DESIGN AND ANALYSIS OF A PLASTIC DOOR MODULE FOR CAR BODY APPLICATION
|
|
- Alberta Simpson
- 6 years ago
- Views:
Transcription
1 Abstract DESIGN AND ANALYSIS OF A PLASTIC DOOR MODULE FOR CAR BODY APPLICATION S. Vinay Seeba 1, S. Srikari 2, V. K. Banthia 3 1- (Engg.) Student, 2- Professor, 3- Professor and Head of Department Department of Automotive Design and Engineering M. S. Ramaiah School of Advanced Studies, Bangalore Door module is preassembly of various components on a carrier plate which can be directly mounted onto the door inner panel. These door modules, when directly shipped to the OEM s, save assembly time and cost in mass manufacturing. Long fiber reinforced thermoplastic polypropylene (PP-LFT) with glass filled fiber material is used for various automotive applications as it has improved structural and material properties over conventional materials like steel. Door modules made of PP-LFT material is manufactured using injection molding method. Although significant work was done on design and analysis of plastic door modules, there was no support information on how the final design of the door module was arrived at. Topology and shape optimisation were used in the present investigation to arrive at a design. 30 % glass filled STAMAX PP-LFT door modules were used to replace the existing steel door module plate. Stress analysis and dynamic door slam analysis were carried out on the door module of new design to assess its performance under various durability loading conditions. Finally Mold flow simulation was performed on the door module part to check its manufacturability in mass manufacturing. Final design of STAMAX PP-LFT based plastic door module is 33 % lighter than the existing steel door module plate and has improved strength, stiffness and manufacturability. Key Words: Plastic Door Module, Door Slam, Mold Flow Analysis, STAMAX Nomenclature E V ω ρ Young s Modulus, MPa Linear velocity, m/s Angular Velocity, rad/sec Density, tones/mm3 Abbreviations PP-LFT Long fiber reinforced thermoplastic polypropylene. 1. INTRODUCTION Doors are one of the major components in a car which provide easy access for passengers into the car. With the growing demand on car styling, comfort, safety and other systems integration (window regulator, latch, speaker, motor and electronics) in the door, designing this system is a great challenge to engineers. Door system mainly consists of window glass, window regulator assembly, door latch, sealing and structural components of the door assembly. Traditionally these parts were designed, manufactured and procured separately. A door module is an assembly of functional elements mounted onto a carrier plate. Unlike conventional door systems, where the window regulator assembly was directly attached to the door inner panel, the door module comprises of a carrier plate with window regulator assembly, glass motor and speaker. The window regulator consists of a motor assembly, one or two rails to guide the glass motion, cursor or glass clamps to support the glass, and mechanisms to move the glass up and down. The window regulator, speaker, and other wire harnesses are mounted on the carrier plate using bolts, rivets, and clips. Detailed figure of door module assembly is shown in Figure 1. The carrier plate is bolted to the inner panel. This module approach helps the car makers in reducing assembly time and hence cost. Thus, design and manufacture of door modules is very important. Fig. 1 Door module A door module should perform the following functions Window regulatory function Latch function Speaker function Sealing function A door module offers several advantages over conventional door systems. Some important advantages include [1]. Higher structural strength Better sealing against water vapour and hence door modules are called Sealed Carrier Systems Better noise insulation Dry side mounting of motor and door electronic components Weight savings and hence cost savings due to reduced sheet metal on the door inner panel SASTECH 1 Volume 9, Issue 1, April 2010
2 Reduced original equipment assembly operations as the module is directly bolted to the door inner panel 2. PROBLEM DEFINITION The present day cars use steel door modules for door structure. Steel door modules are heavier, costlier for assembling and require more time during assembly of doors due to non-integration of components. Literature review presented a great amount of research on door module design and analysis, application of plastic material for automotive structures like door modules. From literature study it was found that there were no references on how the final design of plastic door module was arrived. For example Won- Jong Noh et al. [2] required 8 design iterations to arrive at the final design of plastic door module to replace existing steel door module. The disadvantages with the steel door module and design methodology of door module development provided an opportunity to explore alternate design process methodology and application of plastic material for door module in car body application. 2.1 Definition of the Problem To design and analyze a plastic door module for car body application to achieve a weight reduction of 20% compared to existing weight of steel door module. 2.2 Objectives 1. To review literature on door design, development of door modules, durability assessment of door designs 2. To benchmark steel door module for strength and durability requirements 3. To design a plastic door module to meet the application requirements 4. To assess the plastic door module with respect to durability and manufacturability. Achieve at least 20% weight saving over existing steel door module 2.3 Methodology 1. Design of door module was understood using literature, journals, books and other reference media. 2. Surface model of existing front door assembly with steel door module plate was created using CATIA-v5-r17 using reverse engineering. 3. Benchmark values for existing door assembly under durability loads were arrived by performing stress analysis using Altair HyperMesh, Ansys, and LS-Dyna. 4. Plastic door module to replace existing steel door module was designed with help of optimisation using Altair Optistruct v9.0 and CATIA-v5-R The plastic door module was assessed for durability using Altair HyperMesh, Ansys and LS- Dyna to demonstrate its performance enhancements over existing steel door. 6. Mold flow analysis was performed using Autodesk mold flow analysis tool to assess mass manufacturing capabilities and to check the warping/distortion on plastic door module. 3. BENCHMARKING OF STEEL DOOR MODULE 3.1 Geometric Model of Front Door Assembly The geometric model of front door assembly was generated by reverse engineering. Existing steel front door module plate with window regulator mechanism was measured in the benchmarking lab. Using the measured data and available CAD drawings for other parts of front door the geometric model of the door assembly was created. 3.2 Finite Element Modelling of Front Door Assembly The geometric model of the front door assembly was descritised into small finite elements to analyse the structure. All the components were modelled using shell elements at mid plane. Finite element model of door module, glass rails and front door assembly is shown in Figure 2. Since door module pull and glass motor stall analyses are local phenomenon only door module and glass rails were included for the study [3, 5] Entire front door assembly was included for door slam analysis [3] to understand the effect of assembly components on door module plate and glass rails under dynamic loads. Door seals and latch striker interaction were modelled as load versus displacement curves using non-linear discrete spring in LS-Dyna [4]. Curve plot for door seals and latch striker interaction are shown in Figure 3 Fig. 2 Finite Element model of front door Based on the component geometry, the thickness properties were applied to the corresponding shell elements. All the components of the door module were assigned with high strength low alloy SAE J X grade steel materials [5, 6]. Detailed material property is shown in Figure 4. SASTECH 2 Volume 9, Issue 1, April 2010
3 (a) Fig. 5 Boundary condition for door module pull and glass motor stall analysis (b) Fig. 3 Curves used for (a) door seal and (b) latch striker behavior For the door slam analysis body side hinges, ends of body side seal springs and striker were constrained in all translational and rotational degrees of freedom. The ends of seal springs on the door side were constrained in vertical translation (Uz) and fore-aft translation (Ux) degrees of freedom [3]. 3.4 Model Set up for Solution Door module pull loads are experienced on the door module plate when the passenger pulls the door handle to close the door. The door module plate was subjected to load of 200 N in the lateral direction (Y-axis) of the vehicle co-ordinate system as shown in Figure 6 [1, 2]. Fig. 4 HR SAE J X material property Various components of the front door assembly were connected using rigid elements at bolt and weld locations. Contact between mating parts were represented using Automatic Single Surface contact in LS-Dyna. 3.3 Boundary Conditions Since door module pull and glass motor stall analyses are local phenomenon only door module plate and glass rails are included for the analysis. The location where the door module plate is bolted to the door inner panel was constrained in all translational and rotational degrees of freedom as shown in Figure 5. Fig. 6 Loading condition for door module pull analysis Fig. 7 Loading condition for glass motor stall load analysis SASTECH 3 Volume 9, Issue 1, April 2010
4 Fig. 8 Loading condition for door slam analysis When the window glass reaches full up or full down position the motor is under maximum torque due to winding of the drum. At this position due to maximum torque the motor stalls. During stall, rails and door module on which the rail is mounted experience maximum loads [3]. Loading condition for glass motor stall load analysis is shown in Figure 7. Slam load is experienced on the door module when the door is closed with a bang. In the present study, door assembly was subjected to a slam speed of 1.7 m/s (1.9 rad/s). Loading condition for door slam analysis is shown in Figure 8 [3] Table 1. Summary of benchmark reference parameters for steel door module 4. DESIGN OF PLASTIC DOOR MODULE USING OPTIMISATION Plastic door module plate was designed using optimisation method in Altair OptiStruct software [7]. Topology and shape optimisation were used to arrive at the final design of the door module plate. 3.5 Results and Discussion For the door module pull analysis maximum displacement was observed in the pull handle region. For the glass motor stall analysis maximum displacement was observed for front rail and rear rail bottom stall loads cases. Maximum von-mises stress was observed for front rail and rear rail bottom stall load cases. For the door slam analysis maximum von-mises stress was observed near rear rail lower mount when the door strikes the latch. The results of door module pull, glass motor stall and door slam analysis for existing steel door module are summarised in Table 1. These values are the benchmark reference parameters for plastic door module design. Fig. 9 STAMAX 30YM240 material property 4.1 Material Selection for Plastic Door Module Long fiber reinforced thermoplastic materials like STAMAX have excellent material properties with improved stiffness, strength and manufacturing process advantage [1, 2, 8, 9]. STAMAX 30YM240 with 30% glass filled 12 mm long fiber is used for the study. The material has Young s Modulus of 7000 MPa and break strength of 109 MPa at 23 C [10]. Detailed material property values for STAMAX 30YM240 are shown in Figure 9. SASTECH 4 Volume 9, Issue 1, April 2010
5 4.2 Topology Optimisation Topology optimisation is carried out to find the load path for material distribution of plastic door module design. For the door module plate available packaging space was measured to be 48 mm. Design and non design space was defined in the available packaging space. Base thickness was assumed to be 2 mm [11,12, 13]. Detailed plot of packaging space, design space and non design space is shown in Figure 10. Fig. 11 Critical load path plot from topology optimisation Fig. 10 Topology optimisation parameters Design constraints for optimisation parameters like displacement, mass fraction, and stiffness were defined using responses to achieve the benchmark reference parameters tabulated in Table 1 for plastic door module plate. Objective for the topology optimisation study was to maximize stiffness of the plastic door module part. Topology optimisation was carried out for door module pull loads, glass motor stall loads, motor and speaker self weight loads. Fig. 12 Geometry output from topology optimisation 4.2 Results for Topology Optimisation The results from topology optimisation are shown in Figure 11 and 12. Figure 11 shows the element density plot which identifies the material distribution in the critical load path for the design which satisfies the design objective for the design constraints specified. Figure 12 shows the geometry output from topology optimisation processed using OSS smooth in Altair OptiStruct. Fig. 13 Shape optimisation parameters SASTECH 5 Volume 9, Issue 1, April 2010
6 4.3 Shape Optimisation Topology optimisation provided geometry layout for the plastic door module plate and location for reinforcements on the plastic door module plate to achieve the performance parameters defined in design constraints. Shape optimisation was necessary to define proper shape of the rib topology. Final shape (height) of the reinforcement ribs on the plastic door module carrier plate was fixed by carrying out shape optimisation in Altair OptiStruct software. Shape optimisation was carried out by defining rib geometry shape as domain and handles as shown in Figure 13. Design variable for shape optimisation was defined by varying the rib height of domains at handle locations. Design variable for the rib shape was set as (-1, +1). Design constraints, loads and boundary conditions were similar to the design constraints used for topology optimisation with respect to displacement values. Design objective for the shape optimisation problem was to minimize the mass. 4.4 Results for Shape Optimisation The results from shape optimisation are shown in Figure 14. It shows the final rib pattern with minimized mass of ribs overlaid on original rib pattern. Final weight of the ribs after shape optimisation was 43.7 grams compared to initial weight of 61.1 grams, 28% reduction in rib weight due to shape optimisation. 4.5 Plastic Door Module Plate Final design of plastic door module plate based on topology and shape optimisation results was generated using CATIA V5R17. Plastic door module plate has thickness of 2mm for the plate base and ribs. Pull handle support bracket was integrated to the door module plate. Rear rail lower mount was provided with double screws since the mount had least fatigue life as per benchmarking Fig. 14 Final rib shape obtained from shape optimisation reference parameters listed in Table 4.1. Final design of the plastic door module plate is shown in Figure 15. Final weight of the plastic door module plate is 1.2 kg. Table 2. Fatigue life data for STAMAX 30YM240 STAMAX 30YM240 estimated failure stress [MPA] at 23 C Cycles, n Failure Stress, MPa , , , , Fig. 15 Plastic door module 5. VALIDATION AND RESULTS Plastic door module was assessed for door module pull, glass motor stall and door slam loads to verify its performance so that it can replace the existing steel door module plate. Fatigue life data for STAMAX 30YM240 is shown in Table 4.2. SASTECH 6 Volume 9, Issue 1, April 2010
7 Since only the design of door module plate was changed in the front door assembly modelling details, section properties, contact and connection definitions, loads and boundary condition remain same for door module pull, glass motor stall and door slam analysis. Mold flow analysis was performed on the plastic door module plate to check for its manufacturability by defining the mold material inlet gating locations as shown in Figure Results and Discussion For the door module pull analysis maximum displacement of 3.8 mm was observed in the pull handle region. This value is less than 3.9 mm observed for steel door module pull analysis. For the glass motor stall analysis maximum displacement was observed for front rail and rear rail top stall loads cases. Maximum von-mises stress was observed for front rail top stall and rear rail bottom stall load cases. Maximum von-mises stress on the glass rails with plastic door module plate was less than the stress observed on glass rails with steel door module plate. Maximum displacement on glass rails for stall analysis was 4 mm with plastic door module plate compared to 2.4 mm for steel door module plate. However there was no interference of the glass rails with any other assembly part of the door due to increased Fig. 16 Gating location for material injection into mold Table 3. Summary of results for plastic door module displacement. Hence the design was assumed to be acceptable. For the door slam analysis maximum von-mises stress of 36.1 MPa was observed near rear rail lower mount during the door rebound after the door slam. Maximum von-mises stress of MPA was observed when door hits the striker. Maximum von-mises on door module plate for door slam analysis was 36.1 MPa. Comparing the maximum von-mises stress value observed for door slam analysis with the fatigue life data for STAMAX 30YM240 material in Table 2 it was found that the material has fatigue life greater than 100,000 cycles, meeting the slam life standard to be met for door module designs [3, 11]. From mold flow analysis results it was observed that the time required to fill the door module part with STAMAX material was 3.4 s. Maximum clamp force was 750 tonnes. Maximum out of plane distortion(warpage) on the finished part was 4.9 mm. The maximum distortion observed was less than benchmark reference value of 5 mm [11]. Hence the plastic door module design was assumed to be acceptable for mass manufacturing. The results of door module pull, glass motor stall and door slam analysis for plastic door module design are summarised in Table 3 below. Sl No Load Case Max. displacement mm Max. von-mises stress MPa Fatigue life cycles 1 Door module pull analysis N.A. 2 Glass motor N.A. stall load analysis 3 Door slam analysis N.A >100,000 4 Mold Flow analysis Out of plane distortion/warpage = 4.9 mm 5 Weight of plastic door module plate 1.2 kg SASTECH 7 Volume 9, Issue 1, April 2010
8 6. CONCLUSION 1. The study helped in designing plastic door module plate for car body application using 30% glass fiber PP-LFT (STAMAX ) material, topology and shape optimisation techniques. 2. Final design of the plastic door module is 33% lesser in weight with improved structural, properties compared to existing steel door module plate. 3. The design and analysis methodology adopted here to design plastic door module plate to replace existing steel door module plate can be adopted to design and analyse plastic parts to replace semi structural automotive parts currently made from steel. 7. REFERENCES [1] Maria Ciliberti, Warden Schijve, Developments in Thermoplastic Door Modules SAE Technical paper series, , [2] Won-Jong Noh, Min Ho Choi, Chi Hoon Choi and Tae Won Hwang, Development of Door Module Plate with Long-fiber-reinforced Thermoplastic Polypropylene, SAE Technical Paper, , [3] Devadas Kumbla, Pan Shi, Joseph Saxon, Simulation methods for door module design, SAE Technical Paper, , [4] LS-Dyna User Manual, Version 971, 2006, Livermore Software Technology Corporation. [5] Kalpak Shah, Hong Tae Kang and Upendra Deshmukh, Design of Dual Sliding Door for a Small Size Car and Its Validation Using CAE Tools, SAE Technical Paper, , [6] HR SAE J X HSLA steel material properties, al.pdf, 24 th June, [7] HyperWorks User Manual, Version 9.0, 2009, Altair Incorporation, [8] Takahiro Tochioka, Development of integrated Functions Module Carriers by Injection Molding with Long Glass Fiber Reinforced Polypropylene, SAE Technical Paper series, , [9] Manish Chaturvedi, Warden Schijve, Matthew Marks, Advanced Thermoplastic Composites for Automotive Semi Structural Application, SAE Technical Paper, , [10] Unanimous, product=196c0e98-0f0e-4fd4-a476-51f83d2b8888&template=product, 15 th August, [11] Scott E. Zilincik, Wm. Jeffrey DeFrank, and Scott G. Miller, Slam Life Assessment Method for Closures Durability SAE Technical Paper, , [12] A paper entitled Application of topology, sizing and shape optimisation methods to optimal design of Aircraft components, presented at Altair engineering conference, [13] A paper entitled A new approach for sizing, shape and topology optimisation, SAE International congress and exposition, 2002, 96/sae_org.pdf, 24 th June, SASTECH 8 Volume 9, Issue 1, April 2010
Load Analysis and Multi Body Dynamics Analysis of Connecting Rod in Single Cylinder 4 Stroke Engine
IJSRD - International Journal for Scientific Research & Development Vol. 3, Issue 08, 2015 ISSN (online): 2321-0613 Load Analysis and Multi Body Dynamics Analysis of Connecting Rod in Single Cylinder 4
More informationFatigue Life Estimation of Chassis Frame FESM Bracket for Commercial Vehicle
Fatigue Life Estimation of Chassis Frame FESM Bracket for Commercial Vehicle Shivakumar M.M 1, Nirmala L 2 ¹M-Tech Student, Dept. of Mechanical Engineering,K.S Institute of Technology, Bangalore, India
More informationAdvanced Vehicle Performance by Replacing Conventional Vehicle Wheel with a Carbon Fiber Reinforcement Composite Wheel
Advanced Vehicle Performance by Replacing Conventional Vehicle Wheel with a Carbon Fiber Reinforcement Composite Wheel Jyothi Prasad Gooda Technical Manager Spectrus Informatics Pvt..Ltd. No. 646, Ideal
More informationStudy Of Static And Frequency Responsible Analysis Of Hangers With Exhaust System
International Journal of Advances in Scientific Research and Engineering (ijasre) ISSN: 2454-8006 [Vol. 03, Issue 5, June -2017] Study Of Static And Frequency Responsible Analysis Of Hangers With Exhaust
More informationFE Modeling and Analysis of a Human powered/electric Tricycle chassis
FE Modeling and Analysis of a Human powered/electric Tricycle chassis Sahil Kakria B.Tech, Mechanical Engg UCOE, Punjabi University Patiala, Punjab-147004 kakria.sahil@gmail.com Abbreviations: SAE- Society
More informationPREDICTION OF PISTON SLAP OF IC ENGINE USING FEA BY VARYING GAS PRESSURE
PREDICTION OF PISTON SLAP OF IC ENGINE USING FEA BY VARYING GAS PRESSURE V. S. Konnur Department of Mechanical Engineering, BLDEA s Engineering College, Bijapur, Karnataka, (India) ABSTRACT The automotive
More informationSimulation and Validation of FMVSS 207/210 Using LS-DYNA
7 th International LS-DYNA Users Conference Simulation Technology (2) Simulation and Validation of FMVSS 207/210 Using LS-DYNA Vikas Patwardhan Tuhin Halder Frank Xu Babushankar Sambamoorthy Lear Corporation
More informationAluminum Gear Shift Fork with Supporting Pad for light weighting in Commercial Vehicles
Aluminum Gear Shift Fork with Supporting Pad for light weighting in Commercial Vehicles Suresh Kumar K, Manger VE Commercial Vehicles Limited skkandreegula@vecv.in, Naveen Sukumar N, Dy.Manger VE Commercial
More information305Vehicle Door Sag Evaluation Using FEA
International Journal of Engineering Research and Development e-issn: 2278-067X, p-issn: 2278-800X, www.ijerd.com Volume 11, Issue 03 (March 2015), PP.21-26 305Vehicle Door Sag Evaluation Using FEA Sagar
More informationModal analysis of Truck Chassis Frame IJSER
Modal analysis of Truck Chassis Frame 158 Shubham Bhise 1, Vaibhav Dabhade 1, Sujit Pagi 1, Apurvi Veldandi 1. 1 B.E. Student, Dept. of Automobile Engineering, Saraswati College of Engineering, Navi Mumbai,
More informationSimulating Rotary Draw Bending and Tube Hydroforming
Abstract: Simulating Rotary Draw Bending and Tube Hydroforming Dilip K Mahanty, Narendran M. Balan Engineering Services Group, Tata Consultancy Services Tube hydroforming is currently an active area of
More informationVibration Fatigue Analysis of Sheet Metal Fender Mounting Bracket & It's Subsequent Replacement With Plastic
Vibration Fatigue Analysis of Sheet Metal Fender Mounting Bracket & It's Subsequent Replacement With Plastic Vikas Palve Manager - CAE Mahindra Two Wheelers Ltd D1 Block, Plot No 18/2 (Part), Chinchwad,
More informationDesign, Analysis &Optimization of Crankshaft Using CAE
Design, Analysis &Optimization of Crankshaft Using CAE Dhekale Harshada 1, Jagtap Ashwini 2, Lomte Madhura 3, Yadav Priyanka 4 1,2,3,4 Government College of Engineering and Research Awasari, Department
More informationDesign, Analysis& Optimization of Truck chassis- Rail & Cross member
Design, Analysis& Optimization of Truck chassis- Rail & Cross member Mr. Jinto Joju Thaikkattil 1, Gayatri Patil 2 1 PGScholar, Department of Mechanical Engg., KJCOEMR, Pune, jjt7171@gmail.com 2 Assistant
More informationStatic Structural Analysis & Optimization of Concept Automotive A-Arm Mechanical Engineering Design
Static Structural Analysis & Optimization of Concept Automotive A-Arm Mechanical Engineering Design Ashish R. Pawar 1, Madhuri V. Bodke 2, Aditya R. Wankhade 3 1,3 Mechanical Engineering Department, ABMSP
More informationSTATIC STRUCTURAL ANALYSIS AND OPTIMIZATION OF BRAKE PEDAL
STATIC STRUCTURAL ANALYSIS AND OPTIMIZATION OF BRAKE PEDAL Miss. ASHWINI N.GAWANDE 1, Prof.G.E.KONDHALKAR 2, Prof. ASHISH R.PAWAR 3 1PG Student, Design Engineering, APCOE & R, Parvati, Pune 2HOD, Mechanical
More informationValue Engineering of Engine Rear Cover by Virtual Simulation
Value Engineering of Engine Rear Cover by Virtual Simulation Vishaldeep Sr. Engineer - R&D, CAE vishaldeep.dadwal@sonalika.com Vibhay Kumar Sr. Manager - R&D, CAE vibahy.kumar@sonalika.com Satpal Singh
More informationSTATIC AND FATIGUE ANALYSIS OF LEAF SPRING-AS A REVIEW
STATIC AND FATIGUE ANALYSIS OF LEAF SPRING-AS A REVIEW Vishal Gavali 1, Mahesh Jadhav 2, Digambar Zoman 3 1,2, 3 Mechanical Engineering Department, LGNSCOE Anjaneri Nashik,(India) ABSTRACT In engineering
More informationDesign and Analysis of Engine and Chassis Mounting Bracket
Design and Analysis of Engine and Chassis Mounting Bracket Vidyasagar Kadam 1, Prof.A.C.Mattikali 2 1 M.Tech.,Mechanical Engg. Dept., MMEC, Belagavi 2 Assistant Prof. Mechanical Engg. Dept. MMEC, Belagavi
More informationDESIGN AND FABRICATION OF CHASSIS FOR ELECTRICAL VEHICLE
DESIGN AND FABRICATION OF CHASSIS FOR ELECTRICAL VEHICLE SHAIK.BALA SAIDULU 1, G.VIJAY KUMAR 2 G.DIWAKAR 3, M.V.RAMESH 4 1 M.Tech Student, Mechanical Engineering Department, Prasad V Potluri Siddhartha
More informationAutomotive Seat Modeling and Simulation for Occupant Safety using Dynamic Sled Testing
Automotive Seat Modeling and Simulation for Occupant Safety using Dynamic Sled Testing Dr. Vikrama Singh Professor Mech. Engineering Dept.Pad.Dr.D.Y.Patil Institute of Engineering & Tech.Pimpri Pune Mr.
More informationVehicle Dynamic Simulation Using A Non-Linear Finite Element Simulation Program (LS-DYNA)
Vehicle Dynamic Simulation Using A Non-Linear Finite Element Simulation Program (LS-DYNA) G. S. Choi and H. K. Min Kia Motors Technical Center 3-61 INTRODUCTION The reason manufacturers invest their time
More informationFEM Analysis of Combined Paired Effect on Piston & Connecting Rod using ANSYS
FEM Analysis of Combined Paired Effect on Piston & Connecting Rod using ANSYS Kunal Saurabh Assistant Professor, Mechanical Department IEC Group of Institutions, Greater Noida - India kunalsaurabh.me@ieccollege.com
More informationROOF CRUSH SIMULATION OF PASSENGER CAR FOR IMPROVING OCCUPANT SAFETY IN CABIN
ROOF CRUSH SIMULATION OF PASSENGER CAR FOR IMPROVING OCCUPANT SAFETY IN CABIN Anandkumar. M. Padashetti M.Tech student (Design Engineering), Mechanical Engineering, K L E Dr. M S Sheshagiri College of
More informationRotorcraft Gearbox Foundation Design by a Network of Optimizations
13th AIAA/ISSMO Multidisciplinary Analysis Optimization Conference 13-15 September 2010, Fort Worth, Texas AIAA 2010-9310 Rotorcraft Gearbox Foundation Design by a Network of Optimizations Geng Zhang 1
More informationStatic Analysis of Crankcase and Crankshaft of Single Cylinder Four Stroke Diesel Engine
Static Analysis of Crankcase and Crankshaft of Single Cylinder Four Stroke Diesel Engine Kakade Pratik 1 Post Graduate Student kakadepratik@gmail.com Pasarkar M. D. 2 Assistant Professor mdpasarkar@gmail.com
More informationBIKE SPIRAL SPRING (STEEL) ANALYSIS
BIKE SPIRAL SPRING (STEEL) ANALYSIS Yaluppa Madhukar Benake 1, Prof.Santosh Mali Patil 2 1 M.Tech.,Mechanical Engg. Dept., MMEC, Belagavi 2 Assistant Prof. Mechanical Engg. Dept. MMEC, Belagavi Abstract
More informationINTERNATIONAL JOURNAL OF DESIGN AND MANUFACTURING TECHNOLOGY (IJDMT) CONSTANT SPEED ENGINE CONROD SOFT VALIDATION & OPTIMIZATION
INTERNATIONAL JOURNAL OF DESIGN AND MANUFACTURING TECHNOLOGY (IJDMT) International Journal of Design and Manufacturing Technology (IJDMT), ISSN 0976 6995(Print), ISSN 0976 6995 (Print) ISSN 0976 7002 (Online)
More informationHeat treatment Elimination in Forged steel Crankshaft of Two-stage. compressor.
Research Journal of Engineering Sciences ISSN 2278 9472 Heat treatment Elimination in Forged steel Crankshaft of Two-stage Compressor Abstract Lakshmanan N. 1, Ramachandran G.M. 1 and Saravanan K. 2 1
More informationSTRESS AND VIBRATION ANALYSIS OF A GAS TURBINE BLADE WITH A COTTAGE-ROOF FRICTION DAMPER USING FINITE ELEMENT METHOD
STRESS AND VIBRATION ANALYSIS OF A GAS TURBINE BLADE WITH A COTTAGE-ROOF FRICTION DAMPER USING FINITE ELEMENT METHOD S. Narasimha 1* G. Venkata Rao 2 and S. Ramakrishna 1 1 Dept. of Mechanical Engineering,
More informationDesign and Optimization of HTV Fuel Tank Assembly by Finite Element Analysis
Design and Optimization of HTV Fuel Tank Assembly by Finite Element Analysis Ms.Baseera Banushaik PG Student, Department of Mechanical Engineering, Malla Reddy College of Engineering, Secunderabad. Ms.I.Prasanna
More informationStatic And Modal Analysis of Tractor Power Take Off (PTO) Gearbox Housing
Static And Modal Analysis of Tractor Power Take Off (PTO) Gearbox Housing Gopali S Lamani 1, Prof: S.R.Basavaraddi 2, Assistant Professor, Department of Mechanical Engineering, JSPM NTC RSSOER,India1 Professor,
More informationWeight reduction of Steering Knuckle by Optimization Method
Weight reduction of Steering Knuckle by Optimization Method R.P.Gaikwad #1, Prof.Y.P.Reddy *2 #1 P.G Scholar, Department of Mechanical Engineering, Sinhgad College of Engineering, Pune, India *2 Professor,
More informationModular Analysis of Main Rotor Blade of Light Helicopter using FEM
Modular Analysis of Main Rotor Blade of Light Helicopter using FEM Mahesh N V 1, Raghu T 2 Schlor, IVth Semester M. Tech(Design Engineering), 2 Assistant Professor 1, 2 Mechanical Engineering Department
More informationExhaust System Optimization of Passenger Car for Maximizing Fuel Efficiency through HyperWorks
Exhaust System Optimization of Passenger Car for Maximizing Fuel Efficiency through HyperWorks Dr. S. Rajadurai Head - R&D Sharda Motor Industries Ltd, Research and Development Mahindra World City, Chennai
More informationDesign and Optimisation of Roll Cage of a Single Seated ATV
IOSR Journal of Mechanical and Civil Engineering (IOSR-JMCE) e-issn: 2278-1684,p-ISSN: 2320-334X, Volume 12, Issue 2 Ver. III (Mar - Apr. 2015), PP 56-61 www.iosrjournals.org Design and Optimisation of
More informationSTRUCTURAL ANALYSIS OF STEERING YOKE OF AN AUTOMOBILE FOR WITHSTANDING TORSION/ SHEAR LOADS
STRUCTURAL ANALYSIS OF STEERING YOKE OF AN AUTOMOBILE FOR WITHSTANDING TORSION/ SHEAR LOADS S.K.Chandole 1, M.D.Shende 2, M.K.Bhavsar 3 1 PG Student, Mechanical Engineering, S.N.D. COE & RC, Yeola, Nasik,
More informationSTRUCTURAL OPTIMIZATION & DURABILITY ANALYSIS OF VW BETTLE CROSS EXHAUST MUFFLER SYSTEM
STRUCTURAL OPTIMIZATION & DURABILITY ANALYSIS OF VW BETTLE CROSS EXHAUST MUFFLER SYSTEM Vikram Kumbhar 1, Prof D.C.Patil 2 1Post Graduate Student, Department of Mechanical Engineering, KLEMSSCET, Karnataka,
More informationStatic and Dynamic Strength Analysis on Rear Axle of Small Payload Off-highway Dump Trucks
Static and Dynamic Strength Analysis on Rear Axle of Small Payload Off-highway Dump Trucks Ji-xin Wang, Guo-qiang Wang, Shi-kui Luo, Dec-heng Zhou College of Mechanical Science and Engineering, Jilin University,
More informationMODEL FREQUENCY ANALYSIS OF AUTOMOTIVE EXHAUST SYSTEM
Research Paper ISSN 2278 ñ 0149 www.ijmerr.com Vol. 3, No. 1, January 2014 2014 IJMERR. All Rights Reserved MODEL FREQUENCY ANALYSIS OF AUTOMOTIVE EXHAUST SYSTEM D Jai Balaji 1*, P V Srihari 1 and Veeranna
More informationDesign and Analysis of Front Lower Control Arm by Using Topology Optimization
Design and Analysis of Front Lower Control Arm by Using Topology Optimization Prashant Gunjan 1, Amit Sarda 2 12 Department of Mechanical Engineering, Christian College of Engineering and Technology, Bhilai
More informationNon-Linear Simulation of Front Mudguard Assembly
Non-Linear Simulation of Front Mudguard Assembly Jasdeep Singh Sr. Engineer - R&D, CAE International Tractor Limited (Vill. Chak Gujran) Jalandhar Road Hoshiarpur, Punjab - 146022 jasdeep.s@sonalika.com
More informationAnalysis of Steering Knuckle of All Terrain Vehicles (ATV) Using Finite Element Analysis
IOP Conference Series: Materials Science and Engineering PAPER OPEN ACCESS Analysis of Steering Knuckle of All Terrain Vehicles (ATV) Using Finite Element Analysis To cite this article: S V Dusane et al
More informationCrashworthiness Evaluation of an Impact Energy Absorber in a Car Bumper for Frontal Crash Event - A FEA Approach
Crashworthiness Evaluation of an Impact Energy Absorber in a Car Bumper for Frontal Crash Event - A FEA Approach Pravin E. Fulpagar, Dr.S.P.Shekhawat Department of Mechanical Engineering, SSBTS COET Jalgaon.
More informationS.Sivaraj #1, A.Hazemohzammed *1, M.Yuvaraj *2, N.Karthikeyan *3, V.Murugan *4, # Assistant Prof., Dept, * U.G Students,
Structural Analysis of Ladder Chassis Frame for car UsingAnsys S.Sivaraj #1, A.Hazemohzammed *1, M.Yuvaraj *2, N.Karthikeyan *3, V.Murugan *4, # Assistant Prof., Dept, * U.G Students, Dept of mechanical
More informationStress Analysis of Engine Camshaft and Choosing Best Manufacturing Material
Stress Analysis of Engine Camshaft and Choosing Best Manufacturing Material Samta Jain, Mr. Vikas Bansal Rajasthan Technical University, Kota (Rajasathan), India Abstract This paper presents the modeling
More informationGasket Simulations process considering design parameters
Gasket Simulations process considering design parameters Sonu Paroche Deputy Manager VE Commercial Vehicles Ltd. 102, Industrial Area No. 1 Pithampur, District Dhar MP - 454775, India sparoche@vecv.in
More informationStress Analysis of Piston at Different Pressure Load
Stress Analysis of Piston at Different Pressure Load 1 PG Student, Department of Mechanical Engineering, SKNSITS, Lonavala, India 2 Professor, Department of Mechanical Engineering, SKNSITS, Lonavala, India
More informationDesign Improvement in front Bumper of a Passenger Car using Impact Analysis
Design Improvement in front Bumper of a Passenger Car using Impact Analysis P. Sridhar *1,Dr. R.S Uma Maheswar Rao 2,Mr. Y Vijaya Kumar 3 *1,2,3 Department of Mechanical Engineering, JB Institute of Engineering
More informationVEHICLE ANTI-ROLL BAR ANALYZED USING FEA TOOL ANSYS
VEHICLE ANTI-ROLL BAR ANALYZED USING FEA TOOL ANSYS P. M. Bora 1, Dr. P. K. Sharma 2 1 M. Tech. Student,NIIST, Bhopal(India) 2 Professor & HOD,NIIST, Bhopal(India) ABSTRACT The aim of this paper is to
More informationMODELING SUSPENSION DAMPER MODULES USING LS-DYNA
MODELING SUSPENSION DAMPER MODULES USING LS-DYNA Jason J. Tao Delphi Automotive Systems Energy & Chassis Systems Division 435 Cincinnati Street Dayton, OH 4548 Telephone: (937) 455-6298 E-mail: Jason.J.Tao@Delphiauto.com
More informationDesign Improvement in Kingpin Stub Axle Assembly Using FEA
Design Improvement in Kingpin Stub Axle Assembly Using FEA Yaseen Khan Asst.Manager - R&D, CAE International Tractors Ltd. R&D Center,vill.Chak Gujran Jalandhar Road, Hoshiarpur Punjab - 146001, India
More informationDesign and Analysis of Steering Knuckle Component For Terrain Vehicle
Design and Analysis of Steering Knuckle Component For Terrain Vehicle V.S.Shaisundaram 1, L.Karikalan 2, V.Vignesh 3, R.Tamilmani 4, M.Akash 5 1 Assistant Professor, Department Of Automobile Engineering,
More informationIJESRT. Scientific Journal Impact Factor: (ISRA), Impact Factor: 1.852
IJESRT INTERNATIONAL JOURNAL OF ENGINEERING SCIENCES & RESEARCH TECHNOLOGY Design Analysis and Optimization of Piston and Determination of its Thermal Stresses Using CAE Tools Deovrat Vibhandik *1, Ameya
More informationTHE STUDY ON EFFECT OF TORQUE ON PISTON LATERAL MOTION
THE STUDY ON EFFECT OF TORQUE ON PISTON LATERAL MOTION Vinay V. Kuppast 1, S. N. Kurbet 2, A. M. Yadawad 3, G. K. Patil 4 1 Associate Professor, 2 Professor & Head, 4 Associate Professor, Department of
More informationDESIGN AND ANALYSIS OF TUBULAR CHASSIS OF GO-KART
DESIGN AND ANALYSIS OF TUBULAR CHASSIS OF GO-KART Prashant Thakare 1, Rishikesh Mishra 2, Kartik Kannav 3, Nikunj Vitalkar 4, Shreyas Patil 5, Snehal Malviya 6 1 UG Students, Department of Mechanical Engineering,
More informationDevelopment and Validation of a Finite Element Model of an Energy-absorbing Guardrail End Terminal
Development and Validation of a Finite Element Model of an Energy-absorbing Guardrail End Terminal Yunzhu Meng 1, Costin Untaroiu 1 1 Department of Biomedical Engineering and Virginia Tech, Blacksburg,
More informationDesign Evaluation of Fuel Tank & Chassis Frame for Rear Impact of Toyota Yaris
International Research Journal of Engineering and Technology (IRJET) e-issn: 2395-0056 Volume: 03 Issue: 05 May-2016 p-issn: 2395-0072 www.irjet.net Design Evaluation of Fuel Tank & Chassis Frame for Rear
More informationComparison Of Multibody Dynamic Analysis Of Double Wishbone Suspension Using Simmechanics And FEA Approach
International Journal of Research in Engineering and Science (IJRES) ISSN (Online): 232-9364, ISSN (Print): 232-9356 Volume 2 Issue 4 ǁ April. 214 ǁ PP.31-37 Comparison Of Multibody Dynamic Analysis Of
More informationISSN: [Raghunandan* et al., 5(11): November, 2016] Impact Factor: 4.116
IJESRT INTERNATIONAL JOURNAL OF ENGINEERING SCIENCES & RESEARCH TECHNOLOGY DESIGN AND ANALYSIS OF GO-KART CHASSIS D.Raghunandan*, A.Pandiyan, Shajin Majeed * Mechanical Department, Final year, Saveetha
More informationNon-Linear Finite Element Analysis of Typical Wiring Harness Connector and Terminal Assembly Using ABAQUS/CAE and ABAQUS/STANDARD
Non-Linear Finite Element Analysis of Typical Wiring Harness Connector and Terminal Assembly Using ABAQUS/CAE and ABAQUS/STANDARD Boya Lakshmi Narayana William G Strang Aashish Bhatia Delphi Automotive
More informationDESIGN AND ANALYSIS OF PUSH ROD ROCKER ARM SUSPENSION USING MONO SPRING
Volume 114 No. 9 2017, 465-475 ISSN: 1311-8080 (printed version); ISSN: 1314-3395 (on-line version) url: http://www.ijpam.eu ijpam.eu DESIGN AND ANALYSIS OF PUSH ROD ROCKER ARM SUSPENSION USING MONO SPRING
More informationFinite Element Analysis of Connecting Rod to Improve Its Properties
REST Journal on Emerging trends in Modelling and Manufacturing Vol:1(2),2015 REST Publisher ISSN: 2455-4537 Website: www.restpublisher.com/journals/jemm Finite Element Analysis of Connecting Rod to Improve
More informationANALYSIS AND OPTIMIZATION OF CONNECTING ROD USING ALFASiC COMPOSITES
ANALYSIS AND OPTIMIZATION OF CONNECTING ROD USING ALFASiC COMPOSITES Kuldeep B 1, Arun L.R 2, Mohammed Faheem 3 P.G. Scholar, Department of Mechanical Engineering, The Oxford college of Engineering, Karnataka,
More informationComposite Long Shaft Coupling Design for Cooling Towers
Composite Long Shaft Coupling Design for Cooling Towers Junwoo Bae 1,#, JongHun Kang 2, HyoungWoo Lee 2, Seungkeun Jeong 1 and SooKeun Park 3,* 1 JAC Coupling Co., Ltd., Busan, South Korea. 2 Department
More informationDevelopment of analytical process to reduce side load in strut-type suspension
Journal of Mechanical Science and Technology 24 (21) 351~356 www.springerlink.com/content/1738-494x DOI 1.7/s1226-9-113-z Development of analytical process to reduce side load in strut-type suspension
More informationVirtual Durability Simulation for Chassis of Commercial vehicle
Virtual Durability Simulation for Chassis of Commercial vehicle Mahendra A Petale M E (Mechanical Engineering) G S Moze College of Engineering Balewadi Pune -4111025 Prof. Manoj J Sature Asst. Professor
More informationModeling and Vibration Analysis of a Drum type Washing Machine
Modeling and Vibration Analysis of a Drum type Washing Machine Takayuki KOIZUMI, Nobutaka TSUJIUCHI, Yutaka NISHIMURA Department of Engineering, Doshisha University, 1-3, Tataramiyakodani, Kyotanabe, Kyoto,
More informationApplication and CAE Simulation of Over Molded Short and Continuous Fiber Thermoplastic Composites: Part II
12 th International LS-DYNA Users Conference Simulation(3) Application and CAE Simulation of Over Molded Short and Continuous Fiber Thermoplastic Composites: Part II Prasanna S. Kondapalli BASF Corp.,
More informationParametric study on behaviour of box girder bridges using CSi Bridge
Parametric study on behaviour of box girder bridges using CSi Bridge Kiran Kumar Bhagwat 1, Dr. D. K. Kulkarni 2, Prateek Cholappanavar 3 1Post Graduate student, Dept. of Civil Engineering, SDMCET Dharwad,
More informationDynamic Response Assessment and Design Optimization of Aircraft Tyre Pressure Monitoring Unit (TPMU) Akshay B G 1 Dr. B M Nandeeshaiah 2
IJSRD - International Journal for Scientific Research & Development Vol. 3, Issue 09, 2015 ISSN (online): 2321-0613 Dynamic Response Assessment and Design Optimization of Aircraft Tyre Pressure Monitoring
More informationStatic Stress Analysis of Piston
Static Stress Analysis of Piston Kevin Agrawal B. E. Student, Mechanical Engineering, BITS Pilani K. K. Birla Goa Campus. AH7-352, BITS Pilani, K. K. Birla Goa Campus, NH 17B, Zuarinagar 403726. Parva
More informationEXPERIMENTAL ANALYSIS AND TOPOLOGY OPTIMIZATION OF LOWER SUSPENSION ARM OF CAR
EXPERIMENTAL ANALYSIS AND TOPOLOGY OPTIMIZATION OF LOWER SUSPENSION ARM OF CAR Rupali Dhore 1, Prof. M.L. Thorat 2 1B.E.MECH. (M.E.Pursuing), Mechanical Department, RMD SINHGAD SCHOOL OF ENGINEERING, PUNE
More informationSimulation of Structural Latches in an Automotive Seat System Using LS-DYNA
Simulation of Structural Latches in an Automotive Seat System Using LS-DYNA Tuhin Halder Lear Corporation, U152 Group 5200, Auto Club Drive Dearborn, MI 48126 USA. + 313 845 0492 thalder@ford.com Keywords:
More informationInternational Journal of Scientific & Engineering Research, Volume 7, Issue 3, March ISSN DESIGN AND ANALYSIS OF A SHOCK ABSORBER
International Journal of Scientific & Engineering Research, Volume 7, Issue 3, March-2016 19 DESIGN AND ANALYSIS OF A SHOCK ABSORBER Johnson*, Davis Jose, Anthony Tony Abstract: -Shock absorbers are a
More informationComposites Modeler for Abaqus/CAE. Abaqus 2018
Composites Modeler for Abaqus/CAE Abaqus 2018 About this Course Course objectives In this course you will learn about: Composites Modeler for Abaqus/CAE, an add-on product to Abaqus/CAE How to use Composites
More informationDynamic Load Analysis and Optimization of a Fracture-Split Connecting Rod
Dynamic Load Analysis and Optimization of a Fracture-Split Connecting Rod Dipak Sarmah, Athar M Khan and Anirudh Jaipuria Ashok Leyland Ltd. India. Abstract: This paper summarizes the methodology to design
More informationDesign & Manufacturing of an Effective Steering System for a Formula Student Car
Design & Manufacturing of an Effective Steering System for a Formula Student Car Nikhil N. Gitay 1, Siddharth A. Joshi 2, Ajit A. Dumbre 3, Devesh C. Juvekar 4 1,2,3,4 Student, Department of Mechanical
More informationANALYSIS OF GEAR QUALITY CRITERIA AND PERFORMANCE OF CURVED FACE WIDTH SPUR GEARS
8 FASCICLE VIII, 8 (XIV), ISSN 11-459 Paper presented at Bucharest, Romania ANALYSIS OF GEAR QUALITY CRITERIA AND PERFORMANCE OF CURVED FACE WIDTH SPUR GEARS Laurentia ANDREI 1), Gabriel ANDREI 1) T, Douglas
More informationOptimization of Four Cylinder Engine Crankshaft using FEA
Optimization of Four Cylinder Engine Crankshaft using FEA Prasad P. Gaware 1, Prof. V.S. Aher 2 Department of Mechanical Engineering, AVCOE, Sangamner 1 Department of Mechanical Engineering, AVCOE, Sangamner
More informationCOMPARATIVE ANALYSIS OF CRANKSHAFT IN SINGLE CYLINDER PETROL ENGINE CRANKSHAFT BY NUMERICAL AND ANALYTICAL METHOD
COMPARATIVE ANALYSIS OF CRANKSHAFT IN SINGLE CYLINDER PETROL ENGINE CRANKSHAFT BY NUMERICAL AND ANALYTICAL METHOD Mr. Anant B. Khandkule PG Student Mechanical Engineering Department, Sinhgad Institute
More informationIJESRT. Scientific Journal Impact Factor: (ISRA), Impact Factor: METHODOLOGY Design Parameter [250]
IJESRT INTERNATIONAL JOURNAL OF ENGINEERING SCIENCES & RESEARCH TECHNOLOGY DESIGN AND ANALYSIS OF COMPOSITE LEAF SPRING FOR LIGHT COMMERCIAL VEHICLE (TATA ACE) Miss. Gulshad Karim Pathan*, Prof. R.K.Kawade,
More informationSimulation of proposed FMVSS 202 using LS-DYNA Implicit
4 th European LS-DYNA Users Conference Occupant II / Pedestrian Safety Simulation of proposed FMVSS 202 using LS-DYNA Implicit Vikas Patwardhan Babushankar Sambamoorthy Tuhin Halder Lear Corporation 21557
More informationUSING INSPIRE AS AN UPFRONT DESIGN, OPTIMIZATION & SIMULATION TOOL FOR EXISITNG MANUAL GEARBOX COMPONENTS
USING INSPIRE AS AN UPFRONT DESIGN, OPTIMIZATION & SIMULATION TOOL FOR EXISITNG MANUAL GEARBOX COMPONENTS Lokesh Kumar Gupta Manager Drive Line Eicher Polaris Plot- SP1 & 2, Kukas Jaipur India 302028 Lkgupta@eicherpolaris.in
More informationRedesign and Analysis of Automobile Wheel Rim #1 Pandit Shailesh, #2 Gajjal Shekhar
ISSN 2395-1621 Redesign and Analysis of Automobile Wheel Rim #1 Pandit Shailesh, #2 Gajjal Shekhar 1 shailesh27290@gmail.com 2 shekhar.gajjal@sinhgad.edu #1234 Department of Mechanical Engineering,SavitribaiPhule
More informationStructural Analysis of Student Formula Race Car Chassis
Structural Analysis of Student Formula Race Car Chassis Arindam Ghosh 1, Rishika Saha 2, Sourav Dhali 3, Adrija Das 4, Prasid Biswas 5, Alok Kumar Dubey 6 1Assistant Professor, Dept. of Mechanical Engineering,
More informationDesign And Analysis Of Two Wheeler Front Wheel Under Critical Load Conditions
Design And Analysis Of Two Wheeler Front Wheel Under Critical Load Conditions Tejas Mulay 1, Harish Sonawane 1, Prof. P. Baskar 2 1 M. Tech. (Automotive Engineering) students, SMBS, VIT University, Vellore,
More informationOptimization and comparison of a Mono Parabolic Leaf Spring by Using Design of Experiment & Simulated Annealing Algorithm
International Research Journal of Engineering and Technology (IRJET) e-issn: 2395-56 Volume: 5 Issue: 2 Feb-218 www.irjet.net p-issn: 2395-72 Optimization and comparison of a Mono Parabolic Leaf Spring
More informationStructural Analysis of Pick-Up Truck Chassis using Fem
International Journal of ChemTech Research CODEN (USA): IJCRGG, ISSN: 0974-4290, ISSN(Online):2455-9555 Vol.9, No.06 pp 384-391, 2016 Structural Analysis of Pick-Up Truck Chassis using Fem Rahul.V 1 *,
More informationCAE Services and Software BENTELER Engineering.
CAE Services and Software BENTELER Engineering BENTELER Engineering offers development services in market segments such as Automotive, Public Transportation, Commercial Vehicles, Shipbuilding and Industry.
More informationParametric Optimization of Hydraulic Modular Trailer Frame using ANSYS (APDL)
INSTITUTE OF TECHNOLOGY, NIRMA UNIVERSITY, AHMEDABAD 38 481 1 Parametric Optimization of Hydraulic Modular Trailer Frame using ANSYS (APDL) A. D. M. Chauhan, B. Prof. S. B. Soni and C. Prof. A. M. Gohil
More informationKEYWORDS: ANSYS, Clamping effects, Leaf spring, Pro-E. International Journal of Computational Engineering Research Vol, 03 Issue, 10
International Journal of Computational Engineering Research Vol, 03 Issue, 10 Leaf Spring Analysis with Eyes Using FEA B.Mahesh Babu 1, D.Muralidhar Yadav 2, N.Ramanaiah 3 1 Assistant Professor, Dr.Samuel
More informationROOF STRENGTH ANALYSIS OF A TRUCK IN THE EVENT OF A ROLLOVER
Research Paper ISSN 2278 0149 www.ijmerr.com Vol. 3, No. 3, July 2014 2014 IJMERR. All Rights Reserved ROOF STRENGTH ANALYSIS OF A TRUCK IN THE EVENT OF A ROLLOVER Daniel Esaw 1 * and A G Thakur 1 *Corresponding
More informationFINITE ELEMENT ANALYSIS OF TIE-ROD FOR SPACECRAFTS
FINITE ELEMENT ANALYSIS OF TIE-ROD FOR SPACECRAFTS Kiran S Sankanagoudar 1, Dr.H.K.Amarnath 2, Prashant D. Bagalkot 3, Mukund Thakur 4 1 M.Tech Student, Gogte Institute of Technology, Belgaum, (India)
More informationMODELLING AND STRUCTURAL ANALYSIS OF VEHICLE CHASSIS FRAME MADE OF POLYMERIC COMPOSITE MATERIAL
MODELLING AND STRUCTURAL ANALYSIS OF VEHICLE CHASSIS FRAME MADE OF POLYMERIC COMPOSITE MATERIAL Shaik Neelophar Begum 1, S.P.Bhanu Murthy 2 1Department of Mechanical Engineering, VEMU Institute of Technology,
More informationDesign and Stress Analysis of Crankshaft for Single Cylinder 4-Stroke Diesel Engine
Design and Stress Analysis of Crankshaft for Single Cylinder 4-Stroke Diesel Engine Amit Solanki #1, Jaydeepsinh Dodiya #2, # Mechanical Engg.Deptt, C.U.Shah University, Wadhwan city, Gujarat, INDIA Abstract
More informationINTRODUCTION. Research & Reviews: Journal of Engineering and Technology. Research Article
Aircraft Fuel Manifold Design Substantiation and Additive Manufacturing Technique Assessment Using Finite Element Analysis Prasanna ND, Balasubramanya HS, Jyothilakshmi R*, J Sharana Basavaraja and Sachin
More informationFEA of the Forged Steel Crankshaft by Hypermesh
Global Journal of Researches in Engineering Mechanical and Mechanics Engineering Volume 13 Issue 4 Version 1.0 Year 2013 Type: Double Blind Peer Reviewed International Research Journal Publisher: Global
More informationNUMERICAL ANALYSIS OF IMPACT BETWEEN SHUNTING LOCOMOTIVE AND SELECTED ROAD VEHICLE
Journal of KONES Powertrain and Transport, Vol. 21, No. 4 2014 ISSN: 1231-4005 e-issn: 2354-0133 ICID: 1130437 DOI: 10.5604/12314005.1130437 NUMERICAL ANALYSIS OF IMPACT BETWEEN SHUNTING LOCOMOTIVE AND
More informationTorsional analysis of the chassis and its validation through Finite. Element Analysis
Torsional analysis of the chassis and its validation through Finite Ayush Anand Student(Production) BIT Mesra,Ranchi, Jharkhand-835215,India ayush.aand@gmail.com Element Analysis Keywords: Roll cage, Torsional
More information