint SA 10 E Spherical joint GE 10 C Spherical joint GEH 10 C
Revolute joint

17
The spherical joints elements don’t allow to introduce friction or a limitation in the angle inclination so it
was necessary to introduce another general joint. It was used in the elements such as the push rods, the
pull rods and the steering axles which have the possibility to rotate around themselves. This general joint
has the same properties of a spherical one but with a DOF less.
In the revolute joint could be the possibility to introduce a friction force but it was assumed without it.
Another assumption is that the steering axle is fixed and so it cannot translate.
To introduce the above joints, it was necessary to add two different reference systems for every position
where these bearings were located. One of the two reference systems was oriented parallel to the absolute
one the other it was oriented with the same inclination of the element in exams. They have the same origin
and the angle between these two gives the actual value of the angle that must not be overcame the alpha
maximum value.
Figure 43 - 2 Working planes for each joint
2.8.2 Tire connection
To simply the tires positioning a parametric model was done thanks the used of Macro. A keypoint was
associated to the wheel center and the properties realted to the wheel in exam was generated (element
type, material property, real property). In this way the wheels were built in the correct position. The wheels
were then connected with the uprights thanks the used of a revolute joint. It allows the rotation around the
upright center.
General joint (spherical one less a DOF)
ZOOM

18
3 Modal analysis
Before the dynamic transient analysis, it was useful to do this dynamic linear analysis to determine how the
structure responds to any type of dynamic load analyzing its vibrational characteristics.
The Modal Analysis is the most fundamental of all the dynamic analysis types. It is used to determine a
structure’s vibration characteristics. From this analysis in fact it was possible to find the natural
frequencies, mode shape and mode participation factors.
The car is dynamically excited from uneven or rough road profile, electric motors and transmission
vibration and more that induce the total structure to vibrate. These informations are useful to know
because if the vibration caused from the external excitation is the same as the natural frequency of the
structure it causes a phenomenon called resonance. The resonance is a negative effect because can lead to
excessive deflection of the structure. The total deflection can be enough to cause a failure in one of the
welds holding the frame together. The modal analysis allows the designer to avoid resonant vibrations or to
vibrate the structure at these specified frequencies.
If the resonant frequencies found for the structure correspond to common frequencies created from some
components of the car they should be damped to help reduce the chance of structural failure.
Another benefit of modal analysis is that gives an idea of how the design will respond to different types of
dynamic loads.
For this analysis, the model taken in exam is the total one because the extracted modes are also not
symmetric and so symmetry conditions for the structure couldn’t be applied.
The general equation of motion for a dynamic system is formulated from:
[𝑀]{𝑢̈} + [𝐶]{𝑢̇} + [𝐾]{𝑢} = {𝐹(𝑡)}
Where:
[𝑀] = global mass of the model
[𝐶] = damping of the model
[𝐾] = stiffness matrix of the model
{𝑢̈} = acceleration vector
{𝑢̇} = velocity vector
{𝑢} = displacement vector
For undamped free vibration analysis, the damping and external excitation is zero. The above equation
becomes:
[𝑀]{𝑢̈} + [𝐾]{𝑢} = 0
The solution of the above equation can be written in harmonic form as:
{𝑢} = {𝜙}𝑒 𝑖𝜔𝑡
Where:
{𝜙} = amplitudes of vibration of all the masses (mode shape or eigenvector’s)
𝜔 = natural frequency

19
If we replaced it in the above equation is reduced to:
([𝐾] − 𝜔2[𝑀]){𝜙} = 0
If 𝜔2
is replaced with λ the equation becomes a linear problem in matrix algebra.
{𝜙} has nonzero solution, then coefficient matrix must be equal zero.
Each eigenvector {𝜙} and corresponding eigenvalues was solved using ANSYS.
3.1 Problem approach
For a more detailed study different vehicle models were analyzed in this section. Starting with the analysis
of a simple model was then added further components to see their effects on the final results.
Some assumptions are adopted for this analysis:
• free degrees of freedom of the structure;
• Block Lanczos method to extract the mode shapes;
• consistent mass matrix.
To reach the final results the following steps were performed:
1) mode shapes and natural frequencies of simple structure (without tire and MASS21 elements)
2) convergence analysis of this model;
3) mode shapes and natural frequencies of complex structure (with tire and one time with
MASS21 elements another time without them)
4) mode participation factors;
5) stress analysis.
3.2 Results
3.2.1 Mode shape and natural frequencies of simple structure
The software simulates the vibrations through the structure model using several different frequencies. The
frequencies that create the largest displacements are recorded, and the mode of vibration corresponding
to each is also recorded.
The mode shapes are extracted using Block Lanczos method. It is a default method for the Ansys APDL
software. The numbers of the extracted modes and the elements used for the structure of the model make
this method good. The first modal study was done taking the chassis without tire and MASS21 elements.
Figure 44 – Torsion Figure 45 - Bending

20
3.2.2 Convergence analysis
The convergence study was done with an iteration that increment the number of nodes of the structure
changing the element size. The convergence helps to find a mesh that produce than the right results during
the solution process. The mode of shape that was taken in exam is the seventh one.
43,9
44
44,1
44,2
44,3
44,4
44,5
44,6
44,7
1132 1688 2244 2800 3356 3912 4468 5024 5580 6136
Freq[Hz]
N° Nodes
Convergence 7th mode shape
lumped
consistent
Chassis without tires and mass 21
Mode shape Natural Frequency [Hz]
1 0.000000000000
2 0.000000000000
3 0.000000000000
4 0.000000000000
5 0.000000000000
6 0.4821105167873E-02
7 44.56780336398
8 50.13026121731
9 67.80910234962
10 72.93483902935
11 87.22144848572
12 87.34452111510
13 93.89964111525
14 104.8746291085
15 106.9723254348
16 114.2932188661
17 117.1747318599
18 122.1052020549
19 124.5905001557
20 134.0908770739
21 140.8461604885
22 143.8642883282
23 148.6371927331
24 151.4075623405
25 159.9119638482
26 163.0081601106
27 172.9267851830
28 175.7895689460
29 177.9267138628
30 184.0313027977

21
The difference between the two curves in the above convergence plot depends on the mass matrix
formulation if lumped or consistent.
“Consistent” mass matrix: [𝑀] = ∫[𝑁] 𝑇
𝜌[𝑁]𝑑𝑉
• it is symmetric;
• it has a high computational cost.
“Lumped” mass matrix: ∑ 𝑀𝑗𝑗 = ∫ 𝜌𝑑𝑉
• the mass is concentrated in the nodes, equally distributed;
• it has a lower computational cost.
3.2.3 Mode shape and natural frequencies of complex structure
The modal shapes and the natural frequencies were than found for the total chassis with the tires and one
time without mass21 elements and another time with them. The element size used here was the same of
the one found with the convergence analysis in the simple structure.
The final results are tabulated in the following table:
Chassis without mass 21 and their supports Chassis with mass 21 and their supports
Mode shape Natural Frequency [Hz] Mode shape Natural Frequency [Hz]
1 0.0000 1 0.0000
2 0.0000 2 0.0000
3 0.0000 3 0.0000
4 0.0000 4 0.20313E-04
5 0.95090E-04 5 0.13462E-03
6 0.15538E-03 6 0.22914E-03
7 5.9539 7 5.8989
8 6.7436 8 6.5305
9 9.5285 9 7.3736
10 10.953 10 8.4488
11 14.335 11 14.443
12 14.581 12 14.511
13 19.288 13 19.345
14 20.148 14 19.833
15 25.883 15 26.270
16 28.606 16 28.109
17 34.637 17 29.398
18 39.442 18 38.807
19 41.305 19 42.017
20 47.883 20 44.007
21 51.090 21 47.925
22 51.807 22 49.514
23 55.146 23 50.286
24 66.204 24 53.279
25 72.311 25 53.639
26 74.682 26 57.909
27 78.803 27 63.085
28 83.030 28 66.122
29 84.570 29 72.226
30 87.906 30 73.307

22
Weight of the structure with tires = 119,219 [Kg]
Weight of the structure with tires and mass21 elements = 367,22 [Kg]
From the above results, the first six harmonics are approximately zero. This outcome was reached because
the motion of the frame is completely unconstrained, allowing for six degrees of freedom and thus six rigid
body movements. For harmonics 7 through 30, the frequencies are large enough to be appreciable.
The global vibrational characteristic of a vehicle is related to both its stiffness and mass distribution:
𝜔 =
𝑘
𝑚
As a comparison tool, the design without MASS21 elements has larger natural frequency values at each
harmonic, meaning that for the same vibration, this design has a higher stiffness to weight ratio than the
design with MASS21 elements. The MASS21 connections make the structure more rigid but the resonant
frequencies it isn’t increased because the mass increment is greater than stiffness.
In the context of improving the performance of the structure, the most pertinent mode shapes correspond
to those related to the torsional and flexural rigidity. Thus, calculation of the natural frequencies for these
mode shapes can be used to judge the rigidity figures for each type of loading.
The results related to the structure with MASS21 elements are:
Figure 46 - Mode shape 7: 5.8989 [Hz] Figure 47 - Mode shape 18 : 38.807 [Hz]
The other one is related to the structure without MASS21 elements:
Figure 48 - Mode shape 17: 34.637 [Hz] Figure 49 - Mode shape 18: 39.442 [Hz]

23
3.2.4 Mode participation factors
It shows how much a given mode participates in each direction. All the values are near to zero so there isn’t
a relevant participation of a mode in a particular direction.
3.2.5 Modal stresses
The stress values that can be extracted after the modal analysis have no real meaning, however these can
be used to highlight hot spots.
For the structure with MASS21 elements the results are:
Figure 50 - Mode shape 7: 5.8989 [Hz]
Figure 51 - Mode shape 18: 38.807 [Hz]

24
4 Transient dynamic analysis
Transient analysis (sometimes called time-history analysis) was used to determine the dynamic response of
the structure under the action of time-dependent loads. With this type of analysis was determined the
time-varying displacements, strains, stresses, and forces in the structure as it responds to the combination
of static, transient loads. The time scale of the loading is such that the inertia or damping effects are
important.
The equation for a transient dynamic analysis is the same as the general equation of motion:
[M]{𝑢̈} + [C]{𝑢̇} + [K]{u} = {F(t)}
where:
[M] = mass matrix
[C] = damping matrix
[K] = stiffness matrix
{𝑢̈} = nodal acceleration vector
{𝑢̇} = nodal velocity vector
{u} = nodal displace
The goal of this project is to do a structural analysis of the model. For the high complexity of the simulation
of the real car’s behavior some assumptions must be done.
These assumptions are:
• the motion along the longitudinal direction is constrained;
• the car behavior is affected changing the accelerations along lateral and longitudinal direction;
• the static weight of the car is imposed as a prestress force;
• the tires can’t slip;
• the tires can’t detach from the ground;
• the tires model used is the equivalent one with the springs.
To reach the final results the following steps were performed:
1) equivalent tire system;
2) define boundary conditions;
3) prestressed static nonlinear analysis;
4) solution;
5) postprocessing and results.
4.2 Equivalent tire system
The method used to solve the transient analysis was the full method. This method has a high computational
cost so it was necessary to use an equivalent tire system to reduce it. Therefor this equivalent system was
implemented in the final model of the car for the final transient analysis.
The equivalent system simulates each wheel with two unidirectional springs, one in the vertical direction
and the other in lateral one. To define the stiffness of these springs it was necessary to study the tire model
behavior.
The tire used for the creation of the equivalent model is the one created above in the section of Finite
Element Model. A single tire was analyzed in transient environment with the use of contact elements.

25
The following steps were used to create the model:
1) contact elements definition;
2) weight car distribution;
3) transient analysis;
4) results;
5) creation of an equivalent tire model.
4.2.1 Contact elements definition
4.2.1.1 Assumptions and simplifications adopted in the analysis
• Target element (pilot rim node, road): TARGE170
It is a 3-D "target" surfaces.
Figure 52 - TARGE170 Geometry
Contact element (tire): CONTA174 for deformable surfaces Contact element (rim nodes): CONTA175
Figure 53 - CONTA174 Geometry Figure 54 - CONTA175 Geometry
4.2.1.2 Contact models adopted
Ansys supports three contact models: node-to-node, node-to-surface, and surface-to-surface. Each type of
model uses a different set of Ansys contact elements and is appropriate for specific types of problems.
• Node-to-surface model
This contact type was used to simulate an infinitely rigid rim.

26
Figure 55 – Fixed support for the tire surface bounded to the rim
• Surface-to-surface model
This was used to simulate the tire contact with the infinitely rigid ground.
Figure 56 - Tire-road contact
4.2.2 Weight car distribution
In every simulation was applied the load to simulate the car weight distribution that is different for the rear
and front wheels. It was possible thanks an MASS21 element applied to the center of the wheel because it
represents the gravity center of axle;
Car weight without unsprung elements (wheels) = 324 [Kg]
The different mass distributions were kept from the position of center of mass found in the model of Ansys
APDL software.
Pilot rim node
(TARGE170)
Rim nodes
(CONTA175)
Tire external surfaces
(CONTA174)
Road surfaces
(TARGE170)

27
Figure 57 - Top car view
wheelbase = 1540 [mm]
b = rear axle = 430.35 [mm] = 27.9% of wheel base
a = front axle = 1109.64 [mm] = 72.1% of wheel base
In terms of weight:
• 90 [kg] acts on front wheels = 27.9% of 324 [Kg]
• 233.604 [kg] acts on rear wheels = 72.1% of 324 [Kg]
The final loads on the single wheels are:
Fz load on the front wheel = 45 [Kg] * 9.81 [m/𝑠2
] = 441.45 [N]
Fz load on the rear wheel = 116.802 [Kg] * 9.81 [m/𝑠2
] = 1145.83 [N]
4.2.3 Transient tire analysis
To find the stiffness along the z direction, perpendicular to the ground, was done the following operations
solved in different load steps:
• it was fixed the tire with its pilot node;
• it was applied the weight force of the tire introducing the gravity acceleration.
Wheel weight = 5.46 [Kg];
• an initial temperature of 20 °C it was applied at the pilot node;
wheelbase
b a

28
Figure 58 - Rear tire: Load step 1
• the tire was inflated applying a pressure boundary condition to the constrained pressure node
(hydrostatic pressure of 36 psi = 0.2482128 N/ mm2
);
Figure 59 - Rear tire: Load step 2
• during the operations above the tire wasn’t still in contact with the ground. In this step was given
an z displacement to bring the wheel into contact with the ground and the behavior of the tire was
studied during its deformation;
Figure 60 - Rear load: Load step 3
• in the last load step, the tire was translated in the initial position.
To find the stiffness along the z direction of the front wheels was following the same steps done above for
the rear one with the only difference of the force due to the car distributed weight.
Instead to find the stiffness along the y direction once time the tires come into contact with ground was
translated in y direction.

29
Figure 61 - Rear tire translations
Friction coefficient used: μ = 1.1; In this case the friction coefficient exceeded the 1 value. This is verified
only with very soft and hot slick tires, which can take the shape of the ground roughness. It generates a
mechanical clamping force with a higher grip than the simple friction force.
4.2.4 Results
The results obtained from the transient analysis are:
Figure 62 - Displacement history in time (Rear tire) Figure 63 - Load history in time (Rear tire)
For the vertical stiffness:
Figure 64 - Reaction Force - Displacement (Rear tire) Figure 65 – Reaction Force - Displacement (Front tire)
[s]
[mm]
[s]
[N]
Z Displacement [mm]
ZForce[N]
ZForce[N]
Z Displacement [mm]

30
The figure 64 and figure 65 have a similar nonlinear trend. The difference between the two is given by the
car weight.
For the lateral stiffness:
Figure 66 - Reaction Force - Displacement (Rear tire) Figure 67 - Reaction Force - Displacement (Front tire)
In the figure 66 and figure 67 there is a linear trend differently from the one in Z direction. The lateral
deformation values of the tire are high because the tire shoulder is not as stiff as it is. For this reason, in the
final transient simulation a greater stiffness was used to avoid such possible wrong deformations.
4.2.5 Tire conclusions
To simulate the tire equivalent model with the results obtained above the COMBIN39 element and the
COMBIN14 one was introduced. The first was used for the vertical spring stiffness direction the second one
for the lateral direction.
Figure 68 –Structure with equivalent tires model
YForce[N]
Y Displacement [mm] YForce[N] Y Displacement [mm]

31
It is a unidirectional element with nonlinear generalize force-deflection capability that can be use
in any analysis.
Figure 69 - COMBIN39 geometry
The curves used for this element come from the before tire simulation analysis are discretized in this plot:
To avoid the detach of the contact tire point with the ground an extension of the curves was done.
It is a 3-D longitudinal spring-damper without mass. No bending or torsion is considered.
It was used this element for the lateral stiffness because the above figure 66 and 67 have a linear behavior.
The stiffness used for the simulation is 12000 [N/mm].
-6000
-5000
-4000
-3000
-2000
-1000
0
1000
2000
-20 -15 -10 -5 0 5 10 15
Force[N]
Displacement [mm]
Vertical tire stiffness
kz_front
kz_rear

32
4.3 Boundary conditions
The following constraints were imposed to get the final solution:
• points of tires contacts: the UX displacement (longitudinal direction) was constrained;
• points at the end of the springs: All DOF were constrained.
Figure 70 - Constrained model
4.4 Prestressed Static Nonlinear analysis
At this section, a prestress was implemented to make the structure subject to its own weight avoiding the
car trim changes in the transient analysis.
4.5 Solution
Two methods are available to do a transient dynamic analysis: full and mode-superposition.
The advantages of the full method are:
• it is easy to use, because you do not have to worry about choosing mode shapes;
• it allows all types of nonlinearities;
• it uses full matrices, so no mass matrix approximation is involved;
• all displacements and stresses are calculated in a single pass;
•it accepts all types of loads: nodal forces, imposed (nonzero) displacements (although not
recommended), and element loads (inertia acceleration, temperature) and allows tabular boundary
condition specification via TABLE type array parameters;
• it allows effective use of solid-model loads.
The main disadvantage of the full method is that it is more expensive than the mode-superposition
method.
The advantages of mode-superposition are:
• it is faster and less expensive than the full method for many problems;
• element loads applied in the preceding modal analysis can be applied in the transient dynamic
analysis;
• it accepts modal damping (damping ratio as a function of mode number).

33
The disadvantages of the mode-superposition method are:
• the time step must remain constant throughout the transient, so automatic time stepping is not
allowed;
• the only nonlinearity allowed is simple node-to-node contact (gap condition);
• it does not accept imposed (nonzero) displacements.
For these reasons, considering having a simplified model with beam and springs elements, the full method
was chosen.
The actual accelerations to which the car is subjected were used in this analysis.
The path chosen for this study is a characteristic one in the FSAE competition. This path is called “Skid Pad”.
It is a test that involves running an 8-way track in the shortest time avoiding leaving the track by running at
least two laps per circumference.
The trajectory plotted below was calculated to avoid the wheel slip with the highest possible speed.
To find the ideal path and the accelerations corresponding to it, a Matlab code developed by the dynamic
colleagues was used. The data relating to the accelerations and therefore the forces act on the structure
were passed into the Ansys APDL car model.
Where:
Boundary circuit
Trajectory of tire
Center car
The acceleration curves to which the car is subjected are:
Start
End
Figure 71 - Skid Pad data

34
The related velocities are:
4.6 Results
4.6.1 Loads on tire
To understand how the total structure is stressed the load history must be known. The starting point are
the reaction forces that the car receives from the ground through the wheels.
In the plot below, that represents the tires reaction forces during the skid pad test, the weight car force
was considered in the dynamic load transfer.
Vertical loads results:
At time 1.5 [s] (first acceleration) and at time 10.6 [s] (change of car direction) there are peaks in the
vertical plots loads. In these points, the tire tends to detach from the ground. Especially the internal front
wheel is discharged during the curve so it tends to detach because the vehicle distribution weight is
localized mostly in the rear part.
-200
0
200
400
600
800
1000
1200
0,2
1,6
3
4,4
5,8
7,2
8,6
10
11,4
12,8
14,2
15,6
17
18,4
19,8
Force[N]
Time [s]
Front vertical loads
FZ_front_RIGHT FZ_front_LEFT
0
500
1000
1500
2000
0,2
1,6
3
4,4
5,8
7,2
8,6
10
11,4
12,8
14,2
15,6
17
18,4
19,8
Force[N]
Time [s]
Rear vertical loads
FZ_rear_RIGHT FZ_rear_LEFT

35
Lateral loads results:
The grip limit values found during the tire analysis model are:
• 3800 [N] for the rear wheels;
• 1700 [N] for the front wheels.
Observing the lateral loads results can be seen that the rear wheels in the points of higher acceleration slip.
In fact, the springs that simulate the wheels give a reaction force higher than the real grip condition. This
can lead to have a peaks load on the structure higher to the actual ones.
4.6.2 Stress analysis
The stress peaks occur during trajectory change. There is this event when the machine moves from one
circle to the other one of the path during the skid pad test.
-1500
-1000
-500
0
500
1000
1500
0,2
1,6
3
4,4
5,8
7,2
8,6
10
11,4
12,8
14,2
15,6
17
18,4
19,8
Force[N]
Time [s]
Front lateral loads
FY_front_RIGHT FY_front_LEFT
-6000
-4000
-2000
0
2000
4000
6000
0,2
1,6
3
4,4
5,8
7,2
8,6
10
11,4
12,8
14,2
15,6
17
18,4
19,8
Force[N]
Time [s]
Rear lateral loads
FY_rear_RIGHT FY_rear_LEFT
0
20
40
60
80
100
120
140
160
0,2
0,8
1,4
2
2,6
3,2
3,8
4,4
5
5,6
6,2
6,8
7,4
8
8,6
9,2
9,8
10,4
11
11,6
12,2
12,8
13,4
14
14,6
15,2
15,8
16,4
17
17,6
18,2
18,8
19,4
Stress[Mpa]
Time [s]
Equivalent stress
s_chass [Mpa] s_susp[Mpa]

36
Below it was plotted the structure equivalent stress at the time 10,6 [s] which is the time when the change
of direction takes place.
Figure 72 - Equivalent stress during change of direction
At the same time was plotted the equivalent stress isolating the suspensions group from the total structure.
The final stress scale was redefined and so the stress behaviour in the following group can be better see.
Figure 73 - Suspensions equivalent stress during change of direction
ZOOM

37
4.6.3 Chassis torsion
The primary function of the chassis is to support the load transfer. For this reason, the torsional stiffness is
the main one that affects the vehicle dynamic. Therefore, this aspect has been largely discussed in the
following report.
To find the chassis torsion in Ansys was done the difference between the front and rear rotation of the axes
with respect to the roll center.
As can be seen from the above chart, the chassis behaves like a torsional spring due to the weight
distribution difference. The advantage of having such small deformations is that at each elastic return of
the chassis in the curve exit there are less oscillations, and so less impact on the driver’s guidance.
4.6.4 Camber deformation
The camber angle is given by the inclination of the car’s wheels. In fact, it is the angle between the vertical
axis of the wheels used for steering and the vertical axis of vehicle when viewed from the front or rear.
Figure 74 - Positive and negative camber
Knowing the camber angle is important because from it depends the adherence of the machine in curve. A
variation of it can generate a not optimal road holding.
-0,15
-0,1
-0,05
0
0,05
0,1
0,15
0,2
1
1,8
2,6
3,4
4,2
5
5,8
6,6
7,4
8,2
9
9,8
10,6
11,4
12,2
13
13,8
14,6
15,4
16,2
17
17,8
18,6
19,4
Torsion[Deg]
Time [s]
Chassis torsion

38
4.6.5 Steering deformation
This is another aspect that influences the dynamic behaviour of the car. It was found adding to the model
rigid rods with longitudinal direction and fixed to the uprights centres. Their oscillations respect to the
longitudinal vertical plane during the skid pad test gives the steering deformation.
As can be seen from the above plots the values of these oscillations are small. This is a good result because
otherwise it could generate problems while the pilot drives the car.
Approach the curve in the best possible way without errors it is important especially in the FSAE tracks that
are precise and tight. It is good to keep under control this parameter because the structure is highly
affected by acceleration.
-0,06
-0,04
-0,02
0
0,02
0,04
0,06
0,2
1,6
3
4,4
5,8
7,2
8,6
10
11,4
12,8
14,2
15,6
17
18,4
19,8
Inclination[deg]
Time [s]
Front camber deformation
alpha_front_RIGHT alpha_front_LEFT
-0,06
-0,04
-0,02
0
0,02
0,04
0,06
0,2
1,6
3
4,4
5,8
7,2
8,6
10
11,4
12,8
14,2
15,6
17
18,4
19,8
Inclination[deg]
Time [s]
Rear camber deformation
alpha_rear_RIGHT alpha_rear_LEFT
-0,03
-0,02
-0,01
0
0,01
0,02
0,2
1,6
3
4,4
5,8
7,2
8,6
10
11,4
12,8
14,2
15,6
17
18,4
19,8
Rotation[deg]
Time [s]
Front steering deformation
theta_front_RIGHT theta_front_LEFT
-0,02
-0,015
-0,01
-0,005
0
0,005
0,01
0,015
0,02
0,2
1,6
3
4,4
5,8
7,2
8,6
10
11,4
12,8
14,2
15,6
17
18,4
19,8
Rotation[deg]
Time [s]
Rear steering deformation
theta_rear_RIGHT theta_rear_LEFT

39
5 Validation Model
The Ansys model was compared with the ones obtain with a code implemented in Matlab to verify the
goodness of the model.
The validation starts with the definition of the dynamic loads to which the structure is subjected. These
loads generate a load transfer in different possible directions. The load transfer analyzed in this section was
the one related to the roll rotation.
In the Ansys and Matlab model the load transfer values were found respect to the stiffness of the springs. If
the final results of the two models are the same can be demonstrate that the Ansys model respect the
vehicle dynamic.
The load transfer results from the Matlab code were plotted below for different mass car distribution. At
each different line in the relative plots corresponds a different chassis stiffness:
Figure 75 – 50% distribution mass between front and rear Figure 76 - 73% front distribution mass and 27% rear
distribution mass
As can be seen in the above plots the weight distribution and the chassis stiffness influenced the response
respect the variation of the stiffness springs car. The goal of the structure is to have a linear trend. The
linear behavior is good because it means that the chassis structure is stiffness enough to permit a different
load transfer distribution changing the anti-roll stiffness of the car. In the model to change the anti-roll
stiffness is possible changing the shock absorber stiffness.
Once the linearity of the curve is reached any further increase in stiffness will no longer be appreciable.
In the Ansys and Matlab models the weight force wasn’t introduced because under steady state conditions
it can be simplified without change the finale results.
The Ansys model to validate is the same of the one used in the transient analysis (figure 68):
for the model validation, it was calculated the chassis load transfer changing the distribution of the anti-roll
stiffness between the front and rear of the car.

40
The validation was done with a steady state analysis. A constant lateral acceleration was provided to the
model.
The steps followed for the validation are:
1) vehicle parameters definitions;
2) chassis torsional stiffness calculation;
3) antiroll stiffness (ARS) calculation;
4) static nonlinear analysis in Ansys;
5) Matlab analytical model calculation;
6) results comparison.
5.2 Vehicle parameters
The car’s characteristics that are used in the Matlab code, many of which were extracted from the Ansys
model, are:
Parameters Meaning
B = 0.43 [m] Rear leverage wheelbase
a = 1.540 – 0.43 [m] Front leverage wheelbase
h = 0.228 [m] zCG sprung mass
fT = 1.27 [m] Front truck
rT = 1.24 [m] Rear truck
N = 0.056 [m] Front roll center height
m = 0.034 [m] Rear roll center height
r = 0.203 [m] Center wheel (unsprung mass)
ng = 1.2*9.81 [m/s^2] Lateral acceleration
m_unsprung_front = 0 [Kg] Front unsprung mass
m_unsprung_rear = 0 [Kg] Rear unsprung mass
m_sprung = 324.14 [Kg] Sprung mass
Table 14 - car parameters
5.3 Chassis torsional stiffness
The chassis torsional stiffness is the ability of a structure to resist a pure moment application. It was done
with a static test simulation in ANSYS environment.
Constraints conditions:
• fixed translations UX, UY, UZ and rotations ROTX, ROTZ of the rear hubs leaving the pitch rotation
free;
• shock absorbers infinitely rigid stiffness;
• +/- 6 [mm] imposed displacement along z axis to the front hubs (equal and opposite displacements
to the front). The 6 [mm] value was taken from the tests of other FSAE team.

41
Figure 77 - Structure under constraints
Figure 78 - Torsional analysis results (blue line = deformed structure, dotted white line = initial not deformed structure)
The value of the reaction forces where the displacements were imposed are:
• FL = -388.77 (Front left hub node reaction);
• FR = +388.33 (Front right hub node reaction).
Figure 79 - Torsion axle scheme
θ
𝑀𝑡disp
Ft
θ disp

42
Where:
disp = vertical displacement = 6 [mm]
Ft = front track = 1270 [mm]
𝑀𝑡 = Chassis torsional moment = |𝐹𝐿| ∗ (
𝐹𝑡
2
) + |𝐹𝑅| ∗ (
𝐹𝑡
2
) = 493737.9 [Nmm]
𝜃 = rotaion angle = tan−1
(
𝑑𝑖𝑠𝑝 ∗ 2
𝐹𝑡
) = 0.54 [deg]
𝐾 = torsional stiffness value =
𝑀𝑡
1000
𝜃
= 𝟗𝟏𝟐. 𝟎𝟓 [
Nm
deg
]
5.4 Antiroll stiffness (ARS)
The rear and front ARS it was also find analytically.
• Ft = Front track = 1270 [mm]; H_Ft = Half front track = 1270/2 = 635 [mm];
• Rt = Rear track = 1240 [mm]; H_Rt = Half rear track = 1240/2 = 630 [mm];
• Kt= it is the total springs stiffness that it was assumed constant and its value was fixed equal to 30
[Nm/deg];
• Perc = stiffness distribution front and rear variable
K_front = front springs stiffness = 3 [Nm/deg] (if Perc = 10);
K_rear = rear springs stiffness = 27 [Nm/deg] (if Perc = 10);
The springs stiffness related to the tires is the ones calculated before in the tire results section.
The curves were linearized to find the linear value of the stiffness and they are plotted below:
y = 283,96x - 551,96
-5000
-4000
-3000
-2000
-1000
0
1000
2000
3000
-15 -10 -5 0 5 10 15
Force[N]
Displacement [mm]
Z stiffness rear
y = 271,3x - 432,83
-6000
-4000
-2000
0
2000
4000
-20 -10 0 10 20
Force[N]
Displacement [mm]
Z stiffness front
F
Ft; Rt
θ
θ
F
H_Ft; H_Rt
disp_f ; disp_r
disp_f ; disp_r

43
• Kz_rear = rear vertical tire stiffness = 283.96 [N/mm];
• Kz_front = front vertical tire stiffness = 271.3 [N/mm];
From these stiffness, an equivalent one was calculated as series springs:
• Keq_rear =
K_rear ∗ Kz_rear
K_rear+Kz_rear
;
• Keq_front =
K_front ∗ Kz_front
K_front+Kz_front
;
• F = Random number force apply to the springs = 100 [N];
• disp_f = F/ Keq_front; disp_r = F/ Keq_rear;
• k_antiroll_front =
HFt∗𝐹
atan(
𝑑𝑖𝑠𝑝_𝑓
HFt
)∗(
180
𝜋
)
= 165285.67 [Nmm/deg];
• k_antiroll_rear =
HRt∗𝐹
atan(
𝑑𝑖𝑠𝑝_𝑟
HRt
)∗(
180
𝜋
)
= 20890.64 [Nmm/deg];
• Kt_antiroll = it is the total anti-roll stiffness =
k_antiroll_front + k_antiroll_rear = 186.17 [Nm/deg].
5.5 Static nonlinear analysis in Ansys
The model used for this study is the same of the one used in the transient analysis.
The Ansys mechanical APDL can be schematized in the following way:
Figure 80 - Load transfer due to lateral acceleration
CG = center of gravity
CG
ANSYS model𝐾𝑡𝑜𝑡
perc
𝐾𝑓𝑟𝑜𝑛𝑡
𝐾𝑟𝑒𝑎𝑟
𝚫 𝑓𝑟𝑜𝑛𝑡_𝑛𝑜𝑟𝑚𝑎𝑙𝑖𝑧𝑒𝑑
𝚫 𝑟𝑒𝑎𝑟_𝑛𝑜𝑟𝑚𝑎𝑙𝑖𝑧𝑒𝑑

44
Legend:
• perc = it is an integer that change the distribution of the anti-roll stiffness between the front and
the rear of the car thanks a loop cycle in ANSYS model;
• 𝑲 𝒕𝒐𝒕 = it is the total springs stiffness that it was assumed constant and its value was fixed equal to
30 [Nm/deg];
• 𝑲 𝒇𝒓𝒐𝒏𝒕 = it is the front anti-roll stiffness;
• 𝑲 𝒓𝒆𝒂𝒓 = it is the rear anti-roll stiffness;
• 𝚫 𝑓𝑟𝑜𝑛𝑡_𝑛𝑜𝑟𝑚𝑎𝑙𝑖𝑧𝑒𝑑 = front load transfer / total load transfer;
• 𝚫 𝑟𝑒𝑎𝑟_𝑛𝑜𝑟𝑚𝑎𝑙𝑖𝑧𝑒𝑑 = rear load transfer / total load transfer;
• total load transfer = front load transfer + rear load transfer.
5.6 Matlab analytical model calculation
For the MATLAB model, it was necessary to introduce an analytical equation to calculate the transfer load
when the car is subjected to a lateral acceleration:
𝚫𝐅 𝑧 = 𝚫𝐅 𝑧 𝑠𝑝𝑟𝑢𝑛𝑔 + 𝚫𝐅 𝑧 𝑢𝑛𝑠𝑝𝑟𝑢𝑛𝑔
In the equation above there are two load transfer contributions:
𝚫𝐅 𝑧 𝑠𝑝𝑟𝑢𝑛𝑔 = sprung mass contribution which are those that don’t stand on the ground such as the
suspensions.
𝚫𝐅 𝑧 𝑢𝑛𝑠𝑝𝑟𝑢𝑛𝑔 = unsprung mass contribution which stand on the ground.
Figure 82 - Load transfer components
Front ARS
Rear ARS
Figure 81 - Matlab schematized model

45
The sprung mass contribution can be also divided in two parts:
𝚫𝐅 𝑧 𝑠𝑝𝑟𝑢𝑛𝑔 = 𝚫𝐅 𝑧 𝑒𝑙𝑎𝑠𝑡𝑖𝑐 + 𝚫𝐅 𝑧 𝑔𝑒𝑜𝑚𝑒𝑡𝑟𝑖𝑐
𝚫𝐅 𝑧 𝑒𝑙𝑎𝑠𝑡𝑖𝑐 = it depends on inertia and so it takes time to be absorbed.
𝚫𝐅 𝑧 𝑔𝑒𝑜𝑚𝑒𝑡𝑟𝑖𝑐 = it happens quickly when the car enters in the curve.
The equation above after these considerations becomes:
𝚫𝐅 𝑧 = 𝚫𝐅 𝑧 𝑒𝑙𝑎𝑠𝑡𝑖𝑐 + 𝚫𝐅 𝑧 𝑔𝑒𝑜𝑚𝑒𝑡𝑟𝑖𝑐 + 𝚫𝐅 𝑧 𝑢𝑛𝑠𝑝𝑟𝑢𝑛𝑔
𝚫𝐅 𝑧 𝑒𝑙𝑎𝑠𝑡𝑖𝑐 =
𝑚 𝑠𝑝𝑟𝑢𝑛𝑔 ∗ 𝐿𝑎𝑡𝑔 ∗ (𝑧 𝐶𝐺𝑠𝑝𝑟𝑢𝑛𝑔 − 𝑧 𝑅𝐶)
𝑡𝑟𝑎𝑐𝑘
𝚫𝐅 𝑧 𝑔𝑒𝑜𝑚𝑒𝑡𝑟𝑖𝑐 =
𝑚 𝑠𝑝𝑟𝑢𝑛𝑔 ∗ 𝐿𝑎𝑡𝑔 ∗ 𝑧 𝑅𝐶
𝚫𝐅 𝑧 𝑢𝑛𝑠𝑝𝑟𝑢𝑛𝑔 =
𝑚 𝑢𝑛𝑠𝑝𝑟𝑢𝑛𝑔 ∗ 𝐿𝑎𝑡𝑔 ∗ 𝑧 𝐶𝐺𝑢𝑛𝑠𝑝𝑟𝑢𝑛𝑔
Variables Meaning
𝒎 𝒔𝒑𝒓𝒖𝒏𝒈 Sprung mass
𝒎 𝒖𝒏𝒔𝒑𝒓𝒖𝒏𝒈 Unsprung mass
𝑳𝒂𝒕𝒈 Lateral acceleration
𝒛 𝑪𝑮𝒔𝒑𝒓𝒖𝒏𝒈 Center of gravity z coordinate of
sprung mass
𝒛 𝑪𝑮𝒖𝒏𝒔𝒑𝒓𝒖𝒏𝒈 Center of gravity z coordinate of
unsprung mass
𝒛 𝑹𝑪 Roll center
𝒕𝒓𝒂𝒄𝒌 Track of the car
Figure 83 - Equations variables meaning
Usually in the racing cars the anti-roll stiffness between front and rear change and it permits to better set
the car for the specific competition to do.
In our model, the anti-roll stiffness changes with the different stiffness between front and rear of the shock
absorbers.
After these considerations, it was necessary to readapt the precedent equations introducing the front and
rear load transfer:
𝚫𝐅 𝑧 𝑒𝑙𝑎𝑠𝑡𝑖𝑐 {
𝚫𝐅 𝑧 𝑒𝑙𝑎𝑠𝑡𝑖𝑐, 𝑓𝑟𝑜𝑛𝑡 =
𝑚 𝑠𝑝𝑟𝑢𝑛𝑔,𝑓𝑟𝑜𝑛𝑡 ∗ 𝐿𝑎𝑡𝑔 ∗ (𝑧 𝐶𝐺𝑠𝑝𝑟𝑢𝑛𝑔 − 𝑧 𝑅𝐶𝑓𝑟𝑜𝑛𝑡)
𝐹𝑟𝑜𝑛𝑡𝑇𝑟𝑎𝑐𝑘
𝐹𝑟𝑜𝑛𝑡 𝐴𝑅𝑆
𝑇𝑜𝑡𝑎𝑙 𝐴𝑅𝑆
𝚫𝐅 𝑧 𝑒𝑙𝑎𝑠𝑡𝑖𝑐, 𝑟𝑒𝑎𝑟 =
𝑚 𝑠𝑝𝑟𝑢𝑛𝑔,𝑟𝑒𝑎𝑟 ∗ 𝐿𝑎𝑡𝑔 ∗ (𝑧 𝐶𝐺𝑠𝑝𝑟𝑢𝑛𝑔 − 𝑧 𝑅𝐶𝑟𝑒𝑎𝑟)
𝑅𝑒𝑎𝑟𝑇𝑟𝑎𝑐𝑘
𝑅𝑒𝑎𝑟 𝐴𝑅𝑆
𝑇𝑜𝑡𝑎𝑙 𝐴𝑅𝑆
𝚫𝐅 𝑧 𝑔𝑒𝑜𝑚𝑒𝑡𝑟𝑖𝑐 {
𝚫𝐅 𝑧 𝑔𝑒𝑜𝑚𝑒𝑡𝑟𝑖𝑐, 𝑓𝑟𝑜𝑛𝑡 =
𝑚 𝑠𝑝𝑟𝑢𝑛𝑔,𝑓𝑟𝑜𝑛𝑡 ∗ 𝐿𝑎𝑡𝑔 ∗ 𝑧 𝑅𝐶𝑓𝑟𝑜𝑛𝑡
𝚫𝐅 𝑧 𝑔𝑒𝑜𝑚𝑒𝑡𝑟𝑖𝑐, 𝑟𝑒𝑎𝑟 =
𝑚 𝑠𝑝𝑟𝑢𝑛𝑔,𝑟𝑒𝑎𝑟 ∗ 𝐿𝑎𝑡𝑔 ∗ 𝑧 𝑅𝐶𝑟𝑒𝑎𝑟

46
𝚫𝐅 𝑧 𝑢𝑛𝑠𝑝𝑟𝑢𝑛𝑔 {
𝚫𝐅 𝑧 𝑢𝑛𝑠𝑝𝑟𝑢𝑛𝑔, 𝑓𝑟𝑜𝑛𝑡 =
𝑚 𝑢𝑛𝑠𝑝𝑟𝑢𝑛𝑔,𝑓𝑟𝑜𝑛𝑡 ∗ 𝐿𝑎𝑡𝑔 ∗ 𝑧 𝐶𝐺𝑢𝑛𝑠𝑝𝑟𝑢𝑛𝑔
𝚫𝐅 𝑧 𝑢𝑛𝑠𝑝𝑟𝑢𝑛𝑔, 𝑟𝑒𝑎𝑟 =
𝑚 𝑢𝑛𝑠𝑝𝑟𝑢𝑛𝑔,𝑟𝑒𝑎𝑟 ∗ 𝐿𝑎𝑡𝑔 ∗ 𝑧 𝐶𝐺𝑢𝑛𝑠𝑝𝑟𝑢𝑛𝑔
The chassis also is flexible and so it was introduced in the model.
The result can be summarized in the following matrix form:
[
𝑀𝑟𝑜𝑙𝑙 𝑓𝑟𝑜𝑛𝑡
𝑀𝑟𝑜𝑙𝑙 𝑟𝑒𝑎𝑟
0
] = [
𝐾𝑓𝑟𝑜𝑛𝑡 0 −𝐾𝑐ℎ𝑎𝑠𝑠𝑖𝑠
0 𝐾𝑟𝑒𝑎𝑟 𝐾𝑐ℎ𝑎𝑠𝑠𝑖𝑠
1 −1 1
] [
∅ 𝑓𝑟𝑜𝑛𝑡
∅ 𝑟𝑒𝑎𝑟
∅ 𝑐ℎ𝑎𝑠𝑠𝑖𝑠
]
Figure 84 – Matrix parameters
5.7 Results
The final results from the two software are plotted below:
0,00
20,00
40,00
60,00
80,00
100,00
5 10 15 20 25 30 35 40 45 50 55 60 65 70 75 80 85 90 95
FrontLoadtransf/TotalLoad
Transfer
Front Antiroll stiffness/ total antiroll stifness
Front load trasfert
Ansys model Matlab model
0,00
20,00
40,00
60,00
80,00
100,00
5 10 15 20 25 30 35 40 45 50 55 60 65 70 75 80 85 90 95
RearLoadtransf/TotalLoad
Transfer
Rear load transfert
Ansys model Matlab model
Variables Meaning
𝑴 𝒓𝒐𝒍𝒍 𝒇𝒓𝒐𝒏𝒕 Front anti-roll moment
𝑴 𝒓𝒐𝒍𝒍 𝒓𝒆𝒂𝒓 Rear anti-roll moment
𝑲 𝒇𝒓𝒐𝒏𝒕 Front anti-roll stiffness
𝑲 𝒓𝒆𝒂𝒓 Rear anti-roll stiffness
𝑲 𝒄𝒉𝒂𝒔𝒔𝒊𝒔 Torsional stiffness chassis
∅ 𝒇𝒓𝒐𝒏𝒕 Front roll angle
∅ 𝒓𝒆𝒂𝒓 Rear roll angle
∅ 𝒄𝒉𝒂𝒔𝒔𝒊𝒔 Chassis roll angle

47
In the first and the second above plots the lines are essentially overlapped. This proves the validity of the
Ansys model. In the central zone of the curves, that corresponds to the work range, the lines are the same.
The only difference can be seen in the final parts when the antiroll stiffness rear is low. This low value
generates a non-linearity in the Ansys model not expected in Matlab one.
This non-linearity can be observed in the plot of the structure torsion respect the front antiroll distribution
stiffness:
An assumption done in the Matlab analytical model is that the torsional stiffness of the structure is linear.
On the other hand, as can be seen from the above plot the structure behaviour coming from the Ansys
model it isn’t linear changing the front antiroll distribution stiffness. While calculating the stiffness of the
structure with shock absorbers infinitely rigid the stiffness response is linear.
-0,2
-0,15
-0,1
-0,05
0
0,05
0,1
0 20 40 60 80 100
Torsionstructure[deg]
Behavior of structure

48
6 Conclusions and future developments
The results found in this report, related to the structural dynamic analysis of the FSAE vehicle, have allowed
to evaluate the properties of the structure itself. These results are related to the skid pad test but changing
the accelerations that act on the structure can be evaluated the different vehicle performances and
behaviours. In fact, it is possible to use this vehicle model for any type of possible track.
Thanks to the Modal analysis was possible to see the frequencies values that can lead the structure into
resonance. These resonance frequencies at which the car could be subjected must be avoid. This analysis
gave also an idea of how the structure vibrate under some frequencies. Farther It permitted to know where
the major stresses are localized.
The study was then developed in a Transient analysis. In this analysis was proved that an equivalent tire
model gives good results respect the global behavior of the structure. Among the most relevant results
there is the stress analysis. It has provided the most stressed areas during the Formula SAE skid pad test
(figure 72). These areas must be taken more into account in the design phase of future version of the
vehicle structure. The points most stressed are localized at the connections between the suspensions and
the chassis. These results have allowed to prove the real security of the structural components.
The deformations to which the structure was subjected must be considered and controlled. Among them
there is the chassis torsion that thanks to this analysis was demonstrated its importance for the dynamic
vehicle effects. The amplitudes found for this parameter don’t allow negative effects also during the change
direction of the vehicle. Other possible deformations are related to the camber or the steering axles. They
are the result of the deformation of several components assembled between them (for example bearings,
hub and upright). From the results it pointed out that the chassis’s contribution for the deformation is low.
Through the validation of the model it was possible to demonstrate the model goodness. But under some
conditions the analytical model used in Matlab software loses some non-linearity due to the structure. For
this reason, a control of structural parameters through an analysis can reveal some details that otherwise
wouldn’t have been considered. For example, in the active suspensions changing the vehicle front and rear
stiffness change the vehicle trim and any nonlinear effect can be considered.

49
6 References
• ANSYS, ANSYS Mechanical APDL Structural Analysis Guide, Release 15.0, November 2013
• ANSYS, ANSYS Mechanical APDL Verification Manual, Release 15.0, November 2013
• William F. Milliken, Douglas L. Milliken, Race Car Vehicle Dynamics,1997
• SAE International, Formula SAE® Rules, 2017-18, April 11, 2016
• Alberto Nardin, Università degli studi di Padova, “Progetto e sviluppo di un telaio a traliccio di tubi in acciaio
per vettura FSAE”, 2014-15
• Mohammad Al Bukhari Marzuki, Mohammad Hadi Abd Halim and Abdul Razak Naina Mohamed,
“Determination of Natural Frequencies through Modal and Harmonic Analysis of Space Frame Race Car
Chassis Based on ANSYS”, Department of Mechanical Engineering Malaysia, American Journal of Engineering
and Applied Sciences, October 2014
• University of Delaware, FSAE Chassis: Phase IV Report, October 2010
• William B. Riley and Albert R. George, Cornell University, “Design, Analysis and Testing of a Formula SAE Car
Chassis”, 2002
• Mohammad Al Bukhari Marzuki, Mohd Arzo Abu Bakar and Mohammad Firdaus Mohammed Azmi,
“Designing Space Frame Race Car Chassis Structure Using Natural Frequencies Data from Ansys Mode Shape
Analysis”, International journal of information systems and engineering, April 2015

50
7 APPENDIX
7.1 ANSYS code commands lists
7.1.1 Macro
! ----------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------- --------------------------------------
!SUSPENSIONS DATA
! -------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------
*Create,data_suspensions,mac
!!!!!!REAR SUSPENSION !!!!!!
! > COORDINATES OF CHARACTERISTIC POINTS
! upper arm (a)
*set,a1x,-834.745 !#4
*set,a1y,348
*set,a1z,353.747-52
*set,a2x,-435.293 !#3
*set,a2y,378
*set,a2z,322.977-52
*set,a3x,-695.000 !#6
*set,a3y,512.000
*set,a3z,335-52
! lower arm (b)
*set,b1x,-834.745 !#2
*set,b1y,308
*set,b1z,125.747-52
*set,b2x,-435.293 !#1
*set,b2y,305.822
*set,b2z,104.813-52
*set,b3x,-690.000 !#7
*set,b3y,550.000
*set,b3z,105-52
! tie rod (c)
*set,c1x,-760.000 !#8
*set,c1y,524.000
*set,c1z,108.5-52
*set,c2x,-864.745 !#5
*set,c2y,308
*set,c2z,125.747-52
! push rod (d)
*set,d1x,-680.000 !#10
*set,d1y,525.000
*set,d1z,122-52
*set,d2x,-610 !#11
*set,d2y,390.000
*set,d2z,442-52
! upright (e)
*set,e1x,-695.000 !#6
*set,e1y,512.000
*set,e1z,335-52
*set,e2x,-690.000 !#7
*set,e2y,550.000
*set,e2z,105-52
*set,e3x,-760.000 !#8
*set,e3y,524.000
*set,e3z,108.5-52
*set,e4x,-700.000
!Contact road wheel #PC
*set,e4y,620.000
*set,e4z,0-52
*set,e5x,-700.000
! Center wheel #9
*set,e5y,620.000
*set,e5z,203.2-52
! rocker (f)
*set,f1x,-610.000
! with rod #11
*set,f1y,390.000
*set,f1z,442-52
*set,f2x,-585.000
! pivot #12
*set,f2y,335.000
*set,f2z,407-52
*set,f3x,-574.000
! with shock absorber #13
*set,f3y,300.000
*set,f3z,482-52
! shock absorber (g)
*set,g1x,-574.000
! with rocker #13
*set,g1y,300.000
*set,g1z,482-52
*set,g2x,-435.293
! with chassis #14
*set,g2y,30
*set,g2z,392.977-52
!!!!!!FRONT SUSPENSION !!!!!!
! > COORDINATES OF CHARACTERISTIC POINTS
! upper arm (h)
*set,h1x,559.247 !#4
*set,h1y,333
*set,h1z,312-52
*set,h2x,994.678 !#3
*set,h2y,303
*set,h2z,328.576-52
*set,h3x,845 !#6
*set,h3y,540
*set,h3z,302-52
! lower arm (i)
*set,i1x,994.678 !#1
*set,i1y,237.606
*set,i1z,178.576-52
*set,i2x,520 !#2
*set,i2y,248
*set,i2z,159.5-52
*set,i3x,862.000 !#7
*set,i3y,565.000
*set,i3z,144-52
! tie rod (l)
*set,l1x,934.353 !#8
*set,l1y,595.644
*set,l1z,192.500-52
*set,l2x,910.000 !#5
*set,l2y,225.000
*set,l2z,220.000-52
! pull rod (m)
*set,m1x,830.000 !#10
*set,m1y,500.000
*set,m1z,292-52
*set,m2x,810 !#11
*set,m2y,230
*set,m2z,134.000 - 52
! upright (n)
*set,n1x,845.000 !#6
*set,n1y,540.000
*set,n1z,302-52
*set,n2x,862.000 !#7
*set,n2y,565
*set,n2z,144-52
*set,n3x,934.353 !#8
*set,n3y,595.644
*set,n3z,192.500-52
*set,n4x,840.000
! Contact road wheel #PC
*set,n4y,635
*set,n4z,0-52
*set,n5x,840.000
! Center wheel #9
*set,n5y,635
*set,n5z,203.2-52
! rocker (o)
*set,o1x,810.000
! with rod #11
*set,o1y,230.000
*set,o1z,134-52
*set,o2x,850
! pivot #12
*set,o2y,212.000
*set,o2z,136-52
*set,o3x,837.000
! with shock absorber #13
*set,o3y,143.000
*set,o3z,108-52
! shock absorber (p)
*set,p1x,837.000
! with rocker #13
*set,p1y,143.000
*set,p1z,108-52
*set,p2x,528.547
! with chassis #14
*set,p2y,145
*set,p2z,108-52
*END

51
! ----------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------- --------------------------------------
!REFERENCE SYSTEMS
! -------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------- -----------------------
! RFM, origin, x-direction, Relative_frame_name, absolute_frame_name
*CREATE,RFM,mac
origin = arg1
x_direction = arg2
Relative_frame_ID = arg3
absolute_frame_ID = arg4
!relative
csys,0
k,1000,kx(origin)+50,ky(origin),kz(origin)
KWPLAN,1, origin, x_direction, 1000
CSWPLA, Relative_frame_ID, 0
!absolute
csys,0
k,1001,kx(x_direction),ky(x_direction),kz(origin)
csys,Relative_frame_ID
k,1002,0,50,0
KWPLAN,1, origin, 1001, 1002
CSWPLA, absolute_frame_ID, 0
kdele,1000,1002
csys,0
*END
! ----------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------- --------------------------------------
!JOINTS
! -------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------- -----------------------
!JOINT,Element_type, ID_section, 'joint_type(REVO,SPHE)', Relative_frame_ID, absolute_frame_ID, 'CM_1', 'CM_2'
!Element_type: MPC184 with keyopt selected for the relative joint
!ID_section : number IDentification
!joint_type(REVO,SPHE): revolute=REVO, spherical=SPHE , general=GENE, 3dof fix = LINK, 6dof fix = BEAM
!Relative_frame_ID, absolute_frame_ID : IDentification number of reference frame of node i and j of joint
!'CM_1', 'CM_2' : Component selected for coupling trought joint elements
*CREATE,JOINT,mac
Element_type = arg1
ID_section = arg2
joint_type = arg3
Relative_frame_ID = arg4
absolute_frame_ID = arg5
CM_1 = arg6
CM_2 = arg7
Pi = acos(-1)
CHI_min = -180*(Pi/180) ![RAD] z-axis rotation
CHI_max = +180*(Pi/180) ![RAD] z-axis rotation
x_min = -10 ! [mm] x-axis traslation
x_max = 10 ! [mm] x-axis traslation
*IF,joint_type, EQ, 'BEAM',THEN
CMSEL, s, CM_1, line
CMSEL, a, CM_2, line
nsll, s, 1
type, Element_type
EINTF
alls
*ELSEIF, joint_type, EQ, 'LINK'
nsll, s, 1

52
type, Element_type
EINTF
alls
*ELSEIF, joint_type, EQ, 'GENEZ'
SECTYPE, ID_section, JOINT, 'GENE'
SECJOINT, , Relative_frame_ID, absolute_frame_ID
SECJOINT,RDOF,1,2,3,6, ! constraints rot z
*ELSE
SECTYPE, ID_section, JOINT, joint_type
SECJOINT, , Relative_frame_name, absolute_frame_name
*IF, joint_type, EQ, 'REVO', THEN
!SECSTOP, 6, CHI_min, CHI_max
*ELSEIF, joint_type, EQ, 'PRIS'
!SECSTOP, 1, x_min, x_max
*ELSEIF, joint_type, EQ, 'GENE'
SECJOINT,RDOF,1,2,3,4, ! constraints rot x
*ENDIF
nsll, s, 1
type, Element_type
SECNUM, ID_section
EINTF
alls
*ENDIF
*END
! ----------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------- --------------------------------------
!WHEEL
! -------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------- -----------------------
!wheel,K_origin,ET_in,MP_in,R_in
*CREATE,wheel,mac
/COM,---------------------------------------------------------------------
/COM, inizio macro wheel
/com,---------------------------------------------------------------------
/Prep7
csys,0
*get,K_in,kp,0,num,max
*get,L_in,line,0,num,max
*get,A_in,area,0,num,max
*get,N_in,node,0,num,max
*get,Csys_in,CDSY,0,num,max
NUMSTR, kp, K_in
NUMSTR, Line, L_in
NUMSTR, area, A_in
NUMSTR, node, N_in
ET_in = arg2!6
MP_in = arg3!2
R_in = arg4!2
Xc = kx(arg1)!840
Yc = ky(arg1)!-635
Zc = kz(arg1)!151
rotz = 0
rotx = 0
roty = 0
! >>>>> MODEL PARAMETERS <<<<<<<<<<<<<<<<
Ri = 254/2 !Internal diameter = 10 pollici = 254 [mm]
Ro = 406.4/2 !External diameter = 16 pollici = 406.4 [mm]
w = 158 !Width = 6 [pollici] = 152.4 [mm]
wl = 208
wf = 176 !With [mm]
t =Ro-Ri
th= 10 !thickness [mm]
E_length_T = 5
/PREP7
clocal,Csys_in+111,0,Xc,Yc,Zc,rotz,rotx,roty ! wheel RFM
csys,Csys_in+111
! Elements definition<<<<<<<<<<<<<<
!Tire geometry
ET,ET_in+1,solid186
! Tire Gemetry
k,K_in+1,0,w/2-5,Ri
k,K_in+2,0,w/2,Ro-30
k,K_in+3,0,w/2,Ro
k,K_in+4,0,-w/2,Ro
k,K_in+5,0,-w/2,Ro-30
k,K_in+6,0,-w/2+5,Ri
l,K_in+1,K_in+2
*repeat,5,1,1
lfillt,L_in+1,L_in+2,50

53
lsscale,L_in+1,L_in+9,1,0,(1-(th/ky(K_in+1))),(1-(th/kz(K_in+1)))
l,K_in+1,K_in+6
lcsl,L_in+19,L_in+10
ldele,L_in+24,L_in+25
ldele,L_in+22
KBETW, K_in+10, K_in+11, K_in+27, dist, ky(K_in+10)-ky(K_in+20)
l,K_in+20,K_in+27
KBETW, K_in+11, K_in+10, K_in+28, dist, ky(K_in+10)-ky(K_in+20)
l,K_in+19,K_in+28
lcsl,L_in+21,L_in+3
l,K_in+21,K_in+14
l,K_in+18,K_in+7
lcomb,L_in+13,L_in+18
lcomb,L_in+9,L_in+4
lcomb,L_in+4,L_in+8
lcomb,L_in+4,L_in+3
lcomb,L_in+6,L_in+2
lcomb,L_in+7,L_in+2
!Areas
al,L_in+5,L_in+13,L_in+10,L_in+24
!sizing
ndiv_T=1
lesize,L_in+20,,,ndiv_T
lesize,L_in+11,,,ndiv_T*2
k,K_in+100,0,0,0
!Keypoints defining the axis about which the line pattern is to be rotated
k,K_in+110,0,10,0
division=16
VROTAT,A_in+1,A_in+2,A_in+3,A_in+4,A_in+5,,K_in+100,K_in+110,360,divisio
n
clocal,Csys_in+100,CYLIN,0,0,0,0,90,0
angle=360/division
*do,f,1,16,1
alls
lsel,s,loc,y,f*angle-15,f*angle-10
lesize,all,,,ndiv_T*3
*enddo
alls
csys,Csys_in+111
! meshing Tire<<<
/COM,---------------------------------------------------------------------
/COM, MESHING TYRE
/com,---------------------------------------------------------------------
TYPE,ET_in+1
MAT,MP_in+1
asel,s,area,,A_in+1,A_in+336
vsla,s,1
MSHKEY,1 !mapped mesh
MSHAPE,0,3D !3D mesh with hexahedral elements
VMESH,all
alls
!Fluid <<<<<<<
!GAS
ET,ET_in+2,242 ! Hydrostatic fluid element
KEYOPT,ET_in+2,5,1 ! Fluid mass calculated based on the volume of the fluid
! element
R,R_in+2,0.101 ! Initial air pressure (atmospheric) = 0.10156 N/mm^2
n,N_in+5000,0,0,0 ! Define pressure node
nsel,s,node,,N_in+5000 !save name of pressure node
CM,press_node%N_in%,node
alls
type,ET_in+2
mat,MP_in+2 ! Gas material model used to model the inside fluid
real,R_in+2
Csys,Csys_in+100
asel,s,loc,x,ro-18,ri
asel,r,loc,z,-w/2+10,w/2-10
cm,spalla,Area
asel,s,loc,x,ro-15,ri
asel,r,loc,z,-w/2+18,w/2-18
cm,interno,Area
cmsel,s,spalla
cmsel,a,interno
nsla,s,1
esln
esurf,N_in+5000
inc=3.75
*DO,g,0,360-(inc),inc
/COM,---------------------------------------------------------------------
/COM, cycle %g%
/com,---------------------------------------------------------------------
alls
csys,Csys_in+100
lsel,s,loc,x,ri-1,ri+1
lsel,r,loc,z,-w/2+10,w/2-10
nsll,s,1
csys,Csys_in+111
clocal,Csys_in+200,CART,0,0,0,0,0,g
csys,Csys_in+200
nsel,r,loc,x,0,10
nsel,r,loc,z,0,10000
nsel,r,loc,x,-0.5,+0.5

54
nsel,r,loc,y,-65.016-0.5,-65.016+0.5
*get,n32,node,0,num,max
alls
csys,Csys_in+100
nsll,s,1
csys,Csys_in+200
nsel,r,loc,x,0,10
nsel,r,loc,x,-0.5,+0.5
nsel,r,loc,y,65.016-0.5,65.016+0.5
alls
csys,Csys_in+100
nsll,s,1
csys,Csys_in+200
nsel,r,loc,x,0,10
nsel,r,loc,x,8.3062-0.5, 8.3062+0.5
nsel,r,loc,y,-65.016-0.5,-65.016+0.5
/com, sto eseguendo il ciclo, stampo il nodo della var n33: %n33%
alls
csys,Csys_in+100
nsll,s,1
csys,Csys_in+200
nsel,r,loc,x,0,10
nsel,r,loc,x,8.3062-0.5, 8.3062+0.5
nsel,r,loc,y,65.016-0.5,65.016+0.5
e,n32,n33,n252,n251
emore,N_in+5000
*enddo
alls
csys,Csys_in+111
!RIM
ET,ET_in+4,CONTA175 ! Select contact element
ET,ET_in+5,TARGE170 ! Select target element
KEYOPT,ET_in+4,2,2 ! Use MPC constraints
KEYOPT,ET_in+4,4,0 ! Use rigid surface constraint
KEYOPT,ET_in+4,12,5 ! Always bonded
r,R_in+4,Ri
n,N_in+6000,0,0,0 ! Make node at axle (pilot node)
! Define target element at pilot node
tshap,pilot
type,ET_in+5
*get,Real_in,RCON,0,num,max
real,real_in+1
e,N_in+6000
! Contact element definition
type,ET_in+4
real,real_in+1
! Select contact surface (rim nodes)
csys,Csys_in+100
lsel,s,loc,x,ri,0
nsll,s,1
esurf ! Generate contact element
allsel,all
csys,Csys_in+111
lsel,s,line,,L_in+226
nsll,s,1
alls
csys,0
/COM,---------------------------------------------------------------------
/COM, contact surface
/com,---------------------------------------------------------------------
!CONTACT SURFACE: TIRE
ET,ET_in+6,CONTA174
KEYOPT,ET_in+6,7,4
!transient dynamic analysis with automatic adjustment of time increment
type,ET_in+6
real,real_in+2
csys,Csys_in+100
asel,s,loc,x,ro-0.1,ro+0.1
asel,r,loc,z,-w/2-10,+w/2+10
cm,road_contact,area
alls
asel,s,loc,x,ro-10,ro+0.1
asel,r,loc,z,-w/2,(-w/2)+10
cm,side_wall_DX,area
alls
asel,s,loc,x,ro-10,ro+0.1
asel,r,loc,z,w/2,(w/2)-10
cm,side_wall_sX,area
alls
CMSEL,s,road_contact
CMSEL,a,side_wall_DX
CMSEL,a,side_wall_sX
NSLA,S,1
esurf
allsel
/COM,---------------------------------------------------------------------
/COM, End macro wheel
/com,---------------------------------------------------------------------
*END

55
7.1.2 Accelerations data
skidpad_x_acc.txt
time [s] X_acceleration [mm/𝑠2
]
0.000 10853.86467536
0.113 11290.64587255
0.152 11142.01124718
0.182 11256.21503532
0.208 11164.77793860
0.230 11231.04513666
0.250 11160.22399055
0.268 11209.38728334
0.286 11153.31225981
0.302 11190.34777988
0.317 11145.55853917
0.332 11173.48534443
0.345 11137.50790644
0.359 11158.45557412
0.372 11129.38955372
0.384 11144.93691318
0.396 11121.30014199
0.408 11132.65590701
0.419 11113.29653511
0.430 11121.40624739
.
.
.
19.793 8716.47948364
19.795 8705.86835152
19.798 8695.06509743
19.800 8684.27963939
19.803 8673.18809232
19.805 8662.17898930
19.808 8650.64917139
19.810 8639.37015037
19.813 8627.11899405
19.815 8615.58357723
19.818 8601.96767479
19.820 8590.50360453
19.823 8574.24658443
19.825 8497.44139832
19.828 8327.51085102
19.830 8069.97647190
19.832 7728.00762996
19.835 7306.28744340
19.837 6816.51251896
19.840 6283.48709243
19.842 5751.04188568
skidpad_y_acc.txt
time [s] Y_acceleration [mm/𝑠2
]
0.000 -8.45396832
0.113 114.78073321
0.152 163.44094288
0.182 198.64082999
0.208 213.57004713
0.230 244.84854001
0.250 270.66374590
0.268 311.31895292
0.286 346.04413335
0.302 389.33813931
0.317 425.82272010
0.332 466.80748812
0.345 501.75758707
0.359 539.30894418
0.372 572.35533704
0.384 607.17897527
0.396 638.93504694
0.408 671.99398011
0.419 702.98699208
0.430 734.86093402
.
.
.
19.793 -379.43135094
19.795 -470.05401972
19.798 -559.91669145
19.800 -649.00544393
19.803 -737.29664938
19.805 -824.78217029
19.808 -911.43953054
19.810 -997.26655446
19.813 -1082.24094590
19.815 -1166.36503573
19.818 -1249.61778477
19.820 -1331.99609269
19.823 -1413.52538488
19.825 -1494.58205559
19.828 -1575.64937673
19.830 -1656.92116214
19.832 -1738.49697423
19.835 -1820.34303129
19.837 -1902.35823883
19.840 -1984.42599312
19.842 -2066.49863576

56
7.1.3 Basic model
! Definition element types
ET,1,BEAM189
ET,2,MPC184,1 ! Rigid beam
ET,3,COMBIN14,,,0 ! 3D spring
ET,4,MPC184,6,,,1 ! Revolute JOINT z-axis
ET,5,MPC184,15 ! sferical JOINT
ET,6,MPC184,10 ! Translational JOINT element
ET,7,MASS21,,,0 ! 3-D mass with rotary inertia
ET,8,MPC184,16 ! generical JOINT
ET,9,MPC184,0 ! rigid link
ET,10,COMBIN14,,2 ! unidirection 1D - y spring
ET,11,COMBIN39,,,3, ! unidirection 1D - Z spring
!real costant definition
!Front shock absorber
R,1,K_front,c_front! K1 [N/mm], D1 [N.s/mm]
!Rear shock absorber
R,2,K_rear,c_rear ! K2 [N/mm], D2 [N.s/mm]
!Battery pack
R,3,W*(71.135*10**(-3)),W*(71.135*10**(-3)),W*(71.135*10**(-3)),W*(4415609.399*10**(-3)),W*(4543320.659*10**(-3)),W*(597338.389*10**(-3))
! MASSX[Mg], MASSY[Mg], MASSZ[Mg], IXX[Mg mm^2], IYY[Mg mm^2], IZZ[Mg mm^2]
!Emrax
R,4,W*(9.4*10**(-3)),W*(9.4*10**(-3)),W*(9.4*10**(-3)),W*(43761.612*10**(-3)),W*(30102.130*10**(-3)),W*(30079.592*10**(-3))
!Inverter
R,5,W*(8.929*10**(-3)),W*(8.929*10**(-3)),W*(8.929*10**(-3)),W*(49968.797*10**(-3)),W*(88303.976*10**(-3)),W*(117058.036*10**(-3))
!tire y direction spring
R,6,ky_tire, ! K [N/mm]
!tire front z direction spring
R,8,-14.0,-5135.21,-11.28,-4018.15,-7.53,-2325.36
RMORE,-3.78,-847.688,-2.53,-434.01,-1.28,-211.55
RMORE,0.0,0.0,1.21,170.87,2.46,361.23
RMORE,3.71,504.87,3.72,504.87,10,1000
!tire rear z direction spring
R,9,-10.8,-4448.51,-8.08,-3331.45,-4.33,-1638.66
RMORE,-3.08,-1101.38,-1.83,-581.09,-0.58,-160.98
RMORE,0.0,0.0,1.91,475.14,5.66,1047
RMORE,6.91,1191.57,6.92,1191.57,10,2000
!Definition material propeties
!steel
MP,EX,1,E_Young
MP,PRXY,1,ni
MP,dens,1,Density
!Carbon
MPTEMP,,,,,,,,
MPTEMP,1,0
MPDATA,EX,2,,EX_Young_C
MPDATA,EY,2,,EY_Young_C
MPDATA,EZ,2,,EZ_Young_C
MPDATA,PRXY,2,,ni_C
MPDATA,PRYZ,2,,ni_C
MPDATA,PRXZ,2,,ni_C

57
! -------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------
!SUSPENSION GEOMETRY
! -------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------- -----------------------
! Rear suspension
! Keypoints definition
! upper arm
k,301,a1x,a1y,a1z
k,302,a2x,a2y,a2z
k,303,a3x,a3y,a3z
! lower arm
k,304,b1x,b1y,b1z
k,305,b2x,b2y,b2z
k,306,b3x,b3y,b3z
! tie rod
k,307,c1x,c1y,c1z
k,308,c2x,c2y,c2z
! push rod
k,314,d1x,d1y,d1z
k,315,d2x,d2y,d2z
! upright
k,316,e1x,e1y,e1z
k,317,e2x,e2y,e2z
k,318,e3x,e3y,e3z
k,319,e4x,e4y,e4z
k,320,e5x,e5y,e5z
! rocker
k,309,f1x,f1y,f1z
k,310,f2x,f2y,f2z
k,311,f3x,f3y,f3z
! shock absorber
k,312,g1x,g1y,g1z
k,313,g2x,g2y,g2z
! Lines definition
! upper arm
l,301,303
l,302,303
! lower arm
l,304,306
l,305,306
! tie rod
l,308,307
! push rod
l,315,314
! rocker
l,309,310
l,310,311
l,311,309
! shock absorber
l,312,313
! upright
l,316,317
l,317,318
l,318,316
l,316,320
l,317,320
l,318,320
l,320,319
!front suspension
!Keypoints definition
! upper arm
k,321,h1x,h1y,h1z
k,322,h2x,h2y,h2z
k,323,h3x,h3y,h3z
! lower arm
k,324,i1x,i1y,i1z
k,325,i2x,i2y,i2z
k,326,i3x,i3y,i3z
! tie rod
k,327,l1x,l1y,l1z
k,328,l2x,l2y,l2z
! push rod
k,334,m1x,m1y,m1z
k,335,m2x,m2y,m2z
! upright
k,336,n1x,n1y,n1z
k,337,n2x,n2y,n2z
k,338,n3x,n3y,n3z
k,339,n4x,n4y,n4z
k,340,n5x,n5y,n5z
! rocker
k,329,o1x,o1y,o1z
k,330,o2x,o2y,o2z
k,331,o3x,o3y,o3z
! shock absorber
k,332,p1x,p1y,p1z
k,333,p2x,p2y,p2z
!Lines definition
! upper arm
l,321,323
l,322,323
! lower arm
l,324,326
l,325,326
! tie rod
l,328,327
! push rod
l,335,334
! rocker
l,329,330
l,330,331
l,331,329
! shock absorber
l,332,333
! upright
l,336,337
l,337,338
l,338,336
l,336,340
l,337,340
l,338,340
l,340,339
!overlap keypoints
!rear suspension
ksel,s,kp,,301,302
ksel,a,kp,,304,305
ksel,a,kp,,308
ksel,a,kp,,314
ksel,a,kp,,310
ksel,a,kp,,313
!front suspension
ksel,a,kp,,321,322
ksel,a,kp,,324,325
ksel,a,kp,,328
ksel,a,kp,,334
ksel,a,kp,,330
ksel,a,kp,,333
*get,length,kp,0,count
*do,i,1,length
*get,n,kp,0,num,min
k,340+i,kx(n),ky(n),kz(n)
ksel,u,kp,,n
*enddo
alls

58
! ----------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------- --------------------------------------
!CONNECTIONS
! -------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------- -----------------------
!C rear left attachments!!!!!!!!!!!!!!!!!!!!!!!!!
!C1
k,357,-435.293,346.078,288.464
k,358,-435.293,335.154,253.608
!C2
k,359,-435.293,277.772,70.514
k,360,-435.293,266.807,35.527
!C3
k,361,-834.745,317.792,319.028
k,362,-834.745,311.777,284.381
!c4
k,363,-834.745,278.341,91.789
k,364,-834.745,272.117,55.942
! rear rocker support
k,365,-568.138,340.023,311.210
k,366,-605.996,337.180,314.127
!left shock assorb attachment
k,367,-435.293,47.336,300.977
k,368,-435.293,14.391,300.977
!Lines rear attachments
l,357,342
l,358,342
l,359,344
l,360,344
l,363,343
l,364,343
l,345,364
l,345,363
l,341,361
l,362,341
l,348,306
l,346,365
l,346,366
l,367,347
l,368,347
!C front left attachments!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!!
!C1
k,369,994.678,257.792,259.050
k,370,994.678,280,294.099
!C2
k,371,994.678,206.871,144.232
k,372,994.678,206.871,108.542
!C3
k,373,525.726,214.591,124.803
k,374,525.726,214.591,90.500
!c4
k,375,552.872,283.759,242.386
k,376,560,300,277.593
! rear rocker support
k,377,867.993,196.046,112.152
k,378,834.295,196.428,110.975
!left shock assorb attachment
k,379,520,129.479,100
k,380,520,161.804,100
!Lines rear attachments
l,64,370
l,370,350
l,369,350
l,48,372
l,372,351
l,371,351
l,374,39
l,374,352
l,373,352
l,376,22
l,376,349
l,349,375
l,356,323
l,377,354
l,378,354
l,379,355
l,380,355
! >>>> SYMMETRY <<<<
NUMSTR,kp,381 ! initial keypoint number mirror
LSYMM,y,84,149,1
! keypoints MERGE front left suspension to solve problem due to simmetry
! C_FL_FD
ksel,s,,,50
ksel,a,,,445
NUMMRG,kp
allsel
! C_FL_RD
ksel,s,,,40
ksel,a,,,450
NUMMRG,kp
allsel
! C_FL_RU
ksel,s,,,24
ksel,a,,,454
NUMMRG,kp
allsel
! C_FL_FU
ksel,s,,,74
ksel,a,,,441
NUMMRG,kp
allsel

59
! ----------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------- --------------------------------------
!WHEELS
! -------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------- -----------------------
CIRCLE,340,203.2,419
CIRCLE,419,203.2,340
CIRCLE,320,203.2,399
CIRCLE,399,203.2,320
!divide line itersection
BTOL, 1
!front right
lcsl,31,201
lcsl,232,204
lcsl,46,210
lcsl,235,207
lcsl,14,215
lcsl,235,214
lcsl,48,212
lcsl,235,213
!front left
lcsl,26,135
lcsl,235,138
lcsl,45,144
lcsl,243,141
lcsl,14,148
lcsl,243,149
lcsl,47,147
lcsl,247,146
!rear right
lcsl,62,185
lcsl,247,184
lcsl,249,186
lcsl,247,187
lcsl,60,192
lcsl,247,193
lcsl,60,188
lcsl,247,190
lcsl,55,196
lcsl,257,195
lcsl,52,198
lcsl,259,197
!rear left
lcsl,57,119
lcsl,261,118
lcsl,259,120
lcsl,261,121
lcsl,59,126
lcsl,261,127
lcsl,59,123
lcsl,267,122
lcsl,53,130
lcsl,269,129
lcsl,257,132
lcsl,269,131
! -------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------
!STEERING
! -------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------
k,480,910,0,220-52
k,481,kx(328),ky(328),kz(328) ! Overlapped left line point
k,482,kx(407),ky(407),kz(407) ! Overlapped right line point
k,483,kx(328),ky(328)-50,kz(328) ! left point steering gear
k,484,kx(407),ky(407)+50,kz(407) ! right point steering gear
k,485,kx(483),ky(483),kz(483) ! Overlapped left point steering gear
k,486,kx(484),ky(484),kz(484) ! Overlapped right point steering gear
l,480,485
l,480,486
l,485,481
l,486,482
!C left steering
l,48,483
l,483,39
!C right steering
l,40,484
l,484,50

Structural dynamic analysis of a Formula SAE vehicle

Structural dynamic analysis of a Formula SAE vehicle

Recommended

Recommended

More Related Content

What's hot

What's hot (20)

Similar to Structural dynamic analysis of a Formula SAE vehicle

Similar to Structural dynamic analysis of a Formula SAE vehicle (20)

Recently uploaded

Recently uploaded (20)

Structural dynamic analysis of a Formula SAE vehicle