1) The document describes using finite element analysis to analyze and reduce excessive vibrations in a wheel arch assembly caused by engine idling. 2) Modal analysis identified a global mode of the wheel arch assembly vibrating at a frequency close to engine idle. Frequency response analysis confirmed this mode led to high vibration levels. 3) Different design iterations were analyzed to shift the natural frequency of this mode below the engine idle range. The final design prototyped showed significantly reduced vibrations.

1. Vibration Reduction and Optimization of Wheel Arch Assembly
Gaurav Upadhyay Chetan Raval Pranesh Mahindrakar
Sr Analyst, CAE Sr. Manager, CAE Asst. Manager, NVH
Mahindra Engineering Services Ltd. Mahindra Navistar Automotive Ltd. Mahindra Navistar Automotive Ltd.
Pune, India Pune, India Pune, India
Keywords: Wheel Arch, Vibration, Frequency Response
Abstract
The vibrational response of structure is very important factor in the design of automobile components because it also gives rise to
alternating stresses and can limit the life of component. Finite Element Analysis (FEA) based predictive tools play very crucial role to
understand the fundamental vibration characteristics of the structure and to device design modifications to attenuate the vibration and
extend the life of component.
This paper demonstrates the use of RADIOSS solver to trouble shoot the problem of excessive vibrations seen in the front wheel arch
and mudguard assembly due to engine excitation at idling. First the possible modes of vibrations were analyzed using Eigen frequency
analysis. Data acquisition was also carried out using piezoelectric transducers at select locations on the subject wheel arch assembly
while engine was put at idling. Excitation information at wheel arch base was used further for frequency response analysis using
RADIOSS solver to predict the vibration response of the wheel arch assembly. The predicted vibration response co-related quite well
with test measured vibrations. Subsequently durability analysis of wheel arch assembly and parts was carried out to predict the life of
assembly. Since the coincidence of modes was cause behind the excessive vibrations, design modifications were necessary to shift
the modes and attenuate the vibrations. So, different design iterations were used to find the appropriate design solution.
Introduction:
The wheel arch is a generally made with plastic material and used to contain the splashing water, mud, and
other road debris. In Heavy Commercial Vehicle (HCV), the wheel arc is mostly overhung from inboard
chassis frame section with support from one or two pipes. Because of wheel arc’s cantilever condition
especially near engine mount location on frame, it is quite vulnerable to vibrations from engine as well as
road excitations. As wheel arc is also exterior styling component, visible vibrations in it lead to bad
perception about the vehicle quality.
This paper present interesting case of wheel arc vibrations surfaced due to lowering of the engine’s idle
rpm. It was logical that wheel arc frequency must be shifted away from engine idle frequency. But feasible
increase in strength and cost prohibited increase in the wheel arc frequency over the idle range. On the
other hand lowering of wheel arc frequency was precarious due to low range road excitation which would
cause durability failures. So different design iterations were used to strike the balance between two
demands and park the natural frequency of wheel arc assembly at right location.
Simulation Driven Innovation 1

2. Methodology
The methodology as described in Figure 1 was used to tackle the engine induced vibration problem.
Figure 1: Methodology
FE Modeling:
The wheel arc assembly and frame cut portion where it is mounted was considered sufficient for simulation.
The plastic wheel arch and supporting tubes assembly was modeled using shell elements. The welds were
modeled using Rigid (RBE2) elements. The pump and mud flap masses were represented as lumped
masses located at the CG points and connected to the bolted locations by interpolation elements (see
Figure 2). The masses of individual parts and whole assembly were carefully cross checked for good
accuracy of frequency results.
Figure 2: Wheel Arch Assembly
Boundary Conditions:
This particular analysis was carried out to predict and reduce the engine induced vibration, the suspension
(road tire interactions) was not considered. Hence long member of chassis were fixed at end by applying
zero displacement at concerned nodes. These boundary conditions were used for both Modal as well as
Frequency response analysis.
Simulation Driven Innovation 2

3. Figure 3: Boundary Condition
Analysis and Test Methodology:
Initially modal analysis was carried out to estimate the natural frequencies of the system. First 6 modes
were extracted in this analysis.
Acceleration were measured on the base chassis frame where wheel arch assembly is mounted. Sensor
locations on plastic wheel arch were chosen such that maximum sensitivity was observed (Figure 4). All the
measurements were taken when vehicle was in idling condition.
The measured acceleration signals on the base chassis frame locations were in turn used for the Frequency
Response analysis in Radioss.
Figure 4: Accelerometers Mounting Location
Simulation Driven Innovation 3

4. Results & Discussion:
Base Design: Vibration Measurements
The root cause analysis of excessive wheel arc vibration suggested the change in engine excitation
frequency and change in engine mounts isolation. Subsequently, the physical measurements confirmed that
there are very high amplitude vibrations in rage of 4.5g in the wheel arc assembly (Figure 5). The
measurements also cleared that engine mount isolation is effective at the changed idle frequency also.
Figure 5: Vibration Response at Chassis & Wheel Arch
Base Design: Modal Analysis
Preliminary modal analysis yielded few local and global modes of vibrations due to mud flap and plastic
wheel arc flexibility. However, the global mode where whole wheel arc assembly was found vibrating was
also close to the engine idle frequency. The upper support tube showed maximum flexing (Figure 6). Thus
initial modal analysis indicated the responsible mode for high idling vibrations and possible part for
improvement.
Figure 6: Modal Analysis Result
Simulation Driven Innovation 4

5. Base Design: Frequency Response Analysis
The measured acceleration signals on the base chassis frame locations were used for frequency response
analysis (Figure 8). Response was taken at same location as that of experimental test (Figure 7).
Interpretation from result of frequency response analysis was that global mode of wheel arc assembly at 33
Hz get excited to very high levels of vibrations (Figure 9) which is 10 times higher than base excitation.
Figure 7:Direct Frequency Response Analysis
Figure 8: Excitation Signal at Chassis Figure 9: Response at Wheel arch
Test Correlation
The results of frequency analysis and experimental analysis of base design, as shown in Figure 10, were
correlated well with frequency difference of 1 Hz higher in CAE indicating that the finite element model was
valid for the further analysis. The high amplitude responses as shown in Figure 10, and the mode shape
from the modal analysis results as shown in Figure 6, predict the natural frequency of wheel arch assembly
which is responsible for the increased vibration levels at mudguard. To reduce vibration level in wheel arch
assembly, changing the natural frequency was the best solution for this.
Simulation Driven Innovation 5

6. Figure 10: Correlation between Experimental and CAE of Frequency Response (Base Design)
Design Improvements:
Different design iterations (see Table 1), were analyzed as per the methodology flowchart (see Figure 1), so
as to shift the natural frequency below the excitation range.
st
The 1 design proposal, upper tube outer diameter increased to 50 mm from 38 mm. It has natural
frequency of 34 Hz, which results same vibration levels as base design in frequency response analysis.
nd
In case of 2 design proposal, upper tube outer diameter reduced to 32 mm from 38 mm, resulting in
natural frequency of 29 Hz and vibration levels less than base design but not up to the expectation, in
frequency response analysis.
rd
The 3 Design proposal has natural frequency below the excitation frequency range, resulting in significant
reduction in vibration levels using frequency response analysis.
The finalized design was prototyped and tested on vehicle in idling condition, resulting in low vibration level
(see Figure 11).
Upper Tube Outer Diameter
Iterations Frequency (Hz)
(mm)
Baseline 38 32.5
Design 1 50 34
Design 2 32 29
Design 3 25 27
Table 1: Design Iterations
Simulation Driven Innovation 6

7. Figure 11: Frequency response of Baseline and Design Iteration 3 (Experimental and CAE)
Conclusion:
1. Using FEA based Eigen frequency and frequency response analysis techniques, the vibration
characteristic of wheel arc can be faithfully replicated as observed in the physical test.
2. Multiple design proposals could be evaluated in virtual environment to arrive at best and optimum
design solution. The best design proposal showed reduction in vibration level by 93%. Physical test
on final design reconfirmed simulation results and satisfactory performance of the final design.
ACKNOWLEDGEMENT
We would like to thank Mr.Shekar Paranjape, General Manager, MNAL for allowing us to publish this paper.
Simulation Driven Innovation 7