E                                                                  e                                                      ...
adjustable height is developed and assessed using CFD simulation of 3D turbulent flow around the truck,cab and container. ...
Figure 2: Volume mesh with near truck refinement zoneThe dimensions of computations space is shown in figure 3. To capture...
solver yields robustness and rapid convergence on large unstructured meshes even when high aspectratio and badly distorted...
However formation of stagnant area is inevitable in design. But how this is reduced is the key point toreduce drag force o...
Figure 7: Velocity distribution at center plane at 80 kmph vehicle speed                                   Figure 8: Press...
Figure 9: Variation of drag force with vehicle speed           Later wind pressure load on aero deflector is extracted and...
•      Keeping roof deflector over MNAL flat roof cabin with container reduces aerodynamic drag by         22 % which in t...
Upcoming SlideShare
Loading in …5
×

Cfd01 external aerodynamics_mahindra_navistar

752 views

Published on

Published in: Technology, Business
0 Comments
2 Likes
Statistics
Notes
  • Be the first to comment

No Downloads
Views
Total views
752
On SlideShare
0
From Embeds
0
Number of Embeds
59
Actions
Shares
0
Downloads
0
Comments
0
Likes
2
Embeds 0
No embeds

No notes for slide

Cfd01 external aerodynamics_mahindra_navistar

  1. 1. E e ta x n r lk a A d o y mir c s f T uw h t R F n g o Dg a r R d e c u i t on RamMohanRao Pamoti Raval Chetan Deputy Manager -CAE. Senior Manager -CAE Mahindra Navistar Automotives Ltd Mahindra Navistar Automotives Ltd. Pune - 411019, India Pune - 411019, India Abstract The aerodynamic characteristics of heavy commercial vehicles have received substantial interest recently, because of itsimmediate impact on fuel efficiency at high speed cruising. In this study, a numerical simulation has been carried out for three-dimensional turbulent flows around a MNAL truck carrying a container body. Particularly, the effect of a roof fairing attached on theroof of the truck cabin was investigated. Spalart-allmaras turbulence model available in CFD solver ACUSOLVE was used forevaluating aerodynamic forces, velocity and pressure distribution. The result shows the complex wake formation in the top frontedge of container and high pressure built up at exposed front face of the container. Roof fairing reduces the wake formation anddecreases aerodynamic drag, which in turn help reduce the fuel consumption of the truck. Based on simulation, the height of roof fairing was further fine tuned, according to container height to get the best aerodynamic drag reduction of 23%. Also, the pressure data on roof fairing was used for structural durability prediction under wind loadconditions using RADIOSS.Keywords: Aerodynamics, truck, roof fairing, drag force.Introduction:Many studies of Heavy Commercial Vehicles (HCV) for long distant high way applications have shownthat significant proportion of fuel losses were due to aerodynamic drag [1]. Cost down tests have shownthat at speed above 60 mph, the aerodynamic drag account for 60% and rolling resistance causes 40% oftotal drag. Therefore external aerodynamics study and simulation of HCV to reduce the aerodynamic dragassumes importance in this era of high fuel costs.Heavy commercial vehicles such as trucks and buses generally are large bluff bodies without overallaerodynamic shape which causes strong wakes and trailing vortexes resulting in serious aerodynamicdrag at high speed cruising. Shinsuke, Jongsoo and Shuya etc.[2] investigated 3-dimentional turbulenceflow around bluff body, the effect of underbody slant and rear flaps on bluff body aerodynamics. Kim [3]investigated the effect of rear spoiler on commercial bus body and reduced aerodynamic forces. Manyinternational OEMs have taken sustained measures to reduce air drag using aerodynamic front end, rooffairings, cab extender, side skirts etc. The Department of Energy, USA, has launched Super Truckprogram and set ambitious targets for HCV fuel economy improvements which include aerodynamicimprovements among other measures.This paper presents interesting case of aerodynamic drag reduction of Mahindra Navistar’s 25T truck asused in Indian scenario. MN25 straight truck is used with container load carriers which are of differentheights and built independently by road side body work. Therefore, an appropriate sized roof fairing withSimulation Driven Innovation 8
  2. 2. adjustable height is developed and assessed using CFD simulation of 3D turbulent flow around the truck,cab and container. In addition, the wind pressure loads on air fairing were mapped on structural finiteelement model and the design was evaluated for durability.Process Methodology:A. Truck and Roof Fairing ModelThe aerodynamic drag can be divided in to two components: viscous drag and pressure drag. For flowover heavy vehicles at highway speed the Reynolds number is large enough such that viscous forces canbe safely ignored. Consequently drag experienced by a truck is primarily due to pressure drag which iscomprises of pressure force that exist on front and rear of the vehicle.The truck front end is modeled accurately which consist of cab, bumper, wheels and wheel arcs alongwith container body. Even though container body is corrugated but for the model ease and size it isconsidered as plain box. The container body height varies so in order to get better aerodynamicperformance on all containers adjustable roof deflector is considered. Since this is a comparative studywith or without air deflector, for simplicity other parts of the vehicle like mirrors, few underbodycomponents are not considered. Figure 1: MN25 truck without and with roof deflectorGrid developmentFlow around a vehicle body is usually not symmetrical about the vehicle centerline. Accordingly, a fullmodel should be used. However, grid numbers increase excessively and a very high performancecomputer is needed to analyze such a complicated configuration, especially with the inclusion of the roofdeflector. Because of limited computer capacity, a half model without side mirrors was used to analyzethe aerodynamic characteristics. In complete volume, unstructured grid was generated using Acuconsole.Multi block grid topology was used to generate volume mesh as shown in figure 2.Simulation Driven Innovation 8
  3. 3. Figure 2: Volume mesh with near truck refinement zoneThe dimensions of computations space is shown in figure 3. To capture boundary layer phenomenaaccurately, 15 layers were generated on truck surface with first layer height as 0.3 mm and growth rate as1.3. fine and irregular grid at front and rear of the truck was used for accurate commutation. Total meshsize was 16 Mn. tetrahedral elements. Figure 3: Fluid domain around TruckC. Boundary ConditionThe ground plane was modeled as a no-slip surface, with a constant translational velocity matching theforward speed of the truck. The truck cabin, container, roof deflector and wheels were modeled as no-slipsurfaces with zero relative velocity. The velocity vector direction was chosen to match 00 yaw angle. Aconstant initial eddy viscosity condition was specified to be 0.00001 m2/s. A pressure outlet condition wasapplied to the rear face boundary of the model domain. Fluid domain outer boundary was modeled as slipsurface & vehicle centerline surface is modeled as symmetry. Velocity is imposed at the inlet according tovehicle speeds of 40, 60 and 80 kmph.D. Numerical MethodologyIn this work, the Navier-Stokes equations were solved using AcuSolve, a commercially available flowsolver based on the Galerkin/Least-Squares (GLS) finite element method. AcuSolve is a general purposeCFD flow solver that is used in a wide variety of applications and industries. The flow solver provides fastand accurate transient and steady state solutions for standard unstructured element topologies. AcuSolveensures local conservation for individual elements. Equal-order nodal interpolation is used for all workingvariables, including pressure and turbulence equations. The resultant system of equations is solved as afully coupled pressure/velocity matrix system using a preconditioned iterative linear solver. The iterativeSimulation Driven Innovation 8
  4. 4. solver yields robustness and rapid convergence on large unstructured meshes even when high aspectratio and badly distorted elements are present.The following form of the Navier-Stokes equations were solved by AcuSolve to simulate the flow aroundthe Truck: ∂ρ + ∇ • ρu = 0 ∂t (1) ∂u ρ + ρu • ∇u + ∇P = ∇τ + ρb ∂t (2)where ρ=density, u=velocity vector, P=pressure, τ=viscous stress tensor, b=momentum source vector.Due to low mach number involved in these simulation, the flow was assumed to be incompressible, andthe density time derivative in Eq. (1) was set to zero. the three dimensional steady flow is simulated usingRANS single equation Spalart-Allmaras turbulence model. The turbulence equation is solved using GLSformulation. The model equation is as follows: { } ~∂v ~ 2 1 v  + u • ∇v = C b1 S v − C w1 f w   + ∇ • [(v + v )∇v ] + C b2 (∇v ) ~ ~~ ~ ~ ~2∂t d  σ (3)~ ~ v χ χ3 ~ vS=S + fv f v2 = 1 − f v1 = χ= S = 2 2S ij S ij k 2d 2 2 1 + χf v 1 χ 3 + Cv 3 1 v 1/ 6  1 + Cw 6  1  ∂ui ∂u j  ~ vfw = g 6 3  g = r + C w2 (r 6 − r ) S ij =  +  r= ~ 2 2  g + Cw3  6 2  ∂x j ∂xi    Sk d   ~where v is Spalart-Allmaras auxiliary variable, d=length scale , C b1 =0.1355, σ =2/3 , k=0.41, Cw3=2 ,Cv1=7.1, Cb2 =0.622, Cw1 =(Cb1/k2)+((1+Cb2)/σ)The eddy viscosity is then defined by ~ v1 = v f w1For the steady state solutions presented in this work, a first order time integration approach with infinitetime step size was used to iterate the solution to convergence. Steady state convergence was typicallyreached within 100 time steps.Results & Discussions:Base line vehicle: Velocity and Pressure distribution on surface of front and rear of the truck is presented in fig. 4.and fig.5 respectively. Flow comes from the upstream end forms a stagnation area at middle of the frontfascia and container top surface which are directly exposed to air. The divergent of flow has increasedwith increase in pressure value as a result of stagnation phenomenon and then at each curvature flow isradically faster. The stagnation area at the front body is the main cause of drag force with high pressure.Simulation Driven Innovation 8
  5. 5. However formation of stagnant area is inevitable in design. But how this is reduced is the key point toreduce drag force of the truck. Figure 4: Velocity distribution on centerline plane at 80 kmph vehicle speed Figure 5: Pressure distribution at 80 kmph vehicle speedEffect of roof fairing: Figure 6: Aero deflector Velocity and pressure distribution on surface of front and rear of the truck with roof deflector isshown in fig. 7 and fig. 8 respectively. With roof deflector, stagnation area at the top front face of thecontainer was reduced because of that pressure on container reduced that leads to reduction in dragsignificantly. Roof deflector angle is optimized to reduce flow separation zone, which is formed at tip ofthe container, and for better drag reduction compared to base vehicle.Simulation Driven Innovation 8
  6. 6. Figure 7: Velocity distribution at center plane at 80 kmph vehicle speed Figure 8: Pressure distribution at 80 kmph vehicle speed Aero deflector position is optimized to reduce drag force on the vehicle. In case1, where roofdeflector is placed at the front roof edge, as the deflector angle reduces, stagnation area reduces thatleads to reduction in drag coefficient, but if its angle reduces further then stagnation area at containerfront face is increases. Similar effect was observed for case 2 where roof deflector is placed 0.4 m awayfrom roof front edge. Even though case 1 gives better Cd compared to Case2 but it requires more materialcost.Effect of roof fairing for two different cases as shown in fig. 6 are presented in the below table. Table 1: Variation of drag coefficient according to position of roof deflector at 80 kmph Angle, deg Drag Force, N % reduction with base Base vehicle 2054.27 Case 1(roof 40 1650.20 19.3 deflector at 37 1583.19 22.9 cabin front edge) 35 1552.60 24.5 Case 2 (roof 44 1581.60 23.1 deflector at 0.4 m away from 43.5 1565.40 23.4 front edgeVariation of drag force with respect to vehicle speed is shown in figure 9. as the vehicle speed increasesPressure force on front fascia increases leads to increase in drag force.Simulation Driven Innovation 8
  7. 7. Figure 9: Variation of drag force with vehicle speed Later wind pressure load on aero deflector is extracted and used for structural durability withinertia load conditions. Comparison of stress contours with and without wind loads are shown in figure 10. Figure 10: Comparison of Stress contours with and without wind loadConclusions: The three dimensional turbulent flow around truck and the change in aerodynamiccharacteristics caused by roof fairing were numerically investigated. The result and conclusions obtainedby the present simulation can be summarized as follows. • It was conformed that Stagnation region is formed at front of the container, because of that flow at container edges moves faster and sudden diverged flow leads to flow separation in turn creates drag force.Simulation Driven Innovation 8
  8. 8. • Keeping roof deflector over MNAL flat roof cabin with container reduces aerodynamic drag by 22 % which in turn lead reduction in fuel consumption by 1.5 to 2 %. • It was conformed that Wind pressure effect the structural durability of air deflector mounting bracket.Benefits Summary: With the help of AcuSolve, Leading commercial finite element CFD code, we at MNAL productdevelopment team quickly take a decision, whether we go for roof fairing or not, without doing wind tunneltest which is expensive. And it was very useful for us to do parametric study by changing roof fairingangle without spending much time as it was in physical test.Challenges: When we do parametric study in this project, every time when we modify roof fairing angle weshould generate volume mesh again and again which is time consuming. It would be useful for Acusolveusers, if automatic volume mesh updating option is there. ACKNOWLEDGEMENTSThe authors would like to thank Mr. Sanjeev Bedekar, Altair technical support and Mr. Uday Srinivas, Sr.Manger, MNAL cabin team for their valuable support and contributions during this project. We also would like to thank Mr.Shekar Paranjape, General Manager, MNAL for allowing us topublish this paper. REFERENCES 1. Subrata Roy and Pradeep Srinivasan, "External flow analysis of truck for drag reduction", SAE International, 2000-01- 3500. 2. Shiksuke Kowata, Jong soo Ha, Shuya Yoshioka, Takuma kato and yasuaki kohama, "Drag force reduction of a bluff body with an underbody slant and rear flaps", SAE International, 2008-01-2599. 3. Min-Ho Kim, "Numerical study on wake flow and rear-spoiler effect of a commercial bus body", SAE International, 2003- 01-1253. 4. K.P.Garrey, "Development of container-mounted devices for reducing the aerodynamic drag of commercial vehicles", Journal of Wind Engineering and Industrial Aerodynamics, 1981. 5. Wolf heinrich Hucho (2001), "Aerodynamics of road vehicles ", 4th edition, SAE International, Vol.1, PP. 11-88.Simulation Driven Innovation 8

×