FE Modeling and Analysis of a Human powered/electric Tricycle chassis

Transcription

1 FE Modeling and Analysis of a Human powered/electric Tricycle chassis Sahil Kakria B.Tech, Mechanical Engg UCOE, Punjabi University Patiala, Punjab kakria.sahil@gmail.com Abbreviations: SAE- Society of Automotive Engineers CAD- Computer Aided Design FEA- Finite Element Analysis DOF- Degrees of Freedom CONM- Concentrated Mass NIS- Northern India Section CAE- Computer Aided Engineering HM- HyperMesh SPC- Single Point Constraint CG- Center of Gravity Keywords: Tricycle, FEA, HyperMesh, Optistruct Abstract The paper describes the study carried out on a Tricycle vehicle required to be designed for SAE NIS EFFICYCLE virtual design event. It describes the role of virtual simulation tools in design stage of the Tricycle vehicle. The CAD model of the Tricycle was created using Pro-E software. The chassis structure was imported in ALTAIR HYPERMESH where the Finite Element model was prepared incorporating different boundary conditions (loads/constraints). The model consists of CONM elements for representing concentrated masses (drivers and payload) which are connected using 1-D elements to main structure. The main structure consists of components made of shell elements (2D elements) connected by suitable arc welds. The FE analysis of the chassis was performed using ALTAIR OPTISTRUCT. Firstly, the model was checked by performing the normal modes analysis. The six rigid body modes showed proper connectivity in the model. Subsequently, the normal modes of vibration were visualized to observe the vibration behavior of chassis. The shared load analysis on the 3 wheels was carried out by calculating the CG of the complete structure using Hypermesh. Then the strength analysis of the chassis was performed under static load conditions. Design modifications were carried out in the structure where the stresses/displacements were found higher than acceptable limits. Introduction With a significant increase in pollution due to the use of automobile vehicles, there is a need of an alternate resource which will be helpful in transforming the way people travel for a better, greener tomorrow. The electric tricycle has been designed keeping in mind not only the efficiency part of a vehicle but it also serves as the best alternative to the present day fossil fuel run vehicles. The simultaneous pedal drive mechanism reduces the pedaling cadence required by both the front and the pillion rider, making their touring ride very easy. With the onset of the increasing energy cost, diminished resources, the demand of human powered/electric vehicle will increase in the future. Objective The objective of this project was to design a Tricycle vehicle for participation in SAE NIS EFFICYCLE Go- Green Virtual Design Challenge. The vehicle was designed using computer-aided modeling and simulation, resulting in a safe, high-performance vehicle, with light weight and high strength. The vehicle was designed comprehensively satisfying both the design goals and manufacturing constraints. 1

2 Process Methodology The process methodology followed for the project has been explained below in Fig. 1: CAD Design CAE Geometry cleanup and FE model Mesh generation Loads and Boundary conditions Iterations Solving Post-Processing Final Model Figure 1: Process Methodology CAD Modeling- The detailed design was prepared to meet the SAE rules and regulations with special considerations given to safety of the occupants, ease of manufacturing, cost, quality, weight, and overall attractiveness. The vehicle is human as well as electric powered and has carrier at the back for storage purpose. The design modeled using Pro-E software is shown below in Fig. 2: Figure 2: CAD Model of the Tricycle FE Model Setup: Frame being an integral and primary component of the structure was taken up for analysis purpose. The design model was analyzed using Altair s Hypermesh software (for Pre-processing) in which the finite element model was prepared to discretize the structure. Hypermesh software was chosen because 2

3 it is a high-performance finite element pre and post-processor for major finite element solvers, allowing engineers to analyze design conditions in a highly interactive and visual environment. A good quality criteria of the mesh as shown in Fig. 3 was ensured while meshing the structure. Figure 3: FE model quality criteria The 2-D mesh was generated on the middle surface. Accuracy of structural analysis, to a large extent depends on the FE model. Therefore, care was taken to construct the FE model as close as possible to the geometry of actual vehicle under study. The FE modeling information is mentioned below in Table 1: Table-1: FE Model Info Number of nodes 31,748 1-D 1,155 Number of elements 2-D 27,859 3-D 14,365 Number of mass elements 5 Number of SPC 5 Number of DOF 1,80,600 The FE model of frame was prepared incorporating different boundary conditions (loads/constraints). Concentrated masses were used to equivalently define the weight of 2 drivers, electric motor, battery and carrier luggage. The meshed model of structure of the tricycle chassis is shown below: 3

4 Figure-4: Front view of the FE model Figure-5: Side view of the FE model Figure-6: Top view of the FE model Figure-7: Isometric view of the FE model For connection between the pipes and the bottom plate, CBEAM elements were used for defining the bolts. It is shown below in Fig. 8: Figure-8: Pipe and plate connection using CBEAM at bolt location For defining the spring connection between the pipe and base plate, CELAS elements of appropriate stiffness were used. The electric motor is supported at four mounting locations on 2 cross members provided on the rear structure. It is shown below in Fig. 9: 4

5 Figure-9: Pipe and plate connection using CELAS at spring location A refined mesh is carried out at the weldment locations as shown in Fig. 10 (blue in color). Also gussets are provided at appropriate locations to increase the stiffness of the chassis as shown in Fig. 11. Figure-10: Refined mesh at weld location Figure-11: Gussets provided for increasing chassis stiffness Material properties: The material of the pipes and base plate was taken as AISI 1010 steel with young s modulus 210 GPa, Poisson s ratio 0.3 and density 7.9e-09 tonne/mm 3. The yield strength of the material is 305 MPa. The factor of safety was taken as 2. After meshing the model, the FE model was solved using Optistruct solver. Initially the model was checked by performing the normal modes analysis. The six rigid body modes showed proper connectivity in the model. Then 1 st normal mode of vibration was visualized to observe the vibration behavior of the chassis. After performing the normal modes study, linear static analysis was carried out as per the following extreme conditions: Sitting position: This position is where both riders are in sitting position and whole of weight (115 kg) is considered to distributed for one rider as bearing load on pedals 30% (34.5 kg), load on seat 60% (69 kg), handle10% (11.5 kg). Along with that, 50 kg weight of the carrier, 15 kg weight of the electric motor and 15 kg weight of the battery is also applied. Standing position: This position is where riders lift themselves above seat to pedal aggressively. In this position maximum load is on pedals i.e. 80% (92 kg) and 20% (23 kg) is coming on handles. 5

6 Along with that, 50 kg weight of the carrier, 15 kg weight of the electric motor and 15 kg weight of the battery is also applied. Results and Discussions Linear static study was helpful in depicting the weak regions in the frame. Based on the response, gussets at appropriate joint locations were provided for strengthening the model. Sitting Position: Linear static analysis for sitting position loadcase was carried out. Maximum value of displacement and Von Mises stresses were coming out to be 2.37 mm and 172 MPa respectively. Considering FOS as 2, the permissible value of stress of steel comes to be 153 MPa, which indicates that further modification was required to reduce the stress. The thickness of base strip (which showed maximum stress) was increased from 4 to 6 mm. The new results showed displacement and Von Mises stresses as 1.11 mm and 93.8 MPa respectively which was significantly lower than the previous value and also within the desirable limits. The results are shown below: Figure-12: Displacement Contour Figure-13: Stress Contour Standing Position: After that, linear static analysis for standing position loadcase was carried out. Maximum value of displacement and Von Mises stresses were coming out to be 0.99 mm and 86.8 MPa respectively which was also well within the limits. The results are shown below: Figure-14: Displacement Contour Figure-15: Stress Contour 6

7 Chassis Vertical Stiffness (N/mm) The summary of the results is shown below in table 2: Table-2: Result Summary Sr. No. Output Sitting Position Standing Position 1 Displacement (mm) Von Mises Stress (MPa) Chassis Vertical Stiffness study: The vertical bending stiffness of the chassis is obtained by applying a unit vertical load on the center of gravity of the driver and calculating the maximum vertical displacement. The inverse of this displacement gives the vertical bending stiffness (measured in N/mm). A study had been carried out in which the behaviour of chassis vertical stiffness was observed by varying the spring stiffness as shown in Fig. 16. Chassis Vertical Stiffness Vs Spring Stiffness Spring Stiffness (N/mm) Figure-16: Chassis Vertical Stiffness Vs Spring Stiffness CAE Results conclusion: Maximum induced stress is 93.8 MPa which is less than the allowed stress 153 MPa. This clearly indicates that modified structure is having desired safety margin. The material addition was around 150 g for ensuring safety in the structure. The chassis stiffness study showed that unit increase in spring stiffness led to 1% increase in chassis vertical stiffness. 7

8 Benefits Summary This Tricycle is an economical way of personal transportation with human/electric power thus making it to run at a satisfying speed. It provides best alternative to present day fossil fuel vehicle thereby helps in controlling pollution and maintaining eco-friendly environment. The study helps in reducing the time for testing iterations and number of vehicle prototypes required for testing. This helps in reducing vehicle development time and cost. Conclusions and Future Scope The design and analysis validation provides the direction to improve the design stability of the vehicle. This is done by carrying out the simulation for abuse conditions in sitting and standing loadcases and maintaining the stress and displacement under desired levels. Testing on vehicle prototype will be done on the final vehicle prototype before using it for commercial applications. ACKNOWLEDGEMENTS The author acknowledges the kind support and valuable inputs from team members, faculty and senior management of University College of Engg. (UCOE), Patiala. Sincere thanks to SAE India for giving opportunity to work on a totally new platform which proved to be highly educative and showcasing real life projects. With deep sense of gratitude, special thanks to my parents for the warm blessings, unconditional support and continuous encouragement. [1] OPTISTRUCT- User s Manual- Altair Engineering REFERENCES [2] Nitin S. Gokhale, Sanjay S. Deshpande, Sanjeev V. Bedekar, Anand N. Thite - Practical Finite Element Analysis 8