O os-02 vibration-reduction_and_mahindra_navistar


Published on

Published in: Technology, Business
1 Like
  • Be the first to comment

No Downloads
Total views
On SlideShare
From Embeds
Number of Embeds
Embeds 0
No embeds

No notes for slide

O os-02 vibration-reduction_and_mahindra_navistar

  1. 1. Vibration Reduction and Optimization of Wheel Arch Assembly Gaurav Upadhyay Chetan Raval Pranesh Mahindrakar Sr Analyst, CAE Sr. Manager, CAE Asst. Manager, NVHMahindra Engineering Services Ltd. Mahindra Navistar Automotive Ltd. Mahindra Navistar Automotive Ltd. Pune, India Pune, India Pune, India Keywords: Wheel Arch, Vibration, Frequency Response AbstractThe vibrational response of structure is very important factor in the design of automobile components because it also gives rise toalternating stresses and can limit the life of component. Finite Element Analysis (FEA) based predictive tools play very crucial role tounderstand the fundamental vibration characteristics of the structure and to device design modifications to attenuate the vibration andextend 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 archand mudguard assembly due to engine excitation at idling. First the possible modes of vibrations were analyzed using Eigen frequencyanalysis. Data acquisition was also carried out using piezoelectric transducers at select locations on the subject wheel arch assemblywhile engine was put at idling. Excitation information at wheel arch base was used further for frequency response analysis usingRADIOSS solver to predict the vibration response of the wheel arch assembly. The predicted vibration response co-related quite wellwith test measured vibrations. Subsequently durability analysis of wheel arch assembly and parts was carried out to predict the life ofassembly. Since the coincidence of modes was cause behind the excessive vibrations, design modifications were necessary to shiftthe 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, andother road debris. In Heavy Commercial Vehicle (HCV), the wheel arc is mostly overhung from inboardchassis frame section with support from one or two pipes. Because of wheel arc’s cantilever conditionespecially near engine mount location on frame, it is quite vulnerable to vibrations from engine as well asroad excitations. As wheel arc is also exterior styling component, visible vibrations in it lead to badperception about the vehicle quality.This paper present interesting case of wheel arc vibrations surfaced due to lowering of the engine’s idlerpm. It was logical that wheel arc frequency must be shifted away from engine idle frequency. But feasibleincrease in strength and cost prohibited increase in the wheel arc frequency over the idle range. On theother hand lowering of wheel arc frequency was precarious due to low range road excitation which wouldcause durability failures. So different design iterations were used to strike the balance between twodemands and park the natural frequency of wheel arc assembly at right location.Simulation Driven Innovation 1
  2. 2. MethodologyThe methodology as described in Figure 1 was used to tackle the engine induced vibration problem. Figure 1: MethodologyFE 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 weremodeled using Rigid (RBE2) elements. The pump and mud flap masses were represented as lumpedmasses located at the CG points and connected to the bolted locations by interpolation elements (seeFigure 2). The masses of individual parts and whole assembly were carefully cross checked for goodaccuracy of frequency results. Figure 2: Wheel Arch AssemblyBoundary 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 applyingzero displacement at concerned nodes. These boundary conditions were used for both Modal as well asFrequency response analysis.Simulation Driven Innovation 2
  3. 3. Figure 3: Boundary ConditionAnalysis and Test Methodology:Initially modal analysis was carried out to estimate the natural frequencies of the system. First 6 modeswere extracted in this analysis.Acceleration were measured on the base chassis frame where wheel arch assembly is mounted. Sensorlocations on plastic wheel arch were chosen such that maximum sensitivity was observed (Figure 4). All themeasurements were taken when vehicle was in idling condition.The measured acceleration signals on the base chassis frame locations were in turn used for the FrequencyResponse analysis in Radioss. Figure 4: Accelerometers Mounting LocationSimulation Driven Innovation 3
  4. 4. Results & Discussion:Base Design: Vibration MeasurementsThe root cause analysis of excessive wheel arc vibration suggested the change in engine excitationfrequency and change in engine mounts isolation. Subsequently, the physical measurements confirmed thatthere are very high amplitude vibrations in rage of 4.5g in the wheel arc assembly (Figure 5). Themeasurements also cleared that engine mount isolation is effective at the changed idle frequency also. Figure 5: Vibration Response at Chassis & Wheel ArchBase Design: Modal AnalysisPreliminary modal analysis yielded few local and global modes of vibrations due to mud flap and plasticwheel arc flexibility. However, the global mode where whole wheel arc assembly was found vibrating wasalso close to the engine idle frequency. The upper support tube showed maximum flexing (Figure 6). Thusinitial modal analysis indicated the responsible mode for high idling vibrations and possible part forimprovement. Figure 6: Modal Analysis ResultSimulation Driven Innovation 4
  5. 5. Base Design: Frequency Response AnalysisThe measured acceleration signals on the base chassis frame locations were used for frequency responseanalysis (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 33Hz 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 archTest CorrelationThe results of frequency analysis and experimental analysis of base design, as shown in Figure 10, werecorrelated well with frequency difference of 1 Hz higher in CAE indicating that the finite element model wasvalid for the further analysis. The high amplitude responses as shown in Figure 10, and the mode shapefrom the modal analysis results as shown in Figure 6, predict the natural frequency of wheel arch assemblywhich is responsible for the increased vibration levels at mudguard. To reduce vibration level in wheel archassembly, changing the natural frequency was the best solution for this.Simulation Driven Innovation 5
  6. 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), soas to shift the natural frequency below the excitation range. stThe 1 design proposal, upper tube outer diameter increased to 50 mm from 38 mm. It has naturalfrequency of 34 Hz, which results same vibration levels as base design in frequency response analysis. ndIn case of 2 design proposal, upper tube outer diameter reduced to 32 mm from 38 mm, resulting innatural frequency of 29 Hz and vibration levels less than base design but not up to the expectation, infrequency response analysis. rdThe 3 Design proposal has natural frequency below the excitation frequency range, resulting in significantreduction 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 IterationsSimulation Driven Innovation 6
  7. 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. ACKNOWLEDGEMENTWe would like to thank Mr.Shekar Paranjape, General Manager, MNAL for allowing us to publish this paper.Simulation Driven Innovation 7