College of Engineering and Physical Sciences School of Mechanical Engineering CFD – The Green Bus Company Report Ravi Patel - 1101066
Introduction The Green Bus Company has requested a recommendation for a new design for their existing double decker buses. The new design must aim to be more aerodynamic thereby reducing fuel consumption rates and making the buses more efficient. Computational Fluid Dynamics (CFD) software must be used for the analysis steps and ultimately to determine if the new design is more aerodynamic than the existing model. Design The existing bus design is not as efficient as it could be due to its box-shape design. This design would probably suffer from a large amount of drag force indicated by a large drag co-efficient value. Designing a more aerodynamic bus would mean altering any sharp edges to smooth round ones and making the bus more streamline so the air can flow smoothly around the bus with as little resistance as possible. The frontal area of the bus has been streamlined to reduce the amount of pressure contributing to drag at the front of the bus and to ensure that a boundary (preferably laminar to reduce surface friction) will begin forming along the surface. The backward sloping roof ensures that the bus is more streamlined and flow separation is reduced keeping the boundary layer intact for as long as possible to avoid a very low pressure (from a turbulent wake) at the rear leading to high pressure drag. The intention of the redesign is to reduce the drag co-efficient of the bus.
Old Design (Fig 1)
New Design (Fig 2)
The software used for the CFD analysis was ANSYS Fluent. Both buses were initially designed in Solidworks and imported into Fluent at the initial geometry stage. Fluent Setup and Methodology Geometry The imported body was first frozen so it
couldn’t interact
or be merged with the
enclosure which was created using the enclosure tool to represent the wind tunnel. It
was dimensioned in such a way that there were 3 bus lengths in front and 5 behind as recommended by “Best practice guidelines for handling Automotive External Aerodynamics with FLUENT”(1). Other dimensions were based on judgement for example an extra bus width parallel to the bus and 2 bus heights above. It was essential to ensure the symmetry Fig 3
plane of the bus was correctly applied to create the split along the bus for analysis and to ensure the wheels of the bus were touching the bottom of the enclosure. Finally the Boolean tool was used to subtract the model
volume from the surrounding enclosure and was renamed ‘air ’ (Figure 3). Mesh Most of the default options were kept for the meshing stage except that the advanced size function was changed to “Proximity and Curvature” to help a better mesh form as the mesh approached closer to the bus body and a finer mesh around curved surfaces both leading to a more accurate analysis. The smoothing option was changed to “fine” for the same reason however the mesh size must remain below 500,000. “Named Selections ” were created and specific names were assigned to some faces of the enclosure and for the bus body. The middle, top and outer faces were named “symmetry”, “symmetry-top” and “symmetry-side” respectively. This was to ensure each of these was recognised as a slip wall (zero shear stress wall). The front and rear faces were called “velocityinlet ” and “pressure-outlet” as these are both automatically recognised by Fluent Fig 4 (Meshing of Geometry)
which applies the correct settings.
Setup and Solver Some changes to the default options needed to be made in this section. Firstly, the model was changed to ‘k-epsilon’ which includes more equations for a more complex and accurate analysis. ‘Realizable ’ was also chosen and the Near-Wall treatment was switched to “Non-equilibrium wall functions ”. These options are for more complex flows including turbulent models where rapid changes in flow occur. Under materials, it was ensured the “air ” enclosure made earlier was selected. Next, under boundary conditions, the velocity specification was changed to “magnitude and
direction” and the values 13.41 and –1 in the X component were chosen respectively. This created an airflow velocity of 13.41m/s (30mph) flowing toward the rear of the bus thereby simulating real-life conditions. The turbulence specification method was changed to “intensity and viscosity ratio ”. Intensity (%)
Viscosity (%)
Velocity Inlet
1
10
Pressure Outlet
5
10
(Table 1)
The values in Table 1 were entered as the respective values in t he intensity and viscosity ratio fields. The intensity was chosen as 1 for the flow in front of the vehicle as turbulence would be low and selected slightly higher for the rear as when the flow separates, it becomes slightly turbulent. The viscosities were chosen because they were recommended as typically good values (2). Area and velocity input were required under reference values, and these were 13.41m/s for the velocity and the projected area could be found the reports tab, by selecting the bus body and selecting a minimum feature size of 0.001, the program will compute the projected frontal area of both buses. These were both around 5m 2. The temperature and viscosity values were kept as default. For solution methods and controls, coupled solution was chosen as it solves equations simultaneously and is more efficient for steady state flow models (3). Momentum, turbulent kinetic energy and turbulent dissipation rate were changed to “second order upwind ” for greater accuracy. For solution controls, courant number was changed to 50 and the explicit relaxation factors for momentum and pressure were changed to 0.25 to stabilise skewness which must be under 0.98. For monitors it was essential to select to print and plot f or drag and the X component vector was changed to -1 to go against the bus movement. Again for steady state models, hybrid initialization was recommended as no additional user input was required (4). The number of iterations was altered to 100 as this should be more than enough to reach convergence (Figure 5 and 6) on a value for the drag co-efficient for both buses which are shown in Table 2 below.
Original Design (CD)
New Design (CD)
1.19
0.59
(Table 2)
Results and Discussion
Fig 5
Fig 6
Using ANSYS Fluent, graphs can be generated to show contours, vectors and streamlines of different variables such as velocity, pressure, turbulence intensity, turbulent kinetic energy and many more. The graphs which show the intended results best are the 2D velocity streamline and the turbulent kinetic energy diagrams (A)
(B)
(C)
(D)
Looking at the velocity streamline, the velocity is reduced as it hits the front of the bus in both cases, however with the old design, eddy currents are formed on top and predominantly at the rear of the bus (A). In the new design (B) the velocity streamlines flow smoothly over the surface of the bus and the boundary layer remains intact (predominantly laminar) and the flow remains smooth even after it leaves the bus whereas it becomes turbulent due to the viscosity separating the
boundary layer almost straight away with the old design. In the turbulent kinetic energy diagrams (C) and (D), even though at first glance it may seem as if the turbulent kinetic energy is higher at the rear of the new design however the scales had to be altered to logarithmic to clearly show the variations in turbulence contours in each diagram. Reducing the drag force on a body increases the fuel efficiency. Drag consists of two components; Pressure drag and Frictional drag. Some factors affecting the drag are projected frontal area of the body, vehicle velocity and air density. However these must remain the same for both buses as the average speed on the road will not change and the air density will not change significantly as atmosphere temperature will remain around constant. Frontal area cannot be reduced easily as a double decker bus’s primary objective is public transport. The last factor is the drag coefficient which can be reduced to improve efficiency. The turbulent wake is proportional to the drag force. Due to the original design ’s box shape a high pressure is applied at the front of the bus and very low pressure at the rear in the turbulent wake. It is the difference in these pressures which causes pressure drag whereas the new design’s streamlined shape ensures a smoother flow where the boundary layer separates as late as possible to reduce the size of turbulent wake dramatically thereby reducing the drag co-efficient. The more streamlined shape also reduced surface friction and thereby reducing frictional drag, improving the drag co-efficient further. However the co-efficient cannot be too low as lift may occur. This is when the pressure on the bottom of the body is higher than the pressure on the top or the air causes a lifting force at the front of the vehicle and downward force at the rear casing the body to lift. This is unlikely to be a problem as buses are of and carry substantial weight. Also the buses will travel at fairly low speeds (maximum of 70mph) so t his would not be an issue for the Green Bus company. Verification and Conclusion A simple sphere was modelled on ANSYS Fluent to give a drag co-efficient of 0.1. The Reynolds number was calculated from this value to around 0.96 x 10 6 which was looked up on a Reynolds number- Drag co-efficient graph (5) and the drag coefficient was found to be around 0.1 for this value therefore validating the calibration of the parameter in Fluent. The drag co-efficient value for the new design is 0.59 (normally around 0.7 for buses) which is around half of the 1.19 value of the original. This indicates that the new design is much more aerodynamic and subject to less drag than the original design. Therefore it would have a much better fuel economy.
References 1) 2) 3) 4)
http://www.slashdocs.com/wstzk/external-aerodynamics.html http://www.scribd.com/doc/87384640/Bounday-conditions http://www.afs.enea.it/fluent/Public/Fluent-Doc/PDF/chp22.pdf http://cdlab2.fluid.tuwien.ac.at/LEHRE/TURB/Fluent.Inc/fluent6.2/help/pdf/ug/chp2 6.pdf
5) http://www.dept.aoe.vt.edu/~jschetz/fluidnature/unit02/unit2c.html
